Return to Main Menu
PROGRAMMING MANUAL for
MAZATROL MATRIX (For INTEGREX IV)
MAZATROL Program MANUAL No. :
H740PA0031E
Serial No. :
Before using this machine and equipment, fully understand the contents of this manual to ensure proper operation. Should any questions arise, please ask the nearest Technical Center or Technology Center.
IMPORTANT NOTICE 1. Be sure to observe the safety precautions described in this manual and the contents of the safety plates on the machine and equipment. Failure may cause serious personal injury or material damage. Please replace any missing safety plates as soon as possible. 2. No modifications are to be performed that will affect operation safety. If such modifications are required, please contact the nearest Technical Center or Technology Center. 3. For the purpose of explaining the operation of the machine and equipment, some illustrations may not include safety features such as covers, doors, etc. Before operation, make sure all such items are in place. 4. This manual was considered complete and accurate at the time of publication, however, due to our desire to constantly improve the quality and specification of all our products, it is subject to change or modification. If you have any questions, please contact the nearest Technical Center or Technology Center. 5. Always keep this manual near the machinery for immediate use. 6. If a new manual is required, please order from the nearest Technical Center or Technology Center with the manual No. or the machine name, serial No. and manual name. Issued by Manual Publication Section, Yamazaki Mazak Corporation, Japan 10. 2006
SAFETY PRECAUTIONS
SAFETY PRECAUTIONS Preface Safety precautions relating to the CNC unit (in the remainder of this manual, referred to simply as the NC unit) that is provided in this machine are explained below. Not only the persons who create programs, but also those who operate the machine must thoroughly understand the contents of this manual to ensure safe operation of the machine. Read all these safety precautions, even if your NC model does not have the corresponding functions or optional units and a part of the precautions do not apply.
Rule 1.
This section contains the precautions to be observed as to the working methods and states usually expected. Of course, however, unexpected operations and/or unexpected working states may take place at the user site. During daily operation of the machine, therefore, the user must pay extra careful attention to its own working safety as well as to observe the precautions described below.
2.
Although this manual contains as great an amount of information as it can, since it is not rare for the user to perform the operations that overstep the manufacturer-assumed ones, not all of “what the user cannot perform” or “what the user must not perform” can be fully covered in this manual with all such operations taken into consideration beforehand. It is to be understood, therefore, that functions not clearly written as “executable” are “inexecutable” functions.
3.
The meanings of our safety precautions to DANGER, WARNING, and CAUTION are as follows:
: Failure to follow these instructions could result in loss of life. DANGER : Failure to observe these instructions could result in serious harm to a human life or body. WARNING : Failure to observe these instructions could result in minor injuries or serious machine damage. CAUTION
HGENPA0043E
S-1
SAFETY PRECAUTIONS
Basics ! After turning power on, keep hands away from the keys, buttons, or switches of the operating panel until an initial display has been made. WARNING
! Before proceeding to the next operations, fully check that correct data has been entered and/or set. If the operator performs operations without being aware of data errors, unexpected operation of the machine will result. ! Before machining workpieces, perform operational tests and make sure that the machine operates correctly. No workpieces must be machined without confirmation of normal operation. Closely check the accuracy of programs by executing override, single-block, and other functions or by operating the machine at no load. Also, fully utilize tool path check, Virtual Machining, and other functions, if provided. ! Make sure that the appropriate feed rate and rotational speed are designated for the particular machining requirements. Always understand that since the maximum usable feed rate and rotational speed are determined by the specifications of the tool to be used, those of the workpiece to be machined, and various other factors, actual capabilities differ from the machine specifications listed in this manual. If an inappropriate feed rate or rotational speed is designated, the workpiece or the tool may abruptly move out from the machine. ! Before executing correction functions, fully check that the direction and amount of correction are correct. Unexpected operation of the machine will result if a correction function is executed without its thorough understanding. ! Parameters are set to the optimum standard machining conditions prior to shipping of the machine from the factory. In principle, these settings should not be modified. If it becomes absolutely necessary to modify the settings, perform modifications only after thoroughly understanding the functions of the corresponding parameters. Modifications usually affect any program. Unexpected operation of the machine will result if the settings are modified without a thorough understanding.
Remarks on the cutting conditions recommended by the NC ! Before using the following cutting conditions:
WARNING
- Cutting conditions that are the result of the MAZATROL Automatic Cutting Conditions Determination Function - Cutting conditions suggested by the Machining Navigation Function - Cutting conditions for tools that are suggested to be used by the Machining Navigation Function Confirm that every necessary precaution in regards to safe machine setup has been taken – especially for workpiece fixturing/clamping and tool setup. ! Confirm that the machine door is securely closed before starting machining. Failure to confirm safe machine setup may result in serious injury or death.
S-2
SAFETY PRECAUTIONS
Programming
WARNING
! Fully check that the settings of the coordinate systems are correct. Even if the designated program data is correct, errors in the system settings may cause the machine to operate in unexpected places and the workpiece to abruptly move out from the machine in the event of contact with the tool. ! During surface velocity hold control, as the current workpiece coordinates of the surface velocity hold control axes approach zeroes, the spindle speed increases significantly. For the lathe, the workpiece may even come off if the chucking force decreases. Safety speed limits must therefore be observed when designating spindle speeds. ! Even after inch/metric system selection, the units of the programs, tool information, or parameters that have been registered until that time are not converted. Fully check these data units before operating the machine. If the machine is operated without checks being performed, even existing correct programs may cause the machine to operate differently from the way it did before. ! If a program is executed that includes the absolute data commands and relative data commands taken in the reverse of their original meaning, totally unexpected operation of the machine will result. Recheck the command scheme before executing programs. ! If an incorrect plane selection command is issued for a machine action such as arc interpolation or fixed-cycle machining, the tool may collide with the workpiece or part of the machine since the motions of the control axes assumed and those of actual ones will be interchanged. (This precaution applies only to NC units provided with EIA functions.) ! The mirror image, if made valid, changes subsequent machine actions significantly. Use the mirror image function only after thoroughly understanding the above. (This precaution applies only to NC units provided with EIA functions.) ! If machine coordinate system commands or reference position returning commands are issued with a correction function remaining made valid, correction may become invalid temporarily. If this is not thoroughly understood, the machine may appear as if it would operate against the expectations of the operator. Execute the above commands only after making the corresponding correction function invalid. (This precaution applies only to NC units provided with EIA functions.) ! The barrier function performs interference checks based on designated tool data. Enter the tool information that matches the tools to be actually used. Otherwise, the barrier function will not work correctly. ! The system of G-code and M-code commands differs, especially for turning, between the machines of INTEGREX e-Series and the other turning machines. Issuance of the wrong G-code or M-code command results in totally non-intended machine operation. Thoroughly understand the system of G-code and M-code commands before using this system. Sample program
Machines of INTEGREX e-Series
Turning machines
S1000M3
–1
The milling spindle rotates at 1000 min .
The turning spindle rotates at 1000 min–1.
S1000M203
The turning spindle rotates at 1000 min–1.
The milling spindle rotates at 1000 min–1.
S-3
SAFETY PRECAUTIONS
! For the machines of INTEGREX e-Series, programmed coordinates can be rotated using an index unit of the MAZATROL program and a G68 command (coordinate rotate command) of the EIA program. However, for example, when the B-axis is rotated through 180 degrees around the Y-axis to implement machining with the turning spindle No. 2, the plus side of the X-axis in the programmed coordinate system faces downward and if the program is created ignoring this fact, the resulting movement of the tool to unexpected positions may incite collisions. To create the program with the plus side of the X-axis oriented in an upward direction, use the mirror function of the WPC shift unit or the mirror imaging function of G-code command (G50.1, G51.1). ! After modifying the tool data specified in the program, be sure to perform the tool path check function, the Virtual Machining function, and other functions, and confirm that the program operates properly. The modification of tool data may cause even a field-proven machining program to change in operational status. If the user operates the machine without being aware of any changes in program status, interference with the workpiece could arise from unexpected operation. For example, if the cutting edge of the tool during the start of automatic operation is present inside the clearance-including blank (unmachined workpiece) specified in the common unit of the MAZATROL program, care is required since the tool will directly move from that position to the approach point because of no obstructions being judged to be present on this path. For this reason, before starting automatic operation, make sure that the cutting edge of the tool during the start of automatic operation is present outside the clearance-including workpiece specified in the common unit of the MAZATROL program.
CAUTION
! If axis-by-axis independent positioning is selected and simultaneously rapid feed selected for each axis, movements to the ending point will not usually become linear. Before using these functions, therefore, make sure that no obstructions are present on the path. ! Before starting the machining operation, be sure to confirm all contents of the program obtained by conversion. Imperfections in the program could lead to machine damage and operator injury.
S-4
SAFETY PRECAUTIONS
Operations
WARNING
! Single-block, feed hold, and override functions can be made invalid using system variables #3003 and #3004. Execution of this means the important modification that makes the corresponding operations invalid. Before using these variables, therefore, give thorough notification to related persons. Also, the operator must check the settings of the system variables before starting the above operations. ! If manual intervention during automatic operation, machine locking, the mirror image function, or other functions are executed, the workpiece coordinate systems will usually be shifted. When making machine restart after manual intervention, machine locking, the mirror image function, or other functions, consider the resulting amounts of shift and take the appropriate measures. If operation is restarted without any appropriate measures being taken, collision with the tool or workpiece may occur. ! Use the dry run function to check the machine for normal operation at no load. Since the feed rate at this time becomes a dry run rate different from the program-designated feed rate, the axes may move at a feed rate higher than the programmed value. ! After operation has been stopped temporarily and insertion, deletion, updating, or other commands executed for the active program, unexpected operation of the machine may result if that program is restarted. No such commands should, in principle, be issued for the active program. ! During manual operation, fully check the directions and speeds of axial movement.
CAUTION
! For a machine that requires manual homing, perform manual homing operations after turning power on. Since the software-controlled stroke limits will remain ineffective until manual homing is completed, the machine will not stop even if it oversteps the limit area. As a result, serious machine damage will result. ! Do not designate an incorrect pulse multiplier when performing manual pulse handle feed operations. If the multiplier is set to 1000 times and the handle operated inadvertently, axial movement will become faster than that expected.
S-5
BEFORE USING THE NC UNIT
BEFORE USING THE NC UNIT Limited Warranty The warranty of the manufacturer does not cover any trouble arising if the NC unit is used for its non-intended purpose. Take notice of this when operating the unit. Examples of the trouble arising if the NC unit is used for its non-intended purpose are listed below. 1.
Trouble associated with and caused by the use of any commercially available software products (including user-created ones)
2.
Trouble associated with and caused by the use of any Windows operating systems
3.
Trouble associated with and caused by the use of any commercially available computer equipment
Operating Environment 1.
Ambient temperature During machine operation: 0° to 50°C (32° to 122°F)
2.
Relative humidity During machine operation: 10 to 75% (without bedewing) Note:
As humidity increases, insulation deteriorates causing electrical component parts to deteriorate quickly.
Keeping the Backup Data Note:
Do not attempt to delete or modify the data stored in the following folder. Recovery Data Storage Folder: D:MazakBackUp
Although this folder is not used when the NC unit is running normally, it contains important data that enables the prompt recovery of the machine if it fails. If this data has been deleted or modified, the NC unit may require a long recovery time. Be sure not to modify or delete this data.
S-6 E
CONTENTS Page
1
MAZATROL PROGRAM CONFIGURATION.................... 1-1 1-1
Program Configuration ............................................1-1
2
PROGRAM COORDINATE SYSTEM ......................... 2-1
3
PROGRAM CREATION.................................... 3-1 3-1
Procedure for Program Creation ....................................3-1
3-2
Common Unit ...................................................3-6
3-2-1
3-3
Setting unit data (common data)....................................... 3-6
Materials Shape Unit (MATERIAL) ...................................3-8
3-3-1
Setting unit data................................................... 3-8
3-3-2
Setting sequence data .............................................. 3-8
3-4
Types of the Milling Unit ..........................................3-12
3-4-1
3-5
Planes to be machined and machining methods ......................... 3-12
Point Machining Units............................................3-15
3-5-1
Types of point machining units ....................................... 3-15
3-5-2
Procedure for selecting point machining unit............................ 3-16
3-5-3
Unit data and automatic tool development of the point machining unit ........ 3-17
3-5-4
Automatic tool development for carbide drills ............................ 3-35
3-5-5
New tapping auto-setting scheme .................................... 3-36
3-5-6
Tool sequence data of the point machining unit .......................... 3-41
3-5-7
Tool path of the point machining unit.................................. 3-47
3-5-8
Shape sequence data of the point machining unit........................ 3-96
3-6
Line Machining Units ...........................................3-116
C-1
3-6-1
Types of line machining units ....................................... 3-116
3-6-2
Procedure for selecting line machining unit ............................ 3-117
3-6-3
Unit data, automatic tool development and tool path of the line machining unit ........................................................... 3-118
3-6-4
Tool sequence data of the line machining unit .......................... 3-157
3-6-5
Shape sequence data of the line machining unit ........................ 3-160
3-6-6
Precautions in line machining ....................................... 3-161
3-6-7
Automatic corner override.......................................... 3-165
3-7
Face Machining Units ...........................................3-167
3-7-1
Types of face machining units ...................................... 3-167
3-7-2
Procedure for selecting face machining unit............................ 3-168
3-7-3
Unit data, automatic tool development and tool path of the face machining unit ........................................................... 3-169
3-7-4
Tool sequence data of the face machining unit ......................... 3-214
3-7-5
Precautions in face machining...................................... 3-220
3-7-6
Override in case of the overall width cutting ............................ 3-230
3-7-7
Shape sequence data of the line/face machining unit .................... 3-232
3-8
Turning Units .................................................3-257
3-8-1
Types of turning units ............................................. 3-257
3-8-2
Procedure for selecting turning unit .................................. 3-257
3-9
Bar-Materials Machining Unit (BAR)................................3-259
3-9-1
Setting unit data................................................. 3-259
3-9-2
Setting tool sequence data ......................................... 3-263
3-9-3
Setting shape sequence data ....................................... 3-269
3-10 Copy-Machining Unit (CPY) ......................................3-274
C-2
3-10-1 Setting unit data................................................. 3-274 3-10-2 Setting tool sequence data ......................................... 3-276 3-10-3 Setting shape sequence data ....................................... 3-278
3-11 Corner-Machining Unit (CORNER).................................3-279 3-11-1 Setting unit data................................................. 3-279 3-11-2 Setting tool sequence data ......................................... 3-280 3-11-3 Setting shape sequence data ....................................... 3-282
3-12 Facing Unit (FACING) ..........................................3-283 3-12-1 Setting unit data................................................. 3-283 3-12-2 Setting tool sequence data ......................................... 3-284 3-12-3 Setting shape sequence data ....................................... 3-286
3-13 Threading Unit (THREAD).......................................3-288 3-13-1 Setting unit data................................................. 3-288 3-13-2 Setting tool sequence data ......................................... 3-291 3-13-3 Setting sequence data ............................................ 3-294
3-14 Grooving Unit (T. GROOVE) .....................................3-297 3-14-1 Setting unit data................................................. 3-297 3-14-2 Setting tool sequence data ......................................... 3-300 3-14-3 Setting shape sequence data ....................................... 3-304
3-15 Turning Drilling Unit (T. DRILL) ...................................3-308 3-15-1 Setting unit data................................................. 3-308 3-15-2 Setting tool sequence data ......................................... 3-309 3-15-3 Setting shape sequence data ....................................... 3-315
3-16 Turning Tapping Unit (T. TAP) ....................................3-316
C-3
3-16-1 Setting unit data................................................. 3-316 3-16-2 Setting tool sequence data ......................................... 3-319 3-16-3 Setting shape sequence data ....................................... 3-321
3-17 Mill-Turning Unit (MILLTURN) ....................................3-322 3-17-1 Setting unit data................................................. 3-322 3-17-2 Setting tool sequence data ......................................... 3-323 3-17-3 Setting shape sequence data ....................................... 3-325
3-18 Other Units ...................................................3-326 3-19 Manual Program Machining Unit (MANL PRG) .......................3-327 3-19-1 Setting unit data................................................. 3-327 3-19-2 Setting sequence data ............................................ 3-329
3-20 M-Code Unit (M-CODE) .........................................3-331 3-20-1 Setting unit data (M-code) ......................................... 3-331
3-21 Head Selection Unit (HEAD) .....................................3-333 3-21-1 Setting unit data................................................. 3-333
3-22 Workpiece Transfer Unit (TRANSFER) .............................3-334 3-22-1 Setting unit data................................................. 3-334
3-23 Subprogram Unit (SUB PRO).....................................3-338 3-23-1 Setting unit data................................................. 3-338 3-23-2 Setting sequence data ............................................ 3-339
3-24 Add-In MAZATROL Unit .........................................3-341 3-24-1 Setting unit data................................................. 3-341 3-24-2 Setting sequence data ............................................ 3-341 3-24-3 Help function on Add-in MAZATROL ................................. 3-342
C-4
3-25 End Unit (END)................................................3-346 3-25-1 Setting unit data................................................. 3-346 3-25-2 Setting sequence data ............................................ 3-350
3-26 Simultaneous Machining Unit (SIMULTAN)..........................3-351 3-26-1 Procedure for calling up the SIMULTAN unit ........................... 3-351 3-26-2 Setting unit data................................................. 3-351
3-27 Two-Workpiece Machining Unit (2 WORKPC) ........................3-352 3-27-1 Procedure for calling up the 2 WORKPC unit ........................... 3-352 3-27-2 Setting unit data................................................. 3-352
3-28 Coordinate Measuring Unit (MMS) .................................3-353 3-28-1 Procedure for calling up the MMS unit................................ 3-353 3-28-2 Setting unit data................................................. 3-353 3-28-3 Setting sequence data ............................................ 3-353 3-28-4 Type of measurement............................................. 3-355
3-29 Workpiece Measuring Unit (WORK MES) ...........................3-358 3-29-1 Procedure for selecting workpiece measuring unit ....................... 3-358 3-29-2 Setting the unit data.............................................. 3-358 3-29-3 Setting the sequence data ......................................... 3-359 3-29-4 Selection of a measurement type .................................... 3-360 3-29-5 Offset value and the direction of offset ................................ 3-369 3-29-6 Offset judgment ................................................. 3-373
3-30 Tool Measuring Unit (TOOL MES).................................3-374 3-30-1 Procedure for selecting tool measuring unit ............................ 3-374 3-30-2 Setting the unit data.............................................. 3-374
C-5
3-30-3 Setting the sequence data ......................................... 3-375 3-30-4 Measuring patterns ............................................... 3-376
4
5
PRIORITY FUNCTION FOR THE SAME TOOL.................. 4-1 4-1
Priority Machining Order...........................................4-1
4-2
Priority Machining Zone...........................................4-4
4-3
Editing Function and Input Method of Priority Numbers ...................4-6
4-3-1
Input of priority numbers ............................................. 4-6
4-3-2
Assignment of priority numbers ....................................... 4-7
4-3-3
Change of priority numbers .......................................... 4-8
4-3-4
Deletion of all the priority numbers ..................................... 4-9
4-3-5
How to use the SUB PROG PROC END function ......................... 4-9
4-4
Relation between the Subprogram Unit and the Priority Machining Function......................................................4-11
4-5
Relation between the M-Code Unit and the Priority Machining Function.....4-12
LOWER-TURRET CONTROL FUNCTIONS .................... 5-1 5-1
Machining with the Lower Turret ....................................5-1
5-1-1
Independent machining with the lower turret ............................. 5-1
5-1-2
Simultaneous machining with the upper and lower turrets ................... 5-2
5-1-3
Balanced cutting with the upper and lower turrets ......................... 5-6
5-1-4
Simultaneous machining of processes 1 and 2, using the upper and lower turrets (optional)................................................... 5-7
5-2
Retraction of the Lower Turret.....................................5-10
5-3
Other Setup Items ..............................................5-12
5-3-1
LTUR DIA in common unit .......................................... 5-12
C-6
6
7
8
9
TPC DATA SETTING ...................................... 6-1 6-1
Operating Procedure for Setting TPC (Tool-Path Control) Data.............6-1
6-2
Description of Each TPC Data Item of Turning Unit and Measurement Unit ...........................................................6-4
PROGRAM EDITING...................................... 7-1 7-1
Operating Procedures for Editing Programs............................7-1
7-2
Search ........................................................7-2
7-3
Insertion.......................................................7-6
7-4
Deletion ......................................................7-10
7-5
Copy .........................................................7-14
PROGRAM CREATING/EDITING FUNCTIONS ................. 8-1 8-1
Help Function ...................................................8-1
8-2
Automatic Crossing-Point Calculation Function.........................8-2
8-2-1
Automatic crossing-point calculation in the line and face machining units ....... 8-2
8-2-2
Automatic crossing-point calculation function in the turning unit .............. 8-6
8-3
Automatic Cutting-Conditions Setting Function ........................8-15
8-4
Desk Calculator Functions........................................8-18
8-5
Tool Data Window ..............................................8-19
8-6
Tool File Window ...............................................8-20
SAMPLE PROGRAMS ..................................... 9-1
10 THREE-DIGIT G-FORMAT................................. 10-1 10-1 Outline .......................................................10-1
C-7
10-2 Detailed Description .............................................10-1 10-3 Three-Digit G-Format of MAZATROL Program ........................10-2 10-4 Various Data Description Using G10 ...............................10-20
C-8 E
MAZATROL PROGRAM CONFIGURATION
1 1-1
1
MAZATROL PROGRAM CONFIGURATION Program Configuration MAZATROL programs are each made up of a set of data referred to as unit. The following types of units are prepared for this NC equipment: Common unit Materials shape unit Machining unit
Milling unit
Point machining unit
Drilling Counterbore machining Inversed faced hole machining Reaming Tapping Boring
Through hole Non-through hole Stepped through hole Stepped non-through hole
Back boring Circular milling Counterbore-tapping Line machining unit
Central linear machining Right-hand linear machining Left-hand linear machining Outside linear machining Inside linear machining Right-hand chamfering Left-hand chamfering Outside chamfering Inside chamfering
Face machining unit
Face milling End milling-top End milling-step Pocket milling Pocket milling-mountain Pocket milling-valley End milling slot
Turning unit Manual program machining unit End unit M-code unit Subprogram unit Coordinate measuring unit Workpiece measuring unit Tool measuring unit Head selection unit Workpiece transfer unit Process end unit Simultaneous machining unit Two-workpiece machining unit Add-in MAZATROL unit
Ex
Bar-materials machining Copy-machining Corner-machining Facing Threading Grooving Drilling (turning) Tapping (turning) Mill-turning
1-1
1
MAZATROL PROGRAM CONFIGURATION
Data to be set in the units listed above is classified into the following four major types: 1.
Unit data The data consists of data on the type of machining and the sections to be machined, etc.
2.
Tool sequence data The tool sequence data consists of tool names and other data relating to the operation of the tools. This type of data exists for the milling (point, linear, and face machining) and turning units. For other units, data relating to tools exists with the unit data.
3.
Shape sequence data The data consists mainly of data used to define machining patterns.
4.
TPC data (Tool path control data) TPC data is the auxiliary data to be set on the TPC display. The data consists of tool path/tool change position adjustment data, M-codes, tool offset numbers, etc. Tool paths are automatically generated according to the data set on the PROGRAM display and various parameters. TPC data is intended to eliminate unnecessary paths by changing thus-generated tool paths on an unit-by-unit basis. Machining itself, therefore, will be executed even if TPC data is not set.
Example:
PROGRAM display
UNo. MAT. FC
OD-MAX 70.
A 0
ID-MIN 0.
LENGTH 97.
WORK FACE 2
A
UNo. UNIT MODE POS-B POS-C 1 DRILLING ZC ! !
B
SNo.TOOL NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP RGH DEPTH C-SP 1 CTR-DR 12. A 10. ! ! ! 90. SPOT 25 2 DRILL 10. 10. 20. 0. 100 DRIL T 5. 63
C
FIG PTN 1 PT
A
UNo. UNIT MODE 2 SLOT ZY
SPT-R/x SPT-C/y 0. 0.
DIA 10.
DEPTH 20.
ATC MODE RPM LTUR DIA 0 3000
SPT-Z SPT-Y 0. 0.
NUM. !
POS-B POS-C SRV-A SLOT-WID BTM ! 90. 10. 20. 4
B SNo. TOOL F1 FIG C 1 2
CHMF 0.
ANGLE !
Q !
FR 0.1 0.1
M M M
R 0
WAL FIN-A FIN-R PAT. 4 0. 0. 0
NOM-φ No. # APRCH-1 APRCH-2 TYPE AFD DEP-A DEP-R C-SP FR END MILL 20. A ? ? CW G01 ! ! 120 0.13 PTN SPT-R Z Y R/th I J P CNR RGH LINE 25. 20. 20. LINE ! 20. –20.
M M M
A: Unit data B: Tool sequence data C: Shape sequence data
Specific details and setting procedures of each data are described in Chapter 3. Here (Chapter 1), you should understand what types of units and data constitute a program. Note:
Specify tools in program by their tool names, nominal diameters and suffixes. Specify tools in the tool sequence data. To operate the machine in the automatic operation mode, the tools that have been specified in the program must be registered on the TOOL DATA display.
1-2 E
PROGRAM COORDINATE SYSTEM
2
2
PROGRAM COORDINATE SYSTEM In general, machining dimensions on a drawing are indicated as the distances from a specific reference point. Likewise, within a program, a machining pattern is defined by setting the coordinates from a specific reference point. This reference point is referred to as the program origin and the coordinate system based on the program origin is referred to as the program coordinate system. For MAZATROL programs, the following coordinate system is used to define machining patterns:
Program origin +X +C +Z
+Y Program origin
T3P001
The program origin of X-Z-coordinates system can be set anywhere on the center line of the workpiece. Usually, however, the crossing point of the center line of the workpiece and its finishing edge surface should be taken as the program origin. The program origin of C-axis (rotational axis) can be set at any position convenient for programming. For MAZATROL programs, set X-coordinates as diameter data. That is, the workpiece diameter indicated on the drawing must be set as it is. Example:
For the workpiece shape shown in the diagram below: The coordinates (x, z) of point A are (50, 20), and the coordinates (x, z) of point B (20, 30). A B φ20
φ50
20 30
T3P008
Note 1: For manual program machining units (MANL PRG) and facing units (FACING), the direction of Z-axis is opposite to the one shown in the diagram above. See the relevant items in Chapter 3 for further details. Note 2: Refer to the sections of milling units for details on the C- and Y-axes.
2-1
2
PROGRAM COORDINATE SYSTEM
- NOTE -
2-2 E
PROGRAM CREATION
3
3
PROGRAM CREATION Both the program data and sequence data within a MAZATROL program must be set on the PROGRAM display, and TPC data must be set on the TPC display. The TPC display is called up from the PROGRAM display. This chapter first describes general procedures and precautions related to creating a MAZATROL program and then describes detailed procedures for setting each type of program data on a unit-by-unit basis.
3-1
Procedure for Program Creation (1) Select the PROGRAM display. - Carry out the following operations to call up the PROGRAM display: 1)
Press the display selector key.
!
You will then see the following main-display selection menu in the menu display area of your screen:
POSITION SET UP INFO
PROGRAM
TOOL DATA
CUTTING COND.
PARAM
DIANOS
DATA IN/OUT
TOOL LAYOUT
DISPLAY MAP
2)
Press the [PROGRAM] menu key.
!
The program last selected will be displayed on the PROGRAM display and the current menu will change over to this one:
WORK No.
FIND
PROGRAM BARRIER WPC MSR INFORM.
TOOL PATH
PROCESS PROGRAM CONTROL LAYOUT
HELP
PROGRAM FILE
(2) Press the [WORK No.] menu key. !
The display of [WORK No.] becomes highlighted and the work-Nos. listing window will be displayed.
* The work-Nos. listing window refers to a window that displays a list of work numbers of the programs that have already been registered in the NC equipment. (3) Set the work number of the creating program. - A “work number” refers to a number assigned to each program to distinguish one program from another. A combination of up to 32 alphanumeric characters: 0 to 9 and A to Z, including the symbols “_”, “.”, “+” and “–”, can be used for a work number. Note 1: If a work number is composed of figures alone, it should be a natural number between 1 and 99999999. Note 2: A program name should not begin with a dot (.). - If a work number already registered in the NC unit is set, that program will be displayed on the screen. To create a new MAZATROL program, therefore, you must set a work number not used in other programs. You can check the work-Nos. listing window or the PROGRAM FILE display to see which work numbers are not yet used
3-1
3
PROGRAM CREATION
- If you set a work number not used for the programs that have been registered in the NC unit, the current menu will change over to this one: * WORK No. EIA/ISO MAZATROL PROGRAM PROGRAM
* The EIA/ISO programming function is optional. (4) Press the [MAZATROL PROGRAM] menu key. !
The following line will be displayed on the screen:
UNo. MAT. OD-MAX
ID-MIN
LENGTH
WORK FACE
ATC MODE
RPM
LTUR DIA
0 Cursor
This line denotes the common unit. (5) Set data in each item of the common unit. - See Section 3-2, “Common Unit” for details of the data to be set. - Each time you set data, the cursor moves to the next item automatically. - When you set data in the last item of the common unit, the cursor will move to the starting position of the next line and then the following menu A will be displayed, and pressing the [ >>> ] menu key changes A → B → C → A → B → C in order. POINT LINE FACE TURNING MANUAL MACH-ING MACH-ING MACH-ING PROGRAM M M CODE
END
SHAPE CHECK
SUB WPC MSR WORKPICE TOOL WORKPIECE PROGRAM MEASURE MEASURE SHAPE
SELECT TRANSFER PROCESS HEAD WORKPICE END
SIMUL.
2 WORKPC MODE
>>>
>>>
>>>
'' A
'' B
'' C
(6) From the menus A, B and C, select a unit that is to follow the common unit. !
The unit data line of the selected unit will be displayed in the screen.
Example: UNo. 0
MAT. OD-MAX ID-MIN CBN STL 100.
UNo. 1
If you have selected the bar-materials machining unit (BAR):
UNIT
0.
PART POS-B
LENGTH
WORK FACE
ATC MOCE
RPM
LTUR DIA
100.
2.
0
3000
120.
CPT-X
CPT-Z
FIN-X FIN-Z
BAR
↑ Cursor This line will be displayed.
If you have selected a unit that consists of only unit data (e. g. M-code unit): (7) Set data in each item on the unit data line. - See the relevant part of this section for further detail of the data to be set. - Each time you set data, the cursor moves to the next item automatically. - When you set data in the last item, the cursor will move to the beginning of the next line (unit data line).
3-2
PROGRAM CREATION
3
If you have selected a unit that consists of unit data, tool sequence data, and shape sequence data of only one line (e. g. corner-machining unit): (7)-1 Set data in each item on the unit data line. - See the relevant part of this section for further detail of the data to be set. - Each time you set data, the cursor moves to the next item automatically. - When you set data in the last item, the cursor will move to the beginning of the next line (tool sequence data line). (7)-2 Set data in each item on the tool sequence data line. - See the relevant part of this section for further details of the data to be set. - Each time you set data, the cursor moves to the next item automatically. - When you set data in the last item, the cursor will move to the beginning of the next line (shape sequence data line). (7)-3 Set data in each item on the shape sequence data line. - See the relevant part of this section for further details of the data to be set. - Each time you set data, the cursor moves to the next item automatically. - When you set data in the last item, the cursor will move to the beginning of the next line (unit data line). If you have selected a unit that consists of unit data, tool sequence data, and shape sequence data of multiple lines (e. g. bar-materials machining unit): (7)-1 Set data in each item on the unit data line. - See the relevant part of this section for further details of the data to be set. - Each time you set data, the cursor moves to the next item automatically. - When you set data in the last item, the cursor will move to the beginning of the next line (tool sequence data line). (7)-2 Set data in each item on the tool sequence data line. - See the relevant part of this section for further details of the data to be set. - Each time you set data, the cursor moves to the next item automatically. - When you set data in the last item, the cursor will move to the beginning of the next line (shape sequence data line). (7)-3 Set data in each item on the shape sequence data line. - See the relevant part of this section for further details of the data to be set. - Each time you set data, the cursor moves to the next item automatically. (7)-4 After you have set the entire shape sequence data, press the [SHAPE END] menu key. - The line that immediately succeeds the last shape sequence data line will be displayed as a unit data line. - For a unit that permits you to set more than one line of shape sequence data, you cannot select the next unit unless you carry out this operation (pressing the [SHAPED END] menu key).
3-3
3
PROGRAM CREATION
If you have selected a unit that consists of unit data, tool sequence data of multiple lines and shape sequence data of multiple lines (e. g. drilling unit): (7)-1 Set data in each item on the unit data line. - See the relevant part of this section for further details of the data to be set. - Each time you set data, the cursor moves to the next item automatically. - When you set data in the last item, the tool sequence data is made automatically and the cursor will move to the beginning of the tool sequence data line. (7)-2 Set data in each item on the tool sequence data line. - See the relevant part of this section for further details of the data to be set. - Each time you set data, the cursor moves to the next item automatically. (7)-3 After you have set the entire tool sequence data, set data in each item on the shape sequence data line. - See the relevant part of this section for further details of the data to be set. - Each time you set data, the cursor moves to the next item automatically. (7)-4 After you have set the entire shape sequence data, press the [SHAPE END] menu key. - The line that immediately succeeds the last shape sequence data line will be displayed as a unit data line. - For a unit that permits you to set more than one line of shape sequence data, you cannot select the next unit unless you carry out this operation (pressing the [SHAPED END] menu key). (8) Select the units required for the intended machining operation by repeating steps (6) and (7) above (including steps (7)-1, (7)-2, (7)-3 and (7)-4), and then set data in each of the items displayed on the screen. - A selectable unit differs according to the type of product to be machined. Select a unit in the most suitable order in accordance with your machining drawing, unit sheet, etc. After unit selection, the program can be generated just by setting data as guided by messages. (9) Set the end unit at the end of the program. - Press the [END] menu key. - Without the end unit, the program will not be regarded as a complete one. Therefore, you must set the end unit at the last line of the program. (10) Set data in each item of the end unit. - See the section “End Unit (END)” for details of the data to be set. Note 1: One MAZATROL program can contain a maximum of 1000 units, including the common unit and the end unit. For units that allow you to set multiple lines of sequence data, up to a maximum of 200 lines of shape sequence data can be registered per unit. Note 2: The shape data that you have set can be checked for errors by calling up the SHAPE CHECK display while you are creating the program. See the Operating Manual for details.
3-4
PROGRAM CREATION
Note 3: For the following units, TPC data can be set as required: Turning Milling - BAR unit - DRILLING unit - CPY unit - RGH CBOR unit - CORNER unit - RGH BCB unit - FACING unit - REAMING unit - THREAD unit - TAPPING unit - T. GROOVE unit - BK-CBORE unit - T. DRILL unit - CIRC MIL unit - T. TAP unit - CBOR-TAP unit - MILLTURN unit - BORE T1 unit - BORE S1 unit, Other units - BORE T2 unit - MMS unit - BORE S2 unit - WORK MES unit - LINE CTR unit - TOOL MES unit - LINE RGT unit - TRANSFER unit - LINE LFT unit - LINE OUT unit - LINE IN unit - CHMF RGT unit - CHMF LFT unit, - CHMF OUT unit - CHMF IN unit - FCE MILL unit - TOP EMIL unit - STEP unit - POCKET unit - PCKT MT unit - PCKT VLY unit - SLOT unit See “TPC DATA SETTING” for further details of the data to be set.
3-5
3
3
PROGRAM CREATION
3-2
Common Unit The common unit is the first to be placed in a MAZATROL program, and always takes unit number 0. Data that is set in this unit is referred to as common data, which becomes the base data for the entire program. When creating a MAZATROL program, therefore, you must first set data in this unit.
3-2-1
Setting unit data (common data) UNo.
MAT.
OD-MAX
ID-MIN
LENGTH
WORK FACE
ATC MODE
RPM
LOW TURR
0
[1]
[2]
[3]
[4]
[5]
[6]
[7]
[8]
[1] MAT The following menu will be displayed when the cursor is placed at this item: CST IRN DUCT IRN CBN STL ALY STL STNLESS ALUMINUM L.C.STL AL CAST
From the menu, select the materials type of the workpiece to be machined. If the workpiece to be machined is of a materials type other than those listed above, pre-register that materials type on the CUTTING CONDITION - PERCENTAGE display. See the Operating Manual for details. The data of this item is referred to by the system during automatic setting of cutting conditions. [2] OD-MAX, [3] ID-MIN, [4] LENGTH Set the maximum outside diameter, minimum inside diameter, and maximum length, respectively, of the workpiece.
[2] OD-MAX [2] OD-MAX Program origin
Program origin [3] ID-MIN
[3] ID-MIN
[4] LENGTH
[4] LENGTH
Round bar materials
Molded materials T4P017
- Set the workpiece length, including the edge protrusion (edge section to be cut), in item [4].
3-6
PROGRAM CREATION
3
[5] WORK FACE Set the length of the workpiece edge protrusion in the Z-axis direction.
Protrusion
Program origin [5] WORK FACE
[4] LENGTH
T4P019
- The workpiece edge protrusion refers to a section to be cut during a facing unit (FACING FACE). For units other than facing units, the protrusion is not regarded as part of the workpiece. Therefore, if the workpiece edge is to be cut (that is, if a value other than 0 is set for this item), an facing unit must be selected before selecting a unit involving other machining operations. Either 0 or a plus value must always be set for this item. [6] ATC MODE Specify how to retract the axes before ATC. - Enter 0 to move the axes one by one from the machining end point to the ATC position. - Enter 1 to move the axes all together from the machining end point to the ATC position. [7] RPM If the maximum spindle speed is to be limited, set that maximum value. Data does not need be set if the spindle speed is permitted to reach the maximum value provided for in the specifications. This data has no relation to the milling axial velocity. Note:
For an X-axial tool-tip position over OD-MAX or under ID-MIN (both specified in the common unit), constant cutting speed control will opportunely be relieved by the constant spindle speed control for extra-workpiece area and the spindle will rotate at the speed calculated for the position of OD-MAX or ID-MIN.
The spindle speed for this area is downwards limited to the value calculated for OD-MAX. OD-MAX ID-MIN
The spindle speed for this area is upwards limited to the value calculated for ID-MIN.
* Constant surface speed control is cancelled for extra-workpiece area in order to reduce the machining time.
3-7
3
PROGRAM CREATION
[8] LOW TURR For a machine equipped with upper and lower turrets, enter a safe outside-diameter value for the lower turret. See Chapter 5, “LOWER-TURRET CONTROL FUNCTIONS”, for further details.
3-3
Materials Shape Unit (MATERIAL) The shapes of cast materials or forged materials cannot be defined using the common unit alone. To machine such molded materials, the materials shape unit must be selected following the common unit and the shape data of the materials to be machined must be set. Only the outside-diameter shape and inside-diameter shape of the intended workpiece can be defined using the materials shape unit. This unit of base data, therefore, has no relation to units of machining on the front and back faces, since the tool path for such units are created merely on the basis of the settings in the common unit. This unit need not be set for round-bar materials. Press the [WORKPICE SHAPE] menu key to select the materials shape unit.
3-3-1
Setting unit data UNo.
UNIT
∗
MATERIAL [1]
[1] UNIT The following menu will be displayed when the cursor is placed at this item. OUT
IN
- Select [OUT] to define the outside-diameter shape of the workpiece. - Select [IN] to define the inside-diameter shape of the workpiece. Both OUT and IN can be defined using a maximum of 25 sequences. You must first select [OUT], however, when defining both the outside-diameter and insidediameter shapes of a workpiece. That is, after selecting the materials shape unit as both units No. 1 and No. 2, define the outside-diameter shape using unit No. 1 and then define the insidediameter shape using unit No. 2.
3-3-2
Setting sequence data UNo.
UNIT
∗
MATERIAL ∗∗∗
FIG
PTN
SPT-X
SPT-Z
FPT-X
FPT-Z
RADIUS
1
[1]
[2]
[3]
[4]
[5]
[6]
[1] PTN The following menu will be displayed when the cursor is placed at this item. LIN
TPR
SHAPE END
Select the type of shape from the above menu.
3-8
PROGRAM CREATION
3
The data of the displayed menu denote the following shapes: LIN : Line parallel to the center line of the workpiece TPR : Line not parallel to the center line of the workpiece (Taper line) : Convex arc : Concave arc
Outer diameter shape
TPR
Inner diameter shape
LIN
Material shape
T4P021
[2] SPT-X, [3] SPT-Z, [4] FPT-X, [5] FPT-Z, [6] RADIUS Set the coordinates of the intended start point and end point of the shape you selected for item or . [1]. Also set the radius of the desired circle if you have selected End point
LIN
TPR
End point
Start point [2] SPT-X
[4] FPT-X
[4] FPT-X [3] SPT-Z
[5] FPT-Z
[5] FPT-Z
End point
End point [6] RADIUS
[6] RADIUS Start point
Start point
T4P023
- If you have selected [LIN] for item [1] above, it is good enough just to designate only the coordinates of the end point (FPT-X and -Z). This is because the NC unit will then form automatically two orthogonal lines between the end point of the immediately preceding shape (or the program origin for an LIN as the first shape) and that end point.
3-9
3
PROGRAM CREATION
Start point (The coordinates do not need to be set.) End point
End point of immediately preceding shape T4P022
Note 1: The Z-coordinates of any points located to the right of the program origin must be set with a minus sign.
Plus data
Minus data
T4P024
Note 2: If the start point of a shape is present in the same position as that of the end point of the immediately preceding shape, those coordinates can be automatically set by pressing the [NEXT] menu key. UNo.
UNIT
1
MATERIAL OUT
FIG
PTN
1
LIN
2
TPR
SPT-X SPT-Z FPT-X FPT-Z #
#
20.
RADIUS #
30.
#
Cursor
Pressing the [NEXT] menu key with the cursor at the position shown above sets the following data automatically: UNo.
UNIT
1
MATERIAL OUT
FIG
PTN
1
LIN
SPT-X SPT-Z FPT-X FPT-Z #
#
2
TPR
20.
30.
20.
RADIUS
30.
# #
These values are set automatically.
You can use this function also for BAR and CPY units.
3-10
PROGRAM CREATION
3
Note 1: Although a maximum of 200 lines of shape sequence data can be set in one materials shape unit or turning unit, the maximum usable number of shape sequence data lines may be less than 200 when corner R/C is defined for a complex shape. In that case, alarm 723 EXCEEDS NUMBER OF SHAPES will be displayed, even before the maximum usable number of shape sequence data lines is reached. Note 2: If the maximum usable number of shape sequence data lines is exceeded, alarm 723 EXCEEDS NUMBER OF SHAPES will be displayed during tool path checking, shape checking, shape drawing, or automatic operation.
3-11
3
PROGRAM CREATION
3-4
Types of the Milling Unit The milling unit is available in the following three types : - Point machining unit ... used for drilling of holes (Section 3-5) - Line machining unit .... used for a contour machining (Section 3-6) - Face machining unit ... used for machining an area and machining form (Section 3-7) Each milling unit includes tool sequence and shape sequence.
3-4-1
Planes to be machined and machining methods Data items for setting the plane to be machined and for setting the machining method exist in all point, linear, and face machining unit data. These data items are displayed as MODE, POS-B, and POS-C. Specify the desired face and method under the MODE, POS-B, and POS-C columns. UNo.
UNIT
MODE
DRILLING
[1]
POS-B
[2]
POS-C
DIA
DEPTH
CHMF
[3]
[1] MODE Select the machining method. Mode
Description Cylindrical sides can be machined into the desired shape as specified in the Z-C coordinate system. (C-axial machining)
ZC C
Note: If C-axis function for No. 2 spindle is available, the line machining can be executed on the No. 2 spindle as well.
Edges can be machined into the desired shape as specified in the R-C or X-Y coordinate system. (C-axial machining)
XC C
C
Rear plane can be machined into the desired shape as specified in the R-C or X-Y coordinate system. (C-axial machining)
XC C
Note: The line machining is possible only if the machine has C-axis function for No. 2 spindle.
3-12
PROGRAM CREATION
Mode
3
Description Plane of cylinder can be machined into the desired shape as specified in the Z-Y coordinate system. (Y-axial machining)
ZY
Z
Y
Edges can be machined into the desired shape as specified in the X-Y or R-C coordinate system. (Y-axial machining) X
XY
Y
Rear plane can be machined into the desired shape as specified in the X-Y or R-C coordinate system. (Y-axial machining) X
XY
Y
Holes can be machined on an oblique plane at the desired oblique positioning angle as specified in the B-axial direction. (C-axial machining) This mode cannot be selected for the line or plane machining units.
/C C
The tool approaches from the edge side. Holes can be machined on an oblique plane at the desired oblique positioning angle as specified in the B-axial direction. (C-axial machining) This mode cannot be selected for the line or plane machining units.
/C C
The tool approaches from the rear side. Holes can be machined on an oblique plane at the desired oblique positioning angle as specified in the B-axial direction. (Y-axial machining)
/Y
The tool approaches from the edge side.
3-13
3
PROGRAM CREATION
Mode
Description Holes can be machined on an oblique plane at the desired oblique positioning angle as specified in the B-axial direction. (Y-axial machining)
/Y
The tool approaches from the rear side.
The XC , XY , /C , /Y mode can be selected for a machine model capable of back machining. Note:
For the line machining unit, the /C or /C mode cannot be selected. The ZC, XC, XC , /C or /C mode cannot be selected for a face machining unit.
Precautions for milling with the lower turret 1.
The machine operates in single-workpiece independent machining mode.
2.
The machine operates only in point-machining mode. Drilling, inverse faced hole machining, reaming, tapping, and boring (see Note 2 below) are possible (see Note 1 below). Counterbore machining, back boring, circular milling, or counterbore-tapping is impossible.
3.
It is possible to use ZC, XC, or XC mode. (See Note 1.) It is not possible to use /C, /C , ZY, XY, XY , /Y, or /Y mode.
4.
The machine does not operate in line- or face-machining mode.
5.
The lower turret cannot be used for the M-MANUAL unit that operates the Y-axis.
6.
Simultaneous machining with the milling tools mounted in the upper and lower turrets is impossible.
Note 1: Machining that requires Y-axis operation results in an alarm (for chamfering cycle 2). Note 2: Boring cycle 1 and 2 cannot be used (an alarm occurs for lower-turret milling spindle orientation). [2] POS-B When machining an oblique plane, specify angle B of the oblique plane with respect to a reference angle of 0 degrees of the edge. This data item will become valid when the /C, /Y, /C , /Y mode is selected for a machine model having a B-axis. [3] POS-C Specify the position of the C-axis. This data item will become valid when the ZY, XY, XY , /Y, /Y mode is selected.
3-14
PROGRAM CREATION
3-5
3
Point Machining Units The point machining unit serves to determine the data concerning the machining method and machining form for the drilling of holes. The unit includes the tool sequence determining the tool data used and the shape sequence determining the data concerning the machining dimensions on the drawing.
3-5-1
Types of point machining units As shown below 12 types of point machining units are available: 1. Drilling
NM210-00532
5. Tapping
NM210-00536
6-(4) Boring of stepped non-through hole
NM210-00540
2. Counterbore machining
NM210-00533
6-(1) Boring of through hole
NM210-00537
7. Back boring
3. Inversed faced hole machining
NM210-00534
6 (2) Boring of nonthrough hole
NM210-00538
8. Circular milling
NM210-00541
Fig. 3-1 Types of point machining units
3-15
NM210-00542
4. Reaming
NM210-00535
6 (3) Boring of stepped through hole
NM210-00539
9. Counterbore-tapping
NM210-00543
3
PROGRAM CREATION
3-5-2
Procedure for selecting point machining unit (1) Press the menu selector key (key located at the right of the menu keys) to display the following menu. POINT LINE FACE TURNING MANUAL MACH-ING MACH-ING MACH-ING PROGRAM
END
SHAPE CHECK
>>>
(2) Presse the [POINT MACH-ING] menu key. !
The following unit menu will be displayed.
DRILLING RGH CBOR RGH BCB REAMING TAPPING
BORING
BK CBOR CIRC MIL CBOR TAP HI SPD. DRL.USE
(3) Press the appropriate menu key of the desired machining unit. - When the [BORING] menu key is pressed, the menu of the four following machining subunits is displayed. BORING
BORING
BORING
BORING
Remark: For the function of the [HI SPD. DRL. USE] menu key, refer to the Subsection 3-5-4, “Automatic tool development for cemented carbide drills”.
3-16
PROGRAM CREATION
3-5-3
3
Unit data and automatic tool development of the point machining unit 1.
Drilling unit (DRILLING) Select this drilling unit for machining of a hole with a drill. DRILLING unit
Tool sequence
DIA
DEPTH
CHMF
Centering drill
Drill
(Drill)
M3P085 The tools in parentheses (
(Drill)
(Chamfering cutter)
D740PA030 ) are developed or not developed depending on the particular case.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. Tool Centering drill
Development patterns Development is always executed. A maximum of three tools are developed depending on the diameter of the hole.
Drill
0 < DIA ≤ D8: Development of one tool D8 < DIA ≤ D9: Development of two tools D9 < DIA ≤ D10: Development of three tools
Development is not executed in the following cases: Chamfering cutter
DIA + (CHMF × 2) ≤ D2 – D4 CHMF = 0 The bold codes represent parameter addresses.
Note:
In the following cases the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed. - DEPTH < CHMF - DIA = 0 - D10 < DIA
3-17
3
PROGRAM CREATION
2.
Counterbore machining unit (RGH CBOR) This unit is selected for machining a hole with a counterbore (faced hole). RGH CBOR unit
Tool sequence
CB-DIA CB-DEP
CHAMF
DEPTH
Centering drill
Drill
(Drill)
(Drill)
End mill (Chamfering cutter)
DIA
M3P087 The tools in parentheses (
D740PA031 ) are developed or not developed depending on the particular case.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. Tool Centering drill
Development patterns Development is always executed. A maximum of three tools are developed depending on the diameter of the hole.
Drill
0 < DIA ≤ D8: Development of one tool D8 < DIA ≤ D9: Development of two tools D9 < DIA ≤ D10: Development of three tools
End mill
Development is always executed. Development is not executed in the following casses:
Chamfering cutter
CHMF = 0 DIA + (DEPTH × 2) ≥ CB-DIA + (CHMF × 2) < D13 The bold codes represent parameter addresses.
Note:
In the following cases the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed. - CB-DIA < DIA - DEPTH < CB-DEP - DEPTH < CHMF
3-18
PROGRAM CREATION
3.
3
Inversed faced hole machining unit (RGH BCB) This unit is selected for machining a hole with an inversed faced hole. RGH BCB unit
Tool sequence
DIA
DEPTH
CHMF
Centering drill
CB-DEP
Drill
(Drill)
(Drill)
CB-DIA
M3P089 The tools in parentheses (
(Chamfering Back facing cutter)
D740PA032 ) are developed or not developed depending on the particular case.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. Tool Centering drill
Development patterns Development is always executed. A maximum of three tools are developed depending on the diameter of the hole.
Drill
0 < DIA ≤ D8: Development of one tool D8 < DIA ≤ D9: Development of two tools D9 < DIA ≤ D10: Development of three tools
Development is not executed in the following cases: Chamfering cutter
DIA + (CHMF × 2) ≤ D2 – D4 CHMF = 0
Back facing tool
Development is always executed. The bold codes represent parameter addresses.
Note:
In the following cases the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed. - CB-DIA < DIA - DEPTH < CB-DEP - DEPTH < CHMF
3-19
3
PROGRAM CREATION
4.
Reaming unit (REAMING) Select this unit for performing finish machining with reamer. In reaming, the content of the tool sequence to be set is different according to the preceding process. A.
Case of preceding process = drilling REAMING unit
Tool sequence
DIA
DEPTH
CHMF
Centering drill
Drill
(Drill)
(Drill) (Chamfering cutter) Reamer
M3P091 The tools in parentheses (
D740PA033 ) are developed or not developed depending on the particular case.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. Tool Centering drill
Development patterns Development is always executed. A maximum of three tools are developed depending on the diameter of the hole.
Drill
0 < DIA – D35 ≤ D8: Development of one tool D8 < DIA – D35 ≤ D9: Development of two tools D9 < DIA – D35 ≤ D10: Development of three tools
Development is not executed in the following cases: Chamfering cutter
DIA + (CHMF × 2) ≤ D2 – D4 CHMF = 0
Reamer
Development is always executed. The bold codes represent parameter addresses.
Note:
In the following case the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed. - DEPTH < CHMF
3-20
PROGRAM CREATION
B.
3
Case of preceding process = boring REAMING unit
Tool sequence
DIA
DEPTH
CHMF
Centering drill
(Chamfering cutter)
Drill
(Drill)
Boring
Reamer
M3P093 The tools in parentheses (
(Drill)
D740PA034 ) are developed or not developed depending on the particular case.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. Tool Centering drill
Development patterns Development is always executed. A maximum of three tools are developed depending on the diameter of the hole.
Drill
0 < DIA – D36 ≤ D8: Development of one tool D8 < DIA – D36 ≤ D9: Development of two tools D9 < DIA – D36 ≤ D10: Development of three tools
Boring tool
Development is always executed. Development is not executed in the following cases:
Chamfering cutter
DIA + (CHMF × 2) ≤ D2 – D4 CHMF = 0
Reamer
Development is always executed. The bold codes represent the parameter addresses.
Note:
In the following case the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed. - DEPTH < CHMF
3-21
3
PROGRAM CREATION
C.
Case of preceding process = end mill REAMING unit
Tool sequence
DIA
DEPTH
CHMF
Centering drill
Drill
(Drill)
(Chamfering cutter)
End mill
End mill
Reamer
M3P095 The tools in parentheses (
(Drill)
D740PA035 ) are developed or not developed depending on the particular case.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. Tool Centering drill
Development patterns Development is always executed. A maximum of three tools are developed depending on the diameter of the hole.
Drill
0 < DIA – D37 ≤ D8: Development of one tool D8 < DIA – D37 ≤ D9: Development of two tools D9 < DIA – D37 ≤ D10: Development of three tools
End mill
Development of two tools is executed. Development is not executed in the following cases:
Chamfering cutter
DIA + (CHMF × 2) ≤ D2 – D4
Reamer
Development is always executed.
CHMF = 0
The bold codes represent the parameter addresses.
Note:
In the following case the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed. - DEPTH < CHMF
3-22
PROGRAM CREATION
5.
3
Tapping unit (TAPPING) Select this unit for performing tapping. Example 1:
For 3/4-16 unified thread: Press the [Q (1/4) QUARTER] menu key, and then press the keys 3
Example 2:
–
1
6
and
INPUT
in this order.
For 1 1/8-7 unified thread: Press the [E (1/8) EIGHTH] menu key, and then press the keys INPUT
9
–
7
and
in this order.
Example 1:
For PT 3/8 thread: Press the [E (1/8) EIGHTH] menu key, and then press the keys
3
and
INPUT
in this order. Example 2:
For PF 1 thread: Press the keys
1
and
INPUT
in this order.
Note 1: The thread depths of PT screws or PS screws are set automatically according to MAZAK specifications. Note 2: For planetary tapping, the data to be set for the MAJOR-φ, PITCH, TAP-DEP, and CHMF, depends on the selected type of tool. Enter the data specified in the corresponding tool catalogue. For TAP-DEP, enter the cutting edge length specified in the tool catalogue. Also, set the tool data as follows. - Enter the catalogued nominal diameter in the tool data item ACT-φ. - Enter the catalogued thread outside diameter in the tool data item DIAMETER. - Enter the catalogued cutting edge length in the tool data item LENGTH.
Cutting edge length
Thread outside diameter
3-23
3
PROGRAM CREATION
TAPPING unit
Tool sequence
MAJOR-φ
TAPDEP
CHMF
Centering drill
Drill
(Drill)
(Drill) (Chamfering cutter) Tap
PITCH
M3P097 The tools in parentheses (
D740PA036 ) are developed or not developed depending on the particular case.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. Tool Centering drill
Development patterns Development is always executed. A maximum of three tools are developed depending on the diameter of the hole.
Drill
0 < Diameter of pre-hole drilling ≤ D8: Development of one tool D8 < Diameter of pre-hole drilling ≤ D9: Development of two tools D9 < Diameter of pre-hole drilling ≤ D10: Development of three tools
Development is not executed in the following cases: Chamfering cutter
Diameter of hole + (CHMF × 2) ≤ D2 – D4 CHMF = 0
Tap
Development always takes place. The bold codes represent the parameter addresses.
Note:
In the following cases the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed. - TAP-DEP < CHMF - Case of designation of threading other than the JIS standard threading (however, this can be used for forced insertion).
3-24
PROGRAM CREATION
6.
3
Boring unit (BORING) The boring has the four units as the through hole boring, non-through hole boring, stepped through hole boring and stepped non-through hole boring. A.
Through hole boring unit (BORE T1) Select this unit for performing through-hole boring. BORE T1 unit
Tool sequence
DIA
CHMF DEPTH Centering drill
Drill
(End mill)
Boring
(Boring)
(Chamfering cutter) (Boring)
M3P099 The tools in parentheses (
D740PA037 ) are developed or not developed depending on the particular case.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. Tool Centering drill Drill End mill
Development patterns Development is always executed. Development is always executed. Development is not executed in the following case: DIA – 6.0 < D8 Development of a maximum of three tools is executed depending on the wall roughness.
Boring tool
Wall roughness = 1, 2: Development of one tool Wall roughness = 3, 4: Development of two tools Wall roughness = 5, 6, 7, 8, 9: Development of three tools
Chamfering cutter
Development is not executed in the following case: CHMF = 0 The bold codes represent the parameter addresses.
Note:
In the following cases the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed. - Diameter of faced hole < DIA - DEPTH < Depth of faced hole - DEPTH < CHMF
3-25
3
PROGRAM CREATION
B.
Non-through hole boring unit (BORE S1) Select this unit for performing boring of non-through holes. BORE S1 unit
Tool sequence
DIA
CHMF
DEPTH
Centering drill
Drill
(End mill)
Boring
(Boring)
PRE-DIA
(Chamfering cutter) (Boring)
M3P0101 The tools in parentheses (
D740PA037 ) are developed or not developed depending on the particular case.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. Tool
Development patterns
Centering drill
Development is always executed.
Drill
Development is always executed. Development is not executed if the following three conditions are fulfilled:
End mill
DIA – 6.0 < D8 10.0 < PRE-DIA DIA – PRE-DIA ≤ 6.0 The development of a maximum of three tools is executed according to the wall roughness.
Boring tool
Wall roughness = 1, 2: Development of one tool Wall roughness = 3, 4: Development of two tools Wall roughness = 5, 6, 7, 8, 9: Development of three tools
Chamfering cutter
Development does not take place in the following case: CHMF = 0 The bold codes represent the parameter addresses.
Note:
The alarm 416 AUTO PROCESS IMPOSSIBLE is given in the following cases: - DIA < PRE-DIA - DIA ≤ 6.0 - DEPTH < CHMF - PRE-DIA = 0 → DEPTH < (A/3.328558 – D12) - PRE-DIA ≠ 0 → DEPTH < (A – PRE-DIA)/3.328558 A: DIA – 6.0 (in case of DIA – 6.0 < D8) or A: D8 (in case of D8 ≤ DIA – 6.0)
3-26
PROGRAM CREATION
C.
3
Stepped through hole boring unit (BORE T2) Select this unit for performing stepped through hole boring. BORE T2 unit
Tool sequence
CB-DIA CB-DEP CHMF DEPTH CHMF
Centering drill
Drill
End mill
(End mill)
Boring
(Boring)
DIA
Boring
(Boring)
(Chamfering (Chamfering (Boring) cutter) cutter)
M3P0102 The tools in parentheses (
(Boring)
D740PA038 ) are developed or not developed depending on the particular case.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. Tool Centering drill Drill End mill
Boring tool
Development patterns Development is always executed. Development is always executed. Development of a maximum of two tools is executed depending on the diameter of the hole. 0 < DIA – 6.0 < D8: Development of one tool D8 < DIA – 6.0 ≤ 999.999: Development of two tools The development of a maximum of three tools is executed depending on the wall roughness of the hole and depending on the wall roughness of the large hole, respectively. Wall roughness of hole = 1, 2: Development of one tool Wall roughness of hole = 3, 4: Development of two tools Wall roughness of hole = 5, 6, 7, 8, 9: Development of three tools Wall roughness of large hole = 1, 2: Development of one tool Wall roughness of large hole = 3, 4: Development of two tools Wall roughness of large hole = 5, 6, 7, 8, 9: Development of three tools
Chamfering cutter
Development is not executed when the following two conditions are fulfilled: CHMF = 0 CHMF (CB) = 0 The bold codes represent the parameter addresses.
Note:
The alarm 416 AUTO PROCESS IMPOSSIBLE is given in the following cases: - CB-DEP < CHMF (CB) - CB-DIA < DIA - (CB-DIA – DIA)/2 < CHMF - DEPTH – CB-DEP < CHMF - DIA ≤ 6.0
3-27
3
PROGRAM CREATION
D.
Stepped non-through hole boring unit (BORE S2) Select this unit for performing stepped non-through boring. BORE S2 unit
Tool sequence
CB-DIA CB-DEP
CHMF DEPTH CHMF PRE-DIA
Centering drill
Drill
End mill
(End mill)
Boring
(Boring)
DIA
Boring
(Boring)
(Chamfering (Chamfering (Boring) cutter) cutter)
M3P0104 The tools in parentheses (
(Boring)
D740PA038 ) are developed or not developed depending on the particular case.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. Tool
Development patterns
Centering drill
Development is always executed.
Drill
Development is always executed. Development of a maximum of two tools is executed depending on the diameter of the hole.
End mill
0 < DIA – 6.0 < D8, 10.0 < PRE-DIA and (DIA – PRE-DIA) ≤ 6.0: Development of one tool D8 < DIA – 6.0 ≤ 999.999: Development of two tools
The development of a maximum of three tools is executed depending on the wall roughness of the hole and depending on the wall roughness of the large hole, respectively. Wall roughness of hole = 1, 2: Development of one tool Wall roughness of hole = 3, 4: Development of two tools Boring tool
Wall roughness of hole = 5, 6, 7, 8, 9: Development of three tools Wall roughness of large hole = 1, 2: Development of one tool Wall roughness of large hole = 3, 4: Development of two tools Wall roughness of large hole = 5, 6, 7, 8, 9: Development of three tools Development is not executed when the following two conditions are fulfilled:
Chamfering cutter
CHMF = 0 CHMF (CB) = 0 The bold codes represent the parameter addresses.
3-28
PROGRAM CREATION
Note:
The alarm 416 AUTO PROCESS IMPOSSIBLE is given in the following cases: - CB-DIA < DIA - DIA ≤ PRE-DIA - DEPTH < CB-DEP - CB-DEP < CHMF (CB) - (CB-DIA – DIA)/2 < CHMF - (DEPTH – CB-DEP) < CHMF - DIA ≤ 6.0 - DEPTH < CHMF - B≤0 B: DIA – 6.0 (in case of DIA – 6.0 < D8) or B: D8 (in case of D8 ≤ DIA – 6.0)
3-29
3
3
PROGRAM CREATION
7.
Back boring unit (BK-CBORE) Select this unit for performing back boring. BK-CBOR unit
Tool sequence
PRE-DIA
PRE-DEP
CHMF
Centering drill
DEPTH
Drill
(End mill)
Boring
(Boring)
(Chamfering cutter)
(Back boring)
(Boring)
(Back boring)
DIA
(Back boring)
(Back boring)
(Back boring)
(Back boring)
(Back boring)
M3P106
D740PA039
The tools in parentheses (
) are developed or not developed depending on the particular case.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. Tool
Development patterns
Centering drill
Development is always executed.
Drill
Development is always executed.
End mill
Development is not executed in the following case: PRE-DIA – 6.0 < D8 Development of a maximum of three tools is executed depending on the wall roughness. Wall roughness of pre-hole = 1, 2: Development of one tool (Roughing)
Boring tool
Wall roughness of pre-hole = 3, 4: Development of two tools (Roughing, semi-finishing) Wall roughness of pre-hole = 5, 6, 7, 8, 9: Development of three tools (Roughing, semifinishing, finishing)
Chamfering cutter
Development is not executed in the following case: CHMF = 0 The development of a maximum of five tools is executed according to the value of N (See Note below.)
Back boring tool
N = 2: N = 3: N = 4: N = 5:
Development of two tools Development of three tools Development of four tools Development of five tools
The development of a maximum of two tools is executed depending on the wall roughness. Back boring tool (Semi-finishing, finishing)
Wall roughness of hole = 1, 2: No development Wall roughness of hole = 3, 4: Development of one tool (Semi-finishing) Wall roughness of hole = 5, 6, 7, 8, 9: Development of two tools (Semi-finishing, finishing) The bold codes represent the parameter addresses.
3-30
PROGRAM CREATION
Note:
3
The alarm 416 AUTO PROCESS IMPOSSIBLE is given in the following cases: - DIA < PRE-DIA - PRE-DEP < DEPTH - PRE-DEP < CHMF - PRE-DEP ≤ DIA/2 - 5 tool diameter ≥ (DIA/2)”.
3-33
3
PROGRAM CREATION
9.
Counterbore-tapping unit (CBOR-TAP) Select this unit for machining a tapped hole with a counterbore (faced hole). CBOR-TAP unit
Tool sequence
CB-DIA
CB-DEP CHMF TAP-DEP CHMF Centering drill
PITCH
Drill
(Drill)
(Drill)
End mill
MAJOR-φ
(Chamfering cutter)
(Chamfering cutter)
Tap
M3P110 The tools in parentheses (
D740PA042 ) are developed or not developed depending on the particular case.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. Tool Centering drill
Development patterns Development is always executed. The development of a maximum of three tools is executed depending on the diameter of the hole.
Drill
0 < Hole diameter ≤ D8: Development of one tool D8 < Hole diameter ≤ D9: Development of two tools D9 < Hole diameter ≤ D10: Development of three tools
Development is not executed in the following cases: Chamfering cutter
CHMF (faced hole) = 0 CHMF (threaded hole) = 0
Tap
Development always takes place. The bold codes represent the parameter addresses.
Note:
The alarm 416 AUTO PROCESS IMPOSSIBLE is given in the following cases: - CB-DIA < MAJOR-φ - (CB-DIA – MAJOR-φ)/2 < CHMF (threaded hole) - PRE-DEP < CHMF (faced hole) - TAP-DEP < CHMF (threaded hole)
3-34
PROGRAM CREATION
3-5-4
3
Automatic tool development for carbide drills The Subsection 3-5-3 describes automatic tool development for drilling using high speed steel drills. Automatic tool development for cemented carbide drills is described below. This function allows machining time and programming time to be reduced. Before using this function, thoroughly understand its usage, since mis-use causes tool damage. After point machining unit selection, the following menu is displayed. Press the [HI SPD DRL. USE] menu key to make the function valid (reverse the display status of the menu item) before selecting a unit. Automatic tool development for cemented carbide drills will occur for the tool sequence: DRILLING RGH CBOR RGH BCB REAMING TAPPING
BORING
BK CBOR CIRC MIL CBOR TAP HI SPD. DRL.USE
Automatic tool development for drilling with cemented carbide drills is valid for all poit-machining units and described below using a drilling unit as an example. UNo.
UNIT
2
DRILLING
MODE
POS-B
NOM-φ No.
#
POS-C
DIA
DEPTH
HOLE-φ HOLE-DEP PRE-DIA
CHMF
SNo.
TOOL
PRE-DEP
RGH
DEPTH
1
DRILL
$
$
$
$
$
DRIL
$
2
CHAMFER
$
$
$
$
$
#
$
C-SP FR
M
M
M
1)
Centering drill data for machining a center hole is not developed automatically.
2)
Drilling cycle is developed at RGH in the drilling tool sequence, irrespective of the hole depth.
3)
Only one drill data is developed automatically, even for a large hole diameter.
4)
When the hole diameter is larger than the value of parameter D2 (nominal diameter of a centering drill), chamfering cutter data is developed automatically. Tool data for chamfering with a centering drill is developed automatically for a hole diameter (DIA) smaller than or equal to the value of parameter D2 (nominal diameter of a centering drill).
UNo.
UNIT
MODE
2
DRILLING
SNo.
TOOL
POS-B
NOM-φ No.
#
POS-C
DIA
DEPTH
HOLE-φ HOLE-DEP PRE-DIA
CHMF
PRE-DEP
RGH
DEPTH
1
DRILL
$
$
$
$
$
DRIL
$
2
CTR-DR
$
$
#
#
#
90°
#
C-SP FR
M
M
M
$ : The data displayed here are automatically determined by automatic tool development function. #
: Data are not necessary to be set here.
3-35
3
PROGRAM CREATION
3-5-5
New tapping auto-setting scheme Any given value for tapping with the tapping unit/counterbore-tapping unit can be specified as an auto-set value by editing the required text file within the hard disk. (New tapping auto-setting scheme) The items corresponding to the new tapping auto-setting scheme are listed below. $: New tapping auto-setting scheme applicable —: New tapping auto-setting scheme inapplicable
1.
Tapping/Counterbore-tapping unit
Type of thread to be tapped
MAJOR-φ
PITCH
TAP-DEP
PRE-DIA
PRE-DEP
Metric thread
—
—
—
$
—
Unified thread
—
—
—
$
—
Pipe thread (PT)
$
$
$
$
$
Pipe thread (PF)
$
$
—
$
—
Pipe thread (PS)
$
$
$
$
$
Tapping for metric thread /unified thread In the case of tapping for metric thread/unified thread, the new tapping auto-setting scheme is valid only when parameter D95 is set as follows: D95 bit 2 = 0: The text file is invalid and tapping for metric thread is subject to the conventional auto-setting scheme. = 1: The text file is valid and tapping for metric thread is subject to auto-setting based on editing. D95 bit 1 = 0: The text file is invalid and tapping for unified thread is subject to the conventional auto-setting scheme. = 1: The text file is valid and tapping for unified thread is subject to auto-setting based on editing. The text file format, the text data items, and the editing procedure are shown below. A.
Text file format [M] PRE_DIA_1=8000 ; Diameter of Prehole(1/10000mm)
← Pre-hole diameter
PRE_DIA_2=9000 ; Diameter of Prehole(1/10000mm)
← Pre-hole diameter
M M [UN] PRE_DIA_1=15000; Diameter of Prehole(1/10000mm)
← Pre-hole diameter
PRE_DIA_2=18000; Diameter of Prehole(1/10000mm)
← Pre-hole diameter
M M
B.
Text data items - Pre-hole diameter (Setting unit: 1/10000 mm) This item denotes the auto-setting values for NOM-φ and HOLE-φ in the last drill tool sequence whose automatic tool development will be conducted for the tapping unit/counterbore-tapping unit.
3-36
PROGRAM CREATION
C.
3
Editing procedure (1) Click the Start button and select “Programs” from the Start menu option. Then click “Explorer”. (2) After copying “TapPrDia.org” (an auto-setting model file for metric thread/unified thread tapping) within the “C:nm64tdata” directory into this directory, change the file name to “TapPrDia.txt”. (3) Open “TapPrDia.txt” using a commercially available editor. (4) Edit the file seeing the above description of “Text file format” and “Text data items” and taking notice of each data unit. An example of editing is shown below. Note 1: If data is not entered correctly, alarm 494 AUTO TAP PROCESS IMPOSSIBLE will be displayed when auto-setting is executed. Enter data within the following range: Item Pre-hole diameter
Keyword
Input unit
PRE_DIA
1/10000 mm
Minimum value 1000
Maximum value 9999000
Enter integral decimal numbers. For this item always enter “0” as the least two significant digits (that is, the last two digits). Note 2: Even within the above data range, the particular combination of data settings in each item may display an asterisk (∗) to indicate that the amount of chamfering cannot be calculated. In such a case, to ensure that the amount of chamfering will be calculated properly, enter data in each item so that the calculation results in the following calculation expressions range from “0” to “99.9”: [If parameter D44 is set to “0”] (Chamfering) = {(Tap outside diameter) + (Thread pitch) × 2 – (Prehole diameter)}/2 [If parameter D44 is set to “1”] (Chamfering) = {(Tap outside diameter) – (Prehole diameter)}/2 Note 3: Even when data within the above data range is entered, alarm 416 AUTO PROCESS IMPOSSIBLE may be displayed during automatic development of the tool data. Note 4: Entered prehole diameter value has its respective last two digits cut away. (5) After editing the file, execute “Overwrite & Save”. (6) Close “Explorer”. D.
Example of editing For “M1 tapping”, proceed as follows to auto-set 0.7 mm as the prehole diameter: (1) Open the text file “TapPrDia.txt”. (2) Move the cursor to the masked item required units. Do not edit other items.
shown below and then edit data in the
[M] PRE_DIA_1=7000 ;
Diameter of Prehole(1/10000mm)
PRE_DIA_2=9000 ;
Diameter of Prehole(1/10000mm)
M M
3-37
3
PROGRAM CREATION
Note 1: Since the default settings of the text file data conform to the conventional scheme, auto-set data cannot be modified by merely changing the value of bit 1 or bit 2 in the D95 parameter. Note 2: When modifying the metric thread/unified thread tapping auto-set data, the user itself needs to edit and manage the text file. Note 3: After text file editing, the new data is incorporated into the auto-set data immediately. Note 4: Even for inch specifications, assign data in units of 1/10000 mm to the text file. Note 5: Since auto-set data having an assigned decimal point and exceeding the minimum allowable number of digits cannot be displayed, text file modifications may not be displayed as auto-settings intact. Example:
2.
Even if the value of PRE_DIA_1 is changed to 8600, a nominal drill diameter of 0.9 may be displayed as its auto-set value.
Tapping for pipe thread In the case of tapping for pipe thread, the new tapping auto-setting scheme is valid only when parameter D95 is set as follows: D95 bit 0 = 0: The text file is invalid and tapping for pipe thread is subject to the conventional auto-setting scheme. = 1: The text file is valid and tapping for pipe thread is subject to auto-setting based on editing. The text file format, the text data items, and the editing procedure are shown below. A.
Text file format [PT] ;PT 1/8 DIAMETER_1=97280
;Diameter(1/10000mm)
THREAD_1=280
;Number of Thread(1/10Thread)
DEPTH_1=156000
;Depth(1/10000mm)
PRE_DIA_1=82000
;Diameter of Prehole(1/10000mm)
PRE_DEP_1=184100
;Depth of Prehole(1/10000mm)
← ← ← ← ←
Tap outside diameter Total threads Thread depth Pre-hole diameter Pre-hole depth
M M [PF] ;PF 1/8 DIAMETER_1=97280
;Diameter(1/10000mm)
THREAD_1=280
;Number of Thread(1/10Thread)
PRE_DIA_1=88600
;Diameter of Prehole(1/10000mm)
← Tap outside diameter ← Total threads ← Pre-hole diameter
M M [PS] ;PS1/8 DIAMETER_1=97280
;Diameter(1/10000mm)
THREAD_1=280
;Number of Thread(1/10Thread)
DEPTH_1=155000
;Depth(1/10000mm)
PRE_DIA_1=85000
;Diameter of Prehole(1/10000mm)
PRE_DEP_1=183100
;Depth of Prehole(1/10000mm)
M M
3-38
← ← ← ← ←
Tap outside diameter Total threads Thread depth Pre-hole diameter Pre-hole depth
PROGRAM CREATION
B.
3
Text data items - Tap outside diameter (Setting unit: 1/10000 mm) This item denotes the auto-setting values for MAJOR-φ of the tapping unit/counterbore-tapping unit and HOLE-φ in the tool sequence for the tap. (PT, PF, and PS pipe threads) - Total threads (Setting unit: 1/10 threads) This item refers to the total number of threads per inch of a tap, and this value is used for auto-setting PITCH of the tapping unit/counterbore-tapping unit. (PT, PF, and PS pipe threads) - Thread depth (Setting unit: 1/10000 mm) This item denotes the auto-setting value for TAP-DEP of the tapping unit/counterbore-tapping unit. (PT and PS pipe threads) - Pre-hole diameter (Setting unit: 1/10000 mm) This item denotes the auto-setting values for NOM-φ and HOLE-φ in the last drill tool sequence whose automatic tool development will be conducted for the tapping unit/counterbore-tapping unit. (PT, PF, and PS pipe threads) - Pre-hole depth (Setting unit: 1/10000 mm) This item denotes the auto-setting value for HOLE-DEP in the last drilling tool sequence for which automatic tool development will be conducted for the tapping unit/counterbore-tapping unit. (PT and PS pipe threads)
C.
Editing procedure (1) Click the Start button and select “Programs” from the Start menu option. Then click “Explorer”. (2) After copying “Pipescdt.org” (an auto-setting model file for pipe thread tapping) within the “C:nm64mdata” directory into this directory, change the file name to “Pipescdt.txt”. (3) Open “Pipescdt.txt” using a commercially available editor. (4) Edit the file seeing the above description of “Text file format” and “Text data items” and taking notice of each data unit. An example of editing is shown below. Note 1: If data is not entered correctly, alarm 494 AUTO TAP PROCESS IMPOSSIBLE will be displayed when auto-setting is executed. Enter data within the following range: Item
Keyword
Input unit
Tap outside diameter*
DIAMETER
1/10000 mm
10
999990
THREAD
1/10 threads
26
2147483647
Total threads Thread depth*
Minimum value
Maximum value
DEPTH
1/10000 mm
10
9999990
Pre-hole diameter*
PRE_DIA
1/10000 mm
100
9999000
Pre-hole depth*
PRE_DEP
1/10000 mm
100
9999000
Enter integral decimal numbers. * For these items always enter “0” as the least significant digit (that is, the last digit).
3-39
3
PROGRAM CREATION
Note 2: Even within the above data range, the particular combination of data settings in each item may display an asterisk (∗) to indicate that the amount of chamfering cannot be calculated. In such a case, to ensure that the amount of chamfering will be calculated properly, enter data in each item so that the calculation results in the following calculation expressions range from “0” to “99.9”: [If parameter D44 is set to “0”] (Chamfering) = {(Tap outside diameter) + (Thread pitch) × 2 – (Prehole diameter)}/2 [If parameter D44 is set to “1”] (Chamfering) = {(Tap outside diameter) – (Prehole diameter)}/2 Note 3: Even when data within the above data range is entered, alarm 416 AUTO PROCESS IMPOSSIBLE may be displayed during automatic development of the tool data. Note 4: Entered prehole diameter and depth values have their respective last two digits cut away. (5) After editing the file, execute “Overwrite & Save”. (6) Close “Explorer”. D.
Example of editing For “PT1/8”, proceed as follows to auto-set 10.117 mm as the tap outside diameter, 27 as the number of threads, 11 mm as the thread depth, 8.43 mm as the prehole diameter, and 17 mm as the prehole depth: (1) Open the text file “Pipescdt.txt” and move the cursor to “PT1/8”. (2) Move the cursor to each masked item required units. Do not edit other items.
shown below and then edit data in the
[PT] ;PT 1/8 DIAMETER_1=101170
;Diameter(1/10000mm)
THREAD_1=270
;Number of Thread(1/10Thread)
DEPTH_1=110000
;Depth(1/10000mm)
PRE_DIA_1=84300
;Diameter of Prehole(1/10000mm)
PRE_DEP_1=170000
;Depth of Prehole(1/10000mm)
M M
Note 1: Since the default settings of the text file data conform to the conventional scheme, auto-set data cannot be modified by merely changing the value of bit 0 in the D95 parameter. Note 2: When modifying the thread tapping auto-set data, the user itself needs to edit and manage the text file. Note 3: After text file editing, the new data is incorporated into the auto-set data immediately. Note 4: Even for inch specifications, assign data in units of 1/10000 mm to the text file. Note 5: Since auto-set data having an assigned decimal point and exceeding the minimum allowable number of digits cannot be displayed, text file modifications may not be displayed as auto-settings intact. Example:
Even if the value of PRE_DIA_1 is changed to 62500, a nominal drill diameter of 6.3 may be displayed as its auto-set value.
3-40
PROGRAM CREATION
3-5-6
3
Tool sequence data of the point machining unit The tool sequence data are automatically developed by entering the machining unit. However, certain data must be set by means of menu keys or numeric keys on the basis of the tool used or the machining procedure. Table 3-1 Tool sequence data TOOL
NOM-φ
No.
#
CTR DR
$
$ $ $
$
$
$
#
#
DRILL
$
$ $ $
$
$
$
$
$
CHAMFER
$
$ $ $
$
$
$
$
END MILL
$
$ $ $
$
$
$
$
BCK FACE
$
$ $ $
$
$
$
$
REAMER
$
$ $ $
$
$
$
$
TAP
$
$ $ $
$
$
$
BOR BAR
$
$ $ $
$
$
$
B-B BAR
$
$ $ $
$
$
Reference
1
2
5
6
3
4
HOLE-φ HOLE-DEP PRE-DIA PRE-DEP
RGH
DEPTH
C-SP
FR
M
M
M
#
$
#
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
#
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
#
$
#
#
$
$
$
$
$
#
#
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
$
7
8
9
10
11
12
13
14
15
15
15
$ : Setting possible. # : Not necessary to be set here.
Remark 1: For setting of each data item refer to 1 to 15 below. Remark 2: If [TAPPING CYCLE] menu item is selected for PRE-DIA, there is no need to set data in PRE-DEP. 1.
TOOL Used to specify the name of the tool to be used for machining. The tool designation can be changed by means of menu keys. CENTER DRILL
2.
DRILL
CHAMFER ENDMILL BACKSPOT REAMER CUTTER FACER
TAP
BORING BAR
BACK BOR.BAR
NOM-φ (Nominal diameter) Used to specify the nominal diameter of the tool by means of numeric keys. Note:
3.
The alarm 434 NO ASSIGNED TOOL IN TOOL FILE is given if the tool entered has not been previously recorded in the TOOL FILE display.
NOM-φ (Tool identification code) A code should be selected out of the menu to identify those tools which are of identical type (having an identical name) and have an identical nominal diameter. A
B
C
D
E
F
G
H
HEAVY TOOL
>>>
In order to designate a heavy tool, first of all press the [HEAVY TOOL] menu key to reverse the menu display and then select the desired menu key in the menu thus displayed.
3-41
3
PROGRAM CREATION
4.
NOM-φ (Turret selection) For the machine with the lower turret, select the turret in which the tool to be used is mounted. The following menu is displayed (if [SET UPPER TURRET] is selected, the column will remain blank, and if [SET LOWER TURRET] is selected, “ ” will be displayed). See Section 5, LOWERTURRET CONTROL FUNCTIONS, for further details: SET UPPER TURRET
5.
SET LOWER TURRET
No. (Priority No.) Assign priority levels in the order of machining. The following menu is displayed. A press of a menu key displays the menu item in reverse mode, allowing a priority number to be assigned. DELAY PRIORITY
(a)
PRI.No. PRI.No. CHANGE ASSIGN
(b)
PRI.No. SUB PROG ALL ERAS PROC END
(c)
(d)
(e)
The function of menu item (a) to (e) is described below: Menu item
Function
(a)
Select to conduct subsequent-machining.
(b)
Select to change the priority number for the tool within the particular process. If the cursor is present at a blank space, assign a new number in a usual manner. Entry of an existing priority number displays alarm 420 SAME DATA EXISTS.
(c)
Select to assign a priority number to the tool to be used repeatedly in the particular process. Alarm 420 SAME DATA EXISTS will be displayed if the assigned priority number has already been set on any other unit line.
(d)
Selection of this item displays message ALL ERASE (PROC:0, PROG:1)?. Setting 0 will erase the priority numbers preassigned to the tool to be used repeatedly in the process. Setting 1 will erase the priority numbers preassigned to the tool to be used repeatedly in the program.
(e)
Select to terminate the process with the subprogram unit.
For details see Chapter 4, “PRIORITY FUNCTION FOR THE SAME TOOL.” 6.
# (Retraction position of the lower turret) For a machine having upper and lower turrets, it is possible to specify the position to which the lower turret is to be retracted when machining workpieces using only the upper turret. The following menu is displayed. For details see Chapter 5, “LOWER-TURRET CONTROL FUNCTIONS.” LOWER TURRET POS.1
LOWER TURRET POS.2
3-42
PROGRAM CREATION
7.
3
HOLE-φ (Diameter of machining hole) Used to specify the diameter of the hole to be machined. The data for this article can be modified by means of numeric keys. Note:
For the chamfering cutter, this concerns a value equal to twice the distance from the centerline of the hole to an interference. Enter 999 if there is no interference. Charmfering if there is interference
Chamfering if there is no interference
20
Hole-φ = 40
Hole-φ = 999 M3P112
Fig. 3-2 Specification of diameter of machining hole for chamfering cutter
8.
HOLE-DEP (Depth of machining hole) Used to specify the depth of the hole to be machined. The data for this article can be modified by means of numeric keys. Note 1: For the chamfering cutter, this article is specified as illustrated below. [1]
20
[3]
[2]
[1] Depth of machining hole = 0 [2] Depth of machining hole = 20
[3] Depth of machining hole = 0 M3P113
Fig. 3-3 Specification of depth of machining hole
Note 2: For planetary tapping, the appropriate data for the selected type of tool must be set. Enter the data specified in the corresponding tool catalogue. Enter the catalogued cutting edge length in HOLE-DEP.
Cutting edge length
D735P0072
3-43
3
PROGRAM CREATION
9.
PRE-DIA (Diameter of pre-hole) Used to specify the diameter of the pre-hole for the final hole to be machined. The data for this article can be modified by means of numeric keys. Note 1: In the case of boring, the boring cycle can be selected from the menu. [CYCLE 1] is selected at the time of automatic tool development. CYCLE 1
CYCLE 2
CYCLE 3
For details, refer to Subsection 3-5-7 “Tool path of the point machininig unit”, “8. Boring tool”. Note 2: For back boring, enter the diameter of the through hole. Note 3: In the case of tapping, the tapping cycle can be selected from the menu. [TAPPING CYCLE] is selected at the time of automatic tool development. TAPPING PECKING CYCLE CYCLE
PLANET CYCLE
[TAPPING CYCLE]
Conventional tappping cycle
[PECKING CYCLE]
Pecking cycle using a synchronous tap
[PLANET CYCLE]
Machining cycle using a planetary tapping tool (only for machines with the Y-axis)
For details, refer to Subsection 3-5-7 “Tool path of the point machininig unit”, “7. Tap”. 10. PRE-DEP (Depth of the pre-hole) Used to specify the depth of the pre-hole for the final hole to be machined. The data for this article can be modified by means of numeric keys. Note 1: Enter the depth of the through hole in the case of back facing or back boring for this article. Note 2: Enter the depth of the faced hole in the case of boring for this article. Consequently, preset data of 0 is displayed for through hole boring and non-through hole boring. Note 3: Enter the interference depth in the case of chamfering for this article. Note 4: For the end mill, the direction of cutting can be selected from the menu. [CCW CUT] is selected at the time of automatic tool development. CW CUT
CCW CUT
For the tornado cycle of the circular milling unit, the direction of cutting can be selected from the following menu: CW CUT
CCW CUT
For details, refer to Subsection 3-5-7 “Tool path of the point machininig unit”, “4. End mill”. Note 5: Data setting is not required for [TAPPING CYCLE]. Set “Cutting depth per peck” for [PECKING CYCLE]. The value of the D50 parameter “Pre-hole machining feed” is set for [PLANET CYCLE] automatically.
3-44
PROGRAM CREATION
3
11. RGH (Cutting surface roughness) Enter the cutting surface roughness by means of numeric keys or menu keys. ▼ 1
▼ 2
▼▼ 3
▼▼ 4
▼▼▼ 5
▼▼▼ 6
▼▼▼ 7
▼▼▼▼ 8
▼▼▼▼ 9
Note 1: For the centering drill, the angle of tool tip can be selected from the menu. In automatic tool development mode, 90° is selected. 90o
118o
60o
Note 2: For the drill, the drilling cycle can be selected from the menu. In automatic tool development mode, these data are automatically determined on the basis of the machining depth, the drill diameter and the parameters concerned. DRILLING PECKING PECKING PECKING AUTOPECK CYCLE CYCLE 1 CYCLE 2 CYCLE 3 CYCLE
DECREME PECKING CYCLE 1
DECREME PECKING CYCLE 2
DECREME PECKING CYCLE 3
For details, refer to Subsection 3-5-7 “Tool path of the point machininig unit”, “2. Drill”. Note 3: Enter the duration of the dwell time for the tapping (invalid for synchronous tapping). In automatic tool development mode, FIX is selected. In this case, the dwell time is set by parameter D22. Note 4: For end mill (Tornado cycle) During automatic tool development, the system sets the same value as for the BTM item of the circular milling unit. If the BTM item value of the circular milling unit is 0, bottom finishing will not occur. Unless the BTM item value is 0, bottom finishing will occur. 12. DEPTH (Cutting depth) Used to specify the cutting depth or the amount of chamfering at the time of the machining according to the type of tool: - Cutting depth on Z-axis per pass in the case of drill. - Amount of chamfering in the case of chamfering cutter. - Radial cutting depth or amount of chamfering in the case of circular milling cycle or tornado milling cycle of the end mill, respectively. - In the case of boring with a reamer, specify the return speed of the reamer (as feed per minute) by means of menu keys or numeric keys. In tool automatic development mode [CUT G01] (cutting feed) is selected. CUT G01
RAPID G00
Cutting feed speed is selected by parameter D18. - Thread pitch in the case of tap. - Cutting depth in the radial direction in the case of boring bar and back boring tool.
3-45
3
PROGRAM CREATION
13. C-SP (Surface speed) To auto-set a surface speed (m/min) and feedrate (mm/rev), select the corresponding tool material type from the menu. The tool material types in the menu are the same as those which have been set on the CUTTING CONDITION - W. MAT./T. MAT. display. To register new tool material types, refer to Section of “CUTTING CONDITION - W. MAT./T. MAT. Display”, of the relevant Operating Manual. HSS AUTO
CARBIDE AUTO
Data can also be set using the numeric keys. 14. FR (Feedrate) Used to specify the feedrate of the tool. Same as the surface speed, the entry of data is done by means of menu keys or numeric keys. 15. M (M-code) Set the required M-code(s) to be output immediately after mounting the tool onto the spindle in the ATC mode. A maximum of up to three M-codes may be entered. It is also possible, moreover, to select and enter a general M-code out of the menu.
3-46
PROGRAM CREATION
3-5-7
Tool path of the point machining unit This section shows the path of each tool used during execution of a point machining unit. The initial and reference points in each tool path are as shown below. - When the selected mode is ZC or ZY TC37 Initial point
Reference point
TC37
D734P0006
- When the selected mode is XC or XY Reference point
Initial point
TC39 TC39
D734P0007
- When the selected mode is XC or XY Initial point
Reference point
TC40 TC40
D734P0008
3-47
3
3
PROGRAM CREATION
- When the selected mode is /C or /Y
TC39 Initial point
Reference point TC39
TC39 Initial point
TC39 Reference point
D734P0009
D734P0010
- When the selected mode is /C or /Y
TC40 Initial point
TC40 Reference point
D734P0011
3-48
PROGRAM CREATION
1.
3
Centering drill The cycle of machining with a centering drill is available in the following three types. A
Drilling cycle
Chamfering cycle B
Cycle 1
C
Cycle 2
Rapid feed
Rapid feed
Rapid feed
Cutting feed
Cutting feed
Cutting feed
D735P0130
Remark: Two types of chamfering cycles are provided: “Cycle 1”, which only moves the tool in the Z-axial direction during machining, and “Cycle 2”, which moves the tool in X- and Y-axial directions in addition to the Z-axial direction. Which of the two cycles is to be used for actual machining is automatically selected during operation. For details of the tool paths in the two cycles, see Items A to C below.
3-49
3
PROGRAM CREATION
A.
Centering drilling cycle Machining
After machining
Rapid feed Cutting feed [1] Movement to the intial point above center of hole to be machined Case of return to the initial point Pi
Pi [2] Movement to the R-point Case of return to the R-point
R
R Clearance
[5] Movement to the point R or to the initial point
[3] Machining by cutting feed
Pz
Clearance Pz
h
h
[4] Delayed stop at bottom of hole M3P114 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz
h:
Depth of the hole to be calculated by the data HOLE-φ and RGH (angle of tool tip) entered in the tool sequence and also the data LENG COMP. (tool correction) on the TOOL DATA display Diameter of machining hole h= tan (
Note:
2 Angle of cutting tool tip 2
+ Tool correction )
The time of delayed stop of the axial feed at bottom of hole is set by the parameter D3.
3-50
PROGRAM CREATION
B.
3
Cycle 1 of chamfering cycle Machining
After machining
Rapid feed Cutting feed
Rapid feed
[1] Movement to the initial point above center of hole
Case of return to the initial point
Pi
Pi [2] Movement to the R-point Case of return to the R-point R
R Clearance
[5] Movement to the point R or to the initial point
[3] Chamfering
Clearance
Pz
Pz h
h [4] Delayed stop at bottom of hole
D735P0131 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz
h:
Optimum distance to be automatically calculated by the data PRE-DIA and RGH in the tool sequence and also the data CHMF in the point machining unit.
Note:
The time of delayed stop of the axial feed at bottom of hole is set by the parameter D16.
3-51
3
PROGRAM CREATION
C.
Cycle 2 of chamfering cycle Machining
After machining
Rapid feed
Rapid feed Cutting feed
[1] Movement to the initial point above center of hole to be machined
Case of return to the initial point
Pi
Pi [2] Movement to the R-point Case of return to the R-point R
R [5] [3] Chamfering
Movement to the Rpoint or to the initial point
Pz h
Clearance
Pz h [4] Circular milling along the hole D735P0132 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz Note:
When the following condition is fulfilled, R before machining will be equaled to the parameter D42. However, R after machining is always equaled to the (safety) clearance. - Case where the bit 7 of parameter D91 is 1.
h:
The optimum distance is automatically calculated by the data PRE-DIA and RGH of the tool sequence and also the data CHMF in the point machining unit.
Note:
For the circular milling, refer to the paragraph dealing with 4. End mill, C. Cycle 3.
3-52
PROGRAM CREATION
2.
3
Drill The cycle of machining with drill is available in the following eight types.
A. DRILLING CYCLE
B. Deep-hole drilling cycle (PECKING CYCLE 2)
D. Very deep-hole drilling cycle (PECKING CYCLE 3)
C. High speed deep-hole driilling cycle (PECKING CYCLE 1)
E. Auto-pecking cycle of the cutting load detection type (AUTOPECK CYCLE) The cutting load torque of the drill is continually monitored during the auto-pecking cycle of the cutting load detection type. This pecking cycle will be performed only when required, which prevents tool breakage and reduces machining time. F. Deep-hole drilling cycle for gradual depth reduction (DECREME. PECKING CYCLE 2) In this machining cycle, the cutting depth is decremented with respect to a normal deep-hole drilling cycle each time the workpiece is cut. G. High speed deep-hole drilling cycle for gradual depth reduction (DECREME. PECKING CYCLE 1) In this machining cycle, the cutting depth is decremented with respect to a high deep-hole drilling cycle each time the workpiece is cut. H. Very deep-hole drilling cycle for gradual depth reduction (DECREME. PECKING CYCLE 3) In this machining cycle, the cutting depth is decremented with respect to a very deep-hole drilling cycle each time the workpiece is cut.
Rapide feed Cutting feed D734P0012
Remark 1: See Items A to H for the tool paths in each cycle. Remark 2: Specify the decremental cutting depth in parameter D45, and the minimum cutting depth, in parameter D46. Remark 3: For both “Very deep-hole drilling cycle” and “Very deep-hole drilling cycle for gradual depth reduction”, three types of machining cycle are available: Very deep-hole drilling cycle, Very deep stop-hole drilling cycle and Very deep through-hole drlling cycle.
3-53
3
PROGRAM CREATION
A.
Drilling cycle Machining
After machining Rapid feed Cutting feed
[1] Movement to the intial point above center of hole to be machined
Case of return to the initial point
Pi
Pi [2] Movement to the R-point Case of return to the R-point
R
R
Clearance
[6] Movement to the R-point or to the initial point
[3] Machining by first cutting feed f1
[6]
Pz
Clearance Pz
h
h [4] Machining by second cutting feed f2
hb
[5] M3P116 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz Note:
When the following two conditions are fulfilled, R before machining will be equaled to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance. - Case where the bit 6 of parameter D91 is 1. - Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.
h:
Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction
hb: Feedrate override distance from the hole bottom to be determined by the data PRE-DIA to be set for the tool sequence f1:
Feedrate (FR) to be set for the tool sequence
f2:
Feedrate to be modified by the data PRE-DEP (feedrate updating rate) f2 = f1 × Feedrate updating rate
3-54
3
PROGRAM CREATION
B.
Deep-hole drilling cycle (PECKING CYCLE 2) Machining
After machining
Rapid feed Cutting feed [1]
Case of return to the initial point Pi
Pi [2] Clearance R Pz
Case of return to the R-point R
[7] [3]
[8]
[5]
[4]
Pz
q F13
Clearance
[6]
[11]
q F13
[10] hb [5] Movement to the position determined by F13 [6] Machining by first cutting feed f1 [8] Movement to the position [7] Movement to the R-point determined by F13 [9] Repetition of [5] to [7] to bottom of hole [10]Machining by second cutting feed f2
[1] Movement to the initial point above the center of hole to be machined [2] Movement to the R-point [3] Machining by first cutting feed f1 [4] Movement to the R-point
h
[9]
[11]Movement to the R-point or to the initial point
M3P117
The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz Note:
When the following two conditions are fulfilled, R before machining will be equaled to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance. - Case where the bit 6 of parameter D91 is 1. - Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.
h:
Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction
q:
Cutting depth (DEPTH) to be entered in the tool sequence data
hb: Feedrate override distance from the hole bottom to be determined by the data PRE-DIA to be set for the tool sequence f1:
Feedrate (FR) to be set for the tool sequence
f2:
Feedrate to be modified by the data PRE-DEP (feedrate updating rate) f2 = f1 × Feedrate updating rate
3-55
3
PROGRAM CREATION
C.
High-speed hole drilling cycle (PECKING CYCLE 1) Machining
After machining
Rapid feed Cutting feed
[1]
Case of return to the initial point Pi
Pi [2]
Case of return to the R-point R
Clearance R [3] Pz
Pz
q F12
Clearance
[5] [4]
[9]
q F12
h
[7]
[6] [8] hb [1] Movement to the initial point [5] Machining to the position above center of hole determined by q [2] Movement to the R-point [6] Movement to the position [3] Machining by first cutting of F12 [7] Repetition of [5] and [6] feed f1 down to bottom of hole [4] Movement to the point F12 [8] Machining by second cutting feed f2
[9] Movement to the R-point or to the initial point
M3P118 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz Note:
When the following two conditions are fulfilled, R before machining will be equaled to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance. - Case where the bit 6 of parameter D91 is 1. - Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.
h:
Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction
q:
Cutting depth (DEPTH) to be entered in the tool sequence data
hb: Feedrate override distance from the hole bottom to be determined by the data PRE-DIA to be set for the tool sequence f1:
Feedrate (FR) to be set for the tool sequence
f2:
Feedrate to be modified by the data PRE-DEP (feedrate updating rate) f2 = f1 × Feedrate updating rate
Note:
The feed speed on the paths [4] and [6] is 9999 mm/min or 999.9 inch/min for millimeter or inch specification respectively.
3-56
PROGRAM CREATION
D.
Very deep-hole drilling cycle (PECKING CYCLE 3) Machining
After machining
Rapid feed
Rapid feed Cutting feed
Case of return to the initial point
[1] Pi Clearance R Pz
Dwell D56
a q
f3
L
Pz
D55 f2
Pi Case of return to the R-point R
[2]
f1 [3]
q
3
f2 [5]
[4]
D55
q
f3
Clearance
[9]
[6]
[7] [8] f2
h
D55 f2
q
[10]
[14] D55
f2 [12]
f3 [11] [13] Dwell D56
q
[1] Movement to the initial [6] Movement by D55 to [9] Movement by D55 to [12] Repetition of [7] point the retraction position the advanced position and [9] down to [2] Movement to the R-point at feedrate f3 bottom of hole from the previous [3] Machining of “a” at feed [7] Movement by q at machining end position[13] After movement rate f1 and movement by feedrate f2 [10] Movement by q at feed to bottom of q at feedrate f2 [8] After D53 times hole, wait for rate f2 [4] Movement by D55 to the peckings, movement [11] Movement by D55 to D56 rotations retraction position at to the chip ejection the retraction position feed rate f3 position and wait for at feedrate f3 [5] Movement by q at D56 rotations feedrate f2
[14] Movement to the Rpoint or to the initial point
D734P0013'
The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz Note:
When the following two conditions are fulfilled, R before machining will be equaled to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance. - Case where the bit 6 of parameter D91 is 1. - Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.
h:
Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction
a:
Cutting area (Note 3)
q:
Cutting depth (DEPTH) to be entered in the tool sequence data
f1:
Feedrate (infeed rate) obtained by multiplying “f2” by the “reduction ratio of the starting speed of cutting” specified in parameter D54 where, if D54 = 0 or if D54 > 100, then D54 = 100. D54 f1 = f2 × 100
f2:
Feedrate (FR) to be set for the tool sequence
f3:
Pecking retraction speed (= setting of parameter D57) where, if D57 = 0, then D57 = 1000.
3-57
3
PROGRAM CREATION
L:
Chip ejection distance calculated from the data ACT-φ (tool diameter: D) and data LENG COMP. (tool correction) on the TOOL DATA display D L = Data LENG COMP.– 10 (D: Tool diameter)
Note 1: During the “n”th cutting operation, if (q × n) < D55, retraction through the D55-specified distance does not occur. During machining on the path [3], if the first cutting depth of “q” is greater than or equal to (Clearance at R-point + Cutting area “a” ), machining at feedrate “f1” will occur on the path [3] until (Clearance at R-point + Cutting area “a” ) is reached, then retraction through the D55-specified distance from that position will occur on the path [4], and the workpiece will be cut to the next cutting position (next cutting depth) on the path [5]. Note 2: The feedrate on the path [8] is “G0 speed × D52/100”. (If the input value of D52 is 0, then D52 = 100.) Note 3: Cutting area Machining pattern: Very deep hole drilling cycle a=K+R Where K is LENG COMP. (tool correction) on the TOOL DATA display and R is the clearance. Machining pattern: Very deep stop-hole or very deep through-hole drilling cycle D58 a = D × 100 Where D is the tool diameter and D58 (parameter) is the feedrate updating distance rate at the start of cutting. If D58 > 300, D58 is taken to be 100. If a < R, a is taken to be equal to R. Under the conditions shown below, alarm 748 CANNOT MAKE T-PATH (CHK DEPTH) will be issued. [1] If a > r and a ≥ 2q:
[2] If a ≤ r and r ≥ q:
R-point
R-point r
r
q
a
q
Start point
Start point a
q
End point
End point [3] If a ≥ c and c ≥ q
R-point r
q
Start point a
c
a: q: r: hb: c:
Cutting area 1st cutting depth Clearance Deceleration distance Cutting distance before deceleration
Note: As for a gradual depth reduction cycle, the constant cutting depth (before gradual depth reduction) is compared to the values concerned.
hb
End point
D740PA146
Fig. 3-4
3-58
PROGRAM CREATION
3
Note 4: For very deep stop-hole or very deep through-hole drilling cycles, the feedrate or the surface speed can be changed in some cases within the feedrate updating distance from the hole bottom (hb specified under PRE-DIA of the tool sequence). Machining pattern: Very deep stop-hole drilling cycle When hb (feedrate updating distance from the hole bottom) is reached, machining by second cutting feed f4 starts. The surface speed is kept at the speed (S1) set as C-SP in the tool sequence. (Fig. 3-5) Let Q represent the feedrate updating rate (specified under PRE-DEP of the tool sequence). Then second cutting feed f4 can be calculated from feed f2 set as FR in the tool sequence, using the following equation. Q f4 = f2 × 100 If Q = 0, Q is taken to be 100. If Q > 200, alarm 402 ILLEGAL NUMBER INPUT will be issued.
Distance to the hole bottom h hb
Surface speed: S1 Feedrate: f4 D740PA147 Fig. 3-5
Machining pattern: Very deep through-hole drilling cycle When hb (feedrate updating distance from the hole bottom) is reached, machining by second surface speed S2 and second cutting feed f4 starts. On the return path (G0/G1) after reaching hb, the tool operates at second surface speed S2. After the tool has finished machining and returned to its initial point, its speed returns to first surface speed S1. Second surface speed S2 is calculated from surface speed (S2) set as C-SP in the tool sequence and the surface speed updating rate (set with the parameter D59), using the following equation. D59 S2 = S1 × 100 If D59 = 0 or D59 > 100, D59 is taken to be 100. Let Q represent the feedrate updating rate (specified under PRE-DEP of the tool sequence). Then, second cutting feed f4 can be calculated from feed f2 set for the tool sequence, using the following equation. Q f4 = f2 × 100 If Q = 0, Q is taken to be 100. If Q > 200, alarm 402 ILLEGAL NUMBER INPUT will be issued.
3-59
3
PROGRAM CREATION
Distance to the hole bottom h hb
Surface speed: S2 Feedrate: f4
D740PA148
Fig. 3-6
If hb > h (PRE-DEP of the tool sequence), hb is taken to be equal to h. If the cutting area (a) and the feedrate updating distance from the hole bottom (hb) overlap each other: 1)
If a and hp overlap between the R-point and the start point: Between the R-point and the start point, feedrate f1 for the cutting area (a) is valid and surface speed S1 set as C-SP in the tool sequence is used. Between the start point and the end point, however, feedrate f4 specified for the feedrate updating distance (hb) is valid. (Fig. 3-7)
R-point f1 Start point a f4 hb
End point
D740PA149
Fig. 3-7
2)
If a and hb overlap between the start point and the end point: Feedrate f4 for the feedrate updating distance (hb) is valid and second surface speed S2 is used. (Fig. 3-8)
R-point f1
Start point a
f4
End point
hb
D740PA150
Fig. 3-8
3-60
PROGRAM CREATION
3
Figures below show the relationship between feedrate updating distance from the hole bottom (hb) and each cutting depth (q)/last cutting depth (qn). [1] If feedrate updating distance (hb) < last cutting depth (qn):
[2] If last cutting depth (qn) ≤ feedrate updating distance (hb) ≤ (qn + D55):
f2
f2
q
q f2 D55 f3
D55
f4 f3
f2
qn
qn f4
f4
hb
hb
[3] If (qn + D55) < feedrate override distance (hb):
f2 f2 q
f4 f2
D55
f3 qn
f4
hb
D740PA150 Fig. 3-9
Note 5: Hole bottom dwell [13] in the figure of tool path for “D. Very deep-hold drilling cycle (PECKING CYCLE 3)” is executed when the deceleration distance is zero, but not when it is more than zero (for very deep stop-hole or very deep through-hole drilling cycles or very deep stop-hole or very deep through-hole drilling cycles with a gradual depth reduction).
3-61
3
PROGRAM CREATION
E.
Auto-pecking cycle of the cutting load detection type (Option) (AUTOPECK CYCLE) The cutting load torque of the drill is continually monitored during the auto-pecking cycle of the cutting load detection type. This pecking cycle will be performed only if the cutting load exceeds its reference value. Machining
After machining
Rapid feed
Rapid feed Cutting feed
Case of return to the initial point [1]
Pi
R
Case of return to the R-point
[2]
Clearance [3]
Pz
Pi
[7]
R
[5]
[4]
Pz [8]
Clearance
F13 P1
[6] P2
[11]
F13
h
[9]
[1] Movement to the initial point [5] Movement to the position hb [10] of F13 above center of hole [6] Machining by first cutting [2] Movement to the R-point [8] Movement to the position of feed f1 [3] Machining by first cutting F13 [7] Movement to the R-point feed f1 occurs if the cutting load [9] Repetition of [5] to [7] to [4] Movement to the R-point bottom of hole exceeds its reference occurs if the cutting load [10] Machining by second cutting value exceeds its reference value feed f2
[11] Movement to the R-point or to the initial point D735P0073
The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence P1, P2: The positions where autonomous pecking will occur if the cutting load exceeds its reference value R:
Safety clearance above the point Pz Note: When the following two conditions are fulfilled, R before machining will be equaled to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance. - Case where the bit 6 of parameter D91 is 1. - Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.
h:
Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction
hb: Feedrate override distance from the hole bottom to be determined by the data PRE-DIA to be set for the tool sequence f1:
Feedrate (FR) to be set for the tool sequence
f2:
Feedrate to be modified by the data PRE-DEP (feedrate updating rate) f2 = f1 × Feedrate updating rate
Note:
Cutting load reference value (pecking threshold value) must be set using the DRILL MONITOR function of the MACHIN. MONITOR display mode.
3-62
PROGRAM CREATION
3
F. Deep-hole drilling cycle for gradual depth reduction cycle (DECREME PECKING CYCLE 2) Machining
After machining
Rapid feed Cutting feed
Rapid feed Case of return to the initial point
[1] Pi
Pi [2]
R Pz
Case of return to the R-point R
Clearance [3]
q1
[5]
[4]
[8]
[7]
Pz
F13
Clearance [6]
qi
F13
[11]
[9]
h
[10]
hb
[1] Movement to the initial point [5] Movement to the position [8] Movement to the position above the center of hole determined by F13 determined by F13 [2] Movement to the R-point [6] Machining by first cutting [9] Repetition of [5] and [7] to [3] Machining by first cutting feed f1 bottom of hole feed f1 [7] Movement to the R-point [10] Machining by second cutting [4] Movement to the R-point feed f2
[11] Movement to the R-point or to the initial point
D735P0074 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz Note:
When the following two conditions are fulfilled, R before machining will be equaled to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance. - Case where the bit 6 of parameter D91 is 1. - Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.
h:
Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction
q1 :
Cutting depth to be entered in the tool sequence data (first cutting depth)
qi:
i-th cutting depth The i-th cutting depth qi is calculated by the value of the D45 parameter for drilling gradual reduction depth and of the D46 parameter for minimum drilling depth as follows.
3-63
3
PROGRAM CREATION
1st cut
q1
D: Drilling depth q1: 1st cutting depth qi: i-th cutting depth qi = q1 – D45 × (i – 1) (qi ≥ D46) qi = D46 (qi < D46)
D
qi
i-th cut
D735P0075
hb: Feedrate override distance from the hole bottom to be determined by the data PRE-DIA to be set for the tool sequence f1:
Feedrate (FR) to be set for the tool sequence
f2:
Feedrate to be modified by the data PRE-DEP (feedrate updating rate) f2 = f1 × Feedrate updating rate
G.
High speed deep-hole drilling cycle for gradual depth reduction (DECREME PECKING CYCLE 1) Machining
After machining
Rapid feed Cutting feed
Rapid feed Case of return to the initial point
[1]
Pi
Pi
Case of return to the R-point
[2] R
Clearance
R [3]
[9] Pz
Pz
Clearance
q1 [4]
F12 [5]
[7]
h
qi
F12
[6]
[8] hb [1] Movement to the initial point above [5] Machining up to the position determined by qi the center of hole [6] Movement to the position [2] Movement to the R-point [7] Repetition of [5] and [6] to [3] Machining by first cutting feed f1 determined by F12 bottom of hole [4] Movement to the position [8] Machining by second cutting determined by F12 feed f2
[9] Movement to the R-point or to the initial point D735P0076
The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence
3-64
PROGRAM CREATION
R:
3
Safety clearance above the point Pz Note:
When the following two conditions are fulfilled, R before machining will be equaled to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance. - Case where the bit 6 of parameter D91 is 1. - Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.
h:
Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction
q1 :
Cutting depth to be entered in the tool sequence data (first cutting depth)
qi:
i-th cutting depth The i-th cutting depth q1 is calculated by the value of the D45 parameter for drilling gradual reduction depth and of the D46 parameter for minimum drilling depth as follows.
q1
1st cut D: Drilling depth q1: 1st cutting depth qi: ith cutting depth qi = q1 – D45 × (i – 1) (qi ≥ D46) qi = D46 (qi < D46)
D
qi
i-th cut
D735P0075
hb: Feedrate override distance from the hole bottom to be determined by the data PRE-DIA to be set for the tool sequence f1:
Feedrate (FR) to be set for the tool sequence
f2:
Feedrate to be modified by the data PRE-DEP (feedrate updating rate) f2 = f1 × Feedrate updating rate
Note:
The feed speed on the paths [4] and [6] is 9999 mm/min or 999.9 inch/min for milimeter or inch specification respectively.
3-65
3
PROGRAM CREATION
H.
Very deep-hole drilling cycle for gradual depth reduction (DECREME PECKING CYCLE 3) Machining
After machining
Rapid feed
Rapid feed Cutting feed
Case of return to the initial point
[1] Pi R Pz
f1 [3]
q1
Dwell D56
a q2
f3
L
Pz
D55 f2
Pi Case of return to the R-point R
[2]
Clearance
f2 [5]
[4]
q3
f3
[6]
Clearance
[9] D55
[7] [8] f2
h
D55 f2[10]
q4
[14] D55
q5
f3
[ ] f2 12
[11] [13] Dwell D56
[1] Movement to the initial [6] Movement by D55 to [9] Movement by D55 to [12] Repetition of [7] point the retraction position the advanced position and [9] down to [2] Movement to the R-point at feedrate f3 from the previous bottom of hole [3] Machining of “a” at feed [7] Movement by q at machining end position [13] After movement rate f1 and movement by feedrate f2 [10] Movement by q at to bottom of q at feedrate f2 [8] After D53 times hole, wait for feedrate f2 [4] Movement by D55 to the peckings, movement [11] Movement by D55 to D56 rotations retraction position at to the chip ejection the retraction position feedrate f3 position and wait for at feedrate f3 [5] Movement by q at D56 rotations feedrate f2
[14] Movement to the Rpoint or to the initial point
D734P0013'
The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz Note:
When the following two conditions are fulfilled, R before machining will be equaled to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance. - Case where the bit 6 of parameter D91 is 1. - Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.
h:
Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction
a:
Cutting area Machining pattern: Very deep hole drilling cycle with a gradual depth reduction a=K+R Where K is LENG COMP. (tool correction) on the TOOL DATA display and R is the clearance.
3-66
PROGRAM CREATION
3
Machining pattern: Very deep stop-hole or very deep through-hole drilling cycle with a gradual depth reduction D58 a = D × 100 Where D is the tool diameter and D58 (parameter) is the feedrate updating distance rate at the start of cutting. If D58 > 300, D58 is taken to be 100. If a < R, a is taken to be equal to R. Alarm 748 CANNOT MAKE T-PATH (CHK DEPTH) will be issued under some conditions. For details, see Fig. 3-4 in Note 3 of “D. Very deep-hold drilling cycle (PECKING CYCLE 3).” q1: Cutting depth (DEPTH) to be entered in the tool sequence data qi:
i-th cutting depth The i-th cutting depth q1 is calculated by the value of the D45 parameter for drilling gradual reduction depth and of the D46 parameter for minimum drilling depth as follows. Note:
If the setting of parameter D46 is 0 (zero), the minimum allowable cutting depth is 1 mm (or in inch units, 0.04 inches).
q1
1st cut D: Drilling depth q1: 1st cutting depth qi: ith cutting depth qi = q1 – D45 × (i – 1) (qi ≥ D46) qi = D46 (qi < D46)
D
qi
i-th cut
D735P0075
f1:
Feedrate (infeed rate) obtained by multiplying “f2” by the “reduction ratio of the starting speed of cutting” specified in parameter D54 where, if D54 = 0 or if D54 > 100, then D54 = 100. D54 f1 = f2 × 100
f2:
Feedrate (FR) to be set for the tool sequence
f3:
Pecking retraction speed (= setting of parameter D57) where, if D57 = 0, then D57 = 1000.
L:
Chip ejection distance calculated from the data ACT-φ (tool diameter: D) and data LENG COMP. (tool correction) on the TOOL DATA display D L = Data LENG COMP.– 10 (D: Tool diameter)
3-67
3
PROGRAM CREATION
Note 1: During the “n”th cutting operation, if (q × n) < D55, retraction through the D55-specified distance does not occur. During machining on the path [3], if the first cutting depth of “q” is greater than or equal to (Clearance at R-point + Cutting area “a” ), machining at feedrate “f1” will occur on the path [3] until (Clearance at R-point + Cutting area “a” ) is reached, then retraction through the D55-specified distance from that position will occur on the path [4], and the workpiece will be cut to the next cutting position (next cutting depth) on the path [5]. Note 2: The feedrate on the path [8] is “G0 speed × D52/100”. (If the input value of D52 is 0, then D52 = 100.) Note 3: For very deep stop-hole and very deep through-hole drilling cycles with a gradual depth reduction, the feedrate or the surface speed can be changed in some cases within the feedrate updating distance from the hole bottom (hb specified under the PRE-DIA in the tool sequence). For details, refer to Note 4 of “D. Very deep-hold drilling cycle (PECKING CYCLE 3).” 3.
Chamfering cutter Chamfering is classified into two types: Chamfering performed by the tool which only moves on the Z-axis (Cycle 1) and chamfering performed by the tool which moves on the X-, Y- and Z-axes (Cycle 2). The cycle used is selected automatically. A. Cycle 1
B. Cycle 2
NM210-00544 Fig. 3-10
Cycle 1 and cycle 2
Feedrates that are automatically determined vary according to the machining cycle selected. The feedrate in cycle 1 is the feedrate calculated by multiplying the automatically determined feed rate for cycle 2 by the setting of the parameter D60 (%). The feed rate in cycle 1 is displayed yellow. Parameter D60: Automatic setting ratio of axial cutting feed rate during chamfering in the point machining The following shows the tool path of the chamfering cutter in each cycle.
3-68
PROGRAM CREATION
A.
3
Cycle 1 Machining
After machining
Rapid feed Cutting feed
[1] Movement to the initial point above center of hole
Case of return to the initial point
Pi
Pi [2] Movement to the R-point Case of return to the R-point
R
R
Clearance
[5] Movement to the point R or to the initial point
[3] Chamfering
Clearance Pz
Pz h
h [4] Delayed stop at bottom of hole
M3P119 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz
h:
Optimum distance to be automatically calculated by the data HOLE-φ and HOLE-DEP in the tool sequence and also the data ANG on the TOOL FILE display
Note:
The time of delayed stop of the axial feed at bottom of hole is set by the parameter D16.
3-69
3
PROGRAM CREATION
B.
Cycle 2 Machining
After machining
Rapid feed Cutting feed [1] Movement to the initial point above center of hole to be machined
Case of return to the initial point Pi
Pi [2] Movement to the R-point
Case of return to the R-point R
R [5] [3] Chamfering
Movement to the point R or to the initial point
Clearance
Pz h
Clearance
Pz h [4] Circle milling along the hole
M3P120 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz Note:
When the following condition is fulfilled, R before machining will be equaled to the parameter D42. However, R after machining is always equaled to (safety clearance). - Case where the bit 7 of parameter D91 is 1.
h:
The optimum distance is automatically calculated by the data HOLE-φ and HOLE-DEP of the tool sequence and also the data ANG on the TOOL FILE display.
Note 1: The time of delayed stop of the axial feed at bottom of hole is set by the parameter D16. Note 2: For the circular milling, refer to the paragraph dealing with 4. End mill, C. Cycle 3.
3-70
PROGRAM CREATION
4.
3
End mill According to the set value in item TORNA., one of the following three machining patterns is selected. TORNA.: 0 .........circular milling cycle 1 .........circular tornado milling cycle 2 .........precision rapid boring tornado cycle For tool path of each machining pattern refer to the relevant description below. End milling is divided into the following three types according to the machining hole diameter, the pre-hole diameter and the nominal diameter entered in the tool sequence. At the time of operation, the appropriate cycle is automatically selected. 1.
For RGH CBOR and CBOR-TAP units - Diameter of machining hole = Nominal diameter (Cycle 1) - “Diameter of machining hole > Nominal diameter” and “Diameter of pre-hole > (Tool diameter + Safety clearance)” (Cycle 2) - “Diameter of machining hole > Nominal diameter” and “Diameter of pre-hole ≤ (Tool diameter + Safety clearance)” (Cycle 3)
2.
For units other than those mentioned above - Diameter of machining hole = Tool diameter (Cycle 1) - “Diameter of machining hole > Tool diameter” and “Diameter of pre-hole > (Tool diameter + Safety clearance)” (Cycle 2) - “Diameter of machining hole > Tool diameter” and “Diameter of pre-hole ≤ (Tool diameter + Safety clearance)” (Cycle 3)
Note:
The safety clearance is determined by the parameter D23. A.
Cycle 1
B.
Cycle 2
C.
Cycle 3
NM210-00545 Fig. 3-11
Circular milling cycles 1, 2 and 3
The following shows the tool path of the end mill in each cycle.
3-71
3
PROGRAM CREATION
A.
Cycle 1 Machining
After machining Rapid feed Cutting feed
[1] Movement to the initial point above center of machining hole Case of return to the initial point
Pi
Pi
[2] Movement to the R-point Case of return to the R-point
Clearance R
R Movement to the R-point [5] or to the initial point
[3] Machining to bottom of hole
Pz
Clearance Pz h
h
[4] Delayed stop at bottom of hole
M3P121 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz
h:
Depth of machining hole (HOLE-DEP) to be entered in the tool sequence
Note:
The time of delayed stop of the axial feed at bottom of hole is set by the parameter D19.
3-72
PROGRAM CREATION
B.
3
Cycle 2 Machining
After machining
Rapid feed Cutting feed [1] Movement to the initial point above center of machining hole
Case of return to the initial point
Pi
Pi [2] Movement to the R-point
Clearance R
Case of return to the R-point R Clearance
[3] Movement to the machining position
Pz
Pz q
q
[4]
h
[5] Movement to the point R or to the initial point
Circular milling (Repetition of circular milling to bottom of the hole)
h
q
hf
Circular milling
M3P122 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz
h:
Optimum distance to be automatically calculated by the data HOLE-φ and HOLE-DEP in the tool sequence and also the data ANG on the TOOL FILE display
hf:
Bottom finishing allowance to be determined by the data RGH entered in the tool sequence and also by the parameter D21
q:
Cutting depth in the axial direction per pass to be determined by: h – hf h – hf (Whole part of cmx
)+1
(cmx = Data DEPTH entered in TOOL FILE display) Note:
For the circular milling, see Cycle 3 below.
3-73
3
PROGRAM CREATION
C.
Cycle 3 Machining
After machining
Rapid feed Cutting feed [1] Movement to the initial point above center of machining hole
Case of return to the initial point
Pi
Pi [2] Movement to the R-point
Clearance R
Case of return to the R-point R
[3] Movement to the machining position
Pz
Clearance Pz
q
q
[4]
h q
hf
Circular milling (Repetition of circular milling to bottom of the hole)
[5] Movement to the R-point or to the initial point
h
Circular milling M3P123
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz
h:
Optimum distance to be automatically calculated by the data HOLE-φ and HOLE-DEP in the tool sequence and also the data ANG on the TOOL FILE display
hf:
Bottom finishing allowance to be determined by the data RGH entered in the tool sequence and also by the parameter D21
q:
Cutting depth in the axial direction per pass to be determined by: h – hf h – hf ( Whole part of cmx
)+1
(cmx = Data DEPTH entered in TOOL FILE display) Note:
The feed speed on the tool paths [3] and [4] is equaled to the parameter E17, if bit 0 of parameter D92 is set at 1.
3-74
PROGRAM CREATION
3
Circular milling Circular milling is automatically selected according to the diameter of the machining hole, the diameter of the pre-hole and the cutting depth entered in the tool sequence of the program. Start
No
Cutting (Hole dia. – Pre-hole dia.) depth < 2
Yes Circular milling - A
Circular milling - B
Diameter of pre-hole after machining = Diameter of pre-hole + (2 × amount of cutting depth)
End
M3P124 Fig. 3-12
Note: 1.
Circular milling
In the Cycle 3, the pre-hole diameter (data entered in tool sequence) is equal to the tool diameter (data entered in the TOOL DATA display).
Circular milling-A The movement of circular milling-A is as shown below. Cutting feed
End mill Cutting depth
[3] [1] [2]
Pre-hole diameter Machining hole diameter Fig. 3-13
M3P125
Circular milling-A
- The cutting direction (CW or CCW) can be designated in the program. Note:
The cutting direction designated for the spindle No. 2 is opposite to that for the spindle No. 1.
- The movement is done in the order [1]→[2]→[3]. - The movement of [1] starts with the end point of the preceding circular milling-A.
3-75
3
PROGRAM CREATION
2.
Circular milling-B The movement of circular milling-B is as shown below. Cutting feed
End mill
[3] [5]
Cutting depth
[4] [2] [1]
Pre-hole diameter
Fig. 3-14
Machining hole diameter
M3P126
Circular milling-B
- The movement is done in the order [1]→[2]→[3]→[4]→[5]. - The cutting direction is set to the left. - The movement of [1] starts with the end point of the preceding circular milling-A. Note:
However, when bit 4 (bit 5 in the case of chamfering) of parameter D91 is 1, the movement of [2] and [5] is done by the following shortened (rapid access) method.
Rapid feed Cutting feed
End mill
[4]
[3]
[6]
[1] [2]
[5]
Diameter of pre-hole
Fig. 3-15
Cutting depth
Diameter of machining hole
Circular milling-B (case of shortening in chamfering)
- Case of shortening (rapid access) in chamfering is shown above - The cutting direction (CW or CCW) can be designated in the program. - The movement is done in the order [1]→[2]→[3]→[4]→[5]→[6].
3-76
M3P127
PROGRAM CREATION
3
D735P0065
Machining
After machining
Rapid feed Cutting feed
[1] Movement to the initial point above center of machining hole
Case of return to the initial point Pi Clearance
Pi Case of return to the R-point
[2] Movement to the R-point
R
[3] After movement to the machining position helical milling is performed.
s Pz s
[4] Helical milling (repetition of herical milling to bottom of the hole)
q h q
q
R Clearance Pz [5] Movement to the R-point or to the initial point
h
Helical milling
D735P0066 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz
h:
Optimum distance to be automatically calculated by the data HOLE-φ and HOLE-DEP in the tool sequence and also the data ANG on the TOOL FILE display
q:
PITCH 2 to be entered in the CIRC MIL unit.
s:
PITCH 1 to be entered in the CIRC MIL unit.
3-77
3
PROGRAM CREATION
Circular milling (1) With bottom finishing The operation of the machine when it is programmed to perform bottom finishing operations is shown in Fig. 3-16. Rapid feed Cutting feed
D735P0067
Fig. 3-16
Circular helical processing (with bottom finishing)
After helical interpolation down to the bottom of the hole, one entire circumference of arc interpolation occurs. Next, the tool moves to the center of the hole and then moves in the rapid feed rate to its initial point or to R-point in the axial direction. (2) Without bottom finishing The operation of the machine when it is not programmed to perform bottom finishing operations is shown in the Fig. 3-17. Rapid feed Cutting feed
Returning through a quarter pitch in the axial direction
D735P0068
Fig. 3-17
Circular helical processing (without bottom finishing)
After helical interpolation down to the bottom of the hole, the tool moves to the center of the hole by returning through a quarter pitch in the axial direction and then moves in rapid feed rate to its initial point or to R-point in the axial direction. The bottom of the hole does not undergo arc interpolation.
3-78
PROGRAM CREATION
3
D735P0077
The tool path of end mill is as shown below. Machining
After machining
Rapid feed Cutting feed
Rapid feed
[1] Movement to the initial point above center of machining hole Case of return to the initial point
Pi
Pi
Clearance R q
[2] Movement to the R-point [3] After movement to the machining position helical milling is performed
Case of return to the R-point R Clearance
Pz
Pz
[4] Helical milling (repetition of helical milling to bottom of the hole)
q h q
[7] Movement to the R-point or to the initial point
h
[5] Circular interpolation at botom of the hole [6] Relief to the center of the arc
q
D735P0078
Pi: Pz: R: h: q:
Initial point Start point to be entered in the shape sequence Safety clearance above the point Pz HOLE-DEP in the tool sequence Pitch 2 to be entered in the CIRC MIL unit. The cutting depth on Z per pass “q” should not be greater than the data entered at DEPTH in TOOL FILE display.
Note 1: The precision rapid boring tornado cycle (setting 2 at item TORNA.) requires the shape correction option. Note 2: The precision rapid boring tornado cycle (setting 2 at item TORNA.) is valid only on the G17 plane.
3-79
3
PROGRAM CREATION
Circular milling The movement of circular milling is as shown below. Rapid feed Cutting feed [1] Positioning on the helical interpolation path at rapid feedrate [2] Helical interpolation to bottom of the hole [3] One round of circular interpolation Cutting at bottom of the hole depth [4] Relief of the tool on half round of circular interpolation to the center
[2] [3] End mill
[4] [1]
Pre-hole diameter
D735P0079
Machining hole diameter Fig. 3-18
Circular milling
- The movement is done in the order [1]→[2]→[3]→[4]. - The cutting direction (CW or CCW) can be designated in the program. - The single block function is invalid during the sequence of [2]→[3]→[4]. If the single block function is specified, the program will come to a single-block stop at the ending point of [4]. The feed hold function, however, is valid. Note:
However, when bit 4 of parameter D91 is 1, the movement of [4] is done by the following shortened (rapid access) method. Rapid feed Cutting feed [2][3] End mill Cutting depth [5] [1] [4]
Pre-hole diameter
Fig. 3-19
Machining hole diameter
Circular milling (case of shortening in chamfering)
- The cutting direction (CW or CCW) can be designated in the program. - The movement is done in the order [1]→[2]→[3]→[4]→[5].
3-80
D735P0080
PROGRAM CREATION
5.
3
Back facing tool Before machining
Machining
Cutting feed
Rapid feed Cutting feed
The cutting edge is in the retracted state
After machining Cutting feed
[1] Movement to the initial point above the center of hole
Initial point
Pi
[2] Movement to the R-point 1 R-point 1
R1
Clearance
[9] Movement to the initial point
[6] Delayed stop at bottom of hole
Pz1
Start point hs
[3]
Movement to the R-point 2
h Pz2
[5] Machining to h
Clearance R-point 2
[7] Movement to the Rpoint 2
[4] Rotation of the spindle to the right by M03
[8]
R2
Rotation of the spindle to the left by M04
M3P128 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz1:
Start point to be entered in the shape sequence
Pz2:
Position at a distance of hs from Pz1
R1, R2: Safety clearance above the points Pz1, Pz2 respectively Note:
As for R1 (in Step [2]), the setting of parameter D1 becomes valid in case Bit 1 of parameter D92 is set to “1.” R1-position after machining, however, is always determined by the (safety) clearance.
h:
Depth of hole (HOLE-DEP) to be entered in tool sequence
hs:
Distance equal to the sum of the depth of pre-hole entered in the tool sequence and the tool data LENG COMP. (tool correction) on the TOOL DATA display
Note 1: The time of delayed stop of the feed in the axial direction at bottom of hole is set by the parameter D40. Note 2: Feed speed on the tool path [3] and [9] is set by the parameter D5. Note 3: The rotation of the spindle to the right is performed by M03 entered in the tool sequence, whilst the rotation to the left is performed by M04.
3-81
3
PROGRAM CREATION
6.
Reamer Machining
After machining
Rapid feed Cutting feed
[1] Movement to the initial point above center of hole
Return to the initial point
Pi
Pi [2] Movement to the R-point
[5] Movement to the initial point
R
R Clearance
[3] Boring with reamer
[4] Movement to the R-point
Pz
Pz h
M3P129
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz Note:
When the following two conditions are fulfilled, R before machining will be equaled to the parameter D1. However, R after machining is always equaled to the (safety) clearance. - Case where the bit 2 of parameter D92 is 1. - Case where the respective tool sequence contains a chamfering cutter as premachining tool.
h:
Distance equal to the sum of the depth of hole (HOLE-DEP) entered in the tool sequence and the data LENG COMP. (tool correction) on the TOOL DATA display
Note:
The feed speed of the tool path [4] is determined as follows by the data DEPTH in the tool sequence. When [CUT G01] menu key is pressed ............... Parameter D18 When [RAPID G00] menu key is pressed .............. Rapid feed When the value is entered in the item DEPTH .......... Entered value (/min)
3-82
PROGRAM CREATION
7.
Tap The cycle of machining with tap is available in the following three types. A. TAPPING CYCLE
B. PECKING CYCLE 2
Rapid feed Cutting feed
Rapid feed Cutting feed
C. PLANET CYCLE
Rapid feed Cutting feed
Rapid feed Cutting feed
Case without movement for chip evacuation
Case with movement for chip evacuation D735P0081
Remark: See Items A to C for the tool paths in each cycle.
3-83
3
3
PROGRAM CREATION
A.
Tapping cycle (TAPPING CYCLE) Machining
After machining
Rapid feed Cutting feed [1] Movement to the initial point above center of hole Pi
Execution of M03 after delayed stop [7]
[2] Movement to the R-point
D31
[8] Movement to the R-point R
R Clearance
[3] Movement to the position ha
Pi [8] Movement to the initial point
Clearance
[6] Movement to the position D31 with rotation of spindle to the left by M04
Pz
Pz h
h
ha [5]
[4] Execution of M04 after delayed stop
M3P130 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz Note:
When the following two conditions are fulfilled, R before machining will be equaled to the parameter D1. However, R after machining is always equaled to the (safety) clearance. - Case where the bit 3 of parameter D92 is 1. - Case where the respective tool sequence contains a chamfering cutter as premachining tool.
h:
Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction
ha: Distance to be determined by (A – D32) × Pt A ......D30 when using metric and unified screws, D43 when using pipe screws Pt .....Pitch entered in the machining unit Note 1: The entry of 1 in the bit 0 to 2 of parameter D91 causes the following delayed stop. Bit 0 ......... Delayed stop before execution of M04 at bottom of hole [4] Bit 1 ......... Delayed stop after execution of M04 at bottom of hole [5] Bit 2 ......... Delayed stop before execution of M03 after return [7] Moreover, the delayed stop is entered in the item RGH in the tool sequence. If CYCLE FIX is selected, it will be determined by the parameter D22. Note 2: When M04 is entered in the tool sequence, inversed tapping will be executed.
3-84
PROGRAM CREATION
B.
3
Deep hole drilling cycle (PECKING CYCLE 2) Machining
After machining
Rapid feed
Cutting feed
Cutting feed Case of return to the initial point
[1] Pi
Pi Case of return to the R-point R
[2] Clearance
R
[3]
Pz
[5]
[4]
[6]
[7]
Pz
q
Clearance h [8]
q [1] Movement to the initial point above the center of [5] Machining to the cutting ha hole to be machined depth per peck from [2] Movement to the R-point machining surface [3] Machining to the cutting [6] Movement to the R-point [7] Repetition of [5] to [6] depth per peck by M04 after delayed stop to the position ha [4] Movement to the R-point by M04 after delayed stop
Pi:
h
[8] Movement to the R-point by M04 after delayed stop M3P117
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz Note:
When the following two conditions are fulfilled, R before machining will be equaled to the parameter D1. However, R after machining is always equaled to the (safety) clearance. - Case where the bit 3 of parameter D92 is 1. - Case where the respective tool sequence contains a chamfering cutter as premachining tool.
h:
Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction
ha: Distance to be determined by (A – D32) × Pt A .... D30 when using metric and unified screws, D43 when using pipe screws Pt .... Pitch entered in the machining unit q:
Cutting depth (DEPTH) to be entered in the tool sequence data
Note 1: The entry of 1 in the bit 0 to 2 of parameter D91 causes the following delayed stop. Bit 0 ......... Delayed stop before execution of M04 at bottom of hole [4] Bit 1 ......... Delayed stop after execution of M04 at bottom of hole [5] Bit 2 ......... Delayed stop before execution of M03 after return [7] Moreover, the delayed stop is entered in the item RGH in the tool sequence. If CYCLE FIX is selected, it will be determined by the parameter D22. Note 2: When M04 is entered in the tool sequence, inversed tapping will be executed.
3-85
3
PROGRAM CREATION
C.
Planetary tapping (PLANET CYCLE) The planetary tapping cycle allows three types of machining (pre-hole machining, chamfering, and female threading) with one tool. A machining pattern is selected by the parameter D92. - Set either 0 or 1 in the bit 6. 0
1
D82 = 7 6 5 4 3 2 1 0 bit 6
No movement for chip evacuation before threading
Movement for chip evacuation before threading
D735P0084
The following shows the tool path in each cycle.
3-86
3
PROGRAM CREATION
Case without movement for chip evacuation Machining
After machining
Rapid feed Cutting feed
Rapid feed Cutting feed [1]
Case of return to the initial point Pi
Pi [2]
Case of return to the R-point R
Clearance R [3]
Pz
Pz
[8]
Clearance h [7]
[4]
[9]
h
[6] [5] [1] Movement to the initial point above center of hole [2] Movement to the R-point [3] Machining of (Hole depth – [4] Slow machining down [6] to hole bottom for chamfering stroke) chamfering [5] Relief in the axial [7] direction [8]
Approach by G03-based helical cutting in the axial direction G03-based threading Return to hole center
[9] Movement to the R-point or to the initial point
D735P0082
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz
h:
Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence
Note 1: The inversed tapping cannot be executed. Note 2: The feed rate for chamfering on tool path [4] is calculated as follows: Chamfering feed = Pre-hole machining feed × Chamfering feed override (parameter D48)/100 Note 3: The amount of return from hole bottom on tool path [5] is calculated as follows: Amount of return = Tapping pitch × Number of thread (parameter D49)/10 Note 4: The tool diameter in the tool data is modified for tapping diameter correction (fineadjustment). Note 5: The depth of the section tapped by the actual machining becomes smaller than that of the thread set in the program.
3-87
3
PROGRAM CREATION
Case with movement for chip evacuation Machining
After machining Rapid feed
Rapid feed Cutting feed [1]
Case of return to the initial point
Pi
Pi
[2]
Case of return to the R-point R
Clearance R [5]
[3]
Pz
[6] Pz
[9]
Clearance
h [8] [4]
[5] Movement to the R[1] Movement to the initial point point for chip above center of hole evacuation [2] Movement to the R-point [6] Movement to the [3] Machining of (Hole depth – tapping start position chamfering stroke) [4] Slow machining down to hole bottom for chamfering
[10]
h
[7]
[7] Approach by G03-based helical cutting in the axial direction [8] G03-based threading [9] Return to hole center
[10] Movement to the R-point or to the initial point
D735P0085
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz
h:
Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence
Note 1: The inversed tapping cannot be executed. Note 2: The feed rate for chamfering on tool path [4] is calculated as follows: Chamfering feed = Pre-hole machining feed × Chamfering feed override (parameter D48)/100 Note 3: The distance from hole bottom to the tapping start position on tool path [6] is calculated as follows: Distance from hole bottom to the tapping start position = Tapping pitch × Number of thread (parameter D49)/10 Note 4: The tool diameter in the tool data is modified for tapping diameter correction (fineadjustment). Note 5: The depth of the section tapped by the actual machining becomes smaller than that of the thread set in the program.
3-88
PROGRAM CREATION
8.
3
Boring tool The path of the boring tool is classified in 9 types on the basis of the contents of the program, as shown in the figure below. Table 3-2 Tool path of the boring tool Run-off on Z-axis Yes/No.
Delayed stop Yes/No.
Cycle 1
2
3
A
Roughness 0
Run-off distance
No
No D25
M19
B
Roughness 1
Run-off distance No
Yes
D25
M19
D24
D24
D24
C
Roughness 2-9
Run-off distance Yes
Yes
D28 M19
D25 D26
D24
D24 Rapid feed
D28
D28
D26
D26
D24
Cutting feed
M3P131 The bold codes represent the parameter addresses.
In the following, M19, D24, D25, D26 and D28 shown on the figure above, are explained. M19: M-code to stop the spindle in the pre-determined position (Orientation of spindle) D24: Parameter to determine delayed stop time. The machining is done in excess of the delayed stop time which serves to improve the precision of the hole machining.
3-89
3
PROGRAM CREATION
D25: Parameter to determine the run-off distance on the X-Y plane. (Refer to Fig. 3-20.) The spindle is oriented at the bottom of the hole. The tool moves to the initial point or to R-point after clearance of the machining surface. This is used for the finish machining because any damage to the machining surface can be prevented at the time of the return of the tool. Workpiece to be machined
Tool Oriented position
Run-off distance of XY plane M3P132
Fig. 3-20
Run-off distance on the X-Y plane
D26: Parameter to determine the run-off distance on the Z-axis. The feed speed is reduced to 70% of the programmed value, which allows to improve the machining precision. D28: Parameter to determine the finishing allowance at the bottom of the hole. The feed speed is reduced to 70% of the programmed value, which allows to improve the machining precision. In order to simplify the description, three pattern cycles are described: Cycle 1—Roughness 0, Cycle 2—Roughness 1, and Cycle 3—Roughness 2 to 9. General precautions concerning the path of the boring tool” is also given at the end of the description of cycles.
3-90
PROGRAM CREATION
A.
Cycle 1 with roughness 0 Machining
After machining
Movement to the point of approach and execution of M03 (Rotation of the spindle to the right) Pi
D25
M03
[1] Movement to the initial point above center of hole Pi [2] Movement to the R-point
R
[6]
R
Clearance
Pz
[3] Machining to bottom of hole h
3
M19
Pz Movement to the initial point or to the R-point
[5]
Stop of the spindle by M19 (Oriented stop of spindle) and movement to the position specified by parameter D25.
[4]
Rapid feed Cutting feed D25
M3P133
The bold codes represent the parameter addresses.
Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz h: Distance equal to the sum of the depth of hole (HOLE-DEP) entered in the tool sequence and the data LENG COMP. (tool correction) in the TOOL DATA display Note 1:
Direction of run-off distance on the XY plane (bit 3 and bit 4 of parameter I14)
Note 2:
When M04 is entered in the tool sequence, the spindle rotates to the right.
B.
Cycle 2 with roughness 1 Machining
After machining
[1] Movement to the initial point above center of hole Pi
Pi [2] Movement to the R-point
R
R
Clearance
Pz
Pz
[3] Machining to bottom of hole
h
Movement to the initial point or to the R-point
[4] Delayed stop
[5] Rapid feed Cutting feed M3P134
D24
The bold codes represent the parameter addresses.
Pi: Initial point Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz
h:
Distance equal to the sum of the depth of hole (HOLE-DEP) entered in the tool sequence and the data LENG COMP. (tool correction) in the TOOL DATA display
Note:
The delayed stop time of the axial feed at the bottom of the hole is set by the parameter D24.
3-91
3
PROGRAM CREATION
C.
Cycle 3 with roughness 2 to 9 Machining
After machining
Rapid feed Cutting feed
[1] Movement to the initial point above center of hole Pi
Pi [7] Movement to the initial point
[2] Movement to the R-point R
R
Clearance
Pz
Pz [3] Machining to the position specified by parameter D28
h [4]
D28 Delayed stop D24
Movement to the R-point
[6]
Movement to the position specified by parameter D26
[5]
D26
Machining to bottom of hole M3P135 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz
h:
Distance equal to the sum of the depth of hole (HOLE-DEP) entered in the tool sequence and the data LENG COMP. (tool correction) in the TOOL DATA display
Note 1: The feed speed [4] and [5] is 70% on the programmed value. Note 2: The feed speed [6] is set by the parameter D18. Note 3: The delayed stop time of the axial feed at bottom of hole is set by the parameter D24.
3-92
PROGRAM CREATION
9.
Back boring tool Before machining
Machining
Movement to the initial point above center of hole, then execution of M19 ds
[1] M19
Pi
3
After machining
Movement to the position D26, then execution of M19
Movement of ds, then execution of M03
[10] Pi
Movement of ds [2]
M03
R
R Movement to the Clearance initial point [9]
Delayed stop Pz [3]
[6] hs
Movement of ds, [4] then execution of M03 ds M03
Clearance R2
hs [7]
h
Clearance
Pz
D26
D26 [8] Movement of ds
[5] Machining to bottom of hole
Rapid feed Cutting feed
M3P136 The bold codes represent the parameter addresses.
Pi:
Initial point
Pz:
Start point to be entered in the shape sequence
R, R2:
Safety clearance in the axial direction
h:
Distance equal to the sum of the depth of hole (HOLE-DEP.) entered in the tool sequence and the data LENG COMP. (tool correction) on the TOOL DATA display
hs:
Depth of pre-hole (PRE-DEP) to be entered in the tool sequence
ds:
Run-off distance on the XY plane determined by
d1 – d 2 2
+ D33
d1 ............ Diameter of hole (HOLE-φ) entered in the tool sequence d2 ............ Diameter of pre-hole (PRE-DEP) entered in the tool sequence D33 .......... Movement on the XY plane entered in the parameter Note 1: The direction of movement [2] and [7] are determined by the data set in bit 3 and bit 4 of parameter I14, respectively. The direction of movement [4] and [10] is opposite to that of [2]. Note 2: The delayed stop time of the axial feed is set by the parameter D40.
3-93
3
PROGRAM CREATION
General precautions concerning the path of the boring tool Stepped hole boring and non-stepped hole boring differ in the path of the tool to the machining starting point. Case of non-stepping boring
Case of stepped boring
[1] [1] Movement to the initial point above center of hole Pi
Initial point
[2] Movement to the clearance position and hs
[2] Movement to the R-point
R-point
[3] Machining
Start point
R Clearance
Pz hs
h
h
Machining [3]
Clearance
Rapid feed Cutting feed M3P137
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance in the axial direction
h:
Distance equal to the sum of the depth of hole (HOLE-DEP) entered in the tool sequence and the data LENG COMP. (tool correction) in the TOOL DATA display
hs: Depth of pre-hole (PRE-DEP) to be entered in the tool sequence Note:
Cutting start point is moved from R-point to a distance specified in hs (depth of prehole).
3-94
PROGRAM CREATION
3
10. Chip vacuuming tool (option) Movement 1
Movement 2
[1] Movement to the initial point above center of hole
Return to the initial point Pi
Pi [4] Movement to the initial point
[2] Movement to the R-point
R
R [3] Delayed stop Clearance
Pz
Pz
Rapid feed
Pi:
Initial point
Pz: Start point to be entered in the shape sequence R:
Safety clearance above the point Pz
Note:
The delayed stop time of the axial feed is set by the parameter D29.
3-95
3
PROGRAM CREATION
3-5-8
Shape sequence data of the point machining unit The machining unit and tool sequence data has been set above. Next, set the shape sequence data for the point machining unit. 1.
Types of point maching shape Five types of point machining patterns are provided, and the shape that can be selected differs according to the mode (MODE) specified for the unit. !： Selection possible, ×： Selection impossible
Mode Shape
ZC
XC
XC
/C
/C
ZY
XY
XY
/Y
/Y
PT
!
!
!
!
!
!
!
!
!
!
ARC
!
!
!
!
!
!
!
!
!
!
LIN
×
×
×
×
×
!
!
!
!
!
SQR
×
×
×
×
×
!
!
!
!
!
GRD
×
×
×
×
×
!
!
!
!
!
Refer to the section 3-4-1 “Planes to be machined and machining methods“ for the detail of the modes.
3-96
PROGRAM CREATION
2.
Entry of shape sequence data A.
When the selected mode in the unit is ZC 1.
Point (PT)
D734P0014
FIG
PTN
SPT-R/x
SPT-C/y
SPT-Z
SPT-Y
NUM.
ANG
Q
R
1
PT
[1]
[2]
[3]
[4]
'
'
'
[5]
Cursor position
Description
[1] SPT-R/x
Specify the start point of the hole to be machined.
[2] SPT-C/y
- To set the start point in R-C coordinates, enter the radius and the angle as they are.
[3] SPT-Z
- To set the start point in x-y coordinates, change the [x-y INPUT] menu item to the reverse display mode before entering data.
[4] SPT-Y
–C
+C +Z
–Z
C=0
ｙ –Y
Z=0 Z
Y +Y
Start point
Start point
[5] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-97
R
C
ｘ
3
3
PROGRAM CREATION
2.
Arc (ARC)
D734P0015
FIG
PTN
SPT-R/x
SPT-C/y
SPT-Z
SPT-Y
NUM.
ANG
Q
R
1
ARC
[1]
[2]
[3]
[4]
[5]
[6]
[7]
[8]
Cursor position [1] SPT-R/x
Description Specify the start point of the hole to be machined.
[2] SPT-C/y
- To set the start point in R-C coordinates, enter the radius and the angle as they are.
[3] SPT-Z
- To set the start point in x-y coordinates, change the [x-y INPUT] menu item to the reverse display mode before entering data.
[4] SPT-Y
(See “1 Point (PT)” for further details.) [5] NUM.
Specify the number of holes to be drilled.
[6] ANG
Specify the angle between two adjacent holes.
ANG
[7] Q
Specify if the machining at the start point is executed or not. 0: Actual execution of machining 1: Only positioning without machining
[8] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-98
PROGRAM CREATION
B.
When the selected mode in the unit is XC, XC , /C or /C 1.
Point (PT)
[ XC ]
[ /C ]
[ XC ]
[ /C ]
D734P0016
FIG
PTN
SPT-R/x
SPT-C/y
SPT-Z
NUM.
ANG
Q
R
1
PT
[1]
[2]
[3]
'
'
'
[4]
Cursor position [1] SPT-R/x
Description Specify the start point of the hole to be machined.
[2] SPT-C/y
- To set the start point in R-C coordinates, enter the radius and the angle as they are.
[3] SPT-Z
- To set the start point in x-y coordinates, change the [x-y INPUT] menu item to the reverse display mode before entering data. +C
[ XC ] +Z
–C
–Z
C = 0°
Z=0
y
Z C Start point x
R
Start point
[ /C ]
+C +Z
–C
–Z Z
Z=0
C = 0°
y
C Start point R
Start point
[4] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-99
x
3
3
PROGRAM CREATION
2.
Arc (ARC)
[ XC ]
[ /C ]
[ XC ]
[ /C ]
D734P0017
FIG
PTN
SPT-R/x
SPT-C/y
SPT-Z
NUM.
ANG
Q
R
1
ARC
[1]
[2]
[3]
[4]
[5]
[6]
[7]
Cursor position [1] SPT-R/x
Description Specify the start point of the hole to be machined.
[2] SPT-C/y
- To set the start point in R-C coordinates, enter the radius and the angle as they are.
[3] SPT-Z
- To set the start point in x-y coordinates, change the [x-y INPUT] menu item to the reverse display mode before entering data. (See “1 Point (PT)” for further details.)
[4] NUM.
Specify the number of holes to be drilled.
[5] ANG
Specify the angle between two adjacent holes.
ANG
[6] Q
Specify if the machining at the start point is executed or not. 0: Actual execution of machining 1: Only positioning without machining
[7] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-100
PROGRAM CREATION
C.
When the selected mode in the unit is ZY 1.
Point (PT)
D734P0014
FIG
PTN
SPT-Z
SPT-Y
SPT-R
CZ/PZ
CY/PY
F
M
N
ANG
P
Q
R
1
PT
[1]
[2]
[3]
'
'
'
'
'
'
[4]
'
[5]
Cursor position [1] SPT-Z
Description Specify the start point of the hole to be drilled.
[2] SPT-Y
+Z
–Z
[3] SPT-R
Z
Start point
Y –Y
R
+Y
[4] P
Specify the tool path. Y
Hole to be drilled
P=1 P=0 P=2
Ｚ
Premachining or current position
[5] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-101
3
3
PROGRAM CREATION
2.
Arc (ARC)
D734P0018
FIG
PTN
SPT-Z
SPT-Y
SPT-R
CZ/PZ
CY/PY
F
M
N
ANG
P
Q
R
1
ARC
[1]
[2]
[3]
[4]
[5]
'
[6]
'
[7]
'
[8]
[9]
Cursor position
Description
[1] SPT-Z
Specify the start point of the hole to be machined.
[2] SPT-Y
(See “1 Point (PT)” for further details.)
[3] SPT-R [4] CZ/PZ
Specify the coordinate of the center of the arc.
[5] CY/PY
+Z
–Z Z=0
Start point
ANG ANG
CY/PY
–Y
CZ/PZ +Y
[6] M
Specify the number of holes to be drilled.
[7] ANG
Specify the angle between two adjacent holes. (See the figure of item [4] CZ/ PZ, [5] CY/ PY.)
[8] Q
Specify if the machining at the start point is executed or not. 0: Actual execution of machining 1: Only positioning without machining
[9] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-102
PROGRAM CREATION
3.
Line (LIN)
D734P0019
FIG
PTN
SPT-Z
SPT-Y
SPT-R
CZ/PZ
CY/PY
F
M
N
ANG
P
Q
R
1
LIN
[1]
[2]
[3]
[4]
'
'
[5]
'
[6]
'
[7]
[8]
Cursor position
Description
[1] SPT-Z
Specify the start point of the hole to be machined.
[2] SPT-Y
(See “1 Point (PT)” for further details.)
[3] SPT-R [4] CZ/PZ
Specify the pitch between two adjacent holes in the line of holes. –Ｚ
+Z
Z=0
CZ/PZ
Start point
CZ/PZ
ANG
–Ｙ
+Y
[5] M
Specify the number of holes to be drilled.
[6] ANG
Specify the angle formed by the line of holes and the Z-axis. (See the figure of the item [4] CZ/PZ.)
[7] Q
Specify if the machining at the start point is executed or not. 0: Actual execution of machining 1: Only positioning without machining
[8] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-103
3
3
PROGRAM CREATION
4.
Square (SQR)
D734P0020
FIG
PTN
SPT-Z
SPT-Y
SPT-R
CZ/PZ
CY/PY
F
M
N
ANG
P
Q
R
1
SQR
[1]
[2]
[3]
[4]
[5]
[6]
[7]
[8]
'
[9]
[10]
[11]
Cursor position
Description
[1] SPT-Z
Specify the start point of the hole to be machined.
[2] SPT-Y
(See “1 Point (PT)” for further details.)
[3] SPT-R [4] CZ/PZ
Specify the pitch between holes or the total length of the Z-axis.
CZ/PZ (Total length) CZ/PZ
CY/PY (Total length)
–Z
+Z CZ/PZ (Pitch)
CY/PY (Pitch)
Z=0
Start point
CY/PY
–Ｙ
+Y [5] CY/PY
Specify the pitch between holes or the total length of the Y-axis. (See the figure of the item [4] CZ/ PZ.)
[6] F
Specify whether the data entered in CZ/PZ and CY/PY concern the pitch or the total length. 0: Pitch 1: Total length
[7] M
Specify the number of holes on the line of holes of the Z-axis.
[8] N
Specify the number of holes on the line of holes of the Y-axis.
[9] P
Specify if the machining at the four corners is executed or not. 0: Machining at the four corners 1: No machining at the four corners
[10] Q
Specify if the machining at the start point is executed or not. 0: Actual execution of machining 1: Only positioning without machining
[11] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-104
PROGRAM CREATION
5.
Grid (GRD)
D734P0021
FIG
PTN
SPT-Z
SPT-Y
SPT-R
CZ/PZ
CY/PY
F
M
N
ANG
P
Q
R
1
GRD
[1]
[2]
[3]
[4]
[5]
[6]
[7]
[8]
'
[9]
[10]
[11]
Cursor position
Description
[1] SPT-Z
Specify the start point of the hole to be machined.
[2] SPT-Y
(See “1 Point (PT)” for further details.)
[3] SPT-R [4] CZ/PZ
Specify the pitch between holes or the total length of the Z-axis.
–Z
+Z CZ/PZ (Total length) CZ/PZ
CY/PY (Total length)
CZ/PZ (Pitch)
CY/PY (Pitch)
Z=0
Start point
CY/PY
–Y
+Y [5] CY/PY
Specify the pitch between holes or the total length of the Y-axis. (See the figure of the item [4] CZ/ PZ.)
[6] F
Specify whether the data entered in CZ/PZ and CY/PY concern the pitch or the total length. 0: Pitch 1: Total length
[7] M
Specify the number of holes on the line of holes of the Z-axis.
[8] N
Specify the number of holes on the line of holes of the Y-axis.
[9] P
Specify if the machining at the four corners is executed or not. 0: Machining at the four corners 1: No machining at the four corners
[10] Q
Specify if the machining at the start point is executed or not. 0: Actual execution of machining 1: Only positioning without machining
[11] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-105
3
3
PROGRAM CREATION
D.
When the selected mode in the unit is XY or XY 1.
Point (PT) [ XY ]
[ XY ]
D734P0022
FIG
PTN
SPT-R/x
SPT-C/y
SPT-Z
CX/PX
CY/PY
F
M
N
ANG
P
Q
R
1
PT
[1]
[2]
[3]
'
'
'
'
'
'
[4]
'
[5]
Cursor position [1] SPT-R/x
Description Specify the start point of the hole to be machined.
[2] SPT-C/y
- To set the start point in R-C coordinates, enter the radius and the angle as they are.
[3] SPT-Z
- To set the start point in x-y coordinates, change the [x-y INPUT] menu item to the reverse display mode before entering data. [ XY ]
+C
–C
–Z
+Z
Z=0
y
C = 0°
Z C Start point R
Start point
[4] P
Specify the tool path. Y
Hole to be drilled
P=1 P=0
P=2 Ｚ
Premachining or current position
[5] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-106
x
PROGRAM CREATION
2.
Arc (ARC)
[ XY ]
[ XY ]
D734P0023
FIG
PTN
SPT-R/x
SPT-C/y
SPT-Z
CX/PX
CY/PY
F
M
N
ANG
P
Q
R
1
ARC
[1]
[2]
[3]
[4]
[5]
'
[6]
'
[7]
'
[8]
[9]
Cursor position
Description
[1] SPT-R/x
Specify the start point of the hole to be machined.
[2] SPT-C/y
- To set the start point in R-C coordinates, enter the radius and the angle as they are.
[3] SPT-Z
- To set the start point in x-y coordinates, change the [x-y INPUT] menu item to the reverse display mode before entering data.
[4] CX/PX
Specify the coordinate of the center of the arc.
(See “1 Point (PT)” for further details.)
[5] CY/PY
+x
PositionＣ C=0
+ｙ
ANG ANG Start point CX/PX
CY/PY
[6] M
Specify the number of holes to be drilled.
[7] ANG
Specify the angle between two adjacent holes. (See the figure of the item [4] CX/ PX, [5] CY/ PY.)
[8] Q
Specify if the machining at the start point is executed or not. 0: Actual execution of machining 1: Only positioning without machining
[9] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-107
3
3
PROGRAM CREATION
3.
Line (LIN)
[ XY ]
[ XY ]
D734P0024
FIG
PTN
SPT-R/x
SPT-C/y
SPT-Z
CX/PX
CY/PY
F
M
N
ANG
P
Q
R
1
LIN
[1]
[2]
[3]
[4]
'
'
[5]
'
[6]
'
[7]
[8]
Cursor position
Description
[1] SPT-R/x
Specify the start point of the hole to be machined.
[2] SPT-C/y
- To set the start point in R-C coordinates, enter the radius and the angle as they are.
[3] SPT-Z
- To set the start point in x-y coordinates, change the [x-y INPUT] menu item to the reverse display mode before entering data. (See “1 Point (PT)” for further details.)
[4] CX/PX
Specify the pitch between two adjacent holes in the line of holes. +X ANG +Y CX/PX Start point
CX/PX
Position C
[5] M
Specify the number of holes to be drilled.
[6] ANG
Specify the angle formed by the line of holes and the Z-axis. (See the figure of the item [4] CX/ PX.)
[7] Q
Specify if the machining at the start point is executed or not. 0: Actual execution of machining 1: Only positioning without machining
[8] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-108
PROGRAM CREATION
4.
Square (SQR) [ XY ]
[ XY ]
D734P0025
FIG
PTN
SPT-R/x
SPT-C/y
SPT-Z
CX/PX
CY/PY
F
M
N
ANG
P
Q
R
1
SQR
[1]
[2]
[3]
[4]
[5]
[6]
[7]
[8]
'
[9]
[10]
[11]
Cursor position
Description
[1] SPT-R/x
Specify the start point of the hole to be machined.
[2] SPT-C/y
- To set the start point in R-C coordinates, enter the radius and the angle as they are.
[3] SPT-Z
- To set the start point in x-y coordinates, change the [x-y INPUT] menu item to the reverse display mode before entering data. (See “1 Point (PT)” for further details.)
[4] CX/PX
Specify the pitch between holes or the total length of the X-axis. +X
CY/PY (Total length) CY/PY (Pitch) CY/PY
+Y
CX/PX (Total length)
CX/PX(Pitch)
CX/PX Start point
Position C
[5] CY/PY [6] F
Specify the pitch between holes or the total length of the Y-axis. (See the figure of the item [4] CX/PX.) Specify whether the data entered in CX/PX and CY/PY concern the pitch or the total length. 0: Pitch 1: Total length
[7] M
Specify the number of holes on the line of holes of the X-axis.
[8] N
Specify the number of holes on the line of holes of the Y-axis.
[9] P
Specify if the machining at the four corners is executed or not. 0: Machining at the four corners 1: No machining at the four corners
[10] Q
Specify if the machining at the start point is executed or not. 0: Actual execution of machining 1: Only positioning without machining
[11] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-109
3
3
PROGRAM CREATION
5.
Grid (GRD) [ XY ]
[ XY ]
D734P0026
FIG
PTN
SPT-R/x
SPT-C/y
SPT-Z
CX/PX
CY/PY
F
M
N
ANG
P
Q
R
1
GRD
[1]
[2]
[3]
[4]
[5]
[6]
[7]
[8]
'
[9]
[10]
[11]
Cursor position
Description
[1] SPT-R/x
Specify the start point of the hole to be machined.
[2] SPT-C/y
- To set the start point in R-C coordinates, enter the radius and the angle as they are.
[3] SPT-Z
- To set the start point in x-y coordinates, change the [x-y INPUT] menu item to the reverse display mode before entering data. (See “1 Point (PT)” for further details.)
[4] CX/PX
Specify the pitch between holes or the total length of the X-axis.
+X
CY/PY (Total length) CY/PY (Pitch) CY/PY
+Y CX/PX (Total length)
CX/PX(Pitch)
CX/PX Start point
Position C [5] CY/PY [6] F
Specify the pitch between holes or the total length of the Y-axis. (See the figure of the item [4] CX/PX.) Specify whether the data entered in CX/PX and CY/PY concern the pitch or the total length. 0: Pitch 1: Total length
[7] M
Specify the number of holes on the line of holes of the X-axis.
[8] N
Specify the number of holes on the line of holes of the Y-axis.
[9] P
Specify if the machining at the four corners is executed or not. 0: Machining at the four corners 1: No machining at the four corners
[10] Q
Specify if the machining at the start point is executed or not. 0: Actual execution of machining 1: Only positioning without machining
[11] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-110
PROGRAM CREATION
E.
3
When the selected mode in the unit is /Y or /Y 1.
Point (PT) [ /Y ]
[ /Y ]
D734P0027
FIG
PTN
1
PT
SHIFT-Z SHIFT-R SPT-X SPT-Y CX/PX CY/PY
[1]
[2]
[3]
'
[4]
Cursor position [1] SHIFT-Z [2] SHIFT-R
'
F
M
N
ANG
'
'
'
'
P
Specify the value of shift from the work origin to the oblique plane (the distance to the program origin of the oblique plane).
SHIFT-R
Program origin of oblique plane
Specify the start point of the hole to be drilled.
[4] SPT-Y
+X
Y
+Y
X
[5] P
Specify the tool path.
X
Hole to be drilled P=2 P=0 P=1 Y Premachinining or current position
[6] R
R
Description
SHIFT-Z
[3] SPT-X
Q
[5] ' [6]
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-111
3
PROGRAM CREATION
2.
Arc (ARC)
[ /Y ]
[ /Y ]
D734P0028
FIG
PTN
1
ARC
SHIFT-Z SHIFT-R SPT-X SPT-Y CX/PX CY/PY
[1]
[2]
[3]
[4]
[5]
[6]
Cursor position [1] SHIFT-Z [2] SHIFT-R
F
M
N
ANG
'
[7]
'
[8]
Q
R
Description Specify the value of shift from the work origin to the oblique plane (the distance to the program origin of the oblique plane). (See “1 Point (PT)” for further details.)
[3] SPT-X
Specify the start point of the hole to be machined.
[4] SPT-Y
(See “1 Point (PT)” for further details.)
[5] CX/PX
Specify the central coordinates of the arc. Position C
[6] CY/PY
C=0 +X +Y ANG ANG Start point CX/PX
CY/PY
[7] M
Specify the number of holes to be drilled.
[8] ANG
Specify the angle between two adjacent holes. (See the figure of the item [5] CX/ PX, [6] CY/ PY.)
[9] Q
Specify if the machining at the start point is executed or not. 0: Actual execution of machining 1: Only positioning without machining
[10] R
P
' [9] [10]
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-112
PROGRAM CREATION
3.
3
Line (LIN)
[ /Y ]
[ /Y ]
D734P0029
FIG
PTN
1
LIN
SHIFT-Z SHIFT-R SPT-X SPT-Y CX/PX CY/PY
[1]
[2]
[3]
[4]
'
[5]
Cursor position [1] SHIFT-Z [2] SHIFT-R
F
M
N
ANG
'
[6]
'
[7]
P
Q
R
' [8] [9]
Description Specify the value of shift from the work origin to the oblique plane (the distance to the program origin of the oblique plane). (See “1 Point (PT)” for further details.)
[3] SPT-X
Specify the start point of the hole to be machined.
[4] SPT-Y
(See “1 Point (PT)” for further details.)
[5] CX/PX
Specify the pitch between two adjacent holes in the line of hole. [Top view of the oblique plane] +X
ANG
+Y
CX/PX
Start point
CX/PX
Position C
[6] M
Specify the number of holes to be drilled.
[7] ANG
Specify the angle between the line of holes and the X-axis on the oblique plane. (See the figure of the item [5] CX/PX.)
[8] Q
Specify if the machining at the start point is executed or not. 0: Actual execution of machining 1: Only positioning without machining
[9] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-113
3
PROGRAM CREATION
4.
Square (SQR) [ /Y ]
[ /Y ]
D734P0030
FIG
PTN
1
SQR
SHIFT-Z SHIFT-R SPT-X SPT-Y CX/PX CY/PY
[1]
[2]
[3]
[4]
Cursor position [1] SHIFT-Z [2] SHIFT-R
[5]
[6]
F
M
N
ANG
[7] [8] [9]
'
P
Q
R
[10] [11] [12]
Description Specify the value of shift from the work origin to the oblique plane (the distance to the program origin of the oblique plane). (See “1 Point (PT)” for further details.)
[3] SPT-X
Specify the start point of the hole to be machined.
[4] SPT-Y
(See “1 Point (PT)” for further details.)
[5] CX/PX
Specify the pitch between holes or the total length of the X-axis. [Top view of the oblique plane] +X
CY/PY (Total length) CY/PY
+Y
CX/PX (Pitch)
CX/PX (Total length) CX/PX CX/PX (Pitch)
Start point Position C
[6] CY/PY
Specify the pitch between holes or the total length of the Y-axis. (See the figure of the item [5] CX/PX.)
[7] F
Specify whether the data entered in CX/PX and CY/PY concern the pitch or the total length. 0: Pitch 1: Total length
[8] M
Specify the number of holes on the line of holes of the X-axis.
[9] N
Specify the number of holes on the line of holes of the Y-axis.
[10] P
Specify if the machining at the four corners is executed or not. 0: Machining at the four corners 1: No machining at the four corners
[11] Q
Specify if the machining at the start point is executed or not. 0: Actual execution of machining 1: Only positioning without machining
[12] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-114
PROGRAM CREATION
5.
Grid (GRD) [ /Y ]
[ /Y ]
D734P0031
FIG
PTN
1
GRD
SHIFT-Z SHIFT-R SPT-X SPT-Y CX/PX CY/PY
[1]
[2]
[3]
[4]
Cursor position [1] SHIFT-Z [2] SHIFT-R
[5]
[6]
F
M
N
[7] [8] [9]
ANG '
P
Q
R
[10] [11] [12]
Description Specify the value of shift from the work origin to the oblique plane (the distance to the program origin of the oblique plane). (See “1 Point (PT)” for further details.)
[3] SPT-X
Specify the start point of the hole to be machined.
[4] SPT-Y
(See “1 Point (PT)” for further details.)
[5] CX/PX
Specify the pitch between holes or the total length of the X-axis. [Top view of the oblique plane]
+X
CY/P (Total length) CY/P
+Y
CX/PX (Pitch)
CX/PX (Total length) CX/PX CX/PX (Pitch)
Start point Position C
[6] CY/PY [7] F
Specify the pitch between holes or the total length of the Y-axis. (See the figure of the item [5] CX/PX.) Specify whether the data entered in CX/PX and CY/PY concern the pitch or the total length. 0: Pitch 1: Total length
[8] M
Specify the number of holes on the line of holes of the X-axis.
[9] N
Specify the number of holes on the line of holes of the Y-axis.
[10] P
Specify if the machining at the four corners is executed or not. 0: Machining at the four corners 1: No machining at the four corners
[11] Q
Specify if the machining at the start point is executed or not. 0: Actual execution of machining 1: Only positioning without machining
[12] R
Specify the position to which the tool returns after machining. 0: Initial point 1: Reference point
3-115
3
3
PROGRAM CREATION
3-6
Line Machining Units Line machining units are used to enter a contour machining method and the data relating to a form to be machined. The unit includes two sequences: One is the tool sequence, subject to which data are entered in relation to the operational details of tool and the other the shape sequence, subject to which data are entered in relation to the machining dimensions specified on drawing.
3-6-1
Types of line machining units As shown below 9 types of line machining units are available: 1. Central linear machining
2. Right-hand linear machining
3. Left-hand linear machining
4. Outside linear machining
5. Inside linear machining
6. Right-hand chamfering
7. Left-hand chamfering
8. Outside chamfering
9. Inside chamfering
M3P171 Fig. 3-21
Types of line machining units
3-116
PROGRAM CREATION
3-6-2
3
Procedure for selecting line machining unit (1) Press the menu selector key (key located at the right of the menu keys) to display the following menu. POINT LINE FACE TURNING MANUAL MACH-ING MACH-ING MACH-ING PROGRAM
END
SHAPE CHECK
(2) Presse the [LINE MACH-ING] menu key. !
The following line machining unit menu will be displayed.
LINE CTR LINE RGT LINE LFT LINE OUT LINE IN CHMF RGT CHMF LFT CHMF OUT CHMF IN
(3) Press the appropriate menu key of the desired machining unit.
3-117
>>>
3
PROGRAM CREATION
3-6-3
Unit data, automatic tool development and tool path of the line machining unit 1.
Central linear machining unit (LINE CTR) This unit should be selected to carry out machining so that the tool has its center move on the line of a form. A.
Data setting
UNo.
UNIT
1
LINE CTR
SNo.
TOOL
MODE POS-B POS-C
NOM-φ
No.
#
SRV-A
APRCH-1
SRV-R
APRCH-2
RGH
FIN-A
TYPE
R1
END MILL
◆
F2
END MILL
◆
AFD
START END
DEP-A
WID-R
C-SP
FR
M
M
M
◆ ◆
◆ ': Data are not necessary to be set here.
Remark 1: In this unit, end mills are automatically developed. Nevertheless, they may be switched over to either face mill or ball end mill. Remark 2: For the tool sequence data setting, refer to Subsection 3-6-4. LINE CTR unit
Tool sequence
Roughing
.... .... .... .... ....
SRV-A
FIN-A End mill (for roughing)
End mill (for finishing)
Finishing SRV-R
Shape sequence entered
D740PA121
D740PA043
RGH: A roughness code should be selected out of the menu. FIN-A: An axial finishing allowance is automatically entered once a roughness code has been selected. B.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. In the tool sequence, a maximum of up to two tools are automatically developed, based on SRV-A and on FIN-A. Machining
Pattern
R1 (Roughing)
FIN-A = 0: One tool is selected.
F2 (Finishing)
SRV-A ≤ FIN-A: One tool is selected.
3-118
PROGRAM CREATION
C.
3
Tool path X-Y-axis
Y
Rapid feed Cutting feed
[1] Movement to the approach point
Pa E2 [4] Movement to the cutting start point
E2
Workpiece
Fs Pc
Fe Pe [6] Movement to the escape point after completion of machining
Shape sequence entered
[5] Machining along the form
Workpiece X
M3P174
X-Z-axis Z
[1] Movement to the approach point
Rapid feed Cutting feed Pi
Note 2 [2] Movement to the clearance position
Pa
[3] Movement to the machining Pcface Pc
[5] [4] Movement to the Machining cutting start point along the form
[7] Movement to the initial point
Clearance
Pe [6] Movement to the eacape point after completion of machining
Workpiece
X
M3P175
The bold codes represent parameter addresses.
Pi: Initial point Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Fs: Start point of form to be entered in the shape sequence Fe: End point of form to be entered in the shape sequence Pe: Escape point to be determined automatically
3-119
3
PROGRAM CREATION
Note 1: When ? is displayed in the items APRCH-1, -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operations [2] and [3] are performed. In this case, the coordinate value of the cutting start point will be entered in these items. X-Y-axis
Rapid feed Cutting feed
X-Z-axis
Y
Z [1] Movement to the cutting start point
[1] Movement to the cutting start point
Workpiece [2] Movement to the clearance position Note 2
Fs Pc (Pa) [4] Machining along the Workpiece form
[3] Movement to the machining face
[4] Machining Pc along the form (Pa)
Clearance
Workpiece X
X
M3P176
Note 2: See Subsection 3-6-6, “Precautions in line machining.” Note 3: The feedrate on tool path [3] is dependent upon the data AFD (axial feed) in the tool sequence.
3-120
PROGRAM CREATION
D.
3
Start point (START) and End point (END) Excessive cutting that may occur during approach or retraction can be prevented by specifying wall attributes for the line machining start and end points. The term “walls” are defined as the surfaces perpendicular to the shape at both the start point and the end point. Wall attributes can be specified for the following 5 units. -
LINE CTR LINE RGT LINE LFT CHMF RGT CHMT LFT
X-Z-axis Rapid feed Cutting feed
[1] Movement to the approach point [7]
[2] Movement to E9
[6] Movement to the initial point
[8]
Depth
E9
Z
X
[3] Movement to machining surface
[5] Movement to SRV-A the escape point [9]
[10]
[4] Movement to cutting start point
D740PA044
X-Y-axis Rapid feed Cutting feed
[1] Movement to the approach point [2] Movement to E9 [3] Movement to machining surface
E2
[5] Movement to the escape point [6] Movement to the initial point
Y
X
E2
[4] Movement to cutting start point
D740PA045
3-121
3
PROGRAM CREATION
X-Z-axis [1] Movement to the cutting start point X, Y
Rapid feed Cutting feed
[5] Movement to the initial point
[6] [2] Movement to E9
[3]
E9
Depth
[4]
Z
SRV-A [7]
X
[8]
[3], [7] Movement to cutting start point
[4], [8] Movement to the escape point
D740PA046
X-Y-axis Rapid feed Cutting feed
E30
Y
E30 [1][2][3][6][7]
[4][5][8] D740PA047
X
Note:
The tool path is determined according to the setting of parameter E104 bit 3. - E104 bit 3 = 0 Attribute: OPEN E2
E2
Cutting start point
Shape’s starting point
Shape’s ending point
Cutting end point
Attribute: CLOSED E30
Shape’s starting point
E30
Cutting start point
Cutting end point
Shape’s ending point
- E104 bit 3 = 1 (the same tool path as when MT Pro parameter P3 bit 4 = 1)
Shape’s starting point
Cutting end point
Cutting start point
Shape’s ending point
The starting (or ending) point of the shape and the starting (or ending) point of cutting agree, irrespective of the attributes.
3-122
PROGRAM CREATION
2.
3
Right-hand linear machining unit (LINE RGT) This unit should be selected to carry out machining so that the tool will move on the right side of a form. A.
Data setting
UNo.
UNIT
1
LINE RGT
SNo.
TOOL
MODE POS-B POS-C
NOM-φ
No.
#
SRV-A
SRV-R
APRCH-1
APRCH-2
RGH
FIN-A
TYPE
R1
END MILL
◆
F2
END MILL
◆
AFD
FIN-R
DEP-A
START END INTER-R CHMF
WID-R
C-SP
FR
M
M
M
◆ ◆
◆ ': Data are not necessary to be set here.
Remark 1: For data setting in START and END, refer to “1. Central linear machining unit (LINE CTR).” Remark 2: In this unit, end mills are automatically developed. Nevertheless, they may be switched over to face mill or ball end mill. Remark 3: For the tool sequence data setting, refer to Subsection 3-6-4. LINE RGT unit
Tool sequence
Shape sequence entered Roughing
SRV-A
.... .... .... .... .... .... .... FIN-A Finishing End mill End mill Chamfering (for roughing) (for finishing) cutter
FIN-R SRV-R D740PA123
D740PA048
RGH: A roughness code should be selected out of the menu. FIN-A: An axial finishing allowance is automatically established once a roughness code has been selected. FIN-R: A radial finishing allowance is also automatically established once a roughness code has been selected. B.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool.
3-123
3
PROGRAM CREATION
In the tool sequence, a maximum of up to three tools are automatically developed though dependent upon the data SRV-A, SRV-R, FIN-A and CHMF. Machining
C.
Pattern
R1 (Roughing)
FIN-A = 0 and FIN-R = 0 : One tool is selected.
F2 (Finishing)
SRV-A ≤ FIN-A or SRV-R ≤ FIN-R : One tool is selected.
(Chamfering)
CHMF≠ 0 : One tool is selected.
Tool path X-Y-axis
Y
Rapid feed Cutting feed [1] Movement to the approach point Pa
Shape sequence entered
E2
E2
sr tr Fe
Fs [4] Movement to the cutting start point
Pc
Pe [5] Machining along the form
[6] Movement to the escape point X
M3P178
X-Z-axis Z
Rapid feed Cutting feed
[1] Movement to the approach point Pi Note 2
[2] Movement to the clearance position [7] Movement to the initial point
Workpiece [3] Movement to the machining face
Clearance
Pc
Pa [4] Movement to the cutting start point
Pe
[5] Machining along the form
[6] Movement to the escape point X M3P179 The bold codes represent parameter addresses.
Pi: Initial point Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Fs: Start point of form to be entered in the shape sequence Fe: End point of form to be entered in the shape sequence Pe: Escape point to be automatically established tr:
Radial cutting allowance to be determined by the data SRV-R in the machining unit
sr:
Radial finishing allowance to be determined by the data FIN-R in the machining unit
3-124
PROGRAM CREATION
3
Note 1: When ? is displayed in the items APRCH-1, -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operations [2] and [3] are performed. In this case, the coordinate value of the cutting start point will be entered in these items. X-Z-axis
X-Y-axis Y
Z [1] Movement to the cutting start point
Rapid feed Cutting feed
[1] Movement to the cutting start point
Workpiece Note 2
[2] Movement to the clearance position
Fs Pc (Pa)
[3] Movement to the machining face
[4] Machining along the form
Clearance
Pc [4] Workpiece (Pa) Machining along the form
X
X
M3P180
Note 2: See Subsection 3-6-6 “Precautions in line machining.” Note 3: The feedrate on tool path [3] is dependent upon the data AFD (axial feed) in the tool sequence.
3-125
3
PROGRAM CREATION
3.
Left-hand linear machining unit (LINE LFT) This unit should be selected to carry out machining so that the tool will move on the left side of a form. A.
Data setting
UNo.
UNIT
1
LINE LFT
SNo.
TOOL
MODE POS-B POS-C
NOM-φ
No.
#
SRV-A
APRCH-1
SRV-R
APRCH-2
RGH
FIN-A
TYPE
R1
END MILL
◆
F2
END MILL
◆
AFD
FIN-R START
DEP-A
WID-R
END
C-SP
INTER-R CHMF
FR
M
M
M
◆ ◆
◆ ': Data are not necessary to be set here.
Remark 1: For data setting in START and END, refer to “1. Central linear machining unit (LINE CTR).” Remark 2: In this unit, end mills are automatically developed. Nevertheless, they may be switched over to face mill or ball end mill. Remark 3: For the tool sequence data setting, refer to Subsection 3-6-4. LINE LFT unit
Tool sequence
Shape sequence entered Roughing Finishing
.... .... .... ....
SRV-A FIN-A
End mill End mill Chamfering (for roughing) (for finishing) cutter
FIN-R
SRV-R
D740PA125
D740PA048
RGH: A roughness code should be selected out of the menu. FIN-A: An axial finishing allowance is automatically established once a roughness code has been selected. FIN-R: A radial finishing allowance is also automatically established once a roughness code has been selected. B.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool.
3-126
PROGRAM CREATION
3
In the tool sequence, a maximum of up to three tools are automatically developed though dependent upon the data SRV-A, SRV-R, FIN-A and CHMF. Machining
C.
Pattern
R1 (Roughing)
FIN-A = 0 and FIN-R = 0 : One tool is selected.
F2 (Finishing)
SRV-A ≤ FIN-A or SRV-R ≤ FIN-R : One tool is selected.
(Chamfering)
CHMF≠ 0 : One tool is selected.
Tool path X-Y-axis
Y
Rapid feed Cutting feed
[4]
Pa
[6] Movement to the escape point
[5] Machining along the form
Movement to the cutting start point
Pe
Pc Fe
Fs E2
[1] Movement to the approach point
sr tr
E2
Workpiece
Shape sequence entered X
M3P182
X-Z-axis Rapid feed Cutting feed
[1] Movement to the approach point
Z
Pi Note 2
[2] Movement to the clearance position [7] Movement to the initial point [3] Movement to the machining face
Pa [4] Movement to the cutting start point
Clearance
Pc
Pe [5] Machining along the form
Workpiece
[6] Movement to the eacape point X
M3P183
The bold codes represent parameter addresses.
Pi: Initial point Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Fs: Start point of form to be entered in the shape sequence Fe: End point of form to be entered in the shape sequence Pe: Escape point to be automatically established tr:
Radial cutting allowance to be determined by the data SRV-R in the machining unit
sr:
Radial finishing allowance to be determined by the data FIN-R in the machining unit
3-127
3
PROGRAM CREATION
Note 1: When ? is displayed in the items APRCH-1, -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operations [2] and [3] are performed. In this case, the coordinate value of the cutting start point will be entered in these items. X-Y-axis
X-Z-axis
Y
Z
[1] Movement to the cutting start point
[1] Movement to the cutting start point
Note 2 Pc
[4]
Rapid feed Cutting feed
Fs
[2] Movement to the clearance position
[3] Movement to the Clearance machining face
(Pa)
Workpiece
Workpiece Machining along the form
[4] Pc (Pa) Machining along the form X
X
M3P184
Note 2: See Subsection 3-6-6, “Precautions in line machining.” Note 3: The feedrate on tool path [3] is dependent upon the data AFD (axial feed) in the tool sequence.
3-128
PROGRAM CREATION
4.
3
Outside linear machining unit (LINE OUT) This unit should be selected to carry out machining so that the tool will move to make a turnaround outside a form. A.
Data setting
UNo.
UNIT
1
LINE OUT
SNo.
TOOL
MODE POS-B POS-C
NOM-φ
No.
#
SRV-A
APRCH-1
SRV-R
RGH
APRCH-2
FIN-A
TYPE
R1
END MILL
◆
F2
END MILL
◆
AFD
FIN-R
DEP-A
INTER-R
WID-R
C-SP
FR
CHMF
M
M
M
◆ ◆
◆ ': Data are not necessary to be set here.
Remark 1: In this unit, end mills are automatically developed. Nevertheless, they may be switched over to face mill or ball end mill. Remark 2: For the tool sequence data setting, refer to Subsection 3-6-4. LINE OUT unit
Tool sequence
Shape sequence entered
Roughing
SRV-A
.... .... .... .... .... .... ....
FIN-A Finishing End mill End mill Chamfering (for roughing) (for finishing) cutter
FIN-R SRV-R D740PA126
D740PA048
RGH: A roughness code should be selected out of the menu. FIN-A: An axial finishing allowance is automatically established once a roughness code has been selected. FIN-R: A radial finishing allowance is also automatically established once a roughness code has been selected.
3-129
3
PROGRAM CREATION
B.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. In the tool sequence, a maximum of up to three tools are automatically developed though dependent upon the data SRV-A, SRV-R, FIN-A and CHMF. Machining
C.
Pattern
R1 (Roughing)
FIN-A = 0 and FIN-R = 0 : One tool is selected.
F2 (Finishing)
SRV-A ≤ FIN-A or SRV-R ≤ FIN-R : One tool is selected.
(Chamfering)
CHMF≠ 0 : One tool is selected.
Tool path X-Y-axis Rapid feed Cutting feed
Y
[1] Movement to the approach point Workpiece
Note 1
Pa [4] Movement to the cutting start point
Pc
[5]
Machining along the form
[6] Movement to the escape point Pe X
M3P186
X-Z-axis Z
Rapid feed Cutting feed
[1] Movement to the approach point Pi Note 2
[2] Movement to the clearance position [7] Movement to the initial point
[3] Movement to the machining face
Clearance
Pa
Pc [4]
Movement to the cutting start point
Pe [5] Machining along the form
Workpiece
[6] Movement to the escape point
X
Pi: Initial point Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Pe: Escape point to be automatically established
3-130
M3P187
PROGRAM CREATION
3
Note 1: Detail description of tool path near approach point and escape point When the cutting begins near the convex form - In case of roughing Y
Y
[4] Movement to the cutting start point
Workpiece
E2
sr
Pc
E2
Workpiece
tr
tr
sr
Pe
[6] Movement to the escape point
[5] Machining along the form
X
X
M3P188
X
M3P189
- In case of finishing Y
Y
Workpiece [4] Movement to the cutting start point
E2
Workpiece
E2
sr
Pc
sr
[6] Movement to the escape point
[5] Machining along the form
Pe
X
The bold codes represent parameter addresses.
Tr: Radial cutting allowance to be determined by the data SRV-R in the machining unit sr:
Radial finishing allowance determined by the data FIN-R in the machining unit
3-131
3
PROGRAM CREATION
When cutting begins near the non-convex form - In case of roughing Y
Workpiece
sr
tr E2
E2
Pc
[6]
[5]
Movement to the escape point
Machining along the form [4] Movement to the cutting start point
E1
E21
Pe
E1
X
M3P190
- In case of finishing Y sr Workpiece tr E2
E2
[6]
[5] Pc
[4] Movement to the cutting start point
Machining along the form
E1
Movement to the escape point
E21
Pe
E1
X
M3P191
The bold codes represent parameter addresses.
tr: Radial cutting allowance to be determined by the data SRV-R in the machining unit sr: Radial finishing allowance to be determined by the data FIN-R in the machining unit Note 2: See Subsection 3-6-6, “Precautions in line machining.” Note 3: The feedrate on tool path [3] is dependent upon the data AFD (axial feed) in the tool sequence.
3-132
PROGRAM CREATION
3
Note 4: According to the position of the approach point entered in the tool sequence and to a machining shape entered in the shape sequence, a cutting start point and a cutting method vary as follows: * The description below is entirely given, with the cutting direction taken CCW (counterclockwise). When ? is displayed in the items APRCH-1, -2 - Form having a convex point: Y
Fs
Pc X M3P192
Cutting is started from the convex point nearest the start point (Fs) entered in the shape sequence. - Form having no convex point:
Y
Fs
Pc X M3P193
Cutting is started from the start point (Fs) entered in the shape sequence.
3-133
3
PROGRAM CREATION
When the data is entered in the items APRCH-1, -2 - If there is not any convex point near the approach point:
Y
Pa
Pc
X
M3P194
- If there is a convex point near the approach point: Y
Pa Pc
X M3P195
Pc: Cutting start point to be automatically established Fs: Start point of form to be entered in the shape sequence Pa: Approach point to be determined using the numeric keys When ? is displayed by pressing the [AUTO SET] menu key, the coordinates of the cutting start point will be entered automatically.
3-134
PROGRAM CREATION
5.
3
Inside linear machining unit (LINE IN) This unit should be selected to carry out machining so that the tool will make a turn-around inside of a form. A.
Data setting
UNo.
UNIT
1
LINE IN
SNo.
TOOL
MODE POS-B POS-C
NOM-φ
No.
#
SRV-A
APRCH-1
SRV-R
APRCH-2
RGH
TYPE
R1
END MILL
◆
F2
END MILL
◆
FIN-A
AFD
FIN-R
DEP-A
INTER-R
WID-R
C-SP
FR
CHMF
M
M
M
◆ ◆
◆ ': Data are not necessary to be set here.
Remark 1: In this unit, end mills are automatically developed. Nevertheless, they may be switched over to face mill or ball end mill. Remark 2: For the tool sequence data setting, refer to Subsection 3-6-4. LINE IN unit
Tool sequence
Roughing Finishing
.... .... .... ....
SRV-A FIN-A
Shape sequence entered SRV-R
FIN-R
End mill End mill Chamfering (for roughing) (for finishing) cutter
D740PA127
D740PA048
RGH: A roughness code should be selected out of the menu. FIN-A: An axial finishing allowance is automatically established once a roughness code has been selected. FIN-R: A radial finishing allowance is also automatically established once a roughness code has been selected. B.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. In the tool sequence, a maximum of up to three tools are automatically developed though dependent upon the data SRV-A, SRV-R, FIN-A and CHMF. Machining
Pattern
R1 (Roughing)
FIN-A = 0 and FIN-R = 0 : One tool is selected.
F2 (Finishing)
SRV-A ≤ FIN-A or SRV-R ≤ FIN-R : One tool is selected.
(Chamfering)
CHMF≠ 0 : One tool is selected.
3-135
3
PROGRAM CREATION
C.
Tool path X-Y-axis Rapid feed Cutting feed
Workpiece
Y [1] Movement to the approach point Pa
Movement to the [4] cutting start point
Pc
Pe [6] Movement to the escape point
Machining along the form [5]
Note 2
X
M3P197
X-Z-axis Z
[1] Movement to the approach point
Rapid feed Cutting feed Pi Note 3
[2] Movement to the clearance position [7] Movement to the initial point
Clearance
Workpiece
Pa
[3] Movement to the machining face Pc
Pe
Workpiece
[6] Movement to the [4] Movement to the [5] Machining cutting start point along the form escape point X
Pi:
M3P198
Initial point
Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Pe: Escape point to be automatcially established Note 1: The feedrate on tool path [3] is dependent upon the data AFD (axial feed) in the tool sequence.
3-136
PROGRAM CREATION
3
Note 2: Detail description of tool path near approach point and escape point When the cutting begins near the convex form - In case of roughing Y
Y
[4] Movement to the cutting startpoint [5] Machining along the form
[6] Movement to the escape point
Pc
Pe sr
E2
tr
tr
Workpiece
sr
Workpiece
E2
X
X
M3P199
- In case of finishing Y
Y
[4] Movement to the cutting start point
[6] Movement to the escape point
[5] Machining along the form Pc
sr
sr
E2
Workpiece
Workpiece
Pe
E2
X
X
M3P200
The bold codes represent parameter addresses.
tr: Radial cutting allowance to be determined by the data SRV-R in the machining unit sr: Radial finishing allowance determined by the data FIN-R in the machining unit
3-137
3
PROGRAM CREATION
When the cutting begins near the non-convex form - In case of roughing Y
E1
E21
E1
[4] Movement to the cutting start point
Pc
Movement to the escape point
Machining along the form
Pe
[6]
[5]
E2
E2
sr
tr
Workpiece
X
M3P201
- In case of finishing Y
E1
E21
E1
[4] Movement to the cutting start point
Pc
Machining along the form [5]
Movement to the escape point [6]
Pe
E2
E2
tr
sr Workpiece X
M3P202
The bold codes represent parameter addresses.
tr: Radial cutting allowance to be determined by the data SRV-R in the machining unit sr: Radial finishing allowance determined by the data FIN-R in the machining unit Note 3: See Subsection 3-6-6, “Precautions in line machining.”
3-138
PROGRAM CREATION
3
Note 4: According to the position of the approach point entered in the tool sequence and to a machining shape entered in the shape sequence, a cutting start point and a cutting method vary as follows: * The description below is entirely given, with the cutting direction taken CCW (counterclockwise). When ? is displayed in the items APRCH-1, -2 - Form having a convex point:
Y
Pc Fs
X M3P203
Cutting is started from the convex point nearest the start point (Fs) entered in the shape sequence. - Form having no convex point: Y
Pc
Fs X M3P204
Cutting is started from the start point (Fs) entered in the shape sequence.
3-139
3
PROGRAM CREATION
When the data is entered in the items APRCH-1, -2 - If there is a convex point near the approach point:
Y
Pa
Pc
X M3P205
- If there is not any convex point near the approach point: Y
Pc
Pa
Fs X M3P206
Pc: Cutting start point to be automatically established Fs: Start point of form to be entered in the shape sequence Pa: Approach point to be determined using the numeric keys. When ? is displayed by pressing the [AUTO SET] menu key, the coordinates of the cutting start point will be entered automatically.
3-140
PROGRAM CREATION
6.
3
Right-hand chamfering unit (CHMF RGT) This unit should be selected to carry out chamfering so that a tool will move on the right side of a form. A.
Data setting
UNo.
UNIT
1
CHMF RGT
SNo. 1
MODE POS-B POS-C INTER-AX INTER-R
TOOL
NOM-φ
No.
#
APRCH-1
APRCH-2
CHMF
TYPE
START
AFD
◆
CHAMFER
DEP-A
WID-R
◆
◆
END
C-SP
FR
M
M
M
': Data are not necessary to be set here.
Remark 1: For data setting in START and END, refer to “1. Central linear machining unit (LINE CTR).” Remark 2: In this unit, chamfering cutter is automatically developed. Instead of the chamfering cutter, a centering drill can be used. Remark 3: For the tool sequence data setting, refer to Subsection 3-6-4. Note:
If a centering drill is used, a nose angle of 90 degrees is set for machining. CHMF RGT unit
Tool sequence
Shape sequence entered INTER-R
INTER-AX
Chamfering cutter
CHMF
D740PA128
B.
D740PA049
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool.
3-141
3
PROGRAM CREATION
C.
Tool path X-Y-axis Rapid feed Cutting feed
Y
[1] Movement to the approach point [4] Movement to the cutting start point Pa Fs Pc
Workpiece Fe
fr
Pe [6] Movement to the escape point
[5] Machining along the form
X
M3P209
X-Z-axis Z
[1] Movement to the approach point
Rapid feed Cutting feed Pi
Note 2
[2] Movement to the clearance position [7] Movement to the initial point [3] Movement to the machining face Pa Pc [4] Movement to the cutting start point
Machining along the form [5] Workpiece
Pe [6] Movement to the escape point X
M3P210
Pi: Initial point Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Fs: Start point of form to be entered in the shape sequence Fe: End point of form to be entered in the shape sequence Pe: Escape point to be automatically established fr:
Optimum distance to be automatically established, from the data entered in the PROGRAM and TOOL FILE displays
3-142
PROGRAM CREATION
3
Note 1: When ? is displayed in the items APRCH-1 and -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operations [2] and [3] are performed. In this case, a coordinate of the cutting start point is entered automatically in the items. X-Y-axis
X-Z-axis
Y
Z
Rapid feed Cutting feed
[1] Movement to the cutting start point
[1] Movement to the cutting start point [2] Movement to the clearance position
Workpiece Fs
[3] Movement to the machining face Pc [4] Machining along the form
Pc [4] Machining along the form
X
Workpiece X
M3P211
Note 2: See Subsection 3-6-6, “Precautions in line machining.” Note 3: The feedrate on tool path [3] is dependent upon the data AFD (axial feed) in the tool sequence.
3-143
3
PROGRAM CREATION
7.
Left-hand chamfering unit (CHMF LFT) This unit should be selected to carry out chamfering so that a tool will move on the left side of a form. A.
Data setting
UNo.
UNIT
1
CHMF LFT
SNo. 1
TOOL
MODE POS-B POS-C INTER-AX INTER-R
NOM-φ
No.
#
APRCH-1
APRCH-2
CHMF
TYPE
AFD
◆
CHAMFER
START
END
DEP-A
WID-R
C-SP
◆
◆
FR
M
M
M
': Data are not necessary to be set here.
Remark 1: For data setting in START and END, refer to “1. Central linear machining unit (LINE CTR).” Remark 2: In this unit, chamfering cutter is automatically developed. Instead of the chamfering cutter, a centering drill can be used. Remark 3: For the tool sequence data setting, refer to Subsection 3-6-4. Note:
If a centering drill is used, a nose angle of 90 degrees is set for machining. CHMT LFT unit
Tool sequence
Shape sequence entered INTER-R
INTER-AX
CHMF
D740PA130
B.
Chamfering cutter
D740PA049
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool.
3-144
PROGRAM CREATION
C.
3
Tool path X-Y-axis Rapid feed Cutting feed
Y [1] Movement to the approach point
Pa fr Pc
Fs
Fe
Pe
Workpiece
X
M3P213
X-Z-axis Rapid feed Cutting feed
[1] Movement to the approach point
Z
Pi Note 2
[2] Movement to the clearance position [7] Movement to the initial point [3] Movement to the Machining along the form machining face Pa Pc [5] [4] Movement to the cutting start point
Clearance Pe Workpiece
[6] Movement to the escape point X
M3P214
Pi: Initial point Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Fs: Start point of form to be entered in the shape sequence Fe: End point of form to be entered in the shape sequence Pe: Escape point to be automatically established fr:
Optimum distance to be automatically established, from the data entered in the PROGRAM and TOOL FILE displays
3-145
3
PROGRAM CREATION
Note 1: When ? is displayed in the items APRCH-1 and -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operations [2] and [3] are performed. In this case, a coordinate of the cutting start point is entered automatically in the items. X-Y-axis
Rapid feed Cutting feed
X-Z-axis
Y
Z [1] Movement to the cutting start point
[1] Movement to the cutting start point
[2] Movement to the clearance position
Pc
[4]
Fs
[3] Movement to the machining face
Machining along the form Workpiece
Pc X
[4] Machining along the form
Workpiece X
M3P215
Note 2: See Subsection 3-6-6, “Precautions in line machining.” Note 3: The feedrate on tool path [3] is dependent upon the data AFD (axial feed) in the tool sequence.
3-146
PROGRAM CREATION
8.
3
Outside chamfering unit (CHMF OUT) This unit should be selected to carry out chamfering so that a tool will move on the outside of a form. A.
Data setting
UNo.
UNIT
1
CHMF OUT
SNo. 1
TOOL
MODE POS-B POS-C INTER-AX INTER-R
NOM-φ
No.
#
APRCH-1
APRCH-2
CHMF
TYPE
AFD
CHAMFER
DEP-A
WID-R
◆
◆
C-SP
FR
M
M
M
': Data are not necessary to be set here.
Remark 1: In this unit, chamfering tools are automatically developed. Instead of the chamfering cutter, a centering drill can be used. Remark 2: For the tool sequence data setting, refer to Subsection 3-6-4. Note:
If a centering drill is used, a nose angle of 90 degrees is set for machining. CHMF OUT unit
Shape sequence entered
Tool sequence
INTER-R
INTER-AX
Chamfering cutter
CHMF D740PA131
B.
D740PA049
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool.
3-147
3
PROGRAM CREATION
C.
Tool path X-Y-axis Rapid feed Cutting feed
Y
[1] Movement to the approach point Workpiece
Note 2
Pa [4] Movement to the cutting start point
Pc
[5]
Machining along the form
Pe
[6] Movement to the escape point
X
M3P217
X-Z-axis Z
[1] Movement to the approach point
Rapid feed Cutting feed Pi
Note 3
[2] Movement to the clearance position [7] Movement to the initial point [3] Movement to the machining face Pa [4] Movement to the cutting start point
Pc
[6] Movement to the escape point
Clearance
Pe [5] Workpiece Machining along the form X
M3P218
Pi: Initial point Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Pe: Escape point to be automatically established Note 1: The feedrate on tool path [3] is dependent upon the AFD (axial feed) in the tool sequence.
3-148
PROGRAM CREATION
3
Note 2: Detail description of tool path near approach point and escape point When the cutting begins near the convex form Y
Y
[4] Movement to the cutting start point
fr fr
Pc
[6]
[5] Machining along the form
Movement to the escape point
Pe
X
X
M3P219
When the cutting begins near the non-convex form Y Workpiece
fr
Pc
[6]
[5]
[4] Movement to the cutting start point
E1
Pe
Movement to the escape point
Machining along the form
E21
E1
X
M3P220
The bold codes represent parameter addresses.
fr: An optimum distance is automatically obtained from the data entered in the PROGRAM and TOOL FILE displays Note 3: See Subsection 3-6-6, “Precautions in line machining.”
3-149
3
PROGRAM CREATION
Note 4: According to the position of the approach point entered in the tool sequence and to a machining form entered in the shape sequence, a cutting start point and a cutting method vary as follows: * The description below is entirely given, with the cutting direction taken CCW (counterclockwise). When ? is displayed in the items APRCH-1, -2 - Form having a convex point: Y
Fs
Pc X M3P221
Cutting is started from the convex point nearest the start point (Fs) entered in the shape sequence. - Form having no convex point: Y
Fs
Pc X M3P222
Cutting is started form the start point (Fs) entered in the shape sequence.
3-150
PROGRAM CREATION
3
When the data is entered in the items APRCH-1, -2 - If there is not any convex point near the approach point.
Y
Pa
Pc
X M3P223
- If there is a convex point near the approach point. Y
Pa Pc
X M3P224
Pa: Approach point to be determined using the numeric keys If ? is displayed by pressing the [AUTO SET] menu key, the coordinates of cutting start point will be entered automatically. Pc: Cutting start point to be automatically established Fs: Start point of form to be entered in the shape sequence
3-151
3
PROGRAM CREATION
9.
Inside chamfering unit (CHMF IN) This unit should be selected to carry out chamfering so that a tool will make a turn-around inside of a form. A.
Data setting
UNo.
UNIT
1
CHMF IN
SNo. 1
TOOL
MODE POS-B POS-C INTER-AX INTER-R
NOM-φ
No.
#
APRCH-1
APRCH-2
CHMF
TYPE
AFD
CHAMFER
DEP-A
WID-R
◆
◆
C-SP
FR
M
M
M
': Data are not necessary to be set here.
Remark 1: In this unit, chamfering cutter is automatically developed. Instead of the chamfering cutter, a centering drill can be used. Remark 2: For the tool sequence data setting, refer to Subsection 3-6-4. Note:
If a centering drill is used, a nose angle of 90 degrees is set for machining. CHMF IN unit
Tool sequence
INTER-R
Shape sequence entered
INTER-AX
CHMF Chamfering cutter
D740PA132
B.
D740PA049
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool.
3-152
PROGRAM CREATION
C.
3
Tool path X-Y-axis Rapid feed Cutting feed
Workpiece
Y [1] Movement to the approach point
[4] Pa
Movement to the cutting start point Pc
Pe [6] Movement to the escape point
[5]
Machining along the form Note 3
X
M3P226
X-Z-axis Z
Rapid feed Cutting feed
[1] Movement to the approach point Pi Note 3
[2] Movement to the clearance position [7] Movement to the inital point
Clearance [3] Movement to the machining face Pa Pc
Workpiece
Pe
[4] Movement to [5] Machining [6] Movement to the cutting along the escape start point the form point
Workpiece
X
M3P227
Pi: Initial point Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Pe: Escape point to be automatically established Note 1: The feedrate on tool path [3] is dependent upon the AFD (axial feed) in the tool sequence.
3-153
3
PROGRAM CREATION
Note 2: Detail description of tool path near approach point and escape point When the cutting begins near the convex form Y
Y [4] Movement to the cutting start point
Pc
Pe Movement to the [6] escape point
Machining along [5] the form
fr
fr
X
X
M3P228
When the cutting begins near the non-convex form Y
E1
E21
E1
[4] Movement to the cutting start point Pc
Movement to the escape point [6]
Machining along the form [5]
fr
Pe
Workpiece X
M3P229
The bold codes represent parameter addresses.
fr: An optimum distance is automatically obtained from the data entered in the PROGRAM and TOOL FILE displays Note 3: See Subsection 3-6-6, “Precautions in line machining.”
3-154
PROGRAM CREATION
3
Note 4: According to the position of the approach point entered in the tool sequence and to a machining form entered in the shape sequence, a cutting start point and a cutting method vary as follows: * The description below is entirely given, with the cutting direction taken CCW (counterclockwise). When ? is displayed in the items APRCH-1, -2 - Form having a convex point:
Y
Pc Fs
X M3P230
Cutting is started from the convex point nearest the start point (Fs) entered in the shape sequence. - Form having no convex point: Y
Pc
Fs X M3P231
Cutting is started form the start point (Fs) entered in the shape sequence.
3-155
3
PROGRAM CREATION
When the data is entered in the items APRCH-1, -2 - If there is a convex point near the approach point.
Y
Pa
Pc
X M3P232
- If there is not any convex point near the approach point.
Y
Pc
Pa
Fs X
M3P233
Pa: Approach point to be determined using the numeric keys When ? is displayed by pressing the [AUTO SET] menu key, the coordinates of cutting start point will be entered automatically. Pc: Cutting start point to be automatically established Fs: Start point of form to be entered in the shape sequence
3-156
PROGRAM CREATION
3-6-4
3
Tool sequence data of the line machining unit For line machining tool sequence data only a tool name is automatically selected once a machining unit has been entered. Other data should be entered by use of menu keys or numeric keys according to a form of the workpiece to be machined or to the procedure for machining. Tool sequence data
Item
TOOL
NOM-φ
No.
#
APRCH-1
(1)
(2)(3)(4)
(5)
(6)
(7)
APRCH-2 TYPE
(7)
AFD
(8)
(9)
DEP-A WID-R C-SP
FR
M M M
◆
(12)
(13)
(10) ':
(11)
Not necessary to be set here.
For setting of each data item refer to 1 to 13 below. 1.
TOOL (Tool designation) The name of a tool can be changed by the use of menu keys. In the central linear, right-hand linear, left-hand linear, outside linear and inside linear machining units, either end mill, face mill or ball end mill is selectable. In the right-hand, left-hand, outside and inside chamfering units, a chamfering cutter and a centering drill are selectable. ENDMILL FACEMILL CHAMFER BALL CUTTER ENDMILL
2.
CENTER DRILL
NOM-φ (Nominal diameter of tool) Approximate diameter of a tool is entered. A nominal diameter is the data to identify by diameter those tools which are of identical type (having an identical name).
3.
NOM-φ (Tool identification code) A code should be selected out of the menu to identify those tools which are of identical type (having an identical name) and have an identical nominal diameter. A
B
C
D
E
F
G
H
HEAVY TOOL
>>>
To slowly change a heavy tool in the ATC mode, select a heavy tool identification code. With the [HEAVY TOOL] menu key pressed, the display will change over to the menu for heavy tool identification code. Then select a code from the menu to identify those tools which have an identical nominal diameter. 4.
NOM-φ (Turret selection) For the machine with the lower turret, select the turret in which the tool to be used is mounted. The following menu is displayed (if [SET UPPER TURRET] is selected, the column will remain blank, and if [SET LOWER TURRET] is selected, “ ” will be displayed). See Chapter 5, LOWER-TURRET CONTROL FUNCTIONS, for further details: SET UPPER TURRET
SET LOWER TURRET
3-157
3
PROGRAM CREATION
5.
No. (Priority No.) Assign priority levels in the order of machining. The following menu is displayed. A press of a menu key displays the menu item in reverse mode, allowing a priority number to be assigned. DELAY PRIORITY
(a)
PRI.No. PRI.No. CHANGE ASSIGN
(b)
PRI.No. SUB PROG ALL ERAS PROC END
(c)
(d)
(e)
The function of menu item (a) to (e) is described below: Menu item
Function
(a)
Select to conduct subsequent-machining.
(b)
Select to change the priority number for the tool within the particular process. If the cursor is present at a blank space, assign a new number in a usual manner. Entry of an existing priority number displays alarm 420 SAME DATA EXISTS.
(c)
Select to assign a priority number to the tool to be used repeatedly in the particular process. Alarm 420 SAME DATA EXISTS will be displayed if the assigned priority number has already been set on any other unit line.
(d)
Selection of this item displays message ALL ERASE (PROC:0, PROG:1)?. Setting 0 will erase the priority numbers preassigned to the tool to be used repeatedly in the process. Setting 1 will erase the priority numbers preassigned to the tool to be used repeatedly in the program.
(e)
Select to terminate the process with the subprogram unit.
For details see Chapter 4, “PRIORITY FUNCTION FOR THE SAME TOOL.” 6.
# (Retraction position of the lower turret) For a machine having upper and lower turrets, it is possible to specify the position to which the lower turret is to be retracted when machining workpieces using only the upper turret. The following menu is displayed. For details see Chapter 5, “LOWER-TURRET CONTROL FUNCTIONS”. LOWER TURRET POS.1
7.
LOWER TURRET POS.2
APRCH-1, APRCH-2 (Coordinates of the approach point) Enter coordinates of the position at which a tool is to cut in axially. Pressing the [AUTO SET] menu key sets a question mark (?). After the tool path check is performed, ? will automatically change over to the coordinates of a cutting start point. (Refer to tool path for each unit.)
3-158
PROGRAM CREATION
8.
3
TYPE (Machining method) Use menu keys to select the direction in which machining (turning) is performed in the outside and inside linear machining and outside and inside chamfering units. CW CUT
CCW CUT
CCW
CW
[CW CUT]
[CCW CUT] M3P234
9.
AFD (Axis feedrate) Enter the feedrate in axial direction. It is also possible, moreover, to select rapid feed (G00) or cutting feed (G01) by the use of menu keys. CUT G01
RAPID G00
AFD Initial point
G00
Rapid feed
G01
Parameter E17 may be used to determine: E17 Feed × 10
Numeric value (α)
Feed × α
Determine this rate.
Workpiece
Feedrate
M3P235
10. DEP-A (Cutting stroke) In roughing, a maximum axial cutting stroke in one cycle is entered. With the [AUTO SET] menu key selected, a smaller value is entered, either the data SRV-A entered in the machining unit or the maximum cutting stroke registered on the TOOL FILE display. An actual axial cutting stroke is arithmetically obtained from the data DEP-A, SRV-A and FIN-A, both in the machining unit. (For calculation formula, see Subsection 3-6-6, “Precautions in line machining.”)
3-159
3
PROGRAM CREATION
11. C-SP (Surface speed) To auto-set a surface speed (m/min) and feedrate (mm/rev), select the corresponding tool material type from the menu. The tool material types in the menu are the same as those which have been set on the CUTTING CONDITION - W. MAT./T. MAT display. To register new tool material types, refer to Section of “CUTTING CONDITION - W. MAT./T. MAT Display”, of the relevant Operating Manual. HSS AUTO
CARBIDE AUTO
Data can also be set using the numeric keys. 12. FR (Feedrate) Used to specify the feedrate of the tool. Same as the surface speed, the entry of data is done by means of menu keys or numeric keys. 13. M (M-code) Set the required M-code(s) to be output immediately after mounting the tool onto the spindle in the ATC mode. A maximum of up to three M-codes may be entered. It is also possible, moreover, to select and enter a general M-code out of the menu.
3-6-5
Shape sequence data of the line machining unit The data setting items of shape sequence for the line machining units are the same as those for the face machining units. For the shape sequence data setting, see data entry procedure in Subsection 3-7-7.
3-160
PROGRAM CREATION
3-6-6
3
Precautions in line machining 1.
Tool path during rough-machining with axial removal allowance (SRV-A) > axial cutting depth (DEP-A) Cutting is performed at several pass. The tool path is determined by the parameter E95 which relates with three factors, but not all of these factors may be available for the certain machining unit: - Cutting start position in the axial direction - Type of routing through approach points - Type of escape in the axial direction after machining For each factor refer to A, B and C below. [Basic tool path] Initial point
Rapid feed Cutting feed Clearance [1]
cua
[2]
[3]
cua
[4]
[5]
cua
[6]
ta
Finishing surface sa M3P236
Fig. 3-22
Basic tool path
cua: Cutting depth in the axial direction per pass (Axial cutting depth DEP-A to be entered in the tool sequence) Calculation of cua: cua =
n=
ta – sa n ta – sa cua
ta:
Axial cutting allowance SRV-A to be entered in the machining unit
sa:
Axial finishing allowance FIN-A to be entered in the machining unit
n:
Number of passes in the axial direction (Integer obtained by rounding up the decimal fraction)
3-161
3
PROGRAM CREATION
A.
Cutting start position in the axial direction Select one of the following two types:
(1) Rapid feed to the clearance position above the machining surface First cutting
Second cutting
(2)
Cutting start position fixed
First cutting
Second cutting
Clearance
Clearance
cua
cua
cua
cua
Clearance
M3P237
. B.
Type of routing via approach point Select one of the following two types:
(1) Routing via approach point each time
(2) Routing via approach point only in the first pass
[3] [1]
[3]
[1] [6]
[6]
[4] Escape point [4]
Escape point
[2] [2] [5]
Approach point
Approach point
[5]
Cutting start point
Cutting start point
M3P238
3-162
PROGRAM CREATION
C.
3
Type of escape in the axial direction after machining Select one of the following two types:
(2) Return to the initial point
(1) No axial relief
[1]
[1]
[4]
[2]
cua
cua
cua
cua [2]
[3]
[5]
[4]
Cutting start point
[3]
Escape point
Cutting start point
Escape point
M3P239
Tool path setting parameter Parameter E95 For A: bit 4 = 0: Cutting start position fixed -- (2) 1: Rapid feed to the clearance position above the machining surface -- (1) * As for pattern (1), the starting position of cutting feed is determined by the setting of parameter E7 (instead of clearance) from the second cutting when the following conditions are satisfied: - Bit 6 of parameter E95 is set to “1”, and - The unit concerned is LINE CTR, RGT, LFT, OUT or IN. For B: bit 2 = 0: Routing via approach points only in the first pass -- (2) 1: Routing via approach points each time -- (1) For C: bit 3 = 0: Return to the initial point -- (2) 1: No escape in the axial direction -- (1) Note 1: Both A and B can be used for all line-machining units, whereas C can only be used for inside linear and outside linear machining units. Note 2: The tool path shown at basic tool path above is selected automatically for machining units that are not subject to the selection of the parameter E95.
3-163
3
PROGRAM CREATION
2.
Detail tool path of an axial cut-in - Roughing Rapid feed Cutting feed Pi
Workpiece Clearance cua
ta Finishing surface
sa
M3P240
- Finishing Rapid feed Cutting feed Pi
Workpiece Clearance Finishing surface
sa
M3P241
The bold codes represent parameter addresses.
Pi: Initial point cua: Axial cutting depth DET-A to be entered in the tool sequence ta:
Axial cutting allowance SRV-A to be entered in a machining unit
sa: Axial finishing allowance FIN-A to be entered in a machining unit Note 1: The starting allowance of axial cutting, specified by the (safety) clearance, will become equal to parameter E7 if the following three states occur at the same time: - Bit 6 of parameter E95 is set to 1. - A pre-machining tool is included in that tool sequence. - The machining unit is either central linear, right-hand linear, left-hand linear, outside linear or inside linear machining. Note 2: The starting allowance of cutting in radial direction, specified by parameter E2, will become equal to parameter E5 if the following three states occur at the same time: - Bit 7 of parameter E95 is set to 1. - A pre-machining tool is included in that tool sequence. - The machining unit is either outside linear or inside linear machining. 3.
Other precaution on tool path If shape data, tool data or parameter are modified after the automatic determination of coordinates of approach point (displayed in yellow), the approach point will not be located on the same cutting start point and the tool path will also be modified.
3-164
PROGRAM CREATION
3-6-7
3
Automatic corner override In line and face machining, cutting an inside corner will require a larger allowance to be cut, resulting in an increased load of cutting. The automatic corner override is to automatically override a feedrate at the allowance increased portions to reduce the cutting load. 1.
Operating conditions
Automatically overridden
θ
a
SRV-R
P2
P1
M3P242
Cutting an inside corner will increase a cutting allowance by area a while moving the tool from P1 to P2 in the illustration. In this span, the feedrate is automatically overriden. This override, however, will be valid only when all of the following requirements (A, B, C) are satisfied: A.
Inside corner angle θ is equal to or less than the value entered in the parameter E25 (with θ ≤ E25).
θ
θ
θ
M3P243
3-165
3
PROGRAM CREATION
B.
A radial cutting allowance is equal to or less than the value entered in the parameter E23 (SRV-R ≤ tool diameter × E23/100) The load scarcely varies when SRV-R is near to the tool diameter.
SRV-R
M3P244
C.
A radial cutting allowance is equal to or less than the value entered in the parameter E24 (SRV-R ≤ tool diameter × E24/100) When SRV-R is small, the load varies scarcely.
SRV-R
M3P245
2.
Valid machining The corner override is valid in roughing for each of the right-hand linear machining, left-hand linear machining, outside linear machining, inside linear machining, end milling-step, pocket milling, pocket milling-mountain and pocket milling-valley.
3.
Override rate An override rate on the programmed cutting feedrate should be entered in the parameter E22. With the parameter set at 0, the automatic corner override function is invalid.
3-166
PROGRAM CREATION
3-7
3
Face Machining Units Face machining units are used to enter the data relating to the procedures for machining an area and to the form to be machined. Available in each unit are two sequences; one is the tool sequence in which tool-operation-associated data are entered and the other shape sequence in which the data relating to machining dimensions specified on drawing are entered.
3-7-1
Types of face machining units As shown below 7 types of face machining units are available: 1. Face milling
2. End milling-top
3. End milling-step
4. Pocket milling
5. Pocket milling-mountain
6. Pocket milling-valley
7. End milling-slot
M3P246 Fig. 3-23
Types of face machining unit
3-167
3
PROGRAM CREATION
3-7-2
Procedure for selecting face machining unit (1) Press the menu selector key (key located to the right of the menu keys) to display the following menu. POINT LINE FACE TURNING MANUAL MACH-ING MACH-ING MACH-ING PROGRAM
END
(2) Press the [FACE MACH-ING] menu key. !
The following menu is displayed.
FCE MILL TOP EMIL
STEP
POCKET
PCKT MT
PCKT VLY
SLOT
(3) Press the appropriate menu key of the desired machining unit.
3-168
SHAPE CHECK
>>>
PROGRAM CREATION
3-7-3
3
Unit data, automatic tool development and tool path of the face machining unit 1.
Face milling unit (FCE MILL) This unit is selected to machine a workpiece flatly on the surface by the use of a face milling tool. A.
Data setting
UNo.
UNIT
1
FCE MILL
SNo.
TOOL
R1
FCE MILL
F2
FCE MILL
MODE
NOM-φ
POS-B
No.
#
POS-C
APRCH-1
SRV-A
BTM
APRCH-2 TYPE
FIN-A
AFD
DEP-A
' '
'
WID-R
C-SP
FR
M
M
M
': Data are not necessary to be set here.
Remark 1: In this unit, face mills are automatically developed. Remark 2: For the tool sequence data setting, see Subsection 3-7-4. FCE MILL unit
Tool sequence
Shape sequence entered Finishing
Roughing
............... ............... ............... ............... ............... ............... ............... ...............
SRV-A
Face mill (for roughing)
FIN-A
D740PA133
BTM:
Face mill (for finishing)
D740PA050
A bottom roughness code is selected out of the menu.
FIN-A: An axial finishing allowance is automatically established once a bottom roughness code has been selected. B.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. In the tool sequence, a maximum of up to two tools are automatically developed, based on SRV-A and on FIN-A. Machining
Pattern
R1 (Roughing)
FIN-A = 0 : One tool is selected.
F2 (Finishing)
SRV-A ≤ FIN-A : One tool is selected.
3-169
3
PROGRAM CREATION
C.
Tool path When [X BI-DIR] is selected for the item TYPE in the tool sequence Y
E12 Workpiece
Rapid feed Cutting feed
Pe [1] E12
cur
[4]
Pa
cur Pc E12 X Z
[1] Pi Note 2 [2]
[5] Clearance
Pa
[3]
Pe
Workpiece
Pc
[4] X M3P249 The bold codes represent parameter addresses.
Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Pe: Escape point to be automatically established Pi: Initial point cur: Radial cutting depth to be determined by the data WID-R in the tool sequence [1]
The tool moves at a rapid feedrate to approach point.
[2]
The tool moves at a rapid feedrate to the clearance position.
[3]
The tool moves at a rapid feedrate to the face to be machined.
[4]
The tool moves at a cutting feedrate to the cutting start point and carries out machining.
[5]
Upon completion of machining, the tool moves at a rapid feedrate to initial point.
3-170
PROGRAM CREATION
3
When [X UNI-DIR] is selected for the item TYPE in the tool sequence Rapid feed Cutting feed
Y E12
Pe [1] cur [4]
Pa
cur Pc E12
E12 X
[1]
Z
[6] Note 2 [2]
Pi
[7] Clearance Workpiece
Pa
[3]
Pc
[5][8] Pe
[4] X
M3P250
The bold codes represent parameter addresses.
Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Pe: Escape point to be automatically established Pi: Initial point cur: Radial cutting depth to be determined by the data WID-R in the tool sequence [1]
The tool moves at a rapid feedrate to approach point.
[2]
The tool moves at a rapid feedrate to the clearance position.
[3]
The tool moves at a rapid feedrate to the face to be machined.
[4]
The tool moves at a cutting feedrate to the cutting start point and carries out machining.
[5], [6] and [7] Upon completion of machining in one direction, the tool moves at a rapid feedrate to initial point and to a subsequent cutting start point. [8]
Upon completion of machining, the tool moves at a rapid feedrate to initial point.
3-171
3
PROGRAM CREATION
When [X BI-DIR SHORT] is selected for the item TYPE in the tool sequence Y
Rapid feed Cutting feed
E12 Workpiece Pe
cur
[1]
cur
[4]
fo Pc
Pa E12 X Z
[1] Pi Note 2 [2] Clearance
[5] [3] Pa
Workpiece
Pc
Pe [4]
X M3P251 The bold codes represent parameter addresses.
Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Pe: Escape point to be automatically established Pi: Initial point cur: Radial cutting depth to be determined by the data WID-R in the tool sequence fo:
Form-offsetting clearance fo = tool diameter ×
E15 10
[1]
The tool moves at a rapid feedrate to approach point.
[2]
The tool moves at a rapid feedrate to the clearance position.
[3]
The tool moves at a rapid feedrate to the face to be machined.
[4]
The tool moves at a cutting feedrate to the cutting start point and carries out machining.
[5]
Upon completion of machining, the tool moves at a rapid feedrate to initial point.
3-172
PROGRAM CREATION
When [X BI-DIR ARCSHORT] is selected for the item TYPE in the tool sequence Y E12
Workpiece
Rapid feed Cutting feed
Pe
cur
[1]
cur
[4] Pc Pa
E12 Z
fo
X
[1] Pi [2]
Clearance Workpiece
[5] [3] Pa Note 2
Pc
Pe [4]
X D735P0083 The bold codes represent parameter addresses.
Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Pe: Escape point to be automatically established Pi: Initial point cur: Radial cutting depth to be determined by the data WID-R in the tool sequence fo:
Form-offsetting clearance fo = tool diameter ×
E15 10
[1]
The tool moves at a rapid feedrate to approach point.
[2]
The tool moves at a rapid feedrate to the clearance position.
[3]
The tool moves at a rapid feedrate to the face to be machined.
[4]
The tool moves at a cutting feedrate to the cutting start point and carries out machining.
[5]
Upon completion of machining, the tool moves at a rapid feedrate to initial point.
3-173
3
3
PROGRAM CREATION
Note 1: When ? is displayed in the items APRCH-1, -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operations [2] and [3] are performed. In this case, the coordinate of cutting start point will be entered in these items. Note 2: Detail of the Z-axial tool path. - Roughing Z
Rapid feed Cutting feed
[1] Pi [2] Workpiece Clearance [3] ct
tz Finishing surface
sz
X
M3P252
- Finishing Z
Rapid feed Cutting feed
[1] Pi [2]
Workpiece [3]
Clearance Finishing surface sz
X
M3P253
Pi: Initial point ct:
Z-axial cutting stroke to be determined by the data DEP-A in the tool sequence
tz:
Z-axial cutting allowance to be determined by the data SRV-A in a machining unit
sz: Z-axial finishing allowance FIN-A in a machining unit Note 3: See Subsection 3-7-5, “Precautions in face machining.”
3-174
PROGRAM CREATION
2.
3
End milling-top unit (TOP EMIL) This unit is selected to machine a workpiece flatly on the machine by the use of an end mill. A.
Data setting
UNo.
UNIT
1
TOP EMIL
SNo.
TOOL
R1
END MILL
F2
END MILL
MODE
NOM-φ
POS-B
No.
#
POS-C
APRCH-1
SRV-A
BTM
APRCH-2 TYPE
AFD
FIN-A
DEP-A
WID-R
C-SP
FR
M
M
M
' ': Data are not necessary to be set here.
Remark 1: In this unit, end mills are automatically developed. Remark 2: For the tool sequence data setting, see Subsection 3-7-4. TOP EMIL unit
Tool sequence
Shape sequence entered Finishing
Roughing
............... ............... ............... ............... ............... ............... ............... ...............
SRV-A
End mill (for roughing)
FIN-A
D740PA135
BTM:
End mill (for finishing)
D740PA051
A bottom roughness code is selected out of the menu.
FIN-A: An axial finishing allowance is automatically established once a bottom roughness code has been selected. B.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. In the tool sequence, a maximum of up to two tools are automatically developed, based on SRV-A and on FIN-A. Machining
Pattern
R1 (Roughing)
FIN-A = 0 : One tool is selected.
F2 (Finishing)
SRV-A ≤ FIN-A : One tool is selected.
3-175
3
PROGRAM CREATION
C.
Tool path When [X BI-DIR] is selected for the item TYPE in the tool sequence Y
Rapid feed Cutting feed
Workpiece
Pe [1]
[4]
Pa
Pc Note 3 X Z
[1] Pi Note 2 [2] Clearance
Workpiece
[5]
[3] Pa Pc
Pe X
M3P256
Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Pe: Escape point to be automatically established Pi: Initial point [1]
The tool moves at a rapid feedrate to approach point.
[2]
The tool moves at a rapid feedrate to the clearance position.
[3]
The tool moves to the face to be machined. (The feedrate is dependent upon the data AFD in the tool sequence.)
[4]
The tool moves at a cutting feedrate to the cutting start point and carries out machining.
[5]
Upon completion of machining, the tool moves at a rapid feedrate to initial point.
3-176
PROGRAM CREATION
3
When [X UNI-DIR] is selected for the item TYPE in the tool sequence Y
Rapid feed Cutting feed
Workpiece
Pe [1]
Pa
[4] [6] Pc Note 3 X
Z
[1] [6]
[2]
Pi [5]
[7]
[9] Clearance
[3] Note 2
[8]
Workpiece X
M3P257
Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Pe: Escape point to be automatically established Pi: Initial point [1]
The tool moves at a rapid feedrate to approach point.
[2]
The tool moves at a rapid feedrate to the clearance position.
[3]
The tool moves to the face to be machined. (The feedrate is dependent upon AFD in the tool sequence.)
[4]
The tool moves at a cutting feedrate to the cutting start point and carries out machining.
[5], [6] and [7] Upon completion of machining in one direction, the tool moves at a rapid feedrate to initial point. Then, it moves at a rapid feedrate to the subsequent cutting start point specified by the clearance above the next cutting start point. [8]
The tool moves at a cutting feedrate to the face to be machined and starts machining.
[9]
Upon completion of machining, the tool moves at a rapid feedrate to initial point.
3-177
3
PROGRAM CREATION
Note 1: When ? is displayed in the items APRCH-1, -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operations [2] and [3] are performed. In this case, the coordinates of cutting start point will be entered in these items. Note 2: See Subsection 3-7-5 “Precautions in face machining.” Note 3: Detail description of tool path Y
Cutting feed fo
td
Workpiece
[4]
cur Pc
fo
fo + rs fo X
M3P258
td: Diameter of a tool fo: Form offset clearance dependent upon both td and parameter E13 fo = td ×
E13 10
rs: Form offset amount rectangular to the cutting direction rs =
td 20
cur: Radial cutting depth per cycle, obtainable as follows: lv n lv = lm (*) – 2 × (fo + rs) lv n= cr cur =
cr:
Radial cutting depth (WID-R) to be entered in the tool sequence
n:
Number of radial cutting pass (an integer with fractions below the decimal point rounded up)
Form lm (*)
cur
Cutting direction M3P259
3-178
PROGRAM CREATION
3.
3
End milling-step unit (STEP) This unit is selected to machine a workpiece flatly on the surface by the use of an end mill, with a relief left behind. A.
UNo. 1
Data setting UNIT
MODE
POS-B
POS-C
SRV-A
BTM
WAL
FIN-A
FIN-R
STEP
SNo.
TOOL
R1
END MILL
F2
END MILL
NOM-φ No. # APRCH-1 APRCH-2 TYPE AFD TYPE PK-DEP DEP-A ' '
WID-R
C-SP FR
M
M
M
' ': Data are not necessary to be set here.
Remark 1: In this unit, end mills are automatically developed. Remark 2: For the tool sequence data setting, see Subsection 3-7-4. STEP unit
Tool sequence
Shape sequence entered Finishing Roughing FIN-R
.... .... .... .... .... .... .... ....
SRV-A
.... .... .... .... .... .... .... .... End mill (for roughing)
FIN-A D740PA137
BTM:
A buttom roughness code is selected out of the menu.
WAL:
A wall roughness code is selected out of the menu.
End mill (for finishing)
D740PA051
FIN-A: An axial finishing allowance is automatically established once a bottom roughness code has been selected. B.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. In the tool sequence, a maximum of up to two tools are automatically developed, based on SRV-A, FIN-A and FIN-R. Machining
Pattern
R1 (Roughing)
FIN-A = 0 and FIN-R = 0 : One tool is selected.
F2 (Finishing)
SRV-A ≤ FIN-A : One tool is selected.
3-179
3
PROGRAM CREATION
C.
Machining sequence End milling-step is performed in the following order. FIN-R
Roughing
Machining is performed with the end mill developed in the tool sequence R1. With SRV-A = FINA, this machining is not performed.
Relief FIN-A
SRV-A
Machining is performed with the end mill developed in the tool sequence F1. With FIN-A = 0, this machining is not performed. Bottom
Relief
Finishing Machining is performed with the end mill developed in the tool sequence F1. With FIN-R = 0, this machining is not performed.
Wall
Relief
M3P261
3-180
PROGRAM CREATION
D.
3
Machining pattern For roughing or bottom finishing, a machining pattern is selected by the parameter E91. - Either 0 or 1 in the related bit accordingly. For the details of the parameter E91, refer to the separate Parameter List/Alarm List/M-Code List. 0
1
E91 = 7 6 5 4 3 2 1 0
bit 0
Machining is performed from inside to outside.
Machining is performed from outside to inside.
Cutting direction reversing type: With the cutting direction reserved inside and outside are machined. After that, the rest is machined.
Fixed cutting direction type: Machining is performed in an identical direction while turning along an inside form.
bit 1
bit 7
NM210-00546
In case of machining from the outside, the tool moves inwards along an inside form.
3-181
To machine from the outside, the tool moves inwards along an outside form.
3
PROGRAM CREATION
E.
Tool path Roughing or bottom finishing Y
Rapid feed Cutting feed [6][10] [7]
[1]
[11] cur
Note 3
[15]
[9] sr
[5] [13]
Pe [14]
E2
[8][12]
[4]
Pa = Pc X Z
[1]
Pi [2] Note 2
Clearance [3]
Pa = Pc
X M3P262 The bold codes represent parameter addresses.
Pa, Pc:
Approach point to be determined by the data APRCH-1, -2 to be entered in the tool sequence and cutting start point (In the illustration above, the cutting start point is the approach point.)
Pe:
Escape point automatically established
Pi:
Initial point
cur:
Radial cutting depth to be determined by the data WID-R in the tool sequence
sr:
Radial finishing allowance to be determined by the data FIN-R in a machining unit
3-182
PROGRAM CREATION
3
Note 1: When ? is displayed in the items APRCH-1, -2, by pressing the [AUTO SET] menu key, the tool is postioned directly at the cutting start point and operations [2] and [3] are performed. In this case, the coordinates of cutting start point will be entered in these items. Note 2: See Subsection 3-7-5, “Precautions in face machining.” Note 3: When a tool moves over a tool path distant by the value entered in the parameter E2 from a machining form, the cutting feedrate is multiplied by the number entered in the parameter E16. [1]
The tool moves at a rapid feedrate to approach point (Cutting start point). (See Note 1.)
[2]
The tool moves at a rapid feedrate to the clearance position.
[3]
The tool moves to the face to be machined. (The feedrate is dependent upon the data AFD in the tool sequence.)
[4] - [15] The tool machines along an inside form while turning around a workpiece on the circumference. ([6] and [10] and [4], [8] and [12] have some portions pass through an identical path.) Wall finishing The tool is machining through a tool path identical with that for finishing in the LINE OUT unit. F.
Finishing Finishing is performed, based on the entered data FIN-A and FIN-R. Bottom finishing is performed, with 0 < FIN-A. Wall finishing is performed, with 0 < FIN-R.
3-183
3
PROGRAM CREATION
When both bottom and wall are finished in finishing, the point determined by the data APRCH-1, -2 in the tool sequence will be the approach point in bottom finishing. To transfer from bottom finishing to wall finishing, moreover, the tool moves at a rapid feedrate from the bottom-finishing escape point to the wall-finishing cutting start point as illustrated below. Rapid feed Cutting feed
Y
Wall finishing
Pc2 [7] Pe2 [3]
[6]
[1] Bottom finishing Pe1 X Z
Pi [3] [2]
[4]
[8]
[5] Pe1
Pc2
Pe2 X M3P263
Pe1: Escape point in bottom finishing Pc2: Cutting start point in wall finishing Pe2: Escape point in wall finishing Pi:
Initial point
Note 1: When ? is displayed in the items APRCH-1, -2, by pressing the [AUTO SET] menu key, the tool is postioned directly at the cutting start point and operations [2] and [3] are performed. In this case, the coordinates of cutting start point will be entered in these items. Note 2: When a tool moves over a tool path distant by the value entered in the parameter E2 from a machining form, the cutting feedrate is multiplied by the number entered in the parameter E16.
3-184
PROGRAM CREATION
4.
3
Pocket milling unit (POCKET) This unit is selected to carry out milling of a pocket form by the use of an end mill. A.
UNo.
Data setting UNIT
1
POCKET
SNo.
TOOL
R1
END MILL
F2
END MILL
MODE
POS-B
POS-C
SRV-A
BTM
NOM-φ No. # APRCH-1 APRCH-2 TYPE AFD
WAL
FIN-A
FIN-R
TYPE PK-DEP DEP-A WID-R ' '
INTER-R CHMF
C-SP FR
M
M
M
' ': Data are not necessary to be set here.
Remark 1: In this unit, end mills and a chamfering cutter are automatically developed. Instead of the chamfering cutter, a centering drill can be used for chamfering. Remark 2: For the tool sequence data setting, see Subsection 3-7-4. Note:
If a centering drill is used, a nose angle of 90 degrees is set for machining. POCKET unit
Tool sequence
Roughing Finishing CHMF FIN-R
SRV-A
.......... .......... .......... .......... .......... .......... .......... .......... .......... .......... .......... .......... .......... .......... ..........
Shape sequence entered
Chamfering End mill End mill cutter (for roughing) (for finishing)
FIN-A D740PA138
BTM:
A bottom roughness code is selected out of the menu.
WAL:
A wall roughness code is selected out of the menu.
D740PA052
FIN-A: An axial finishing allowance is automatically established once a bottom roughness code has been selected. FIN-R: A radial finishing allowance is automatically established, once a wall roughness code has been selected. B.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. In the tool sequence, a maximum of up to three tools are automatically developed, based on SRV-A, FIN-A, FIN-R and CHMF. Machining
Pattern
R1 (Roughing)
FIN-A = 0 and FIN-R = 0 : One tool is selected.
F2 (Finishing)
SRV-A ≤ FIN-A : One tool is selected.
(Chamfering)
CHMF ≠ 0 : One tool is selected.
3-185
3
PROGRAM CREATION
C.
Machining sequence Pocket milling is performed in the following order. Machining is performed with the end mill developed in the tool sequence R1. With SRV-A = FIN-A, this machining is not performed.
FIN-R
Roughing
SRV-A
FIN-A
Machining is performed with the end mill developed in the tool sequence F1. With FIN-A = 0, this machining is not performed. Bottom
Finishing
Machining is performed with the end mill developed in the tool sequence F1. With FIN-R = 0, this machining is not performed. Wall
M3P265
Machining is performed with the chamfering cutter or centering drill in the tool sequence. With CHMF = 0, this machining is not performed.
Chamfering
D.
Machining pattern For roughing or bottom finishing, a machining pattern is selected by the parameter E92. - Either 0 or 1 is entered in the related bit accordingly 0
1
E92 = 7 6 5 4 3 2 1 0
bit 0
M3P266
Machining is performed from inside to outside.
3-186
Machining is performed from outside to inside.
PROGRAM CREATION
E.
Tool path Machining from outside (roughing or bottom finishing) Rapid feed Cutting feed
Y
[1]
cur cur [7] [6] [4]
[5]
Pa
Pc sr
X [1] Z
Pi [2] [8]
Clearance [3] Pe
Pa
Note 2
X
M3P267
Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Pe: Escape point automatically established Pi: Initial point cur: Radial cutting depth to be determined by the data WID-R in the tool sequence sr:
Radial finishing allowance to be determined by the data in the machining unit
3-187
3
3
PROGRAM CREATION
Note 1: When ? is displayed in the items APRCH-1, -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operation [2] and [3] are performed. In this case, the coordinates of cutting start point will be entered in these items. Note 2: See Subsection 3-7-5, “Precautions in face machining.” [1]
The tool moves at a rapid feedrate to approach point. (See Note 1.)
[2]
The tool moves at a rapid feedrate to the clearance position.
[3]
The tool moves to the face to be machined. (The feedrate is dependent upon the data AFD in the tool sequence.)
[4]
The tool moves at a cutting feedrate to the cutting starting point.
[5], [6] and [7] The tool machines on an around by around basis inwards. [8]
Upon completion of machining, the tool moves at a rapid feedrate to initial point.
3-188
PROGRAM CREATION
Machining from inside (roughing or bottom finishing) Y
Rapid feed Cutting feed
[1]
cur cur
[4]
Pa
[5] Pc [6] [7] Pe sr
X Z
[1]
Pi [2] Clearance
[8] [3] Note 2
Pe
Pa
X
M3P268
Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Pe: Escape point automatically established Pi: Initial point cur: Radial cutting depth to be determined by the data WID-R in the tool sequence sr:
Radial finishing allowance to be determined by the data in the machining unit
3-189
3
3
PROGRAM CREATION
Note 1: When ? is displayed in the items APRCH-1, -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operation [2] and [3] are performed. In this case, the coordinates of cutting start point will be entered in these items. Note 2: See Subsection 3-7-5, “Precautions in face machining.” [1]
The tool moves at a rapid feedrate to approach point. (See Note 1.)
[2]
The tool moves at a rapid feedrate to the clearance position.
[3]
The tool moves to the face to be machined. (The feedrate is dependent upon the data AFD in the tool sequence.)
[4]
The tool moves at a cutting feedrate to the cutting starting point.
[5], [6] and [7] The tool machines on an around by around basis outwards. [8]
Upon completion of machining, the tool moves at a rapid feedrate to initial point.
Wall finishing The tool is machining through a tool path identical with that for finishing in the LINE IN unit. F.
Finishing Finishing is performed, based on the entered values of FIN-A and FIN-R. - Bottom finishing is performed, with 0 < FIN-A. - Wall finishing is performed, with 0 < FIN-R.
3-190
PROGRAM CREATION
3
When both bottom and wall are finished in finishing, the point determined by the data APRCH-1, -2 of the tool sequence will be the approach point in bottom finishing. To transfer from bottom finishing to wall finishing, moreover, the tool moves at a rapid feedrate from the bottom-finishing escape point to the wall-finishing cutting start point as illustrated below. Y
Rapid feed Cutting feed
Bottom finishing
[1]
Pe1 [3]
Wall finishing [6]
[7]
Pc2
X Z Pi [3] [2] Pe1
[4]
[5] Pc2 X
M3P269
Pe1: Escape point in bottom finishing Pc2: Cutting start point in wall finishing Pi: Note:
Initial point When ? is displayed in the items APRCH-1, -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operation [2] and [3] are performed. In this case, the coordinates of cutting start point will be entered in these items.
3-191
3
PROGRAM CREATION
5.
Pocket milling-mountain unit (PCKT MT) This unit is selected to carry out milling of a pocket form with relief left behind by the use of an end mill. A.
UNo. 1
Data setting UNIT
MODE
POS-B
POS-C
SRV-A
BTM
WAL
FIN-A
FIN-R
PCKT MT
SNo.
TOOL
R1
END MILL
F2
END MILL
NOM-φ No. #
APRCH-1 APRCH-2 TYPE AFD
TYPE PK-DEP DEP-A WID-R C-SP FR ' '
M
M
M
' ': Data are not necessary to be set here.
Remark 1: In this unit, end mills are automatically developed. Remark 2: For the tool sequence data setting, see Subsection 3-7-4. PCKT MT unit
Tool sequence
FIN-R Finishing Roughing
.. .. .. .. .. .. .. .. .. .. .. .. .. .. ..
SRV-A
Shape sequence entered
.. .. .. .. .. .. .. .. .. .. .. .. .. .. .. End mill (for roughing)
FIN-A D740PA140
BTM:
A buttom roughness code is selected out of the menu.
WAL:
A wall roughness code is selected out of the menu.
End mill (for finishing)
D740PA051
FIN-A: An axial finishing allowance is automatically established once a bottom roughness code has been selected. FIN-R: A radial finishing allowance is automatically established, once a wall roughness code has been selected. B.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. In the tool sequence, a maximum of up to two tools are automatically developed, based on SRV-A, FIN-A and FIN-R. Machining
Pattern
R1 (Roughing)
FIN-A = 0 and FIN-R = 0 : One tool is selected.
F2 (Finishing)
SRV-A ≤ FIN-A : One tool is selected.
3-192
PROGRAM CREATION
C.
3
Machining sequence Pocket milling is performed in the following order. Machining is performed with the end mill developed in the tool sequence R1. With SRV-A = FINA, this machining is not performed.
FIN-R
Roughing
Relief
SRV-A
FIN-A
Machining is performed with the end mill developed in the tool sequence F1. With FIN-A = 0, this machining is not performed. Bottom
Finishing
Relief
Machining is performed with the end mill developed in the tool sequence F1. With FIN-R = 0, this machining is not performed.
Outer wall
Relief
Inner wall
Relief
M3P271
3-193
3
PROGRAM CREATION
D.
Machining pattern For roughing or bottom finishing, a machining pattern is selected by the parameter E93. - Enter 0 or 1 in the related bit accordingly. 0
1
E93 = 7 6 5 4 3 2 1 0
bit 0
Machining is performed from inside to outside.
Machining is performed from outside to inside.
Cutting direction reversing type:
Fixed cutting direction type:
With the cutting direction reversed, inside and outside are machined. After that, the rest is machined.
Machining is performed in an identical direction along an inside form.
bit 1
M3P272
3-194
PROGRAM CREATION
E.
Tool path Machining from outside (roughing or bottom finishing) - Machining along outer and inner walls: Rapid feed Cutting feed
Y
[1] [7]
[8][11]
[10]
Pa
[12] [4] [9]
[6] cur
[5]
sr X Z
[1]
Pi Note 2
[2]
Clearance [3]
Pa
X M3P273
3-195
3
3
PROGRAM CREATION
- Machining the rest: Rapid feed Cutting feed
Y
[13] [14] Pe
[12]
[11]
X Z
Pi
[15] Pe
X M3P274
Pa: Approach point to be determined by the data APRCH-1, -2 in the tool sequence Pc: Cutting start point to be automatically established Pe: Escape point to be automatically established Pi: Initial point cur: Radial cutting depth to be determined by the data WID-R in the tool sequence sr:
Radial finishing allowance to be determined by the data FIN-R in a machining unit
3-196
PROGRAM CREATION
3
Note 1: When ? is displayed in the items APRCH-1, -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operation [2] and [3] are performed. In this case, the coordinates of cutting start point will be entered in these items. Note 2: See Subsection 3-7-5, “Precautions in face machining.” [1]
The tool moves at a rapid feedrate to approach point. (See Note 1.)
[2]
The tool moves at a rapid feedrate to the clearance position.
[3]
The tool moves to the face to be machined. (The feedrate is dependent upon the data AFD in the tool sequence.)
[4]
The tool moves at a cutting feedrate to the cutting starting point.
[5] and [6] The tool machines along the outside form. [7]
Once it has interfered with the inside form, the tool machines along the inside form.
[8]
Once it has got out of the inside form, the tool moves along the outside form.
[9]
To machine along the inside form, the tool moves along the same path as that in [6].
[10] Because of the path reversed, once it has interfered with the inside form, the tool machines along the inside form. [11] To machine the rest, the tool moves along the same path as that in [8]. [12], [13] and [14] [15]
The rest is machined inwards on an around by around basis.
Upon completion of machining, the tool moves at a rapid feedrate to initial point.
3-197
3
PROGRAM CREATION
Machining from inside (roughing or bottom finishing) Rapid feed Cutting feed
Y [1]
[9]
[6] [10]
[4]
[5] [7]
[12] [13]
[8] Pa Pe
[11] Pc
cur
sr X Z [1]
Pi Note 2
[2] [14] Clearance [3]
Pa = Pc
Pe
X M3P275
Pa, Pc:
Approach point to be determined by the data APRCH-1, -2 to be entered in the tool sequence and cutting start point. (In the illustration above, the cutting start point is the approach point.)
Pe:
Escape point to be automatically established
In [7] and [8], and [5] and [10], the tool moves reversely on an identical path. Note 1: When ? is displayed in the items APRCH-1, -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operation [2] and [3] are performed. In this case, the coordinates of cutting start point will be entered in these items. Note 2: See Subsection 3-7-5, “Precautions in face machining.”
3-198
PROGRAM CREATION
3
Outer wall finishing The tool is machining through a tool path identical with that for finishing in the LINE IN unit. Inner wall finishing The tool is machining through a tool path identical with that for finishing in the LINE OUT unit. F.
Finishing Finishing is performed, based on the entered data FIN-A and FIN-R. - Bottom finishing is performed, with 0 < FIN-A. - Outer and inner walls are finished, with 0 < FIN-R. When both bottom and wall are finished in finishing, the point determined by the data APRCH-1, -2 of the tool sequence will be the approach point in bottom finishing. To transfer from bottom finishing to wall finishing or from outer wall finishing to inner wall finishing, moreover, the tool moves at a rapid feedrate from the escape point to the cutting start point as illustrated below.
3-199
3
PROGRAM CREATION
When wall-finishing is performed in finishing, outer wall and inner wall are finished in this order (outer wall finishing → inner wall finishing), irrespective of setting for parameter E93 bit 0. Y
Rapid feed Cutting feed
Inner wall finishing
[11]
[1]
Bottom finsihing
Pe1 [3] [6]
Pe2
Pe3
Outer finishing Pc2
Pc3
X Z [3]
[8]
[12]
[9]
Pi [7]
[4]
[10]
[2]
[5]
Pe3 Pc3 Pe2
Pc2
Pe1 X M3P276
Pe1: Escape point in bottom finishing Pc2: Cutting start point in outer wall finishing Pe2: Escape point in outer wall finishing Pc3: Cutting start point in inner wall finishing Pe3: Escape point in inner wall finishing Pi: Note:
Initial point When ? is displayed in the items APRCH-1, -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operation [2] and [3] are performed. In this case, the coordinates of cutting start point will be entered in these items.
3-200
PROGRAM CREATION
6.
3
Pocket milling-valley unit (PCKT VLY) This unit is selected to carry out pocket milling-valley by the use of an end mill. A.
Data setting
UNo.
UNIT
1
PCKT VLY
SNo.
TOOL
R1
END MILL
F2
END MILL
MODE
POS-B
NOM-φ No. #
POS-C
SRV-A
BTM
WAL
FIN-A
FIN-R
APRCH-1 APRCH-2 TYPE AFD TYPE PK-DEP DEP-A WID-R C-SP FR ' '
M
M
M
' ': Data are not necessary to be set here.
Remark 1: In this unit, end mills are automatically developed. Remark 2: For the tool sequence data setting, see Subsection 3-7-4. PCKT VLY unit
Tool sequence
Roughing
FIN-R
Finishing
SRV-A
Shape sequence entered
... ... ... ... ...
... ... ... ... ...
FIN-A End mill (for roughing)
D740PA141
BTM:
A buttom roughness code is selected out of the menu.
WAL:
A wall roughness code is selected out of the menu.
End mill (for finishing)
D740PA051
FIN-A: An axial finishing allowance is automatically established once a bottom roughness code has been selected. FIN-R: A radial finishing allowance is automatically established, once a wall roughness code has been selected. B.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. In the tool sequence, a maximum of up to two tools are automatically developed, based on SRV-A, FIN-A and FIN-R. Machining
Pattern
R1 (Roughing)
FIN-A = 0 and FIN-R = 0 : One tool is selected.
F2 (Finishing)
SRV-A ≤ FIN-A : One tool is selected.
3-201
3
PROGRAM CREATION
C.
Machining sequence Pocket milling-valley is performed in the following order. Machining is performed with the end mill developed in the tool sequence R1. With SRV-A = FINA, this machining is not performed.
FIN-R
Roughing
SRV-A Hollow FIN-A
Machining is performed with the end mill developed in the tool sequence F1. With FIN-A = 0, this machining is not performed. Bottom
Hollow
Finishing
Machining is performed with the end mill developed in the tool sequence F1. With FIN-R = 0, this machining is not performed. Wall Hollow
M3P278
3-202
PROGRAM CREATION
D.
3
Machining pattern For roughing or bottom finishing, a machining pattern is selected by the parameter E94. - Enter 0 or 1 in the related bit accordingly. 0
1
E94 = 7 6 5 4 3 2 1 0
bit 0
Machining is performed from inside to outside.
Machining is performed from outside to inside.
Cutting direction reversing type:
Fixed cutting direction type: Machining is performed in an identical direction along an inside form.
bit 1
D740PA159
With the cutting direction reversed, inside and outside are machined. After that, the rest is machined.
3-203
3
PROGRAM CREATION
E.
Tool path Machining from inside (roughing or bottom finishing) - Machining along an outer wall after expanding a valley along an inside form: Y
[1]
Rapid feed Cutting feed
[10]
[7] [5] [11]
[8] Pa = Pc cur [4] [6]
[9] [12]
sr Z
X
[1]
Pi [2] Note 2
Clearance [3]
Pa = Pc
X D740PA160
3-204
PROGRAM CREATION
3
- Machining the rest: Rapid feed Cutting feed
Y
[13] [14]
cur
[11] Pe
[12]
X Z
Pi [15] Pe
X M3P281
Pa, Pc: Approach point to be determined by the data APRCH-1, -2 in the tool sequence and cutting start point (In the illustration above, the cutting start point is the approach point.) Pe:
Escape point to be automatically established
Pi:
Initial point
cur:
Radial cutting depth to be determined by the data WID-R in the tool sequence
sr:
Radial finishing allowance to be determined by the data FIN-R in a machining unit
Note 1: When ? is displayed in the items APRCH-1, -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operation [2] and [3] are performed. In this case, the coordinates of cutting start point will be entered in these items. Note 2: See Subsection 3-7-5, “Precautions in face machining.”
3-205
3
PROGRAM CREATION
[1]
The tool moves at a rapid feedrate to approach point (cutting start point). (See Note 1.)
[2]
The tool moves at a rapid feedrate to the clearance position.
[3]
The tool moves to the face to be machined. (The feedrate is dependent upon the data AFD in the tool sequence.)
[4]
The tool moves to the cutting position in a workpiece.
[5] and [6] The tool expands a hole along the valley form. [7]
Once it has interfered with the wall of an outside form, the tool machines along the outside form.
[8]
Once it has got out of the outside form, the tool expands the hole along the valley form.
[9]
To machine along the outside form, the tool moves along the same path as that in [8].
[10] Once it has interfered with the outside form, the tool machines along the outside form. [11] To machine the rest, the tool moves along the same path as that in [6]. [12], [13] and [14]
The rest is machined outwards on an around by around basis.
[15] Upon completion of machining, the tool moves at a rapid feedrate to initial point.
3-206
PROGRAM CREATION
3
Machining from outside (roughing or bottom finishing) Y
Rapid feed Cutting feed [1] [7] [10] [6] [9]
[12] [13]
[11] [5]
[8] [4]
Pa = Pc
X Z
[1]
Pi Note 2
[2] [14]
Pa = Pc
[3]
Clearance X D740PA161
Pa, Pc:
Approach point to be determined by the data APRCH-1, -2 in the tool sequence. (In the illustration above, the cutting start point is the approach point.)
Pe:
Escape point to be automatically established
Tool path [8] and [10] is the same as that of [5] and [7] respectively. Note 1: When ? is displayed in the items APRCH-1, -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operation [2] and [3] are performed. In this case, the coordinates of cutting start point will be entered in these items. Note 2: See Subsection 3-7-5, “Precautions in face machining.” Outer wall finishing The tool is machining through a tool path identical with that for finishing in the LINE IN unit.
3-207
3
PROGRAM CREATION
F.
Finishing Finishing is performed, based on the entered data FIN-A and FIN-R. Bottom finishing is performed, with 0 < FIN-A. Wall finsihing is performed, with 0 < FIN-R. When both bottom and wall are finished in finishing, the point determined by the data APRCH-1, -2 of the tool sequence will be the approach point in bottom finishing. To transfer from bottom finishing to wall finishing, moreover, the tool moves at a rapid feedrate from the bottom-finishing escape point to the wall-finishing cutting start point as illustrated below. Y
Rapid feed Cutting feed
Wall finishing
Bottom finishing
[1] [3] [7]
Pc2
Pe1
[6]
X Z [3] Pi
[8]
[4]
[2]
Pc2 Pe1 [5]
Pe2
X M3P283
Pe1: Escape point in bottom finishing Pc2: Cutting start point in wall finishing Pe2: Escape point in wall finishing Pi: Note:
Initial point When ? is displayed in the items APRCH-1, -2 by pressing the [AUTO SET] menu key, the tool is positioned directly at the cutting start point and operation [2] and [3] are performed. In this case, the coordinates of cutting start point will be entered in these items.
3-208
PROGRAM CREATION
7.
3
End milling-slot unit (SLOT) This unit is selected to carry out slot machining by the use of an end mill. A.
UNo. 1
Data setting UNIT
MODE
POS-B
POS-C
SRV-A
SLOT-WID
BTM
WAL FIN-A
FIN-R
SLOT
SNo.
TOOL
R1
END MILL
F2
END MILL
NOM-φ No.
#
APRCH-1 APRCH-2 TYPE AFD TYPE PK-DEP DEP-A WID-R C-SP FR ' '
M
M
M
' ': Data are not necessary to be set here.
Remark 1: In this unit, end mills are automatically developed. Remark 2: For the tool sequence data setting, see Subsection 3-7-4. SLOT unit
Shape sequence entered
Tool sequence
Roughing FIN-R
Finishing
...... ...... ...... ...... ...... ...... ...... ...... ...... ...... ...... ......
SRV-A
FIN-A
End mill (for roughing)
SLOT-WID
End mill (for finishing)
D740PA142
BTM:
A buttom roughness code is selected out of the menu.
WAL:
A wall roughness code is selected out of the menu.
D740PA051
FIN-A: An axial finishing allowance is automatically established once a bottom roughness code has been selected. FIN-R: A radial finishing allowance is automatically established, once a wall roughness code has been selected. B.
Automatic tool development The tools are automatically developed according to different patterns on the basis of the data entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool. In the tool sequence, a maximum of up to two tools are automatically developed, based on SRV-A, SLOT-WID, FIN-A and FIN-R. Machining
Pattern
R1 (Roughing)
FIN-A = 0 and FIN-R = 0 : One tool is selected.
F2 (Finishing)
SRV-A ≤ FIN-A or SLOT-WID ≤ (2 × FIN-R) : One tool is selected.
3-209
3
PROGRAM CREATION
C.
Tool path SLOT-WID 2
With tool radius + FIN-R
Finishing allowance: One tool for roughing is automatically selected.
F2 (Finishing)
Finishing allowance > 0 : One tool for finishing is automatically selected.
[1] TOOL (Name) The name of the tool to be used for machining is set automatically. When the cursor is present at this item, the following menu is displayed to allow the tool to be changed: GENERAL
GROOVE
THREAD
T.DRILL
T.TAP
SIMUL DRILL ROTATION
SPECIAL
[1] TOOL (Section to be machined) When the cursor is present at this item, the appropriate menu according to the tool name that was selected at item [1] TOOL (Name) is displayed as shown below. - If either GENERAL, GROOVE, or THREAD has been selected OUT IN OUTER INNER DIAMETER DIAMETER
EDG EDGE
IN INNER (BAK)
EDG EDGE (BAK)
- If either T-DRILL, or T-TAP has been selected EDG EDGE
EDG EDGE (BAK)
- If SPECIAL has been selected 0001
0002
0003
0004
0005
0006
0007
0008
0009
When creating a copy-machining unit, usually select tools as follows according to the machining section that has been selected for the unit: PART in the unit (Section to be machined)
TOOL (Name)
TOOL (Section to be machined)
OUT
OUT OUTER DIAMETER
OUT
OUT OUTER DIAMETER IN INNER DIAMETER, IN INNER (BAK)
IN IN FACE
GENERAL
IN INNER DIAMETER, IN INNER (BAK) OUT OUTER DIAMETER, EDG EDGE, EDG EDGE (BAK)
FACE
EDG EDGE, EDG EDGE (BAK)
BACK
OUT OUTER DIAMETER, EDG EDGE (BAK)
BACK
EDG EDGE (BAK)
3-276
PROGRAM CREATION
Note:
3
The above example applies when the tools best suited to a general machining shape pattern are to be used. Tools other than those shown in the above example may be suitable for the shape actually specified.
[3] NOM. (Nominal size) Enter the nominal size of tools using the numeric keys. See the description of the relevant items for BAR unit. [4] NOM. (Suffix) A code should be selected out of the menu to identify those tools which are of identical type (having an identical name) and have an identical nominal size. A
B
C
D
E
F
G
H
HEAVY TOOL
>>>
[5] NOM. (Turret selection) For a machine equipped with upper and lower turrets, select the turret in which the tool to be used is mounted. The following menu will be displayed. See the description of the relevant item for BAR unit. SET UPPER TURRET
SET LOWER TURRET
[6] No. (Priority No.) Assign priority levels in the order of machining. See the description of the relevant item for BAR unit. [7] # (Simultaneous machining No., balanced cutting, or retraction position of the lower turret) For a machine equipped with upper and lower turrets, to use the tools mounted in both turrets, specify either the simultaneous machining number or balanced cutting. It is also possible to specify the position to which the lower turret is to be retracted when machining workpieces using only the upper turret. The following menu will be displayed. When specifying the simultaneous machining number, enter the number directly from the keyboard, not using the menu: LOWER TURRET ESCAPE
BALANCE FEED 2
Note:
See Chapter 5, “LOWER-TURRET CONTROL FUNCTIONS”, for details of items [5] and [7].
[8] DEP-1 (Maximum cutting depth) Specify the maximum cutting depth per roughing pass. The maximum cutting depth in the X-axial direction is to be specified in terms of radius. See the description of the relevant item for BAR unit. [9] FIN-X, [10] FIN-Z Specify the allowance to be left for the next finishing tool sequence. See the description of the relevant items for BAR unit. [11] C-SP Specify the surface speed for the turning spindle. See the description of the relevant item for BAR unit.
3-277
3
PROGRAM CREATION
[12] FR Enter the desired feedrate of the tool in terms of turning spindle speed per revolution. See the description of the relevant item for BAR unit. [13] M Specify the M-code to be issued for the tool immediately after it is selected. See the description of the relevant item for BAR unit.
3-10-3 Setting shape sequence data FIG
PTN
S-CNR
SPT-X
SPT-Z
FPT-X
FPT-Z
F-CNR/$
R/th
RGH
1
[1]
[2]
[3]
[4]
[5]
[6]
[7]
[8]
[9]
The shape sequence data for the copy-machining unit is the same as that for the bar-materials machining unit. See the description of the relevant item in Section 3-9 “Bar-Materials Machining Unit (BAR)”.
3-278
PROGRAM CREATION
3
3-11 Corner-Machining Unit (CORNER) Part of the corners of a workpiece may remain uncut because of the particular tool shape for the bar-materials machining unit (BAR) or the copy-machining unit (CPY). Select the cornermachining unit (CORNER) when uncut portions are to be removed to make all corners rightangled.
C: Subsidiary cutting-edge angle
Uncut portion
Removed portion
Machining pattern
Corner-machining unit T4P063’
Press the [CORNER
] menu key to select this unit.
3-11-1 Setting unit data UNo.
UNIT
PART
POS-B
FIN-X
FIN-Z
∗
CORNER
[1]
[2]
[3]
[4]
[1] PART The following menu will be displayed when the cursor is placed at this item. OUT
IN
FACE
BACK
From the menu, select the section to be machined. Sections to be machined that correspond to the data of the displayed menu are as follows. OUT IN FACE BACK
: : : :
Uncut portion on outer periphery Uncut portion on inner periphery Uncut portion on front face Uncut portion on back face
[2] POS-B From the menu, select an angle for indexing the B-axis. You can specify an angle using numeric keys. See the description of the relevant item for BAR unit. [3] FIN-X, [4] FIN-Z Specify the allowance to be left for the next finishing tool sequence. See the description of the relevant items for BAR unit.
3-279
3
PROGRAM CREATION
3-11-2 Setting tool sequence data SNo.
TOOL
NOM.
No.
#
PAT. DEP-1 DEP-2/NUM. DEP-3
R1
!
!
!
!
FIN-X FIN-Z C-SP FR !
!
!
↑
↑
↑
↑
↑
↑
↑
↑
↑
[1]
[2] [3] [4] [5] [6]
[7]
[8]
[9]
[10]
[11]
[12]
F2
Remark 1:
↑ ↑ ↑
!:
M
M
M
!
↑
↑ ↑ ↑
[13] [14] [14] [14]
Data are not necessary to be set here.
Remark 2: In the tool sequence, a maximum of up to two tools are automatically developed as follows. Machining
Pattern
R1 (Roughing)
One tool for roughing is automatically selected.
F2 (Finishing)
Finishing allowance > 0 : One tool for finishing is automatically selected.
[1] TOOL (Name) The name of the tool to be used for machining is set automatically. When the cursor is present at this item, the following menu is displayed to allow the tool to be changed: GENERAL
GROOVE
THREAD
T.DRILL
T.TAP
SIMUL DRILL ROTATION
SPECIAL
[2] TOOL (Section to be machined) When the cursor is present at this item, the appropriate menu according to the tool name that was selected at item [1] TOOL (Name) is displayed as shown below. - If either GENERAL, GROOVE, or THREAD has been selected OUT IN OUTER INNER DIAMETER DIAMETER
EDG EDGE
IN INNER (BAK)
EDG EDGE (BAK)
- If either T-DRILL, or T-TAP has been selected EDG EDGE
EDG EDGE (BAK)
- If SPECIAL has been selected 0001
0002
0003
0004
0005
0006
0007
0008
0009
When creating a corner-machining unit, usually select tools as follows according to the machining section that has been selected for the unit: PART in the unit (Section to be machined)
TOOL (Name)
OUT IN FACE BACK
Note:
TOOL (Section to be machined) OUT OUTER DIAMETER IN INNER DIAMETER, IN INNER (BAK)
GENERAL
OUT OUTER DIAMETER, EDG EDGE, EDG EDGE (BAK) OUT OUTER DIAMETER, EDG EDGE (BAK)
The above example applies when the tools best suited to a general machining shape pattern are to be used. Tools other than those shown in the above example may be suitable for the shape actually specified.
3-280
PROGRAM CREATION
3
[3] NOM. (Nominal size) Enter the nominal size of tools using the numeric keys. See the description of the relevant item for BAR unit. [4] NOM. (Suffix) A code should be selected out of the menu to identify those tools which are of identical type (having an identical name) and have an identical nominal size. A
B
C
D
E
F
G
H
HEAVY TOOL
>>>
[5] NOM. (Turret selection) For a machine equipped with upper and lower turrets, select the turret in which the tool to be used is mounted. The following menu will be displayed. See the description of the relevant item for BAR unit. SET UPPER TURRET
SET LOWER TURRET
[6] No. (Priority No.) Assign priority levels in the order of machining. See the description of the relevant item for BAR unit. [7] # (Simultaneous machining No., balanced cutting, or retraction position of the lower turret) For a machine equipped with upper and lower turrets, to use the tools mounted in both turrets, specify either the simultaneous machining number or balanced cutting. It is also possible to specify the position to which the lower turret is to be retracted when machining workpieces using only the upper turret. The following menu will be displayed. When specifying the simultaneous machining number, enter the number directly from the keyboard, not using the menu: LOWER TURRET ESCAPE
BALANCE FEED 2
Note:
See Chapter 5, “LOWER-TURRET CONTROL FUNCTIONS”, for details of items [5] and [7].
[8] PAT. (Machining pattern) The following menu will be displayed when the cursor is placed at this item. #0
#1
(a)
(b)
Select a rough-machining pattern from (a) or (b) above. See the description of the relevant item for BAR unit. [9] DEP-1 (Maximum cutting depth) Specify the maximum cutting depth per roughing pass. The maximum cutting depth in the X-axial direction is to be specified in terms of radius. See the description of the relevant item for BAR unit.
3-281
3
PROGRAM CREATION
[10] FIN-X, [11] FIN-Z Specify the allowance to be left for the next finishing tool sequence. See the description of the relevant items for BAR unit. [12] C-SP Specify the surface speed for the turning spindle. See the description of the relevant item for BAR unit. [13] FR Enter the desired feedrate of the tool in terms of turning spindle speed per revolution. See the description of the relevant item for BAR unit. [14] M Specify the M-code to be issued for the tool immediately after it is selected. See the description of the relevant item for BAR unit.
3-11-3 Setting shape sequence data FIG
SPT-X
SPT-Z
FPT-X
FPT-Z
F-CNR/$
RGH
1
[1]
[2]
[3]
[4]
[5]
[6]
[1] SPT-X, [2] SPT-Z, [3] FPT-X, [4] FPT-Z Set the coordinates of the desired start and end points of cornering. The position of the start point and the end point are shown below.
End point Corner
Cutting portion
Start point Cutting portion
Start point Corner
End point
Corner
Corner Start point
Start point
End point
End point Cutting portion
Cutting portion
T4P066
[5] F-CNR/$ This item applies to the corners shown in the figure below, not the ending-point section. Enter data in this item to perform C-chamfering, R-chamfering, or polish-necking operations. For data setting method, see the relevant items for BAR unit. [6] RGH Set the appropriate, finish-machining feedrate for particular finishing surface roughness. For data setting method, see the relevant items for BAR unit.
3-282
PROGRAM CREATION
3
3-12 Facing Unit (FACING) Select the facing unit when chipping off any protrusions of the workpiece edges (front face or back face).
Workpiece edge
NM210-00431
Press the [FACING
] menu key to select this unit.
3-12-1 Setting unit data UNo.
UNIT
PART
POS-B
FIN-Z
∗
FACING
[1]
[2]
[3]
[1] PART The following menu will be displayed when the cursor is placed at this item. FACE
BACK
From the menu, select the section to be machined. Sections to be machined that correspond to each menu item are as follows: FACE : Right edge of the workpiece BACK : Left edge of the workpiece [2] POS-B From the menu, select an angle for indexing the B-axis. You can specify an angle using numeric keys. See the description of the relevant item for BAR unit. [2] FIN-Z Set the finishing allowances for the Z-axis directions (removal allowances during finishing). See the description of the relevant item for BAR unit.
3-283
3
PROGRAM CREATION
3-12-2 Setting tool sequence data SNo.
TOOL
NOM.
No.
#
PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP !
R1
!
F2
↑ ↑ ↑
!
!
!
!
!
!
!
FR
M
M
M
↑
↑
↑
↑
!
↑
↑
↑
↑
↑
↑
↑
[1]
[2] [3] [4] [5] [6]
[7]
[8]
[9]
[10]
[11] [12] [12] [12]
Remark 1: !: Data are not necessary to be set here. Remark 2: In the tool sequence, a maximum of up to two tools are automatically developed as follows. Machining
Pattern
R1 (Roughing)
One tool for roughing is automatically selected.
F2 (Finishing)
Finishing allowance > 0 : One tool for finishing is automatically selected.
[1] TOOL (Name) The name of the tool to be used for machining is set automatically. When the cursor is present at this item, the following menu is displayed to allow the tool to be changed: GENERAL
GROOVE
THREAD
T.DRILL
T.TAP
SIMUL DRILL ROTATION
SPECIAL
[2] TOOL (Section to be machined) When the cursor is present at this item, the appropriate menu according to the tool name that was selected at item [1] TOOL (Name) is displayed as shown below. - If either GENERAL, GROOVE, or THREAD has been selected OUT IN OUTER INNER DIAMETER DIAMETER
EDG EDGE
IN INNER (BAK)
EDG EDGE (BAK)
- If either T-DRILL, or T-TAP has been selected EDG EDGE
EDG EDGE (BAK)
- If SPECIAL has been selected 0001
0002
0003
0004
0005
0006
0007
0008
0009
When creating a facing unit, usually select tools as follows according to the machining section that has been selected for the unit: PART in the unit (Section to be machined) FACE BACK
Note:
TOOL (Name)
TOOL (Section to be machined) OUT OUTER DIAMETER, EDG EDGE, EDG EDGE (BAK)
GENERAL
OUT OUTER DIAMETER, EDG EDGE (BAK)
The above example applies when the tools best suited to a general machining shape pattern are to be used. Tools other than those shown in the above example may be suitable for the shape actually specified.
3-284
PROGRAM CREATION
3
[3] NOM. (Nominal size) Enter the nominal size of tools using the numeric keys. See the description of the relevant item for BAR unit. [4] NOM. (Suffix) A code should be selected out of the menu to identify those tools which are of identical type (having an identical name) and have an identical nominal size. A
B
C
D
E
F
G
H
HEAVY TOOL
>>>
[5] NOM. (Turret selection) For a machine equipped with upper and lower turrets, select the turret in which the tool to be used is mounted. The following menu will be displayed. See the description of the relevant item for BAR unit. SET UPPER TURRET
SET LOWER TURRET
[6] No. (Priority No.) Assign priority levels in the order of machining. See the description of the relevant item for BAR unit. [7] # (Simultaneous machining No. or retraction position of the lower turret) For a machine equipped with upper and lower turrets, to use the tools mounted in both turrets, specify the simultaneous machining number. It is also possible to specify the position to which the lower turret is to be retracted when machining workpieces using only the upper turret. The following menu will be displayed: LOWER TURRET POS.1
Note:
LOWER TURRET POS.2
See Chapter 5, “LOWER-TURRET CONTROL FUNCTIONS”, for details of items [5] and [7].
[8] DEP-1 (Maximum cutting depth) Specify the maximum cutting depth per roughing pass. The maximum cutting depth in the X-axial direction is to be specified in terms of radius. See the description of the relevant item for BAR unit. [9] FIN-Z Specify the allowance to be left for the next finishing tool sequence. See the description of the relevant items for BAR unit. [10] C-SP Specify the surface speed for the turning spindle. See the description of the relevant item for BAR unit. [11] FR Enter the desired feedrate of the tool in terms of turning spindle speed per revolution. See the description of the relevant item for BAR unit.
3-285
3
PROGRAM CREATION
[12] M Specify the M-code to be issued for the tool immediately after it is selected. See the description of the relevant item for BAR unit.
3-12-3 Setting shape sequence data FIG
SPT-X
SPT-Z
FPT-X
FPT-Z
RGH
1
[1]
[2]
[3]
[4]
[5]
[1] SPT-X, [2] SPT-Z, [3] FPT-X, [4] FPT-Z Set the coordinates of the machining start point and end point. For the facing unit, set as a plus value the Z-coordinates of all points located to the right of the program zero-point, or set as a minus value the Z-coordinates of all points located to the left of the program origin.
: Start point : End point
35 5
4
φ60
φ60
φ20
Negative value
SPT-X 60.
φ20
Program origin
SPT-Z 5.
Negative value
Positive value
FPT-X 20.
FPT-Z 0.
Program origin
SPT-X 60.
SPT-Z –35.
FPT-X 20.
Positive value
FPT-Z –31.
[5] RGH Set the appropriate finish-machining feedrate for particular finishing surface roughness. This setting can be done by selecting a surface roughness code or by directly setting any desired feedrate. See related items of “Bar-materials machining unit (BAR)”.
3-286
PROGRAM CREATION
Note:
3
The tool path for BAR and CPY units is calculated in general with the end-face clearance set in parameter TC39. For a BAR or CPY unit preceded by a FACING unit, in particular, the value of parameter TC45 is used as the end-face clearance.
BAR machining not preceded by FACING machining
BAR machining after FACING machining
TC39
TC45
BAR
BAR
FACING
TC45 is valid even in the following case: TC45
BAR
FACING
3-287
3
PROGRAM CREATION
3-13 Threading Unit (THREAD) Select the threading unit to thread the outer peripheries, inner peripheries or front faces or back faces of a workpiece.
NM210-00432
Press the [THREAD
] menu key to select this unit.
3-13-1 Setting unit data UNo.
UNIT
∗
THREAD
PART POS-B CHAMF
[1]
[2]
[3]
LEAD
ANG
MULTI
HGT
[4]
[5]
[6]
[7]
[1] PART The following menu will be displayed when the cursor is placed at this item. OUT
IN
FACE
BACK
From the menu, select the section to be machined. Sections to be machined that correspond to the data of the displayed menu are as follows. OUT IN FACE BACK
: : : :
Outer periphery (male thread) Inner periphery (female thread) Right edge of the workpiece (front face) Left edge of the workpiece (back face)
BACK OUT
IN
3-288
FACE
PROGRAM CREATION
3
- For taper threading, select the appropriate machining section as follows according to the desired taper angle:
θ
θ θ
θ
0° < θ ≤ 45°.... OUT
0° < θ ≤ 45° ....OUT
45° < θ ≤ 90° .... BACK
45° < θ ≤ 90°.....FACE
0° < θ ≤ 45° ....IN 45° < θ ≤ 90°.....BACK
0° < θ ≤ 45° ....IN 45° < θ ≤ 90° ....FACE
[2] POS-B From the menu, select an angle for indexing the B-axis. You can specify an angle using numeric keys. See the description of the relevant item for BAR unit. [3] CHAMF Set a chamfering angle for the section you want to thread. - Set 0 if chamfering is not required. - Set 1 for a chamfering angle of 45 degrees. - Set 2 for a chamfering angle of 60 degrees. Designate chamfering to maintain the lead up to the ending point of threading.
With chamfering angle specified
Without chamfering
End point Start point
End point
Chamfering angle
Use the parameter TC82 to specify the chamfering amount.
3-289
Start point
3
PROGRAM CREATION
Note:
For the machine specifications with a threading start position automatic correction option, when the spindle override ratio is updated during the threading process, if no chamfering is required, the thread runout path will change. The thread runout speed will increase for a spindle override ratio up to 100%, or decrease for a spindle override ratio greater than 100%. Thread runout path for 100% Thread runout path for up to 100%
Thread runout path for more than 100%
Workpiece front view
Bottom of the thread Examples of changes in the thread runout path by spindle override ratio updating
[4] LEAD Set the threading lead given by the following expression: (Lead) = (Pitch) × (Number of threads) [5] ANG Set a threading angle. - Usually, set a several degrees smaller value than the nose angle of the tool. ANG = 0
0° < ANG < Tool nose angle
ANG = Tool nose angle
ANG ANG 0°
[6] MULTI Set the desired number of threads. [7] HGT Set the threading height. Pressing the [AUTO SET] menu key with the cursor at item [7] will automatically set data into items [7].
3-290
PROGRAM CREATION
3
3-13-2 Setting tool sequence data SNo.
TOOL
NOM.
No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP !
1
↑ ↑ ↑
!
!
M
M
M
!
↑
↑
↑
↑
↑
↑
↑
↑ ↑ ↑
[1]
[2] [3] [4] [5] [6] [7]
[8]
[9]
[10]
[11]
[12] [12] [12]
Remark 1:
!:
↑
FR
Data are not necessary to be set here.
Remark 2: In the tool sequence, one tool is automatically developed as follows. Machining
Pattern
1
One tool for machining is selected.
[1] TOOL (Name) The name of the tool to be used for machining is set automatically. When the cursor is present at this item, the following menu is displayed to allow the tool to be changed: GENERAL
GROOVE
THREAD
T.DRILL
T.TAP
SIMUL DRILL ROTATION
SPECIAL
[2] TOOL (Section to be machined) When the cursor is present at this item, the appropriate menu according to the tool name that was selected at item [1] TOOL (Name) is displayed as shown below. - If either GENERAL, GROOVE, or THREAD has been selected OUT IN OUTER INNER DIAMETER DIAMETER
EDG EDGE
IN INNER (BAK)
EDG EDGE (BAK)
- If either T-DRILL, or T-TAP has been selected EDG EDGE
EDG EDGE (BAK)
- If SPECIAL has been selected 0001
0002
0003
0004
0005
0006
0007
0008
0009
When creating a threading unit, usually select tools as follows according to the machining section that has been selected for the unit: PART in the unit (Section to be machined)
TOOL (Name)
OUT IN FACE BACK
Note:
TOOL (Section to be machined) OUT OUTER DIAMETER IN INNER DIAMETER, IN INNER (BAK)
THREAD
OUT OUTER DIAMETER, EDG EDGE, EDG EDGE (BAK) OUT OUTER DIAMETER, EDG EDGE (BAK)
The above example applies when the tools best suited to a general machining shape pattern are to be used. Tools other than those shown in the above example may be suitable for the shape actually specified.
3-291
3
PROGRAM CREATION
[3] NOM. (Nominal size) Enter the nominal size of tools using the numeric keys. See the description of the relevant item for BAR unit. [4] NOM. (Suffix) A code should be selected out of the menu to identify those tools which are of identical type (having an identical name) and have an identical nominal size. A
B
C
D
E
F
G
H
HEAVY TOOL
>>>
[5] NOM. (Turret selection) For a machine equipped with upper and lower turrets, select the turret in which the tool to be used is mounted. The following menu will be displayed. See the description of the relevant item for BAR unit. SET UPPER TURRET
SET LOWER TURRET
[6] No. (Priority No.) Assign priority levels in the order of machining. See the description of the relevant item for BAR unit. [7] # (Retraction position of the lower turret) For a machine equipped with upper and lower turrets, specify the position to which the lower turret is to be retracted when machining workpieces using only the upper turret. The following menu will be displayed: LOWER TURRET POS.1
Note:
LOWER TURRET POS.2
See Chapter 5, “LOWER-TURRET CONTROL FUNCTIONS”, for details of items [5] and [7].
[7] PAT. (Machining pattern) The following menu will be displayed when the cursor is placed at this item: #0
#1
STANDARD CONST. DEPTH
(a)
#2
#0
#1
CONST. STANDARD CONST. AREA DEPTH
#2
CONST. AREA
(b)
From the menu, select the threading pattern to be machined.
3-292
PROGRAM CREATION
3
Patterns to be machined that correspond to the data of the displayed menu are as follows. #0,
#0 ：Standard patterns The threading amount gradually decreases as the number of passes increases.
Threading amount d1
d1/4 a 1 #1,
#1 ：Constant-threading pattern The threading amount always stays constant, irrespective of the number of passes.
n/2
#2 ：The threading amount is inversely proportional to the number of passes.
n: d1: a: di:
n
Number of passes
d1
Threading amount d1
Number of passes The first threading amount The n-th threading amount The i-th threading amount
di × i =（constant）
di 1
Note:
Number of passes
Threading amount
1 #2,
n
i
n
Number of passes T4P077
If you select #0 , #1 or #2 zigzag threading (alternate threading with the left and right cutting edges) will occur unless you set a value of 30 or less in item [5], ANG in the unit data.
Tool
2 1 4
3 5
1 to 5: Threading order
[9] DEP-1 (First cutting depth) Enter the first cutting depth during the threading pass. For X-axial cutting, enter this value in terms of radius. The above value can likewise be auto-set by pressing the [AUTO SET] menu key. [10] DEP-2/NUM. (Number of cutting passes) Enter the number of cutting passes (how often the threading pass is to be repeated). Note:
Specify at least three cutting passes.
3-293
3
PROGRAM CREATION
[11] C-SP Specify the surface speed for the tool in terms of turning spindle. See the description of the relevant item for BAR unit. [12] M Specify the M-code to be issued for the tool immediately after it is selected. See the description of the relevant item for BAR unit.
3-13-3 Setting sequence data FIG
SPT-X
SPT-Z
FPT-X
FPT-Z
1
[1]
[2]
[3]
[4]
[1] SPT-X, [2] SPT-Z, [3] FPT-X, [4] FPT-Z Set the coordinates of the machining start point and end point.
Start point
End point
End point
Start point
Start point
Start point
End point
End point
T4P081
- For usual threading, set the nominal diameter of the thread as the X-coordinate. - Incompletely threaded portions occur near the end point of threading. Therefore, if grooves are present at the position of the end point as shown in the diagrams above, set the end point at a position slightly deeper than the section to be threaded. - Even if the spindle override value is changed using the threading start position automatic correction option, the acceleration distance for threading will be the distance existing when the spindle override value is 100%. Since the use of a spindle override value exceeding 100% may result in an incomplete thread due to the insufficiency of the acceleration distance, specify a spindle override value not exceeding 100%. However, do not set the override value to 0%. Otherwise, operation will stop during threading.
3-294
PROGRAM CREATION
3
Note 1: The continuous threading pattern shown in the diagram below can be generated by setting multiple lines of sequence data. In that case, the coordinates of the second and subsequent start points do not need be set (items [1] and [2] will be marked with !).
End point 2
Start point
End point 1 φ20
φ12
15 35 T4P082
FIG
SPT-X
SPT-Z
FPT-X
FPT-Z
1
12.
0.
12.
15.
2
!
!
20.
35.
Note 2: Threading action begins at a position that is away from the start point specified in the program by the acceleration distance. Before carrying out a threading operation, therefore, check for possible interference with the tailstock or the workpiece during threading.
SPT
FPT
Machining start point Threading acceleration distance
Note 3: The actuation of feed-hold function during a pass of threading will not interrupt the machine operation until the chamfering at the end point of threading has been completed.
3-295
3
PROGRAM CREATION
Note 4: For the machine specifications with a threading start position automatic correction option, percentage (%) display can be changed by pressing the spindle/milling spindle override key during the threading process. The spindle speed, however, does not change. The specified percentage value is incorporated into the actual spindle speed, only after the threading block. For continuous threading, the specified value is incorporated after the continuous threading process. The spindle override ratio update is valid from this position. G00 G00
G00 G32 End point on the program
Start point of machining Start point on the program
Change of the spindle override ratio during threading
Note 5: Threading start position automatic correction and re-threading functions (both optional) are only valid for a longitudinal threading by cutting feed on the Z-axis: THREAD OUT or IN. (Invalid for THREAD FACE and BACK) Note 6: Re-threading function (optional) is only valid for constant lead threading.
3-296
PROGRAM CREATION
3
3-14 Grooving Unit (T. GROOVE) Select the grooving unit to groove the outer peripheries, inner peripheries, front faces or back faces or to cut off workpiece.
NM210-00433
Press the [T. GROOVE
] menu key to select this unit.
3-14-1 Setting unit data UNo.
UNIT
PART
POS-B
PAT.
No.
PITCH
∗
T.GROOVE
[1]
[2]
[3]
[4]
[5]
WIDTH FINISH
[6]
[7]
[1] PART The following menu will be displayed when the cursor is placed at this item. OUT
IN
FACE
BACK
From the menu, select the section to be machined. Sections to be machined that correspond to the data of the displayed menu are as follows. OUT IN FACE BACK
: : : :
Outer periphery Inner periphery Right edge of the workpiece (front face) Left edge of the workpiece (back face)
T4P089
3-297
3
PROGRAM CREATION
[2] POS-B From the menu, select an angle for indexing the B-axis. You can specify an angle using numeric keys. See the description of the relevant item for BAR unit. [3] PAT. The following menu will be displayed when the cursor is placed at this item. #0
#1
#2
#3
#4
#5
Select a grooving pattern from the menu. The data of the displayed menu denote the following grooving patterns: #0 : Right-angled grooves or oblique grooves
#1 : Isosceles trapezoidal grooves
#4 : Right-corner cut-off grooves
#2 : Right-tapered grooves #5 : Left-corner cut-off grooves
#3 : Left-tapered grooves
T4P090
Note 1: Grooving patterns #4 and #5 (both, cutting-off) are available only when outside diameter (OUT) is selected for item [1] PART. Note 2: For grooving patterns #4 and #5, the feed reduction count can be changed using parameter TC50. [4] No. Set the number of grooves when multiple grooves of the same shape are to be machined at fixed spacings.
3-298
PROGRAM CREATION
3
[5] PITCH Set a pitch when multiple grooves of the same shape are to be made at fixed spacings. The pitch can be set as either a plus value or a minus value. Setting the pitch as a plus value causes sequential grooving in a forward direction. Setting the pitch with a minus sign causes sequential grooving in a reverse direction. 15 Start point End point
2
No. = 2 PITCH = 15 or –15
1
–15
1 , 1
2
: Grooving order
2 T4P092
[6] WIDTH Set a grooving width.
WIDTH
WIDTH
WIDTH
WIDTH
T4P093
- If you have selected grooving pattern #4 or #5, a cutting-off tool tip width is considered as a grooving width.
3-299
3
PROGRAM CREATION
[7] FINISH - No data can be set if you have selected grooving pattern #0. - Set a finish-machining removal allowance if you have selected grooving pattern #1, #2 or #3.
F
F
Section to be finish-machined
F
Note:
F
F
F F: FINISH T4P094
No finishing allowance will be provided to right-angled walls if you have selected grooving pattern #2 or #3.
- Set a cutting-off tool overshoot if you have selected grooving pattern #4 or #5.
Cutting-off tool
Cutting-off tool
End point
End point F
F F: FINISH T4P095
3-14-2 Setting tool sequence data SNo.
TOOL
NOM.
No.
#
PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP FR M
R1
!
!
!
F2
!
!
!
↑ ↑ ↑
!
↑
↑
!
↑
↑
↑
↑
↑
↑
[1]
[2] [3] [4] [5] [6]
[7]
[8]
[9]
[10]
!:
M
!
↑
Remark 1:
M
↑
↑
[11] [12] [12] [12]
Data are not necessary to be set here.
Remark 2: In the tool sequence, a maximum up to two tools are automatically developed as follows. Machining
Pattern
R1 (Roughing)
Grooving patterns #1 to #3: One tool for roughing is automatically selected.
F2 (Finishing)
One tool for machining is automatically selected.
Remark 3: For grooving patterns #1 to #3, DEP-1 in the finishing tool sequence is displayed with a ! mark to indicate that a data cannot be set here. Remark 4: For grooving patterns #0, #4, and #5, FIN-X is displayed with a ! mark to indicate that a data cannot be be set here.
3-300
PROGRAM CREATION
3
[1] TOOL (Name) The name of the tool to be used for machining is set automatically. When the cursor is present at this item, the following menu is displayed to allow the tool to be changed: GENERAL
GROOVE
THREAD
T.DRILL
T.TAP
SIMUL DRILL ROTATION
SPECIAL
[2] TOOL (Section to be machined) When the cursor is present at this item, the appropriate menu according to the tool name that was selected at item [1] TOOL (Name) is displayed as shown below. - If either GENERAL, GROOVE, or THREAD has been selected OUT IN OUTER INNER DIAMETER DIAMETER
EDG EDGE
IN INNER (BAK)
EDG EDGE (BAK)
- If either T-DRILL, or T-TAP has been selected EDG EDGE
EDG EDGE (BAK)
- If SPECIAL has been selected 0001
0002
0003
0004
0005
0006
0007
0008
0009
When creating a grooving unit, usually select tools as follows according to the machining section that has been selected for the unit: PART in the unit (Section to be machined)
TOOL (Name)
TOOL (Section to be machined)
OUT
OUT OUTER DIAMETER IN INNER DIAMETER, IN INNER (BAK)
IN
GROOVE
FACE
OUT OUTER DIAMETER, EDG EDGE, EDG EDGE (BAK) OUT OUTER DIAMETER, EDG EDGE (BAK)
BACK
Note:
The above example applies when the tools best suited to a general machining shape pattern are to be used. Tools other than those shown in the above example may be suitable for the shape actually specified.
[3] NOM. (Nominal size) Enter the nominal size of tools using the numeric keys. See the description of the relevant item for BAR unit. [4] NOM. (Suffix) A code should be selected out of the menu to identify those tools which are of identical type (having an identical name) and have an identical nominal size. A
B
C
D
E
3-301
F
G
H
HEAVY TOOL
>>>
3
PROGRAM CREATION
[5] NOM. (Turret selection) For a machine equipped with upper and lower turrets, select the turret in which the tool to be used is mounted. The following menu will be displayed. See the description of the relevant item for BAR unit. SET UPPER TURRET
SET LOWER TURRET
[6] No. (Priority No.) Assign priority levels in the order of machining. See the description of the relevant item for BAR unit. [7] # (Simultaneous machining No. or retraction position of the lower turret) For a machine equipped with upper and lower turrets, to use the tools mounted in both turrets, specify the simultaneous machining number. It is also possible to specify the position to which the lower turret is to be retracted when machining workpieces using only the upper turret. The following menu will be displayed: LOWER TURRET POS.1
Note:
LOWER TURRET POS.2
See Chapter 5, “LOWER-TURRET CONTROL FUNCTIONS”, for details of items [5] and [7].
[8] DEP-1 (Max. depth of cut), [9] C-SP, [10] FR For each grooving pattern, set data into these items as follows: Pattern
Sequence
#0
F (Finishing)
#1, #2 or #3
R (Roughing) F (Finishing)
#4 or #5 (Parameter TC50 = 0, 1)
F (Finishing)
#4 or #5 (Parameter TC50 ≥ 2)
F (Finishing)
DEP-1 (Max. depth of cut)
Max. depth of cut per pass (Designate in radius for OUT or IN)
—
Max. depth of cut per pass (Designate in radius; without pecking if 0 is set)
C-SP
FR
Surface speed during grooving
Feedrate during grooving (Shape seq. data RGH ineffective)
Surface speed during roughing
Feedrate during roughing
Surface speed during finishing
Feedrate during finishing
Surface speed during grooving (limited by the rotational speed specified by the parameter TC49)
Feedrate during grooving (Shape seq. data RGH effective for cutting-off area specified by the parameter TC9)
Number of revolutions during grooving (*)
Starting feedrate for grooving (**)
The monitor will display “S500” if “500” is entered in an attempt to set a number of revolutions of 500 min–1. The section from the starting point of machining before the cutting-off area (specified by the parameter TC9) is machined at the rotational speed designated here. In the cutting-off area the machining is performed at the rotational speed set by the parameter TC49. ** The feedrate is reduced in several steps (set by the parameter TC50) to the value of shape sequence data RGH.
*
3-302
PROGRAM CREATION
3
During grooving, pecking is repeated with each cutting operation in the direction of the groove depth. Use parameter TC74 to specify the returning stroke of pecking. If TC74 = 0, pecking will not occur and the machine will come to a dwelling stop while the spindle rotates the number of revolutions specified in parameter TC69.
D Dwelling for the fixed number of revolutions (TC69)
P D P D P
D: Depth per cutting operation P: Pecking return stroke (TC74)
D
D740PA158
Note:
Setting pecking return stroke parameter TC74 to zero allows the machining time required to be reduced since pecking is not conducted. However, vibration and/or unusual operating sounds may occur under specific cutting conditions. If this is the case, machine the workpiece in normal pecking mode.
[11] FIN-X Specify the allowance to be left for the next finishing tool sequence. See the description of the relevant items for BAR unit. [12] M Specify the M-code to be issued for the tool immediately after its ATC (automatic tool change). See the description of the relevant item for BAR unit.
3-303
3
PROGRAM CREATION
3-14-3 Setting shape sequence data FIG
S-CNR
SPT-X
SPT-Z
FPT-X
FPT-Z
F-CNR
ANG
RGH
1
[1]
[2]
[3]
[4]
[5]
[6]
[7]
[8]
[1] S-CNR Set the chamfering amount if C-chamfering is required. For R-chamfering, set a rounding radius after pressing the [CORNER R] menu key. - If you have selected grooving pattern #0, the data specified here will become invalid. - If you have selected a grooving pattern other than #0, set data in this item when C-chamfering or R-chamfering (rounding) is to be done on the corners shown in the diagrams below.
S-CNR
S-CNR
F-CNR
F-CNR
S-CNR
F-CNR
S-CNR
S-CNR
T4P096
3-304
PROGRAM CREATION
3
[2] SPT-X, [3] SPT-Z, [4] FPT-X, [5] FPT-Z Set the coordinates of the start point and end point of grooving. Set the position of the start point and the end point as follows according to the selected grooving pattern. - For grooving pattern #0: Start point
End point
End point Start point
Start point End point Start point
Start point
End point
End point Start point
Start point
Start point
End point
For pattern #0, oblique grooves can be machined by setting the start and end points as shown above. - For grooving pattern #1
Start point
End point
Start point
End point
Start point
End point
3-305
Start point End point
3
PROGRAM CREATION
- For grooving pattern #2:
Start point
End point
Start point
End point
Start point
End point
Start point End point
- For grooving pattern #3:
Start point
End point End point
End point Start point
Start point
End point Start point
- For grooving pattern #4 or #5:
#4
#5
Start point
Start point
End point
End point
Note 1: For grooving pattern #0, #1, #2 or #3, the machining drawing may have an indicated taper angle but not have a clearly indicated position for the start point or the end point. In such cases, temporarily set the question mark ? in all unclear items by pressing the [ ? ] menu key. You will be able to set data automatically at a later time using the automatic calculation function of the crossing-point. See “Automatic Crossing-Point Calculation Function” for further details.
3-306
PROGRAM CREATION
3
Note 2: If multiple grooves of the same shape are to be machined (according to the setting of unit data No.), set the coordinates of the start point and end point of grooving of the first groove. Note 3: If grooving pattern #4 or #5 is selected, no data setting is required for FPT-Z. [6] F-CNR The data for the ending corner is only effective for patterns #1, #2, and #3. See the description and the diagram for item [1], S-CNR, for further details. [7] ANG Set a taper angle if you have set the question mark “?” in one of the four items from [2] to [5] above. See “Function of automatically calculating a point of intersection” for details of setting a taper angle. [8] RGH For each grooving pattern, set data into this item as follows: Pattern #0
Description of RGH data Invalid. (Set the feedrate in item FR of sequence data.)
#1, #2, #3
Set the feedrate during finishing. (Finishing will also be executed at the FR feed rate of tool sequence data if no data is designated here.)
#4 and #5
Set the feedrate for the cutting-off area. (Cutting-off will be executed at the half of the FR feed rate of tool sequence data if no data is designated here.)
3-307
3
PROGRAM CREATION
3-15 Turning Drilling Unit (T. DRILL) Select the turning drilling unit when preholes are to be drilled in the middle of a workpiece using a turning drill.
NM210-00434
Press the [T. DRILL
] menu key to select this unit.
3-15-1 Setting unit data UNo.
UNIT
PART
POS-B
DIA
∗
T.DRILL
[1]
[2]
[3]
[1] PART The following menu will be displayed when the cursor is placed at this item. FACE
BACK
From the menu, select the section to be machined. Sections to be machined that correspond to each menu item are as follows: FACE : Right edge of the workpiece BACK : Left edge of the workpiece Note:
PART may not be specified for special machine specifications.
[2] POS-B From the menu, select an angle for indexing the B-axis. You can specify an angle using numeric keys. See the description of the relevant item for BAR unit. [3] DIA Set the diameter of the hole to be drilled (nominal diameter of the turning drill).
3-308
PROGRAM CREATION
3
3-15-2 Setting tool sequence data SNo.
TOOL
NOM.
No.
#
↑ ↑ ↑
PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z !
1
C-SP FR
↑
↑
↑
↑
↑
↑
↑
↑
[1]
[2] [3] [4] [5] [6]
[7]
[8]
[9]
[10]
[11]
[12]
!:
M
M
!
↑
Remark 1:
M
↑
↑ ↑ ↑
[13] [14] [14] [14]
Data are not necessary to be set here.
Remark 2: In the tool sequence, one tool is automatically developed as follows. Machining
Pattern
1
One tool for machining is automatically selected.
Remark 3: When [SIMUL DRILL ROTATION] is selected for item [1] TOOL (Name), the following tool sequence is displayed: SNo.
TOOL
NOM.
No.
↑ ↑ ↑
#
PAT. DEP-1 DEP-2/NUM. DEP-3 RPM SPDL ROT. C-SP FR
M
M
M
1
↑
↑
↑
↑
↑
↑
↑
↑
↑
↑
↑
[1]
[2] [3] [4] [5] [6]
[7]
[8]
[9]
[10]
[11]
[15]
[16]
[17]
↑
↑ ↑ ↑
[18] [14] [14] [14]
[1] TOOL (Name) The name of the tool to be used for machining is set automatically. When the cursor is present at this item, the following menu is displayed to allow the tool to be changed: GENERAL
GROOVE
THREAD
T.DRILL
T.TAP
SIMUL DRILL ROTATION
SPECIAL
[2] TOOL (Section to be machined) When the cursor is present at this item, the appropriate menu according to the tool name that was selected at item “[1] TOOL (Name)” is displayed as shown below. - If either GENERAL, GROOVE, or THREAD has been selected OUT IN OUTER INNER DIAMETER DIAMETER
EDG EDGE
IN INNER (BAK)
EDG EDGE (BAK)
- If either T-DRILL, or T-TAP has been selected EDG EDGE
EDG EDGE (BAK)
- If SPECIAL has been selected 0001
0002
0003
0004
0005
0006
0007
0008
0009
When creating a turning drilling unit, usually select tools as follows according to the machining section that has been selected for the unit: PART in the unit (Section to be machined) FACE BACK
TOOL (Name)
T. DRILL
TOOL (Section to be machined) EDG EDGE EDG EDGE (BAK)
3-309
3
PROGRAM CREATION
Note:
The above example applies when the tools best suited to a general machining shape pattern are to be used. Tools other than those shown in the above example may be suitable for the shape actually specified.
[3] NOM. (Nominal diameter) Set the diameter of the hole to be drilled (nominal diameter of the turning drill or milling drill). [4] NOM. (Suffix) A code should be selected out of the menu to identify those tools which are of identical type (having an identical name) and have an identical nominal diameter. A
B
C
D
E
F
G
H
HEAVY TOOL
>>>
[5] NOM. (Turret selection) For a machine equipped with upper and lower turrets, select the turret in which the tool to be used is mounted. The following menu will be displayed. See the description of the relevant item for BAR unit. SET UPPER TURRET
SET LOWER TURRET
[6] No. (Priority No.) Assign priority levels in the order of machining. See the description of the relevant item for BAR unit. [7] # (Retraction position of the lower turret) For a machine equipped with upper and lower turrets, specify the position to which the lower turret is to be retracted when machining workpieces using only the upper turret. The following menu will be displayed: LOWER TURRET POS.1
Note:
LOWER TURRET POS.2
See Chapter 5, “LOWER-TURRET CONTROL FUNCTIONS”, for details of items [5] and [7].
[8] PAT. (Machining pattern) The following menu will be displayed when the cursor is placed at this item. #0
#1
#2
#3
#4
>>>
DRILLING PECKING PECKING REAMER PECKING BOTTOMED BOTTOMED BOTTOMED BOTTOMED BOTTOMED
#0
#1
#2
#3
#4
DRILLING PECKING PECKING REAMER PECKING THROUGH THROUGH THROUGH THROUGH THROUGH
From the menu, select the turning drilling pattern.
3-310
>>>
PROGRAM CREATION
3
The data of the displayed menu represent following drill patterns. #0,
#0
: Conventional type of drilling cycle The drill returns to the drilling start point at a cutting feedrate after each infeed operation has been completed. Start point
Cutting feed Rapid feed
Drilling end point
Drilling start point TC39
T4P114
#1,
#1
: Deep-hole drilling cycle The drill returns to the drilling start point at a rapid feedrate after each infeed operation has been completed. Start point Cutting feed Rapid feed
Drilling end point
Drilling start point TC47
#2,
#2
TC47
TC39
T4P115
: High-speed deep-hole drilling cycle The drill returns through the specified distance (data specified in parameter TC47) at a cutting feedrate after each infeed operation has been completed. Start point Cutting feed Rapid feed
Drilling end point
Drilling start point TC47
TC47
TC39
T4P116
3-311
3
PROGRAM CREATION
#3,
#3
: Reaming cycle Drilled holes are finished with a reamer. Start point
Cutting feed Rapid feed
Machining end point
Machining end point TC39
T4P117 #4,
#4
: Very-deep-hole drilling cycle Each time the normal pecking has been executed the parameter-designated number of times, the tool returns at a rapid feedrate to a position near the drilling start point. Start point L= L
D + D 10 2 × tan θ 2
D : Drill diameter θ : Cutting-edge angle
Drilling start point Drilling end point
Cutting feed TC47
TC47
TC47
TC47
TC39
Rapid feed T4P118
Note 1: Select either #0, #1, #2, #3 or #4 to drill stop-holes. Select either #0, #1, #2, #3 or #4 to drill through-holes. Note 2: For patterns #0 to #4, the tool dwells at the bottom of the hole while the spindle rotates in accordance with the parameter-designated value. For patterns #4 and #4 the tool dwells for the same while after it has returned to a position near the drilling start point. Note 3: With patterns #4 and #4, the rapid feedrate during the cycle can be reduced to the value designated in parameter D52.
3-312
PROGRAM CREATION
3
[9] DEP-1, [10] DEP-2/NUM., [11] DEP-3 You can automatically set data in these items. When machining pattern other than #3 or #3 is selected. Pressing the [AUTO SET] menu key with the cursor at item [8] and setting a tool will automatically set the data that has been calculated by the NC unit into items [9] through [11]. When machining pattern #3 or #3 is selected. Items [9] through [11] will be marked with !. (Data cannot be set.) Any desired data can be set in these items, and automatically set data can be changed. The data items denote the following data: DEP-1 : DEP-2/NUM. : DEP-3 :
First infeed depth Infeed decrement Minimum infeed amount Machining start point
Machining end point D4
D3
D2
D1 D1 – D2 = D2 – D3 = D3 – D4 = α Dn : n-th infeed depth (n = 1 to 4) α : Infeed decrement T4P118
Taking the infeed decrement as α, one can calculate the n-th infeed amount, Dn (n ≥ 2), as follows: Dn = Dn–1 – α = D1 – α (n – 1) However, if Dn–1 – α ≤ Dmin (Dmin: minimum infeed amount), then Dn (= Dn+1 = Dn+2 = '''') = Dmin [12] C-SP Specify the surface speed for the turning spindle. See the description of the relevant item for BAR unit. [13] FR Enter the desired feedrate of the tool in terms of turning spindle speed per revolution. See the description of the relevant item for BAR unit. [14] M Specify the M-code to be issued for the tool immediately after it is selected. See the description of the relevant item for BAR unit. [15] RPM If [SIMUL DRILL ROTATION] is selected for item [1] TOOL (name), specify the number of revolutions of the turning spindle. Note:
The number of revolutions of the drilling tool (milling spindle) is calculated from the relative number of revolutions calculated from the surface speed specified in item [17] and the number of revolutions of the turning spindle.
3-313
3
PROGRAM CREATION
[16] SPDL ROT. If [SIMUL DRILL ROTATION] is selected for item [1] TOOL (name), specify the rotational direction of the turning spindle. The following menu is displayed. FWD
REV
To rotate the spindle in the forward direction, select [FWD]. To rotate the spindle in the reverse direction, select [REV]. Note:
The drilling tool (milling spindle) rotates in the forward (clockwise) direction, as with the drill used for point machining.
[17] C-SP If [SIMUL DRILL ROTATION] is selected for item [1] TOOL (name), specify the relative surface speeds of the turning spindle and milling spindle. The relative number of revolutions of the turning spindle and that of the milling spindle are calculated from their relative surface speeds. [18] FR If [SIMUL DRILL ROTATION] is selected for item [1] TOOL (name), specify the feedrate of the milling/drilling tool by entering the rate at which the tool is fed each time the turning spindle and the milling spindle make one revolution relative to each other.
3-314
PROGRAM CREATION
3
3-15-3 Setting shape sequence data FIG
SPT-Z
FPT-Z
1
[1]
[2]
[1] SPT-Z, [2] FPT-Z Set the coordinates of the start point and end point of the intended drilling pattern. - The start point and end point for drilling stop-holes, for example, are positioned as shown below. 70
T. DRLL BACK
T. DRLL FACE 40
5
30
Program origin
End point
SPT-Z -5.
Start point
End point
Start point
FPT-Z 40.
SPT-Z 70.
Program origin
FPT-Z 30.
T4P119
- The position of the end point differs from stop-hole to through-hole as follows: For through-hole
For stop-hole
Start point
Drilling end point Programmed end point
End point
L The drilling feed will be stopped when the tool tip has reached the programmed end point.
Program the through-hole depth as the end point. Automatic drilling will then be performed up to the position (of tool tip) deeper than the programmed end point by the distance L given by the following expression: L=
L=
D D + 10 2 × tan θ 2
(0 < θ < 180°)
D 10
(θ = 180°) D : Tool diameter θ : Cutting-edge
3-315
Start point
3
PROGRAM CREATION
3-16 Turning Tapping Unit (T. TAP) Select the turning tapping unit when holes in the middle of a workpiece are to be tapped using a turning tap.
NM210-00435
Press the [T. TAP
] menu key to select this unit.
3-16-1 Setting unit data UNo.
UNIT
PART
POS-B
NOM-DIA
PITCH
∗
T.TAP
[1]
[2]
[3]
[4]
[1] PART The following menu will be displayed when the cursor is placed at this item. FACE
BACK
From the menu, select the section to be machined. Sections to be machined that correspond to each menu item are as follows: FACE : Right edge of the workpiece BACK : Left edge of the workpiece Note:
The [BACK] menu item may not be selectable for special machine specifications.
[2] POS-B From the menu, select an angle for indexing the B-axis. You can specify an angle using numeric keys. See the description of the relevant item for BAR unit. [3] NOM-DIA The following menu will be displayed when the cursor is placed at this item. METRIC
UNFY
PIPE
PIPE
PIPE
OTHER
THRD(M) THRD(UN) THRD(PT) THRD(PF) THRD(PS)
(a)
(b)
(c)
(d)
(e)
(f)
From (a) through (f) above, select the type of threads to be tapped. Then, set the nominal diameter of the threads.
3-316
PROGRAM CREATION
3
The data of the displayed menu denote the following types of threads: (a)
METRIC THRD(M)
: Metric threads
(b)
UNFY THRD(UN)
: Unified threads
(c)
PIPE THRD(PT)
: Tapered pipe threads (PT)
(d)
PIPE THRD(PF)
: Parallel pipe threads (PF)
(e)
PIPE THRD(PS)
: Tapered pipe threads (PS)
(f)
OTHER
: Other thread types
- If you select metric threads, the message NOMINAL SIZE OF TAP? will be displayed. In that case, set the nominal diameter of the threads to be tapped. Example: To tap M8 metric threads: Press the keys
METRIC THRD(M)
8 , and
,
INPUT
in this order.
- If you select unified thread types, the message TAP NOMINAL SIZE ? will be displayed and then the menu will change over to: No.
H(1/2)
Q(1/4)
HALF
QUARTER
E(1/8)
S(1/16)
NOM-φ SELECT
EIGHTH SIXTENTH
Using the menu, set the nominal diameter of the threads to be tapped. Example 1: To tap unified thread of the 3/4-16UN size: Press the keys
UNFY THRD(UN)
,
Q(1/4) QUARTER
, 3 , – , 1 , 6 , and
INPUT
in this order.
Example 2: To tap unified thread of the 1-1/8-7UN size: Press the keys
UNFY THRD(UN)
,
E(1/8) EIGHTH
, 9 , – , 7 , and
INPUT
in this order.
Example 3: To tap unified thread of the No. 1-16UN size: Press the keys
UNFY THRD(UN)
,
No.
,
1 , – , 1 , 6 , and
INPUT
in this order.
- Also, a press of the [NOM-φ SELECT] menu key displays the following nominal tap diameter window to allow the desired nominal thread diameter to be entered by selecting it using the cursor keys. UNIFY THREAD
3-317
3
PROGRAM CREATION
- If you select pipe thread types, the message TAP NOMINAL SIZE ? will be displayed and then the menu will change over to: H(1/2) HALF
Q(1/4) QUARTER
E(1/8) S(1/16) EIGHTH SIXTENTH
NOM-φ SELECT
Using the menu, set the nominal diameter of the threads to be tapped. Example 1:
To tap pipe thread of the PT3/8 size: Press the keys
Example 2:
,
E(1/8) EIGHTH
,
3 , and
INPUT
in this order.
,
1 , and
INPUT
in this order.
,
1 , and
INPUT
in this order.
To tap pipe thread of the PF1/4 size: Press the keys
Example 3:
PIPE THRD(PT)
PIPE THRD(PF)
,
Q(1/4) QUARTER
To tap pipe thread of the PS1/8 size: Press the keys
PIPE THRD(PS)
,
E(1/8) EIGHTH
- Also, a press of the [NOM-φ SELECT] menu key displays the following nominal tap diameter window to allow the desired nominal thread diameter to be entered by selecting it using the cursor keys. [Tapered pipe thread (PT)]
[Tapered pipe thread (PF)]
[Tapered pipe thread (PS)]
PIPE THREAD PT
PIPE THREAD PF
PIPE THREAD PS
[4] PITCH Set the pitch of the threads to be tapped (pitch of turning tapping tool to be used). When the appropriate nominal tool diameter is entered in item [3] NOM-DIA, data will be auto-set, except for special threads. Any data, however, can also be entered instead.
3-318
PROGRAM CREATION
3
3-16-2 Setting tool sequence data SNo.
TOOL
NOM.
No.
#
↑ ↑ ↑
PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP !
1
!
!
!
!
!
FR
M
M
M
!
↑
↑
↑
↑
↑
↑ ↑ ↑
[1]
[2] [3] [4] [5] [6]
[7]
[8]
[9] [9] [9]
Remark 1:
!:
Data are not necessary to be set here.
Remark 2: In the tool sequence, one tool is automatically developed as follows. Machining
Pattern
1
One tool for machining is automatically selected.
[1] TOOL (Name) The name of the tool to be used for machining is set automatically. When the cursor is present at this item, the following menu is displayed to allow the tool to be changed: GENERAL
GROOVE
THREAD
T.DRILL
T.TAP
SIMUL DRILL ROTATION
SPECIAL
[2] TOOL (Section to be machined) When the cursor is present at this item, the appropriate menu according to the tool name that was selected at item [1] TOOL (Name) is displayed as shown below. - If either GENERAL, GROOVE, or THREAD has been selected OUT IN OUTER INNER DIAMETER DIAMETER
EDG EDGE
IN INNER (BAK)
EDG EDGE (BAK)
- If either T-DRILL, or T-TAP has been selected EDG EDGE
EDG EDGE (BAK)
- If SPECIAL has been selected 0001
0002
0003
0004
0005
0006
0007
0008
0009
When creating a turning-tapping unit, usually select tools as follows according to the machining section that has been selected for the unit: PART in the unit (Section to be machined)
TOOL (Name)
FACE BACK
Note:
T. TAP
TOOL (Section to be machined) EDG EDGE EDG EDGE (BAK)
The above example applies when the tools best suited to a general machining shape pattern are to be used. Tools other than those shown in the above example may be suitable for the shape actually specified.
[3] NOM. (Nominal diameter) Set the diameter of the hole to be tapped (nominal diameter of the turning tap). See the description of [3] NOM-DIA in the unit.
3-319
3
PROGRAM CREATION
[4] NOM. (Suffix) A code should be selected out of the menu to identify those tools which are of identical type (having an identical name) and have an identical nominal size. A
B
C
D
E
F
G
H
HEAVY TOOL
>>>
[5] NOM. (Turret selection) For a machine equipped with upper and lower turrets, select the turret in which the tool to be used is mounted. The following menu will be displayed See the description of the relevant item for BAR unit. SET UPPER TURRET
SET LOWER TURRET
[6] No. (Priority No.) Assign priority levels in the order of machining. See the description of the relevant item for BAR unit. [7] # (Retraction position of the lower turret) For a machine equipped with upper and lower turrets, specify the position to which the lower turret is to be retracted when machining workpieces using only the upper turret. The following menu will be displayed: LOWER TURRET POS.1
Note:
LOWER TURRET POS.2
See Chapter 5, “LOWER-TURRET CONTROL FUNCTIONS”, for details of items [5] and [7].
[8] C-SP Specify the surface speed for the turning spindle. See the description of the relevant item for BAR unit. [9] M Specify the M-code to be issued for the tool immediately after it is selected. See the description of the relevant item for BAR unit.
3-320
PROGRAM CREATION
3-16-3 Setting shape sequence data FIG
SPT-Z
FPT-Z
1
[1]
[2]
[1] SPT-Z, [2] FPT-Z Set the coordinates of the start point and end point of the thread shape. T. TAP FACE
T. TAP BACK
90
40
50 Complete thread section
Complete thread section End point
End point Start point
SPT-Z 0.
Start point
FPT-Z 40.
SPT-Z 90.
3-321
FPT-Z 50.
3
3
PROGRAM CREATION
3-17 Mill-Turning Unit (MILLTURN) Select the mill-turning unit to lathe the outer peripheries of round-bar-materials using milling tools.
D740PA162
Press the [MILLTURN
] menu key to select this unit.
3-17-1 Setting unit data UNo.
UNIT
POS-B
CPT-X
CPT-Z
FIN-X
FIN-Z
SHIFT-Y
∗
MILLTURN
[1]
[2]
[3]
[4]
[5]
[6]
[1] POS-B Select an angle at which the B-axis is to be indexed. The desired angle can likewise be set up using the numeric keys. See the description of the relevant item for BAR unit. Note:
If an angle other than 90 degrees is set up as POS-B, interference with the workpiece may occur at specific inclination angles of the tool. The workpiece may also be machined too much or partly remain unmachined. Modify the program in such cases.
[2] CPT-X, [3] CPT-Z, [4] FIN-X, [5] FIN-Z Set the X- and Z-coordinates of the desired infeed point. After that, set the allowances to be left for the X-axis and Z-axis directions.
[2] [3] CPT-X, Z
[5] FIN-Z
[4] FIN-X ×
1 2
D740PA163
3-322
PROGRAM CREATION
3
[6] SHIFT-Y Set the Y-axial shifting distance. X [6] SHIFT-Y
Y
D740PA164
When SHIFT-Y is set, the tool path will be as follows: SHIFT-Y
Z-DEC
DEP-1
A shift-Y reference angle is determined at the point where the tool nose of the milling tool which has been moved through the specified shifting distance (SHIFT-Y) comes into contact with the workpiece, and then the tool is fed in the direction of the reference angle. D740PA165
Note 1: During machining with the Y-axis shifted, part of the workpiece is not machined. Note 2: Enter 0 under SHIFT-Y if an angle other than 90 degrees is set up as POS-B.
3-17-2 Setting tool sequence data SNo.
TOOL
NOM-φ No.
#
PAT. DEP-1 Z-DEC
RPM
FIN-X FIN-Z C-SP !
R1
FR
M
↑
↑ ↑
↑
↑
↑
↑
↑
↑
↑
↑
↑
[1]
[2] [3]
[4]
[5]
[6]
[7]
[8]
[9]
[10]
[11]
[12]
Remark 1:
!:
Data are not necessary to be set here.
Remark 2: In the tool sequence, one tool is automatically developed as follows. Machining R1 (Roughing)
Pattern One tool for machining is automatically selected.
3-323
M
M
↑
↑
!
[12] [12]
3
PROGRAM CREATION
[1] TOOL (Name) The name of the tool to be used for machining is set automatically. When the cursor is present at this item, the following menu is displayed to allow the tool to be changed: ENDMILL FACEMILL
[2] NOM-φ (Nominal diameter) Enter the nominal diameter of tools using the numeric keys. See the description of the relevant item for BAR unit. [3] NOM-φ (Suffix) A code should be selected out of the menu to identify those tools which are of identical type (having an identical name) and have an identical nominal size. A
Note:
B
C
D
E
F
G
H
HEAVY TOOL
>>>
This unit is applicable only for the upper turret. Therefore tool in the lower turret cannot be selected.
[4] No. (Priority No.) Assign priority levels in the order of machining. See the description of the relevant item for BAR unit. [5] # (Retraction position of the lower turret) For a machine equipped with upper and lower turrets, specify the position to which the lower turret is to be retracted when machining workpieces using only the upper turret. The following menu will be displayed: LOWER TURRET POS.1
LOWER TURRET POS.2
[6] PAT. (Rotational direction of the turning spindle) Set rotational direction of the turning spindle. The following menu will be displayed: CW
CCW
[7] DEP-1 (Maximum cutting depth) Specify the maximum cutting depth per roughing pass. The maximum cutting depth in the X-axial direction is to be specified in terms of radius. See the description of the relevant item for BAR unit.
3-324
PROGRAM CREATION
3
[8] Z-DEC The amount of Z-axial relief per cutting operation can be set to prevent interference between the workpiece and the tool. Z-DEC is accumulated with each cutting operation. [8] Z-DEC
[8] Z-DEC
When the shape is stepped
When the shape is not stepped
D740PA166
[9] RPM Set the turning spindle speed using the numeric keys. Constant surface speed control cannot be conducted. Note:
When the spindle override value is changed during the rotations of both the turning spindle and the milling spindle, both spindle speeds will change according to the entered percentage value (%). Both spindles will stop if 0% is entered.
[10] C-SP Enter the the surface speed for milling tool. [11] FR Enter the desired feedrate of the milling tool in terms of turning spindle speed per revolution. Set the feedrate using the menu or numeric keys. Note:
When VFC is conducted during the execution of this function, the surface speed and feedrate of the milling tool will be updated.
[12] M Specify the M-code to be issued for the tool immediately after it is selected. See the description of the relevant item for BAR unit.
3-17-3 Setting shape sequence data FIG
PTN
SPT-X
SPT-Z
FPT-X
FPT-Z
F-CNR/$
R/th
[1]
[3]
[4]
[5]
[6]
[7]
[8]
The shape sequence data for the mill-turning unit is the same as that for the bar-materials machining unit. See the description of the relevant item in Section 3-9 “Bar-Materials Machining Unit (BAR)”. Note 1: An arc shape, corner R/C at the starting or ending point, and roughness cannot be specified. Note 2: Since nose R of the tool is not taken into account, part of the workpiece may remain unmachined.
3-325
3
PROGRAM CREATION
3-18 Other Units Twelve units are provided moreover: - Manual program machining unit - M-code unit - Head selection unit - Workpiece transfer unit - Subprogram unit - Add-in MAZATROL unit - End unit - Simultaneous machining unit - 2-workpiece machining unit - Coordinate measuring unit - Workpiece measuring unit - Tool measuring unit
3-326
PROGRAM CREATION
3
3-19 Manual Program Machining Unit (MANL PRG) The manual program machining unit complements the turning and milling units described so far (BAR, CPY, CORNER, FACING, THREAD, T. GROOVE, T. DRILL and T. TAP units and point/line/face machining units). These machining units have respective tool paths automatically generated according to the unit data and sequence data you have set, whereas the manual program machining unit requires user setting of its tool path. Select this unit if a machining type or machine action that cannot be programmed in usual machining units is required, or if it is likely to be more convenient to directly set a tool path. Press the [MANUAL PROGRAM] menu key to select this unit.
3-19-1 Setting unit data UNo.
UNIT
TOOL
NOM-φ
No.
#
POS-B
∗
MANL PRG
[1]
[2]
[3]
[4]
[5]
[1] TOOL Specify the tool to be used. If a tool is not specified, the currently valid tool will be used as it is. Select menu key corresponding to the tool used. Pressing the [ >>> ] menu key changes the menu a → b → c → a in this order. ENDMILL FACEMILL CHAMFER BALL CUTTER ENDMILL CENTER DRILL
DRILL
GENERAL
GROOVE
BACKSPOT REAMER FACER THREAD
T.DRILL
OTHER TOOL
TOUCH SENSOR
TAP
BORING BAR
T.TAP
>>> a
BACK BOR.BAR
>>>
CHIP VACUUM
b
SPECIAL
>>>
c
[2] NOM-φ Enter the nominal diameter of the tool by means of numeric keys. Input range is 0.1 to 999.9. In the case of the identical designation and length but of different materials, it is necessary to differentiate them by identification code. The identification code is selected from the menu: A
B
C
D
E
F
G
H
HEAVY TOOL
>>>
In order to designate the heavy tool, select the desired menu item after having displayed the menu for heavy tool identification code by pressing the [HEAVY TOOL] menu key. For the machine with the lower turret, select the turret in which the tool to be used is mounted. The following menu is displayed (if [SET UPPER TURRET] is selected, the column will remain blank, and if [SET LOWER TURRET] is selected, “ ” will be displayed). See Section 5, LOWERTURRET CONTROL FUNCTIONS, for further details: SET UPPER TURRET
SET LOWER TURRET
3-327
3
PROGRAM CREATION
Note:
When one of the menu items [END MILL], [FACE MILL], [CHAMFER CUTTER] and [BALL ENDMILL] is selected in the article TOOL, the alarm 434 NO ASSIGNED TOOL IN TOOL FILE is displayed if a tool with the specified nominal diameter has not been previously recorded in the TOOL FILE display.
[3] No. Determine the priority machining number (prior machining, subsequent machining). The input of data is done in accordance with the following 3 methods; - Priority No. for prior machining: Enter the number by means of numeric keys. Input range is 0 to 99. - Priority No. for subsequent machining: Press the [DELAY PRIORITY] menu key, then enter the number by means of numeric keys. Input range is 0 to 99. MACHINING PRIORITY No? DELAY PRIORITY
PRI.No. PRI.No. CHANGE ASSIGN
PRI.No. SUB PROG ALL ERAS PROC END
- Without input: Normal machining: The machining order is not specified. Note:
For details, refer to Chapter 4, “PRIORITY FUNCTION FOR THE SAME TOOL.”
[4] # (Simultaneous machining No. or retraction position of the lower turret) For a machine equipped with upper and lower turrets, to use the tools mounted in both turrets, specify the simultaneous machining number. It is also possible to specify the position to which the lower turret is to be retracted when machining workpieces using only the upper turret. The following menu will be displayed: LOWER TURRET POS.1
Note:
LOWER TURRET POS.2
See Chapter 5, “LOWER-TURRET CONTROL FUNCTIONS”, for details of item [4].
[5] POS-B From the menu, select an angle for indexing the B-axis. You can specify an angle using numerical keys. See the description of the relevant item for BAR unit.
3-328
PROGRAM CREATION
3
3-19-2 Setting sequence data In the manual program machining unit, one sequence data line corresponds to one EIA/ISO program block. For the details of each of the commands, refer to the Programming Manual (Programming EIA/ISO). SEQ
G1
G2
DATA-1
DATA-2
DATA-3
DATA-4
DATA-5
DATA-6
S
M/B
1
[1]
[2]
[3]
[4]
[5]
[6]
[7]
[8]
[9]
[10]
[1] G1, [2] G2 Enter the G-codes (preparatory function) by means of menu keys or numeric keys. G00
Note:
G01
G02
G03
G40 CANCEL
G41 LEFT
G42 RIGHT
G98 /MIN
MANUAL END
G99 /REV
Up to two G-code commands can be designated in one sequence data line.
[3] [2], [3] # (Turret selection and simultaneous machining No.) - For the machine with the lower turret, select the turret for which M-codes are to be output. The following is displayed: SET UPPER TURRET
SET LOWER TURRET
- For the machine with the lower turret, set the simultaneous machining number to be used to operate the upper and lower turrets at the same time. [4] #1 to #12 Set the desired M-code number in each of the 12 items by means of the following menu or numeric keys. Pressing the [ >>> ] menu key changes the menu a → b → c → a in this order. 01 08 09 153 154 206 207 306 307 OPTIONAL FLOOD FLOOD MILL-THR MILL-THR HD1 CHK HD1 CHK HD2 CHK HD2 CHK STOP COOL ON COOL OFF COOL ON COOL OFF OPEN CLOSE OPEN CLOSE 901 HEAD1 SELECT
902 202 302 HEAD2 HEAD1 HEAD2 SELECT TRN MODE TRN MODE
03 T-SP1 CW
200 300 203 204 205 C1-AXIS C2-AXIS MILL-SP MILL-SP MILL-SP CONNECT CONNECT CW CCW STOP
3-331
04 T-SP1 CCW
303 T-SP2 CW
304 T-SP2 CCW
>>> a
>>> b
>>> c
3
PROGRAM CREATION
The M-codes you have set are executed in the following order: #1
#2
#3
#4
#5
#6
#7
#8
#9
#10
#11
#12
∗∗∗
∗∗∗
∗∗∗
∗∗∗
∗∗∗
∗∗∗
∗∗∗
∗∗∗
∗∗∗
∗∗∗
∗∗∗
∗∗∗
1. (Synchronous)
2. (Synchronous)
3. (Synchronous)
If not all of the intended M-codes are to be executed at the same time, therefore, divide them into three groups (#1 through #4, #5 through #8, and #9 through #12) and then set those M-codes separately. Note 1: For the list of M-codes provided in the NC system, see the Operating Manual. The M-codes M02 (Program End), M98 (Subprogram Call), or other dedicated M-codes for EIA/ISO program cannot be selected. Note 2: For a machine with an optional second miscellaneous function, second miscellaneous function codes can be issued with #4, #8, and #12. In such a case, make the [OTHER CODE] menu function valid and enter code numbers. Note 3: The M-codes listed in the menu vary from machine to machine. Note 4: For details of M-codes, refer to the Operating Manual of the machine.
3-332
PROGRAM CREATION
3
3-21 Head Selection Unit (HEAD) With the head selection unit, select a spindle (No. 1 or No. 2) you are going to operate, before programming various machining units. Once an operation side (pattern) has been selected, it will remain valid until a different operation pattern is selected with another head selection unit. Press the [SELECT HEAD] menu key to select this unit.
3-21-1 Setting unit data UNo.
UNIT
TYPE
HEAD
SPDL
*
HEAD
[1]
[2]
!
[1] TYPE From the following menu, select an operation pattern for each spindle. SINGLE
SYNCH.
SINGLE : Only the spindle you are going to set in the following item [2] will operate. SYNCH. : The spindle specified in item [2] will rotate (master action) and the other spindle will perform synchronous rotation (slave action; same direction and speed). [2] HEAD Select the spindle to be operated. - Set 1 or 2 to operate the No. 1 or the No. 2 spindle, respectively. Note:
Ａ
B
C
Enter 1 for SYNC set in item [1]. UNo. 0 UNo. 1 UNo. 2 UNo. 3 UNo. 4 UNo. 5 UNo. 6 UNo. 7 UNo. 8 UNo. 9 UNo. 10 UNo. 11 UNo. 12
UNIT TYPE HEAD SIN UNIT PART ～ FACING FACE UNIT PART ～ BAR OUT UNIT PAT. ～ TRANSFER BAR UNIT TYPE HEAD SYNC UNIT PART ～ T.GROOVE OUT UNIT PART ～ BAR OUT UNIT PAT. ～ TRANSFER BAR UNIT TYPE HEAD SIN UNIT PART ～ FACING BACK UNIT PART ～ T.DRILL BACK UNIT ～ END
BAR OUT
HEAD 1
HEAD 2 HEAD 1
BAR OUT
HEAD 1 HEAD 2
T. GROOVE OUT
FACING BACK
T. DRILL BACK
A: Machining on the No. 1 spindle side B: Machining in synchronization of the No. 1 and No. 2 spindles C: Machining on the No. 2 spindle side
3-333
FACING FACE
3
PROGRAM CREATION
3-22 Workpiece Transfer Unit (TRANSFER) Select the workpiece transfer unit to change the chucking position of the workpiece, to deliver it from one spindle to the other or to move the No. 2 spindle. Press the [TRANSFER WORKPICE] menu key to select this unit.
3-22-1 Setting unit data UNo. ∗
UNIT
PAT. HEAD SPDL
TRANSFER [1]
[2]
PUSH
[3]
[4]
CHUCK W1 [5]
[6]
W2 Z-OFFSET C1 C2 C-OFFSET LTUR ESC TNo. [7]
[8]
[9] [10]
[11]
[12]
[1] PAT. From the following menu, select a transfer pattern. CHUCK WORK
BAR LOOP
T-SPDL MOVE
CHUCK: To deliver a chuck work from No. 1 to No. 2 spindle or vice versa. BAR: To rechuck a bar work. MOVE: To move the No. 2 spindle on the Z-axis. [2] HEAD - If you have selected CHUCK for data item [1] above: The following menu will be displayed when the cursor is placed at this item. HEAD 1
HEAD 2
→HEAD 2 →HEAD 1
Select [HEAD 1 → HEAD 2] to deliver a workpiece from the No. 1 to the No. 2 spindle. Select [HEAD 2 → HEAD 1] to deliver a workpiece from the No. 2 to the No. 1 spindle. - If you have selected BAR for data item [1] above: The following menu will be displayed when the cursor is placed at this item. HEAD 1
HEAD 2
Select [HEAD 1] to rechuck a workpiece on the No. 1 spindle side. Select [HEAD 2] to rechuck a workpiece on the No. 2 spindle side. - If you have selected MOVE for data item [1] above: No data setting is required. [3] SPDL From the following menu, specify a spindle action (status) during the unit. 0 KEEP
1 2 FORWARD REVERSE
3 ORIENT
4 5 C-AXIS KEEP POSITION POSITION
3-334
[13]
PROGRAM CREATION
3
Specify a spindle action pattern during workpiece rechucking/delivering by selecting one of the items 0 through 5. 0 KEEP: 1 FORWARD: 2 REVERSE: 3 ORIENT:
The spindle does not rotate. The spindle rotates forward at the speed set previously in parameter TC58. The spindle rotates backward at the speed set previously in parameter TC58. The spindle is orientated.
4 C-AXIS POSITION: The No. 1 spindle undergoes C-axis positioning. The No. 2 spindle undergoes orientation or C-axis positioning, depending on the machine specifications. 5 KEEP POSITION: The spindle status specfied in the previous unit is held. [4] PUSH Only when CHUCK is selected for data item [1] above, select whether the workpiece is to be pressed by the No. 2 spindle when workpiece delivery is performed. Set 0 if pressing is to be done, or set 1 if pressing is not to be done. [5] CHUCK Only when BAR is selected for data item [1] above, specify whether the chuck of the spindle indicated in item [3] is to be left open or to be closed after movement of the No. 2 spindle. Set 0 to leave the chuck open Set 1 to close the chuck. [6] W1 - When CHUCK is selected for data item [1] above, set W-axial machine coordinate of the spindle No. 2 for workpiece delivering. - When BAR is selected for data item [1] above, set W-axial machine coordinate of the spindle No. 2 for workpiece rechucking. [7] W2 - When CHUCK is selected for data item [1] above, set W-axial machine coordinate of the spindle No. 2 after workpiece delivering. - When BAR is selected for data item [1] above, set W-axial machine coordinate of the spindle No. 2 after workpiece rechucking. - When MOVE is selected for data item [1] above, set W-axial machine coordinate of the spindle No. 2 after movement. [8] Z-OFFSET Set the Z offset value which becomes valid after delivering the workpiece. [9] C1 Set C-axial machine coordinate of the spindle No. 1 for workpiece delivering. [10] C2 Set C-axial machine coordinate of the spindle No. 2 for workpiece delivering. [11] C-OFFSET Set the C offset value which becomes valid after delivering the workpiece.
3-335
3
PROGRAM CREATION
[12] LTUR ESC Set the Z-axial machine coordinate of the anti-interference standby position to which the lower turret is to be moved for workpiece delivering. [13] TNo. Specify the TNo. of the lower-turret tool to be indexed during workpiece delivering. Example 1: UNo. ∗
UNIT
TRANSFER CHUCK PAT. HEAD SPDL
TRANSFER CHUCK 1→2
1
PUSH 1
CHUCK W1 ◆
No. 1 spindle
W2 Z-OFFSET C1 C2 C-OFFSET LTUR ESC TNo.
∗∗∗ ∗∗∗
∗∗∗
◆
◆
◆
∗∗∗
∗
No. 2 spindle
The chuck of the No. 2 spindle opens. (SPDL = 1: Forward rotation)
The No. 2 spindle moves to the position W1.
The chuck of the No. 2 spindle closes and that of the No. 1 spindle opens.
The No. 2 spindle moves to the position W2.
T4P269
3-336
PROGRAM CREATION
Example 2: UNo. ∗
UNIT
3
TRANSFER BAR PAT. HEAD SPDL
TRANSFER BAR
1
2
PUSH ◆
No. 1 spindle
CHUCK W1 1
◆
W2 Z-OFFSET C1 C2 C-OFFSET LTUR ESC TNo. ∗∗∗
∗∗∗
◆
◆
◆
∗∗∗
∗
No. 2 spindle
The chuck of the No. 1 spindle opens. (SPDL=2: Reverse rotation)
Chuck opens
The No. 2 spindle moves to the position W2. Then the chuck of the spindle indicated in item HEAD will close according to CHUCK=1.
Chuck closes after movement of the No. 2 spindle. T4P270
Example 3: UNo. ∗
UNIT
TRANSFER MOVE PAT. HEAD SPDL
PUSH
◆
◆
TRANSFER MOVE
No. 1 spindle
◆
CHUCK W1 ◆
◆
W2 Z-OFFSET C1 C2 C-OFFSET LTUR ESC TNo. ∗∗∗
∗∗∗
◆
◆
◆
∗∗∗
∗
No. 2 spindle
The No. 2 spindle moves to the position W2.
T4P271
3-337
3
PROGRAM CREATION
3-23 Subprogram Unit (SUB PRO) When the same movement is repeated in a machining process or when a common movement is used in several programs, it is desirable to prepare and call up a special program for this movement with this subprogram unit. In this case, the calling side is referred to as the Main program and the called side is referred to as the Subprogram. Moreover, the call of the sub-program is called Nesting. The subprogram can be used both in the MAZATROL program and in the EIA/ISO program. However, the maximum number of nesting is nine for the MAZATROL program and eight for the EIA/ISO program. Press the [SUB PROGRAM] menu key to select this unit.
3-23-1 Setting unit data UNo.
UNIT
WORK No.
NUM.
∗
SUB PRO
[1]
[2]
#
[3]
[4]
[1] WORK No. Enter the work number of the desired subprogram. The following menu is displayed: MEASURE MACRO
PROGRAM FILE
Enter the work number using the numerical keys, or press the [PROGRAM FILE] menu key and select the work number from the work-Nos. listing window. Note:
To call up as a subprogram the measuring macro whose execution will result in origin coordinates or tool correction data being changed, press the [MEASURE MACRO] menu key and then select the work number while the menu is displayed in reverse mode. Selecting the program while the menu is displayed in reverse mode displays the selected work number in yellow. Selecting the program while the menu is not displayed in reverse mode displays the selected work number in white.
[2] NUM. Enter the number of repetitions of the subprogram. If no data is entered here, the subprogram will be executed one time. [3], [4] # (Turret selection and simultaneous machining No.) For the machine with the lower turret, select the turret for which subprogram call are to be output. The following menu is displayed: SET UPPER TURRET
SET LOWER TURRET
For the machine with the lower turret, set the simultaneous machining number to be used to operate the upper and lower turrets at the same time.
3-338
PROGRAM CREATION
3
3-23-2 Setting sequence data UNo.
UNIT
WORK No.
NUM.
#
∗
SUB PRO
∗∗∗
∗∗∗
∗∗∗
SEQ
ARGM 1
ARGM 2
ARGM 3
ARGM 4
ARGM 5
ARGM 6
1
[1] [2]
[1] [2]
[1] [2]
[1] [2]
[1] [2]
[1] [2]
[1] [2] ARGM First enter the address [1] and then input the data [2] of an argument in pairs. To set a macro variable as the argument data, press the [MACRO INPUT] menu key before entering the number of the macro variable. In this case, a symbol # is displayed before the numerical data. Note 1: If no argument is required, press the [SEQUENCE END] menu key with the cursor placed at the position [1] under ARGM 1. Note 2: The Z/C offsets in the subprogram inherit the Z/C offsets of the main program, registered in the SET UP MANAG. display. Note 3: When control returns from the subprogram to the MAZATROL program, the settings of the coordinate systems in the subprogram are canceled and control is returned to the coordinate systems existing before execution of the subprogram unit. Note 4: The subprogram does not inherit the active modal information within the main program. The subprogram is executed in accordance with reset modal information. Note 5: During the return of control from the subprogram to the MAZATROL program, modal information is reset to the status existing before subprogram unit execution. Note 6: The subprogram will be executed only once, even if “0” is set as the number of program repetitions. Note 7: Do not use a Cross command (G110) in the subprogram to be called. Note 8: Do not use a queuing P-code in the subprogram to be called. Note 9: The MAZATROL program cannot be called up from the EIA/ISO subprogram that has been called up by the subprogram unit.
3-339
3
PROGRAM CREATION
Note 10: Execution of the subprogram including the upper/lower turret command (G109L_) uses only the program sections for the head/turret specified in the subprogram unit. Other program sections are ignored. See the diagram below. Pattern 1
MAZATROL
Pattern 2
(WNo. 1000) Subprogram
MAZATROL
(G109L1) Machining with upper turret at HD1 :
. . .
Spindle No. 1 Subpro. 1000 Upper turret specified
(G109L2) Machining with upper turret at HD2 :
. . .
(G109L3) Machining with lower turret :
Pattern 3
MAZATROL . . .
Subpro. 3000 Lower turret specified . . .
(WNo. 3000) Subprogram G109L1) Machining with upper turret at HD1 : (G109L2) Machining with upper turret at HD2 : (G109L3) Machining with lower turret :
3-340
. . .
Spindle No. 2 Subpro. 2000 Upper turret specified . . .
(WNo. 2000) Subprogram (G109L1) Machining with upper turret at HD1 : (G109L2) Machining with upper turret at HD2 : (G109L3) Machining with lower turret :
PROGRAM CREATION
3
3-24 Add-In MAZATROL Unit Select the Add-in MAZATROL unit to call up an Add-in MAZATROL as a subprogram from the MAZATROL program.
3-24-1 Setting unit data UNo.
UNIT
WORK No.
REPEAT
*
[1]
[2]
[3]
# [4]
[5]
[1] UNIT Name of the unit is displayed. [2] WORK No. The work number of the Add-in MAZATROL is displayed. [3] REPEAT Enter the number of repetitions of the Add-in MAZATROL. If no data is entered here, the Add-in MAZATROL will be executed one time. [4], [5] # (Turret selection and simultaneous machining No.) - For the machine with the lower turret, select the turret for which command for calling Add-in MAZATROL is to be output. The following is displayed: SET UPPER TURRET
SET LOWER TURRET
- For the machine with the lower turret, set the simultaneous machining number to be used to operate the upper and lower turrets at the same time.
3-24-2 Setting sequence data UNo.
UNIT
WORK No.
REPEAT
∗
∗∗∗
∗∗∗
∗∗∗
SEQ
ARGM 1
ARGM 2
ARGM 3
ARGM 4
1
[1] [2]
[1] [2]
[1] [2]
[1] [2]
[1] [2] ARGM 1 to 4 Address and title are displayed in [1]. Input the data of an argument in [2]. To set a macro variable as the argument data, press the [MACRO INPUT] menu key before entering the number of the macro variable. In this case, a symbol # is displayed before the numerical data. Note 1: The subprogram command mode comes into effect the moment that the tool has reached the safety profile position after machining of the preceding unit. The modal status at the beginning of the called subprogram is the same as the status after resetting. All subprograms must terminate with an M99 command (return from subprogram). Note 2: In the control mode where the coordinate system of the main program is conveyed to the subprogram (bit 7 of F161 is set to 1), the Z-offset data registered in the SET UP MANAG. display for the main program will remain valid for a subprogam in which the MAZATROL coordinate system is selected.
3-341
3
PROGRAM CREATION
3-24-3 Help function on Add-in MAZATROL When the name of the Add-in MAZATROL to be called up, the titles of macro arguments, and other information are defined in any internal text file of the hard disk, the titles of the macro arguments can be displayed in sequence lines, and massage can be displayed for argument setting, just by specifying that Add-in MAZATROL as a subprogram. A special help display for Add-in MAZATROL can also be created. Thus, macro arguments can be easily modified by providing the help display. Note 1: Assign a file name of “EIAMACRO.txt” to the text file to be created. Note 2: The language of the text file is selected according to the setting of parameter K11. Store the text file into the folder matching the display language. Example: For English “C:nm64mdataengEIAMACRO.txt”. Note 3: The help display does not always need to be created. Note 4: This function becomes valid, only when, after the text file and the bmp or png file of the help display have been saved on the hard disk, bit 3 in parameter F81 is set to “1” and then power is turned off and back on. A.
Format of the text file [EIAMACRO-[1]] UnitName=[2] MenuName=[3] WNo.=[4] HelpFileName=[5] Data[6]-[7]=[8], [9], [10], [11], [12], [13] Data[6]-[7]=[8], [9], [10], [11], [12], [13] Data[6]-[7]=[8], [9], [10], [11], [12], [13] : : :
EIA macroprogramspecifying area Argument-specifying area
(Up to 9 programs)
(Up to 24 arguments)
[1] EIA macro number Specify the position of the desired macroprogram menu item. Macroprogram menu items are displayed at the time of unit selection in the MAZATORL programs. A maximum of nine menu items can be displayed. 1
2
3
4
5
6
7
8
9
>>>
[2] Title to be displayed in the PROGRAM display Enter the title for the Add-in MAZATROL which is to be displayed on the PROGRAM display when the menu key corresponding to the position specified in data item [1] above is pressed. Up to eight ASCII characters can be displayed as the title. Example:
UnitName=PTHR OUT
UNo.
UNIT
∗
PTHR OUT
WORK No.
REPEAT
3-342
PROGRAM CREATION
3
[3] Menu item for the PROGRAM display Enter the menu item to be displayed in the menu item display position that was specified in [1] above. In both upper and lower lines, up to eight ASCII characters can be displayed as the menu item. Example:
MenuName=P-THR
P-THR OUT
OUT
[4] Program number of the Add-in MAZATROL Specify the program number of the Add-in MAZATROL. Program numbers 1 to 999999999 can be displayed. Example:
WNo.=777
UNo.
UNIT
WORK No.
∗
PTHR OUT
777
REPEAT
Remark: Program numbers are automatically assigned when the unit is selected. [5] File name of the help display Assign a file name to the graphics within the help display that is to be displayed when macro arguments are entered. This file name must be entered in up to 30 characters, except for an extension. Example:
HelpFileName=PTHROUT
Remark: This line can be omitted when a help display is not to be created. Note 1: Use the following folder to store the graphics within the help display: c:nm64mdata________.bmp (.png) Note 2: When drawing graphics on the help display, use a format of 900 dots (horizontal) by up to 440 dots (vertical). [6] Sequence number of the argument, [7] Display position, [8] Address, [9] Title, [10] Message [6]: Enter the sequence number of the macro argument to be displayed. Up to six SEQ lines can be entered. [7]: Enter the display position (ARGM 1 to 4) of the macro argument. [8]: Enter the address of the macro argument in the alphabet (A to Z). [9]: Enter the title of the macro argument. Up to seven ASCII characters can be displayed as the title. [10]: Enter the message to be displayed when the macro argument is set. Up to 29 ASCII characters can be displayed as the message. Example:
SEQ
Enter data as follows to specify 2 as the sequence number, 4 as the ARGM column number, I as the address, “STP-Z” as the title, and “SPT Z” as the message: Data2-4=I,STP-Z,SPT Z ARGM 1
ARGM 2
ARGM 3
ARGM 4
1
[8]:[9]
[8]:[9]
[8]:[9]
[8]:[9]
2
[8]:[9]
[8]:[9]
[8]:[9]
I:STP-Z
3
[8]:[9]
[8]:[9]
[8]:[9]
[8]:[9]
4
[8]:[9]
[8]:[9]
[8]:[9]
[8]:[9]
5
[8]:[9]
[8]:[9]
[8]:[9]
[8]:[9]
6
[8]:[9]
[8]:[9]
[8]:[9]
[8]:[9]
3-343
3
PROGRAM CREATION
[11] Display of the argument title on the help display Select whether the title of the macro argument that was specified in data item [9] above is to be displayed on the help display. Enter 1 to display the title. Enter 0 if the title is not to be displayed. [12] Horizontal display position in the help display, [13] Vertical display position in the help display [12]: Specify in dots where in the horizontal direction of the help display the title of the macro argument that was specified in data item [9] is to be displayed. [13]: Specify in dots where in the vertical direction of the help display the title of the macro argument that was specified in data item [9] is to be displayed. Note:
If 0 was entered in [11], enter 0 in both [12] and [13].
Example:
Specify the upper left of the title as the display position and enter data as follows: For “STP-Z”, enter 580 in [12] and 235 in [13]. [12]
[13]
D740PA167E
3-344
PROGRAM CREATION
B.
3
Example of text file entry Create the text file [EIAMACRO-1] for the Add-in MAZATROL numbered “777” that contains the following arguments:
D740PA168E
[EIAMACRO-1] UnitName=PTHR OUT MenuName= P-THR OUT WNo.=777 HelpFileName=PTHROUT Data1-1=A,MULTI,NUMBER OF ENTRANCE,0,0,0 Data1-2=B,DEPTH,DEPTH PER PASS,0,0,0 Data1-3=C,FIN,FINISH ALLOWANCE,0,0,0 Data1-4=D,CHAMF,CHAMFERING ANGLE,1,270,200 Data2-1=E,C-SP,CUTTING SPEED,0,0,0 Data2-2=F,TOOL,TOOL NUMBER,0,0,0 Data2-3=H,SPT-X,SPT X,1,625,400 Data2-4=I,SPT-Z,SPT Z,1,580,235 Data3-1=J,FPT-X,FPT X,1,205,345 Data3-2=K,FPT-Z,FPT Z,1,485,170 Data3-3=V,ANGLE,THREAD ANGLE,1,405,405 Data3-4=M,LEAD,THREAD LEAD,1,420,210
Remark 1: Enter a comment after the semicolon (;). [Ex] UnitName=PTHR OUT ；Specification of unit name Remark 2: The file of the graphics in the above help display is “c:nm64mdataPTHROUT.bmp”.
3-345
3
PROGRAM CREATION
3-25 End Unit (END) Select the end unit after the entire program data required for machining has been set. For this unit, set data about the machine action to occur at the end of machining and about the program execution mode. Such data is referred to as end data. You must set this unit on the last line of a program. Press [END] menu key to select this unit. POINT LINE FACE TURNING MANUAL MACH-ING MACH-ING MACH-ING PROGRAM
END
SHAPE CHECK
>>>
3-25-1 Setting unit data UNo.
UNIT
∗
END
CONTI. REPEAT
[1]
[2]
SHIFT
[3]
NUMBER ATC
[4]
[5]
RETURN
LOW RET.
[6]
[7]
WORK No. EXECUTE
[8]
[9]
[1] CONTI. Specify whether you want to carry out the machining operation repeatedly in succession. - Set 0 to execute the current program once. - Set 1 to execute the current program perpetually. - Always set 1 for the subprogram. At this time, the settings in REPEAT and SHIFT become invalid. Note:
If no data has been set in this item, the NC will interpret that 0 has been set.
[2] REPEAT If the current program is to be executed repeatedly, set the desired number of times of execution. [3] SHIFT Shifting the origin of the current program and repeatedly executing it enable multiple parts of the same shape, or a single part of identical recurring shape patterns as shown in diagram below, to be made from one workpiece.
SHIFT
T4P280
For such machining, set the desired shift amount of the program origin in this item. Note 1: If no data has been set in this item, the shift amount will be regarded as 0. Note 2: Data must not be set in this item if a measurement unit is to be executed. Setting data other than 0 will cause alarm 657 ILLEGAL NUMBER INPUT at the second measurement. Note 3: As for repetitive machining on a single workpiece, the following condition must be satisfied: LENGTH
> REPEAT × SHIFT +
(Common data)
(END unit)
3-346
WORK FACE (Common data)
PROGRAM CREATION
3
[4] NUMBER Specify whether you want the NC unit to count the number of machined workpieces (number of program loops). - Set 1 if counting is desired. - Set 0 if counting is not desired. If you set 1, the number of machined workpieces will be displayed at COUNTER of the POSITION display. Note:
Counting does not occur if no data has been set in this item.
[5] ATC Specify the ATC movement at the end of machining. - Set 0 if the tool is not returned. - Set 1 if the axes are moved after returning the tool. - Set 2 if the tool is returned after axis movement Note:
If no data is set, it is regarded that 1 has been set.
[6] RETURN Specify from the menu the position to which the turret is to be returned after machining. TOOL ZERO FIXED CHANGE POSITON POSITION POSITION
ARBITRAR POSITION
Note 1: The tool change position of the turret is specified by parameter SU10, the fixed position by parameter M5. To return the turret to a specific position, do not change the setting of parameter M5. Instead, select [ARBITRAR POSITION] and specify the coordinates of that position. (Refer to the separate Parameter List/Alarm List/M-Code List for further details.) Note 2: If no data is set in this item, the tool change position will be regarded as having been specified. Note 3: During returning, linear axes move at first and then rotational axes. Note 4: If the setting for CONTI. is “1”, whether RETURN is to be executed can be selected by assigning the appropriate value to bit 5 in parameter TC144. 0: Non-execute, 1: Execute Even when “0” (Non-execute) is set, however, RETURN will be executed if REPEAT is specified or if the target count in the POSITION display is reached with NUMBER set equal to “1” and the machine comes to a stop. Note 5: The axes for which the returning function is valid differs according to the value specified in RETURN. The returning function is performed on either of the following axes: RETURN
Axes for which the returning function is valid
TOOL CHG (SU10)
X-axis, Z-axis
HOME
X-axis, Y-axis, Z-axis
FIXED PT (M5)
X-axis, Y-axis, Z-axis
ARB PT
Axes for which the returning position has been set in arbitrary position sequence
3-347
3
PROGRAM CREATION
Even if RETURN = HOME, axes other than the X-, Y-, or Z-axes will not be returned to the respective home positions. To return axes other than the X-, Y-, or Z-axes to the home positions, select [ARBITRAR POSITION] and then specify the desired axes in the arbitrary position sequence. Example:If 'X0, Y0, Z0, B0, C0' is set in the arbitrary position sequence, the X-, Y-, Z-, B-, and C-axes will be returned to the respective home positions. [7] LOW RET. Specify from the menu the position to which the lower turret is to be returned after machining. TOOL LOWER ZERO FIXED CHANGE POSITON POSITION TURRET POSITION POS.1
LOWER ARBITRAR TURRET POSITION POS.2
Note 1: The tool change position of the lower turret is specified by parameter SU10, the fixed position by parameter M5, lower-turret retraction position 1 by parameters SU97, SU98, and lower-turret retraction position 2 by parameters SU99, SU100. When lower-turret retraction position 1 is set, the lower turret moves to the retraction position, after the tool specified by parameter SU52 is indexed. When lower-turret retraction position 2 is set, the lower turret moves to the retraction position, after the tool specified by parameter SU53 is indexed. No tool index occurs when 0 is set to SU52 or SU53 respectively. (Refer to the separate Parameter List/Alarm List/M-Code List.for further details.) Note 2: If no data is set in this item, the tool change position will be regarded as having been specified. Note 3: When the lower turret is present at a returning position, selection of that retraction position in LOW RET. does not move the turret. Selection of a different returning position or of the home position, fixed position, or any other position moves the lower turret directly to the particular selected position. [8] WORK No. If the starting part of a different program is to be called up after machining, set the work number of that program. Note:
If no data has been set in this item, the starting part of the current program will be called up automatically after machining.
[9] EXECUTE Set whether operation is to be executed after call of the program specified in item [8]. - Set 1 to execute operation based on the called program. - Set 0 if the program is only to be called and operation is not to be executed.
3-348
PROGRAM CREATION
3
Examples of program execution mode The program execution mode is determined by the data that has been set in items [1], [2], [3], [8] and [9] above. If the following data has been set for the end unit of the program of work number A: CONTI.
REPEAT
SHIFT
WORK No.
EXECUTE
Example 1
0 or blank
!
!
Blank
!
Example 2
0 or blank
!
!
B
1 (execute)
Example 3
0 or blank
!
!
B
0 (not execute)
Example 4
1
Blank
!
!
!
Example 5
1
N
0 or blank
Blank
!
Example 6
1
N
0 or blank
B
1 (execute)
Example 7
1
N
0 or blank
B
0 (not execute)
Example 8
1
N
s
Blank
!
Example 9
1
N
s
B
1 (execute)
Example 10
1
N
s
B
0 (not execute)
1:
The program of work number A is executed only once and the machine stops. At that time, the starting part of the same program is called up automatically.
2:
The program of work number A is executed only once, and following this, the program of work number B is executed.
3:
The program of work number A is executed only once and the machine stops. At that time, the starting part of the program of work number B is called up automatically.
4:
The program of work number A is executed repeatedly.
5:
The program of work number A is executed an N number of times and the machine stops. At that time, the starting part of the same program is called up automatically.
6:
The program of work number A is executed an N number of times, and following this, the program of work number B is executed.
7:
The program of work number A is executed an N number of times and the machine stops. At that time, the starting part of the program of work number B is called up automatically.
8:
The program of work number A is repeatedly executed an N number of times while having its origin shifted through the distance s and the machine stops. At that time, the starting part of the same program is called up automatically.
9:
The program of work number A is repeatedly executed an N number of times while having its origin shifted through the distance s and following this, the program of work number B is executed.
10: The program of work number A is repeatedly executed an N number of times while having its origin shifted through the distance s and the machine stops. At that time, the starting part of the program of work number B is called up automatically.
3-349
3
PROGRAM CREATION
3-25-2 Setting sequence data Any position can be specified in the arbitrary-position specification sequence by specifying ARB PT in RETURN or LOW RET. SNo.
DATA-1
DATA-2
DATA-3
DATA-4
DATA-5
DATA-6
DATA-7
DATA-8
DATA-9
∗
The arbitrary-position specification sequence allows coordinates to be specified for each axis and moves the axis to the specified coordinate position in rapid feed mode. Note:
“Arbitrary Position” (ARB PT) must be selected in RETURN or LOW RET. before it becomes possible to move the axis for which any position has been specified.
UNo.
UNIT
∗
END
SNo.
DATA-1
CONTI.
REPEAT
SHIFT
NUMBER
RETURN END
DATA-2
DATA-3
DATA-4
DATA-5
DATA-6
LOW RET. WORK No. EXECUTE ARB PT
The following menu will be displayed.
SELECT TRANSFER PROCESS HEAD WORKPICE END
(4) Press the [SIMUL.] menu key.
3-26-2 Setting unit data UNo.
UNIT
No.
SIMUL.No.
RPM
∗
SIMULTAN
[1]
[2]
[3]
[1] No. Specify the priority machining number for the the simultaneous machining [2] SIMUL. No. Specify the group number for the simultaneous machining using both turrets. [3] RPM Enter the turning spindle speed of the simultaneous machining group specified in [2] above.
3-351
3
PROGRAM CREATION
3-27 Two-Workpiece Machining Unit (2 WORKPC) If you are using a machine equipped with a lower turret, select this unit when machining the 2 workpieces on the No. 1 and No. 2 spindles simultaneously, using the upper and lower turrets. See Chapter 5, “LOWER-TURRET CONTROL FUNCTIONS”, for further details of this unit.
3-27-1 Procedure for calling up the 2 WORKPC unit (1) Press the menu selector key (key located at the right of the menu keys). The following menu will be displayed. POINT LINE FACE TURNING MANUAL MACH-ING MACH-ING MACH-ING MACH-ING PROGRAM
END
SHAPE CHECK
>>>
(2) Press the [ >>> ] menu key. '
The following menu will be displayed. M CODE
SUB PROGRAM
WPC MSR
WORKPICE TOOL WORKPICE MEASURE MEASURE SHAPE
>>>
SIMUL. 2 WORKPC MODE
>>>
(3) Press the [ >>> ] menu key. '
The following menu will be displayed.
SELECT TRANSFER PROCESS END HEAD WORKPICE
(4) Press the [2 WORKPC MODE] menu key.
3-27-2 Setting unit data UNo.
UNIT
PAT.
SP1/SP2
∗
2 WORKPC
[1]
[2]
[1] PAT. Specify the start and end points for machining 2 workpieces simultaneously. The following menu is displayed. START
END
[2] SP1/SP2 When machining the workpieces on the No. 1 and No. 2 spindles, specify which turret to use: upper or lower turret. The following menu is displayed.
3-352
PROGRAM CREATION
3
3-28 Coordinate Measuring Unit (MMS) The coordinate measuring unit measures coordinates using a touch sensor during automatic operation and automatically establishes the workpiece coordinate system. The position of the reference face is measured and the Z-offset value is automatically set. Or the center of a projection or a groove is measured and the C-offset value is automatically set.
3-28-1 Procedure for calling up the MMS unit (1) Press the menu selector key (key located at the right of the menu keys). The following menu will be displayed. POINT LINE FACE TURNING MANUAL MACH-ING MACH-ING MACH-ING MACH-ING PROGRAM
END
>>>
SHAPE CHECK
(2) Press the [ >>> ] menu key. '
The following menu will be displayed. M CODE
SUB PROGRAM
WPC MSR
WORKPICE
>>>
TOOL WORKPICE MEASURE MEASURE SHAPE
(3) Press the [WORKPICE MEASURE] menu key.
3-28-2 Setting unit data UNo.
UNIT
TOOL
NOM-φ
No.
U.SKIP
$
MMS
TOL SENS
[1]
[2]
[3]
!
[1] NOM-φ Specify the nominal diameter of the feeler. Enter the approximate diameter of the point of feeler by means of numeric keys. [2] No. Specify the priority machining number for the coordinate measuring. [3] U. SKIP Specify whether the MMS unit is executed or not.
3-28-3 Setting sequence data SNo.
PTN
X
Y
Z
C
X
R
D/L
K
DIR
1
[1]
[2]
[2]
[2]
[2]
!
[3]
[4]
[5]
[6]
[1] PTN Select the type of measurement from the following menu. Z FACE
C FACE
C GROOVE
C STEP
CALIBR.
For details, refer to “Type of measurement.” [2] X, Y, Z, C Specify the measurment starting position by means of numeric keys.
3-353
PTN END
>>>
3
PROGRAM CREATION
[3] R Specify the surface coordinates to be measured by means of numeric keys. The contents of the entry vary according to the type of measurement. [4] D/L Specify the width of the groove, the width of the projection, etc., or specify for measurement retry the angle of shift of the measurement start point, by means of numeric keys. The contents of the entry differ according to the type of measurement. For details, see Subsection “Type of measurement.” [5] K Specify the feed distance at skip speed by means of numeric keys. The term skip speed means the feed speed at the time when the probe comes into contact with the surface to be measured. [6] DIR. Select from the menu the direction (arrow) of the milling spindle head during measurement, and the approach/escape direction to be applied to the measurement. ← Z
← X
↓ Z
↓ X
→ Z
→ X
Selection of the [ ←X ] menu key specifies the B-axis (milling spindle head) facing in the direction of the arrow (left) and the approach/escape in X-axial direction during the measurement.
X ←X
↓X
←Z
↓Z
Z
D736P0107
Note 1: During the process of the measurement movement, the block by block stop and rapid feed deceleration are effective, but not the override of skip feed. Note 2: The coordinate measuring unit operates in the original programmed coordinate system until all measuring patterns contained in the unit have been executed to completion. Measured data becomes valid for the next unit onward. Under normal operating conditions, set this unit at the beginning of the program. Note 3: Before execution of the coordinate measuring unit turn off the symmetrical image function. The measurement movement after contact with the workpiece may not be correctly performed if the symmetrical image function is valid.
3-354
PROGRAM CREATION
3
3-28-4 Type of measurement Select the type of measurement for the offset of the coordinates system. The four types of measurement are available. Measurement of the reference surface ..... Z-FACE, C-FACE Measurement of groove center ........... C-GRV Measurement of center of projection width .. C-STP Each measurement type is described in the following descriptions 1 to 4: 1.
Z-FACE The Z-offset value can be adjusted by entering the distance from the workpiece origin to reference surface Z. SNo.
PTN
X
Y
Z
C
X
R
D/L
K
DIR.
1
Z-FACE
x1
y1
z1
c1
!
rz
!
k
←X
!: Not necessary to be set here.
[5]
[4]
[1]
[2]
[3]
[1] Movement to measurement start point x1, c1 and to the clearance point z [2] Movement to measurement start point z1 [3] Measurement at the skip feed [4] Movement to the measurement start point from the skipping position [5] Movement to the clearance point z
z1
rz
x1
2.
D740PA011
C-FACE The C-offset value can be adjusted by entering the distance from the workpiece origin to reference surface C. SNo.
PTN
X
Y
Z
C
X
R
D/L
K
DIR.
1
C-FACE
x1
!
z1
c1
!
rc
l
!
←X
!: Not necessary to be set here.
[1] [3] [2] [1]
CW CCW
[5] [4]
Measurement start point x1, z1, c1
[2] [3] [4] [5]
Movement to measurement start point z1, c1 and to the clearance point x Movement to measurement start point x1 Measurement at the skip feed Movement to the measurement start point from the skipping position Movement to the clearance point x D740PA012
Remark: The measurement direction is determined as follows: CW, when c1 (measurement start point C) ≥ rc (coordinate C of the surface to be measured) and CCW, when c1 (measurement start point C) < rc (coordinate C of the surface to be measured).
3-355
3
PROGRAM CREATION
3.
C-GRV The C-offset value can be adjusted by entering the distance from the workpiece origin to the groove center and the groove width. SNo.
PTN
X
Y
Z
C
DIR.
R
D/L
K
DIR.
1
C-GRV
x1
!
z1
c1
CCW
rc
l
k
←X
!: Not necessary to be set here.
[1] [2]
[1]
[3] [3]
[2]
[4]
[5]
Measurement start point x1, z1, c1
[4]
[9]
[5] [6]
[8]
[6]
[7]
[7]
[8] [9]
Movement to measurement start point z1, c1 and to the clearance point x Movement to measurement start point x1 at the measuring approach speed Pre-measurement at the measuring approach speed Movement through measuring return stroke “k” from the skipping position The first measurement at the skip feed Movement to the measuring start point at the opposite side The second measurement at the skip feed Movement through measuring return stroke “k” from the skipping position Movement to the clearance point x D740PA014
Remark 1: If the sensor operates during movement at the measuring approach speed in step [2], this step will be repeated again (this is referred to as the retry function). The retry function is described later in this manual. Remark 2: If 0 is entered for the amount of measurement return, only pre-measurement at the measuring approach speed for one side will occur and both-side measurement at the measuring speed will not occur. 4.
C-STP The C-offset value can be adjusted by entering the distance from the workpiece origin to the projection center and the projection width. SNo.
PTN
X
Y
Z
C
X
R
D/L
K
DIR.
1
C-STP
x1
!
z1
c1
!
rc
l
k
←X
!:
[1] Movement to measurement start point z1, c1 and to the clearance point x [2] Movement to measurement start point x1 [3] Pre-measurement at the measuring approach speed [4] Movement through measuring return stroke “k” from the skipping position [5] The first measurement at the skip feed [6] Movement through measuring return stroke “k” from the skipping position [7] Movement to the clearance point x [8] C-axis movement to the measurement start point at the opposite side. [9] X-axis movement to the measurement start point at the opposite side. [10] The second measurement at the skip feed [11] Movement through measuring return stroke “k” from the skipping position [12] Movement to the clearance point x
[8] [9] [12]
[10] [11] [1]
[7]
[6] [5][4] [2]
[3]
Not necessary to be set here.
l rc
Measurement start point x1, z1, c1
D740PA016
3-356
PROGRAM CREATION
3
Remark 1: If the sensor operates during movement at the measuring approach speed in step [2], this step will be repeated again (this is referred to as the retry function). The retry function is described below. Remark 2: If 0 is entered for the amount of measurement return, only pre-measurement at the measuring approach speed for one side will occur and both-side measurement at the measuring speed will not occur. [Measurement retry] After temporarily returning to the outside diameter clearance point, the feeler shifts in a circumferential direction through the distance corresponding to [Measuring width × Parameter K21 (Measurement retry width) / 100] and then returns to measurement. The retry function is executed the number of times specified in parameter K22 (measurement retry count). If the sensor operates in spite of this count being exceeded, an alarm will result. Note:
During the retry function for C-STP measurement, an actual retry count may be less than the setting of K22 (specified retry count). Since the retry count is limited to such a value that does not cause the total shifting width by retry to exceed a projection width of 100%, the system operates as follows: If K22 × K21 < 100, measurement is repeated as often as the setting of K22. If K22 × K21 ≥ 100, measurement is repeated as often as the number of times obtained by rounding any fractions of 100/K21.
ON
D736P0139
3-357
3
PROGRAM CREATION
3-29 Workpiece Measuring Unit (WORK MES) The workpiece measuring unit uses a touch sensor to measure the dimensions of the workpiece. Also, measurement results are used for automatic setting of tool correction data. The workpiece measuring unit measures coordinates after indexing the spindle head in the direction specified by DIR. in sequence data, not to the B-axis angle specified in the index unit. Enter the coordinates of actual axes of the machine coordinate system as the coordinates in sequence data.
3-29-1 Procedure for selecting workpiece measuring unit (1) Press the menu selector key (key located at the right of the menu keys). The following menu will be displayed. POINT LINE FACE TURNING MANUAL MACH-ING MACH-ING MACH-ING PROGRAM
END
SHAPE CHECK
>>>
(2) Press the [ >>> ] menu key. '
The following menu will be displayed. M CODE
SUB PROGRAM
WPC MSR
WORKPICE
TOOL WORKPICE MEASURE MEASURE SHAPE
>>>
(3) Press the [WORKPICE MEASURE] menu key.
3-29-2 Setting the unit data UNo.
UNIT
COMPENSATE OFS-TOOL
WORK MES
[1]
[2]
COMP.DATA
SNS-TOOL
No.
#
INTERVAL
OUTPUT
[3]
[4] TOL SENS
[5]
[6]
[7]
[8]
[1] COMPENSATE Select from the menu whether the measurement results are to be used to correct tool data. YES
NO
[2] OFS-TOOL Specify by its tool name, nominal diameter (nominal size) and identification code, the tool for which the measurement results are to be incorporated. If NO has been specified in COMPENSATE, a ! mark is displayed to indicate that no data can be entered. [3] COMP. DATA When the offset tool is either an end-milling tool, a face-milling tool, a ball end-milling tool, a special tool, or a tap, select the measurement results incorporating destination from the menu. DIAMETER LENGTH
If a tool other than those mentioned above has been selected as the offset tool, a ! mark is displayed to indicate that no data can be entered. If NO has been specified in COMPENSATE, a ! mark is displayed to indicate that no data can be entered.
3-358
3
PROGRAM CREATION
[4] SNS-TOOL Enter the nominal diameter and identification code of the touch sensor. [5] No. Enter the machining priority number. [6] # Specify the retraction position of the lower turret during measurement. [7] INTERVAL Specify the intervals at which the workpiece measuring unit is to be executed. [8] OUTPUT Select whether the measurement results are to be sent to external equipment. 0: No output 1: Output to a text file on the HDD. The text files that can be sent to HDD are up to 100 MB in file size. (This maximum size can be changed using parameter DPR8.) 2: Output to a serial printer via an RS-232C interface Note:
Specify output items in parameter F112.
3-29-3 Setting the sequence data SNo.
PTN
SPT-X
SPT-Y
SPT-Z
FPT-X
FPT-Y
FPT-Z
1
[1]
[2]
[2]
[2]
[3]
[3]
[3]
T LIM+ T LIM–
[4]
BASE
DIR
[6]
[7]
[5]
[1] PTN Select a workpiece measuring pattern from the menu. A press of the [ >>> ] menu key displays menus in the order of [1]→[2] →[3] →[1]. OUTER X OUTER Y INNER X INTER Y DIA DIA DIA DIA X WIDTH
Y WIDTH
Z WIDTH
+X STEP
INNER GRV
INNER WIDTH
EXT M.TOOL
EXT T.TOOL
-X STEP
X GRV
Y GRV
Z GRV
+Y STEP
-Y STEP
+Z STEP
>>>
-Z STEP
>>>
>>>
[1]
[2]
[3]
When [OUTER X DIA] or [INNER X DIA] is selected, specify the measuring method next. 0: Both-side measurement 1: Single-side measurement [2] SPT-X, SPT-Y, SPT-Z Specify the starting position of measurement. Setup data items differ according to the selected measuring pattern. [3] FPT-X, FPT-Y, FPT-Z Specify the ending position of measurement. Setup data items differ according to the selected measuring pattern.
3-359
3
PROGRAM CREATION
[4] T LIM+ Set the upper-limit value of the tolerance. [5] T LIM– Set the lower-limit value of the tolerance. [6] BASE Set the reference position for measurement. 0: The starting position is defined as reference. 1: The ending position is defined as reference. [7] DIR. Select from the menu the direction (arrow) of the milling spindle head during measurement, and the approach/escape direction to be applied to the measurement. ← Z
← X
↓ Z
↓ X
→ Z
→ X
Selection of the [ ←X ] menu key specifies the B-axis (milling spindle head) facing in the direction of the arrow (left) and the approach/escape in X-axial direction during the measurement. X ←X
↓X
←Z
↓Z
Z
D736P0107
3-29-4 Selection of a measurement type The following measurement types are provided for the workpiece measurement unit. - Outside-diameter measurement (OUTER X, OUTER Y) ....... To measure the outside-diameter of machined workpiece. - Inside-diameter measurement (INNER X, INNER Y) ....... To measure the inside-diameter of machined workpiece. - Groove width measurement (X GRV, Y GRV, Z GRV, IN GRV) ....... To measure the width of groove or other recesses. - Protrusion width measurement (X WIDTH, Y WIDTH, Z WIDTH, IN WIDTH) ....... To measure the width of protrusion or other convexities. - Step distance measurement (+X STEP, –X STEP, +Y STEP, –Y STEP, +Z STEP, –Z STEP) ....... To measure the step distance of machined workpiece - External measurement (EXT MILL, EXT TURN) ....... To read the measurement data of an external measuring unit. (During this unit, the data is only read in for compensating the tool data registered in the NC unit; no machine action takes place.)
3-360
PROGRAM CREATION
1.
3
Outside-diameter measurement Select OUTER X to measure X-axial points on the outside-diameter section of the workpiece. Select OUTER Y to measure Y-axial points on the outside-diameter section of the workpiece. Also, a measuring method can be selected for OUTER X. 0: Both-side measurement (Measuring the distance between two points with the position of X = 0 as its center) 1: Single-side measurement (Measuring the distance between the reference point and measuring point within the plus area of the X-axis) SNo.
PTN
SPT-X SPT-Y
1
OUTER X 0
SNo.
PTN
1
OUTER X 1
!
x1
SPT-X SPT-Y x1
SPT-Z
FPT-X
FPT-Y
FPT-Z
z1
!
!
!
T LIM+ T LIMt1
SPT-Z
FPT-X
FPT-Y
FPT-Z
!
z1
x2
!
z2
SNo.
PTN
SPT-X
SPT-Y
SPT-Z
FPT-X
FPT-Y
FPT-Z
1
OUTER Y
!
y1
z1
!
!
!
z1
!
←X
BASE
DIR.
S
←X
BASE
DIR.
!
←X
t2
T LIM+ T LIMt1
DIR.
t2
T LIM+ T LIMt1
BASE
t2
z1
OUTER X (Both-side)
OUTER Y
y1
x1
x1, y1: Outside-diameters to be measured z1: Z-coordinate of the measuring position
D736P0113
z1 z2 OUTER X (Single-side)
x1, z1: Reference point x2: Outside-diameter to be measured z2: Z-coordinate of the measuring position
x1
x2
D737P0002
Set “0” as the reference position in the case of single-side measurement.
3-361
3
PROGRAM CREATION
[Measurement movement (OUTER)] Rapid feed Approach speed (parameter K14)
[1] [2] [3]
TC37
Skip feed
[6] [7]
[4] [5]
K19
[8]
TC39 [11] K19
[10] [9]
[12] [13]
D740PA151
2.
Inside-diameter measurement Select INNER X to measure any two X-axial points on the inside-diameter section of the workpiece. Select INNER Y to measure any two Y-axial points on the inside-diameter section of the workpiece. Also, a measuring method can be selected for INNER X. 0: Both-side measurement (Measuring the distance between two points with the position of X = 0 as its center) 1: Single-side measurement (Measuring the distance between the reference point and measuring point within the plus area of the X-axis) SNo.
PTN
SPT-X SPT-Y
1
INNER X 0
SNo.
PTN
1
INNER X 1
x1
◆
SPT-X SPT-Y x1
SPT-Z
FPT-X
FPT-Y
FPT-Z
z1
◆
◆
◆
SPT-Z
FPT-X
FPT-Y
FPT-Z
◆
z1
x2
◆
z2
SNo.
PTN
SPT-X
SPT-Y
SPT-Z
FPT-X
FPT-Y
FPT-Z
1
INNER Y
◆
y1
z1
◆
◆
◆
3-362
T LIM+ T LIMt1
t2
T LIM+ T LIMt1
t2
T LIM+ T LIMt1
t2
BASE
DIR.
◆
←Z
BASE
DIR.
S
←Z
BASE
DIR.
◆
←Z
PROGRAM CREATION
z1
3
z1
INNER X (Both-side)
INNER Y
x1
y1
x1, y1: Inside-diameters to be measured z1: Z-coordinate of the measuring position D736P0115
z1
INNER X (Single-side)
x1, z1: Reference point x2: Inside-diameter to be measured z2: Z-coordinate of the measuring position
z2
x2
x1
D737P0003
[Measurement movement (INNER)] Rapid feed Approach speed (parameter K14) [6]
[5]
[7]
[4]
Skip feed [1] [2]
K19
[3] [8]
[9]
[10] [11] [14] K19
[12]
[15] TC38
[13] TC39 TC37
D736PA152
3-363
3
PROGRAM CREATION
3.
Groove width measurement For X GRV, Y GRV, and Z GRV measurements are performed on X-axial, Y-axial, and Z-axial groove widths, respectively. For IN GRV, the groove width at the inside diameter side is measured. SNo.
PTN
SPT-X
SPT-Y
SPT-Z
FPT-X
FPT-Y
FPT-Z
1
X GRV
x1
y1
z1
x2
y2
z2
SNo.
PTN
SPT-X
SPT-Y
SPT-Z
FPT-X
FPT-Y
FPT-Z
1
IN GRV
x1
y1
z1
x2
y2
z2
T LIM+ T LIMt1
t2
T LIM+ T LIMt1
t2
BASE
DIR.
S
←Z
BASE
DIR.
S
←Z
IN GRV
X GRV z2
z2
z1 z1
x1 x2
x1, y1, z1: Measurement start point # x2, y2, z2: Measurement end point $
x1
x2
D736P0117
[Measurement movement (X GRV)]
[1] [2]
[1] [2]
TC37
[4] K19
[4] [3]
[5]
[6] [8] [9]
K19
[7]
[7] [9]
[11] [10]
K19
K19
TC39 #:Start point $: End point
X
Rapid feed
X
Z
Y
Approach speed (parameter K14) Skip feed D740PA153
3-364
3
PROGRAM CREATION
[Measurement movement (IN GRV)]
Rapid feed Approach speed (parameter K14)
TC37 K19
K19
Skip feed
TC39
[10]
[6] [1] [2]
[7]
Z2 [11] [12]
[9] [8]
[5] [4]
TC38
[3]
[13]
D740PA154
4.
Protrusion width measurement For X WIDTH, Y WIDTH, and Z WIDTH measurements are performed on X-axial, Y-axial, and Z-axial protrusion widths, respectively. For IN WIDTH, the protrusion width at the inside diameter side is measured. SNo.
PTN
SPT-X
SPT-Y
SPT-Z
FPT-X
FPT-Y
1
X WIDTH
x1
y1
z1
x2
y2
SNo.
PTN
SPT-X
SPT-Y
SPT-Z
FPT-X
FPT-Y
1
IN WIDTH
x1
y1
z1
x2
y2
X WIDTH
z2
FPT-Z T LIM+ T LIM- BASE z2
t1
t2
S
FPT-Z T LIM+ T LIM- BASE z2
t1
t2
S
DIR. ←Z DIR. ←Z
IN WIDTH z2
z1
z1
x1 x2 x2
x1
x1, y1, z1: Measurement start point # x2, y2, z2: Measurement end point $ D736P0120
3-365
3
PROGRAM CREATION
[Measurement movement (X WIDTH)]
[1][2] [1] [2] [3]
TC37
[4]
[4]
[6]
K19
[5]
K19
[7]
[7] [9]
[9] [8]
[10] K19
K19
[11]
TC39
X
X
#:Start point $: End point
Y
Z
Rapid feed Approach speed (parameter K14)
D740PA155
Skip feed
Note:
The safety profile clearance back (TC40) is used for measurement at the No. 2 spindle side.
[Measurement movement (IN WIDTH)]
TC37 K19
K19
TC39
Rapid feed Approach speed (parameter K14)
[5]
[11]
[1] [2] [12]
[10] [9]
[6] [8]
[7]
Skip feed
[4] [3]
TC38
[13]
#:Start point $: End point
D740PA156
3-366
PROGRAM CREATION
5.
3
Step distance measurement For +X STEP, +Y STEP, and +Z STEP, surface level differences in the plus directions of the Xaxis, Y-axis, and Z-axis, respectively, are measured. For –X STEP, –Y STEP, and –Z STEP, surface level differences in the minus directions of the X-axis, Y-axis, and Z-axis, respectively, are measured. SNo.
PTN
SPT-X
SPT-Y
SPT-Z
FPT-X
FPT-Y
FPT-Z
1
+X STEP
x1
y1
z1
x2
y2
z2
+X STEP
T LIM+ T LIMt1
t2
BASE
DIR.
S
←Z
–X STEP z1
z1 z2
z2
x1
x1 x2
x1, y1, z1: Measurement start point # x2, y2, z2: Measurement end point $
x2
D736P0123
[Measurement movement (–X STEP)] Rapid feed
[1][2]
Approach speed (parameter K14) Skip feed
[3]
TC37
[6]
[4]
[7] [5]
K19
[8] [9] K19
X [11]
[10]
Z
TC39
D740PA157
3-367
3
PROGRAM CREATION
6.
External measurement For EXT MILL, data that has been measured using an external measuring unit is read and the measured data is incorporated into milling tool data. For EXT TURN, measured data is incorporated into turning tool data. SNo.
PTN
SPT-X
SPT-Y
SPT-Z
FPT- X
FPT-Y
1
EXT MILL
P
N
z1
◆
◆
SNo.
PTN
SPT-X
SPT-Y
SPT-Z
FPT- X
FPT-Y
1
EXT TURN
P
N
z1
◆
◆
P:
FPT-Z T LIM+ T LIM- BASE ◆
t1
t2
◆
FPT-Z T LIM+ T LIM- BASE ◆
t1
t2
◆
DIR. ◆ DIR. ◆
Select an offset item from the menu below. WEAR X
WEAR Z
TOOL DIAMETER
- For EXT MILL, COMP. DATA item on the unit line is invalid. - TOOL DIAMETER is displayed only for EXT MILL. N: Enter the number of the section to be measured using an external measuring unit. z1: Enter the target value for the section which is to be measured using an external measuring unit.
3-368
PROGRAM CREATION
3
3-29-5 Offset value and the direction of offset 1.
Outside- and inside-diameter measurement Offset value Offset value Target value
Measurement result
Target value
Measurement result
Offset value Offset value Target value
Measurement result
Target value
Measurement result D736P0125
Target value X (Y) = Starting position X (Y) Measurement result X = (Measurement point #1 – Measurement point #2) /2 – 2 × Touch sensor stylus ball radius Measurement result Y = (Measurement point #1 – Measurement point #2) – 2 × Touch sensor stylus ball radius Offset value X (Y) = Target value X (Y) – Measurement result X (Y) [Offset for outside- and inside-diameter measurement] Measuring direction Turning tool
Offset
X
Wear offset X = Wear offset X + Offset X
Y
Wear offset X = Wear offset X + Offset Y
3-369
3
PROGRAM CREATION
2.
Groove width and inner groove width measurements
Measurement result Target value
Offset value
Ending position
Measurement result
Starting position
Ending position
Target value
Offset value
Starting position
始点
Starting position as reference (BASE = 0)
Ending position as reference (BASE = 1) D736P0126
Target value X (YZ) = Starting position X (YZ) – Ending position X (YZ) Measurement result X = Measurement point #1 – Measurement point #2 + 4 × Touch sensor stylus ball radius Measurement result Y (Z) = Measurement point #1 – Measurement point #2 + 2 × Touch sensor stylus ball radius Offset value X (YZ) = Target value X (YZ) – Measurement result X (YZ) [Offset for groove width measurement]
Turning tool
Milling tool
Starting position as reference (BASE = 0)
Ending position as reference (BASE = 1)
Measuring direction
Offset
X
Wear offset X =
Wear offset X – Offset X
Wear offset X + Offset X
Y
Wear offset X =
Wear offset X – (Offset Y × 2)
Wear offset X + (Offset Y × 2)
Wear offset Z – Offset Z
Wear offset Z + Offset Z
Z
Wear offset Z =
X
Tool diameter =
Tool diameter + Offset X
Y
Tool diameter =
Tool diameter + (Offset Y × 2)
Z
Tool diameter =
Tool diameter + (Offset Z × 2)
X
Wear offset X =
Wear offset X – Offset X
Wear offset X + Offset X
Y
Wear offset Y =
Wear offset Y – Offset Y
Wear offset Y + Offset Y
Z
Wear offset Z =
Wear offset Z – Offset Z
Wear offset Z + Offset Z
3-370
PROGRAM CREATION
3.
3
Protrusion width and inner protrusion width measurements
Measurement result
Measurement result
Target value
Target value
Offset value
Ending position
Starting position
Starting position as reference (BASE = 0)
Ending position
Offset value
Starting position Ending position as reference (BASE = 1) D736P0127
Target value X (YZ) = Starting position X (YZ) – Ending position X (YZ) Measurement result X = Measurement point #1 – Measurement point #2 – 4 × Touch sensor stylus ball radius Measurement result Y (Z) = Measurement point #1 – Measurement point #2 – 2 × Touch sensor stylus ball radius Offset value X (YZ) = Target value X (YZ) – Measurement result X (YZ) [Offset for protrusion width measurement]
Turning tool
Milling tool
Measuring direction
Offset
Starting position as reference (BASE = 0)
Ending position as reference (BASE = 1)
X
Wear offset X =
Wear offset X – Offset X
Wear offset X + Offset X
Y
Wear offset X =
Wear offset X – (Offset Y × 2)
Wear offset X + (Offset Y × 2)
Wear offset Z – Offset Z
Wear offset Z + Offset Z
Z
Wear offset Z =
X
Tool diameter =
Tool diameter – Offset X
Y
Tool diameter =
Tool diameter – (Offset Y × 2)
Z
Tool diameter =
X
Wear offset X =
Wear offset X – Offset X
Tool diameter – (Offset Z × 2) Wear offset X + Offset X
Y
Wear offset Y =
Wear offset Y – Offset Y
Wear offset Y + Offset Y
Z
Wear offset Z =
Wear offset Z – Offset Z
Wear offset Z + Offset Z
3-371
3
PROGRAM CREATION
4.
Step distance measurement Excessive cutting
Insufficient cutting Measurement result
Measurement result Offset value
Target value
Target value
Ending position
Offset value
Ending position Starting position
Starting position
Starting position as reference (BASE = 0)
Ending position as reference (BASE = 1)
Insufficient cutting
Excessive cutting Measurement result Target value
Measurement result
Offset value
Target value
Offset value
Starting position
Starting position Ending position
Starting position as reference (BASE = 0)
Ending position Ending position as reference (BASE = 1) D736P0128
Target value X (YZ) = Starting position X (YZ) – Ending position X (YZ) Measurement result X (YZ) = Measurement point #1 – Measurement point #2 Offset value X (YZ) = Target value X (YZ) – Measurement result X (YZ) [Offset for step distance measurement]
Turning tool
Milling tool
The reference position is in a plus direction with respect to the other position.
The reference position is in a minus direction with respect to the other position.
Wear offset X – Offset X
Wear offset X + Offset X
Measuring direction
Offset
X
Wear offset X =
Y
Wear offset X =
Wear offset X – (Offset Y × 2)
Wear offset X + (Offset Y × 2)
Z
Wear offset Z =
Wear offset Z – Offset Z
Wear offset Z + Offset Z
X
Tool diameter =
Tool diameter – Offset X
Tool diameter + Offset X
Y
Tool diameter =
Tool diameter – (Offset Y × 2)
Tool diameter + (Offset Y × 2)
Z
Tool diameter =
Tool diameter – (Offset Z × 2)
Tool diameter + (Offset Z × 2)
X
Wear offset X =
Wear offset X – Offset X
Wear offset X + Offset X
Y
Wear offset Y =
Wear offset Y – Offset Y
Wear offset Y + Offset Y
Z
Wear offset Z =
Wear offset Z – Offset Z
Wear offset Z + Offset Z
3-372
PROGRAM CREATION
5.
3
External measurement Target value = Value specified in the workpiece measuring sequence Offset value = Target value – Measured value [Offset for remote measurement] Object of offset Turning tool
Milling tool
Offset
Wear offset X =
Wear offset X + Offset X
Wear offset Z =
Wear offset Z + Offset Z
Tool diameter =
Tool diameter + Offset value / 2
Wear offset X =
Wear offset X + Offset X
Wear offset Z =
Wear offset Z + Offset Z
3-29-6 Offset judgment Offset data that has been obtained from measurements is handled as follows: [Offset judgment conditions] Condition Offset value >
Result
Tolerance upper – Tolerance lower × K18 100
An alarm is displayed.
Tolerance upper – Tolerance lower × K18 ≥ 100 Tolerance upper – Tolerance lower Offset value ≥ × K17 100
The offset is performed.
Tolerance upper – Tolerance lower × K17 > 100 Tolerance upper – Tolerance lower × K17 Offset value > – 100
The offset is not performed.
–
–
Tolerance upper – Tolerance lower × K17 ≥ 100 Tolerance upper – Tolerance lower Offset value ≥ – × K18 100
The offset is performed.
Tolerance upper – Tolerance lower × K18 > Offset value 100
An alarm is displayed.
Parameter K17: Lower-limit value of the measurement tolerance Parameter K18: Upper-limit value of the measurement tolerance Tolerance upper/Tolerance lower: Settings in the program Offset value:
Calculated from the target value, the measurement result, and tolerance upper/tolerance lower.
3-373
3
PROGRAM CREATION
3-30 Tool Measuring Unit (TOOL MES) This unit measures tool data using TOOL EYE during automatic operation and then automatically corrects the tool wear offset value.
3-30-1 Procedure for selecting tool measuring unit (1) Procedure for selecting tool measuring unit Press the menu selector key (key located at the right of the menu keys) to display the following menu. POINT LINE FACE TURNING MANUAL MACH-ING MACH-ING MACH-ING MACH-ING PROGRAM
END
>>>
SHAPE CHECK
(2) Press the [ >>> ] menu key. The following menu will be displayed. M CODE
SUB PROGRAM
WPC MSR
WORKPICE
>>>
TOOL WORKPICE MEASURE MEASURE SHAPE
(3) Press the [TOOL MEASURE] menu key.
3-30-2 Setting the unit data UNo.
UNIT
COMPENSATE
OFS-TOOL
No.
#
INTERVAL
OUTPUT
TOOL MES
[1]
[2]
[3]
[4]
[5]
[6]
[1] COMPENSATE Select from the menu whether the measurement results are to be used to correct tool data. NO
YES
[2] OFS-TOOL Enter the name, nominal diameter (nominal size), identification code and turret number of the tool to be measured. [3] No. Enter the machining priority number. [4] # Specify the retraction position of the lower turret during measurement. [5] INTERVAL Specify the intervals at which the tool measuring unit is to be executed. [6] OUTPUT Select whether the measurement results are to be sent to external equipment. 0: No output 1: Output to a text file on the HDD 2: Output to a serial printer via an RS-232C interface Note:
Specify output items in parameter F112.
3-374
PROGRAM CREATION
3
3-30-3 Setting the sequence data 1.
Setting TOOL MES sequence data SNo.
PTN
T-LIM-X
T-LIM-Z
TOOLEYE
DIR.
1
[1]
[2]
[3]
[4]
[5]
[1] PTN Select a tool measuring pattern from the menu. TOOL EYE TOOL EYE TOOL EYE TOOL EYE #1 #2 #3 #4
Specify the following measuring directions for the TOOL EYE: #2. O.D., reverse
#1. O.D., forward
#3. I.D., forward
#4. I.D., reverse
D736P0129
[2] T-LIM-X Enter the X-axial tolerance upper-limit value. If the X-axial tolerance is not entered, X-axial measurement will not occur. [3] T-LIM-Z Enter the Z-axial tolerance upper-limit value. If the Z-axial tolerance is not entered, Z-axial measurement will not occur. [4] TOOLEYE Enter 0 to retract the TOOL EYE after execution of the measuring unit, or enter 1 if it is not to be retracted. When the noses of multiple tools are to be measured in succession, the measuring time can be minimized by entering 1, since the TOOL EYE does not need to be extended or retracted each time. However, enter 0 for the last tool whose nose is to be measured using this unit. If 1 remains entered, the next machining unit will be executed with TOOL EYE extended. [5] DIR. Select from the menu the direction (arrow) of the milling spindle head during measurement, and the approach/escape direction to be applied to the measurement. ← Z
← X
↓ Z
↓ X
→ Z
3-375
→ X
3
PROGRAM CREATION
Selection of the [ ←X ] menu key specifies the B-axis (milling spindle head) facing in the direction of the arrow (left) and the approach/escape in X-axial direction during the measurement. X ←X
↓X
←Z
↓Z
Z
D736P0107
Note:
The measurement may not be possible according to the particular type of tool. Example:
A sharply pointed cutting tool with a cutting angle less than 90 degrees
Vertical direction
Horizontal direction
Not measurable
The tip of the tool cannot be moved to the sensor section of the TOOL EYE.
Not measurable
3-30-4 Measuring patterns 1.
Tool path during TOOL EYE measurement
Tool-change position for tool measurement
TOOL EYE
(Touch sensor)
Note:
The moment that the tool-change position for tool measurement is reached, the TOOL EYE begins to advance. This must be considered when setting the parameter for tool measurement tool-change position to prevent collision between TOOL EYE and tool.
3-376 E
PRIORITY FUNCTION FOR THE SAME TOOL
4
4
PRIORITY FUNCTION FOR THE SAME TOOL The program is executed by numeric order from its head. Consequently, tool change cycle is repeated for each of the tools specified in the tool sequence. This priority function for the same tool is intended to reduce the frequency of tool change and therefore the machining time by assigning the priority number to tools developed and by performing the machining according to the numbers thus assigned. It is in the following units and tool sequences that the priority number can be specified. - Tool sequence of machining unit - Manual program machining unit (In the case of absence of a tool, the priority number cannot be specified.) - Coordinate measuring unit - Workpiece measuring unit - M-code unit
4-1
Priority Machining Order In a program containing specified priority numbers, the machining is done in the following order. Prior machining ........The priority number is specified if the necessity of machining with complete priority occurs; for example, in the case of turning roughmachining, machining with a centering drill, etc. The machining is done by numeric order of the tools with priority number (displayed in yellow). Ordinary machining .....The machining is done in the programmed order of the tools developed by the tool sequence (tools without priority number). Subsequent machining..The priority number is specified when the need for machining lastly is arises; for example, in the case of chamfering cutter. The machining is done by the numeric order of the tools with priority numbers (displayed in reversed status).
4-1
4
PRIORITY FUNCTION FOR THE SAME TOOL
Program without priority number UNo. 0
MAT. CBN STL
OD-MAX 150.
UNo.
UNIT
PART
1
FACING
FACE
ID-MIN 0.
LENGTH 73.
WORK FACE 3.
FIN-Z 0.1
SNo.
TOOL
NOM.
R 1
GENERAL OUT
25. A
F 2
GENERAL OUT
20. B
FIG
SPT-X
SPT-Z
FPT-X
1
150.
3.
0.
No.
#
◆ ◆
UNo.
UNIT
PART
CPT-X
2
BAR
OUT
150.
SNo.
TOOL
NOM.
R 1
GENERAL OUT
25. A
F 2
GENERAL OUT
20. B
PAT.
FPT-Z 0. CPT-Z 0.
No.
#
PAT. ◆ ◆
FIG
PTN
S-CNR
SPT-X
SPT-Z
FPT-X
FPT-Z
1
LIN
C 0.5
◆
◆
120.
15.
2
TPR
120.
15.
130.
35.
3
LIN
◆
◆
135.
UNo.
UNIT
MODE
POS-C
◆
DIA
◆
40.
DEPTH
CHMF
50.
5.
3
DRILLING
SNo.
TOOL
NOM-φ
1
CTR-DR
20.
10.
◆
◆
2
DRILL
10.
10.
0.
100.
99.
999.
0.
3
CHAMFER
FIG
PTN
1
ARC
UNo.
UNIT
XC
POS-B No.
#
10.
HOLE-φ
SPT-R/x. SPT-C/y. 50. MODE
4
TAPPING
SNo.
TOOL
NOM-φ
XC
1
CTR-DR
20.
2
DRILL
3
CHAMFER
◆ No.
16. NUM.
ANG
0.
3
90.
POS-C
NOM.
◆ #
PRE-DIA
SPT-Z
0 POS-B
HOLE-DEP
MAJOR-φ PITCH TAP-DEP
M16.
HOLE-φ
16
2.
HOLE-DEP
PRE-DIA ◆
10.
◆
14.2
14.2
27.
0.
99.
999.
0.
16.
16.
20.
TAP
4
TAP
FIG
PTN
1
ARC
30.
–90.
UNo.
UNIT
CONTI.
REPEAT
5
END
0
M16 SPT-R/x. SPT-C/y.
SPT-Z
NUM.
ANG
0.
3
120.
NUMBER
RETURN
SHIFT
4-2
30.
LOW RET.
PRIORITY FUNCTION FOR THE SAME TOOL
4
Program with priority number UNo. MAT. OD-MAX ID-MIN LENGTH WORK FACE 0 CBN STL 150. 0. 73. 3. UNo. UNIT PART FIN-Z 1 FACING FACE 0.1 # PAT. No. NOM. TOOL No. ◆ 1 25. A GENERAL OUT R 1 ◆ 2 20. B GENERAL OUT F 2 FIG SPT-X SPT-Z FPT-X FPT-Z 1 150. 3. 0. 0. UNo. UNIT PART CPT-X CPT-Z 2 BAR OUT 150. 0. SNo. TOOL NOM. No. # PAT. R 1 GENERAL OUT 25. A 1 ◆ F 2 GENERAL OUT 20. B 2 ◆ FIG PTN S-CNR SPT-X SPT-Z FPT-X FPT-Z 1 LIN C 0.5 ◆ ◆ 120. 15. 2 TPR 120. 15. 130. 35. 3 LIN ◆ ◆ 135. 40. UNo. UNIT MODE POS-B POS-C DIA DEPTH CHMF 3 DRILLING XC ◆ ◆ 10. 50. 5. SNo. TOOL NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA 1 CTR-DR 20. 3 10. ◆ ◆ 2 DRILL 10. 10. 0. 100. 3 CHAMFER 99. 1 999. 0. 16. FIG PTN SPT-R/x. SPT-C/y. SPT-Z NUM. ANG 1 ARC 50. 0 0. 3 90. UNo. UNIT MODE POS-B POS-C NOM. MAJOR-φ PITCH TAP-DEP 4 TAPPING XC ◆ ◆ M16. 16. 2. 30. NOM-φ No. # TOOL HOLE-DEP PRE-DIA SNo. HOLE-φ 3 20. ◆ CTR-DR ◆ 1 10. 14.2 0. DRILL 27. 2 14.2 99. 16. CHAMFER 0. 3 1 999. M16 TAP TAP 20. 4 16. FIG PTN SPT-R/x. SPT-C/y. SPT-Z NUM. ANG 1 ARC 30. –90. 0. 3 120. UNo. UNIT CONTI. REPEAT SHIFT NUMBER RETURN LOW RET. 5 END 0
Prior machining priority number
Subsequent machining priority number
If one reclassifies these two programs by machining order, the following tables are obtained. Program without priority number UNo.
SNo.
Tool
1
1
GENERAL OUT 25 A
Program with priority number Tool change
UNo.
SNo.
Tool
○
1
1
GENERAL OUT 25 A
2
1
GENERAL OUT 25 A
1
2
GENERAL OUT 20 B
○
2
1
GENERAL OUT 25 A
○
1
2
GENERAL OUT 20 B
2
2
GENERAL OUT 20 B
○
2
2
GENERAL OUT 20 B
3
1
CTR-DR 20
○
3
2
DRILL 10
○
3
3
CHAMFER 99
4
1
4
2
4 4
Tool change ○
○
3
1
CTR-DR 20
4
1
CTR-DR 20
○
3
2
DRILL 10
○
CTR-DR 20
○
4
2
DRILL 14.2
○
DRILL 14.2
○
4
4
TAP M16
○
3
CHAMFER 99
○
3
3
CHAMFER 99
4
TAP M16
○
4
4
CHAMFER 99
11 times
4-3
○ 7 times
○
4
PRIORITY FUNCTION FOR THE SAME TOOL
Without a specified priority number, the machining is done by the programmed order and the tool change cycle is executed for each tool. Consequently, in this example, the tool change cycle is executed 11 times. By specifying the priority number, two machinings of the same type are done at the same time by the same tool, which permits reducing the number of tool change cycles to 7. Note 1: If a different priority number is assigned to the same tool, the machining is done in the order of the priority number. Note 2: When the priority number is assigned to all the tools of the same process, the M-code unit without a priority number is executed once for extra between the prior machining and the subsequent machining.
4-2
Priority Machining Zone The priority machining zone for the same tool is delimited by the following units. The zone delimited by these units is called process. In the case of different processes, it is possible to specify the same priority number for a different tool. - Process end unit - Workpiece transfer unit - Head selection unit - End unit (if WORK No. is specified)
4-4
PRIORITY FUNCTION FOR THE SAME TOOL
Example:
Process1
Process 2
Case where the process end unit has been programmed. If the program is executed which contains the priority numbers specified for GENERAL, CTR-DR and CHAMFER, the machining is done in the following order.
UNo.
MAT.
OD-MAX
ID-MIN
LENGTH
WORK FACE
0
CBN STL
150.
0.
73.
3.
UNo.
UNIT
PART
1
FACING
FACE
FIN-Z 0.1
SNo.
TOOL
NOM.
No.
R 1
GENERAL OUT
25. A
1
◆
F 2
GENERAL OUT
20. B
2
◆
#
PAT.
FIG
SPT-X
SPT-Z
FPT-X
1
150.
3.
0.
0.
UNo.
UNIT
PART
CPT-X
CPT-Z
2
BAR
OUT
150.
0.
SNo.
TOOL
NOM.
No.
R 1
GENERAL OUT
25. A
1
F 2
GENERAL OUT
20. B
2
FPT-Z
#
Priority number for prior machining: 1, 2, 3
PAT. ◆ ◆
FIG
PTN
S-CNR
SPT-X
SPT-Z
FPT-X
FPT-Z
1
LIN
C 0.5
◆
◆
120.
15.
2
TPR
120.
15.
130.
35.
3
LIN
◆
◆
135.
UNo.
UNIT
MODE
POS-B
POS-C
DIA
DEPTH
CHMF
3
DRILLING
XC
◆
◆
10.
50.
5.
#
HOLE-φ
HOLE-DEP
10.
◆
◆
10.
0.
100.
999.
0.
SNo.
TOOL
NOM-φ
No.
1
CTR-DR
20.
3
2
DRILL
10.
3
CHAMFER
FIG
PTN
SPT-R/x.
SPT-C/y.
SPT-Z
50.
0
0.
1
ARC
UNo.
UNIT
4
PROC END
1
99.
UNIT
MODE
POS-B
POS-C
NOM.
5
TAPPING
XC
◆
◆
M16.
SNo.
TOOL
1
CTR-DR
2
DRILL
3
CHAMFER
No.
20.
#
HOLE-φ
3
14.2 99.
1
Priority number for subsequent machining 1
PRE-DIA
16. NUM. ANG 3
UNo.
NOM-φ
40.
90.
MAJOR-φ PITCH TAP-DEP 16.
2.
30.
HOLE-DEP
PRE-DIA
10.
◆
◆
14.2
27.
0.
0.
16.
999.
4
TAP
FIG
PTN
SPT-R/x.
SPT-C/y.
SPT-Z
NUM.
ANG
1
ARC
30.
-90.
0.
3
120.
UNo.
UNIT
CONTI.
6
END
0
16.
M16
REPEAT
20.
SHIFT
TAP
NUMBER
RETURN
LOW RET.
GENERAL OUT No. 1
Process 1
GENERAL OUT No. 2
DRILL No. CHAMFER No. 1
CTR-DR No. 3 PROC END
CTR-DR No. 3
Process 2
4
DRILL No.
CHAMFER No. 1
TAP No. END
4-5
4
PRIORITY FUNCTION FOR THE SAME TOOL
4-3 4-3-1
Editing Function and Input Method of Priority Numbers Input of priority numbers The priority number is of two types: for prior machining and for subsequent machining, it is entered by means of menu keys and numeric keys. The priority number is entered in ascending order of the tool sequence. (1) In creating mode, move the cursor to the item No. UNo.
UNIT
PART
2
BAR
OUT
SNo.
TOOL
NOM.
1
GENERAL OUT
25.A
!
No.
#
PAT.
The message ACHINING PRIORITY No.? is displayed and the menu changes as follows. MACHINING PRIORITY No.? DELAY PRIORITY
PRI. No. PRI. No. CHANGE ASSIGN
PRI. No. SUB PROG ALL ERAS PROC END
(2) Enter the priority number. There are the three following entry methods (refer to Note 1 to 3 below): Prior machining priority number To be set by means of numeric keys. ! The number is displayed in yellow. Subsequent machining priority number 1) Press the [DELAY PRIORITY] menu key. ! The display of [DELAY PRIORITY] is reversed. 2) Set the subsequent machining priority number by means of numeric keys. ! The priority number is displayed in reversed status. Without entry (ordinary machining) The priority number is not entered. Move the cursor to the following article. ! When the priority number is entered, the cursor moves to the following article. SNo.
TOOL
NOM.
No.
1
GENERAL OUT
25.A
1
#
PAT.
Note 1: The prior machining and subsequent machining can receive a priority number from 1 to 99, respectively. Moreover, it is not always necessary to mark the priority of the sequence numbers. Note 2: It is possible to assign the same priority number or a different priority number to the same tool, but it is impossible to assign the same priority number to different tools; this will cause the alarm 420 SAME DATA EXISTS to display. Note 3: In order to cancel a priority number after it has been entered, move the cursor to the position concerned and press the data cancellation key
4-6
.
PRIORITY FUNCTION FOR THE SAME TOOL
4-3-2
4
Assignment of priority numbers This function is used to make the assignment of priority numbers entered for all the identical tools in the same process. Note:
This function is only useful for a program in the process of editing.
Menu selection: [PRI. No. ASSIGN] ( → [DELAY PRIORITY]) (1) In creating mode, move the cursor to the item No. UNo.
UNIT
PART
2
BAR
OUT
SNo.
TOOL
NOM.
1
GENERAL OUT
25.A
No.
#
PAT.
'← Cursor
(2) Press the [PRI. No. ASSIGN] menu key. !
The display of [PRI. No. ASSIGN] is reversed and the message MACHINING PRIORITY No.? is displayed in the message zone of the display.
(3) Enter the priority number by means of numeric keys. Example:
Entry of 2 2
Press the following keys:
INPUT
- For subsequent machining, enter the intended number after having pressed the [DELAY PRIORITY] menu key. Note: !
If the data cancellation key is pressed, all the priority numbers for the identical tools in the process will be erased. The same priority number is assigned to all the identical tools in the process and the cursor moves to the following article.
SNo.
TOOL
NOM.
No.
#
1
GENERAL OUT
25.A
2
'
UNo.
UNIT
PART
#
3
BAR
OUT
SNo.
TOOL
NOM.
No.
1
GENERAL OUT
25.A
2
Note:
PAT.
PAT.
Regardless of whether the priority number is entered or not, all the identical tools in the process are marked with the same priority number.
4-7
4
PRIORITY FUNCTION FOR THE SAME TOOL
4-3-3
Change of priority numbers This function is used for changing the priority number entered for all the identical tools in a process. Note:
This function is only useful for a program in the process of editing.
Menu selection: [PRI. No. CHANGE] ( → [DELAY PRIORITY]) (1) In creating mode, move the cursor to the item No. UNo.
UNIT
PART
2
BAR
OUT
SNo.
TOOL
NOM.
1
GENERAL OUT
25.A
No.
#
PAT.
'← Cursor
(2) Press the [PRI. No. CHANGE] menu key. !
The display of [PRI. No. CHANGE] is reversed and the message MACHINING PRIORITY No.? is displayed in the message zone of the display.
(3) Enter the priority number by using numeric keys. Example:
Entry of 5 5
Press the following keys:
INPUT
- For subsequent machining, press the [DELAY PRIORITY] menu key, and then enter the intended number. Note: !
If the data cancellation key is pressed, all the priority numbers for the identical tools in the process will be erased. The same priority number is assigned to all the identical tools in the process and the cursor moves to the next item.
SNo.
TOOL
NOM.
No.
#
1
GENERAL OUT
25.A
5
'
UNo.
UNIT
PART
#
3
BAR
OUT
SNo.
TOOL
NOM.
No.
1
GENERAL OUT
25.A
5
Note:
PAT.
PAT.
Regardless of whether the priority number is entered or not, the same priority number is assigned to all the identical tools in the process.
4-8
PRIORITY FUNCTION FOR THE SAME TOOL
4-3-4
4
Deletion of all the priority numbers This function is used for deleting all the priority numbers contained in the process or in the program. Note:
This function is only useful for a program in the process of editing.
Menu selection: [PRI. No. ALL ERAS] (1) In creating mode, move the cursor to the item No. UNo.
UNIT
PART
2
BAR
OUT
SNo.
TOOL
NOM.
1
GENERAL OUT
25.A
No.
#
PAT.
'← Cursor
(2) Press the [PRI No. ALL ERAS] menu key. !
The display of [PRI. No. ALL ERAS] is reversed and the message ALL ERASE ? is displayed in the message zone of the screen.
(3) By means of numeric keys, specify the zones to be deleted. - Enter 1 to delete all the priority numbers contained in the program. - Enter 0 to delete all the priority numbers contained in a process where the cursor is located. Example:
Deletion of all the priority numbers contained in a program 1
Press the following keys: !
4-3-5
INPUT
.
All the priority numbers in the specified zone are deleted.
SNo.
TOOL
NOM.
1
GENERAL OUT
25.A
UNo.
UNIT
PART
3
BAR
OUT
SNo.
TOOL
NOM.
1
GENERAL OUT
25.A
No.
#
PAT.
'
No.
#
PAT.
How to use the SUB PROG PROC END function When the priority number has been edited in the main program, it is necessary to perform the same editing for the subprogram. If in the process constituting the subject of the editing, there is a subprogram containing a process delimitation unit (process end unit), press the [SUB PROG PROC END] menu key in order to invert the display, which has the result that the subprogram is treated the same as the process end unit. (See Fig. 4-1.)
4-9
4
PRIORITY FUNCTION FOR THE SAME TOOL
SUB PROG PROC END
SUB PROG PROC END
Menu display normal
Menu display reversed
Process
(Main program)
[1]
(1)
Process (1)
Process [4] (2)
UNo. 0 UNo. 1 SNo. R 1 F 2 FIG 1 UNo. 2 SNo. R 1 F 2 FIG 1 2 3 UNo. 3 UNo. 4 SNo. 1 2 3 FIG 1 UNo. 5
MAT. OD-MAX ID-MIN LENGTH WORK FACE CBN STL 150. 0. 73. 3. UNIT PART FIN-Z FACING FACE 0.1 No. # PAT. NOM. TOOL ◆ 25. A GENERAL OUT ◆ 20. B GENERAL OUT SPT-X SPT-Z FPT-X FPT-Z 150. 3. 0. 0. UNIT PART CPT-X CPT-Z BAR OUT 150. 0. No. # PAT. NOM. TOOL ◆ 25. A GENERAL OUT ◆ 20. B GENERAL OUT FPT-Z FPT-X S-CNR SPT-X SPT-Z PTN 15. 120. ◆ C 0.5 ◆ LIN 35. 130. 15. 120. TPR 40. 135. ◆ ◆ LIN
[2]
Subprogram UNIT MODE POS-B POS-C DIA DEPTH CHMF DRILLING XC ◆ ◆ 10. 50. 5. NOM-φ No. # HOLE-DEP PRE-DIA TOOL HOLE-φ ◆ ◆ CTR-DR 10. 20. 100. 0. DRILL 10. 10. 16. 0. CHAMFER 999. 99. PTN SPT-R/x. SPT-C/y. SPT-Z NUM. ANG ARC 50. 0. 0. 3 90. UNIT CONTI. REPEAT SHIFT NUMBER RETURN LOW RET. END 0
[3]
(Subprogram)
[2]
[3]
Fig. 4-1
UNo. 1 SNo. 1 2 FIG 1 UNo. 2 UNo. 3 SNo. 1 2 3 4 FIG 1 UNo. 4
UNIT MODE POS-B POS-C DIA DEPTH CHMF DRILLING XC ◆ ◆ 10. 50. 0. No. # HOLE-φ HOLE-DEP PRE-DIA NOM-φ TOOL ◆ ◆ 10. 20. CTR-DR 100. 0. 10. 10. DRILL PTN SPT-R/x. SPT-C/y. SPT-Z NUM. ANG ARC 50. 0. 0. 3 90. PROC END UNIT TAPPING TOOL CTR-DR DRILL CHAMFER TAP PTN ARC UNIT END
MODE POS-B POS-C NOM. MAJOR-φ PITCH TAP-DEP XC ◆ ◆ M16. 16 2. 30. No. # HOLE-φ HOLE-DEP PRE-DIA NOM-φ ◆ ◆ 10. 20. 0. 27. 14.2 14.2 16. 0. 999. 99. TAP 20. 16. M16 SPT-R/x. SPT-C/y. SPT-Z NUM. ANG 30. -90. 0. 3 120. CONTI. REPEAT SHIFT NUMBER RETURN LOW RET. 0
Subprogram unit = process end unit
Remark 1: The editing function zone can be divided by the subprogram unit. Even if the editing function is executed in delimited zone [1], this has no effect in the zone [2], [3] and [4]. Remark 2: Display of [SUB PROG PROC END] is reversed: Two processes (1) and (2) Display of [SUB PROG PROC END[ is not reversed: One process (1)
4-10
PRIORITY FUNCTION FOR THE SAME TOOL
4-4
4
Relation between the Subprogram Unit and the Priority Machining Function If one program contains a subprogram unit and the priority function for the same tool, the machining order is as mentioned below. Example:
Entry of priority number for GENERAL, CTR-DR and CHAMFER UNo.
Machining order
GENERAL OUT 25A GENERAL OUT 20B GENERAL OUT 25A GENERAL OUT 20B
Subprogram
CTR-DR 20
DRILL 14.2
CHAMFER 99
CTR-DR 20
TAP M16
DRILL 10
S CHAMFER 99
END
0 UNo. 1 SNo. R 1 F 2 FIG 1 UNo. 2 SNo. R 1 F 2 FIG 1 2 3 UNo. 3
MAT.
OD-MAX
ID-MIN
LENGTH
WORK FACE
CBN STL 150. 0. 73. 3. UNIT PART FIN-Z FACING FACE 0.1 # PAT. No. NOM. TOOL ◆ 1 25. A GENERAL OUT ◆ 2 20. B GENERAL OUT SPT-X SPT-Z FPT-X FPT-Z 150. 3. 0. 0. UNIT PART CPT-X CPT-Z BAR OUT 150. 0. # PAT. No. NOM. TOOL ◆ 1 25. A GENERAL OUT ◆ 2 20. B GENERAL OUT FPT-Z FPT-X S-CNR SPT-X SPT-Z PTN 15. 120. ◆ C 0.5 ◆ LIN 35. 130. 15. 120. TPR 40. 135. ◆ ◆ LIN Subprogram
UNo. 4 SNo. 1 2 3 FIG 1 UNo. 5
UNIT MODE POS-B POS-C DIA DEPTH CHMF DRILLING XC ◆ ◆ 10. 50. 5. NOM-φ No. # HOLE-DEP PRE-DIA TOOL HOLE-φ ◆ ◆ CTR-DR 3 10. 20. 100. 0. DRILL 10. 10. 16. 0. CHAMFER 999. 99. 1 PTN SPT-R/x. SPT-C/y. SPT-Z NUM. ANG ARC 50. 0. 0. 3 90. UNIT CONTI. REPEAT SHIFT NUMBER RETURN LOW RET. END 0 Priority number Prior: 1, 2, 3 Subsequent: 1 (Subprogram) UNo. 3 SNo. 1 2 3 4 FIG 1 UNo. 4
UNIT TAPPING TOOL CTR-DR DRILL CHAMFER TAP PTN ARC UNIT END
MODE POS-B POS-C NOM. MAJOR-φ PITCH TAP-DEP XC ◆ ◆ M16. 16 2. 30. No. PRE-DIA NOM-φ # HOLE-φ HOLE-DEP 3 ◆ 20. ◆ 10. 0. 14.2 27. 14.2 16. 99. 0. 999. 1 TAP M16 20. 16. SPT-R/x. SPT-C/y. SPT-Z NUM. ANG 30. -90. 0. 3 120. CONTI. REPEAT SHIFT NUMBER RETURN LOW RET. 0
In the process of priority machining search, the subprogram unit is executed as follows: - In the case where subprogram is a MAZATROL program, the subprogram unit is always executed. (The machinings specified in the subprogram are executed in the numeric order of the priority numbers.) - In the case where subprogram is an EIA/ISO program, the subprogram unit is only executed once at the time of ordinary machining.
4-11
4
PRIORITY FUNCTION FOR THE SAME TOOL
4-5
Relation between the M-Code Unit and the Priority Machining Function The machining order differs as follows, according to whether the M-code unit contains the priority code for the same tool or not. UNo. Without priority No.
M
M
M
END In the process of the search for the priority No., the M-code unit is executed each time it is read.
With priority No.
M
END The M-code unit is executed only once in conformity with the priority No.
0 UNo. 1 SNo. R 1 F 2 FIG 1 UNo. 3 UNo. 2 SNo. R 1 F 2 FIG 1 2 3 UNo. 4 SNo. 1 2 3 FIG 1 UNo. 5
MAT.
OD-MAX
ID-MIN
LENGTH
WORK FACE
CBN STL 150. 0. 73. 3. UNIT PART FIN-Z FACING FACE 0.1 # PAT. No. NOM. TOOL ◆ 1 25. A GENERAL OUT ◆ 2 20. B GENERAL OUT SPT-X SPT-Z FPT-X FPT-Z 150. 3. 0. 0. UNIT M-code unit M-CODE UNIT PART CPT-X CPT-Z BAR OUT 150. 0. # PAT. No. NOM. TOOL ◆ 1 25. A GENERAL OUT ◆ 2 20. B GENERAL OUT FPT-Z FPT-X S-CNR SPT-X SPT-Z PTN 15. 120. ◆ C 0.5 ◆ LIN 35. 130. 15. 120. TPR 40. 135. ◆ ◆ LIN UNIT MODE POS-B POS-C DIA DEPTH CHMF DRILLING XC ◆ ◆ 10. 50. 5. NOM-φ No. # HOLE-DEP PRE-DIA TOOL HOLE-φ ◆ ◆ CTR-DR 10. 20. 100. 0. DRILL 10. 10. 16. 0. CHAMFER 999. 99. PTN SPT-R/x. SPT-C/y. SPT-Z NUM. ANG ARC 50. 0 0. 3 90. UNIT CONTI. REPEAT SHIFT NUMBER RETURN LOW RET. END 0
4-12 E
LOWER-TURRET CONTROL FUNCTIONS
5
5
LOWER-TURRET CONTROL FUNCTIONS This chapter describes the programming methods that use the lower turret (turret 2) mounted under twin-turret machine specifications.
5-1
Machining with the Lower Turret There are four types of machining which uses the lower turret: independent machining with the lower turret, simultaneous machining with the upper and lower turrets, balanced cutting with the upper and lower turrets, and simultaneous machining of processes 1 and 2 with the upper and lower turrets.
5-1-1
Independent machining with the lower turret
D737P0004
To execute machining that uses only the lower turret, select one of the tools mounted in the lower turret and then specify turret 2 (marked “ ”). UNo.
MAT.
0
CST IRN
UNo. 1
UNIT BAR
SNo.
TOOL
OD-MAX ID-MIN LENGTH WORK FACE 100.
0.
40.
1 UNo.
CPT-Z
FIN-X
FIN-Z
OUT
90
100.
0.
0.2
0.2
NOM. No. #
2
S-CNR
PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP 0
END
!
5.
! SPT-X
CONTI. REPEAT
LTUR DIA
2000
CPT-X
LIN UNIT
0.
POS-B
F 2 GENERAL OUT 30. PTN
RPM
PART
R 1 GENERAL OUT 45. A FIG
ATC MODE
!
!
!
!
SPT-Z
FPT-X
FPT-Z
!
80. NUMBER
!
120
0.
0.
196
F-CNR/$
55. RETURN
!
M M M
0.1
R/th
RGH
!
4
LOW RET. WORK No.
: Identification mark for the lower turret
FR 0.45
EXECUTE !
The above program is intended to perform the UNo. 1 – SNo. R1 process as roughing with the upper turret (turret 1) and then perform the UNo. 1 – SNo. F2 process as finishing with the lower turret (turret 2).
5-1
5
LOWER-TURRET CONTROL FUNCTIONS
5-1-2
Simultaneous machining with the upper and lower turrets
D737P0005
In the simultaneous machining unit both the upper and lower turrets are used at the same time. This unit is valid only for the BAR, CPY, CORNER, FACING, and T. GROOVE unit. 1.
Specification of the simultaneous machining unit To set the simultaneous machining unit, it is necessary first to specify the turning spindle speed for simultaneous machining. While simultaneous machining is in progress, the turning spindle speed is kept constant and surface speed constant control does not work. Since multiple sets of simultaneous machining may occur, it is also necessary to specify the simultaneous machining group number to identify those sets of simultaneous machining. Specify the above two values in the simultaneous machining unit. UNo. 0 UNo. 1
MAT. CST IRN UNIT SIMULTAN
OD-MAX
ID-MIN
100.
0.
No.
LENGTH WORK FACE 40.
ATC MODE
0.
SIMUL.No.
RPM
50
2000
RPM
LTUR DIA
2000
Machining identified by simultaneous machining group number 50 occurs at a speed of 2000 min–1. When a machining priority number is assigned, all processes assigned the simultaneous machining group number (in this example, 50) will be conducted in the order specified by the machining priority number.
5-2
LOWER-TURRET CONTROL FUNCTIONS
2.
5
Specification in the turning units Specify the turrets to be used for each turning unit, and the respective simultaneous machining group numbers. UNo. 0 UNo. 1 UNo. 2
MAT.
OD-MAX
CST IRN
No.
SIMULTAN UNIT
PTN
CPT-Z
FIN-X
FIN-Z
0.
0.2
0.2
NOM. No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP
S-CNR
3
T.GROOVE
2000 100.
LIN UNIT
2000
90
TOOL
LTUR DIA
RPM Specify the simultaneous machining group number and the turret.
OUT
BAR
UNo.
TOOL
F 1 GROOVE OUT 1
0.
RPM
CPT-X
30.E
FIG
40.
SIMUL.No. 50
F 2 GENERAL OUT
SNo.
0.
ATC MODE
POS-B
45.A
1
WORK FACE
PART
R 1 GENERAL OUT FIG
LENGTH
100.
UNIT
SNo.
ID-MIN
5.
!
!
!
!
!
0.45
!
!
!
!
0.
0.
196
0.1
SPT-X
SPT-Z
FPT-X
FPT-Z
!
!
80.
55.
POS-B
PAT.
No.
OUT
90
0
1
F-CNR/$
R/th
RGH
!
4
50
!
2.
M M M
PITCH WIDTH FINISH 0
10.
!
NOM. No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP 10.
FR
0
PART
S-CNR C 1.
50
!
!
!
SPT-X
SPT-Z
FPT-X
FPT-Z
F-CNR
100.
70.
90.
70.
C 1.
! ANG
!
FR
M M M
0.1 RGH
The above program is intended to perform simultaneously the UNo. 2 – SNo. R1 process as bar materials O.D. roughing with the upper turret (turret 1) and the UNo. 3 – SNo. F1 process as grooving with the lower turret (turret 2) and then perform the UNo. 2 – SNo. F2 process as finishing with the upper turret.
5-3
5
LOWER-TURRET CONTROL FUNCTIONS
3.
Example of multiple sets of simultaneous machining Multiple sets of simultaneous machining can be performed using multiple simultaneous machining units. A sample program is shown below. UNo. 0 UNo. 1 UNo. 2
MAT.
OD-MAX
ID-MIN
LENGTH
100.
20.
100.
CST IRN UNIT
No.
BAR
SNo.
ATC MODE
RPM
1.
SIMUL.No.
RPM
50
2000
SIMULTAN UNIT
WORK FACE
2000
PART
POS-B
CPT-X
CPT-Z
FIN-X
FIN-Z
OUT
90
100.
0.
0.2
0.2
TOOL
NOM. No. #
LTUR DIA
PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP
R 1 GENERAL OUT 45.A
50
0
5.
!
!
!
!
!
F 2 GENERAL OUT 30.E
50
!
!
!
!
0.
0.
196
FIG 1
PTN
S-CNR
SPT-X
SPT-Z
FPT-X
FPT-Z
!
!
80.
55.
LIN
UNo.
UNIT
3
T.GROOVE
SNo.
PART NOM. No.
UNo. 4
No.
90
0
1
#
F 1 GROOVE OUT 10.
!
0.
!
SPT-Z
FPT-X
FPT-Z
F-CNR
70.
90.
70.
C 1.
PART
POS-B
FIN-Z
FACE
90
0
NOM. No.
#
R 1 GENERAL EDGE 10.
4
!
100.
UNIT TOOL
RGH
! !
10.
!
2.
FACING
SNo.
R/th
PITCH WIDTH FINISH
SPT-X
C 1.
!
FR
!
ANG
!
!
0.2
!
!
!
RGH
FR
!
SPT-X
SPT-Z
FPT-X
FPT-Z
RGH
1
80.
1.
20.
0.
4
MODE
POS-B
POS-C
DIA
DEPTH
CHMF
ZC
!
!
5.
20.
0.
UNIT
5
DRILLING
SNo.
TOOL
1 FIG 1 UNo. 6
NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP
DRILL
5.
PTN
SPT-R/x
SPT-C/y
50.
0.
ARC
5.
UNIT
No.
20.
PCK1 T
SPT-Z
SPT-Y
NUM.
ANGLE
Q
R
90.
0.
4
90.
0
1
RPM
70
1500
UNo.
UNIT
PART
POS-B
CPT-X
CPT-Z
7
CORNER
OUT
90
0.2
0.2
SNo.
TOOL
NOM. No.
R 1 GENERAL OUT 50. F
#
0
5.
!
!
!
!
70
FIG
SPT-X
SPT-Z
FPT-X
FPT-Z
1
70.
20.
90.
10.
8
UNIT BAR
SNo.
TOOL
1 UNo. 9
PTN
!
!
0.
0.
196
F-CNR/$
CPT-X
CPT-Z
FIN-X
FIN-Z
0
20.
0.
0.2
0.2
S-CNR
LIN UNIT
!
POS-B
F 1 GENERAL IN 15.A FIG
!
IN
#
CONTI.
25
!
PART NOM. No.
2.5
FR
FR
!
!
!
!
SPT-X
SPT-Z
FPT-X
FPT-Z
!
!
30.
10.
REPEAT
NUMBER
0.
F-CNR/$
RETURN LOW RET.
0.2
RGH
0. R/th !
WORK No.
FR
196
0.1 RGH 4
EXECUTE ◆
END
5-4
M M M
0.45
PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP
70
M M M
0.089
PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP
F 2 GENERAL OUT 50.
UNo.
DEPTH C-SP
100
SIMUL.No.
SIMULTAN
RGH
0.
M M M
0.1
FIG UNo.
M M M
0.1
PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP
50
M M M
0.1
PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP
50
S-CNR
1
PAT.
OUT
TOOL
FIG
POS-B
F-CNR/$
FR 0.45
M M M
LOWER-TURRET CONTROL FUNCTIONS
For the above machining program, the timing chart is as follows: Upper turret (turret 1)
Lower turret (turret 2)
UNo. 2 BAR
R1
UNo. 2 BAR
F2
UNo. 3 T. GROOVE SIMUL. No. 50 UNo. 4 FACING
Waiting UNo. 5 DRILLING
Waiting UNo. 8 BAR
UNo. 7 CORNER
R1
F1 SIMUL. No. 70
R1 Waiting
Waiting
UNo. 7 CORNER
F2
The above machining sequence can be edited on the PROCESS LAYOUT display.
5-5
5
5
LOWER-TURRET CONTROL FUNCTIONS
5-1-3
Balanced cutting with the upper and lower turrets
D737P0006
The same shape can be created using both the upper and lower turrets at the same time. This is referred to as balanced cutting and can be used in the BAR, CPY, and CORNER unit. The loads on the tools can be reduced to half by causing the upper and lower turrets to act exactly the same. Thus, the feed rate can be increased by a factor of two. 1.
Programming method UNo. 2
UNIT BAR
SNo.
TOOL
PART
POS-B
CPT-X
CPT-Z
FIN-X
FIN-Z
OUT
90
100.
45.
0.2
0.2
NOM. No. # PAT. DEP-1 DEP-2/NUM.
R 1 GENERAL OUT 50. C
'
F 2 GENERAL OUT 50. A
DEP-3 FIN-X FIN-Z
C-SP
FR
0
5.
!
!
!
!
120
0.45
!
!
!
!
0.
0.
196
0.2
M M M
Move the cursor to the simultaneous machining number input column of the tool sequence data. Pressing the [BALANCE FEED 2] menu key first and then the enter key adds a lower-turret tool sequence for balanced cutting. UNo. 2 SNo.
UNIT BAR TOOL
PART
POS-B
CPT-X
CPT-Z
FIN-X
FIN-Z
OUT
90
100.
45.
0.2
0.2
NOM.
No.# PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP
R 1 GENERAL OUT 50. C
B2
R 2 GENERAL
B2
F 3 GENERAL OUT 50. A
0 !
!
!
FR
5.
!
!
!
!
!
!
!
!
!
!
!
!
0.
0.
196
0.2
120
M M M
0.45
- B2 means balanced cutting at twice a normal cutting feed rate. - Since balanced cutting at twice a normal cutting feed rate has been specified, actual machining operates at twice the feed rate specified in the program. The feed rate in the above example is 0.45 × 2 = 0.9 mm/rev. - Balanced cutting can be specified for the machining portion (PART) OUT and OUT of the roughing process of the BAR, CPY, and CORNER unit.
5-6
LOWER-TURRET CONTROL FUNCTIONS
5-1-4
5
Simultaneous machining of processes 1 and 2, using the upper and lower turrets (optional) The use of the two-workpiece machining unit (2 WORKPC) allows machining in processes 1 and 2 to be performed simultaneously.
D740PA063
1.
Flow of processes 1 and 2 simultaneous machining program For simultaneous machining of processes 1 and 2, you need to set up the workpiece transfer unit before setting up the two-workpiece machining unit. Then, set up the two-workpiece machining unit (START), machining on the No. 1 spindle side, machining on the No. 2 spindle side, and two-workpiece machining unit (END). Common unit
#
(Removing the workpiece from the No. 2 spindle)
TRANSFER unit (HEAD: 1 → 2)
#
(Mounting a workpiece in the No. 1 spindle
2 WORKPC unit
(START)
# Machining unit for the No. 1 spindle
# Machining unit for the No. 2 spindle
# 2 WORKPC unit
(END)
# END unit
2.
(CONTI.: 1)
Setting data in the 2 WORKPC unit UNo.
UNIT
PAT.
SP1/SP2
∗
2 WORKPC
[1]
[2]
[1] PAT. Specify START when starting simultaneous machining of processes 1 and 2, and specify END when stopping it. Note 1: If END is specified before START, the alarm DBL SPDL OPER UNIT ERROR is issued. Note 2: If START is specified again between START and END, the alarm DBL SPDL OPER UNIT ERROR is issued.
5-7
5
LOWER-TURRET CONTROL FUNCTIONS
[2] SP1/SP2 When using the upper turret for machining on the No. 1 spindle side and the lower turret for marching on the No. 2 spindle side, select HI/LOW. When using the upper turret for machining on the No. 2 spindle side and the lower turret for marching on the No.1 spindle side, select LOW/HI. 3.
Example of program Here is an example of a program for the machining of 10 workpieces that need to be machined in two processes each.
UNo. 0 UNo. 1
MAT.
OD-MAX
ID-MIN
LENGTH
WORK FACE
100.
0.
80.
0.
CST IRN
PAT.
HEAD
TRANSFER CHUCK
UNIT
1→2
UNo.
UNIT
No.
SPDL PUSH CHUCK 4
M1
M2
M3
2
M-CODE
UNo.
UNIT
PAT.
SP1/SP2
3
2 WORKPC
START
HI/LOW
UNo.
UNIT
M4
RPM
W2 Z-OFFSET C1
-950
0
750
M5
M6
M7
0 M8
No.
M1
M2
M3
M4
M5
M6
M7
UNIT
TYPE
HEAD
SPDL
5
HEAD
SIN
1
!
UNo.
UNIT
PART
POS-B
CPT-X
CPT-Z
FIN-X
FIN-Z
OUT
90
100.
0.
0.2
0.2
TOOL
NOM. No. #
PAT. DEP-1 DEP-2/NUM.
R 1 GENERAL OUT 45.A
0
5.
F 2 GENERAL OUT 30.E
!
!
1 UNo. 7
S-CNR
LIN UNIT HEAD
8
DRILLING
SNo.
TOOL
1
10
Note:
M
M
M
0.
196
! 30.
2
!
0. F-CNR/$
MODE
POS-B
POS-C
DIA
DEPTH
CHMF
XC
!
!
5.
20.
0.
0.
END
M
0.45
80. SPDL
SPT-C/y
UNIT
M
FR
!
!
50.
UNo.
M
C-SP
!
HEAD
SPT-R/x
UNIT
M12
!
!
PTN
2 WORKPC
101 M12
M11
FIN-Z
FPT-Z
5.
9
M10
!
FPT-X
DRILL
UNo.
M9
FIN-X
NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP
ARC
M11
!
SPT-Z
SIN
UNIT
FIG
M10
DEP-3
!
SPT-X
TYPE
UNo.
1
TNo.
-450
0
BAR
PTN
0
M9
M8
M-CODE
FIG
0
Set START/END in the 2 WORKPC unit.
4
SNo.
C2 C-OFFSET LTUR ESC
0
UNo.
6
LTUR DIA
2000
W1
!
1
ATC MODE
5.
PAT. END
0.1
R/th
RGH
!
4
RGH
DEPTH
C-SP
FR
0.
100
PCK1 T
2.5
25
0.089
SPT-Z
SPT-Y
NUM.
ANGLE
Q
R
30.
0.
4
90.
0
1
20.
SP1/SP2 !
CONTI.
REPEAT
1
11
NUMBER
RETURN LOW RET.
WORK No.
EXECUTE ◆
Air cutting occurs in the No. 2 spindle when machining the first workpiece, and in the No. 1 spindle when machining the last workpiece.
5-8
LOWER-TURRET CONTROL FUNCTIONS
4.
5
Other precautions - If there is a discrepancy between the SP1/SP2 setting and the turret setting in the tool sequence, the alarm DBL SPDL OPER ILLEGAL TUR ASIGN is issued. - During the machining of 2 workpieces, the item # cannot be specified in the tool sequence. - During the machining of 2 workpieces, the following operations cannot be performed: transfer of workpieces, simultaneous machining, balanced cutting and retraction. - During the machining of 2 workpieces, the measuring unit cannot be used. - During the machining of 2 workpieces, only SINGLE operation in the head selection unit can be selected. - During the machining of 2 workpieces, cross commands cannot be entered in the subprogram and manual program machining unit. - In the 2 WORKPC unit with START designation, the upper and the lower turrets are placed in a queue. - If the turrets interfere with each other during the machining of 2 workpieces, set the 2 WORKPC unit with END designation and use the unit anew to time the operation of the upper and lower turrets.
5-9
5 5-2
LOWER-TURRET CONTROL FUNCTIONS
Retraction of the Lower Turret
Retraction D737P0011
When performing upper-turret machining operations near the rotational center of the turning spindle, interference between the upper and lower turrets can be avoided by retracting the lower turret. 1.
Programming method The use of the tool sequence menu allows the following two retraction positions to be selected for the lower turret: TURRET 2 TURRET 2 POS.1 POS.2
1: After the return of the turret to its X2/Z2 axial second home position, retraction tool 1 is indexed and then the turret is retracted to fixed position 1 in the X2/Z2 axial direction. 2: After the return of the turret to its X2/Z2 axial second home position, retraction tool 2 is indexed and then the turret is retracted to fixed position 2 in the X2/Z2 axial direction. UNo.
UNIT
1
DRILLING
XY
SNo.
TOOL
NOM-φ #
1 FIG 1
MODE
DRILL PTN
10.
POS-B
POS-C
DIA
DEPTH
CHMF
!
45.
10.
30.
0.
HOLE-φ HOLE-DEP PRE-DIA PRE-DEP
1
10.
CY/PY
F
M
N ANGLE
P
Q
R
25.
!
!
4
!
!
0
1
POS-B 90
TOOL
Note:
OUT S-CNR
C 1. END
0.294
CX/PX
OUT
3
FR
36
0.
PART
UNIT
C-SP
5.
SPT-Z
UNIT
1
DEPTH
–50.
T.GROOVE
UNo.
RGH DRIL T
SPT-C/y
2
FIG
100
3.
UNo.
F 1 GROOVE
0.
SPT-R/x
LIN
SNo.
30.
PAT. No. 0
NOM.
#
10.
50
1
PITCH
WIDTH
FINISH
0.
10.
!
0.
PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z !
!
2.
!
!
SPT-X
SPT-Z
FPT-X
FPT-Z
CNR
130.
70.
120.
70.
C 1.
! ANG
C-SP !
M M M
FR M M M 0.1
RGH
COUNTER RETURN WK.No. CONT. NUM. SHIFT During drilling with the upper turret, the lower turret is retracted to fixed position 1.
The retraction tool is always indexed at a lower-turret retraction tool changing position (second home position), not the normal lower-turret tool changing position designated with parameter SU10.
5-10
LOWER-TURRET CONTROL FUNCTIONS
2.
5
Description of operation Upper turret
Lower turret
[1] Movement to tool-rotating position
[1] Movement to lower-turret tool changing position [2] Movement to lower-turret retraction tool changing position (second home position) in accordance with the command from the upper turret [3] Retraction tool indexing in accordance with the command from the upper turret [4] Retraction to fixed position 1
[5] Tool change [6] Approach to starting position of machining [7] Machining Before machining with the lower turret is started following completion of the retraction: [8] Movement to lower-turret retraction tool changing position (second home position) [9] Tool indexing (Note) [10] Approach, followed by machining
[5]
[1] [6] [7] [10]
[3]
[1] [2]
[4] [8] Second home position [9]
Note:
3.
Fixed position 1 D737P0012
Even if the currently indexed tool and the tool to be used for next machining are the same (no tool change is conducted), the lower turret will move temporarily to the lower-turret retraction tool changing position (second home position) and the next unit will be executed.
Description of parameters Parameters relating to the lower-turret retraction function are listed below. See the separate Parameter List/Alarm List/M-Code List for further details. SU52： Tool number of retraction tool 1 SU53： Tool number of retraction tool 2 SU97： X-axis coordinate of fixed position 1 SU98： Z-axis coordinate of fixed position 1 SU199： X-axis coordinate of fixed position 2 SU100： Z-axis coordinate of fixed position 2 M5 (X, Z)： Second home position
5-11
5
LOWER-TURRET CONTROL FUNCTIONS
5-3 5-3-1
Other Setup Items LTUR DIA in common unit
Section to be machined with the upper turret
Outside diameter of the workpiece
LTUR DIA
Downward movement from this position is prohibited because of a stroke limit.
Section to be machined with the lower turret
D737P0007
As shown in the above view, when a large-size workpiece is machined, the lower turret may come into the outside-diameter section of the workpiece. In this case, although the lower turret may attempt moving out of the outside-diameter section of the workpiece for safety reasons during the start of machining with the upper turret, operation comes to a software-limited stroke alarm stop because of a stroke limit. In such a case, specify LTUR DIA in the common unit as the safe outside-diameter value for the lower turret. The lower turret judges the setting of LTUR DIA to be a safe position, and when the upper turret performs the machining operation, the lower turret moves to this position and does not suffer the stroke limit. UNo. 0
MAT. CST IRN
OD-MAX
ID-MIN
LENGTH
WORK FACE
280.
0.
55.
0.
In other cases, no data needs to be specified in LTUR DIA.
5-12 E
ATC MODE
RPM
LTUR DIA
2000
130.
6
TPC DATA SETTING
6
TPC DATA SETTING Tool path control (TPC) data can be set for each unit of the program. The TPC data consists of data items used to adjust tool paths and relay points. Tool paths are automatically created using the data that has been set on the PROGRAM display, and the data that has been set in various parameters. The TPC data is intended to allow unitby-unit modification of the tool paths that have thus been created, and thus to remove unnecessary paths or prevent interference. The TPC data, therefore, does not always need to be set to perform machining operations. The TPC data cannot be set for the following units: - Common unit - M-code unit - End unit - Subprogram unit - Process end unit - Materials shape unit - Head selection unit - Simultaneous machining unit
6-1
Operating Procedure for Setting TPC (Tool-Path Control) Data (1) First, place the cursor at the unit data line of the unit for which the TPC data is to be set. Example: UNo.
MAT.
0
CBN STL
UNo. 1 SNo.
To set TPC data for the bar-materials machining unit (BAR) (UNo. 1): OD-MAX ID-MIN LENGTH WORK FACE
UNIT BAR
60.
0.
60.
POS-B
CPT-X
CPT-Z
FIN-X
FIN-Z
90.
60.
0.
0.2
0.1
TOOL
NOM.
No. #
PAT.
20. A
0
2.5
OUT
20. B
!
!
PTN
S-CNR C
SPT-X
SPT-Z
!
!
2.
UNo.
UNIT
PART
2
T.GROOVE
OUT
SNo.
90.
TOOL
NOM.
F 1 GROOVE OUT
5.
FIG
S-CNR
1 UNo. 3
0
!
!
25
0.1
! 0. 0. 63 ! Place the cursor at this line. FPT-Z F-CNR/$ R/θ RGH
0.1
50.
C
!
5.
PITCH
WIDTH
FINISH
1
20.
5.
!
!
A SPT-Z
50.
20. !
!
▼▼ 4
PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP
SPT-X
!
!
No.
0
No. #
UNIT CONTI. REPEAT SHIFT END
FPT-X 50.
POS-B PAT.
LTUR DIA
DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP FR M M M
OUT
LIN
2000
OUT
F 2 GENERAL
1
RPM
0
PART
R 1 GENERAL
FIG
ATC MODE
0.
!
2. FPT-X
FPT-Z
40.
20.
!
!
F-CNR
120
M M M
0.08
RGH ▼▼ 4
NUMBER
ATC
RETURN
LOW RET.
0
0
END
END
6-1
!
ANG
FR
WORK No.
EXECUTE !
6
TPC DATA SETTING
(2) Press the menu selector key, and then the [TPC] menu key. - Pressing the [TPC] menu key indicates the TPC display for the unit specified at step (1). For the case of the example above, the following TPC display will be presented on the screen. UNo. 1
UNIT BAR
PARAMETER
PART OUT
POS-B CPT-X CPT-Z 90. 60. 0.
TC37 ■ TC1 ■ TC13 ■
TC38 ■ TC67 ■ TC15 ■
TC39 ■ TC68 ■
FIN-X 0.2 TC40 ■ TC5 ■
FIN-Z 0.1 TC62 ■ TC6 ■
←A TC45 ■ TC71 ■
ROTATE POSITION SU10 APPROACH RELAY POINT X Y Z 1 □ □ □ 2 □ □ □ 3 □ □ □
■ SU50 ■ [AUTO] M S □ □ □ □ □ □
SU51 ■ X □ ESCAPE RELAY X Y 1 □ □ 2 □ □ 3 □ □
Z □ POINT [AUTO] Z M S □ □ □ □ □ □ □ □ □
FINISH ROTATE POSITION SU10 APPROACH RELAY POINT X Y Z 1 □ □ □ 2 □ □ □ 3 □ □ □
■ SU50 ■ [AUTO] M S □ □ □ □ □ □
SU51 ■ X □ ESCAPE RELAY X Y 1 □ □ 2 □ □ 3 □ □
Z □ POINT [AUTO] Z M S □ □ □ □ □ □ □ □ □
UPPER ROUGH
LOWER ROUGH
ROTATE POSITION SU10 ■ SU50 ■ SU51 ■ X □ Z □ APPROACH RELAY POINT [AUTO] ESCAPE RELAY POINT [AUTO] X Z M S X Z M S 1 □ □ □ □ 1 □ □ □ □ 2 □ □ □ □ 2 □ □ □ □ 3 □ □ □ □ 3 □ □ □ □
FINISH ROTATE POSITION SU10 ■ SU50 ■ APPROACH RELAY POINT [AUTO] X Z M S 1 □ □ □ □ 2 □ □ □ □ 3 □ □ □ □
Z □ SU51 ■ X □ ESCAPE RELAY POINT [AUTO] X Z M S 1 □ □ □ □ 2 □ □ □ □ 3 □ □ □ □
TPC data
(3) Set the data in indicated item or change the data displayed in indicated item. - On line (A) above, unit data that was set on the PROGRAM display will be displayed as it is. The data cannot be changed on the TPC display. - Data that is preset in related parameters will be displayed at items marked with '. Parameters denoting the distance are usually preset in 0.001 mm (0.0001 inch) steps, but on the TPC display, they will be displayed in 1 mm (1 inch) steps. Example:
Data preset in parameter SU50:
2500 (in 0.001 mm steps) ↓ SU50 data displayed on the TPC display: 2.500 (in 1 mm steps)
Data being displayed at these items can be changed to any other data. If changes are made to the data, the corresponding unit will have its parameter settings overriden with the new data. The parameter settings will not change even if the displayed data is changed on the TPC display.
6-2
TPC DATA SETTING
6
- Items marked with # can be filled with data as required. To specify relay points for the tool approach or escape (return) path, first move the cursor to the item “[AUTO]” of the required data section, and then press the [MANUAL] menu key. The item marked with the cursor will change over to “[MANU]” and you can set required data for the relay points. - See the next section for the contents of each TPC data. The same items are displayed except the items for line of PARAMETER in any machining unit. Note 1: The following menu is displayed while the TPC display remains on the screen: TPC
TPC
END
CANCEL
Pressing the [TPC END] menu key calls up the PROGRAM display anew. Note 2: Setting or changing TPC data displays “+” mark on the left side of the corresponding unit number. For units whose TPC data has been set or changed, eight blocks of program memory (maximum) will be used. If TPC data has been set for unit No. 1：
If TPC data has not been set: UNo.
MAT.
OD-MAX
ID-MIN
UNo.
MAT.
OD-MAX
0
CBN STL
60.
0.
0
CBN STL
60.
ID-MIN 0.
UNo.
UNIT
PART
POS-B
UNo.
UNIT
PART
POS-B
1
BAR
OUT
90.
+1
BAR
OUT
90.
SNo.
TOOL
NOM.
F1
GENERAL OUT
20. A
F2
GENERAL OUT
No. + mark
20. B
SNo.
TOOL
NOM.
F1
GENERAL OUT
20. A
F2
GENERAL OUT
No.
20. B
FIG
PTN
S-CNR
SPT-X
FIG
PTN
S-CNR
1
LIN
C 2.
!
1
LIN
C 2.
!
UNo.
UNIT
PART
POS-B
UNo.
UNIT
PART
POS-B
2
T.GROOVE
OUT
90.
2
T.GROOVE
OUT
90.
SNo.
TOOL
F1
GROOVE OUT
FIG
NOM. 5. A S-CNR
1
SNo.
TOOL
F1
GROOVE OUT
SPT-X
FIG
50.
1
TPR
SPT-X
NOM. 5. A S-CNR
SPT-X 50.
UNo.
UNIT
CONTI.
REPEAT
UNo.
UNIT
CONTI.
REPEAT
3
END
0
!
3
END
0
!
Note 3: Carry out the following procedure to cancel the entire TPC data that has been set (or changed): 1) Press [TPC CANCEL] menu key. 2) Set “–9999”. The entire current TPC data is cancelled and initial TPC data is displayed on the TPC display. Also, the + mark on the PROGRAM display is deleted. This procedure, of course, only cancels the TPC data for the respective unit. Note 4: After TPC data has been set (or changed), the + mark will become ! mark if you update the unit data. In that case, you must carry out the procedure above (described in Note 3) to temporarily initialize the TPC data. Subsequently, you can set (or change) the desired TPC data once again. An alarm will occur if you make an attempt to execute the program with the ! mark displayed.
6-3
6 6-2
TPC DATA SETTING
Description of Each TPC Data Item of Turning Unit and Measurement Unit UNo. UNIT 1 BAR PARAMETER
UPPER
ROUGH
(f)
FINISH
(f)
LOWER ROUGH
(f)
FINISH
(f)
PART OUT TC37 1. TC1 100 TC13 100
POS-B 90. TC38 1. TC67 1. TC15 100
ROTATE POSITION
CPT-X 60. TC39 2. TC68 1.
CPT-Z 0. TC40 2. TC5 50
SU10 6
SU50 2.5
APPROACH RELAY POINT [AUTO] X Y Z M S 1 2 (d) 3 ROTATE POSITION
SU10 6
SU10 6
APPROACH RELAY POINT X Z M 1 2 (d) 3 ROTATE POSITION
SU10 6
APPROACH RELAY POINT X Z M 1 2 (d) 3
X
(b)
Z
(c)
SU51 5.
X
Z
(c)
SU51 5.
X
Z
(c)
ESCAPE RELAY POINT [AUTO] X Z M S 1 2 (e) 3
SU50 2.5
[AUTO] S
SU51 5.
(a)
ESCAPE RELAY POINT [AUTO] X Y Z M S 1 2 (e) 3
SU50 2.5
[AUTO] S
FIN-Z 0.1 TC45 0.2 TC71 1000
ESCAPE RELAY POINT [AUTO] X Y Z M S 1 2 (e) 3
SU50 2.5
APPROACH RELAY POINT [AUTO] X Y Z M S 1 2 (d) 3 ROTATE POSITION
FIN-X 0.2 TC62 0 TC6 50
SU51 5.
X
Z
(c)
ESCAPE RELAY POINT [AUTO] X Z M S 1 2 (e) 3
(a) Unit data for which the TPC display is called up. The data cannot be changed with the TPC data displayed on the screen. (b) The addresses of related parameters and the data that have been set on the PARAMETER display are displayed according to the particular type of unit. Modification of the data allows the machine to be correspondingly operated only during that unit. The data settings on the PARAMETER display, however, will not change by their modification on the TPC display. Refer to the separate Parameter List/Alarm List/M-Code List for details of parameter data. Parameters denoting the distance are usually set in 0.001 mm (or 0.0001 in.) steps, but they will be displayed here in 1 mm (or 1 in.) steps.
6-4
TPC DATA SETTING
6
Data of items (c), (d), and (e) can be set for each turret and each process. Set TPC data only for the corresponding process. For example, TPC data for the lower turret does not need to be set in a unit intended only for machining with the upper turret, and TPC data for the finishing does not need to be set in a unit intended only for rough machining, either. (c) Data related to the position of tool change (turret rotation) for each roughing or finishing unit. - For items X and Z, specify the coordinates (in the machine coordinate system) of the required fixed point in mm (or in.). - Refer to the separate Parameter List/Alarm List/M-Code List for details of SU10, SU50 and SU51. (d) Use this section to modify the approach path so that interference does not occur. To modify the path, first set the cursor at “[AUTO]” of the required section and then press the [MANUAL] menu key, to display “[MANU]”. Finally enter the coordinates of the relay points, required M-codes, and S-codes for revolution speed on three lines (1, 2 and 3) in the desired order of relaying. M- and S-codes in the line without axis feed command are invalid.
P2 (P2X, P2Z)
P1 (P1X, P1Z)
P3 (P3X, P3Z)
Tool change position
Machining start point
Program origin
For approaching path from the tool change position through relay points P1, P2 and P3 to the machining start point, as shown above, set data as follows: APPROACH RELAY POINT [MANU] X
Y
Z
M
S
1
P1X
P1Z
← Path through P1
2
P2X
P2Z
← Path through P2
3
P3X
P3Z
← Path through P3
Specify the position using the program coordinate system. - Enter X-coordinates in diameter or in radius values, for the turning or milling unit respectively. - For Z-axis positions on the right of the program origin, enter negative values except for the FACING unit for which a negative Z-coordinate denotes a position on the left of the program origin.
6-5
6
TPC DATA SETTING
(e) Use this section to modify the escape path so that interference does not occur. Refer to the description in (d) for details on data setting. （P2’X, P2’Z) P2’
P3’(P3’X, P3’Z)
（P1’X, P1’Z) P1’ Tool change position Machining end point
Program origin
ESCAPE RELAY POINT [MANU] X
(f)
Y
Z
M
S
1
P1’X
P1’Z
← Path through P1’
2
P2’X
P2’Z
← Path through P2’
3
P3’X
P3’Z
← Path through P3’
For the MMS unit, WORK MES unit, TOOL MES unit, and TRANSFER unit set M-codes to be executed. - When two M-codes are set here, they are executed simultaneously.
Note:
The manually input data for relay points are not cancelled by changing “[MANU]” over to “[AUTO]”. They will automatically be restored by changing “[AUTO]” back to “[MANU]” again. To change the data, therefore, first clear the displayed data with the data cancellation key and then input new data as required. Machine operation is always carried out according to the data setting on the TPC display.
6-6 E
PROGRAM EDITING
7
7
PROGRAM EDITING This chapter describes operating procedures for editing programs already created. It also describes the various editing functions of the NC unit.
7-1
Operating Procedures for Editing Programs 1.
Operating procedures for editing a MAZATROL program (1) Call up the PROGRAM display. - Press the display selector key and then the [PROGRAM] menu key. (2) Specify the work number of the program to be edited. - After pressing the [WORK No.] menu key, specify the work number. The work-No. can also be specified in the work-Nos. listing window which will appear after pressing the above menu key. Using the cursor keys, place the cursor on the desired work-No. and press the input key. - The selected program will be displayed on the screen. (3) Press the [PROGRAM] menu key. - Now, program data setting is possible; you can move the cursor to the desired position in the program using the cursor keys. Unless you press this menu key, you cannot change the program data being displayed; the cursor will only move vertically through the left end of each line even if you press the cursor keys. (4) Edit the program. (5) When necessary corrections or other edits to the program are completed, press the [PROGRAM COMPLETE] menu key.
2.
Program editing functions Pressing the menu changeover key with the PROGRAM display remaining on the screen displays the following menu: PROGRAM SEARCH CALCULAT COMPLETE 1
TPC
INSERT
ERASE
SHAPE COPY
UNIT COPY
PROGRAM COPY
2
3
4
4
4
You can use functions 1 to 4 above to carry out the editing operations listed below. No.
Menu item
Function
1
FIND
2
INSERT
To insert one blank line for unit or sequence into any position on the PROGRAM display
3
ERASE
To delete a specific unit or sequence existing in the program currently being displayed on the PROGRAM display
4
COPY
To copy the data in unit of program, unit or machining shape (sequence)
To search for the intended unit or sequence in the program
7-1
HELP
7 7-2
PROGRAM EDITING
Search There are the following five types of search: - Search for a unit number - Search for the end of a program - Search for a unit name - Search for a name of a tool - Search for a workpiece transfer unit 1.
Search for a unit number This function is used for displaying a unit to be checked or modified in the program. The cursor is displayed at the intended unit. (1) Display the menu including [SEARCH]. During program editing, press the menu selector key to display the menu. PROGRAM SEARCH CALCULAT COMPLETE
TPC
ERASE
INSERT
SHAPE COPY
UNIT COPY
PROGRAM COPY
HELP
(2) Press the [SEARCH] menu key. !
This causes the display of the search menu. UNIT No. LAST SEARCH SEARCH
UNIT SEARCH
TRS SEARCH
TOOL SEARCH
(3) Press the [UNIT No. SEARCH] menu key. !
This causes the display of [UNIT No. SEARCH] to reverse and the screen displays the message UNIT NUMBER ?.
(4) Enter the number of the unit to be found. Example:
Unit number 10 Press the following keys:
!
1
0
INPUT
The cursor moves to the number of the unit entered and the unit is displayed on the screen.
UNo. UNIT ← The cursor moves here. 10 SNo. TOOL 1 2 FIG PTN
Note 1: When the entered number of the unit does not exist in the program, the alarm 407 DESIGNATED DATA NOT FOUND is displayed. Note 2: In the UNIT No. SEARCH function mode, the number of the unit entered is searched for from the head of the program, wherever the present position of the cursor is.
7-2
PROGRAM EDITING
2.
7
Search for the end This LAST SEARCH function moves the cursor to the end of the program. This function is used for resuming the programming whilst in progress. (1) Display the menu including [SEARCH]. During program editing, press the menu selector key to display the menu. PROGRAM SEARCH CALCULAT COMPLETE
TPC
INSERT
ERASE
SHAPE COPY
UNIT COPY
PROGRAM COPY
HELP
(2) Press the menu key [SEARCH]. !
This causes the display of the search menu. UNIT No. LAST SEARCH SEARCH
UNIT SEARCH
TOOL SEARCH
TRS SEARCH
(3) Press the [LAST SEARCH] menu key. !
This causes the display of [LAST SEARCH] to reverse and the screen displays the message LAST SEARCH ?.
(4) Press the input key !
INPUT
.
The cursor goes to the end of the program and the last line is displayed on the screen.
FIG UNo. UNIT ← The cursor moves here.
3.
Search for a unit name This function serves to display the line of a required unit on the basis of the unit name. The cursor is displayed at the intended unit. (1) Display the menu including [SEARCH]. During program editing, press the menu selector key to display the menu. PROGRAM SEARCH CALCULAT COMPLETE
TPC
INSERT
ERASE
SHAPE COPY
UNIT COPY
PROGRAM COPY
HELP
(2) Press the [SEARCH] menu key. !
This causes the display of the search menu. UNIT No. LAST SEARCH SEARCH
UNIT SEARCH
TOOL SEARCH
TRS SEARCH
(3) Press the [UNIT SEARCH] menu key. !
The unit menu is displayed and the message UNIT NAME SEARCH ? is indicated on the screen. UNIT NAME SEARCH ?
POINT LINE FACE TURNING MANUAL MACH-ING MACH-ING MACH-ING PROGRAM
7-3
END
>>>
7
PROGRAM EDITING
(4) Select the name of the unit to be found. Example:
Search under the name of the RGH CBOR machining unit.
1)
Presse the [POINT MACH-ING] menu key.
!
The point machining unit menu is displayed. UNIT NAME SEARCH ?
DRILLING
RGH BCB
REAMING
TAPPING
BORING
BK CBOR
(
CIRC MIL
CBOR TAP
) HI SPD. DRL.USE
2)
Press the menu key [RGH CBOR].
!
The display of [RGH CBOR] is then reversed.
3)
Press the input key
!
The cursor then goes to the line of the entered unit and the unit is displayed on the screen.
UNo. 10 SNo.
TOOL CTR-DR
2
DRILL
UNo. 24
.
The cursor moves here.
Another pressing of the input key unit name.
INPUT
results in the searching for the following same
UNIT RGH CBOR
SNo.
TOOL
1
CTR-DR
2
DRILL
Note:
INPUT
UNIT RGH CBOR
1
4)
4.
RGH CBOR
The cursor moves to the following same unit name.
The alarm 407 DESIGNATED DATA NOT FOUND is displayed when the name of the unit specified for the search does not exist after the cursor position.
Search for name of a tool This function, TOOL SEARCH, serves to display the sequence line of the required tool on the basis of the name of the tool. The cursor is displayed at the intended tool sequence line. (1) Display the menu including [SEARCH]. During program editing, press the menu selector key to display the menu. PROGRAM SEARCH CALCULAT COMPLETE
TPC
INSERT
ERASE
(2) Press the [SEARCH] menu key. !
This causes the display of the search menu. UNIT No. LAST SEARCH SEARCH
UNIT SEARCH
TOOL SEARCH
7-4
TRS SEARCH
SHAPE COPY
UNIT COPY
PROGRAM COPY
HELP
PROGRAM EDITING
7
(3) Press the [TOOL SEARCH] menu key. !
The tool names menu is displayed and the screen displays the message TOOL NAME SEARCH ?. TOOL NAME SEARCH ?
ENDMILL FACEMILL CHAMFER BALL CUTTER ENDMILL
OTHER TOOL
>>>
TOUCH SENSOR
a
- Pressing the [ >>> ] menu key changes the menu a → b → c → a in this order. CENTER DRILL
DRILL
GENERAL
GROOVE
Example:
BACKSPOT REAMER FACER THREAD
TAP
T.DRILL
BORING BAR
T.TAP
BACK BOR.BAR SPECIAL
CHIP VACUUM
>>> b
>>>
c
Search under the tool name: DRILL
1)
Press the [DRILL] menu key.
!
This will cause the display of [DRILL] to reverse.
2)
Press the input key
!
The cursor moves to the sequence line of the tool entered and the sequence line is displayed on the screen.
SNo.
TOOL
1
CTR-DR
2
DRILL
3
CHAMFER
INPUT
.
The cursor moves here.
3)
Another pressing of the input key name.
SNo.
TOOL
1
CTR-DR
2
DRILL
3
CHAMFER
4
END MILL
INPUT
results in finding the following same tool
The cursor moves to the following same unit name.
Note:
The alarm 407 DESIGNATED DATA NOT FOUND is displayed when the name of the tool specified for search does not exist after the cursor position.
7-5
7
PROGRAM EDITING
5.
Search for a workpiece transfer unit This function searches for a workpiece transfer unit and move the cursor to the unit. (1) Display the menu including [SEARCH]. During program editing, press the menu selector key to display the menu. PROGRAM SEARCH CALCULAT COMPLETE
TPC
INSERT
ERASE
SHAPE COPY
UNIT COPY
PROGRAM COPY
HELP
(2) Press the [SEARCH] menu key. !
This causes the display of the search menu. UNIT No. LAST SEARCH SEARCH
UNIT SEARCH
TOOL SEARCH
TRS SEARCH
(3) Press the [TRS SEARCH] menu key. !
The display of menu item is reversed and the message TRS UNIT SEARCH ? is indicated on the screen.
(4) Press the input key !
INPUT
.
The cursor then goes to the line of the workpiece transfer unit and the unit is displayed on the screen.
FIG UNo. 26 UNo. 27
UNIT TRANSFER UNIT
The cursor moves here.
Another pressing of the input key unit.
INPUT
results in finding the following workpiece transfer
FIG UNo. 38 UNo. 39
Note:
7-3
UNIT TRANSFER UNIT
The cursor moves to the following workpiece transfer unit.
The alarm 407 DESIGNATED DATA NOT FOUND is displayed when the workpiece transfer unit does not exist after the cursor position.
Insertion This INSERT function is used to insert (add) one unit, one tool sequence or one shape sequence during the creating or editing of a program. The following three types of insertion are available: - Insertion of a unit - Insertion of a tool sequence - Insertion of a shape sequence The line to be inserted (unit, tool) is determined depending on the cursor position.
7-6
PROGRAM EDITING
1.
7
Insertion of a unit Perform the following procedure to insert a unit. Menu selection: [INSERT] (1) Bring the cursor to the next line of the unit to be inserted. UNo.
MAT
0
CBN STL
UNo.
In the case where a line is inserted here, the cursor is to be located here.
UNIT DRILLING
1 SNo.
TOOL
1
CTR-DR
2
DRILL
(2) Display the menu for editing. PROGRAM SEARCH CALCULAT COMPLETE
TPC
INSERT
ERASE
SHAPE COPY
UNIT COPY
PROGRAM COPY
HELP
(3) Press the [INSERT] menu key. !
The display of [INSERT] is reversed and the screen displays the message LINE INSERT ?.
(4) Press the input key
INPUT
.
UNo.
MAT.
UNo.
MAT.
0
CBN STL
0
CBN STL
UNIT
UNo.
UNIT
UNo. 1
Unit inserted
1
DRILLING
SNo.
TOOL
UNo.
1
CTR-DR
2
UNIT
2
DRILL
SNo.
TOOL
1
CTR-DR
2
DRILL
DRILLING
Note 1: When the cursor is located on the line of the unit which follows the line of the shape sequence at step (1), the empty shape sequence is inserted. Then, pressing the [SHAPE END] menu key results in the insertion of an empty unit. ! SNo.
TOOL
This causes the insertion of an empty unit. SNo.
TOOL
SNo.
1
CTR-DR
1
CTR-DR
1
2
DRILL
2
DRILL
2
FIG 1 UNo.
FIG
PTN
PT
1 2
PT
UNIT FCE MILL
2 SNo. 1
PTN
TOOL FCE MILL
UNo. 2 SNo.
FIG 1
TOOL CTR-DR DRILL PTN PT UNIT
UNIT
UNo. 2
FCE MILL
UNo.
UNIT
TOOL
Shape sequence inserted
3
FCE MILL
Unit inserted
Note 2: When the insertion operation is done in UNo. 0 (common unit), the alarm 409 ILLEGAL INSERTION is displayed.
7-7
7
PROGRAM EDITING
(5) Enter the data. Refer to the Chapter 3, “PROGRAM CREATION” for the selection of each unit and data setting. Note:
2.
When the machining unit is inserted, the tool sequence and the shape sequence are successively inserted progressively with the development of the operation.
Insertion of a tool sequence Perform the following procedure to insert a tool sequence. Menu selection: [INSERT] (1) Bring the cursor to the next line of the tool sequence to be inserted. UNo. 0
MAT. CBN STL
UNo. 1
UNIT DRILLING
SNo.
TOOL
1
CTR-DR
2
DRILL
FIG
Case where a tool sequence line is to be inserted here
PTN
1
PT
(2) Display the menu for editing. PROGRAM SEARCH CALCULAT COMPLETE
TPC
ERASE
INSERT
SHAPE COPY
UNIT COPY
PROGRAM COPY
HELP
(3) Press the [INSERT] menu key. !
The display of [INSERT] is reversed and the screen displays the message LINE INSERT ?.
(4) Press the input key !
INPUT
.
This causes the insertion of an empty tool sequence line.
UNo.
MAT.
UNo.
MAT.
0
CBN STL
0
CBN STL
UNo.
UNIT
UNo.
UNIT
1
DRILLING
1
DRILLING
SNo.
TOOL
SNo.
1
CTR-DR
1
2
DRILL
2
CTR-DR
3
DRILL
FIG 1
PTN PT
TOOL Tool sequence inserted
FIG 1
PTN PT
(5) Enter the data. Refer to the Chapter 3, “PROGRAM CREATION” for the selection of each unit and data setting. Note:
When the insertion operation is done in UNo. 0 (common unit), the alarm 409 ILLEGAL INSERTION is displayed.
7-8
PROGRAM EDITING
3.
7
Insertion of a shape sequence Perform the following procedure to insert a shape sequence. Menu selection: [INSERT] (1) Bring the cursor to the next line of the shape sequence to be inserted. UNo.
UNIT
1
DRILLING
SNo.
TOOL
1
CTR-DR
2
DRILL
FIG
Case where a shape sequence line is to be inserted here
PTN PT
1 UNo. 2
UNIT FCE MILL
(2) Display the menu for editing. PROGRAM SEARCH CALCULAT COMPLETE
TPC
ERASE
INSERT
SHAPE COPY
UNIT COPY
PROGRAM COPY
HELP
(3) Press the [INSERT] menu key. !
The display of [INSERT] is reversed and the screen displays the message LINE INSERT ?.
(4) Press the input key ! UNo. 1
INPUT
.
This causes the insertion of an empty shape sequence line. UNIT
UNo.
DRILLING
1
UNIT DRILLING
SNo.
TOOL
SNo.
TOOL
1
CTR-DR
1
CTR-DR
2
DRILL
2
DRILL
FIG 1
PTN
FIG
PT
PTN
1
UNo.
UNIT
2
2
FCE MILL
UNo. 2
7-9
PT UNIT FCE MILL
Shape sequence inserted
7
PROGRAM EDITING
Note:
SNo.
When the cursor is located on the line of the unit which follows the line of the shape sequence, an empty shape sequence is inserted as follows.
TOOL
1
CTR-DR
2
DRILL
FIG 1 UNo. 2 SNo. 1
SNo.
PTN
TOOL
1
CTR-DR
2
DRILL
FIG
PTN
PT
1
PT
UNIT
2
.
FCE MILL
UNo.
TOOL
2
FCE MILL
SNo. 1
← Shape sequnce
UNIT
inserted
FCE MILL TOOL FCE MILL
(5) Enter the data. Refer to the Chapter 3, “PROGRAM CREATION” for the selection of each unit and data setting. Note:
7-4
When the insertion operation is done in UNo. 0 (common unit), the alarm 409 ILLEGAL INSERTION is displayed.
Deletion This ERASE function is used to erase the unit, the tool sequence or the shape sequence which has become unnecessary during the creating or editing of a program. The following three types of deletion are available: - Deletion of the unit - Deletion of the tool sequence - Deletion of the shape sequence 1.
Deletion of the unit Menu selection: [ERASE] (1) Place the cursor on the unit to be deleted. UNo.
MAT.
0
CBN STL
UNo.
UNIT
1
DRILLING
SNo.
TOOL
1
CTR-DR
2
DRILL
Case where this unit is to be deleted
(2) Display the menu for editing. PROGRAM SEARCH CALCULAT COMPLETE
TPC
INSERT
ERASE
SHAPE COPY
UNIT COPY
PROGRAM COPY
HELP
(3) Press the [ERASE] menu key. ! !
The display of [ERASE] is reversed and the screen displays the message: SELECT PROGRAMS - CURSOR?. The unit on which the cursor is located is selected (display of the unit line is reversed).
7-10
PROGRAM EDITING
7
(4) When multiple units are to be deleted at a time, use the upward and downward cursor keys to designate the area. (5) Press the input key !
UNo. 0 UNo. 1 SNo. 1 2 FIG 1 UNo. 2 SNo. 1 2 3 4 FIG 1 UNo. 3
Note:
2.
INPUT
.
The selected units are then deleted. The tool sequence and the shape sequence in this unit will equally be deleted. MAT. . CBN STL UNIT DRILLING TOOL CTR-DR DRILL PTN PT UNIT RGH CBOR TOOL CTR-DR DRILL END MILL CHAMFER PTN LIN UNIT SLOT
UNo. 0 UNo. 1
MAT. CBN STL UNIT SLOT
← Units to be deleted (reversed display)
When the deletion operation is done for UNo. 0 (common unit), the alarm 410 ILLEGAL DELETION is displayed.
Deletion of the tool sequence Menu selection: [ERASE] (1) Place the cursor on the tool sequnece to be deleted. UNo.
MAT.
0
CBN STL
UNo. 1
UNIT DRILLING
SNo.
TOOL
1
DRILL
FIG 1 UNo. 2
Case where this sequence is to be deleted
PTN PT UNIT FCE MILL
(2) Display the menu for editing. PROGRAM SEARCH CALCULAT COMPLETE
TPC
INSERT
ERASE
SHAPE COPY
UNIT COPY
PROGRAM COPY
HELP
(3) Press the [ERASE] menu key. !
The display of [ERASE] is reversed and the screen displays the message: SELECT PROGRAMS - CURSOR?.
7-11
7
PROGRAM EDITING
!
The tool sequence on which the cursor is located is selected (display of the sequence line is reversed).
(4) When multiple tool sequences are to be deleted at a time, use the upward and downward cursor keys to designate the area. ! !
When unit line is inclueded in the area, deletion occurs in the same manner as in “1. Deletion of the unit.” When tool sequence line is inclueded in the area, deletion occurs in the same manner as in “3. Deletion of the shape sequence.”
(5) Press the input key !
MAT.
UNIT
CTR-DR
2
DRILL
FIG
3.
PTN
CBN STL
UNo. 1
TOOL
1
MAT.
0
DRILLING
SNo.
1
UNo.
CBN STL
UNo. 1
.
The designated tool sequence, unit and shape sequence are deleted.
UNo. 0
INPUT
UNIT DRILLING
SNo. Tool sequence to be deleted (reversed display)
1
TOOL DRILL
FIG 1
PTN PT
PT
Deletion of the shape sequence Menu selection: [ERASE] (1) Place the cursor on the shape sequnece to be deleted. UNo.
MAT.
0
CBN STL
UNo. 1
UNIT DRILLING
SNo.
TOOL
1
CTR-DR
2
DRILL
FIG
PTN
1
LINE
2
PT
UNo.
UNIT
2
SLOT
Case where this sequence is to be deleted
(2) Display the menu for editing. PROGRAM SEARCH CALCULAT COMPLETE
TPC
INSERT
ERASE
SHAPE COPY
UNIT COPY
PROGRAM COPY
HELP
(3) Press the [ERASE] menu key. ! !
The display of [ERASE] is reversed and the screen displays the message: SELECT PROGRAMS - CURSOR?. The shape sequence on which the cursor is located is selected (display of the sequence line is reversed).
7-12
PROGRAM EDITING
7
(4) When multiple shape sequences are to be deleted at a time, use the upward and downward cursor keys to designate the area. ! !
When unit line is inclueded in the area, deletion occurs in the same manner as in “1. Deletion of the unit.” When tool sequence line is inclueded in the area, deletion occurs in the same manner as in “2. Deletion of the tool sequence.”
(5) Press the input key !
INPUT
.
The designated shape sequence, unit and tool sequence are deleted.
UNo.
MAT.
UNo.
MAT.
0
CBN STL
0
CBN STL
UNo.
UNIT
UNo.
UNIT
1
DRILLING
SNo.
1
TOOL
DRILLING
SNo.
TOOL
1
CTR-DR
1
CTR-DR
2
DRILL
2
DRILL
FIG 1 2 UNo. 2
PTN LINE PT UNIT
FIG Shape sequence to be deleted (reversed display)
1 UNo. 2
SLOT
7-13
PTN PT UNIT SLOT
7 7-5
PROGRAM EDITING
Copy During the process of creating or editing of a program, this COPY function is used to copy another program or one unit/shape sequence of a program in the process of creating or editing. There are three types of copying depending on the contents to be copied. - Copying of a program - Copying of a unit - Copying of a shape 1.
Copying of a program This PROGRAM COPY function is used to copy another program in the process of creating or editing of a program. However, the common unit and the end unit cannot be copied. Menu selection: [PROGRAM COPY] (1) Move the cursor to the line on which another program is inserted. UNo. 0
MAT. CBN STL Case where another program is inserted here
UNo. 1 SNo.
UNIT DRILLING TOOL
1
CTR-DR
2
DRILL
Note 1: When the cursor is not located on the unit line, the alarm 454 CURSOR POSITION INCORRECT will be displayed when selecting the [PROGRAM COPY] menu key. Note 2: When the cursor is located on the common unit, the alarm 454 CURSOR POSITION INCORRECT will be displayed when selecting the menu key [PROGRAM COPY]. (2) Display the menu for editing. PROGRAM SEARCH CALCULAT COMPLETE
TPC
INSERT
ERASE
SHAPE COPY
UNIT COPY
PROGRAM COPY
HELP
(3) Press the [PROGRAM COPY] menu key. !
The display of [PROGRAM COPY] is then reversed and the WORK No. window is displayed.
7-14
PROGRAM EDITING
7
(4) Enter the workpiece number of the program to be copied. Example:
Workpiece number 1000 1
Press the following keys: !
0
0
The program of workpiece number 1000 is then copied.
Example:
Program of WNo. 1000 is copied as follows:
Program in the process of editing
Program of WNo. 1000
UNo.
MAT.
UNo.
MAT.
0
CBN STL
0
CST IRN
UNIT
UNo.
UNIT
1
WPC-0
UNo. 1
0
DRILLING
SNo.
TOOL
UNo.
UNIT
1
CTR-DR
2
M-CODE
2
DRILL
UNo. 3
Program to be copied
UNIT END
Program after copying UNo.
MAT.
0
CBN STL
UNo.
UNIT
1
WPC-0
UNo.
UNIT
2
M-CODE
UNo. 3
Program copied
UNIT DRILLING
SNo.
TOOL
1
CTR-DR
2
DRILL
Note 1: When a workpiece number which is not recorded is entered, the alarm 405 PROGRAM No. NOT FOUND is displayed. Note 2: When an EIA/ISO program workpiece number is entered, the alarm 440 EIA/ISO PROGRAM DESIGNATED is displayed.
7-15
7
PROGRAM EDITING
2.
Copying of a unit In the process of creating or editing a program, this UNIT COPY function is used to perform the copying, unit by unit from the program or from another program. The unit and also the tool sequence and the shape sequence which follow are copied. Menu selection: [UNIT COPY] (1) Move the cursor to the line on which a unit is copied. UNo.
MAT.
0
CBN STL
UNo.
UNIT
1
Case where another unit is inserted here
DRILLING
SNo.
TOOL
1
CTR-DR
2
DRILL
Note 1: When the cursor is not located on the unit line, the alarm 454 CURSOR POSITION INCORRECT will be displayed when selecting the menu key [UNIT COPY]. Note 2: When the cursor is located on the common unit (UNo. 0), the alarm 454 CURSOR POSITION INCORRECT will be displayed when selecting the menu key [UNIT COPY]. (2) Display the menu for editing. PROGRAM SEARCH CALCULAT COMPLETE
TPC
ERASE
INSERT
SHAPE COPY
UNIT COPY
PROGRAM COPY
HELP
(3) Press the [UNIT COPY] menu key. !
The display of [UNIT COPY] is then reversed and the WORK No. window is displayed.
(4) Enter the workpiece number of the program containing the unit to be copied. Example:
Workpiece number 1000 Press the following keys:
!
1
0
0
0
INPUT
When the workpiece number is entered, the screen displays the message UNIT NUMBER ?.
7-16
PROGRAM EDITING
7
(5) Enter the number of the unit to be copied. Example:
Unit number 1 1
Press the following keys: !
Unit number 1 in the program of workpiece No. 1000 is then copied.
Example:
UNo. 1 of program WNo. 1000 is copied as follows:
Program in the process of editing UNo.
MAT.
0 UNo. 1
INPUT
Program of WNo. 1000 UNo.
MAT.
CBN STL
0
CST IRN
UNIT
UNo.
UNIT
DRILLING
1
SNo.
TOOL
SNo.
1
CTR-DR
1
2
DRILL
LINE CTR TOOL
FIG
PTN
1
SQR
UNo.
UNIT
2
Unit to be copied
FCE MILL
RGH CBOR
Program after copying UNo.
MAT.
0
CBN STL
UNo.
UNIT
1 SNo. 1
LINE CTR TOOL FCE MILL
FIG.
PTN
1
SQR
UNo.
UNIT
2
Unit copied
DRILLING
SNo.
TOOL
1
CTR-DR
2
DRILL
Note 1: The common unit UNo. 0 cannot be copied. Any attempt to make such a copy will cause the alarm 402 ILLEGAL NUMBER INPUT to be displayed. Note 2: When an unregistered workpiece number is entered, the alarm 405 PROGRAM No. NOT FOUND is displayed. Note 3: When a workpiece number of the EIA/ISO program is entered, the alarm 440 EIA/ISO PROGRAM DESIGNATED is displayed.
7-17
7
PROGRAM EDITING
3.
Copying of shape This SHAPE COPY function is used to copy the shape sequence in the process of creation or editing of a program. However, it is impossible to perform the copying if the shape sequence line has already been filled with data. Menu selection: [SHAPE COPY] (1) Move the cursor to the position in which the shape sequence is to be copied. Example: UNo. 1
UNIT DRILLING
SNo. 1
TOOL DRILL
FIG
PTN
1
PT
2
CIR
3
SQR
UNo. 2
UNIT DRILLING
SNo. 1
TOOL DRILL
FIG
PTN Case where the shape sequence of the unit No. 1 is copied on this shape sequence line
1
Note:
When the cursor is located in a position other than the shape sequence or when data have already been entered in the shape sequence, the alarm 454 CURSOR POSITION INCORRECT is displayed.
(2) Display the menu for editing. PROGRAM SEARCH CALCULAT COMPLETE
TPC
INSERT
ERASE
SHAPE COPY
UNIT COPY
PROGRAM COPY
HELP
(3) Press the [SHAPE COPY] menu key. !
The display of [SHAPE COPY] is then reversed and the screen displays the message UNIT NUMBER ?.
7-18
PROGRAM EDITING
7
(4) Enter the number of the unit containing the shape sequence to be copied. Example:
Unit number 1 1
Press the following keys: !
The shape sequence under unit No. 1 is then copied.
Example:
The shape sequence under unit No. 1 is copied as follows: Program after copying
Program before copying UNo. 1
UNIT
PT CIR
3
SQR
2
1 FIG 1
1
PTN
2
UNIT DRILLING TOOL DRILL PTN
UNIT DRILLING
SNo.
DRILL
1
SNo.
1
TOOL
FIG
UNo.
UNo.
DRILLING
SNo. 1
INPUT
TOOL DRILL
FIG Shape sequence to be copied
PTN
1
PT
2
CIR
3
SQR
UNo. 2
UNIT DRILLING
SNo. 1
TOOL DRILL
FIG
PTN
1
PT
2
CIR
3
SQR
Shape sequence copied
Note 1: When the number of an unestablished unit is entered, the alarm 407 DESIGNATED DATA NOT FOUND is displayed. Note 2: When the number of the unit entered does not contain the shape sequence, the alarm 452 NO SHAPE DATA IN UNIT is displayed. Note 3: When the type of the shape of the unit entered is different from that of the unit to be copied, the alarm 453 NO SHAPE DATA TO COPY IN UNIT is displayed.
7-19
7
PROGRAM EDITING
- NOTE -
7-20 E
PROGRAM CREATING/EDITING FUNCTIONS
8 8-1
8
PROGRAM CREATING/EDITING FUNCTIONS Help Function A help function is provided in the NC unit to give an illustrated description of program data. Help window shown below will be called up by pressing the [HELP] menu key with the cursor placed on a unit data item on the PROGRAM display. In the illustration the display of the respective item is highlighted according to the cursor position. Example:
Help window for the bar-materials machining unit (BAR)
MAZATROL: 5101001 File
Window
Help
UNo.
UNIT
PART
4
BAR
■
OUT
POS-B
SPT-X
CPT-Z
SPT-Z
FIN-X
FIN-Z
IN
CPT-Z
CPT-X CPT-X
CPT-Z
CPT-Z
CPT-X CPT-X
FACE
BACK
In the Help window, you can check details of the data to be set. Note 1: Not all types of data can be plotted in the Help window. See the relevant section of this manual if you are placed at a loss what type of data to set in the program. Note 2: Items which will be auto-set and those which will have an illustration on the menu display may not be indicated in the Help window.
8-1
8
PROGRAM CREATING/EDITING FUNCTIONS
8-2
Automatic Crossing-Point Calculation Function Automatic crossing-point calculation function for the NC system is to compute unknown coordinates of a point of intersection on an arbitrary form and to automatically enter the result in a program.
8-2-1
Automatic crossing-point calculation in the line and face machining units A crossing-point of arbitrary form is automatically calculated in the line and face machining units. In the description below machining unit for ZY mode (setting for MODE in unit data) is explained as example. Automatic crossing-point calculation can be also used in a similar manner for other machining modes. 1.
Coordinates of the crossing-point Even if coordinates of a crossing-point are unknown as illustrated below, the NC system will automatically obtain it from the coordinates of the start and end points and from angles involved. FIG
PTN
SHIFT-R
Z
Y
R/th
1
LINE
10.
50.
20.
2
LINE
!
?
?
30.
3
LINE
!
150.
20.
100.
FIG
PTN
SHIFT-R
Z
Y
R/th
1
LINE
10.
50.
20.
2
LINE
!
3
LINE
!
140.7604 72.4005 150.
20.
I
J
I
J
P
CNR R-FEED
RGH
P CNR R-FEED Displayed in yellow
RGH
30. 100.
150 50
Program origin Z 20
100°
30°
Start point
Y
After checking the plane, return to the PROGRAM display again and the coordinates so automatically obtained as a crossing-point will be displayed in yellow. Coordinates are also caluculated when the cursor is set on the ? item and the [CALCULAT] menu key is pressed.
8-2
PROGRAM CREATING/EDITING FUNCTIONS
Note:
8
When unknown coordinates of a crossing-point are automatically obtained in a combination of a line with an arc or of two arcs, do not fail to enter P. (Select the position of crossing-point.)
FIG
PTN
SHIFT-R
Z
Y
R/th
1
LINE
10.
50.
20.
2
LINE
!
?
?
30.
3
CW
!
165.
20.
40.
I
125.
J
P
CNR
R-FEED
RGH
20. RGT
125 50
(125, 20)
Program origin
(165, 20) Z 30° R:40
20 Y
(?, ?) Select LEFT or DOWN in the item P. Select RIGHT or UP in the item P.
To find a crossing point with the automatic crossing-point calculation function, first view the Ydirection from the origin in either ZY, XY or /Y mode and compare the positions of two crossing points. If the crossing point at right is the desired one, select RGT by pressing the [RIGHT] menu key. If the crossing point at left is the desired one, select LEFT by pressing the [LEFT] menu key. If the crossing point at the plus side is the desired one, this crossing point can likewise be specified by selecting UP with the [UP] menu key. If the crossing point at the minus side is the desired one, this crossing point can likewise be specified by selecting DOWN with the [DOWN] menu key.
8-3
8
PROGRAM CREATING/EDITING FUNCTIONS
2.
Examples of automatic crossing-point calculation A crossing-point is automatically calculated for combinations of line with line, line with arc and arc with arc as shown in the examples below. Pattern
Shape
Shape sequence
150 50
FIG PTN SCHIFT-R
LINE 20
LINE
1 LINE
30°
120°
X
R/th I
J
P
CNR
J
P
CNR
50. 20.
2 LINE 3 LINE
Y
?
?
30.
150. 20. 120.
( ?, ? )
150 FIG PTN SHIFT-R
50
LINE
1 LINE

20
(120, 20)
ARC (Contact)
Y
R/th I
50. 20.
2 LINE 3 CW
R30
X
?
?
150. 20. 30. 120.20.
( ?, ? )
50
LINE
(200, 0)
ARC
FIG PTN SHIFT-R
20

1 LINE
(200, 80) 30° Z
(Cross)
2 LINE
X
Y
R/th I
J
P
CNR
50. 20. ?
?
LEFT
30.
R80
3 CW
Select LEFT or DOWN for P
0. 80. 200.80.
200.
Y
Closed R4
FIG PTN SHIFT-R R10
(40, 5)
(20, 5)
X
Y R/th I
J
P
CNR
1 CW
?
?
10. 20. 5.
UP
R4
2 CW
?
?
15. 40. 5. DOWN
R4
X
Y
R/th I
CNR
R5 R4
ARC
Open
ARC (55, ?) R10
(?, ?)
FIG PTN SHIFT-R
10
(45, ?)
1 LINE
(25, 5)
5
R15
8-4
J
P
10. 5.
2 CW
?
?
15. 25. 5. DOWN
3 CCW
55.
?
10. 45.
?
PROGRAM CREATING/EDITING FUNCTIONS
Pattern
Shape
8
Shape sequence
g4 (?, ?) g5 (?, ?)
ARC
(55, 5)
FIG
R10
LINE
(?, ?) g2
ARC
(?, ?) g3
ARC
g3 (75, 5)
Y
R/th I
J
1 LINE
?
?
2 CW
?
?
3 LINE
?
?
4 CCW
?
?
X
Y
10.
5.
?
?
10. 20. 5.
P
CNR
P
CNR
10. 20. 5.
FIG (20, 5)
5
ARC
PTN SHIFT-R
1 LINE 2 CW
R15
15. 55. 5.
10
g2 (?, ?) (60, 5)

X
(20, 5)
R15

PTN SHIFT-R
R10
ARC
J
3 CCW
?
?
45.
4 CCW
75.
5.
15. 60. 5.
R45
':
Both Z and Y coordinates are known (i, j in the case of the center of an arc).
#:
Both Z and Y coordinates are not known (i, j in the case of the center of an arc).
8-5
R/th I
8
PROGRAM CREATING/EDITING FUNCTIONS
8-2-2
Automatic crossing-point calculation function in the turning unit When a TPR, or shape is to be defined on the sequence line of the bar-materials machining unit (BAR) or the copy-machining unit (CPY), or when an oblique groove, isopodic trapezoidal groove, or tapered groove shape is to be defined on the sequence line of the groove-machining unit (T. GROOVE), you can make the NC unit automatically calculate any unknown coordinates of the start point or end point of that shape. Automatic calculation may be performed within one sequence or it may span over two sequences. Conditions for automatic calculation are as follows. - Automatic calculation within one sequence Unit
Shape pattern
BAR or CPY T. GROOVE
Conditions
1. TPR
One of the items SPT-X, SPT-Z, FPT-X and FPT-Z is unknown; tapering angle known.
2. Arc
One item of the data pair (SPT-X, SPT-Z) or (FPT-X, FPT-Z) is unknown; center coordinates and radius of arc known.
3. -
One of the items SPT-X, SPT-Z, FPT-X and FPT-Z is unknown; tapering angle known.
- Automatic calculation over two sequences Unit
Shape pattern
BAR or
Conditions
4. Intersection of two TPRs
X- and Z-coordinates of the intersecting point of two taperings are unknown; two angels of tapering known.
5. Intersection of TPR and arc
X- and Z-coordinates of the intersecting point of tapering and arc are unknown; tapering angle and center coordinates and radius of arc known.
6. Osculation of TPR and arc
X- and Z-coordinates of the osculation point of tapering and arc are unknown; center coordinates and radius of arc, or tapering angle and radius of arc, are known.
7. Intersection of two arcs
X- and Z-coordinates of the intersecting point of two arcs are unknown; center coordinates and radii of both arcs known.
8. Osculation of two arcs
X- and Z-coordinates of the osculation point of two arcs are unknown; center coordinates and radius of one arc, and radius of the other arc are known.
CPY
- “Intersecting point” refers to a non-smoothly crossing point. Press the [INTER PT] menu key for an unknown intersecting point. - “Osculation point” refers to a smoothly crossing point. Press the [CONT PT] menu key for an unknown osculation point. TPR and TPR
Arc and TPR
Arc and Arc
Intersecting point
Arc and TPR
Osculation point
8-6
Arc and Arc
PROGRAM CREATING/EDITING FUNCTIONS
8
- Automatic calculation can also be performed in grafically checking the programmed data on the TOOL PATH or SHAPE CHECK display and the result is entered in a program. Given below is the procedure of data setting for automatic calculation in cases 1 to 8 shown in the table above. 1.
If start or end point of tapering is unknown. Example:
FPT-Z of tapering is unknown. 20 End point to of tapering
30° φ50
Start point of tapering φ30
T4P288
Set data as follows: UNo.
UNIT
PART
POS-B
CPT-X
CPT-Z
FIN-X
FIN-Z
*
BAR
OUT
90.
***
***
***
***
FIG
PTN
S-CNR
1
LIN
◆
◆
30.
20.
◆
2
TPR
30.
20.
50.
?
30.
SPT-X SPT-Z FPT-X FPT-Z
F-CNR/$
R/th
RGH
Press the [INTER PT] menu key for the unknown FPT-Z. Enter the tapering angle, 30°, for R/th. Note:
Enter positive angle value to designate upward tapering, or negative value for downward tapering.
Section to be machined
OUT ( OUT )
IN ( IN )
FACE ( FACE )
BACK ( BACK )
Sign
th: Positive value
th th th
th
th
th: Negative value th th
8-7
th
8
PROGRAM CREATING/EDITING FUNCTIONS
2.
If start or end point of arc is unknown. Example:
SPT-Z and FPT-X of convex arc is unknown.
60 Start point of arc End point of arc R30 40
φ10
φ30
Set data as follows. UNo. *
UNIT BAR
FIG
PTN
PART
POS-B
CPT-X
CPT-Z
FIN-X
FIN-Z
OUT
90.
***
***
***
***
S-CNR
1 2
CTR
◆
SPT-X SPT-Z FPT-X FPT-Z 30.
?
?
60.
10.
40.
◆
◆
4
R/th
RGH
30. ◆
◆
Press the [INTER PT] menu key for the unknown SPT-Z and FPT-X. Enter the radius of the convex arc, 30, for R/th. For the sequence data line next to that of convex arc, first press the [CENTER] menu key and then enter the X- and Z-coordinates of the arc center in SPT-X and SPT-Z, respectively. 1.
Enter the X-coordinate with minus sign for a center below the workpiece center line; likewise the Z-coordinate for a center on the right of program origin. Example:
10
R40 φ40
φ20
FIG
PTN
S-CNR
1 2
CTR
◆
SPT-X SPT-Z FPT-X FPT-Z ?
0.
40.
?
-20.
-10.
◆
◆
8-8
F-CNR/$
R/th
RGH
40. ◆
LEFT
PROGRAM CREATING/EDITING FUNCTIONS
2.
8
In general, an arc and a line cross each other at two points. To specify which one is to be set, use the menu keys [UP], [DOWN], [LEFT] or [RIGHT] on the CTR sequence line at the R/th item for unknown SPT or at RGH for FPT. To find a crossing point with the automatic crossing-point calculation function, first view the X-direction from the origin and compare the positions of two crossing points. If the crossing point at right is the desired one, select RGT by pressing the [RIGHT] menu key. If the crossing point at left is the desired one, select LEFT by pressing the [LEFT] menu key. If the crossing point at the plus side is the desired one, this crossing point can likewise be specified by selecting UP with the [UP] menu key. If the crossing point at the minus side is the desired one, this crossing point can likewise be specified by selecting DOWN with the [DOWN] menu key. Example:
47.321
（a）
（b） R20
SPT
FPT φ50 φ40
30 φ20
FIG
PTN
S-CNR
1 2
CTR
◆
SPT-X SPT-Z FPT-X
FPT-Z
50.
?
40.
47.321
20.
30.
◆
◆
F-CNR/$
R/th
RGH
20. ◆
RGT
To specify (a) for calculation of SPT-Z, press the [RIGHT] menu key at R/th since the one point (a) lies on the right of the other possible point (b).
8-9
8
PROGRAM CREATING/EDITING FUNCTIONS
3.
If start or end point of tapered shape is unknown (for T. GROOVE unit). As for the case 1, one of the items SPT-X to FPT-Z can be auto-set if the tapering angle is clearly known. Example:
FPT-Z of tapering is unknown. 50 SPT 60°
φ80
FPT φ40
Set data as follows: UNo.
UNIT
PART
*
T.GROOVE
OUT
SNo. F1
TOOL
POS-B PAT. No. 0
PITCH
WIDTH
FINISH
0.
30.
◆
1
NOM. No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP FR M M M
GROOVE OUT 50.B
FIG
90.
S-CNR
SPT-X
1
80.
◆
◆
2.
◆
SPT-Z FPT-X FPT-Z 50.
40.
◆
CNR
◆ ANG
?
105 0.2 RGH
60.
For the grooving pattern #0, the ANG data must be entered as a positive or negative value according to the direction of the respective tapering. Enter positive values for ANG (θ).
Enter negative values for ANG (θ).
OUT
OUT
θ θ
θ θ
BACK
BACK
FACE
θ
FACE
θ
θ
θ IN
IN
For the patterns #1 to #3, the sign of the ANG data is insignificant.
8-10
PROGRAM CREATING/EDITING FUNCTIONS
4.
If intersecting point of two taperings is unknown. Example: 40 PTN
30°
SPT-X SPT-Z FPT-X FPT-Z
TPR
20.
0.
TPR
?
?
(?, ?)
*1
?
?
80.
40.
*1
R/th 45. *2 30. *3
φ80 *1. Press the [INTER PT] menu key for unknown coordinates of the intersecting point of two taperings. *2. Enter the tapering angle. *3. Enter the tapering angle.
45° φ20
5.
If intersecting point of tapering and arc is unknown. (?, ?) (b)
(60, 55) (a)
R25
30°
40
φ20
PTN
S-CNR
TPR CTR
*1. *2. *3. *4. *5.
!
φ20
SPT-X SPT-Z FPT-X FPT-Z 20.
0.
?
?
20.
40.
*1
?
?
60.
55.
!
!
*4
F-CNR
*1 !
R/th 30.
*2
25.
*3
LEFT
RGH
*5
Press the [INTER PT] menu key for unknown coordinates of the intersecting point of tapering and arc ( ). Enter the tapering angle. Enter the radius of arc. Enter the coordinates of arc center. To specify (b) from among the two intersecting points of tapering and arc, press the [LEFT] (or [UP]) menu key.
8-11
8
8
PROGRAM CREATING/EDITING FUNCTIONS
6.
If osculation point of tapering and arc is unknown.
(?, ?) (60, 65) R25
50 φ20
φ20
PTN
S-CNR
SPT-X SPT-Z FPT-X FPT-Z
TPR
20. ? # !
CTR
20.
? #
0.
? # *1 60. 50. *3 !
F-CNR
? # *1 65. !
R/th
RGH
25. *2 !
*1. Press the [CONT PT] menu key for unknown coordinates of the osculation point of tapering and arc ( ). *2. Enter the radius of arc. *3. Enter the coordinates of arc center.
7.
If intersecting point of two arcs is unknown.
(80, 50) R30
(?, ?) (40, 0) R25
φ20
φ10
20
50 PTN
S-CNR
CTR
!
CTR
!
SPT-X SPT-Z FPT-X FPT-Z F-CNR 40. 0. ? ? *1 ! ! ! 10. 20. *3 ? ? *1 80. 50. ! ! 20. 50. *5 !
R/th 25. *2
RGH UP *6
30.
*4
*1. Press the [INTER PT] menu key for unknown coordinates of the intersecting point of two convex arcs. *2. *3. *4. *5. *6.
Enter the radius of arc. Enter the coordinates of arc center. Enter the radius of arc. Enter the coordinates of arc center. To specify the upper one of the two possible intersecting points, press the [UP ] menu key in response to the message INTERSEC POS OF FINAL POINT?.
8-12
PROGRAM CREATING/EDITING FUNCTIONS
8.
If osculation point of two arcs is unknown. 95
R50
(?, ?)
φ140
R25 φ70 φ20
PTN
S-CNR
CTR !
SPT-X SPT-Z FPT-X FPT-Z 70.
0.
20.
0.
?
#
?
? *3
# !
?
F-CNR
# *1 !
# *1 140. 95.
R/th 25.
!
RGH
*2
50. *4
*1. Press the [CONT PT] menu key for unknown coordinates of the osculation point of convex and concave arcs. *2. Enter the radius of convex arc. *3. Enter the center coordinates of convex arc. *4. Enter the radius of concave arc.
8-13
8
8
PROGRAM CREATING/EDITING FUNCTIONS
9.
Supplement In cases 5 to 8, the following unknown intems can also be auto-set. Example:
For intersecting point of tapering and arc, SPT-X or -Z of tapering and FPT-X or -Z of arc are unknown. 60
(b) (d)
(c) R20 (a) 30°
φ50
30 φ20
φ20
PTN TPR
CTR LINE *1. *2. *3.
S-CNR
!
SPT-X SPT-Z FPT-X FPT-Z 20. 0. ? ? ?
?
20.
30.
!
!
50.
*1 ! *5 50.
? ! 60.
F-CNR *1 *3
!
R/th 30. *2 20. *4 RGT *6
RGH
LEFT
*7
Press the [INTER PT] menu key for unknown coordinates of the intersecting point of tapering and convex arc. Enter the tapering angle. Press the [INTER PT] menu key for unknown FPT-Z of the convex arc.
In general, even an unknown coordinate of arc end point can be calculated with the intersecting point of tapering and arc remaining unknown. Enter the radius of convex arc. *4. Enter the center coordinates of convex arc. *5. *6, 7 Press the menu key [UP], [DOWN], [LEFT] or [RIGHT] at the items R/th. and RGH to specify one of the two possible intersecting points of arc and tapering. Press at R/th the [RIGHT] (or [DOWN]) menu key to specify (a) from among the two intersecting points of tapering and convex arc. Press at RGH the [LEFT] menu key to specify (d) from among the two intersecting points of arc and straight line.
8-14
PROGRAM CREATING/EDITING FUNCTIONS
8-3
8
Automatic Cutting-Conditions Setting Function For machining units except for manual program machining units, the items of cutting conditions can be automatically set upon specifying a tool for the respective unit. The automatic setting is performed using the data registered on the CUTTING CONDITION displays and other various parameters (refer to the table shown below for details of the calculation expressions). If the programmed feedrate or surface speed is modified using the VFC function, the new modified value will be stored together with the corresponding basic conditions (machining mode, materials type of workpiece and tool, outside diameter and length of workpiece) into the system memory. Those modified values will then be given priority in the next and subsequent autosettings (and displayed in reverse form) if the basic conditions agree with the stored ones. Example:
For BAR OUT roughing
Before VFC UNo.
MAT.
0
CBN STL
100.
0.
UNo.
UNIT
PART
POS-B
CPT-X
CPT-Z
FIN-X
FIN-Z
90.
100.
0.
0.
0.
1
BAR
SNo.
OD-MAX ID-MIN LENGTH WORK FACE ATC MODE
OUT
TOOL
NOM.
40.
0.
RPM
0
LTUR DIA
2000
No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X
R 1 GENERAL OUT 45. A
0
3.
!
!
!
FIN-Z
C-SP
FR
!
100
0.3
M M M
After VFC UNo.
MAT.
0
CBN STL
100.
0.
40.
UNo.
UNIT
PART
POS-B
CPT-X
CPT-Z
FIN-X
FIN-Z
90.
100.
0.
0.
0.
1 SNo.
BAR
OD-MAX ID-MIN LENGTH WORK FACE
OUT
TOOL
NOM.
R 1 GENERAL OUT 45. A
ATC MODE
RPM
0
2000
0.
No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X 0
3.
!
!
!
LTUR DIA
FIN-Z
C-SP
FR
!
120
0.33
M M M
Registered with “cermet” on the TOOL DATA display
After modification of programmed data using the VFC function during machining, the new values of cutting conditions (surface speed, etc.) will be stored together with the basic conditions ( ). If a program, such as (A) shown below, is subsequently created, those new values will be ‘autoset’ since all basic conditions agree with the jointly stored ones. For program (B), which has different basic conditions, the auto-setting function will set values normally calculated using the fixed expressions.
8-15
8
PROGRAM CREATING/EDITING FUNCTIONS
(A) UNo. 0 UNo. 1 SNo.
MAT. OD-MAX ID-MIN LENGTH WORK FACE CBN STL 100. UNIT BAR
0.
PART OUT
TOOL
40.
ATC MODE
RPM
0
2000
0.
POS-B
CPT-X
CPT-Z
FIN-X
90.
100.
0.
0.
NOM.
No. # PAT.
R 1 GENERAL OUT 45. A
DEP-1
DEP-2/NUM. !
0
LTUR DIA
FIN-Z 0. DEP-3 FIN-X FIN-Z C-SP FR M M M !
!
!
Pressing the [AUTO SET] menu key.
UNo.
MAT.
0
CBN STL
UNo. 1 SNo.
UNIT BAR
OD-MAX ID-MIN 100.
0.
PART OUT
TOOL
LENGTH WORK FACE 40.
ATC MODE
RPM
0
2000
0.
LTUR DIA
POS-B
CPT-X
CPT-Z
FIN-X
FIN-Z
90.
100.
0.
0.
0.
NOM.
No. # PAT.
R 1 GENERAL OUT 45. A
DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP
0
!
3.
!
!
!
120
FR
M M M
0.33
Stored data displayed in reverse form
(B) UNo. 0 UNo. 1 SNo.
MAT. 5052 UNIT BAR
OD-MAX ID-MIN LENGTH WORK FACE ATC MODE 30.
0.
PART OUT
TOOL
NOM.
40.
0.
RPM
LTUR DIA
0
2000
POS-B
CPT-X
CPT-Z
FIN-X
FIN-Z
90.
100.
0.
0.
0.
No. # PAT.
R 1 GENERAL OUT 45. A
DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP FR M M M !
0
!
!
!
Pressing the [AUTO SET] menu key.
UNo. 0 UNo. 1 SNo.
MAT. 5052 UNIT BAR TOOL
OD-MAX
ID-MIN LENGTH WORK FACE ATC POS
PART
POS-B
CPT-X
CPT-Z
FIN-X
FIN-Z
90.
100.
0.
0.
0.
NOM.
R 1 GENERAL OUT 45. A
No. # PAT. 0
0.
LTUR DIA
0.
OUT
40.
RPM
30.
2000
DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP 3.
!
!
!
!
FR
MMM
300 0.45
Data calculated using fixed expressions displayed.
Note:
For internally checking the basic conditions for equality, the data of OD-MAX and LENGTH are roughly managed under parametrically specified classification into four groups. If the three classifying values for LENGTH data are 30, 60 and 110 mm (four groups: 0 to 30, 30 to 60, 60 to 110, and from 110 upwards), for example, then the data “75” and “90” will be managed here as equal to each other.
8-16
PROGRAM CREATING/EDITING FUNCTIONS
8
Calculation expressions of auto-setting function Unit BAR CPY CORNER FACING
Calculation expressions C-SP (R) = R-SPD in CUT. COND. (TURN.) display × [R-SPD% (WRKP.) in CUT. COND. (MAT.) display/100] × [R-SPD% (TOOL) in CUT. COND. (MAT.) display/100] C-SP (F) = F-SPD in CUT. COND. (TURN.) display × [F-SPD% (WRKP.) in CUT. COND. (MAT.) display/100] × [F-SPD% (TOOL) in CUT. COND. (MAT.) display/100] FR (R) = R-FEED in CUT. COND. (TURN.) display × [R-FEED% (WRKP.) in CUT. COND. (MAT.) display/100] × [R-FEED% (TOOL) in CUT. COND. (MAT.) display/100] DEP (R) = R-DEPTH in CUT. COND. (TURN.) display × [R-DEP% (WRKP.) in CUT. COND. (MAT.) display/100 × [R-DEP% (TOOL) in CUT. COND. (MAT.) display/100]
T. GROOVE C-SP (R) = R-SPD in CUT. COND. (TURN.) display × [R-SPD% (WRKP.) in CUT. COND. (MAT.) display/100] × [R-SPD% (TOOL) in CUT. COND. (MAT.) display/100] C-SP (F) = F-SPD in CUT. COND. (TURN.) display × [F-SPD% (WRKP.) in CUT. COND. (MAT.) display/100] × [F-SPD% (TOOL) in CUT. COND. (MAT.) display/100] FR =
R-FEED in CUT. COND. (TURN.) display × [R-FEED% (WRKP.) in CUT. COND. (MAT.) display/100] × [R-FEED% (TOOL) in CUT. COND. (MAT.) display/100]
DEP = R-DEPTH in CUT. COND. (TURN.) display × [R-DEP% (WRKP.) in CUT. COND. (MAT.) display/100] × [R-DEP% (TOOL) in CUT. COND. (MAT.) display/100] THREAD
HGT = Thread pitch × K24/10000 (when OUT/FACE/BACK is selected for metric threads) HGT = Thread pitch × K25/10000 (when IN is selected for metric threads) HGT = Thread pitch × K26/10000 (when OUT/FACE/BACK is selected for inch threads) HGT = Thread pitch × K27/10000 (when IN is selected for inch threads) NUMBER = (see the description given afterwards) V = F-SPD in CUT. COND. (TURN.) display × [F-SPD% (WRKP.) in CUT. COND. (MAT.) display/100] × [F-SPD% (TOOL) in CUT. COND. (MAT.) display/100] DEPTH = (see the description given afterwards)
T. DRILL
DEP-1 = Hole diameter (DRL-DIA) × K17/100 DEP-2 = U44/A DEP-3 = U46/A
A = 1000 for metric system 10000 for inch system
V = R-SPD in CUT. COND. (TURN.) display x [R-SPD% (WRKP.) in CUT. COND. (MAT.) display/100] × [R-SPD% (TOOL) in CUT. COND. (MAT.) display/100] FEED = R-FEED in CUT. COND. (TURN.) display × [R-FEED% (WRKP.) in CUT. COND. (MAT.) display/100] × [R-FEED% (TOOL) in CUT. COND. (MAT.) display/100] T. TAP
PITCH = Data based on JIS (Japan Industrial Standards); depends on the nominal diameter of the thread. V = F-SPD in CUT. COND. (TURN.) display × [F-SPD% (WRKP.) in CUT. COND. (MAT.) display/100] × [F-SPD% (TOOL) in CUT. COND. (MAT.) display/100]
8-17
8
PROGRAM CREATING/EDITING FUNCTIONS
Details on calculation expressions for THREAD unit - NUMBER #0,
#0
Metric Inch
3.4 × LEAD + 3.59 MULTI 3.4 × LEAD × 25.4 + 3.59 MULTI
The first decimal is rounded off. #1,
#1
N = （D – a）/D1 (N: any decimals are cut away) If （D – a）/N – D1 > 0.000475, then N = N + 1
#2,
#2
N = （D - a） /D1
2
If a: D: D1: N:
(N: any decimals are cut away)
D – a – D1 × √ Ｎ > 0.000475, then N = N + 1 N
Finishing allowance for threading (parameter) HGT (programmed data) DEPTH (programmed data) NUMBER (solution to be sought)
- DEPTH #0,
#0
If NUMBER is even: 8 × D – 2 (N + 2) × a/2 D1 = 3×N–1 If NUMBER is odd: 2 (N – 2) × (4 × N × D – (N + 1)2 × a/2) D1 = (N – 1) × (3 × N2– 4 × N – 1)
8-4
#1,
#1
D1 = (D – a)/N
#2,
#2
D1 = (D – a)/ √Ｎ
Desk Calculator Functions When entering shapes (sequence data) for a MAZATROL program, add/subtract/multiply/divide operations and calculations using trigonometric functions and/or square roots can be carried out by selecting [Calculator] from the menu bar [Window]. Enter a calculation expression and press the input key one time. The calculation result will then be displayed in the data input area at the bottom right of the display. If the result is correct, press the input key once again. The particular data will then be set at the cursor position. If the result is not correct, enter the correct calculation expression after pressing the data cancellation key (this deletes the entire expression) or the clear key (this deletes character by character). In the menu, the asterisk sign (∗) means multiplication and the slash sign (/) means division.
8-18
PROGRAM CREATING/EDITING FUNCTIONS
8-5
8
Tool Data Window A tool data window can be displayed by pressing the [TOOL DAT WINDOW] menu key while the cursor remains set at a NOM. (NOM-φ), C-SP or FR item for the machining unit. Only the tools corresponding to the current machining unit or the tool sequence are selected and displayed in the window. Data in FW/RV R/L is displayed blue in reversed status, when the tool index angle is set to “reverse”. - Press the page key to view the next page. - Pressing the menu key once again closes the window. Moving the cursor to an item of other data type also closes it. Example 1: UNo. 1 SNo.
Turning tool
UNIT BAR
PART OUT
TOOL
NOM.
POS-B
CPT-X
CPT-Z
FIN-X
FIN-Z
90.
100.
0.
0.
0.
No. # PAT.
DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP FR M M M !
R 1 GENERAL OUT
Example 2:
!
!
!
$
Milling tool
UNo.
UNIT
MODE
POS-B
POS-C
SRV-A
SRV-R
RGH
FIN-A
START
END
3
LINE CTR
ZY
!
45.
5.
10.
7
0.068
OPEN
OPEN
SNo.
TOOL
NOM-φ
No. #
APRCH-1 APRCH-2
TYPE
AFD
DEP-A
DEP-R C-SP FR M M M $
R 1 END MILL
8-19
8 8-6
PROGRAM CREATING/EDITING FUNCTIONS
Tool File Window A tool file window can be displayed by pressing the [TOOL. F WINDOW] menu key while the cursor remains set at a NOM-φ item in the tool sequence data for the end mill, face mill, chamfering cutter, or ball end mill of the milling unit. Only the data for tools corresponding to the current tool sequence are selected from the tool file data registered on the TOOL FILE display and displayed in the window. - Press the page key to view the next page. - Pressing the menu key once again closes the window. Moving the cursor to an item of other data type also closes it. Example: UNo.
MODE
POS-B
POS-C
SRV-A
SRV-R
RGH
FIN-A
FIN-R
START
3
LINE CTR
UNIT
ZY
!
45.
5.
10.
7
0.068
!
OPEN
SNo.
TOOL
NOM-φ
AFD
DEP-A DEP-R C-SP
R 1 END MILL
No. #
APRCH-1
APRCH-2
$
8-20 E
TYPE
FR
END OPEN M M M
SAMPLE PROGRAMS
9
9
SAMPLE PROGRAMS Example 1:
2-axes machining (BAR, T. GROOVE)
Machining drawing
20
10
Unit: mm
15
C5 C2
φ60
5
φ50
Workpiece materials type: CBN STL Workpiece size: φ60 × 60
φ40
T4P314
Program UNo.
MAT.
0
CBN STL
UNo.
UNIT
1 SNo. R 1 F 2
OD-MAX ID-MIN LENGTH WORK FACE ATC MODE 60.
CPT-Z
FIN-X
FIN-Z
60.
0.
0.2
0.1
NOM.
UNIT T.GROOVE TOOL
No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP FR ◆ ◆ ◆ ◆ A 0 2.5 130 0.3 ◆ ◆ ◆ ◆ B 0. 0. 200 0.1
SPT-X ◆
UNIT
3
END
SPT-Z ◆
FPT-X
FPT-Z
F-CNR/$
50.
50.
C 5.
PART POS-B PAT. No. OUT
90.
NOM.
OUT
S-CNR
1 UNo.
LTUR DIA
CPT-X
2 SNo. FIG
RPM 2000
90.
C 2.
GROOVE
0
POS-B
UNo.
F 1
0.
OUT
GENERAL OUT 0.5 GENERAL OUT 0.1 LIN
60.
PART
BAR TOOL
FIG PTN S-CNR 1
0.
3.
A
0
PITCH
WIDTH
10.
5.
2
RGH ▼▼4
FINISH ◆
M M M No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP FR ◆ ◆ ◆ ◆ ◆ 2. 120 0.08
SPT-X
SPT-Z
FPT-X
50. 20. 40. CONTI. REPEAT SHIFT NUMBER 0
R/th ◆
M M M
◆
◆
0
9-1
FPT-Z
F-CNR
ANG
RGH
20. ATC
RETURN
LOW RET.
0
END
END
WORK No.
EXECUTE ◆
9
SAMPLE PROGRAMS
Example 2:
2-axes machining (FACING, BAR, T. GROOVE, THREAD)
Machining drawing 125
25
Unit: mm 70 45
R50
35 C5 M50P2.0
φ80
φ70
C5
φ40
Workpiece materials type: CBN STL Workpiece size: φ80 × 155 L As-finished roughness: ▽▽3 T4P315’
Program UNo.
MAT.
0
CBN STL
UNo. 1 SNo.
OD-MAX ID-MIN LENGTH 80.
0.
ATC MODE
RPM
5.
0
2000
UNIT
PART
POS-B
FIN-Z
FACING
FACE
0.
0.1
TOOL
A
F 2 GENERAL EDGE 0.5
B
FIG 1
PART
2
BAR
OUT
0. 80.
◆
◆
◆
◆
◆
◆
FPT-Z
0.
FIN-Z
0.2
0.1
◆
0.5
A
F 2 GENERAL OUT
0.1
B
FIG PTN
S-CNR
SPT-X
SPT-Z
FPT-X
FPT-Z
2.5
◆
◆
0.3
0.
160
0.1
◆
◆
◆
◆
0.
FIN-Z C-SP
F-CNR/$ R/th
0.3
0.
200
0.1
RGH
LIN
C 5.
◆
◆
50.
45.
◆
▼▼3
LIN
C 5.
◆
◆
70.
70.
◆
▼▼3
70.
70.
80.
125.
50.
▼▼3
UNIT
PART
POS-B
3
T.GROOVE
OUT
90.
SNo.
TOOL
NOM.
F 1
GROOVE OUT
FIG
S-CNR
3.
4 SNo. 1
UNIT THREAD
FINISH
0.
10.
◆
1
No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP ◆
A
2.
◆
SPT-Z
FPT-X
FPT-Z
45.
40.
45.
POS-B CHAMF LEAD
OUT
90. NOM.
OUT
WIDTH
50. PART
TOOL THREAD
0
PITCH
SPT-X
1 UNo.
PAT. No.
0
2.
MULTI
HGT
55
1
1.299
◆
0
10
SPT-X
SPT-Z
FPT-X
FPT-Z
50.
0.
50.
38.
5
END
◆ ANG
◆
◆
◆
FIN-Z C-SP ◆
CONTI.
REPEAT
SHIFT
NUMBER
ATC
RETURN
LOW RET.
0
◆
◆
0
0
END
END
9-2
120
FR
M M M
0.08
RGH
No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X
1. A
1 UNIT
F-CNR
ANG
FIG UNo.
◆
M M M
130
2 UNo.
FR
◆
1 3
M M M
120
▼▼3
FIN-X
No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X 0
FR
◆ RGH
0.
CPT-X CPT-Z
90. NOM.
R 1 GENERAL OUT
◆ FPT-X
5. POS-B
TOOL
2.
◆ SPT-Z
80. UNIT
◆
2
SPT-X
UNo.
LTUR DIA
No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP
NOM.
R 1 GENERAL EDGE 0.5
SNo.
WORK FACE
155.
120
FR
M M M
◆
WORK No.
EXECUTE ◆
SAMPLE PROGRAMS
Example 3:
9
Point milling
Machining drawing 8-φ1.3 depth 14
A
45°
(11) φ1.3 depth 7
B A: Milling of eight oblique holes (A in program) B: Milling of center hole (B in program)
Program UNo. 0 UNo.
A
B
MAT. FC
OD-MAX ID-MIN LENGTH 24.
UNIT
MODE
0.
WORK FACE ATC MODE
37.
POS-B
0.
POS-C
0
DIA
RPM
LTUR DIA
10000
DEPTH
CHMF
1 DRILLING /C 45. 1.3 14. 0. ! SNo. TOOL NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP RGH DEPTH C-SP FR M M M 1 CTR-DR 4. 1.3 90° CTR-DR 10 0.1 ! ! ! 2 DRILL 1.3 1.3 14. 0. 100 PCK2 T 0.65 9 0.019 FIG
PTN
SPT-R/x
SPT-C/y
SPT-Z
NUM.
ANG
Q
R
1
ARC
11.
0.
0.
8
45
0
1
UNo.
UNIT
MODE
POS-B
POS-C
DIA
DEPTH
CHMF
2 DRILLING XC 1.3 7. 0. ! ! SNo. TOOL NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP RGH DEPTH C-SP FR M M M 1 CTR-DR 4. 1.3 90° CTR-DR 10 0.1 ! ! ! 2 DRILL 1.3 1.3 7. 0. 100 PCK2 T 0.65 9 0.019 FIG
PTN
SPT-R/x
SPT-C/y
SPT-Z
NUM.
ANG
1
PT
0.
0.
0.
!
!
UNo. 3
UNIT END
CONTI.
REPEAT
0
◆
SHIFT NUMBER ATC ◆
0
9-3
0
Q
R
! 0
RETURN
LOW RET.
END
END
WORK No.
EXECUTE ◆
9
SAMPLE PROGRAMS
Example 4:
Point/line milling
Machining drawing (39)
* All the holes are 4-M4, 10 deep and 12 in depth of prepared hole.
(37)
D
(16) B
3
B-axis = 78.3 A B-axis = 42.0
9
12
C
(29.614)
(5.388)
(7)
8
12
A: Milling of the oblique face (A in program) B: Oblique tapping in the groove (B in program) C: Oblique tapping (C in program) D: Tapping (D in program)
Program UNo. MAT. 0 FC
A
OD-MAX ID-MIN LENGTH WORK FACE ATC MODE RPM LTUR DIA 58. 0. 320. 0 0 10000
UNo. UNIT MODE POS-B POS-C SRV-A SRV-R RGH FIN-A 6 LINE CTR /Y 78.3 180. 2. 6. 1 0. SNo. TOOL NOM-φ No. # APRCH-1 APRCH-2 TYPE AFD DEP-A R 1 END MILL 20. A ? ? ◆ G01 2. FIG PTN SHIFT-Z SHIFT-R X Y R/th I J 1 LINE 0. 3. 0. 0. 2 LINE ! ! 29.614 0.
START END CLOSED CLOSED DEP-R C-SP FR M M M ◆ 100 0.2 P CNR R-FEED RGH
UNo.
B
C
D
UNIT MODE POS-B POS-C NOM. MAJOR-φ PITCH TAP-DEP CHMF TAPPING /Y 78.3 180. M 4. 4. 0.7 10. 1. SNo. TOOL NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP RGH DEPTH C-SP 1 CTR-DR 4. 10 ! ! ! 90° CTR-DR 10 2 DRIL 3.4 3.4 12. 0. 100 T 1.7 9 3 TAP M 4. J 4. 10. TAP ! FIX P 0.7 10 FIG PTN SHIFT-Z SHIFT-R SPT-X SPT-Y CX/PX CY/PY F M N ANG 1 PT 0. 3. 12. 0. ! ! ! ! ! !
FR M M M 0.1 0.037 0.7 P Q R 0 ! 0
UNo. 3 SNo. 1 2 3 FIG 1
UNIT MODE POS-B POS-C NOM. MAJOR-φ PITCH TAP-DEP CHMF TAPPING /Y 42.0 180. M 4. 4. 0.7 10. 1. TOOL NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP RGH DEPTH C-SP CTR-DR 4. 10 ! ! ! 90° CTR-DR 10 DRIL 3.4 3.4 12. 0. 100 PCK1 T 1.7 9 TAP M 4. J 4. 10. TAP ! FIX P 0.7 10 PTN SHIFT-Z SHIFT-R SPT-X SPT-Y CX/PX CY/PY F M N ANG LIN 37. 9. 5.388 -7. 14 ! ! 2 ! 90.
FR M M M 0.1 0.037 0.7 P Q R 0 0 1
UNo. 4 SNo. 1 2 3 FIG 1
UNIT MODE POS-B POS-C NOM. MAJOR-φ PITCH TAP-DEP CHMF TAPPING ZC ! ! M 4. 4. 0.7 10. 1. TOOL NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP RGH DEPTH C-SP FR M M M CTR-DR 4. 10 ! ! ! 90° CTR-DR 10 0.1 DRIL 3.4 3.4 12. 0. 100 PCK1 T 1.7 9 0.037 TAP M 4. J 4. 10. TAP ! FIX P 0.7 10 0.7 PTN SPT-R/x SPT-C/y SPT-Z SPT-Y NUM. ANG Q R PT 16. 0. 39. 0. ! ! ! 0
UNo. 3
UNIT END
CONTI.
REPEAT
0
◆
SHIFT NUMBER ATC ◆
0
9-4
0
RETURN
LOW RET.
END
END
WORK No.
EXECUTE ◆
SAMPLE PROGRAMS
Example 5:
Workpiece transfer
Machining drawing
6-φ5 hole drilling depth 10
60°
6-φ8 hole drilling depth 15 15
60°
10
φ58
150°
φ66
13.5° φ60 φ40
φ75
Machining outline B E C F
D
A
F C E B
Program outline UNo. 0
Commen data
UNo. 1
HEAD unit
UNo. 2
Maschining unit A
UNo. 3
Maschining unit B
UNo. 4
Maschining unit C
UNo. 5
TRANSFER unit
(Head selection: Independent machining with SP1)
(Machining at the SP1 side)
(CHUCK)
9-5
UNo. 6
HEAD unit
UNo. 7
Maschining unit D
UNo. 8
Maschining unit E
UNo. 9
Maschining unit F
UNo. 10
END unit
(Head selection: Independent machining with SP2)
(Machining at the SP2 side)
9
9
SAMPLE PROGRAMS
Program UNo. MAT. OD-MAX POS-B LENGTH WORK FACE ATC MODE RPM LTUR DIA 0 CBN STL 75. 0. 62. 1. 0 1500 UNo. UNIT TYPE HEAD SPDL 1 HEAD SIN 1 ! UNo. UNIT PART POS-B FIN-Z 2 FACING FACE 0. 0.1 SNo. TOOL NOM. No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP FR M M M ◆ ◆ ◆ ◆ ◆ 120 0.25 R 1 GENERAL EDGE 0.5 A 2 2. ◆ ◆ ◆ ◆ ◆ 0. 160 0.2 F 2 GENERAL EDGE 0.5 B FIG SPT-X SPT-Z FPT-X FPT-Z RGH ▼▼4 1 75. 1. 0. 0. UNo. UNIT PART POS-B CPT-X CPT-Z FIN-X FIN-Z 3 BAR OUT 90. 75. 0. 0.2 0.1 SNo. TOOL NOM. No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-X C-SP FR M M M 150 0.25 R 1 GENERAL OUT 0.5 A 0 2.5 ! ! ! ! 0. 0. 250 0.1 F 2 GENERAL OUT 0.1 B ! ! ! ! FIG PTN S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ R/th RGH ▼▼4 1 LIN 60. 15. ! ! ! ▼▼4 2 TPR 60. 15. 75. 27.99 UNo. UNIT MODE POS-B POS-C DIA DEPTH CHMF 4 DRILLING /C 60. 8. 15. 0. ! SNo. TOOL NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP RGH DEPTH C-SP FR M M M 1 CTR-DR 20. 10. 90° CTR-DR 25 0.09 ! ! ! 2 DRILL 8. 8. 15. 0. 100 DRIL T 4. 25 0.129 FIG PTN SPT-R/x SPT-C/y SPT-Z NUM. ANG Q R 1 ARC 33. 0. 20.196 6 60. 0 0 UNo. UNIT PAT. HEAD SPDL PUSH CHUCK W1 W2 Z-OFFSET C1 C2 C-OFFSET LTUR ESC TNo. 5 TRANSFER CHUCK 1→2 4 1 -1020 0 760 0. 0. 0. -430. ! UNo. UNIT TYPE HEAD SPDL 6 HEAD SIN 2 ! UNo. UNIT PART POS-B FIN-Z 7 FACING BACK 180. 0. SNo. TOOL NOM. No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP FR M M M R 1 GENERAL EDGE 0.5 C 1. 150 0.3 ! ! ! ! ! FIG SPT-X SPT-Z FPT-X FPT-Z RGH ▼▼4 1 75. -61. 0. -60. UNo. UNIT PART POS-B CPT-X CPT-Z FIN-X FIN-Z 8 BAR OUT 90. 75. 60. 0.2 0.1 SNo. TOOL NOM. No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP FR M M M R 1 GENERAL OUT 0.5 C 0 1.5 150 0.3 ! ! ! ! F 2 GENERAL OUT 0.1 D 0. 0. 196 0. ! ! ! ! FIG PTN S-CNR SPT-X SPT-Z FPT-X FPT-Z F-CNR/$ R/th RGH ▼▼4 1 LIN 40. 50. ! ! ! ▼▼4 2 TPR 40. 50. 75. 32.5 45. UNo. UNIT MODE POS-B POS-C DIA DEPTH CHMF 9 DRILLING /C 135. 5. 10. 0.3 ! SNo. TOOL NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP RGH DEPTH C-SP FR M M M 1 CTR-DR 20. 5.6 90° CTR-DR 25 0.09 ! ! ! 2 DRILL 5. 5. 10. 0. 100 DRIL T 2.5 25 0.088 FIG PTN SPT-R/x SPT-C/y SPT-Z NUM. ANG Q R 1 ARC 29. 0. 41. 6 60. 0 0 UNo. UNIT CONTI. REPEAT SHIFT NUMBER ATC RETURN LOW RET. WORK No. EXECUTE 10
END
0
◆
◆
0
9-6
0
END
END
◆
SAMPLE PROGRAMS
Example 6:
9
Machining with upper and lower turrets
Machining drawing 10 2-M6 depth10
25
φ100 φ20 φ80
C1
30
Unit: mm
D737P0024
Program UNo. 0 UNo. 1 SNo.
MAT.
OD-MAX ID-MIN LENGTH WORK FACE ATC MODE RPM
CST IRN 100. UNIT FACING
0.
101. POS-B
FIN-Z
FACE
0.
0.1 ◆
EDGE
F 2 GENERAL
EDGE 10. B 2
FIG
2
BAR
10. SPT-Z
100.
1.
PART
90.
PTN
1
LIN
2
TPR
UNo.
UNIT
3
TAPPING
SNo.
TOOL
1
CTR-DR
2
DRIL
3
TAP
FIG 1 UNo. 4
PTN ARC UNIT END
S-CNR
MODE
◆
◆
◆
FIN-Z
0.
0.2
0.1
◆
2
◆
1.5 ◆
SPT-Z
◆
FPT-X
FPT-Z
◆
◆
20.
10.
80.
10.
100.
30.
◆
◆
◆
◆
◆
0.
F-CNR/$
6.
2
M6. 25.
◆
8.134
12.
SPT-R/x
0.15
0.
200
0.1
1. ◆
◆
12.
0.
100
6.
10.
TAP
◆
0.
CONTI.
REPEAT
0
◆
SPT-Z 10. SHIFT NUMBER ATC ◆
0
9-7
0
M M M
150
0.17
0.
200
0.1
R/th
RGH
◆
▼▼3
CHMF
10.
5.1 SPT-C/y
FR
◆
▼▼3
NOM. MAJOR-φ PITCH TAP-DEP M6.
M M M
150
▼▼3
0.
1.5
NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP 5.1 D
FR
◆ RGH
FIN-X
1
POS-B POS-C
XC
◆
CPT-Z
100.
SPT-X
C 1.
◆
FPT-Z
0.
5.
F 2 GENERAL OUT 10. B FIG
◆
No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP
NOM.
R 1 GENERAL OUT
◆ FPT-X
POS-B CPT-X
OUT
TOOL
1.5
◆
SPT-X
1
SNo.
LTUR DIA
1500
NOM. No. # PAT. DEP-1 DEP-2/NUM. DEP-3 FIN-X FIN-Z C-SP
TOOL
UNIT
0
PART
R 1 GENERAL
UNo.
1
RGH 90°
DEPTH C-SP
FR M M M
CTR-DR
59
0.09
DRIL T 2.55
25
0.08
39
1.
FIX
P1.
NUM.
ANG
Q
R
2
180.
0
0
RETURN
LOW RET.
END
END
WORK No.
EXECUTE ◆
9
SAMPLE PROGRAMS
- NOTE -
9-8 E
THREE-DIGIT G-FORMAT
10
10 THREE-DIGIT G-FORMAT 10-1 Outline The three-digit G-format is a format of expressing MAZATROL program data and other NC data. The various types of data within the NC unit are each assigned to a specific “three-digit G + address + data” set. Use of the data input/output functions based on the three-digit G-format allows the NC-stored data to be managed under the same environment as those of EIA/ISO programs. Data that have been output to external units in the three-digit G-format can be edited using a personal computer, and if the edited data are restored into the NC unit, the corresponding original data within the NC unit will be auto-modified according to the required edition.
10-2 Detailed Description 1.
MAZATROL program data - Unit data have an assigned specific three-digit G-code for each unit. - Tool sequence data succeed the block of the three-digit G-code of the Unit data and are positioned between code G424, which denotes the beginning of the sequence data, and code G425, which denotes the end of the sequence data. - The shape data, if present, succeed the block of the three-digit G-code of sequence data and are positioned between code G420, which denotes the beginning of the shape data, and code G421, which denotes the end of the shape data. - The TPC data, if present, succeed the block of the three-digit G-code of the Unit data and are positioned between code G422, which denotes the beginning of TPC data, and code G423, which denotes the end of TPC data. - The order of output of the machining program data is predetermined. That is, Unit data, TPC data (barrier information included), sequence data and shape data are output in that order. Do not change the order. - Machining set-up information is keyed to the address that immediately succeeds code G426. - Process layout information is keyed to the address that immediately succeeds code G427. - The output data of machining programs may include additional lower digits which are not displayed on the screen. This is the case, for example, with the values of approach point or crossing point which are automatically calculated and internally used by the NC unit. Such data should not therefore be modified with respect to the displayed data. Example: SNo. 1
TOOL END MILL
NOM-φ
APRCH-1
APRCH-2
1.234
2.345
10.A
Displayed data
Output data N1T15D10.S1 X&1.2345 Y&2.3455 ~ Output longer by one digit than displayed.
10-1
10
THREE-DIGIT G-FORMAT
2.
Data on the TOOL OFFSET, TOOL DATA, TOOL FILE, PARAMETER, MACRO VARIABLE, CUTTING COND. and WORK OFFSET displays, etc. - The code G10 is used to input/output the above data. The codes for data identification are listed up and described in detail on the following pages.
10-3 Three-Digit G-Format of MAZATROL Program 1.
Program number and program name In the three-digit G-format input/output of MAZATROL programs, the number and name of a program is described in the following format:
(Without program name) EOB
Program No. O99999999
( M G 3 — 2 5 1 )
EOB
Description in
EOB EOR
3-digit G-format
%
Identifier (With program name) EOB
Program No. O99999999
( M G 3 — 2 5 1 :
Program name
)
EOB
Description in 3-digit G-format
EOB EOR %
Identifier
- Program number The program number is assigned following “O”. - Identifier The code “(MG3-251)” succeeding the program number identifies a MAZATROL program described in the three-digit G-format of the MAZATROL MATRIX. - Program name The program name is assigned in the parentheses with the identifier separated by a colon. The maximum available number of characters is usually 48 for naming a program stored in the NC memory. An excess in characters will be given away.
10-2
THREE-DIGIT G-FORMAT
2.
10
Special unit A.
Common unit
G300
- Unit data UNo. U
Program type
ODMAX
MAT
P
()
X
ID-MIN I
WORK FACE
LENGTH Z
ATCMODE
C
A
LTUR DIA
RPM S
J
1: MTPro
B.
End unit
G301
- Unit data UNo. CONTI.
REPEAT SHIFT NUMBER
U
K
B
I
ATC
RETURN
C
A
D
0: No
0: No
0: None
0: None
1: Yes
1: Yes
1: ATC → Axis feed 1: END
LOW RET. WORK No. EXECUTE L
()
E 0: No 1: Yes
2: Axis feed → ATC 2: FEXED PT 3: ARB PT 4: ESC 1 5: ESC 2
- Sequence data (Setting retraction position) SNo.
DATA-1
N
?
・・・
DATA-9
・・・
?
For example, set as follows: “X12345.6789”. For axis name of 2 characters, the second characters 1 to 3 are converted to A to C respectively. Ex. To set “123.456” for the X2-axis: “XB123.456”
C.
Subprogram unit G303 - Unit data UNo.
U
Measuring flag F
WORK No. ()
$
NUM. Turret
V
L
0: Including measurement
0 to 9:
1: Not including measurement
–1 to –4: Multi-workpiece machining(A to D)
K
1 to 99: Simultaneous machining No.
Unit skip (0 to 9)
- Sequence data SNo. N
ARGM 1 ?
ARGM 2 ?
ARGM 3 ?
ARGM 4 ?
ARGM 5 ?
ARGM 6 ?
Address and data are set as specified, e.g. “X123.456.” (If macro variable has been specified, “X#100” is used.)
10-3
# Q
101:
Lower turret retraction position 1
102:
Lower turret retraction position 2
111:
Lower turret retraction position 1
112:
Lower turret retraction position 2
10
THREE-DIGIT G-FORMAT
D.
Manual program machining unit G382 - Unit data UNo.
TOOL
Tool shape
U
T
&T
T:
Tool name
NOM-φ D
&T:
Suffix
Turret
S
K
Tool shape
S:
# Q
Suffix
K:
CTR-DR
1
OUT
2
DRILL
2
IN
3
REAMER
3
EDGE
8
H
4
TAP (M)
4
IN
9
J
5
TAP (UN)
5
EDGE
6
TAP (PT)
17
001
13
N
101
Balanced cutting B2
7
TAP (PF)
18
002
14
P
110
Turret-2 retraction pos. 1
8
TAP (PS)
19
003
111
Turret-2 retraction pos. 2
9
TAP (OTHER)
20
004
24
Z
10
BCK FACE
21
005
-1
A
11
BOR BAR
22
006
12
B-B BAR
23
007
-8
H
13
CHAMFER
24
008
-9
J
14
FCE MILL
25
009
15
END MILL
-13
N
16
OTHER
-14
P
-24
Z
CHIP VAC
18
TOL SENS
19
BAL EMIL
33
GENERAL
34
GROOVE
35
THREAD
36
T-DRILL
37
T-TAP (M)
38
T-TAP (UN)
39
T-TAP (PT)
40
T-TAP (PF)
41
T-TAP (PS)
42
T-TAP (OTHER)
43
SPECIAL
A
Turret
1
17
1
No. P
0
Turret 1
1
Turret 2
Q: 1 to 99
Turret 2 Simultan. machining No.
P:
Priority No.
0
None
1 to 99
Priority machining
–1 to –99 Subsequent machining
- Sequence data SNo. N
G1 G
G2 &G
DATA-1 ?
…. ….
DATA-6 ?
S S
M/B M/B
Address and data are set as specified, e.g. “X123.456.”
10-4
THREE-DIGIT G-FORMAT
E.
M-code unit
10
G302
- Unit data UNo. U
No. (Priority No.)
Turret
P
K
0: None
0: Upper turret
1 to 99: Priority machining
1: Lower turret
M1 MA
…. ….
M12 ML
–1 to –99: Subsequent machining
F.
Coordinates measuring unit G304 - Unit data UNo. U
TOOL T
Tool shape
NOM-φ
&T
D
Suffix S
Turret
Priority No.
R
P
U. SKIP K
$ (External unit skip) V
G.
Process end unit G385 - Unit data UNo.
U
H.
Materials shape unit
G307
- Unit data UNo.
Shape
U
E 1: OUT 3: IN
- Shape sequence data SNo. N
PTN A
SPT-X X
SPT-Z Z
FPT-X &X
FPT-Z &Z
1: LIN 2: TPR 3: 4:
10-5
RADIUS I
# (Lower turret setting) W
10
THREE-DIGIT G-FORMAT
I.
Workpiece measuring unit
G308
- Unit data UNo. U
COMPENSATE OFS-TOOL
OFS-TOOL OFS-TOOL Shape Nom. dia./size
H
&T
T
D
OFS-TOOL Suffix I
OFS-TOOL Turret C
COMP.DATA J
0: Yes
0: Diameter
1: No
1: Length
SNSTOOL K
SNS-TOOL Nom. dia
SNS-TOOL SNS-TOOL Suffix Turret
R
S
E
Priority No. P
# (Lower turret INTERVAL retraction) W
L
OUTPUT Q 0: No output 1: HD 2: Printer
- Sequence data (Internal measurement) SNo. N
PTN A
SPT-X X
SPT-Y Y
SPT-Z Z
FPT-X &X
FPT-Y
FPT-Z
&Y
&Z
1: OUTER X
0: Diameter
2: OUTER Y
1: Length
3: INNER X 4: INNER Y
T LIM+
5: X GRV
V
T LIM– W
BASE
Approach
Head angle
Q
L
R
6: Y GRV
0: SPT
0: Z direction
7: Z GRV
1: FPT
1: X direction
8: X WIDTH 9: Y WIDTH 10: Z WIDTH 11: +X STEP 12: –X STEP 13: +Y STEP 14: –Y STEP 15: +Z STEP 16: –Z STEP 17: IN WIDTH 18: IN GRV
- Sequence data (External measurement) SNo. N
PTN
COMP.DATA
A
I
19: EXT MIL
0: WEAR X
20: EXT TURN
1: WEAR Z
MEASURING POINT J
TARGET DATA K
10-6
T LIM+ V
T LIM– W
THREE-DIGIT G-FORMAT
J.
Workpiece transfer unit
10
G309
- Unit data UNo. U
PAT.
HEAD
SPDL
CHUCK
P
H
S
J
K
1: CHUCK
0: Spindle stop
0: With pushing
0: Chuck open
2: BAR
1: 1→2
1: Spindle forward
1: Without pushing
1: Chuck close
3: MOVE
2: 2→1
2: Spindle reverse
3: Spindle orient
1: HEAD1
4: C-axis positioning
2: HEAD2
5: Spindle mov. keep
W1/Z1 W2/Z2 Z-OFFSET ZA
K.
PUSH
ZB
Head selection unit
L
C1 CA
C2 CB
C-OFFSET LTUR ESCZ X LTUR ESC Z P
X
Z
TNo. R
G310
- Unit data UNo. U
TYPE
HEAD
SPDL
Turret
P
H
L
K
1: SIN
1: HEAD1
0: THE OTHER SPDL SYNCRO
0: TR1
2: SYNC
2: HEAD2
1: THE OTHER SPDL STOP
1: TR2
3: CROSS
L.
Tool measuring unit
G311
- Unit data UNo. U
COMPENSATE H
OFS-TOOL T
Tool shape &T
Nom.dia./size D
Suffix
Turret
S
K
Priority No. P
0: Yes 1: No Lower turret retraction
INTERVAL
W
L
- Sequence data SNo. N
PTN
T-LIM-X
A
T-LIM-Z
V
W
Q
R
0: Retract
←:0
2: TOOL EYE #1
1: Not retract
↓:90 →:180
4: TOOL EYE #3 5: TOOL EYE #4
Simultaneous machining unit
G312
- Unit data UNo. U
DIR
1: Laser
3: TOOL EYE #2
M.
TOOL EYE
Priority No. P
SIMUL.No. L
RPM S
10-7
OUTPUT Q
10
THREE-DIGIT G-FORMAT
N.
2-workpiece machining unit G313 - Unit data UNo.
U
3.
PAT.
SP1/SP2
A
B
0: START
0: HI/LOW
1: END
1: LOW/HI
Turning units A.
Bar-materials machining unit
G320
- Unit data UNo. U
PART
POS-B
E
B
CPT-X X
CPT-Z Z
FIN-X
FIN-Z
&X
&Z
1: OUT (Outside-diameter open type) 2: OUT (Outside-diameter middle type) 3: IN (Inside-diameter open type) 4: IN (Inside-diameter middle type) 5: FACE (Front-face open type) 6: FACE (Front-face middle type) 7: BACK (Back-face open type) 8: BACK (Back-face middle type)
B.
Copy-machining unit
G321
- Unit data UNo. U
PART E
POS-B B
CPT-X X
CPT-Z Z
SRV-X I
Refer to “Bar-materials machining unit”.
C.
Corner-machining unit
G322
- Unit data UNo. U
PART E
POS-B B
FIN-X &X
FIN-Z &Z
Refer to “Bar-materials machining unit”.
D.
Facing unit
G323
- Unit data UNo. U
PART E
POS-B B
FIN-Z &Z
Refer to “Bar-materials machining unit”.
10-8
SRV-X J
FIN-X &X
FIN-Z &Z
THREE-DIGIT G-FORMAT
E.
Threading unit
G324
- Unit data UNo. U
PART E
POS-B B
CHAMF
LEAD
C
K
ANG D
MULTI R
HGT H
1: 45°
Refer to “Bar-materials machining unit”.
F.
Grooving unit
2: 60°
G325
- Unit data UNo. U
PART E
POS-B B
PAT. I
No. K
PITCH F
0: #0 (Right-angled or oblique)
Refer to “Bar-materials machining unit”.
1: #1 (Isosceles trapezoidal) 2: #2 (Right-tapered) 3: #3 (Left-tapered) 4: #4 (Right-corner cut-off) 5: #5 (Left-corner cut-off)
G.
Turning drilling unit
G326
- Unit data UNo. U
PART E
POS-B B
DIA D
Refer to “Bar-materials machining unit”.
H.
Turning tapping unit
G327
- Unit data UNo. U
PART E
POS-B B
NOM. *
PITCH F
Refer to “Tapping unit”. Refer to “Bar-materials machining unit”.
10-9
WIDTH J
FINISH/ Overshoot Z
10
10
THREE-DIGIT G-FORMAT
I.
Bar-materials machining/Copy-machining/Corner-machining/Facing unit - Sequence data (turning tool) SNo. N
Tool shape
TOOL T
&T
Nom. dia./ size D
Suffix S
Turret K
Priority No. P
#
PAT.
L
Q
1 to 99: Simultan. machining No. 100: Balanced cut (cut × 2) 101: Balanced cut (feed × 2) 110: Lower turret retraction pos. 1 111: Lower turret retraction pos. 2
DEP-1 RA
DEP-2/ NUM. RB
DEP-3 RC
No. of cut passes E
FIN-X X
FIN-Z Y
C-SP I
FR J
M
M
M
MA
MB
MC
R/F F R: 0 F: 1
PAT. Q
BAR and CORNER units
0
Normal cycle
#0 STANDARD (Standard pattern)
Drilling cycle (blind hole)
1
High-speed roughmachining cycle
#1 CONST. DEPTH (Constant-threading pattern)
Deep-hole drilling cycle (blind hole)
2
Inside diameter enlarging #2 CONST. AREA cycle (Area-constant pattern)
High-speed deep-hole drilling cycle (blind hole)
3
Normal + Chip cutting cycle
Reaming cycle (blind hole)
4
High-speed + Chip cutting #1 CONST. DEPTH cycle (zigzag threading)
5
THREAD unit
#0 STANDARD (zigzag threading)
#2 CONST. AREA (zigzag threading)
T.DRILL unit
Ultra-deep-hole drilling cycle (blind hole) Drilling cycle (through-hole)
6
Deep-hole drilling cycle (through-hole)
7
High-speed deep-hole drilling cycle (through-hole)
8
Reaming cycle (through-hole)
10-10
THREE-DIGIT G-FORMAT
J.
10
Bar-materials machining/Copy-machining unit - Sequence data (Shape) FIG
PTN
N
S-CNR
A
C/R
SPT-X
SPT INTER PT
SPT-Z
X
Z
K
F-CNR/$
FPT-X
FPT-Z
&C/&R/Q &X
&Z
FIN INTER PT L
1: LIN
1: UP
1: UP
2: TPR
2: DOWN
2: DOWN
3:
3: LEFT
3: LEFT
4:
4: RGT
4: RGT
5: CTR FGH/ Feedrate set flag
R/th I/J
Feedrate
E
INTER PT flag
0: ROUGHNESS
F
H bit0=1: SPT-X?
1: FEEDRATE/rev
bit1=1: SPT-Z? bit2=1: FIN-X? bit3=1: FIN-Z? bit4=1: SPT-X CONT? bit5=1: SPT-Z CONT? bit6=1: FIN-X CONT? bit7=1: FIN-Z CONT?
K.
Corner-machining unit - Sequence data (Shape) FIG
N
L.
SPT-X X
SPT-Z
F-CNR/$
Z
FPT-X
&C/&R/Q
FPT-Z
&X
&Z
RGH code E
Feedrate F
Facing unit - Sequence data (Shape) FIG N
M.
SPT-X X
SPT-Z
FPT-X
Z
&X
FPT-Z &Z
RGH code E
Feedrate F
Threading unit - Sequence data (Shape) FIG
N
N.
SPT-X X
SPT-Z
FPT-X
Z
&X
FPT-Z &Z
Grooving unit - Sequence data (Shape) FIG
N
S-CNR C/R
SPT-X X
SPT-Z Z
F-CNR &C/&R
FPT-X &X
10-11
FPT-Z &Z
ANGLE J
RGH code E
Feedrate INTER PT flag F
H
10
THREE-DIGIT G-FORMAT
O.
Turning drilling/Turning tapping unit - Sequence data (Shape) FIG
N
4.
FPT-X
FPT-Z
&X
&Z
Milling units A.
Point machining unit - Drilling unit G350
UNo. U
MODE
POS-B
Q
Y
65:ZC
69:XY
73:/Y
66:XC
70:XY
74:/Y
67:XC
71:/C
68:ZY
72:/C
- Counterbore machining unit UNo. MODE U
POS-C
POS-B
Q
Y
W
DEPTH
D
CHMF
H
C
G351
POS-C W
DIA
CB-DIA &D
CB-DEP &H
CHMF C
BTM
DIA
F
D
DEPTH H
Refer to “Drilling unit”.
- Inversed faced hole machining unit G352 UNo. U
MODE
POS-B
Q
POS-C
Y
W
CB-DIA &D
CB-DEP &H
DIA D
DEPTH CHMF H
C
Refer to “Drilling unit”.
- Reaming unit UNo. U
MODE
G353 POS-B
Q
Y
POS-C
DIA
W
D
DEPTH H
CHMF C
PRE-REAM A 1: Drilling 2: Boring
Refer to “Drilling unit”.
- Tapping unit UNo. MODE U
Q
G354
POS-B Y
3: End milling
POS-C W
NOM. *
MAJOR-φ E
PITCH P
TAP-DEP H
CHMF C
Refer to “Drilling unit”. Tap screw type A:
Example: M10. UNn 1-2
Tap fraction B
1
M
1
1/2
2
UNn
2
1/4
3
UN
3
1/8
A1D10.
4
PT
4
1/16
A2D1V2
5
PF
Nominal dia. D: Nominal dia. 2 V:
UN 1H-2
A3D1V2B1
6
PS
PT 2Q
A4D2B2
7
OTHER
10-12
10
THREE-DIGIT G-FORMAT
- Through hole boring unit G358 UNo.
MODE POS-B
U
Q
Y
POS-C W
DIA D
DEPTH
CHMF
H
C
WAL J
Refer to “Drilling unit”.
- Non-through hole boring unit G359 UNo.
MODE
U
Q
POS-B Y
POS-C W
DIA D
DEPTH
CHMF
H
C
BTM WAL I
J
PRE-DIA E
Refer to “Drilling unit”.
- Stepped through hole boring unit G360 UNo.
MODE
U
Q
POS-B Y
POS-C W
CB-DIA &D
CB-DEP
CHMF
&H
&C
BTM WAL &I
&J
DIA
DEPTH CHMF
D
H
C
WAL J
Refer to “Drilling unit”.
- Stepped non-through hole boring unit UNo.
MODE
U
Q
POS-B Y
POS-C
CB-DIA
W
&D
G361
CB-DEP
CHMF
&H
&C
BTM WAL &I
&J
PRE-DIA E
DIA
DEPTH
D
Refer to “Drilling unit”.
H
CHMF C
BTM I
WAL J
- Back boring unit G355 UNo.
MODE
U
Q
POS-B Y
POS-C W
DIA D
DEPTH H
BTM WAL PRE-DIA I
J
&D
PRE-DEP &H
CHMF WAL C
&J
Refer to “Drilling unit”.
- Circular milling unit G356 UNo. U
TORNA. K
MODE Q
POS-B Y
POS-C DIA W
D
DEPTH H
CHMF BTM PRE-DIA CHMF PITCH1 PITCH2 C
I
&D
&C
E
F
0: CIRCUL 1: TORNADE
Refer to “Drilling unit”.
2: HIGH AC.
- Counterbore-tapping unit G357 UNo. MODE POS-B POS-C NOM. MAJOR-φ PITCH TAP-DEP
CHMF
U
C
Q
Y
W
*
E
P
H
Refer to “Tapping unit”. Refer to “Drilling unit”.
10-13
CB-DIA &D
CB-DEP CHMF BTM
CHP
&H
K
&C
I
10
THREE-DIGIT G-FORMAT
B.
Line machining unit - Central linear machining unit G362 UNo.
U
MODE Q
POS-B POS-C Y
W
SRV-A
SRV-R
Z
R
RGH F
FIN-A
Start/End pt. attribute
&Z
A bit 0: ON = Start pt. CLOSED
Refer to “Drilling unit”.
bit 1: ON = End pt. CLOSED
- Right-hand/Left-hand linear machining unit G363/G364 UNo. U
MODE Q
POS-B POS-C Y
W
SRV-A
SRV-R
Z
R
RGH F
FIN-A
FIN-R
&Z
&R
Start/End pt. attribute A
Refer to “Drilling unit”.
- Outside/Inside linear machining unit UNo. U
MODE Q
POS-B POS-C Y
W
SRV-A
G365/G366
SRV-R
Z
R
RGH F
FIN-A
FIN-R
&Z
&R
Start/End pt. attribute A
Refer to “Drilling unit”.
- Right-hand/Left-hand chamfering unit UNo. U
MODE
POS-B
Q
POS-C
Y
W
G367/G368 INTER-Z
INTER-R
I
J
CHMF C
Start/End pt. attribute A
Refer to “Drilling unit”.
- Outside/Inside chamfering unit UNo. U
MODE Q
POS-B POS-C Y
W
G369/G370
INTER-Z I
INTER-R J
CHMF C
R
1: Rounding
Face machining unit - Face milling unit G371 UNo.
U
MODE Q
POS-B Y
POS-C W
SRV-A Z
BTM I
FIN-A &Z
Refer to “Drilling unit”.
- End milling-top unit G372 UNo. U
MODE Q
POS-B Y
POS-C W
SRV-A Z
BTM I
Refer to “Drilling unit”.
10-14
FIN-A &Z
Start/End pt. attribute A
0: Chamfering
Refer to “Drilling unit”.
C.
R-chamfering flag
THREE-DIGIT G-FORMAT
10
- End milling-step unit G373 UNo. U
MODE
POS-B
Q
POS-C
Y
SRV-A
W
BTM
Z
WAL
I
FIN-A
J
&Z
FIN-R &R
Refer to “Drilling unit”.
- Pocket milling unit G374 UNo. U
MODE Q
POS-B Y
POS-C W
SRV-A
BTM
Z
I
WAL J
FIN-A &Z
FIN-R &R
INTER-R CHMF R-chamfering flag K
C
R 0: Chamfering
Refer to “Drilling unit”.
1: Rounding
- Pocket milling-mountain unit G375 UNo. U
MODE Q
POS-B Y
POS-C W
SRV-A Z
BTM I
WAL J
FIN-A &Z
FIN-R &R
Refer to “Drilling unit”.
- Pocket milling-valley unit G376 UNo. U
MODE
POS-B
Q
Y
POS-C W
SRV-A Z
BTM I
WAL J
FIN-A &Z
FIN-R &R
Refer to “Drilling unit”.
- End milling-slot unit G377 UNo. U
MODE Q
POS-B Y
POS-C W
SRV-A Z
SLOT-WID D
Refer to “Drilling unit”.
10-15
BTM I
WAL J
FIN-A &Z
FIN-R &R
10
THREE-DIGIT G-FORMAT
D.
Tool sequence - Point machining tool sequence Lower turret retraction
SNo. TOOL NOM-φ Suffix Turret Priority No. N
T
D
S
K
P
L
HOLE-φ E
HOLE-DEP H
RGH F
T:
Tool name
&T:
Tool shape
S:
Suffix
PRE-DIA PRE-DEP &E
DEPTH Z
&H
C-SP I
FR J
P:
M
M
M
MA
MB
MC
Priority No.
1
CTR-DR
1
OUT
0
2
DRILL
2
IN
1
A
1 to 99
Priority machining
3
REAMER
3
EDGE
:
:
–1 to –99
Subsequent machining
4
TAP (M)
4
IN (BACK)
8
H
5
TAP (UN)
5
EDGE (BACK)
9
J
L:
Lower turret retraction pos.
6
TAP (PT)
17
001
:
:
110:
Position 1
7
TAP (PF)
18
002
13
N
111:
Position 2
8
TAP (PS)
19
003
14
P
9
TAP (OTHER)
20
004
:
:
10
BCK FACE
21
005
24
Z
11
BOR BAR
22
006
-1
A
12
B-B BAR
23
007
:
:
13
CHAMFER
24
008
-8
H
14
FCE MILL
25
009
-9
J
15
END MILL
:
:
16
OTHER
K:
-13
N
17
CHIP VAC
0
TR1
-14
P
18
TOL SENS
1
TR2
:
:
19
BAL EMIL
-24
Z
33
GENERAL
34
GROOVE
35
THREAD
36
T-DRILL
37
T-TAP (M)
38
T-TAP (UN)
39
T-TAP (PT)
40
T-TAP (PF)
41
T-TAP (PS)
42
T-TAP (OTHER)
43
SPECIAL
Turret
10-16
0
None
THREE-DIGIT G-FORMAT
10
- Line/Face machining tool sequence SNo. TOOL NOM-φ N
T
D
Suffix
Turret Priority No. # APRCH-1 APRCH-2 TYPE ZFD TYPE CPT-Z DEP-R
S
K
P
L
X
Y
Q
F
C-SP
H
FR
I
J
Z
R
M
M
M
MA
MB
MC
Refer to “Point machining tool sequence”.
R/F B 0: R 1: F
X, Y:
APRCH-1, 2
?
Q:
? for auto-set
1
TYPE
F:
1BI
ZFD
–1
G01 G00
H:
Approach type
1
Bidirectional X
&123.456
Auto-set
2
2BI
0
123.456
Normal input
3
1UN
0.1 to 9.9
4 5 6
2BI-S
6
Bidirectiona, arc Y
7
CW
16
CW
8
CCW
17
CCW
E.
2
Bidirectional Y
3
Unidirectional X
2UN
4
Unidirectional Y
1BI-S
5
Bidirectional, arc X
Shape sequence - Linear/face (arbitrary) machining shape sequence ZC PTN
FIG N
A
Z Z
C J
SPT-R I
R/th
I
&R/&C
J
V
W
P
CNR
L
RGH/ Feedrate set flag
R/C/K E
32: LINE
1: LEFT
33: CW
2: RIGHT
34: CCW
3: DOWN
35: FIG-SH
4: UP
36: CW-SH 37: CCW-SH 38: REP-EN RGH code/ Feedrate F
Type of shape
SPT S
? mark
B (1: arbitrary) Q
AUTO SET H
R feedrate &F
- Linear/face (arbitrary) machining shape sequence XC FIG PTN N
A
Control flag P
R/x
C/y SHIFT-Z
I/X
J/Y
Z
R/th
I
&R/&C
J
P
CNR
V/&X W/&Y L R/C/K RGH code/ Feedrate F
10-17
E Type of shape
SPT S
RGH/ Feedrate set flag
B
? mark Q
AUTO R SET feedrate H
&F
10
THREE-DIGIT G-FORMAT
- Linear/face (arbitrary) machining shape sequence XY FIG N
Control flag
PTN A
R/x
P
I/X
C/y J/Y
SHIFT-Z
R/th
Z
RGH/ Feedrate set flag E
I
&R/&C RGH code/ Feedrate F
J
V/&X
P
W/&Y
L
Type of ? mark shape
SPT S
B
Q
CNR R/C/K
AUTO SET H
R feedrate &F
Wall &W
- Linear/face (arbitrary) machining shape sequence ZY FIG N
PTN A
Z Z
Y
SHIFT-Z
Y
I
R/th
I
&R/&C
RGH/ Feedrate set flag E
J
V
W
RGH code/ Feedrate F
P
CNR
L
SPT S
R/C/K
Type of ? mark shape B
Q
AUTO SET H
R feedrate &F
Wall &W
- Linear/face (arbitrary) machining shape sequence /Y FIG N
PTN A
SHIFT-Z Z
SHIFT-R I
X
Y
X
Y
RGH/ Feedrate set flag E
R/th
I
&R/&C
V
RGH code/ Feedrate F
J
SPT S
W
P L
Type of ? mark shape B
Q
CNR R/C/K AUTO SET H
Feedrate, R-feedrate [RGH code input]
[Feedrate input]
0: Surface roughness 0
Unit: mm/10000
1: Surface roughness 1
Input range: 0 to 99.999
inch/100000
2: Surface roughness 2 3: Surface roughness 3
[Rapid feed specified]
4: Surface roughness 4
–1
5: Surface roughness 5 6: Surface roughness 6 7: Surface roughness 7 8: Surface roughness 8 9: Surface roughness 9
Data format for the other shape sequence is same as for conventional type.
10-18
R feedrate &F
Wall &W
THREE-DIGIT G-FORMAT
5.
10
TPC data A.
Parameter A
B
DRILLING
D1
D3
D16 D17
RGH CBOR
D1
D3
D16 D17
RGH BCB
D1
D3
D16 D17
REAMING
D1
D3
D16 D17 D18 D19 D23 D24 D25 D26 D28 D29 D41 D42 D91 D92 D45 D46 TC37 TC38 TC39 TC40
TAPPING
D1
D3
D16 D17 D22
BK-CBORE
D1
D3
D16 D17 D18 D19 D23 D24 D25 D26 D28 D33 D41 D42 D91 D92 D45 D46 TC37 TC38 TC39 TC40
CIRC. MIL
D1
CBOR-TAP
D1
D3
D16 D17 D22 D19 D23 D48 D31 D32 D49 D29 D41 D42 D91 D92 D45 D46 TC37 TC38 TC39 TC40
BORE T1 S1 T2 S2 D1
D3
D16 D17 D18 D19 D23 D24 D25 D26 D28
LINE CTR
E2
E7
E9
E17
E95
TC37 TC38 TC39 TC40
LINE RGT, LFT
E2
E7
E9
E17
E22 E23 E24 E25 E95
TC37 TC38 TC39 TC40
LINE OUT, IN
E1
CHMF RGT, LFT CHMF OUT, IN
E1
C
D
E
E5
H
I
J
K
L
M
P
Q
R
S
D41 D42 D91 D19 D23 D5
D16 D17
E2
F
D19
Y
Z
&C &D &E &X &Y
D45 D46 TC37 TC38 TC39 TC40
D41 D42 D91 D92 D45 D46 TC37 TC38 TC39 TC40 D40
D41 D42 D91 D92 D45 D46 TC37 TC38 TC39 TC40
D48 D31 D32 D49 D29 D41 D42 D91 D92 D45 D46 TC37 TC38 TC39 TC40
D19 D23
D41 D42 D91 D92
TC37 TC38 TC39 TC40
D41 D42 D91 D92 D45 D46 TC37 TC38 TC39 TC40
E7
E9
E17
E21 E22 E23 E24 E25 E95
TC37 TC38 TC39 TC40
E2
E8
E9
E11 E17
E95
TC37 TC38 TC39 TC40
E2
E8
E9
E11 E17
E95
TC37 TC38 TC39 TC40
E9
E12 E15
FCE MILL
E21
TC37 TC38 TC39 TC40
E7
E9
E13 E17
STEP
E1
E2
E5
E7
E9
E16 E17
POCKET
E1
E2
E5
E7
E9
E17 E18 E21 E22 E23 E24 E25 E92
PCKT MT
E1
E2
E5
E7
E9
E17 E18 E21 E22 E23 E24 E25 E93
TC37 TC38 TC39 TC40
PCKT VLY
E1
E2
E5
E7
E9
E17 E18 E21 E22 E23 E24 E25 E94 E98
TC37 TC38 TC39 TC40
E7
E9
E17
TC37 TC38 TC39 TC40
TOP EMIL
SLOT
E9
ANG. FACE L2
E97 E21 E22 E23 E24 E25 E91 E98
E21
E96
E12
TC37 TC38 TC39 TC40 TC37 TC38 TC39 TC40 TC37 TC38 TC39 TC40
TC37 TC38 TC39 TC40
K21 K22
TC37 TC38 TC39 TC40
TC62
WORK MES
K17 K18 K19 K23
TC37 TC38 TC39 TC40
TC62
TOOL MES
K17 K18 K20
TC37 TC38 TC39 TC40
TC62
MMS
L1
&Z
TC44 TC57 TC58 TC59
TRANSFER BAR
TC67 TC68 TC1 TC5 TC6
TC37 TC38 TC39 TC40
TC62
COPY
TC7
TC37 TC38 TC39 TC40
TC62
CORNER
TC67 TC68 TC1
TC37 TC38 TC39 TC40
TC62
TC37 TC38 TC39 TC40
TC62
TC56 TC76 TC1
FACING
TC41 TC77 TC78
TC82
TC37 TC38 TC39 TC40
TC62
T. GROOVE
TC52 TC42 TC43 TC73 TC74
TC75
TC37 TC38 TC39 TC40
TC62
T. DRILL
TC47 TC20 TC11 TC12
TC37 TC38 TC39 TC40
TC62
T-TAP
TC21 TC22
TC37 TC38 TC39 TC40
TC62
THREAD
10-19
10
THREE-DIGIT G-FORMAT
B.
Common data for unit Common/Relay point
Turret
Rough/Finish
Tool rotational position P
C
K
F
0: Relay point section
0: UPPER
0: ROUGH
1: Common data for unit
1: LOWER
1: FINISH
C.
Rotation Rotation Fixed clearance X clearance Z point X XA
ZA
XB
Fixed point Z ZB
Relay point Common/Relay point
Rough/ Finish
Turret
Relay point type
F
Relay point X1 Y1 Z1 X2 Y2 Z2 X3 Y3 Z3 setting
C
K
0: Relay point section
0: UPPER 0: ROUGH 0: APPROACH 0: MANU
A
1: Common data for unit 1: LOWER 1: FINISH
D.
B
1: ESCAPE
XA YA ZA XB YB ZB XC YC ZC
1: AUTO
Barrier information - Barrier information for turning spindle Type
Jaw No.
A
Jaw code/Name
B
Gripping dia.
C/( )
Parts count
E
D
Z offset F
C offset J
0: Turning spindle 1 1: Turning spindle 2
- Barrier information for tailstock Taistock used/ not used
Type
Tailstock barrier
A
H
I
1: (Fixed)
0: Not used
0: Invalid
1: Used
1: Valid
Projection length L
Tailstock pos. 1
End coordinate Z Z
P
Tailstock pos. 2 Q
10-4 Various Data Description Using G10 “G10” is normally used to express the other various data than program data, and address “L” that follows denotes the type of the data. G10L_ Data type
1.
Tool data A.
TOOL DATA 1 - Milling tool G10L40T_H_C_&C_D_I_S_P_A_E_ TNo.
T
Turret H
TOOL C
PART
NOM-φ
&C
D
INTERFER. ID CODE PKNo. I
S
P
LENGTH A
ACT-φ E
- Turning tool (GENERAL, GROOVE, THREAD and OTHER) G10L40T_H_C_&C_D_I_S_P_A_E_B_ TNo. T
Turret H
TOOL C
PART &C
INTERFER.
NOM-φ D
I
10-20
ID CODE S
PKNo. P
LENGTH LENGTH NOSE-R A B A
E
B
THREE-DIGIT G-FORMAT
10
- Turning tool (T-DRILL and T-TAP) G10L40T_H_C_&C_D_I_S_P_A_E_B_ TNo. T
Turret
TOOL
H
C:
PART
C
TOOL
&C
INTERFER. ID CODE PKNo.
NOM-φ D
I
S
TOOL (Section to be machined)
&C:
LENGTH
P
S:
ACT-φ
A
B
Nominal diameter of tap and turning tap
ID code
1 CTR-DR
1 OUT
0
2 DRILL
2 IN
1 A
3 REAMER
3 EDGE
: :
2 UNn
4 TAP (M)
4 IN (BACK)
8 H
3 UN
5 EDGE (BACK)
9 J
4 PT
5 TAP (UN)
A:
Tap screw type 1 M
6 TAP (PT)
17 001
: :
5 PF
7 TAP (PF)
18 002
13 N
6 PS
8 TAP (PS)
19 003
14 P
7 OTHER
9 TAP (OTHER)
20 004
: :
10 BCK FACE
21 005
24 Z
11 BOR BAR
22 006
–1 A
1 1/2
12 B-B BAR
23 007
: :
2 1/4
13 CHAMFER
24 008
–8 H
3 1/8
14 FCE MILL
25 009
–9 J
4 1/16
15 END MILL
B:
Tap fraction
: :
16 OTHER
–13 N
Nominal diameter D:
17 CHIP VAC
–14 P
Nominal diameter 2V：
18 TOL SENS
: :
19 BAL EMIL
–24 Z
33 GENERAL 34 GROOVE
P:
CUT DIR.
35 THREAD
0 None
36 T.DRILL
1 ←RIGHT
37 T.TAP (M)
2 →RIGHT
38 T.TAP (UN)
3 ←LEFT X
39 T.TAP (PT) 41 T.TAP (PS)
A1D10. A2D1V2 A3D1V2B1 A4D2B2
4 →LEFT
Tap function 0: FLOAT 1: FIX
40 T.TAP (PF)
Example M10. UNn 1-2 UN 1H-2 PT 2Q
5 ← 6 →
42 T.TAP (OTHER) 43 SPECIAL
B.
Tool data 2 - Milling tool G10L41T_H_Y_C_P_R_F_D_S_(_)Q_I_V_M_B_ TNo.
T
Turret
LENG COMP.
TAP TYPE
H
Y
C
THRUST F. P
EDGANG
REC. FEED R
F
HOLDER Q
HORSE PW D
BORDER I
MAX. ROT
MAT.
S
()
TIP POS. V
CORNER R M
THEETH B
- Turning tool G10L41T_H_K_A_F_E_(_)Q_J_V_Z_ TNo. T
Turret H
CUT DIR. K
CUT ANGLE/ GRV DEPTH A
EDG-ANG/ TIP-WID F
WIDTH E
10-21
MAT. ()
HLD. TYPE
HOLDER. Q
J
INDEX ANG. V
LBB No. Z
10
THREE-DIGIT G-FORMAT
C.
Tool data 3 G10L42T_H_M_N_P_Q_F_(_)D_E_V_W_X_Y_Z_&X_&Y_&Z_F_A_B_C_I_J_K_ TNo.
T
LIFE TIME
Turret H
M
CUT TIME N
LIFE NUM. P
USED GROUP IDNo. NUM. No. Q
F
()
WEAR COMP X/Y/Z X/Y/Z
2.
ACT-φ CO. D
MAX WEAR &X/&Y/&Z &X/&Y/&Z
Tool offset A.
Type A G10L10H_P_R_
B.
Type B Geometric compensation for tool length ... Wear compensation for tool length ....... Geometric compensation for tool radius ... Wear compensation for tool radius .......
C.
G10L10H_P_R_ G10L11H_P_R_ G10L12H_P_R_ G10L13H_P_R_
Type C Geometric compensation Z ............. Wear compensation Z .................. Geometric compensation for tool radius .... Wear compensation for tool radius ........ Geometric compensation X ............. Wear compensation X.................. Geometric compensation Y.............. Wear compensation Y.................. Direction ............................
D.
G10L10H_P_R_ G10L11H_P_R_ G10L12H_P_R_ G10L13H_P_R_ G10L14H_P_R_ G10L15H_P_R_ G10L16H_P_R_ G10L17H_P_R_ G10L18H_P_R_
Type D Offset Z............................. Tool radius .......................... Offset X ............................. Offset Y ............................. Direction ............................
E.
G10L10H_P_R_ G10L11H_P_R_ G10L12H_P_R_ G10L13H_P_R_ G10L14H_P_R_
Without EIA option Offset Z............................. G10L10H_P_R_ Offset X ............................. G10L11H_P_R_ Offset Y ............................. G10L12H_P_R_ Turret H
Offset No. P
OFFSET R
10-22
LENG. CO.
ACT-φ CO. No. E
V TOOL PROJ
R
LENG. CO. No. W
EASY COMP CONS. COMP X/Y/Z A/B/C
I/J/K
THREE-DIGIT G-FORMAT
3.
10
Tool file A.
End mill and ball-end mill G10L49P_C_D_S_（_）R_H_
Tool file No.
TOOL
P
NOM-φ
C
ID code
D
MAT.
S
( )
DEPTH R
No. H Refer to “Tool data.”
B.
Face mill G10L49P_C_D_S_（_）R_H_F_
Tool file No.
TOOL
P
NOM-φ
C
ID code
D
MAT.
S
( )
DEPTH R
No. H
ANG F Refer to “Tool data.”
C.
Chamfering cutter G10L49P_C_D_S_(_)E_H_M_F_
Tool file No.
TOOL
P
NOM-φ
C
ID code
D
MAT.
S
( )
MIN-φ E
No. H
ANG
R-chamfering flag F
M 0: Chamfering 1: Rounding Refer to “Tool data.”
4.
Cutting condition A.
Cutting condition (WORK MAT) G10L52P_(_) Material No. P
B.
WORK MAT (
)
Milling cutting condition (TOOL MAT, C-SP, FR) G10L_P_S_F_(_) DRILL G10L53
CTR-DR REAMER G10L54
No. P
C.
BOR BAR
B-B BAR
BCK FACE
G10L55 G10L56 G10L57 G10L58 G10L59
SPD S
TAP
FR F
CHAMFER G10L60
END MILL
)
Cutting condition for turning G10L65P_A_B_C_D_ No. P
D.
R-SPD A
F-SPD B
R-FEED C
R-DEP. D
Cutting condition for turning (WORK MATERIAL PERCENTAGE) G10L66P_A_B_C_D_ No. P
R-SPD A
F-SPD B
R-FEED C
R-DEP. D
10-23
BAL EMIL
OTHER
G10L61 G10L62 G10L63 L10L64
TOOL MAT. (
FCE MILL
10
THREE-DIGIT G-FORMAT
E.
Cutting condition for turning (TOOL MATERIAL PERCENTAGE) G10L67P_A_B_C_D_(_) No. P
F.
R-SPD
F-SPD
A
B
R-DEP.
C
TOOL MAT
D
(
)
Cutting condition parameter Cutting condition parameter A1 to A108 Cutting condition parameter B1 to B108 Cutting condition parameter C1 to C108
G10L68A_Z_ G10L68B_Z_ G10L68C_Z_ Parameter address
Setting
A/B/C
5.
R-FEED
Z
Workpiece offset A.
Standard G10L2N_P_ N1 (System 1) to N4 (System 4) Coordinate sytem
Coordinate sytem shifting
P
B.
0
G54
G55
1
G56
2
3
G57 4
G58 5
G59 6
Additional workpiece coordinate system G10L20N_P_ N1 (System 1) to N4 (System 4) P: Axis No.
6.
Axis No.
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
P
X
Y
Z
A
B
C
D
E
F
H
I
J
K
M
N
O
Parameter A.
User parameter G10L50 D1Z1 D2Z2 : G11 Parameter
G10 format
User parameter setting start 1 is set to D1 (example).
User parameter setting end D:
E:
TC:
IO:
D1 to D144 E1 to E144 T1 to T154
H1 to H456 57*8
10-24
I: I1 to I384 24*16
SU:
SD:
F:
A1 to A672 B1 to B168 F1t o F168 168*4
THREE-DIGIT G-FORMAT
B.
Machine parameter Machine parameter setting start 1 is set to J1 (example).
G10L51 J1Z1 J2Z1 M G11
Machine parameter setting end
Parameter
J:
G10 format
K:
L:
M:
J1 to J144 K1 to K144 L1 to L144
SV:
P1 to P2048 256*8
BA:
V1 to V6144 384*16
R register
X1 to X528 132*4
R2100 to R2527 R10500 to R11199 R16176 to R16383
Common variable 100 is set to #100 of the spindle 1 (N: Spindle No. 1 or 2).
G10L44N1#100=100 B.
Common variable (for checking) 100 is set to #100 of the spindle 1 (N: Spindle No. 1 or 2).
G10L45N1#100=100 Pallet management
G10L46P_U_R_W_S_J_N_K_M_A_B_C_D_Q_X_Y_Z_E_ 9.
SA:
Macro variable A.
8.
S:
M1 to M768 N1 to N768 S1 to S768 W1 to W1152 48*16 48*16 48*16 144*8
SP:
7.
N:
Maintenance check A.
Regular check item G10L70P_T_C_Y_M_D__（ ） Check No. P
B.
Target time T
Current time C
Year Y
Month M
Long-term check item G10L70P_（ ） Check No. Check item P
(
)
10-25
Day D
Check item (
)
10
10
THREE-DIGIT G-FORMAT
- NOTE -
10-26 E