Page 1
Page 2
Page 3
MELDAS is registered trademarks of Mitsubishi Electric Corporation.
Other company and product names that appear in this manual are trademarks or registered trademarks of the respective
companies.
Page 4
Page 5
Introduction
CAUTION
This manual is a guide for using the MITSUBISHI CNC M700V/M70V Series.
Programming is described in this manual, so read this manual thoroughly before starting programming. Thoroughly study
the "Precautions for Safety" on the following page to ensure safe use of this NC unit.
Details described in this manual
For items described as "Restrictions" or "Usable State" in this manual, the instruction manual issued by
the machine tool builder takes precedence over this manual.
Items not described in this manual must be interpreted as "no t possible".
This manual is written on the assumption that all option functions are added.
Refer to the specifications issued by the machine tool builder before starting use.
Refer to the Instruction Manual issued by each machine tool builde r for details on each machine tool.
Some screens and functions may differ depending on the NC system (or its version), and some functions
may not be possible. Please confirm the specifications before use.
General precautions
(1) Refer to the following documents for details on handling
MITSUBISHI CNC M700V/M70 Series Instruction Manual ............ IB-1500922
Page 6
Page 7
Precautions for Safety
WARNING
CAUTION
DANGER
Always read the specifications issued by the machine tool builder, this manual, related manuals and attached documents
before installation, operation, programming, maintenance or inspection to ensure correct use.
Understand this numerical controller, safety items and cautions before using the unit.
This manual ranks the safety precautions into "DANGER", "WARNING" and "CAUTION".
DANGER
Note that even items ranked as " CAUTION", may lead to major results depending on the situation. In any case,
important information that must always be observed is described.
Not applicable in this manual.
When the user may be subject to imminent fatalities or major injuries if handling is
mistaken.
When the user may be subject to fatalities or major injuries if handling is mistaken.
When the user may be subject to injuries or when physical damage may occur if
handling is mistaken.
WARNING
1. Items related to operation
If the operation start position is set in a block which is in the middle of the program and the program is
started, the program before the set block is not executed. Please confirm that G and F modal and
coordinate values are appropriate. If there are coordinate system shift commands or M, S, T and B
commands before the block set as the start position, carry out the required commands using the MDI, etc.
If the program is run from the set block without carrying out these operations, there is a danger of
interference with the machine or of machine operation at an unexpect ed speed, which may result in
breakage of tools or machine tool or may cause damage to the operators.
Under the constant surface speed control (during G96 modal), if the ax is targeted for the constant surface
speed control (normally X axis for a lathe) moves toward the spindle center, the spindle rotation speed will
increase and may exceed the allowable speed of the workpiece or chuck, etc. In this case, the workpiece,
etc. may jump out during machining, which may result in breakage of tools or machine tool or may cause
damage to the operators.
Page 8
1. Items related to product and manual
For items described as "Restrictions" or "Usable State" in this manual, the instruction manual issued by
the machine tool builder takes precedence over this manual.
Items not described in this manual must be interpreted as "not possible".
This manual is written on the assumption that all opti on functions are added. Refer to the specifications
issued by the machine tool builder before starting use.
Refer to the Instruction Manual issued by each machine tool builder for details on each machine tool.
Some screens and functions may differ depending on the NC system (or its version), and some functions
may not be possible. Please confirm the specifications before use.
2. Items related to operation
Before starting actual machining, always carry out graphic check, dry ru n operation and single block
operation to check the machining program, tool compensation amount, workpiece compensation amount
and etc.
If the workpiece coordinate system offset amount is changed during single block stop, the new setting will
be valid from the next block.
Turn the mirror image ON and OFF at the mirror image center.
CAUTION
If the tool offset amount is changed during automatic operation (including during single block stop), it will
be validated from the next block or blocks onwards.
Do not make the synchronous spindle rotation command OFF with one workpiece ch ucked by the basic
spindle and synchronous spindle during the spindle synchronization.
Failure to observe this may cause the synchronous spindle stop, and hazardous situation.
3. Items related to programming
The commands with "no value after G" will be handled as "G00".
";" "EOB" and "%" "EOR" are expressions used for explanation. The actual codes are: For ISO: "CR, LF", or
"LF" and "%".
Programs created on the Edit screen are stored in the NC memory in a "CR, LF" fo rmat, but programs
created with external devices such as the FLD or RS-232C may be stored in an "LF" format.
The actual codes for EIA are: "EOB (End of Block)" and "EOR (End of Record)".
When creating the machining program, select the appropriate machining conditions, and make sure that
the performance, capacity and limits of the machine and NC are not exceeded. The examples do not
consider the machining conditions.
Do not change fixed cycle programs without the prior approval of the machine tool build er .
When programming the multi-part system, take special care to the mov ements of the programs for other
part systems.
Page 9
Disposal
(Note)This symbol mark is for EU countries only.
This symbol mark is according to the directive 2006/66/EC Article 20 Information for endusers and
Annex II.
Your MITSUBISHI ELECTRIC product is designed and manufact ured with high quality materials and
components which can be recycled and/or reused.
This symbol means that batteries and accumulators, at their end-of-life, should be disposed of sep arately
from your household waste.
If a chemical symbol is printed beneath the symbol shown above, this chemical symbol means that the
battery or accumulator contains a heavy metal at a certain concentration.
This will be indicated as follows:
Hg: mercury (0,0005%), Cd: cadmium (0,002%), Pb: lead (0,004%)
In the European Union there are separate collection systems for used batteries and accumulators.
Please, dispose of batteries and accumulators correctly at your local community waste collection/recycling
centre.
Please, help us to conserve the environment we live in!
Page 10
Page 11
CONTENTS
1 Control Axes .... ....................................... ... .... ... ... ... ....................................... ... ... .... ... ................................. 1
1.1 Coordinate Words and Control Axes ................................................................ ... ... ... .... ... ... ... .............. 2
1.2 Coordinate Systems and Coordinate Zero Point Symbols .................................................................... 4
2 Least Command Increments ........... ... ... ... .... ... ... ....................................... ... ... ... .... .................................... 5
2.1 Input Setting Unit ............................................. ... ....................................... ... .... ... ... ... ........................... 6
2.2 Indexing Increment ............................................................................................................................... 7
3 Program Formats ...................................... ....................................... ... .... ... ... ... ........................................... 9
3.1 Program Format ............................ ... ... .... ... ... ... ....................................... ... ... .... ... ............................... 10
3.2 File Format ................................. ... ... ... .... ... ... ....................................... ... ... ... .... .................................. 14
3.3 Optional Block Skip ............................................................................................................................. 16
3.3.1 Optional Block Skip; / ........ ... ... ... ....................................... ... .... ... ... ... ... ...................................... 16
3.3.2 Optional Block Skip Addition ; /n ................................................................................................. 17
3.4 G code .................................................... ... ....................................... ... ... ... ... .... .................................. 19
3.4.1 Modal, unmodal .......................................................................................................................... 19
3.4.2 G code Lists ................................................................................................................................ 19
3.4.3 Table of G Code Lists ................................................................................................................. 20
3.5 Precautions Before Starting Machining ................... ...... ... .... ... ... ... .... ... ... ... ... .... ... ... ... .... ...... ... ............ 25
4 Pre-read Buffers ........... ... .... ... ... ... .... ...................................... .... ... ... ... ...................................................... 27
4.1 Pre-read Buffers ............................ ....................................... ... ... ... .... ... ............................................... 28
5 Position Commands ....... .... ... ... ....................................... ... ... .... ... ............................................................ 29
5.1 Incremental/Absolute Value Commands ; G90,G91........................................................................... 30
5.2 Radius/Diameter Designation ............. .... ... ... ....................................... ... ... ... .... .................................. 32
5.3 Inch/Metric Conversion ; G20,G21....................................................................................................... 33
5.4 Decimal Point Input ............................. .... ... ... ... ... .... ...................................... .... ... ... ... ......................... 35
6 Interpolation Functions ............................................................................................................................ 39
6.1 Positioning (Rapid Traverse) ; G00..................................................................................................... 40
6.2 Linear Interpolation ; G01 .................................................................................................................... 46
6.3 Circular Interpolation ; G02,G03......................................................................................................... 48
6.4 R Specification Circular Interpolation ; G02,G03 ................................................................................. 52
6.5 Plane Selection ; G17,G18,G19........................................................................................................... 54
6.6 Thread Cutting.................. ... ... .... ... ... ... .... ...................................... .... ... ... ... ... ...................................... 56
6.6.1 Constant Lead Thread Cutting ; G33............... ... ... ... .... ... ... ....... ... ... ... ... .... ... ... ... .... ... ... ... ... .... . .... 56
6.6.2 Inch Thread Cutting ; G33........................................................................................................... 60
6.6.3 Continuous Thread Cutting ; G33............................................................................................... 62
6.6.4 Variable Lead Thread Cutting ; G34............................................................................................ 63
6.6.5 Circular Thread Cutting ; G35,G36............................................................................................. 65
6.7 Helical Interpolation ; G17,G18,G19 and G02,G03 .............................................................................69
6.8 Milling Interpolation ; G12.1 ............................................................................................................... 73
6.8.1 Selecting Milling Mode ................................................................................................................ 75
6.8.2 Milling Interpolation Control and Command Axes . ... .... ...... ... .... ... ... ... ... .... ... ... ... .... ... ... ... ... ....... .. 76
6.8.3 Selecting a Plane during the Milling Mode ; G17,G19,G16 ........................................................ 78
6.8.4 Setting Milling Coordinate System .............................................................................................. 80
6.8.5 Preparatory function..................................................................................................................... 82
6.8.6 Switching from Milling Mode to Turning Mode; G13.1 ................................................................ 87
6.8.7 Feed Functions ........................................................................................................................... 87
6.8.8 Program Support Functions ........................................................................................................ 87
6.8.9 Miscellaneous Functions ................................................. ... ... .... ... ... ... ....... ... ... ... .... ... ... ......
6.8.10 Tool Length Compensation ....................................................................................................... 89
6.8.11 Tool Radius Compensation ....................................................................................................... 92
6.8.11.1 Tool Radius Compensation Operation .............................................................................. 93
6.8.11.2 Interference Check ......................................................................................................... 110
......... 88
Page 12
6.9 Cylindrical Interpolation ; G07.1 (only 6 and 7 in G code list) ........................................................... 120
6.10 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113 (Only 6, 7 in G code list) ...................... 128
6.11 Exponential Interpolation ; G02.3,G03.3..........................................................................................135
7 Feed functions ......................................................................................................................................... 141
7.1 Rapid Traverse Rate.......................................................................................................................... 142
7.2 Cutting Feedrate ...................................................... .... ... ....................................... ... ........................ 143
7.3 F1-digit Feed.......... ... ... ... .... ... ... ... ....................................... ... .... ... ... ... ...............................................144
7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed) ; G94,G95...........147
7.5 Feedrate Designation and Effects on Control Axes ........................................................................... 149
7.6 Thread Cutting Mode ....................................................... ... ... .... ... ..................................................... 154
7.7 Automatic Acceleration/Deceleration................................................................................................ 155
7.8 Rapid Traverse Constant Inclination Acceleration/Deceleration ............... ........................................156
7.9 Speed Clamp .. .... ... ... ....................................... ... ... ... .... ...................................... .... ... ........................ 159
7.10 Exact Stop Check ; G09................................................................................................................... 160
7.11 Exact Stop Check Mode ; G61......................................................................................................... 164
7.12 Deceleration Check. ......................................................................................................................... 165
7.12.1 G1 -> G0 Deceleration Check.................................................................................................. 167
7.12.2 G1 -> G1 Deceleration Check.................................................................................................. 168
7.13 Automatic Corner Override ; G62..................................................................................................... 169
7.14 Tapping Mode ; G63 ........................................................................................................................ 174
7.15 Cutting Mode ; G64......................................................................................................................... 175
8 Dwell.......................................................................................................................................................... 177
8.1 Dwell (Time Designation) ; G04......................................................................................................... 178
9 Miscellaneous Functions ....................................................................................................................... 181
9.1 Miscellaneous Functions (M8-digits) ................................................................................................. 182
9.2 Secondary Miscellaneous Functions (A8-digits, B8-digits or C8-digits) ............................................ 184
9.3 Index Table Indexing ......................................................................................................................... 185
10 Spindle Functions.................................................................................................................................. 187
10.1 Spindle Functions................................. ... .... ... ... ... ... .... ...................................... .... ... ... .....................188
10.2 Constant Surface Speed Control ; G96,G97.................................................................................... 189
10.3 Spindle Clamp Speed Setting ; G92 ................................................................................................191
10.4 Spindle/C Axis Control...................................... ... ... .... ...................................... .... ... ... ... .................. 193
10.5 Spindle Synchronization................................................................................................................... 196
10.5.1 Spindle Synchronization Control I ; G114.1....................................................... ... .................. 197
10.5.2 Spindle Synchronization Control ll......................... ... ... .... ...................................... .... ... ... ........ 206
10.5.3 Precautions for Using Spindle Synchronization Control .......................................................... 211
10.6 Tool Spindle Synchronization lA (Spindle-Spindle, Polygon) ; G114.2........................................... 213
10.7 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon) ;
G51.2 (only 6 and 7 in G code list) ..................................................................................................221
10.8 Tool Spindle Synchronization IC (Spindle-NC Axis, Polygon) ;
G51.2 (only 6 and 7 in G code list) .................................................................................................. 228
10.9 Tool Spindle Synchronization II (Hobbing) ; G114.3..................................................... .... ... ... ... .....231
10.10 Multiple-spindle Control.................................................................................................
.10.1 Multiple-spindle Control I (spindle control command) ; S○ = ............................... ... ... ... ... .. 246
10
10.10.2 Multiple-spindle Control I (spindle selection command) ; G43.1,G44.1,G47.1 ..................... 247
10.10.3 Multiple-spindle Control II ...................................................................................................... 251
................. 245
11 Tool Functions ...................................................................................................................................... 255
11.1 Tool Functions (T8-digit BCD) .........................................................................................................256
12 Tool Compensation Functions ............................................................................................................ 257
12.1 Tool Compensation.......................................................................................................................... 258
12.1.1 Tool Compensation Start ........................................................................................................ 259
12.1.2 Expanded Method at Starting Tool Compensation ................................................................. 260
12.2 Tool Length Compensation.............................................................................................................. 262
12.3 Tool Nose Wear Compensation .................................... .................................................................. 264
Page 13
12.4 Tool Nose R Compensation ; G40,G41,G42,G46........................................................................ 265
12.4.1 Tool Nose Point and Compensation Directions ...................................................................... 267
12.4.2 Tool Nose Radius Compensation Operations ......................................................................... 270
12.4.3 Other Operations during Tool Nose Radius Compensation .................................................... 288
12.4.4 G41/G42 Commands and I, J, K Designation .. ... ... ....... ... ... .... ... ... ... ... .... ... ... ... .... ... ... ... ....... ... 296
12.4.5 Interrupts during Tool Nose Radius Compensation ................................................................ 300
12.4.6 General Precautions for Tool Nose Radius Compensation .................................................... 304
12.4.7 Interference Check ........................... ... ... ... .... ...................................... .... ... ... ... .... ................... 305
12.5 Compensation Data Input by Program ; G10 L2/L10/L11, G11....................................................... 311
12.6 Tool Life Management II ; G10 L3, G11.......................................................................................... 314
12.6.1 Counting the Tool Life ............................................................................................................. 317
13 Program Support Functions ................................................................................................................ 321
13.1 Fixed Cycles for Turning Machining ................................................................................................ 322
13.1.1 Longitudinal Cutting Cycle ; G77 ............................................................................................ 323
13.1.2 Thread Cutting Cycle ; G78 ... ... .... ... ... ... ... .... ...................................... .... ... ... ... .... ................... 326
13.1.3 Face Cutting Cycle ; G79........................................................................................................ 329
13.2 Fixed Cycles for Turning Machining (MITSUBISHI CNC special format) ; G77,G78,G79.............. 332
13.3 Compound Type Fixed Cycle for Turning Machining ...................................................................... 333
13.3.1 Longitudinal Rough Cutting Cycle ; G71................................................................................. 334
13.3.2 Face Rough Cutting Cycle ; G72........................................................................................... 348
13.3.3 Formed Material Rough Cutting Cycle ; G73.......................................................................... 350
13.3.4 Finishing Cycle ; G70.............................................................................................................. 354
13.3.5 Face Cut-Off Cycle ; G74........................................................................................................ 355
13.3.6 Longitudinal Cut-off Cycle ; G75............................................................................................. 357
13.3.7 Compound Thread Cutting Cycle ; G76 ..................................... ... ... ... .... ... ............................. 359
13.3.8 Precautions for Compound Type Fixed Cycle for Turning Machining; G70 to G76 ............... 363
13.4 Compound Type Fixed Cycle for Turning Machining (MITSUBISHI CNC special format) ;
G71,G73,G74,G76................................................................................................................................... 365
13.5 Fixed Cycle for Drilling ....................................................... ... ... ... .... ................................................ 370
13.5.1 Face Deep Hole Drilling Cycle 1 (Longitudinal deep hole drilling cycle 1) ; G83 (G87).......... 373
13.5.2 Face Tapping Cycle (Longitudinal tapping cycle) / Face Reverse Tapping Cycle
(Longitudinal reverse tapping cycle) ; G84 (G88) / G84.1 (G88.1)........................................ 375
13.5.3 Face Boring Cycle (Longitudinal boring cycle) ; G85 (G89).................................................... 383
13.5.4 Deep Hole Drilling Cycle 2 ; G83.2 ......................................................................................... 384
13.5.5 Fixed Cycle for Drilling Cancel; G80 ....................................................................................... 386
13.5.6 Precautions When Using a Fixed Cycle for Drilling ................................................................ 387
13.5.7 Initial Point and R Point Level Return ; G98,G99.................................................................... 388
13.5.8 Setting of Workpiece Coordinates in Fixed Cycle Mode ......................................................... 389
13.5.9 Drilling Cycle High-Speed Retract ................................................... ....................................... 390
13.6 Fixed Cycle for Drilling (MITSUBISHI CNC special format) ............ ... ... ....................................... ... 391
13.6.1 Drilling Cycle, Spot Drilling Cycle ; G81................................................................................. 394
13.6.2 Drilling Cycle, Counter Boring Cycle ; G82............................................................................. 395
13.6.3 Deep Hole Drilling Cycle ; G83................................................................................................ 396
13.6.4 Stepping Cycle ; G83.1.....................................................................................................
13.6.5 Tapping Cycle ; G84................................................................................................................ 400
13.6.6 Synchronous tapping cycle ; G84.2 ........................................................................................ 402
13.6.7 Boring Cycle ; G85................................................................................................................... 404
13.6.8 Boring Cycle ; G89................................................................................................................... 405
13.6.9 Precautions for Using Fixed Cycle for Drilling (MITSUBISHI CNC special format) ................ 406
13.7 Subprogram Control; M98, M99, M198 ........................................................................................... 408
13.7.1 Subprogram Call ; M98,M99................................................................................................... 408
13.7.2 Subprogram Call ; M198......................................................................................................... 413
13.8 Variable Commands ....................................................................................................................... 414
13.9 User Macro ............................................ ... ....................................... ... ... ... ... .... ................................ 418
13.9.1 User Macro ............................................................................................................................. 418
13.9.2 Macro Call Instruction ............................................................................................................. 419
13.9.2.1 Simple Macro Calls ; G65............................................................................................... 419
13.9.2.2 Modal Call A (Movement Command Call) ; G66............................................................. 422
13.9.2.3 Modal Call B (for each block) ; G66.1............................................................................. 423
13.9.2.4 G Code Macro Call ......................................................................................................... 424
....... 398
Page 14
13.9.2.5 Miscellaneous Command Macro Call (for M, S, T, B Code Macro Call) ......................... 425
13.9.2.6 Detailed Description for Macro Call Instruction .............................................................. 426
13.9.3 ASCII Code Macro ... ... ... ... ....... ... ... .... ... .................................................................................. 428
13.9.4 Variable........................... ... .... ... ... ... .... ... ....................................... ... ... ... ... .... ........................... 433
13.9.5 Types of Variables .................................................................................................................. 435
13.9.5.1 Common Variables ......................................................................................................... 435
13.9.5.2 Local Variables (#1 to #33) .............. ... ... .... ... ... ... ....................................... ... .... ... ... ........436
13.9.5.3 Macro Interface Inputs/Outputs (#1000 to #1035, #1100 to #1 135, #1200 to #1295,
#1300 to #1395) .............................................................................................................. 439
13.9.5.4 Tool Compensation ......................................................................................................... 446
13.9.5.5 Workpiece Coordinate System Compensation (#5201 - #532n)...................................... 448
13.9.5.6 NC Alarm (#3000) ........................................................................................................... 449
13.9.5.7 Integrating Time (#3001, #3002) ..................................................................................... 450
13.9.5.8 Suppression of Single Block Stop and Miscellaneous Function Finish
Signal Waiting (#3003) ....................................................................................................450
13.9.5.9 Feed Hold, Feedrate Override, G09 Valid/Invalid (#3004) .............................................. 451
13.9.5.10 Message Display and Stop (#3006) ..... ....... ... ... .... ... ... ... .... ... ... ... ... .... ... ... ... ....... ... ... ... .. 451
13.9.5.11 Mirror Image (#3007) .................................................................................................... 452
13.9.5.12 G Command Modals (#4001-#4021, #4201-#4221) ....................................... ... ... ... ... .. 453
13.9.5.13 Other Modals (#4101 - #4120, #4301 - #4320) ............................................................. 454
13.9.5.14 Position Information (#5001 - #5140 + n) ..................................................................... 455
13.9.5.15 External Workpiece Coordinate System Compensation (#2501, #2601) .............. ...... .. 457
13.9.5.16 Number of Workpiece Machining Times (#3901, #3902) .............................................. 457
13.9.5.17 Tool Life Management (#60000 - #63016) .................................................................... 458
13.9.5.18 Reading The Parameters (#100000-#100002, #100010) ............................................. 463
13.9.5.19 Reading PLC data (#100100-#100103,#100110) ....................... ..................................467
13.9.5.20 Time Reading Variables (#3001, #3002, #3011, #3012) ......................................... ... .. 471
13.9.5.21 R Device Access Variables (#50000 - #50749, #51000 - #51749, #52000 - #52749) .. 473
13.9.6 Operation Commands ........................ ...................................... .... ... ... ... ... ............................... 479
13.9.7 Control Commands .................................................. ... .... ... ... ... .... ........................................... 484
13.9.8 External Output Commands ; POPEN,PCLOS,DPRNT ......................................................... 487
13.9.9 Precautions . ...... ... .... ... ... ... .... ... ... ... .........................................................................................491
13.10 Mirror Image for Facing Tool Posts ; G68,G69.............................................................................. 493
13.11 Corner Chamfering/Corner Rounding I ................................. ... ....................................... ... ... ... ..... 504
13.11.1 Corner Chamfering "I_" ; G01 X_ Z_ ,C_/I_/K_/C_............................................................... 504
13.11.2 Corner Rounding I ; G01 X_ Z_ ,R_/R_................................................................................ 506
13.11.3 Corner Chamfering/Corner Rounding Expansion ................................................................. 508
13.11.4 Interrupt during Corner Chamfering/Corner Rounding ..................... ................... .................. 510
13.12 Corner Chamfering/Corner Rounding II ...................................................................... .... ... ... ... ..... 511
13.12.1 Corner Chamfering II ; G01/G02/G03 X_ Z_ ,C_/I_/K_/C_..................................................512
13.12.2 Corner Rounding II ; G01/G02/G03 X_ Z_ ,R_/R_ ............................................................... 514
13.12.3 Corner Chamfering/Corner Rounding Expansion ................................................................. 516
13.12.4 Interrupt during Corner Chamfering/Corner Rounding ..................... ................... .................. 516
13.13 Linear Angle Command ; G01 X_/Z_ A_/,A_................................................................................. 517
13.14 Geometric ....................................... ....................................... ... ... ... .... ... ........................................ 518
13.14.1 Geometric I ; G01 A_ ............................................................................................................ 518
13.14.2 Geometric IB ......................................................................................................................... 520
13.14.3 Geometric IB (Automatic calculation of two-arc contact) ; G02/G03 P_Q_ /R_.................... 521
13.14.4 Geometric IB (Automatic calculation of linear - arc intersection) ;
G01 A_ , G02/G03 P_Q_H_ .............................................................................................
13.14.5 Geometric IB (Automatic calculation of linear - arc intersection) ;
G01 A_ , G02/G03 R_H_....................................................................................................... 529
13.15 Programmable Parameter Input ; G10 L70/L50, G11.................................................................... 533
13.16 Macro Interruption ; M96,M97............... .... ... ... ... ....................................... ... ... .... ... ........................ 535
13.17 Tool Change Position Return ; G30.1 - G30.5.......................... ... ... .... ... ... ... .................................. 543
13.18 Balance Cut ; G15,G14................................................................................................................. 546
13.19 Waiting-and-simultaneous operation.............................................................................................. 550
13.19.1 Waiting-and-simultaneous Operation ; !L................... .... ... ... ... .... ... ...................................... .. 550
13.19.2 Waiting-and simultaneous Operation with Start Point Designated (Type 1) ; G115..............553
13.19.3 Waiting-and simultaneous Operation with Start Point Designated (Type 2) ; G116.............556
13.19.4 Waiting-and-simultaneous Operation Function Using M codes ; M*** .................................. 558
..... 525
Page 15
13.20 Control Axis Superimposition ; G126 ........................................................................................... 562
13.21 2-part System Simultaneous Thread Cutting Cycle.......................................... ... ... .... ... ................ 575
13.21.1 2-part System Simultaneous Thread Cutting Cycle Parameter Setting Command ; G76.....575
13.21.2 2-part System Simultaneous Thread Cutting Cycle l ; G76.1 ................................................ 576
13.21.3 2-part System Simultaneous Thread Cutting Cycle ll ; G76.2................................... ... ... ....... 578
13.22 2-part System Simultaneous Thread Cutting Cycle (MITSUBISHI special format) ;
G76.1,G76.2 ................................................................................................................................... 582
14 Coordinate System Setting Functions................................................................................................. 585
14.1 Coordinate Words and Control Axes .............................................................................................. 586
14.2 Basic Machine, Workpiece and Local Coordinate Systems............................................................. 588
14.3 Machine Zero Point and 2nd Reference Position (Zero point) ........................................................ 589
14.4 Automatic Coordinate System Setting ............................................................................................. 590
14.5 Basic Machine Coordinate System Selection ; G53 ........................................................................ 591
14.6 Coordinate System Setting ; G92 .................................................................................................... 592
14.7 Reference Position (Zero point) Return ; G28,G29.......................................................................... 593
14.8 2nd, 3rd, and 4th Reference Position (Zero point) Return ; G30 ..................................................... 597
14.9 Reference Position Check ; G27...................................................................................................... 600
14.10 Workpiece Coordinate System Setting and Offset ; G54 to G59 (G54.1)...................................... 601
14.11 Local Coordinate System Setting ; G52........................................................................................ 607
14.12 Workpiece Coordinate System Preset ; G92.1 ............................................................................. 608
14.13 Coordinate System for Rotary Axis................................................................................................ 613
15 Protection Function............................................................................................................................... 617
15.1 Chuck Barrier/Tailstock Barrier ; G22,G23 ...................................................................................... 618
15.2 Stored Stroke Limit ; G22,G23......................................................................................................... 622
16 Measurement Support Functions ........................................................................................................ 623
16.1 Automatic Tool Length Measurement ; G37 ....................................................................................624
16.2 Skip Function ; G31 .................................................... ... .... ... ... ....................................................... 627
16.3 Multi-step Skip Function 1 ; G31.n ,G04......................................................................................... 631
16.4 Multi-step Skip Function 2 ; G31 P ................................................................................................. 633
16.5 Speed Change Skip ; G31 Fn ........................................................................................................ 635
16.6 Programmable Current Limitation ; G10 L14 ;....................... ....................................... ... ... ... ... .... ... 639
Appendix 1 Parameter Input by Program N No. Correspondence Table .............................................. 641
Appendix 2 Program Errors....................................................................................................................... 645
Page 16
Page 17
1
1
Control Axes
Page 18
1 Control Axes
MITSUBISHI CNC
1.1 Coordinate Words and Control Axes
Function and purpose
In the case of a lathe, axis names (coordinate words) and directions are defined as follows.
The axis at right angles to the spindle
Axis name: X axis
The axis parallel to the spindle
Axis name: Z axis
Coordinate axes and polarities
(b)
(a)
(c)
+Y
Since coordinates based on the right hand rule are used with a lathe, in the above figure, the positive direction
of the Y axis which is at right angles to the X-Z plane is downward.
Note that a circular on the X-Z plane is expressed as clockwise or counterclockwise as seen from the forward
direction of the Y axis.
(Refer to the section on circular interpolation.)
(d)
+Z
+X
(a) Spindle stock
(b) Tailstock
(c) Tool
(d) Turret
2
Page 19
M700V/M70V Series Programming Manual (Lathe System)
1.1 Coordinate Words and Control Axes
Relationship between coordinates
G54
G52
G58
G55
G59
G30
G28
+X
+Y
+Z
Reference position
Basic machine coordinate
Workpiece coordinate zero points
Local coordinate zero point
3
Page 20
1 Control Axes
MITSUBISHI CNC
1.2 Coordinate Systems and Coordinate Zero Point Symbols
G52
Reference position:
A specific position to establish coordinate systems and change tools
Basic machine coordinate zero point:
A position specific to machine
Workpiece coordinate zero points (G54 to G59)
A coordinate zero point used for workpiece machining
The basic machine coordinate system is the coordinate system that expresses the position (tool change
position, stroke end position, etc.) that is specific to the machine.
Workpiece coordinate systems are used for workpiece machining.
Upon completion of the dog-type reference position return, the parameters are referred and the basic machine
coordinate system and workpiece coordinate systems (G54 to G59) are automatically set.
The offset of the basic machine coordinate zero point and reference position is set by a parameter. (Normally,
set by machine manufacturers)
Workpiece coordinate systems can be set with coordinate systems setting functions, workpiece coordinate
offset measurement (additional specification), and etc.
G54
G92
EXT
Reference position
Basic machine coordinate zero point
Workpiece coordinate zero points
Local coordinate zero point
G52
G55
G52 Local coordinate system offset (*1)
G54 Workpiece coordinate (G54) system offset (*1)
G55 Workpiece coordinate (G55) system offset
G92 G92 Coordinate system shift
EXT External workpiece coordinate offset
The local coordinate systems (G52) are valid on the coordinate systems designated by workpiece coordinate
systems 1 to 6.
Using the G92 command, the basic machine coordinate system can be shifted and made into a hypothetical
machine coordinate system. At the same time, workpiece coordinate systems 1 to 6 are also shifted.
4
Offset set by a parameter
Offset set by a program
("0" is set when turning the power ON)
(*1) G52 offset is independently possessed by G 54
to G59 respectively.
Page 21
5
2
Least Command
Increments
Page 22
2 Least Command Increments
MITSUBISHI CNC
2.1 Input Setting Unit
Function and purpose
The input setting units are the units of setting data including tool compensation amounts and workpiece
coordinates compensation.
The program command units are the units of movement amounts in programs.
These are expressed with mm, inch or degree (°).
Detailed description
Program command units for each axis and input setting units, common for all axes, are determined by the
setting of parameters as follows.
Input setting unit
Program command
unit
Parameter
#1003 iunit = B 0.001 0.0001 0.001
= C 0.0001 0.00001 0.0001
= D 0.00001 0.000001 0.00001
= E 0.000001 0.0000001 0.000001
#1015 cunit = 0 Follow #1003 iunit
= 1 0.0001 0.00001 0.0001
= 10 0.001 0.0001 0.001
= 100 0.01 0.001 0.01
= 1000 0.1 0.01 0.1
= 10000 1.0 0.1 1.0
Linear axis
Millimeter Inch
Rotary axis
(°)
Precautions
(1) Inch/metric changeover can be handled by either a parameter screen (#1041 I_inch: valid only when the
power is turned ON) or G commands (G20 or G21).
However, the changeover by a G command applies only to the program command units, and not to the
input setting units. Consequently, the tool offset amounts and other compensation amounts as well as
the variable data should be preset in order to correspond to input setting units.
(2) The millimeter and inch systems cannot be used together.
(3) When performing a circular interpolation between the axes whose program command units are different,
the center command (I, J, K) and the radius command (R) are designated by the input setting units. Use
a decimal point to avoid confusion. )
6
Page 23
M700V/M70V Series Programming Manual (Lathe System)
2.2 Indexing Increment
2.2 Indexing Increment
Function and purpose
This function limits the command value for the rotary axis.
This can be used for indexing the rotary table, etc. It is possible to cause a program error with a progra m
command other than an indexing increment (parameter setting value).
Detailed description
When the indexing increment (parameter) which limits the command value is set, the rotary axis can only be
positioned with that indexing increment. If a program other than the indexing increment setting value is
commanded, a program error (P20) will occur.
The indexing position will not be checked when the parameter is set to 0.
(Example)When the indexing increment setting value is 2 degrees, the machine coordinate position at the end
point can only be commanded with the 2-degree increment.
G90 G01 C102.000 ; ... Moves to the 102 degree angle.
G90 G01 C101.000 ; ... Program error
G90 G01 C102 ; ... Moves to the 102 degree angle. (Decimal point type II)
The following axis specification parameter is used.
# Item Details Setting range (unit)
2106 Index unit
Indexing
increment
Set the indexing increment with which the rotary axis can be
positioned.
0 to 360(°)
Precautions
(1) When the indexing increment is set, positioning will be conducted in degree unit.
(2) The indexing position is checked with the rotary axis, and is not checked with other axes.
(3) When the indexing increment is set to 2 degrees, the rotary axis is set to the B axis, and the B axis is
moved with JOG to the 1.234 position, an indexing error will occur if "G90B5." or "G91B2." is
commanded.
7
Page 24
2 Least Command Increments
MITSUBISHI CNC
8
Page 25
9
3
Program Formats
Page 26
3 Program Formats
MITSUBISHI CNC
3.1 Program Format
%
Block
Block
Block
Block
Block
Block
Block
Block
Block
%
A collection of commands assigned to an NC to move a machine is called "program".
A program is a collection of units called "block" which specifies a sequence of machine tool operations.
Blocks are written in the order of the actual movement of a tool.
A block is a collection of "words" which constitutes a command to an operation.
A word is a collection of characters (alphabets, numerals, signs) arranged in a specific sequence.
10
Page 27
M700V/M70V Series Programming Manual (Lathe System)
3.1 Program Format
Detailed description
Program
A program format looks as follows.
(1)
(2)
(3)
(4)
(5)
%
O 㧧
(COMMENT)
Block
Block
Block
Block
Block
Block
Block
Block
%
(1) Program start
Input an End Of Record (EOR, %) at the head of a program.
It is automatically added when writing a program on an NC. When using an external device, do not forget
to input it at the head of a program. For details, refer to the description of the file format.
(2) Program No.
Program Nos. are used to classify programs by main program unit or subprogram unit. They are
designated by the address "O" followed by numbers of up to 8 digits. Program Nos. must be written at
the head of programs. A setting is available to prohibit O8000s and O9000s from editing (edit lock). Refer
to the instruction manual for the edit lock.
(3) Comment
Data between control out "(" and control in ")" is ignored.
Information including program names and comments can be written in.
(4) Program section
A program is a collection of several blocks.
(5) Program end
Input an end of record (EOR, %) at the end of a program.
It is automatically added when writing a program on an NC.
11
Page 28
3 Program Formats
MITSUBISHI CNC
Block and word
EOB
Word Word
Word
...
;
Word
(a) (n)
[Block]
A block is a least command increment, consisting of words.
It contains the information which is required for a tool machine to execute a specific operation. One block unit
constitutes a complete command.
The end of each block is marked with an End of Block (EOB, expressed as ";" for the sake of convenience).
[Word]
(a) Alphabet (address)
(n) Numerals
A word consists of a set of an alphabet, which is called an address, and numerals (numerical information).
Meanings of the numerical information and the number of significant digits of words differ according to an
address.
The major contents of a word are described below.
N_ _ _ G _ _ X _ _ Z__ F__ ;
(1) (2)
(1) Sequence No.
A "sequence No." consists of the address "N" followed by numbers of up to 6 digits (Normally 3 or 4
digits). It is used as an index when searching a necessary block in a program (as branch destination and
etc.).
It does not affect the operation of a tool machine.
(2) Preparatory functions (G code, G function)
"Preparatory function (G code, G function)" consists of the address G followed by numbers of 2 or 3
digits (it may include 1 digit after the decimal point). G codes are mainly used to designate functions,
such as axis movements and setting of coordinate systems. For example, G00 executes a positioning
and G01 executes a linear interpolation.
There are 6 types of G code systems, 2, 3, 4, 5, 6 and 7. Refer to the description of G code system for
available G codes.
(3) Coordinate words
"Coordinate words" specify the coordinate position and movement amounts of tool machine axes. They
consist of an address which indicates each axis of a tool machine followed by numerical information (+ or
- signs and numerals).
X, Y, Z, U, V, W, A, B and C are used as address. Coordinate positions and movement amounts are
specified by either "incremental value commands" or "absolute value commands".
(3)
(4) EOB
12
(4) Feed Functions (F functions)
"Feed Functions (F functions)" designate the speed of a tool relative to a workpiece. They consist of the
address F followed by numbers.
Page 29
M700V/M70V Series Programming Manual (Lathe System)
3.1 Program Format
Main program and subprograms
(MP) (S1)
(S2)
O0010;
M98P1000;
M98P2000;
M02;
O1000;
M99;
O2000;
M99;
(MP) Main program
(S1) Subprogram 1
(S2) Subprogram 2
Fixed sequences or repeatedly used parameters can be stored in the memory as subprograms which can
then be called from the main program when required.
If a command is issued to call a subprogram while a main program is being executed, the subprogram will be
executed. And when the subprogram is completed, the main program will be resumed.
Refer to the description of subprogram control for the details of the execution of subprograms.
13
Page 30
3 Program Formats
MITSUBISHI CNC
3.2 File Format
(COMMENT) ;
G28XYZ ;
M02 ;
%
Function and purpose
Program file can be created using NC edit screen and PC.
It can be input/output between NC memory and an external I/O device. Hard discs stored in NC unit are
regarded as an external I/O device. For the details of input/output method, refer to the instruction manual.
Program file format differs depending on the device which creates the program.
Detailed description
Devices available for input/output
Devices which can input/output program files are as follows.
NC memory
HD (internal hard disc) ○ --
Serial ○○○
Memory card (front IC card) ○○○
DS (NC control unit side compact flash) ○ --
FD ○ -USB memory - ○ -
Ethernet ○○○
Anshin-net server ○○○
External I/O device M700VW M700VS M70V
○○○
Program file format
The file format for each external I/O device is as follows.
(1) NC memory (Creates program on NC)
End of record (EOR, %)
Program No. (O No.) Not necessary.
File transfer
The end of record (EOR, %) is automatically added.
It does not need to be input purposely.
When multiple programs within the NC memory are transferred to an external device as serial, they will be integrated into one file in the external device.
When a file containing multiple programs in an external device is transferred to NC
memory as serial, it will be divided into one file per one program.
14
Page 31
M700V/M70V Series Programming Manual (Lathe System)
3.2 File Format
(2) External device (except for serials, such as memory card, DS, FD, USB memory)
CRLF
CRLF
G28 XYZ
CRLF
:
:
M02
CRLF
O101(COMMENT1)
CRLF
:
M02
CRLF
%
^Z
O100(COMMENT)
[Single program] [Multiple programs]
CRLF
(COMMENT)
G28 XYZ
CRLF
CRLF
:
:
M02
CRLF
%
^Z
The first line (from % to LF, or CR LF) will be skipped. Also, the content after the
End of record (EOR, %)
second % will not be transferred.
"%" must be included in the first line because if not, the necessary information
when transferring a file to an NC memory cannot be transferred.
Program No. (O No.)
O No. before (COMMENT) will be ignored and the file name will be given the priority.
Transfer and check of multiple programs between external devices, except for serial <_> serial, are not available.
When a file containing multiple programs in an external device is transferred to NC
File transfer
memory as serial, it will be divided into one file per one program.
When transferring divided programs one by one from an external device, which is
not serial, (multiple programs) to an NC memory, the head program name can be
omitted like "(COMMENT)" only when the transferring destination file name is designated to the file name field of device B.
Program name
Program name should be designated with up to 32 alphanumeric characters (29
characters for a multi-part system program).
End of block (EOB, ;) When the I/O parameter "CR output" is set to "1", EOB becomes CRLF.
(3) External device (serial)
LF
%
O100(COMMENT)
G28 XYZ
LF
LF
:
:
M02
LF
%
The first line (from % to LF, or CR LF) will be skipped. Also, the content after the
End of record (EOR, %)
second % will not be transferred.
"%" must be included in the first line because if not, the necessary information
when transferring a file to an NC memory cannot be transferred.
Transfer and check of multiple programs between external devices, except for serial <_> serial, are not available.
File transfer
When transferring a file as serial, the head program name can be omitted like
"(COMMENT)" only when the transferring destination file name is designated to
the file name field of device B.
Program name
Program name should be designated with up to 32 alphanumeric characters (29
characters for a multi-part system program).
End of block (EOB, ;) When the I/O parameter "CR output" is set to "1", EOB becomes CRLF.
15
Page 32
3 Program Formats
MITSUBISHI CNC
3.3 Optional Block Skip
3.3.1 Optional Block Skip; /
Function and purpose
This function selectively ignores specific blocks in a machining program which starts with the "/" (slash) code.
Detailed description
Provided that the optional block skip switch is ON, blocks starting with the "/" code are ignored. They are
executed if the switch is OFF.
Parity check is valid regardless of whether the optional block skip switch is ON or OFF.
When, for instance, all blocks are to be executed for one workpiece but specific blocks are not to be executed
for another workpiece, the same command tape can be used to machine different parts by inserting the "/"
code at the head of those specific blocks.
Precautions
(1) Put the "/" code for optional block skip at the beginning of a block. If it is placed inside the block, it is
assumed as a user macro, a division instruction.
(Example)
N20 G1 X25. /Z25. ; ..........NG (User macro, a division instruction; a program error results.)
/N20 G1 X25. Z25. ; ..........OK
(2) Parity checks (H and V) are conducted regardless of the optional block skip switch position.
(3) The optional block skip is processed immediately before the pre-read buffer.
Consequently, it is not possible to skip up to the block which has been read into the pre-read buffer.
(4) This function is valid even during a sequence No. search.
(5) All blocks with the "/" code are also input and output during tape storing and tape output, regardless of
the position of the optional block skip switch.
16
Page 33
M700V/M70V Series Programming Manual (Lathe System)
3.3 Optional Block Skip
3.3.2 Optional Block Skip Addition ; /n
N4 N2
N2N3N4
Function and purpose
Whether the block with "/n (n:1 to 9)" (slash) is executed during automatic operation and searching is
selected.
By using the machining program with "/n" code , di ff ere nt parts can be machined by the same program.
Detailed description
The block with "/n" (slash) code is skipped when the "/n" is programmed to the head of the block and the
optional block skip n signal is turned ON. For a block with the "/n" code inside the block (not at the head of the
block), the program is operated according to the value of the parameter "#1226 aux10/bit1" setting.
When the optional block skip n signal is OFF, th e block with "/n" is executed.
Program example
(1) When the 2 parts like the figure below are machined, the following program is used. When the optional
block skip 5 signal is ON, the part 1 is created. When the optional block skip 5 signal is OFF, the part 2 is
created.
Part 1
Optional block skip 5 signal ON
N1 G54 ;
N2 G90 G81 X50. Z-20. R3. F100 ;
/5 N3 X30. ;
N4 X10. ;
N5 G80 ;
M02 ;
Part 2
Optional block skip 5 signal OFF
17
Page 34
3 Program Formats
MITSUBISHI CNC
(2) When two or more "/n" codes are commanded at the head of the same block, the block will be ignored if
either of the optional block skip n signals corresponding to the command is ON.
N01 G90 Z3. M03 S1000 ; (a) Optional block skip 1 signal ON
/1/2 N02 G00 X50. ;
/1/2 N03 G01 Z-20. F100 ;
/1/2 N04 G00 Z3. ;
/1 /3 N05 G00 X30. ; (b) Optional block skip 2 signal ON
/1 /3 N06 G01 Z-20. F100 ;
/1 /3 N07 G00 Z3. ;
/2/3 N08 G00 X10. ; (c) Optional block skip 3 signal ON
/2/3 N09 G01 Z-20. F100 ;
/2/3 N10 G00 Z3. ;
N11 G28 X0 M05 ;
N12 M02 ;
(Optional block skip 2.3 signal OFF)
N01 -> N08 -> N09 -> N10 -> N11 -> N12
(Optional block skip 1.3 signal OFF)
N01 -> N05 -> N06 -> N07 -> N11 -> N12
(Optional block skip 1.2 signal OFF)
N01 -> N02 -> N03 -> N04 -> N11 -> N12
(3) When the parameter "#1226 aux10/bit1" is "1"and two or more "/n" are commanded inside the same
block, the commands following "/n" in the block are ignored if either of the optional block skip n signals
corresponding to the command is ON.
N01 G91 G28 X0.Y0.Z0.; N03 block will operate as follows.
N02 G01 F1000;
N03 X1. /1 Y1. /2 Z1.;
N04 M30;
(a) Optional block skip 1 signal ON
Optional block skip 2 signal OFF
"Y1. Z1." is ignored.
(b) Optional block skip 1 signal OFF
Optional block skip 2 signal ON
"Z1." is ignored.
18
Page 35
M700V/M70V Series Programming Manual (Lathe System)
3.4 G code
3.4 G code
3.4.1 Modal, unmodal
G codes define the operation modes of each block in programs.
G codes can be modal or unmodal command.
Modal commands always designate one of the G codes in the group as the NC operation mode. The
operation mode is maintained until a cancel command is issued or other G code among the same group is
commanded.
An unmodal command designates the NC operation mode only when it is issued. It is invalid for the next
block.
3.4.2 G code Lists
G codes include the six G code lists 2, 3, 4, 5, 6 and 7.
cmdtyp G code lists
32
43
54
65
76
87
Here, G functions are explained using the G code list 3.
19
Page 36
3 Program Formats
MITSUBISHI CNC
3.4.3 Table of G Code Lists
G code lists
Group Function Section Standard Special
234567
ΔG00 ΔG00 ΔG00 ΔG00 ΔG00 ΔG00 01 Positioning 6.1
ΔG01 ΔG01 ΔG01 ΔG01 ΔG01 ΔG01 01 Linear interpolation 6.2
G02 G02 G02 G02 G02 G02 01
G03 G03 G03 G03 G03 G03 01
G02.3 G02.3 G02.3 G02.3 G02.3 G02.3 01 Exponential interpolation CW 6.11
G03.3 G03.3 G03.3 G03.3 G03.3 G03.3 01 Exponential interpolation CCW 6.11
G04 G04 G04 G04 G04 G04 00 Dwell 8.1
G07.1
G107
G09 G09 G09 G09 G09 G09 00 Exact stop check 7.10
G10 G10 G10 G10 G10 G10 00
G11 G11 G11 G11 G11 G11 00
G12.1
G112
G13.1
G113
G12.1 G12.1 G12.1 G12.1 19 Milling interpolation ON 6.8
*G13.1 *G13.1 *G13.1 *G13.1 19 Milling interpolation cancel 6.8
*G14 *G14 *G14 *G14 18 ● Balance cut OFF 13.18
G15 G15 G15 G15 18 ● Balance cut ON 13.18
G16 G16 G16 G16 02
ΔG17 ΔG17 ΔG17 ΔG17 ΔG17 ΔG17 02 Plane selection X-Y 6.5
ΔG18 ΔG18 ΔG18 ΔG18 Δ
ΔG19 ΔG19 ΔG19 ΔG19 ΔG19 ΔG19 02 Plane selection Y-Z 6.5
G18 ΔG1
G07.1
G107
G12.1
G112
G13.1
G113
19 Cylindrical interpolation 6.9
19 Polar coordinate interpolation ON 6.10
19 Polar coordinate interpolation cancel 6.10
8 02 Plane selection Z-X 6.5
Circular interpolation CW/Helical interpolation CW
Circular interpolation CCW/Helical interpolation CCW
Programmable parameter/Compensation
data input
/Tool life management data registration
Programmable parameter input
/Tool life management data registration
cancel
Milling interpolation plane selection Y-Z
cylindrical plane
6.3
6.4
6.7
6.3
6.4
6.7
12.5
13.15
12.5
13.15
6.8.3
20
Page 37
M700V/M70V Series Programming Manual (Lathe System)
3.4 G code
G code lists
234567
ΔG20 ΔG20 ΔG20 ΔG20 ΔG20 ΔG20 06 Inch command 5.3
ΔG21 ΔG21 ΔG21 ΔG21 ΔG21 ΔG21 06 Metric command 5.3
G22 G22 G22 G22 04 Barrier check ON 15.1
*G23 *G23 *G23 *G23 04 Barrier check OFF 15.1
G22 G22 00 Soft limit ON 15.2
G23 G23 00 Soft limit OFF 15.2
G27 G27 G27 G27 G27 G27 00 Reference position check 14.9
G28 G28 G28 G28 G28 G28 00 Automatic reference position return 14.7
G29 G29 G29 G29 G29 G29 00 Start position return 14.7
G30 G30 G30 G30 G30 G30 00 2nd, 3rd and 4th reference position return 14.8
G30.1 G30.1 G30.1 G30.1 G30.1 G30.1 00 Tool change position return 1 13.17
G30.2 G30.2 G30.2 G30.2 00 Tool change position return 2 13.17
G30.3 G30.3 G30.3 G30.3 00 Tool change position return 3 13.17
G30.4 G30.4 G30.4 G30.4 00 Tool change position return 4 13.17
G30.5 G30.5 G30.5 G30.5 00 Tool change position return 5 13.17
Group Function Section
G31 G31 G31 G31 G31 G31 00 Skip/Multi-step skip function 2
G31.1 G31.1 G31.1 G31.1 G31.1 G31.1 00 Multi-step skip function 1-1 16.3
G31.2 G31.2 G31.2 G31.2 G31.2 G31.2 00 Multi-step skip function 1-2 16.3
G31.3 G31.3 G31.3 G31.3 G31.3 G31.3 00 Multi-step skip function 1-3 16.3
G32 G33 G32 G33 G32 G33 01 Thread cutting
G34 G34 G34 G34 G34 G34 01 Variable lead thread cutting 6.6.4
G35 G35 G35 G35 G35 G35 01 Circular thread cutting CW 6.6.5
G36 G36 G36 G36 G36 G36 01 Circular thread cutting CCW 6.6.5
G36/G37
G37 G37 G36/G37 G36/G37
*G40 *G40 *G40 *G40 *G40 *G40 07 Tool nose radius compensation cancel 12.4
G41 G41 G41 G41 G41 G41 07 Tool nose radius compensation left 12.4
G42 G42 G42 G42 G42 G42 07 Tool nose radius compensation right 12.4
G46 G46 G46 G46 G46 G46 07
G43.1 G43.1 G43.1 G43.1 G43.1 G43.1 20 1st spindle control mode ON 10.10.2
G44.1 G44.1 G44.1 G44.1 G44.1 G44.1 20 Selected spindle control mode 10.10.2
G47.1 G47.1 G47.1 G47.1 G47.1 G47.1 20
G37.1
G37.2
G36/G37
G37.1
G37.2
00 Automatic Tool Length Measurement 16.1
Tool nose radius compensation (automatic direction identification) ON
All spindles simultaneous control mode
ON
16.2
16.4
6.6.1
6.6.2
12.4
10.10.2
G50 G92 G50 G92 G50 G92 00
*G50.2 *G50.2 *G50.2 *G50.2 11 Scaling cancel
G51.2 G51.2 G51.2 G51.2 11 Scaling ON
G50.2
G250
G51.2
G251
G52 G52 G52 G52 G52 G52 00 Local coordinate system setting 14.11
G53 G53 G53 G53 G53 G53 00
G50.2
G250
G51.2
G251
00
00
Spindle Clamp Speed Setting
Coordinate system setting
Polygon machining mode cancel
(spindle-tool axis synchronization)
Polygon machining mode ON
(spindle-tool axis synchronization)
Basic Machine Coordinate System Selection
10.3
14.6
10.7
10.7
14.5
21
Page 38
3 Program Formats
MITSUBISHI CNC
G code lists
234567
*G54 *G54 *G54 *G54 *G54 *G54 12 Workpiece coordinate system selection 1 14.10
G55 G55 G55 G55 G55 G55 12 Workpiece coordinate system selection 2 14.10
G56 G56 G56 G56 G56 G56 12 Workpiece coordinate system selection 3 14.10
G57 G57 G57 G57 G57 G57 12 Workpiece coordinate system selection 4 14.10
G58 G58 G58 G58 G58 G58 12 Workpiece coordinate system selection 5 14.10
G59 G59 G59 G59 G59 G59 12 Workpiece coordinate system selection 6 14.10
G54.1 G54.1 G54.1 G54.1 G54.1 G54.1 12
G61 G61 G61 G61 G61 G61 13 Exact stop check mode 7.11
G62 G62 G62 G62 G62 G62 13 Automatic Corner Override 7.13
G63 G63 G63 G63 G63 G63 13/19 Tapping mode 7.14
*G64 *G64 *G64 *G64 *G64 *G64 13/19 Cutting mode 7.15
G65 G65 G65 G65 G65 G65 00 User macro call 13.9.1
G66 G66 G66 G66 G66 G66 14 User macro modal call A 13.9.1
G66.1 G66.1 G66.1 G66.1 G66.1 G66.1 14 User macro modal call B 13.9.1
*G67 *G67 *G67 *G67 *G67 *G67 14 User macro modal call cancel 13.9.1
G68 G68 G68 G68 15 Mirror image for facing tool posts ON 13.10
G69 G69 G69 G69 15 Mirror image for facing tool posts OFF 13.10
G68 G68 15
*G69 *G69 15
Group Function Section
Work coordinate system selection 48 sets
expanded
Mirror image for facing tool posts ON or
balance cut mode ON
Mirror image for facing tool posts OFF or
balance cut mode cancel
14.10
13.10
13.10
G70 G70 G70 G70 G70 G70 09 Finishing cycle 13.3.4
G71 G71 G71 G71 G71 G71 09 Longitudinal rough cutting cycle 13.3.1
G72 G72 G72 G72 G72 G72 09 Face rough cutting cycle 13.3.2
G73 G73 G73 G73 G73 G73 09 Formed material rough cutting cycle 13.3.3
G74 G74 G74 G74 G74 G74 09 Face cut-off cycle 13.3.5
G75 G75 G75 G75 G75 G75 09 Longitudinal cut-off cycle 13.3.6
G76 G76 G76 G76 G76 G76 09 Compound thread cutting cycle 13.3.7
G76.1 G76.1 G76.1 G76.1 G76.1 G76.1 09
G76.2 G76.2 G76.2 G76.2 G76.2 G76.2 09
G90 G77 G90 G77 G90 G77 09 Longitudinal cutting fixed cycle 13.1.1
G92 G78 G92 G78 G92 G78 09 Thread cutting fixed cycle 13.1.2
G94 G79 G94 G79 G94 G79 09 Face cutting fixed cycle 13.1.3
*G80 *G80 *G80 *G80 *G80 *G80 09 Fixed cycle for drilling cancel
G81 G81 G81 G81 G81 G81 09 Fixed cycle (drill/spot drill)
G82 G82 G82 G82 G82 G82 09 Fixed cycle (drill/counter boring)
G79 G83.2 G79 G83.2 G79 G83.2 09 Deep hole drilling cycle 2 13.5.4
G83 G83 G83 G83 G83 G83 09
G83.1 G83.1 G83.1 G83.1 G83.1 G83.1 09 Stepping cycle
● 2-part system synchronous thread-cutting cycle (1)
● 2-part system synchronous thread-cutting cycle (2)
Deep hole drilling cycle (Z axis)
/Small-diameter deep-hole drilling cycle
13.21.2
13.21.3
13.5
13.5.5
13.6
13.6
13.6.1
13.6
13.6.2
13.5
13.5.1
13.6
13.6.4
22
Page 39
M700V/M70V Series Programming Manual (Lathe System)
3.4 G code
G code lists
234567
G84 G84 G84 G84 G84 G84 09 Tapping cycle (Z axis)
G85 G85 G85 G85 G85 G85 09 Boring cycle (Z axis)
Group Function Section
13.5
13.5.2
13.5
13.5.3
G87 G87 G87 G87 G87 G87 09 Deep hole drilling cycle (X axis)
G88 G88 G88 G88 G88 G88 09 Tapping cycle (X axis)
G89 G89 G89 G89 G89 G89 09 Boring cycle (X axis)
G84.1 G84.1 G84.1 G84.1 G84.1 G84.1 09 Reverse tapping cycle (Z axis) 13.5.2
G84.2 G84.2 G84.2 G84.2 G84.2 G84.2 09 Synchronous tapping cycle
G88.1 G88.1 G88.1 G88.1 G88.1 G88.1 09 Reverse tapping cycle (X axis) 13.5.2
G50.3 G92.1 G50.3 G92.1 G50.3 G92.1 00 Workpiece coordinate preset 14.12
ΔG96 ΔG96 ΔG96 ΔG96 ΔG96 ΔG96 17 Constant surface speed control ON 10.2
ΔG97 ΔG97 ΔG97 ΔG97 ΔG97 ΔG97 17 Constant surface speed control OFF 10.2
ΔG98 ΔG94 ΔG98 ΔG94 ΔG98 ΔG94 05 Feed per minute (asynchronous feed) 7.4
ΔG99 ΔG95 ΔG99 ΔG95 ΔG99 ΔG95 05 Feed per revolution (synchronous feed) 7.4
- ΔG90 - ΔG90 - ΔG90 03 Absolute value command 5.1
- ΔG91 - ΔG91 - ΔG91 03 Incremental value command 5.1
- *G98 - *G98 - *G98 10 Fixed cycle initial level return
- G99 - G99 - G99 10 Fixed cycle R point level return
Spindle synchronization cancel
G113 G113 G113 G113 00
G114.1 G114.1 G114.1 G114.1 00 Spindle synchronization 10.5.1
G114.2 G114.2 G114.2 G114.2 00
G114.3
G114.3 G114.3 G114.3 00
/Polygon machining (spindle-spindle synchronization) mode cancel
Polygon machining (spindle-spindle synchronization) mode ON
Tool spindle synchronization II (Hobbing)
ON
13.5
13.5.1
13.5
13.5.2
13.5
13.5.3
13.6
13.6.6
13.5
13.5.7
13.5
13.5.7
10.5
10.6
10.6
10.9
G115 G115 G115 G115 G115 G115 00
G116 G116 G116 G116 G116 G116 00
G117 G117 G117 G117 G117 G117 00 ● M code output during axis traveling
G126 G126 G126 G126 00 ● Control axis superimposition 13.20
● Start point designation synchronization
Type 1
● Start point designation synchronization
Type 2
13.19.2
13.19.3
23
Page 40
3 Program Formats
MITSUBISHI CNC
Precautions
CAUTION
(1) A program error (P34) will occur if a G code unlisted on the Table of G code lists is commanded.
(2) An alarm will occur if a G code without additional specifications is commanded.
(3) A (*) symbol indicates the G code to be selected in each group when the power is turned ON or when a
reset is executed to initialize the modal.
(4) A (Δ) symbol indicates the G code for which parameters selection is possible as an initialization status
when the power is turned ON or when a reset is executed to initialize the modal. Note that inch/metric
changeover can only be selected when the power is turned ON.
(5) A ( ● ) symbol indicates a function dedicated for multi-part system.
(6) If two or more G codes from the same group are commanded in a block, the last G code will be valid.
(7) This G code list is a list of conventional G codes. Depending on the machine, movements that differ from
the conventional G commands may be included when called by the G code macro. Refer to the
Instruction Manual issued by the tool builder.
(8) Whether the modal is initialized or not depends on each reset input.
- "Reset 1"
The modal is initialized when the reset initialization parameter (#1151 rstinit) is ON.
- "Reset 2 "and "Reset and Rewind"
The modal is initialized when the signal is input.
- Reset at emergency stop release
Conforms to "Reset 1".
- When modal is automatically reset at the start of individual functions such as reference point return.
Conforms to "Reset & rewind".
Precautions for G code lists 6 and 7
(1) G68,G69
When both the mirror image for facing tool posts option and balance cut option are valid, G68 and G69
will be handled as the command to turn the mirror image for facing tool posts ON/OFF.
(The mirror image for facing tool posts has the priority.)
(2) G36
G36 is used for the two functions, automatic tool length measurement and circular thread cutting (CCW).
Which function to be applied depend on the setting of the parameter "#1238 set10/bit0" (circular thread
cutting).
When "#1238 set10/bit0" is set to "0"
G code Function
G35 Circular thread cutting clockwise rotation (CW)
G36 Automatic tool length measurement X
G37 Automatic tool length measurement Z
When "#1238 set10/bit0" is set to "1"
G code Function
G35 Circular thread cutting clockwise rotation (CW)
G36
G37 Automatic tool length measurement Z
Circular thread cutting counterclockwise rotation
(CCW)
24
1. The commands with "no value after G" will be handled as "G00".
Page 41
M700V/M70V Series Programming Manual (Lathe System)
3.5 Precautions Before Starting Machining
3.5 Precautions Before Starting Machining
CAUTION
1. When creating the machining program, select the appropriate machining conditions, and
make sure that the performance, capacity and limits of the machine and NC are not
exceeded. The examples do not consider the machining conditions.
2. Before starting actual machining, always carry out graphic check, dry run operation and
single block operation to check the machining program, tool offset amount, workpiec e
offset amount and etc.
25
Page 42
3 Program Formats
MITSUBISHI CNC
26
Page 43
27
4
Pre-read Buffers
Page 44
4 Pre-read Buffers
MITSUBISHI CNC
4.1 Pre-read Buffers
Function and purpose
During automatic processing, the contents of 1 block are normally pre-read so that program analysis
processing is conducted smoothly. However, during tool nose radius compensation, a maximum of 5 blocks
are pre-read for the intersection point calculation including interference check.
Detailed description
The specifications of pre-read buffers in 1 block are as follows:
(1) The data of 1 block is stored in this buffer.
(2) When comments and the optional block skip function is ON, the data extending from the "/" (slash) code
up to the EOB code are not read into the pre-read buffer.
(3) The pre-read buffer contents are cleared with resetting.
(4) When the single block function is ON during continuous operation, the pre-read buffer stores the next
block's data and then stops operation.
(5) The way to prohibit the M command which operates the external controls from pre-reading, and to make
it to recalculate, is as follows:
Identify the M command which operates the external controls by a PLC, and turn on the "recalculation
request" on PLC output signal. (When the "recalculation request" is turned ON, the program that has
been pre-read is recalculated.)
Precautions
(1) Depending on whether the program is executed continuously or by single blocks, the timing of the
validation/invalidation of the external control signals including optional block skip, differ.
(2) If the external control signal such as optional block skip is turned ON/OFF with the M command, the
external control operation will not be effective for the program pre-read with the buffer register.
28
Page 45
29
5
Position Commands
Page 46
5 Position Commands
MITSUBISHI CNC
5.1 Incremental/Absolute Value Commands ; G90,G91
z1 w1 P1
P2
u1
x1
X
Z
2
Function and purpose
There are two methods of issuing tool movement amount commands: the incremental value method and the
absolute value method.
To designate the coordinates of a point to be moved, the incremental value method issues a command using
the distance from the present point; on the other hand, the absolute value method issues a command using
the distance from the coordinate zero point.
Use an axis address or a G command to choose between the incremental or absolute value command.
Whether an axis address or a G command is valid can be selected according to the parameter setting.
The following figure shows what happens when the tool is moved from point P1 to point P2.
(1) Movement command by an axis address (when "#1076 AbsInc" is "1")
Absolute value command: G00 Xx1 Zz1 ;
Incremental value command: G00 Uu1 Ww1 ;
(2) Movement command by a G command (when "#1076 AbsInc" is "0")
Absolute value command: G90 G00 Xx1 Zx1 ;
Incremental value command: G91 G00 Xu1 Zw1 ;
Command format
G90; ... Absolute value command
G91; ... Incremental value command
When the parameter "#1076 AbsInc" is set to "0", a G command selects either the incremental or absolute
value commands.
After commanding G90/ G91, coordinates will be commanded with incremental or absolute values.
30
Page 47
M700V/M70V Series Programming Manual (Lathe System)
5.1 Incremental/Absolute Value Commands ; G90,G91
Detailed description
Selection between incremental or absolute value commands by an axis address
When the parameter "#1076 AbsInc" is set to "1", an axis address selects either the incremental or absolute
value commands.
(1) Set correspondence between addresses and axes with the following parameters.
#1013 axname
#1014 incax
Following table shows the example of when "X,Z,C,Y" are set to "#1013 axname" and "U,W,H,V" are set
to "#1014 incax".
Command method
Absolute
value
Incremental
value
(Note 1) The C/Y axis is an example of additional axes.
X axis Address X
Z axis Address Z
C/Y axis Address C/Y
X axis Address U
Z axis Address W
C/Y axis Address H/V
(2) Absolute and incremental values can be used together in the same block.
(Example) X__ W__ ; ... An absolute value command for X axis and an incremental value command for Z
axis
Precautions
(1) Designation of a circular radius (R) and center (I,J,K) is always conducted with incremental values.
(2) When parameter "#1076 AbsInc" is 1, and H is used for the incremental command address, address H of
blocks in M98, G114.2, and G10 L50 modal will be handled as the parameter of each command, and the
axis will not be moved.
31
Page 48
5 Position Commands
MITSUBISHI CNC
5.2 Radius/Diameter Designation
P1
P2
X
Z
r2
r1
Function and purpose
On a lathe, a workpiece rotates, so its coordinate positions, dimensions, and commands can be designated by
radius/ diameter values. Commands using diameter values are called diameter designation, and commands
with radius values are called radius designation.
Either radius or diameter designation can be used depending on the setting of the parameter (#1019 dia).
The figure below shows the command procedure when the tool is to be moved from point P1 to point P2.
X command U command Remarks
Radius Diameter Radius Diameter Even when a diameter designation has been selected, the
U command can exclusively be changed into a radius des-
X = r1 X = 2 * r1 U = r2 U = 2 * r2
ignation by the parameter "#1077 radius".
(Note) "U"is an incremental command address.
Precautions and restrictions
(1) In the above example, the tool moves from P1 to P2 in the minus direction of the X axis. So when this is
using incremental value command, the minus sign is given to the numerical value being commanded.
(2) In this manual, diameter commands are used in descriptions of both the X and U axes for the sake of
convenience.
32
Page 49
M700V/M70V Series Programming Manual (Lathe System)
5.3 Inch/Metric Conversion ; G20,G21
5.3 Inch/Metric Conversion ; G20,G21
Function and purpose
The commands can be changed between inch and metric with the G20/G21 command.
Command format
G20; ... Inch command
G21; ... Metric command
Detailed description
The G20 and G21 commands merely select the command units. They do not select the Input units.
G20 and G21 selection is meaningful only for linear axes. It is invalid for rotation axes.
Output unit, command unit and setting unit
The counter or parameter setting and display unit is determined by parameter "#1041 I_inch". The movement/
speed command will be displayed as metric units when "#1041 I_inch" is ON during the G21 command mode.
The internal unit metric data of the movement/speed command will be converted into an inch unit and
displayed when "#1041 I_inch" is OFF during the G20 command mode. The command unit fo r when the
power is turned ON and reset is decided by combining the parameters "#1041 I_inch", "#1151 rstint" and
"#1210 RstGmd/bit5".
NC axis
Initial inch OFF
Item
Movement/speed command Metric Inch Metric Inch
Counter display Metric Metric Inch Inch
Speed display Metric Metric Inch Inch
User parameter setting/display Metric Metric Inch Inch
Workpiece/tool offset setting/display Metric Metric Inch Inch
Handle feed command Metric Metric Inch Inch
(metric internal unit)
#1041 I_inch=0
G21 G20 G21 G20
Initial inch ON
(inch internal unit)
#1041 I_inch=1
PLC axis
Item #1042 pcinch=0 (metric) #1042 pcinch=1 (inch)
Movement/speed command Metric Inch
Counter display Metric Inch
User parameter setting/display Metric Inch
33
Page 50
5 Position Commands
MITSUBISHI CNC
Precautions
(1) The parameter and tool data will be input/output with the unit set by "#1041 I_inch".
If "#1041 I_inch" is not found in the parameter input data, the unit will follow the unit currently set to NC.
(2) The unit of read/write used in PLC window is fixed to metric unit regardless of a parameter and G20/G21
command modal.
(3) A program error (P33) will occur if G20/G21 command is issued in the same block as following G code.
Command in a separate block.
- G7.1 (Cylindrical Interpolation)
- G12.1 (Polar coordinate interpolation)
34
Page 51
M700V/M70V Series Programming Manual (Lathe System)
5.4 Decimal Point Input
5.4 Decimal Point Input
Function and purpose
This function enables to input decimal points. It assigns the decimal point in millimeter or inch units for the
machining program input information that defines the tool paths, distances and speeds.
Use the parameter "#1078 Decpt2" to select whether minimum input command increment (type I) or zero point
(type II) to apply to the least significant digit of data without a decimal point.
Detailed description
(1) The decimal point command is valid for the distances, angles, times and speeds in machining programs.
(2) Refer to the table "Addresses used, validity of decimal point commands" for details on the valid
addresses for the decimal point commands.
(3) In decimal point command, the valid range of command value is as shown below. (for input command
increment cunit=10)
Input unit
[mm]
Input unit
[inch]
Movement command
(linear)
-99999.999 to
99999.999
-9999.9999 to
9999.9999
Movement command
(rotary)
-99999.999 to
99999.999
Feedrate Dwell
0.001 to
10000000.000
0.0001 to
1000000.0000
0 to 99999.999
(4) The decimal point command is valid even for commands defining the variable data used in subprograms.
(5) Decimal point commands for decimal point invalid addresses are processed as an integer only data
which everything below the decimal point is ignored. Decimal point invalid addresses include the
followings; D,H,L,M,N,O,P,S,T.
All variable commands, however, are treated as data with decimal points.
Decimal point input I, II and decimal point command validity
Decimal point input I and II will result as follows when decimal points are not used in an address which a
decimal point command is valid. Whether an address is valid or invalid for the decimal point command is
shown in the table below.
Both decimal point input I and II will produce the same result when a command uses a decimal point.
(1) Decimal point input I
The least significant digit of command data matches the command unit.
(Example) When "X1" is commanded in 1μm system, the same result occurs as for an "X0.001"
command.
(2) Decimal point input II
The least significant digit of command data matches the command unit.
(Example) When "X1" is commanded in 1μm system, the same result occurs as for an "X1." command.
35
Page 52
5 Position Commands
MITSUBISHI CNC
-Addresses used, validity of decimal point commands-
Decimal
Ad-
dress
Point
Command
Application Remarks
Valid Coordinate position data
Invalid 2nd miscellaneous function code
Valid Angle data
Invalid MRC program No.
A
Invalid
Valid
Valid
Valid Coordinate position data
B
Invalid 2nd miscellaneous function code
Programmable parameter input
Axis No.
Deep hole drilling cycle (2)
Safety distance
Spindle synchronous acceleration/deceleration time constant
Valid Coordinate position data
J
K
Invalid 2nd miscellaneous function code
Valid Corner chamfering amount ,C
C
Valid
Program tool compensation input
Nose R compensation amount (incremental)
Valid Chamfering width (slitting cycle)
Valid
D
Invalid
Invalid
Valid
E
Automatic tool length measurement,
deceleration range d
Programmable parameter input
byte type data
Synchronous spindle No. at
spindle synchronization
Inch threads
Precision thread lead
L
Valid Corner cutting feedrate
Valid Feedrate
F
Valid Thread lead Invalid Synchronization
Decimal
Ad-
dress
Point
Command
Valid Circular center coordinates
Nose R compensation/
Valid
tool radius compensation vector components
Invalid
Valid
Deep hole drilling cycle (2)
Dwell at return point
Hole drilling cycle
G1 in-position width
Valid Circular center coordinates
Nose R compensation/
Valid
tool radius compensation vector components
Invalid
Valid
Valid
Invalid
Invalid
Invalid
Invalid
Hole drilling cycle
Number of repetitions
Deep hole drilling cycle (2)
Second and subsequent cut amounts
Thread lead increase/decrease amount
(variable lead thread cutting)
Subprogram
Number of repetitions
Program tool compensation input
Type selection
Programmable parameter input selection
Programmable parameter input
two-word type data
G Valid Preparatory function code Invalid Tool life data
Valid Coordinate position data M Invalid Miscellaneous function codes
Invalid
Invalid
H
Invalid
Invalid
Sequence Nos. in subprograms
Programmable parameter input
bit type data
Selection of linear - arc
intersection (geometric)
Basic spindle No. at spindle
synchronization
Valid Circular center coordinates
Nose R compensation/
Valid
tool radius compensation vector components
I
Valid
Valid
Deep hole drilling cycle (2)
First cut amount
G0/G1 in-position width
Hole drilling cycle G0 in-position width
,I
Invalid Sequence Nos.
N
Invalid
Programmable parameter input
No.
data
O Invalid Program No.
Invalid Dwell time
Invalid
Invalid
Invalid
P
Invalid
Valid
Subprogram call
Program No.
2nd, 3rd and 4th reference
position No.
Constant surface speed control, axis
No.
MRC finishing shape start
sequence No.
Cut-off cycle
shift amount/cut amount
Compound thread cutting cycle
Invalid
number of cutting passes,
chamfering, tool nose angle
Application Remarks
,J
L2
L10
L11
L70
4
byte
(Note 1) Decimal points are all valid in user macro arguments.
36
Page 53
M700V/M70V Series Programming Manual (Lathe System)
5.4 Decimal Point Input
Decimal
Ad-
dress
Point
Command
Valid
Invalid
Invalid
Compound thread cutting cycle
Thread height
Program tool compensation
input compensation No.
Programmable parameter input
section No.
Valid Coordinate position data Valid Coordinate position data
Application Remarks
R
Invalid Skip signal command
P
Valid
Arc center coordinates (absolute value)
(geometric)
Subprogram return destination se-
Invalid
quence No.
Invalid
Extended workpiece coordinate system
No.
Decimal
Ad-
dress
Point
Command
Valid
Compound thread cutting cycle
turning cycle, taper difference
Hole drilling cycle/deep hole
Valid
drilling cycle (2)
Distance to R point
Valid
Valid
Invalid
Valid
Program tool compensation input
Nose R compensation
Rough cutting cycle
(longitudinal) (face) pull amount
Synchronous tap/ asynchronous
tap changeover
Synchronous spindle phase shift
amount
Invalid Spindle function codes
Application Remarks
Invalid Maximum spindle clamp rotation speed
Invalid Tool life data group No.
Invalid Minimum spindle clamp rotation speed
Invalid
Valid
Valid
Valid
Q
Valid
Invalid
Invalid
Valid
MRC finishing shape end
Cut-off cycle
Cut amount/shift amount
Compound thread cutting cycle
Minimum cut amount
Compound thread cutting cycle
First cut amount
Deep hole drilling cycle 1
Cut amount of each pass
Program tool compensation input
Hypothetical tool nose point No.
Deep hole drilling cycle (2)
Dwell at cut point
Arc center coordinates (absolute value)
(geometric)
Valid Thread cutting start shift angle
Invalid Tool life data management method Valid Program tool compensation input
Valid R-designated arc radius
Valid Arc radius of corner rounding ,R Valid Program tool compensation input
Valid
Valid MRC longitudinal/face escape amount
R
Invalid MRC shaping division No.
Automatic tool length measurement,
deceleration range r
S
Invalid
Invalid
Constant surface speed control, surface
speed
Programmable parameter input
word type data
T Invalid Tool function codes
Valid Coordinate position data
Valid Program tool compensation input
U
Valid
Rough cutting cycle (longitudinal)
Cut amount
Valid Dwell
Valid Coordinate position data
V
Valid Program tool compensation input
Valid Coordinate position data
Valid Program tool compensation input
W
Valid
Rough cutting cycle (longitudinal)
Cut amount
Valid Coordinate position data
X
Valid Dwell
Valid Program tool compensation input
Valid
Y
Valid Coordinate position data
Z
Coordinate position data
Valid Cut-off cycle, return amount
Valid Cut-off cycle, escape amount
Valid
Compound thread cutting cycle
Finishing allowance
,R
2
byte
(Note 1) Decimal points are all valid in user macro arguments.
37
Page 54
5 Position Commands
MITSUBISHI CNC
Program example
(1) Program example of decimal point valid address
Program example
G0 X123.45
(decimal points are all mm points)
G0 X12345
#111 = 123 #112 = 5.55
X#111 Z#112
#113 = #111 + #112
(addition)
#114 = #111 - #112
(subtraction)
#115 = #111 * #112
(multiplication)
#116 = #111 / #112
#117 = #112 / #111
(division)
X123.450 mm X123.450 mm X123.450 mm
X12.345 mm
(last digit is 1μm unit)
X123.000 mm
Z5.550 mm
#113 = 128.550 #113 = 128.550 #113 = 128.550
#114 = 117.450 #114 = 117.450 #114 = 117.450
#115 = 682.650 #115 = 682.650 #115 = 682.650
#116 = 22.162
#117 = 0.045
Decimal point command 1 Decimal point
When 1 = 10μm When 1 = 10μm
X123.450 mm X12345.000 mm
X123.000 mm
Z5.550 mm
#116 = 22.162
#117 = 0.045
When 1 = 1mm
X123.000 mm
Z5.550 mm
#116 = 22.162
#117 = 0.045
command 2
Precautions
(1) If an arithmetic operator is inserted, the data will be handled as data with a decimal point.
(Example1) G00 X123+0 ;
This is the X axis command 123mm command. It will not be 123μm.
38
Page 55
39
6
Interpolation Functions
Page 56
6 Interpolation Functions
MITSUBISHI CNC
6.1 Positioning (Rapid Traverse) ; G00
CAUTION
Function and purpose
This command is accompanied by coordinate words and performs high-speed positioning of a tool, from the
present point (start point) to the end point specified by the coordinate words.
Command format
G00 X__/U__ Z__/W__ ; ... Positioning (Rapid Traverse)
X_/U_
Z_/W_
The command addresses are valid for all additional axes.
X axis end point coordinate (X is the absolute value of workpiece coordinate system, U is the
incremental value from present position)
Z axis end point coordinate (Z is the absolute value of workpiece coordinate system, W is the
incremental value from present position)
Detailed description
(1) Positioning will be performed at the rapid traverse rate set in the parameter "#2001 rapid".
(2) G00 command belongs to the 01 group and is modal. When G00 command is successively issued, the
following blocks can be specified only by the coordinate words.
(3) In the G00 mode, acceleration and deceleration are always carried out at the start point and end point of
the block. Before advancing to the next block, a commanded deceleration or an in-position check is
conducted at the end point to confirm that the movement is completed.
(4) G functions (G83 to G89) in the 09 group are cancelled (G80) by the G00 command.
1. The commands with "no value after G" will be handled as "G00".
40
Page 57
M700V/M70V Series Programming Manual (Lathe System)
6.1 Positioning (Rapid Traverse) ; G00
Tool path
300
(mm)
(E)
(S)
fx=6400mm/min
X
Z
400
fz=9600mm/min
300
(mm)
(E)
(S)
fx=9600mm/min
X
Z
400
fz=9600mm/min
Whether the tool moves along a linear or non-linear path can be selected by the parameter "#1086 G0Intp".
The positioning time does not change according to the path.
(1) Linear path: When the parameter "#1086 G0Intp" is set to "0"
In positioning, a tool follows the shortest path which connects the start point and the end point. The
positioning speed is automatically calculated so that the shortest distribution time is obtained in order
that the commanded speeds for each axis do not exceed the rapid traverse rate.
When, for instance, the X-axis and Z-axis rapid traverse rates are both 9600mm/min;
G00 Z-300000 X400000 ; (With an input setting unit of 0.001mm)
The tool will follow the path shown in the figure below.
(S) Start point
(E) End point
(fx) Actual X axis rate
(fz) Actual Z axis rate
(2) Non-linear path: When the parameter "#1086 G0Intp" is set to "1"
In positioning, the tool will move along the path from the start point to the end point at the rapid traverse
rate of each axis.
When, for instance, the X-axis and Z-axis rapid traverse rates are both 9600mm/min;
G00 Z-300000 X400000 ; (With an input setting unit of 0.001mm)
The tool will follow the path shown in the figure below.
(S) Start point
(E) End point
(fx) Actual X axis rate
(fz) Actual Z axis rate
41
Page 58
6 Interpolation Functions
MITSUBISHI CNC
Program example
+X
+Z
(E)
(S)
(mm)
(+180,+300)
(+100,+150)
G00 X100. Z150. ; Absolute value command
G00 U-80. W-150. ; Incremental value command
Precautions for deceleration check
(S) Start point
(E) End point
There are two methods for the deceleration check; commanded deceleration method and in-position check
method. Select a method with the parameter "#1193 inpos".
A block with an in-position width command performs an in-position check with a temporarily changed inposition width. (Programmable in-position width command)
The deceleration check method set in basic specification parameter "#1193 inpos" is used for blocks that do
not have the in-position width command.
When the error detection is ON, the in-position check is forcibly carried out.
Rapid traverse (G00)
,I command
Cutting feedrate
,I command
No
Yes In-position check method (In-position check by ",I", "#2077 G0inps", "#2224 SV024")
(G01)
No
Yes In-position check method (In-position check by ",I", "#2078 G1inps", "#2224 SV024")
01
Commanded deceleration method (Commanded deceleration check which varies according to the type of acceleration/
deceleration, set in "#2003 smgst" bit3-0)
01
Commanded deceleration method (Commanded deceleration check which varies according to the type of acceleration/
deceleration, set in "#2003 smgst" bit7-4)
#1193 inpos
In-position check method (In-position check by
"#2077 G0inps", "#2224 SV024")
#1193 inpos
In-position check method (In-position check by
"#2078 G1inps", "#2224 SV024")
* Following descriptions are for the case of rapid traverse. For G01, interpret the parameters into suitable
ones.
42
Page 59
M700V/M70V Series Programming Manual (Lathe System)
6.1 Positioning (Rapid Traverse) ; G00
Commanded deceleration method when "inpos" = "0"
Td Ts
G00 Xx1; G00 Xx2;
2×Ts
Ts
Td
G00 Xx1; G00 Xx2;
Upon completion of the rapid traverse (G00), the next block will be executed after the deceleration check time
(Td) has elapsed.
The deceleration check time (Td) is as follows, depending on the acceleration/deceleration type set in the
parameter "#2003 smgst".
(1) Linear acceleration/linear deceleration
G00 Xx1; G00 Xx2;
Ts
Td
(Ts) Acceleration/deceleration time constant (Td) Deceleration check time: Td = Ts + (0 to 7ms)
(2) Exponential acceleration/linear deceleration
(Ts) Acceleration/deceleration time constant (Td) Deceleration check time: Td = 2 × Ts + (0 to 7ms)
(3) Exponential acceleration/exponential deceleration (Primary delay)
(Ts) Acceleration/deceleration time constant (Td) Deceleration check time: Td = 2 × Ts + (0 to 7ms)
The time required for the deceleration check is the longest among the deceleration check times of each axis
determined by the acceleration/deceleration mode and time constants of the axes commanded
simultaneously.
43
Page 60
6 Interpolation Functions
MITSUBISHI CNC
In-position check method when "inpos" = 1
SV024
(a)
(b)
G0inps
A
G0inps
(a)
(b)
SV024
A
Upon completion of the rapid traverse (G00), the next block will be executed after confirming that the
remaining distances for each axis are below the fixed amounts.
The confirmation of the remaining distance should be done with the imposition width.
The bigger one of the servo parameter "#2224 SV024" or G0 in-position width "#2077 G0inps" (For G01, inposition width "#2078 G1inps"), will be adapted as the in-position width.
The purpose of the rapid traverse deceleration check is to minimize the positioning time. The bigger the
setting value for the in-position width, the shorter the time is, but the remaining distance of the previous block
at the start of the next block also becomes larger, and this could become an obstacle in the actual processing
work.
The check for the remaining distance is done at set intervals. Accordingly, it may not be possible to get the
effect of time reduction for positioning as in-position width setting value.
(1) In-position check by the G0inps: When SV024 < G0inps (Stop is judged at A in the figure)
(a) Command to motor
(b) Outline of motor movement
(2) In-position check using SV024: When G0inps < SV024 (Stop is judged at A in the figure)
44
(a) Command to motor
(b) Outline of motor movement
Page 61
M700V/M70V Series Programming Manual (Lathe System)
6.1 Positioning (Rapid Traverse) ; G00
Programmable in-position width command
This command commands the in-position width for the positioning command from the machining program.
G00 X_ Z_ ,I_ ;
X,Z Positioning coor din ate value of each axis
,I In-position width
Execution of the next block starts after confirming that the position error amount of the positioning (rapid
traverse: G00) command block is less than the in-position width issued in this command.
The bigger one of in-position width (SV024，G0inps (For G01, G1inps)) with parameter or in-position width
specified by program will be adapted as the in-position width.
When there are several movement axes, the system confirms that the position error amount of each
movement axis in each part system is less than the in-position width issued in this command before executing
the next block.
The differences of In-position check
The differences between the in-position check with parameter and with programmable command are as
follows:
(1) In-position check with parameter
After completing deceleration of the command system (A), the servo system's position error amount and
the parameter setting value (in-position width) are compared.
(a)
(b)
(c)
(a) Servo machine position
G00 Xx1;
Ts
(b) Command
(c) In-position width (Servo system position error amount)
(Ts) Acceleration/deceleration time constant
(Td) Deceleration check time: Td = Ts + (0 to 7ms)
Td
A
(2) In-position check with programmable command (",I" address command)
After starting deceleration of the command system (A), the position error amount and commanded inposition width are compared.
(a)
G00 Xx1;
Ts
(b)
(c)
(a) Servo machine position
(b) Command
(c) In-position width (Error amount between command end point and
machine position)
(Ts) Acceleration/deceleration time constant
(Td) Deceleration check time: Td = Ts + (0 to 7ms)
Td
A
45
Page 62
6 Interpolation Functions
MITSUBISHI CNC
6.2 Linear Interpolation ; G01
X
U
/
2
Z W
Z
X
Function and purpose
This command is accompanied by coordinate words and a feedrate command. It makes the tool move
(interpolate) linearly from its current position to the end point specified by the coordinate words at the speed
specified by address F. In this case, the feedrate specified by address F always acts as a linear speed in the
tool nose center advance direction.
Command format
G01 X__/U__ Z__/W__ α__ F__ ,I__ ; ... Linear interpolation
X,U,Z,W,α Coordinate values (where α is the additional axis.)
F Feedrate (mm/min or °/min)
,I
In-position width. This is valid only in the commanded block. A block that does not contain
this address will follow the parameter "#1193 inpos" settings. 1 to 999999 (mm)
46
Detailed description
(1) G01 command is a modal command in the 01 group. When G01 command is issued in succession, it can
only be issued with coordinate words in subsequent blocks.
(2) The feedrate for a rotation axis is commanded by °/min (decimal point position unit). (F300=300°/min)
(3) The G functions (G70 to G89) in the 09 group are cancelled (G80) by the G01 command.
Programmable in-position width command for linear interpolation
This command commands the in-position width for the linear interpolation command from the machining
program.
G01 X_ Z_ F_ ,I_ ;
X,Z Linear interpolation coordinate value of each axis
F Feedrate
,I In-position width
The commanded in-position width is valid in the linear interpolation command only when carrying out
deceleration check.
- When the error detection switch is ON.
- When G09 (exact stop check) is commanded in the same block.
- When G61 (exact stop check mode) is selected.
(Note 1) Refer to section "Positioning (Rapid Traverse); G00" for details on the in-position check operation.
Page 63
M700V/M70V Series Programming Manual (Lathe System)
6.2 Linear Interpolation ; G01
Program example
20.0
50.0
X
Z
(mm)
(Example 1)
G01 X50.0 Z20.0 F300 ;
(Example 2) Cutting in the sequence of P1 -> P2 -> P3 -> P4 at 300mm/min feedrate.
However, P0 -> P1 and P4 -> P0 are for tool positioning.
240
P1
200
140
P3
100
P2
2209040 230160
G00 X200. Z40. ; P0 -> P1
G01 X100. Z90. F300 ; P1 -> P2
Z160. ; P2 -> P3
X140. Z220. ; P3 -> P4
G00 X240. Z230. ; P4 -> P0
+X
P0
+Z
P4
(mm)
47
Page 64
6 Interpolation Functions
MITSUBISHI CNC
6.3 Circular Interpolation ; G02,G03
X
Z
KW
U/2
I
Z
X
(E)
(S)
(CP)
Function and purpose
These commands serve to move the tool along a circular.
Command format
G02 X__/U__ Z__/W__ I__ K__ F__ ; ... Circular interpolation : Clockwise (CW)
G03 X__/U__ Z__/W__ I__ K__ F__ ; ... Circular interpolation : Counterclockwise (CCW)
X/U
Z/W
I
K
F Feedrate
Circular end point coordinates, X axis (X is the absolute value of workpiece coordinate system, U is
the incremental value from present position)
Circular end point coordinates, Z axis (Z is the absolute value of workpiece coordinate system, W is
the incremental value from present position)
Circular center, X axis (I is the radius command incremental value of X coordinate at the center as
seen from the start point.)
Circular center, Z axis (K is the incremental value of Z coordinate at the center as seen from the start
point.)
Detailed description
(1) The arc center coordinate value is commanded with an input setting unit. Caution is required for the
circular command of an axis for which the program command unit (#1015 cunit) differs. Command with a
decimal point to avoid confusion.
48
(S) Start point
(E) End point
(CP) Center
Page 65
M700V/M70V Series Programming Manual (Lathe System)
6.3 Circular Interpolation ; G02,G03
(2) G02 (G03) is a modal command of the 01 group. When G02 (G03) command is issued continuously, the
next block and after can be commanded with only coordinate words.
The circular rotation direction is distinguished by G02 and G03.
G02 Clockwise (CW)
G03 Counterclockwise (CCW)
+X
CCW(G03)
+X
CW(G02)
+Z
+Z
CW(G02)
+Z
+X
CCW(G03)
+X
(3) An arc which extends for more than one quadrant can be executed with a single block command.
(4) The following information is needed for circular interpolation.
(a) Rotation direction : Clockwise (G02) or counterclockwise (G03)
(b) Circular end point coordinates : Given by addresses X, Z, U, W
(c) Circular center coordinates : Given by addresses I, K (incremental value commands)
(d) Feedrate : Given by address F
(5) A program error results when I, K or R is not commanded.
Consideration must be given to the sign for I and K since I is the distance in the X-axis direction to the arc
center from the start point and K in the Z-axis direction.
(6) No T commands can be issued in the G2/G3 modal status.
A program error (P151) will occur if a T command is issued in the G2/G3 modal status.
49
Page 66
6 Interpolation Functions
MITSUBISHI CNC
Change into linear interpolation command
N1
N3
20
0
120.0
20.0
70.0 50.0
50.0
X
Z
(mm)
Program error (P33) will occur when the center and radius are not designated at circular command.
When the parameter "#11029 Arc to G1 no Cent (Change command from arc to linear when no arc center
designation)" is set, the linear interpolation can be operated up to the terminal coordinate value only for that
block. However, a modal is the circular modal.
This function is not applied to a circular command by a geometric function.
(Example)The parameter "#11029 Arc to G1 no Cent (Change command from arc to linear when no arc center
designation)" = "1"
G90 X0 Y0 ;
N1 G02 X20. I10. F500 ; ... (a)
N2 G00 X0 ;
N3 G02 X20. F500 ; ... (b)
M02 ;
(a) The circular interpolation (G02) is executed because there is a center command.
(b) The linear interpolation (G01) is executed because there is no center and radius command.
Program example
G2 X120.0 Z70.0 I50.0 F200 ; Absolute value command
G2 U100.0 W-50.0 I50.0 F200 ; Incremental value command
50
Page 67
M700V/M70V Series Programming Manual (Lathe System)
6.3 Circular Interpolation ; G02,G03
Precautions
G02Z80.K50. ;
R
X
Z
(AL)
(S)
(SR)
(E)
(ER)
(CP)
R
G02Z90.K50. ;
X
Z
(SI)
(S)
(SR)
(E)
(ER)
(CP)
(1) The terms "clockwise" (G02) and "counterclockwise" (G03) used for circular operations are defined as a
case where, in a right-hand coordinate system, the negative direction is viewed from the positive
direction of the coordinate axis which is at right angles to the plane in question.
(2) If all the end point coordinates are omitted or the end point is at the same position as the start point,
commanding the center using I and K is the same as commanding a 360°arc (perfect circle).
(3) The following occurs when the start and end point radius do not match in a circular command :
(a) Program error (P70) results at the circular start point when error ΔR is greater than parameter "#1084 RadErr".
#1084 RadErr Parameter value 0.100
Start point radius=5.000
End point radius=4.899
ErrorΔR=0.101
(S) Start point
(CP) Center
(E) End point
(SR) Start point radius
(ER) End point radius
(AL) Alarm stop
(b) Spiral interpolation in the direction of the commanded end point will be conducted when error ΔR is less than the
parameter value.
#1084 RadErr Parameter value 0.100
Start point radius=5.000
End point radius=4.900
ErrorΔR=0.100
(S) Start point
(CP) Center
(E) End point
(SR) Start point radius
(ER) End point radius
(SI) Spiral interpolation
51
Page 68
6 Interpolation Functions
MITSUBISHI CNC
6.4 R Specification Circular Interpolation ; G02,G03
L
1
2
r
Function and purpose
Along with the conventional circular interpolation commands based on the circular center coordinate (I, K)
designation, these commands can also be issued by directly designating the circular radius R.
Command format
G02 X/U__ Z/W__ R__ F__ ; ... R specification circular interpolation Clockwise (CW)
G03 X/U__ Z/W__ R__ F__ ; ... R specification circular interpolation Counterclockwise (CCW)
X/U X axis end point coordinate
Z/W Z axis end point coordinate
R Circular radius
F Feedrate
The arc radius is commanded with an input setting unit. Caution is required for the arc command of an axis
for which the input command unit differs. Command with a decimal point to avoid confusion.
Detailed description
The circular center is on the bisector line which is perpendicular to the line connecting the start and end points
of the circular. The point, where the circular with the specified radius whose start point is the center intersects
the perpendicular bisector line, serves as the center coordinates of the circular command.
If the R sign of the commanded program is plus, the circular is smaller than a semicircular; if it is minus, the
circular is larger than a semicircular.
R < 0
(E)
(S) Start point
(E) End point
R > 0
L
(S)
The following condition must be met with an R-specified arc interpolation command:
r
When (L/2 - r) > (parameter : #1084 RadErr), an alarm will occur.
Where L is the line from the start point to the end point. If an R specification and I, K specification are given at
the same time in the same block, the circular command with the R specification takes precedence. In the case
of a full-circle command (where the start and end points coincide), an R specification circular command will be
completed immediately even if it is issued and no operation will be executed . An I, K specification circular
command should therefore be used in such a case.
52
Page 69
M700V/M70V Series Programming Manual (Lathe System)
6.4 R Specification Circular Interpolation ; G02,G03
Circular center coordinate compensation
010
N1, N3
N5
When "the error margin between the segment connecting the start and end points" and "the commanded
radius × 2" is less than the setting value because the required semicircle is not obtained by calculation error in
R specification circular interpolation, "the midpoint of segment connecting the start and end points" is
compensated as the circular center.
Set the setting value to the parameter "#11028 Tolerance Arc Cent (Tolerable correction value of arc center
error)".
(Example)"#11028 Tolerance Arc Cent" = "0.000 (mm)"
Setting value Tolerance value
Setting value < 0 0(Center error will not be interpolated)
Setting value = 0 2×minimum setting increment
Setting value > 0 Setting value
G90 X0 Y0 ;
N1 G02 X10. R5.000;
N2 G0 X0; ...(a)
N3 G02 X10. R5.001;
N4 G0 X0; ...(b)
N5 G02 X10. R5.002;
N6 G0 X0;
M02 ;
(a) Compensate the center coordinate: Same as N1 path
(b) Do not compensate the center coordinate: Inside path a little than N1
Calculation error margin compensation allowance value: 0.002 mm
Segment connecting the start and end paints: 10.000
N3: Radius × 2 = 10.002 "Error 0.002 -> Compensate"
N5: Radius × 2 = 10.004 "Error 0.004 -> Do not compensate"
Therefore, this example is shown in the above figure.
Program example
(Example 1)
G03 Zz1 Xx1 Rr1 Ff1 ; R specification circular on Z-X plane
(Example 2)
R specification circular on X-Z plane
G02 Xx1 Zz1 Ii1 Kk1 Rr1 Ff1 ;
(When the R specification and I, K specification are contained in
the same block, the R specification has priority in processing.)
53
Page 70
6 Interpolation Functions
MITSUBISHI CNC
6.5 Plane Selection ; G17,G18,G19
J
I
G02
G03
G02
G03
G02
G03
J
I
K
K
J
I
K
G3
G3
G3
G2
G2
G2
G17 (I-J)
G18 (K-I)
G19 (J-K)
Function and purpose
These commands are used to select the control plane and the plane on which the circular exists.
If the 3 basic axes and the parallel axes corresponding to these basic axes are entered as parameters, the
commands can select the plane composed of any 2 axes which are not parallel axes. If a rotation axis is
entered as a parallel axis, the commands can select the plane containing the rotation axis.
These commands are used to select:
- The plane for circular interpolation
- The plane for nose R compensation
Command format
G17; ... I-J plane selection
G18 ; ... K-I plane selection
G19; ... J-K plane selection
Detailed description
I, J and K indicate each basic axis or parallel axis.
When the power is turned ON or when the system is reset, the plane set by the parameters "#1025 I_plane" is
selected.
54
Page 71
M700V/M70V Series Programming Manual (Lathe System)
6.5 Plane Selection ; G17,G18,G19
Parameter entry
G17XY;
Y
X
G02
G03
G18XZ;
X
Z
G02
G03
G19YZ;
Z
Y
G02
G03
#1026 to 1028
base_I,J,K
IX Y
JY
KZ
#1029 to 1031
aux_I,J,K
Basic axes and parallel axes can be entered in the parameters. The
same axis name can be entered in duplication, but when it is assigned in duplication, the plane is determined by plane selection system (4).
The axis which is not registered as the control axis cannot be set.
Table 1 Examples of plane selection parameter entry
Plane selection system
This section describes the plane selection shown in the "Table 1 Examples of plane selection parameter
entry".
(1) Axis addresses assigned in the same block as the plane selection (G17, G18, G19) command determine
which of the basic axes or parallel axes are to be in the actual plane selected.
(Example)
(2) Plane selection is not performed with blocks in which the plane selection G code (G17, G18, G19) is not
assigned.
G18 X_ Z_ ; Z-X plane
Y_ Z_ ; Z-X plane (no plane change)
(3) When the axis addresses are omitted in the block containing the plane selection G codes (G17, G18,
G19), it is assumed that the axis addresses of the 3 basic axes have been assigned.
G18 ; (Z-X plane = G18 XZ ;)
(4) When the basic axes or their parallel axes are duplicated and assigned in the same block as the plane
selection G code (G17, G18, G19), the plane is determined in the order of basic axes, and then parallel
axes.
G18 XYZ ; The Z-X plane is selected. Therefore, the Y movement is unrelated to the selected plane.
(Note 1) When the "2" in the parameter "#1025 I_plane" is kept ON, the G18 plane is selected when the
power is turned ON or when the system is reset.
55
Page 72
6 Interpolation Functions
MITSUBISHI CNC
6.6 Thread Cutting
F/E
F/E
F/E
F/E
z
u/2
x
Q
w
2 1
(S)
(E)
(a)
(b)
X
Z
6.6.1 Constant Lead Thread Cutting ; G33
Function and purpose
The G33 command exercises feed control over the tool which is synchronized with the spindle rotation and so
this makes it possible to conduct constant-lead straight thread-cutting, tapered thread-cutting, and continuous
thread-cutting.
Straight thread Scrolled thread Continuous thread
Command format
G33 Z/W__ X/U__ F__ Q__ ; ... Normal lead thread cutting
Z,W,X,U Thread end point
F Lead of long axis (axis which moves most) direction
Q Thread cutting start shift angle, 0.001 to 360.000°
G33 Z/W__ X/U__ E__ Q__ ; ... Precision lead thread cutting
Z,W,X,U Thread end point
E Lead of long axis (axis which moves most) direction
Q Thread cutting start shift angle, 0.001 to 360.000°
δ1 > Illegal lead at start of thread cutting
δ2 > Illegal lead at end of thread cutting
(S) Start point (E) End point
(a) One-rotation synchronization signal
(b) Thread cutting start position
56
Page 73
M700V/M70V Series Programming Manual (Lathe System)
6.6 Thread Cutting
Detailed description
(1) The E command is also used for the number of ridges in inch thread cutting, and whether the number of
ridges or precision lead is to be designated can be selected by parameter setting.(Parameter "#1229 set
01/bit" is set to "1" for precision lead designation.)
(2) The lead in the long axis direction is commanded for the taper thread lead.
X
(E)
u/2
Thread cutting metric input
Input set-
ting unit
Command
address
Least
Command
Increments
Command
range
Input set-
ting unit
Command
address
Least
Command
Increments
Command
range
F (mm/rev) E (mm/rev) E (ridges/inch) F (mm/rev) E (mm/rev) E (ridges/inch)
1(=1.0000)
(1.=1.0000)
0.0001 -
999.9999
F (mm/rev) E (mm/rev) E (ridges/inch) F (mm/rev) E (mm/rev) E (ridges/inch)
1(=1.000000)
(1.=1.000000)
0.000001 -
999.999999
w
a°
(t)
(S)
(t) Tapered thread section (E) End point (S) Start point
When a < 45°, Lead is in Z-axis direction.
When a < 45°, Lead is in X-axis direction.
When a = 45°, Lead can be in either Z or X-axis direction.
Z
B (0.000mm) C (0.0001mm)
1(=1.00000)
(1.=1.00000)
0.00001 -
999.99999
D (0.00001mm) E (0.000001mm)
1(=1.0000000)
(1.=1.0000000)
0.0000001 -
999.9999999
1(=1.00)
(1.=1.00)
0.03 -
999.99
1(=1.0000)
(1.=1.0000)
0.0255 -
224580.0000
1(=1.00000)
(1.=1.00000)
0.00001 -
999.99999
1(=1.0000000)
(1.=1.0000000)
0.0000001 -
999.9999999
1(=1.000000)
(1.=1.000000)
0.000001 -
999.999999
1(=1.00000000)
(1.=1.00000000)
0.00000001 -
999.99999999
1(=1.000)
(1.=1.000)
0.026 -
222807.017
1(=1.00000)
(1.=1.00000)
0.02540 -
224719.00000
Thread cutting inch input
Input set-
ting unit
Command
address
Least
Command
Increments
Command
range
Input set-
ting unit
Command
address
Least
Command
Increments
Command
range
F (inch/rev) E (inch/rev) E (ridges/inch) F (inch/rev) E (inch/rev) E (ridges/inch)
1(=1.00000)
(1.=1.00000)
0.00001 -
39.37007
F (inch/rev) E (inch/rev) E (ridges/inch) F (inch/rev) E (inch/rev) E (ridges/inch)
1(=1.0000000)
(1.=1.0000000)
0.0000001 -
39.3700787
B (0.0001inch) C (0.00001inch)
1(=1.000000)
(1.=1.000000)
0.000001 -
39.370078
D (0.000001inch) E (0.0000001inch)
1(=1.00000000)
(1.=1.00000000)
0.00000001 -
39.37007873
1(=1.000)
(1.=1.000)
-
0.025
9999.999
1(=1.00000)
(1.=1.00000)
0.02540 -
9999.99999
1(=1.000000)
(1.=1.000000)
0.000001 -
39.370078
1(=1.00000000)
(1.=1.00000000)
0.00000001 -
39.37007873
1(=1.0000000)
(1.=1.0000000)
0.0000001 -
39.3700787
1(=1.000000000)
(1.=1.000000000)
0.000000001 -
39.370078736
1(=1.0000)
(1.=1.0000)
0.0254 -
9999.9999
1(=1.000000)
(1.=1.000000)
0.025400 -
9999.999999
(Note 1) It is not possible to assign a lead where the feedrate as converted into feed per minute exceeds the
maximum cutting feedrate.
57
Page 74
6 Interpolation Functions
MITSUBISHI CNC
(3) The constant surface speed control function should not be used for taper thread cutting commands or
scrolled thread cutting commands.
(4) The spindle rotation speed should be kept constant throughout from the rough cutting until the finishing.
(5) If the feed hold function is employed during thread cutting to stop the feed, th e thread ridges will lose
their shape. For this reason, feed hold does not function during thread cutting. Note that this is valid from
the time the thread cutting command is executed to the time the axis moves.
If the feed hold switch is pressed during thread cutting, block stop will occur at the end point of the block
following the block in which thread cutting is completed (no longer G33 mode).
(6) The converted cutting feedrate is compared with the cutting feed clamp rate when thread cutting starts,
and if it is found to exceed the clamp rate, an operation error will occur.
(7) In order to protect the lead during thread cutting, a cutting feedrate which has been converted may
sometimes exceed the cutting feed clamp rate.
(8) An illegal lead is normally produced at the start of the thread and at the end of the cutting because of
servo system delay and other such factors.
Therefore, it is necessary to command a thread length which is determined by adding the illegal lead
lengths δ1 and δ2 to the required thread length.
(9) The spindle rotation speed is subject to the following restriction :
1 <= R <= Maximum feed rate/Thread lead
Where R <= Tolerable speed of encoder (r/min)
R: Spindle rotation speed (r/min)
Thread lead = mm or inches
Maximum feedrate= mm/min or inch/mm (this is subject to the restrictions imposed by the machine
specifications.)
(10) A program error (P97) may occur when the result of the expression (9) is R<1 because the thread lead is
very large to the highest cutting feedrate.
(11) Dry run is valid for thread cutting but the feedrate based on dry run is not synchronized with the spindle
rotation.
The dry run signal is checked at the start of thread cutting and any switching during thread cutting is
ignored.
(12) Synchronous feed applies for the thread cutting commands even with an asynchronous feed command
(G94).
(13) Spindle override and cutting feed override are invalid and the speeds are fixed to 100% during thread
cutting.
(14) When a thread cutting command is programmed during nose R compensation, the compensation is
temporarily canceled and the thread cutting is executed.
(15) When the mode is switched to another automatic mode while G33 is executed, the following block which
does not contain a thread cutting command is first executed and then the automatic operation stops.
(16) When the mode is switched to the manual mode while G33 is executed, the following block which does
not contain a thread cutting command is first executed and then the automatic operation stops. In the
case of a single block, the following block which does not contain a thread cutting command (G33 mode
is cancelled) is first executed and then the automatic operation stops. Note that automatic operation is
stopped until the G33 command axis starts moving.
(17) The thread cutting command waits for the single rotation synchronization signal of the rotary encoder
and starts movement.
Note that carry out waiting-and-simultaneous operation between part systems before issuing a thread
cutting command with multiple part systems. For example, when using the 1-spindle specifications with
multi-part systems, if one part system issues a thread cutting command during ongoing thread cutting by
another part system, the movement will start without waiting for the rotary encoder single rotation
synchronization signal.
(18) The thread cutting start shift angle is not modal. If there is no Q command with G33, this will be handled
as "Q0".
(19) The automatic handle interrupt/interruption is valid during thread cutting.
(20) If a value exceeding 360.000 is command in G33 Q, a program error (P35) will occur.
(21) G33 cuts one row with one cycle. To cut two rows, change the Q value, and issue the same command.
58
Page 75
M700V/M70V Series Programming Manual (Lathe System)
6.6 Thread Cutting
Program example
40.0 50.0
90.0
20.0
Z
X
(mm)
G33 X90.0 Z40.0 E12.34567 ; Absolute value command
G33 U70.0 W-50.0 E12.34567 ; Incremental value command
59
Page 76
6 Interpolation Functions
MITSUBISHI CNC
6.6.2 Inch Thread Cutting ; G33
F/EZ
z
u/2
x
Q
w
2 1
X
Z
(S)
(E)
(a)
(b)
Function and purpose
If the number of ridges per inch in the long axis direction is assigned in the G33 command, the feed of the tool
synchronized with the spindle rotation will be controlled, which means that constant-lead straight threadcutting and tapered thread-cutting can be performed.
Command format
G33 Z/W__ X/U__ E__ Q__ ; ... Inch thread cutting
Z,W,X,U Thread end point
E
Q Thread cutting start shift angle, 0.001 to 360.000°
Number of ridges per inch in the long axis direction (axis which moves the most) (decimal point
command can also be assigned)
δ1 > Illegal lead at start of thread cutting
δ2 > Illegal lead at end of thread cutting
(S) Start point (E) End point
(a) One-rotation synchroniza-
tion signal
Detailed description
(1) The number of ridges in the long axis direction is assigned as the number of ridges per inch.
(2) The E code is also used to assign the precision lead length, and whether the number of ridges or
precision lead length is to be designated can be selected by parameter setting. (The number of ridges is
designated by setting the parameter "#1229 set01/bit1" to "0".) )
(3) The E command value should be set within the lead value range when converted to lead.
(4) See Section "Constant lead thread cutting" for other details.
60
(b) Thread cutting start position
Page 77
M700V/M70V Series Programming Manual (Lathe System)
6.6 Thread Cutting
Program example
40.0 50.0
90.0
20.0
Z
X
(mm)
G33 X90.0 Z40.0 E12.0 ; Absolute value command
G33 U70.0 W-50.0 E12.0 ; Incremental value command
61
Page 78
6 Interpolation Functions
MITSUBISHI CNC
6.6.3 Continuous Thread Cutting ; G33
G33
G33
G33
Function and purpose
Continuous thread cutting is possible by assigning thread cutting commands continuously.
In this way, it is possible to cut special threads whose lead or shape changes.
Command format
G33 Zz1/Ww1 Xx1/Uu1 Ff1/Ee1 Qq1 ; ... Co ntinuous thread cutting
Zzn,Wwn,Xxn,Uun Thread end point
Ffn/Een Lead of long axis (axis which moves most) direction
Qqn Thread cutting start shift angle, 0.001 to 360.000°
Detailed description
(1) The first thread cutting block in the continuous thread cutting command waits for the spindle's single
rotation synchronization signal before starting thread cutting. From the second and following blocks,
movement starts without waiting for the spindle's single rotation synchronization command.
Thus, the thread cutting start shift angle (Q) can be commanded only in the first block.
(2) G33 command can be omitted from the second and following blocks.
(3) When commanding continuous thread cutting, command the thread cutting commands in successive
blocks. If a command other than thread cutting is issued, continuous thread cutting will not take place.
Note that if a command that does not involve axis movement (G4 dwell command, MST command, etc.)
is commanded between the thread cutting command blocks, whether to wait for the spindle's single
rotation synchronization signal after the 2nd block can be selected with the parameters.
# No. Item Details
Set the continuous thread cutting Z phase wait operation.
0: If there is no movement command (MST command, etc.) between the thread
1270 ext06/bit6
cutting blocks, the 2nd block thread cutting waits for the spindle's single rotation
synchronization signal before starting movement.
1: Even if there is no movement command (MST command, etc.) between the
thread cutting blocks, the 2nd block thread cutting starts movement without
waiting for the spindle's single rotation synchronization signal.
Setting
range
0 / 1
(4) See "Constant lead thread cutting" for other details.
62
Page 79
M700V/M70V Series Programming Manual (Lathe System)
6.6 Thread Cutting
6.6.4 Variable Lead Thread Cutting ; G34
Function and purpose
Variable lead thread cutting is enabled by a command specifying a lead increment or decrement amount per
turn of the screw.
Command format
G34 X/U__ Z/W__ F/E__ K__ ; ... Variable lead thread cutting
X/U Z/W Thread end point
F/E Standard screw lead
K Lead increment or decrement amount per turn of the screw
(a)
F+3.5K F+2.5K F+1.5K F+0.5K
F+4K F+3K F+2K F+K F
(a) Non-lead axis (b) Lead axis (F) Lead speed
(b)
63
Page 80
6 Interpolation Functions
MITSUBISHI CNC
Detailed description
㧔F2+2KZ㧕
LL=
NP= (-F + LL) / K
(1) The command range is as shown below.
Thread cutting metric input
Input set-
ting unit
Command
address
Least
Command
Increments
Command
range
Input set-
ting unit
Command
address
Least
Command
Increments
Command
range
F (mm/rev) E (mm/rev) F (mm/rev) E (mm/rev)
1(=1.0000)
(1.=1.0000)
0.0001 -
999.9999
F (mm/rev) E (mm/rev) F (mm/rev) E (mm/rev)
1(=1.000000)
(1.=1.000000)
0.000001 -
999.999999
Thread cutting inch input
Input set-
ting unit
Command
address
Least
Command
Increments
Command
range
F (inch/rev) E (inch/rev) F (inch/rev) E (inch/rev)
1(=1.00000)
(1.=1.00000)
0.00001 -
39.37007
B (0.001mm) C (0.0001mm)
1(=1.00000)
(1.=1.00000)
0.00001 -
999.99999
D (0.00001mm) E (0.000001mm) B/C/D/E
1(=1.0000000)
(1.=1.0000000)
0.0000001 -
999.9999999
B (0.0001inch) C (0.00001inch)
1(=1.000000)
(1.=1.000000)
0.000001 -
39.370078
1(=1.00000)
(1.=1.00000)
0.00001 -
999.99999
1(=1.0000000)
(1.=1.0000000)
0.0000001 -
999.9999999
1(=1.000000)
(1.=1.000000)
0.000001 -
39.370078
1(=1.000000)
(1.=1.000000)
0.000001 -
999.999999
1(=1.00000000)
(1.=1.00000000)
0.00000001 -
999.99999999
1(=1.0000000)
(1.=1.0000000)
0.0000001 -
39.3700787
K(n*mm/rev)
n:Number of pitches
Same as F or E
(signed)
64
Input set-
ting unit
Command
address
Least
Command
Increments
Command
range
(1.=1.0000000)
D (0.000001inch) E (0.0000001inch) B/C/D/E
F (inch/rev) E (inch/rev) F (inch/rev) E (inch/rev)
1(=1.0000000)
0.0000001 -
39.3700787
(2) A positive value of K indicates incremental pitches.
Movement amount of one block (n pitches) = (F + K) + (F + 2K) + (F + 3K) + ・ ・ + (F + nK)
(3) A negative value of K indicates decremental pitches.
Movement amount of one block (n pitches) = (F - K) + (F - 2K) + (F - 3K) + ・ ・ + (F - nK)
(4) A program error will occur if the thread lead is not set correctly.
Error No. Details Remedy
Illegal pitch value
(1) An invalid value is specified for F/E or K in a
P 93
thread cutting command.
(2) The last lead goes outside of the F/E command range.
(5) The other details are the same as G33.
Refer to "Constant lead thread cutting ; G33".
1(=1.00000000)
(1.=1.00000000)
0.00000001 -
39.37007873
1(=1.0000
(1.=1.00000000)
0.00000001 -
39.37007873
0000)
1(=1.000000000)
(1.=1.000000000)
0.000000001 -
39.370078736
The last lead goes outside of the F/E command range.
LL : Last lead
NP : Number of pitches
K(n*inch/rev)
n:Number of pitches
Same as F or E
(signed)
Page 81
M700V/M70V Series Programming Manual (Lathe System)
6.6 Thread Cutting
6.6.5 Circular Thread Cutting ; G35,G36
zw
u/2
x
R
I
K
Z
X
(E)
(S)
(CP)
Function and purpose
Circular thread cutting making the longitudinal direction the lead is possible.
Command format
G35 X/U__ Z/W__ I__ K__ (R__) F/E__ Q__ ; ... Circular thread cutting Clockwise (CW)
G36 X/U__ Z/W__ I__ K__ (R__) F/E__ Q__ ; ... Circular thread cutting Counterclockwise (CCW)
X/U
Z/W
I X axis circular center (incremental value of circular center looking from start point)
K Z axis circular center (incremental value of circular center looking from start point)
R Circular radius
F/E
Q Thread cutting start shift angle, 0 to 360.000°
X axis circular end point coordinate (X is the absolute value of axis workpiece coordinate system, U is the incremental value from current position)
Z axis circular end point coordinate (Z is the absolute value of workpiece coordinate system,
W is the incremental value from current position)
Longitudinal (axis with largest movement amount) direction lead
(F.. normal lead thread cutting/E .. precision lead thread, inch thread)
(S) Start point
(E) End point
(CP) Center
(a) Circular thread
F/E
(a)
65
Page 82
6 Interpolation Functions
MITSUBISHI CNC
Detailed description
R
(a)
(E)
(CP) (b)
(S)
(c)
ZZ
X
X
(S) (E)
(S) (E)
(a) (b)
(CP) (CP)
(1) A program error (P33) will occur if the start point and end point match or if the arc center angle is more
than 180°.
(2) The following will occur if the start point radius and end point radius do not match.
- A program error (P70) will occur if the error ΔR is more than parameter "#1084 RadErr" (arc error).
- Interpolation will start from the arc center where the start point radius and end point radius match if the
error ΔR is less than parameter "#1084 RadErr".
(a) End point radius (b) Start point radius (c) Obtained center
(S) Start point (E) End point (CP) Center
(3) A program error (P33) will occur if the R_ sign is negative.
(4) A program error (P33) will occur if there is no I_K_ command and R_ command.
(5) The R_ command will have the priority if the I_K_ command and R_ command are issued in the same
block.
(6) If the arc center is (0,0), the arc command can be issued for two successive quadrants. A program error
(P33) will occur if an arc with more than three quadrants is issued.
[When Z axis is long axis]
(a) 1st and 4th quadrant (b) 2nd and 3rd quadrant
(S) Start point (E) End point (CP) Center
66
Page 83
M700V/M70V Series Programming Manual (Lathe System)
6.6 Thread Cutting
(7) When the movement amount is equal, the horizontal direction in the selected plane will be the long axis.
Plane selection
G17 (XY plane) I axis
G18 (ZX plane) K axis
G19 (YZ plane) J axis
Long axis when movement amount is
equal
(8) G36 is used for the two functions, automatic tool length measurement and circular thread cutting (CCW).
Which function to be applied depends on the setting of the parameter "#1238 set10/bit0" (circular thread
cutting).
When "#1238 set10/bit0" is set to "0"
G code Function
G35 Circular thread cutting clockwise (CW)
G36 Automatic tool length measurement X
When "#1238 set10/bit0" is set to "1"
G code Function
G35 Circular thread cutting clockwise (CW)
G36 Circular thread cutting counterclockwise (CCW)
G37 Automatic tool length measurement Z
G37.1 Automatic tool length measurement X
G37.2 Automatic tool length measurement Z
(9) If the lead axis and non-lead axis cutting feedrate is faster than the clamp speed when thread cutting is
started, the "M01 operation error 107" will occur, and thread cutti ng will not start.
(10) During thread cutting, the cutting feed rate may exceed th e clamp speed to guarantee the lead. In this
case, the error "M01 operation error 107" will appear, but thread cutting will continue. However, if the
"cutting feedrate > clamp speed" is established during circular thread cutting commanded in the second
or following block of continuous thread cutting, automatic operation will be stopped just before the
circular thread cutting command in the 2nd block, and the error "M01 operation error 107" will appear.
(11) Continuous thread cutting is possible by assigning thread cutting commands continuously. In this way, it
is possible to cut special threads whose lead or shape changes midway.
The continuous thread cutting command can be issued in the order of arc -> arc, arc -> constant lead,
and constant lead -> arc.
(12) An illegal lead is normally produced at the start of the thread and at the end of the cutting because of
servo system delay.
Thus, command the length of the required thread length and also the illegal thread length of the start and
end of the thread cutting.
As another method, command the required thread length as a circular thread (G35/G36), and then
command the illegal lead length before and after that command (start and end of thread cutting) as a
constant lead thread (G33). (Continuous thread cutting in order of constant lead -> arc -> constant lead.)
67
Page 84
6 Interpolation Functions
MITSUBISHI CNC
Relation with other functions
(1) A program error (P113) will occur if the G35/G36 command is issued to an axis not within the plane.
(2) The thread cutting speed is not synchronized with the spindle rotation when dry run is valid. (The thread
pitch is not guaranteed.)
(3) If the dry run switch is turned ON during thread cutting, the dry run signal will be ignored.
(4) If the feed hold switch is pressed during thread cutting, block stop will occur at the end point of the block
following the block in which thread cutting is completed (when the thread cutting mode is terminated).
(5) Circular thread cutting will function normally even during mirror image.
(6) A program error (P201) will occur if the G35/G36 circular thread cutting command is issued in the finish
shape program of the compound type fixed cycle for turning machining.
(7) A program error (P385) will occur if thread cutting corner rounding or corner chamfering is commanded
during circular thread cutting or the next block.
(8) Geometric and circular thread cutting cannot be commanded simultaneously. If commanded
simultaneously, a program error (P395 or P70) will occur.
(9) If thread cutting is commanded during nose R compensation, nose R compensation will be temporarily
canceled, and thread cutting will be executed.
(10) Do not issue the circular thread cutting command during constant surface speed control. The thread will
not be cut correctly because the spindle rotation speed will change during thread cutting.
Precautions
(1) Spindle override does not function during thread cutting.
(2) A program error (P39) will occur if G35/G36 is commanded when the additional specifications are not
provided.
68
Page 85
M700V/M70V Series Programming Manual (Lathe System)
6.7 Helical Interpolation ; G17,G18,G19 and G02,G03
6.7 Helical Interpolation ; G17,G18,G19 and G02,G03
Function and purpose
This function is for circularly interpolating 2 axes on the selected plane and simultaneously interpolating the
other axis linearly in synchronization with the circular motion.
When this interpolation is performe d wi th 3 orthogonal axes, the tool will travel helically.
Z
Y
(a)
(E)
(E)
j
i
(S)
(b)
X
(a) Program command path (b) XY plane projection path in command program
(d) XY plane path (projection path) (S) Start point (E) End point
Y
(d)
Command format
G17/G18/G19 G02/G03 X/U__ Y/V__ Z/W__ I__ J__ F__ (R__ F__); ... Helical interpolation
G17/G18/G19 Arc plane (G17: X-Y plane, G18: Z-X plane, G19: Y-Z plane)
G02/G03 Arc rotation direction (G02: clockwise, G03: counterclockwise)
X/U, Y/V Arc end point coordinates
Z/W Linear axis end point coordinates
I, J Arc center coordinates
R Arc radius
F Feedrate
(Note 1) In this manual, the following setting descriptions are used: I axis: X, J axis: Y, K axis: Z
X
(S)
69
Page 86
6 Interpolation Functions
MITSUBISHI CNC
Detailed description
Y
Z
X
F'
F
Y
X
(S)
(E)
(S)
(E)
Speed designation during the helical interpolation
Normally, the helical interpolation speed is designated with the tangent speed F' including the 3rd axis
interpolation element as shown in the lower drawing of Fig. 1. However, when designating the arc plane
element speed, the tangent speed F on the arc plane is commanded as shown in the upper drawing of Fig. 1.
The NC automatically calculates the helical interpolation tangent speed F' so that the tangent speed on the
arc plane is F.
(S) Start point (E) End point
The arc plane element speed designation and normal speed designation can be selected with the parameter.
#1235 set07/bit0 Meaning
1 Arc plane element speed designation is selected.
0 Normal speed designation is selected.
70
Page 87
M700V/M70V Series Programming Manual (Lathe System)
6.7 Helical Interpolation ; G17,G18,G19 and G02,G03
Arc plane element speed designation selection
I-100
W
J100
If arc plane element speed designation is selected, the F command will be handled as modal data in the same
manner as the normal F command. This will also apply to the following G01, G02 and G03 commands.
For example, the program will be as follows.
G17 G91 G02 X10. Y10. Z-4. I10. F100 ;
G01 X20. ; Linear interpolation at F100
G02 X10. Y-10. Z4. J-10. ;
G01 Y-40. F120; Linear interpolation at F120
G02 X-10. Y-10. Z-4. I-10. ;
G01 X-20. ; Linear interpolation at F120
Helical interpolation at speed at which arc plane element is
F100
Helical interpolation at speed at which arc plane element is
F100
Helical interpolation at speed at which arc plane element is
F120
When the arc plane element speed designation is selected, only the helical interpolation speed command is
converted to the speed commanded with the arc plane element and operates. The other linear and arc
commands operate as normal speed commands.
(1) The actual feedrate display (Fc) indicates the tangent element of the helical interpolation.
(2) The modal value speed display (FA) indicates the command speed.
(3) The speed data acquired with API functions follows the Fc and FA display.
(4) This function is valid only when feed per minute (asynchronous feed: G94) is selected. If feed per
revolution (synchronous feed: G95) is selected, the arc plane element speed will not be designated.
(5) The helical interpolation option is required to use this function.
Program example
G17 G02 X100. Y100. Z100. I-100. J100. F120 ;
Z
(a)
Y
(E)
X
(S)
(S)
(E)
Y
(b)
X
(a) Program command path (b) XY plane projection path in command program
(S) Start point (E) End point
The left drawing shows the process as an exploded view, and the right drawing shows the arc plane from
directly above.
At the start of the block, the axis centers at the point -100mm in the X axis direction and 100mm in the Y axis
direction from the workpiece coordinates (start point), and starts cutting at the feedrate 120mm/min while
rotating.
71
Page 88
6 Interpolation Functions
MITSUBISHI CNC
Precautions and restrictions
(1) When executing helical interpolation, command another linear axis (several axis can be commanded)
that does not contain the circular interpolation command and arc axis.
(2) Up to the number of simultaneous contouring control axes can be commanded simultaneously.
(3) A command exceeding one rotation cannot be issued. (It is complied with the circular interpolation
command specifications.)
(4) Command the feedrate as the composite speed for each axis.
(5) With helical interpolation, the axis that configures the plane is the circular interpolation axis, and the other
axes are the linear interpolation axes.
(6) The movement of the linear interpolation axis is stopped and only the circular interpolation axis operates
during the corner chamfering or corner R commands.
(7) Refer to the circular interpolation (G02,G03) for other precautions.
72
Page 89
M700V/M70V Series Programming Manual (Lathe System)
6.8 Milling Interpolation ; G12.1
6.8 Milling Interpolation ; G12.1
C
Z
(Y)
X
Function and purpose
Milling interpolation is used to perform contouring control by converting commands programmed in an
orthogonal coordinate system into movements of a linear axis and rotation axis (workpiece rotation).
(Y) Hypothetical axis
G12.1 command starts a milling and G13.1 command cancels the milling to return to a normal turning.
Command format
G12.1 D__ E=__ ; ... Milling mode ON
D Selection of milling hypothetical axis name
E= Designation of milling interpolation rotation axis
G13.1; ... Milling mode OFF (Turning mode)
Address Meaning of address Command range (unit) Remarks
- If there is no D command, the milling hypothetical axis name will follow parameter (#1517
mill_C).
D
E=
Selection of milling hypothetical axis name
Milling Interpolation
Designation of rotation axis
0: Y axis
1: Rotation axis name
G12.1 command system
rotation axis command
address
- If only the D command is issued, it will be handled as D0.
- A program error (P35) will occur if a value other
than 0 or 1 is set to the numerical command following the D command.
- If there is no E command, the parameter (#1516
mill_ax) will be followed.
- A program error (P33) will occur if only an E
command is issued.
- A program error (P33) will occur if an axis address is not commanded after "E=".
- A program error (P300) will occur if an axis that
does not exist in the command system is designated as the rotation axis name.
- A program error (P32) will occur if a value is
commanded for the rotation axis name.
- To issue a program command after the "E= rotation axis name", delimit the "E= rotation axis
name" and the other command with a comma (,).
A program error (P33) will occur if there is no
comma.
73
Page 90
6 Interpolation Functions
MITSUBISHI CNC
The following G codes are used to select milling and to set the conditions.
G13.1 G12.1
G19 G16 G17 G19G18
G46 G41 G42/G40 G42 G40,, ,G41 /
Machining mode
(Turning mode) (Milling mode)
(Nose R compensation) (Tool compensation)
(X-Y plane) (Z-X plane) (Y-Z plane) (X-Y plane)Y-Z
cylindrical
plane
(Y-Z plane)
G code Function Remarks
G12.1
G13.1
G16
G17
G19
G41
G42
Milling mode ON
Milling mode OFF
Selection of Y-Z cylindrical
plane
Selection of X-Y plane
Selection of Y-Z plane
Tool radius compensation left
Tool radius compensation right
Default is G13.1
One of G17, G16, and G19 can be designated
as the default value (when G12.1 is issued) by
the parameter.
#8113 Milling initial G16
#8114 Milling initial G19
Default is G40 (radius compensation cancel).
G17
74
Page 91
M700V/M70V Series Programming Manual (Lathe System)
6.8 Milling Interpolation ; G12.1
6.8.1 Selecting Milling Mode
Detailed description
(1) The G12.1 and G13.1 commands are used to switch between the turning (G13.1) and milling (G12.1)
modes.
(2) These commands are modal and the initial mode effective at power ON is the turning mode.
(3) The following requirements must be satisfied before a G12.1 command is issued. Otherwise, a program
error (P485) will occur.
(a) Nose R compensation has been canceled.
(b) Constant surface speed control has been canceled.
(4) If one of the command axes in the milling mode has not completed reference position return, a program
error (P484) will occur.
(5) The G12.1 command automatically cancels an asynchronous mode F command. Therefore, specify an
F value in milling mode.
Precautions
(Note 1) If G12.1 is executed without movement command after nose R compensation is canceled by an
independent G40 command, nose R compensation is canceled in the G12.1 block.
(Note 2) If the milling interpolation command is issued during the mirror image, a program error (P486) will
occur.
(Note 3) When the G12.1 command is issued, the deceleration check is executed.
(Note 4) If a command other than a plane selection is issued in the same block as G12.1 command, a
program error (P33) will occur.
75
Page 92
6 Interpolation Functions
MITSUBISHI CNC
6.8.2 Milling Interpolation Control and Command Axes
Z
X
(Y)
Detailed description
(1) The two orthogonal linear axes (X and Z axis) and a rotation axis are used as control axes for milling
interpolation. The rotation axis is selected with the E command. The axis designated with the parameter
(#1516 mill_ax) will be selected if there is no E command.
(2) The command axes for milling interpolation are three orthogonal linear axes. The names of axes should
be X, Z, and a hypothetical axis.
A hypothetical axis is a virtual axis for interpolation command which intersects the X and Z axes at right
angles. The hypothetical axis name will be either of the control rotation axis names which are selected in
Y or (1) by a D command. The axis name designated with the parameter (#1517 mill_C) will be selected
if there is no D command.
(Y) Hypothetical axis
(3) Command axis X for milling is not just the interpolated one of control axis X. It is handled as X in the
milling coordinate system when a G12. 1 command is issued.
(4) Whether the position in the milling coordinate system is handled by a diameter command or radius
command is selected by the following parameter.
Parameter Details
#8111 Milling Radius
0 : Radius command for all axes
1 : Follows parameter (#1019 dia) for each axis
(Example 1)
When C axis is used for rotation axis, and "Y" for hypothetical axis name
X
(Y)
20
N3
10
010
(Program 1)
:
:
:
N1 G0 X40. ;
N2 G12.1 ;
(or G12.1 E=C, D0 ;)
N3 G1 X10. Y10. F10. ;
:
:
:
(Y) Hypothetical axis
76
(mm)
Page 93
M700V/M70V Series Programming Manual (Lathe System)
6.8 Milling Interpolation ; G12.1
N3 of program 1 is executed as follows:
X = Mill _ X
Mill _ X
(d)
(a)
X
10
10
(Y)
(b)
Mill _ X
X
(Y)
(Y)
Mill _ X
(c)
X
(mm)
(Y)
(Y) Hypothetical axis
Current values of (d)
X 28.284 (diameter value display)
C 45.000 (Except tool radius compensation amount)
(5) Milling interpolation is also available for a two-control-axis system consisting of one linear axis and one
rotation axis. The X axis must be used as the linear axis. The rotation and milling hypothetical axes are
selected as shown above. In milling mode, the G17 plane must be selected.
(6) The table below lists the incremental axis names of the hypothetical axis used in milling mode. These
axis commands are radius commands only.
Selected hypothetical axis Absolute axis name Incremental axis name
Y axis Y V
Rotation axis (C) #1013 axname set axis name (C) #1014 incax set axis name (H)
(The following description uses Y for the hypothetical axis name and C for the rotation axis name. )
77
Page 94
6 Interpolation Functions
MITSUBISHI CNC
6.8.3 Selecting a Plane during the Milling Mode ; G17,G19,G16
Function and purpose
A plane selection command decides the plane on which a tool moves by circular interpolation or tool radius
compensation in milling mode.
Command format
G17; ... X-Y plane
G19; ... Y-Z plane
G16 C; ... Y-Z cylindrical plane
C Cylinder radius value
Detailed description
These G commands for plane selection are modal. A plane is automatically selected according to parameters
each time the turning mode is switched to the milling mode by a G12.1 command.
Plane selection default value G17 G19 G16
#8113 Milling initial G16 0011
#8114 Milling initial G19 0101
When the milling mode is switched back to the turning mode by a G13.1 command, the plan e, that was
selected before the milling mode is entered, is restored.
78
Page 95
M700V/M70V Series Programming Manual (Lathe System)
6.8 Milling Interpolation ; G12.1
Planes to be selected
X
Z
Y
X
Y
Z
(C)
The three planes to be selected are explained below.
(1) G16 Y-Z cylindrical plane
G16 indicates the plane obtained by developing a cylinder with its bottom radius X. This is useful to
process the side face of a workpiece.
X
Z
Y
(2) G17 X-Y plane
G17 is an X-Y plane in an XYZ orthogonal coordinate system. This is useful to process the end face of a
workpiece.
(3) G19 Y-Z plane
G19 is a Y-Z plane in an XYZ orthogonal coordinate system.
(C) Center of workpiece
79
Page 96
6 Interpolation Functions
MITSUBISHI CNC
6.8.4 Setting Milling Coordinate System
Function and purpose
The coordinate system in a milling mode is set depending on a plane which is selected each time the turning
mode (G13.1) is switched to the milling mode by a G12.1 command.
Detailed description
G16 plane
(1) To select a G16 plane, specify the radius value of a cylinder by "G16 C__ ;". If no radiu s value is
specified, the current X axis value at the time of G16 command is used as the radius value to define a
cylinder. If no radius value can be defined, a program error (P485) will occur.
(2) As in normal turning mode, the X axis indicates the distance from the center line of the workpiece.
(3) G16 (Y-Z cylindrical plane) is actually the side of a cylinder.
(4) The X axis indicates the distance from the center line of the workpiece. The Y axis indica tes the
circumference with the radius value of the bottom of the cylinder which is defined by a G16 command.
(5) The zero point of the Y axis is the position where a G12.1 command is issued.
(Example)
::: :
::: :
G12.1 G16 C50. ; or G12.1; or G12.1 Ee,Dd or G12.1 Ee,Dd;
G16 C50. ; G16 C50. ; G16 C50. ;
::: :
::: :
Y
X
r
Z
80
Page 97
M700V/M70V Series Programming Manual (Lathe System)
6.8 Milling Interpolation ; G12.1
G17 and G19 planes
Z
X
Y
(1) For the X and Z axes, the current positions are set as radius value in the coordinate value.
(2) The Y axis is fixed as an axis which intersects the X and Z axes at right angles. Y=0 is set in a G12.1
command.
(Note 1) In the milling mode on the G17 plane, the X axis is operated in the area (positive or negative side)
that existed before issuing the G12.1 command. To control the X axis in the positive side in the
milling mode, move the X axis to the positive area (including 0) before issuing the G12.1 command.
To control the X axis in the negative side in the milling mode, move the X axis to the negative area
(not including 0) before issuing the G12.1 command.
81
Page 98
6 Interpolation Functions
MITSUBISHI CNC
6.8.5 Preparatory function
Detailed description
Valid G codes in milling mode
Classi-
fication
* G00 Positioning G65 Macro call
* G01 Linear interpolation G66 Macro modal call A
* G02 Circular interpolation (CW) G66.1 Macro modal call B
* G03 Circular interpolation (CWW) G67
○ G16
G code Function
G04 Dwell
G09 Exact stop check G80 Hole drilling cycle cancel
G13.1 Turning mode G84 Tap cycle (Z axis)
Plane selection Y-Z cylindrical
plane
G17 Plane selection X-Y G89 Boring cycle (X axis)
G19 Plane selection Y-Z G91 Incremental value command
G22 Barrier check ON G94 Asynchronous feed
G23 Barrier check OFF
Classi-
fication
G code Function
Macro modal call
Cancel
G83 Deep hole drilling cycle (Z axis)
G85 Boring cycle (Z axis)
G87 Deep hole drilling cycle (X axis)
G88 Tap cycle (X axis)
G90 Absolute value command
G98 Hole drilling cycle initial point return
G99 Hole drilling cycle R point return
G61 Exact stop mode
G40 Tool radius compensation cancel
G41 Tool radius compensation left G64 Cutting mode
G42 Tool radius compensation right
*: Milling interpolation command
○ : G code effective only in milling mode
(1) If an invalid G code is issued in milling mode, a program error (P481) will occur.
If the milling interpolation ON (G12.1) is issued in milling mode, a program error (P481) wil l occur.
(2) In milling mode, all movement commands are issued by the coordinate system which is already
determined by the selected machining plane. The rotation axis thus cannot be moved by a direct
command in milling mode. To perform milling to a workpiece at a specific position, therefore, positioning
must be done before a milling mode command.
(Example)
:
G0 X100. C180. ; =>Positioning before milling
G12.1 ; (or G12.1 E=C,D0 ;)
G0 X50. ;
:
(3) If an axis other than X, Z, and Y (rotation axis) is specified in milling mode, a program error (P481) will
occur.
82
Page 99
M700V/M70V Series Programming Manual (Lathe System)
6.8 Milling Interpolation ; G12.1
(4) In milling mode, the Y axis can be specified by only four G codes: G00, G01, G02, and G03. These are
(S)
Y
z
y
(E)
X
Z
z
y
(S)
(E)
called the milling interpolation commands.
(5) The G84, G88 synchronous tapping cycles cannot be used in the milling mode. The asynchronous
tapping can be used during the milling mode; however, the synchronous tapping command must not be
issued.
Positioning (G00)
If a G00 command is issued in milling mode, positioning is made to the specified point on the selected plane at
a rapid traverse rate.
G00 X/U__ Y/V__ Z/W__ ;
Linear interpolation (G01)
If a G01 command is issued in milling mode, linear interpolation is made to the specified point on the selected
plane at the speed specified by an F command modal speed.
(1) G16 mode (plane selection Y-Z cylindrical plane)
Program format
G01 Y/V__ Z/W__ X/U__ F__ ;
(S) Start point (E) End point
83
Page 100
6 Interpolation Functions
MITSUBISHI CNC
(2) G17 mode (plane selection X-Y)
Program format
G01 X/U__ Y/V__ Z/W__ F__ ;
X
(E)
Y
(S) Start point (E) End point
(3) G19 mode (plane selection Y-Z)
Program format
G01 Y/V__ Z/W__ X/U__ F__ ;
A
x
(S)
y
X
y
(S)
z
(E)
x
z
A
(E)
Z
Z
Y
(S) Start point (E) End point
(E)
84
Loading...