advertisement
▼
Scroll to page 2
of 534
Introduction This manual describes how to carry out MITSUBISHI CNC programming. Supported models are as follows: Supported models M800W series M800S series M80W series M80 series C80 series Abbreviations in this manual M800 series, M800, M8 M80 series, M80, M8 C80 This manual describes programming, therefore, read this manual thoroughly before using this NC system. To ensure safe use of this NC system, thoroughly study the "Precautions for Safety" on the following page before using this NC system. Be sure to always keep this manual on hand so that users can refer to it at any time. Details described in this manual The description concerning "Signals" in the main text refers to information transmission between a machine and PLC or between NC and PLC. The method for controlling the signals (ON/OFF) differs depending on the machine. Refer to the manual issued by the machine tool builder (MTB). Some parameters can be used by end-users and some parameters are set by the MTB according to the specifications. End-users may not be able to set or change some of the parameters described as "... can be set with the parameter #XXXX" in the main text. Confirm the specifications for your machine with the manual issued by the MTB. CAUTION For items described as "Restrictions" or "Usable State" in this manual, the instruction manual issued by the machine tool builder (MTB) 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 the applicable functions are included. Some of them, however, may not be available for your NC system. Refer to the specifications issued by the machine tool builder before use. Refer to the Instruction Manual issued by the MTB for details regarding each machine tool. Some screens and functions may differ depending on the NC system (or its version), and some functions may not be available. Please confirm the specifications before use. General precautions (1) Refer to the following documents for details handling MITSUBISHI CNC M800/M80 Series Instruction Manual ............... IB-1501274 MITSUBISHI CNC C80 Series Instruction Manual ......................... IB-1501453 (2) Refer to the following documents for details on programming MITSUBISHI CNC M800/M80/C80 Series Programming Manual Lathe System (1/2) ................................................................... Lathe System (2/2) ................................................................... Machining Center System (1/2) ................................................ Machining Center System (2/2) ................................................ IB-1501275 IB-1501276 IB-1501277 IB-1501278 Precautions for Safety 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 When the user may be subject to imminent fatalities or major injuries if handling is mistaken. WARNING When the user may be subject to fatalities or major injuries if handling is mistaken. CAUTION When the user may be subject to injuries or when physical damage may occur if handling is mistaken. 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. The following sings indicate prohibition and compulsory. This sign indicates prohibited behavior (must not do). For example, indicates "Keep fire away". This sign indicated a thing that is pompously (must do). For example, indicates "it must be grounded". The meaning of each pictorial sing is as follows. CAUTION CAUTION rotated object CAUTION HOT Danger Electric shock risk Danger explosive Prohibited Disassembly is prohibited KEEP FIRE AWAY General instruction Earth ground For Safe Use Mitsubishi CNC is designed and manufactured solely for applications to machine tools to be used for industrial purposes. Do not use this product in any applications other than those specified above, especially those which are substantially influential on the public interest or which are expected to have significant influence on human lives or properties. DANGER Not applicable in this manual. 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 unexpected 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 axis 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. CAUTION 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 the applicable functions are included. Some of them, however, may not be available for your NC system. Refer to the specifications issued by the machine tool builder before 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 run operation and single block operation to check the machining program, tool offset 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. 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 synchronized spindle rotation command OFF with one workpiece chucked by the reference spindle and synchronized spindle during the spindle synchronization. Failure to observe this may cause the synchronized 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" format, 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 builder. When programming the multi-part system, take special care to the movements of the programs for other part systems. 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 manufactured 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 separately 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! Trademarks MELDAS, MELSEC, EZSocket, EZMotion, iQ Platform, MELSEC iQ-R, MELSOFT, GOT, CC-Link, CC-Link/LT and CC-Link IE are either trademarks or registered trademarks of Mitsubishi Electric Corporation in Japan and/or other countries. Ethernet is a registered trademark of Xerox Corporation in the United States and/or other countries. Microsoft®, Windows®, SQL Server® and Access® are either trademarks or registered trademarks of Microsoft Corporation in the United States and/or other countries. SD logo and SDHC logo are either registered trademarks or trademarks of LLC. UNIX is a registered trademark of The Open Group in the United States and/or other countries. Intel® and Pentium® are either trademarks or registered trademarks of Intel Corporation in the United States and/or other countries. MODBUS® is either a trademark or a registered trademark of Schneider Electric USA, Inc. or the affiliated companies in Japan and/or other countries. EtherNet/IP is a trademark of Open DeviceNet Vendor Association,Inc. PROFIBUS-DP is a trademark of Profibus International. Oracle® is a registered trademark of Oracle Corporation, the subsidiaries, or the affiliated companies in the United States and /or other countries. Other company and product names that appear in this manual are trademarks or registered trademarks of the respective companies. 本製品の取扱いについて ( 日本語 /Japanese) 本製品は工業用 ( クラス A) 電磁環境適合機器です。販売者あるいは使用者はこの点に注意し、住商業環境以外で の使用をお願いいたします。 Handling of our product (English) This is a class A product. In a domestic environment this product may cause radio interference in which case the user may be required to take adequate measures. 본 제품의 취급에 대해서 ( 한국어 /Korean) 이 기기는 업무용 (A 급 ) 전자파적합기기로서 판매자 또는 사용자는 이 점을 주의하시기 바라며 가정외의 지역에 서 사용하는 것을 목적으로 합니다 . Contents Chapter 1 - 14 : Refer to Programming Manual (Machining Center System) (1/2) Chapter 15 and later : Refer to Programming Manual (Machining Center System) (2/2) 1 Control Axes................................................................................................................................................. 1 1.1 Coordinate Words and Control Axes ........................................................................................................................ 2 1.2 Coordinate Systems and Coordinate Zero Point Symbols ....................................................................................... 3 2 Minimum Command Unit............................................................................................................................. 5 2.1 Input Setting Unit ...................................................................................................................................................... 6 2.2 Input Command Increment Tenfold .......................................................................................................................... 7 2.3 Indexing Increment ................................................................................................................................................... 8 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 .................................................................................................................... 18 3.4 G Codes.................................................................................................................................................................. 20 3.4.1 Modal, Unmodal ............................................................................................................................................. 20 3.4.2 G Code Lists .................................................................................................................................................. 20 3.5 Precautions Before Starting Machining .................................................................................................................. 25 4 Pre-read Buffer ........................................................................................................................................... 27 4.1 Pre-read Buffer ....................................................................................................................................................... 28 5 Position Commands .................................................................................................................................. 29 5.1 Position Command Methods ; G90,G91 ................................................................................................................. 30 5.2 Inch/Metric Conversion ; G20,G21 ......................................................................................................................... 32 5.3 Decimal Point Input................................................................................................................................................. 34 6 Interpolation Functions ............................................................................................................................. 41 6.1 Positioning (Rapid Traverse) ; G00 ....................................................................................................................... 42 6.2 Linear Interpolation ; G01 ....................................................................................................................................... 45 6.3 Circular Interpolation ; G02,G03 ............................................................................................................................ 47 6.4 R Specification Circular Interpolation ; G02,G03 .................................................................................................... 53 6.5 Plane Selection ; G17,G18,G19 ............................................................................................................................. 56 6.6 Thread Cutting ........................................................................................................................................................ 58 6.6.1 Constant Lead Thread Cutting ; G33 ............................................................................................................. 58 6.6.2 Inch Thread Cutting ; G33............................................................................................................................. 62 6.7 Helical Interpolation ; G17,G18,G19 and G02,G03 ................................................................................................ 64 6.8 Unidirectional Positioning ....................................................................................................................................... 70 6.8.1 Unidirectional Positioning ; G60 ..................................................................................................................... 70 6.8.2 Axis-based Unidirectional Positioning ............................................................................................................ 72 6.9 Cylindrical Interpolation ; G07.1.............................................................................................................................. 73 6.10 Circular Cutting ; G12,G13 ................................................................................................................................... 80 6.11 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113................................................................................... 82 6.12 Exponential Interpolation ; G02.3,G03.3............................................................................................................... 89 6.13 Polar Coordinate Command ; G16 ....................................................................................................................... 96 6.14 Spiral/Conical Interpolation ; G02.1/G03.1(Type1), G02/G03(Type2) ................................................................ 103 6.15 3-dimensional Circular Interpolation ; G02.4,G03.4............................................................................................ 108 6.16 NURBS Interpolation ; G06.2.............................................................................................................................. 113 6.17 Hypothetical Axis Interpolation ; G07.................................................................................................................. 119 7 Feed Functions......................................................................................................................................... 121 7.1 Rapid Traverse Rate............................................................................................................................................. 122 7.1.1 Rapid Traverse Rate .................................................................................................................................... 122 7.1.2 G00 Feedrate Command (,F Command) ..................................................................................................... 123 7.2 Cutting Feed Rate................................................................................................................................................. 127 7.3 F1-digit Feed......................................................................................................................................................... 128 7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed) ; G94,G95 ............................. 130 7.5 Inverse Time Feed ; G93 ...................................................................................................................................... 133 7.6 Feedrate Designation and Effects on Control Axes.............................................................................................. 138 7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration........................................................................... 142 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration .......................................................... 147 7.9 Cutting Feed Constant Inclination Acceleration/Deceleration............................................................................... 155 7.10 Exact Stop Check ; G09 ..................................................................................................................................... 161 7.11 Exact Stop Check Mode ; G61 ........................................................................................................................... 165 7.12 Deceleration Check ............................................................................................................................................ 166 7.12.1 Deceleration Check.................................................................................................................................... 166 7.12.2 Deceleration Check when Movement in The Opposite Direction Is Reversed........................................... 174 7.13 Rapid Traverse Block Overlap; G0.5 P1............................................................................................................. 176 7.13.1 Rapid Traverse Block Overlap for G00; G0.5 ............................................................................................ 178 7.13.2 Rapid Traverse Block Overlap for G28 ...................................................................................................... 186 7.14 Automatic Corner Override ................................................................................................................................. 188 7.14.1 Automatic Corner Override ; G62............................................................................................................... 194 7.14.2 Inner Arc Override...................................................................................................................................... 195 7.15 Tapping Mode ; G63 ........................................................................................................................................... 196 7.16 Cutting Mode ; G64............................................................................................................................................ 197 8 Dwell.......................................................................................................................................................... 199 8.1 Dwell (Time Designation) ; G04............................................................................................................................ 200 9 Miscellaneous Functions ........................................................................................................................ 203 9.1 Miscellaneous Functions (M8-digits) .................................................................................................................... 204 9.2 Secondary Miscellaneous Functions (A8-digits, B8-digits or C8-digits) ............................................................... 206 9.3 Index Table Indexing ............................................................................................................................................ 207 10 Spindle Functions .................................................................................................................................. 213 10.1 Spindle Functions ............................................................................................................................................... 214 10.2 Constant Surface Speed Control ; G96,G97 ...................................................................................................... 215 10.3 Spindle Clamp Speed Setting ; G92 ................................................................................................................... 221 10.4 Spindle Position Control (Spindle/C Axis Control) .............................................................................................. 223 11 Tool Functions (T command)................................................................................................................ 231 11.1 Tool Functions (T8-digit BCD) ............................................................................................................................ 232 12 Tool Compensation Functions ............................................................................................................. 233 12.1 Tool Compensation............................................................................................................................................. 234 12.1.1 Tool Compensation .................................................................................................................................... 234 12.1.2 Number of Tool Offset Sets Allocation to Part Systems............................................................................. 238 12.2 Tool Length Compensation/Cancel ; G43,G44/G49 ........................................................................................... 240 12.3 Tool Radius Compensation ; G38,G39/G40/G41,G42 ....................................................................................... 245 12.3.1 Tool Radius Compensation Operation ....................................................................................................... 246 12.3.2 Other Commands and Operations during Tool Radius Compensation...................................................... 255 12.3.3 G41/G42 Commands and I, J, K Designation ............................................................................................ 265 12.3.4 Interrupts during Tool Radius Compensation............................................................................................. 271 12.3.5 General Precautions for Tool Radius Compensation................................................................................. 273 12.3.6 Changing of Compensation No. during Compensation Mode.................................................................... 274 12.3.7 Start of Tool Radius Compensation and Z Axis Cut in Operation .............................................................. 277 12.3.8 Interference Check..................................................................................................................................... 279 12.3.9 Diameter Designation of Compensation Amount ....................................................................................... 289 12.3.10 Workpiece Coordinate Changing during Radius Compensation.............................................................. 291 12.4 Tool Nose Radius Compensation (for Machining Center System) ..................................................................... 293 12.5 3-dimensional Tool Radius Compensation ; G40/G41,G42................................................................................ 296 12.6 Tool Position Offset ; G45 to G48....................................................................................................................... 308 13 Fixed Cycle ............................................................................................................................................. 317 13.1 Fixed Cycles ....................................................................................................................................................... 318 13.1.1 Drilling, Spot Drilling ; G81 ......................................................................................................................... 322 13.1.2 Drilling, Counter Boring ; G82 .................................................................................................................... 323 13.1.3 Deep Hole Drilling Cycle ; G83 .................................................................................................................. 324 13.1.3.1 Deep Hole Drilling Cycle ................................................................................................................... 324 13.1.3.2 Small Diameter Deep Hole Drilling Cycle .......................................................................................... 326 13.1.4 Tapping Cycle ; G84 .................................................................................................................................. 329 13.1.5 Boring ; G85 ............................................................................................................................................... 341 13.1.6 Boring ; G86 ............................................................................................................................................... 342 13.1.7 Back Boring ; G87 ...................................................................................................................................... 343 13.1.8 Boring ; G88 ............................................................................................................................................... 345 13.1.9 Boring ; G89 ............................................................................................................................................... 346 13.1.10 Stepping Cycle ; G73 ............................................................................................................................... 347 13.1.11 Reverse Tapping Cycle ; G74 .................................................................................................................. 349 13.1.12 Circular Cutting ; G75............................................................................................................................... 351 13.1.13 Fine Boring ; G76 ..................................................................................................................................... 353 13.1.14 Precautions for Using a Fixed Cycle ........................................................................................................ 355 13.1.15 Initial Point and R Point Level Return ; G98,G99..................................................................................... 357 13.1.16 Setting of Workpiece Coordinates in Fixed Cycle Mode .......................................................................... 358 13.1.17 Drilling Cycle High-Speed Retract............................................................................................................ 359 13.1.18 Acceleration/Deceleration Mode Change in Hole Drilling Cycle .............................................................. 363 13.2 Special Fixed Cycle ............................................................................................................................................ 365 13.2.1 Bolt Hole Cycle ; G34................................................................................................................................. 366 13.2.2 Line at Angle ; G35 .................................................................................................................................... 367 13.2.3 Arc ; G36 .................................................................................................................................................... 368 13.2.4 Grid ; G37.1................................................................................................................................................ 369 14 Macro Functions .................................................................................................................................... 371 14.1 Subprogram Control; M98, M99, M198 .............................................................................................................. 372 14.1.1 Subprogram Call ; M98,M99 ..................................................................................................................... 372 14.1.2 Subprogram Call ; M198 ........................................................................................................................... 378 14.1.3 Figure Rotation ; M98 I_J_K_ .................................................................................................................... 379 14.2 Variable Commands ........................................................................................................................................... 382 14.3 User Macro ......................................................................................................................................................... 387 14.4 Macro Call Instructions ....................................................................................................................................... 388 14.4.1 Simple Macro Calls ; G65 ......................................................................................................................... 388 14.4.2 Modal Call A (Movement Command Call) ; G66 ....................................................................................... 392 14.4.3 Modal Call B (for Each Block) ; G66.1 ...................................................................................................... 394 14.4.4 G Code Macro Call..................................................................................................................................... 396 14.4.5 Miscellaneous Command Macro Call (for M, S, T, B Code Macro Call) .................................................... 397 14.4.6 Detailed Description for Macro Call Instruction .......................................................................................... 399 14.4.7 ASCII Code Macro ..................................................................................................................................... 401 14.5 Variables Used in User Macros .......................................................................................................................... 405 14.5.1 Common Variables..................................................................................................................................... 407 14.5.2 Local Variables (#1 to #33) ........................................................................................................................ 408 14.5.3 System Variables ....................................................................................................................................... 411 14.6 User Macro Commands ...................................................................................................................................... 412 14.6.1 Operation Commands ................................................................................................................................ 412 14.6.2 Control Commands .................................................................................................................................... 416 14.6.3 External Output Commands ; POPEN, PCLOS, DPRNT.......................................................................... 419 14.6.4 Precautions ................................................................................................................................................ 423 14.6.5 Actual Examples of Using User Macros..................................................................................................... 425 14.7 Macro Interruption; M96, M97............................................................................................................................. 429 15 Program Support Functions ................................................................................................................. 439 15.1 Corner Chamfering I /Corner Rounding I............................................................................................................ 440 15.1.1 Corner Chamfering I ; G01 X_ Y_ ,C ......................................................................................................... 440 15.1.2 Corner Rounding I ; G01 X_ Y_ ,R_........................................................................................................... 442 15.1.3 Corner Chamfering Expansion/Corner Rounding Expansion..................................................................... 444 15.1.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding ..................................................... 446 15.2 Corner Chamfering II /Corner Rounding II .......................................................................................................... 447 15.2.1 Corner Chamfering II ; G01/G02/G03 X_ Y_ ,C_....................................................................................... 447 15.2.2 Corner Rounding II ; G01/G02/G03 X_ Y_ ,R_ .......................................................................................... 449 15.2.3 Corner Chamfering Expansion/Corner Rounding Expansion..................................................................... 450 15.2.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding ..................................................... 450 15.3 Linear Angle Command ; G01 X_/Y_ A_/,A_...................................................................................................... 451 15.4 Geometric ; G01 A_ ............................................................................................................................................ 452 15.5 Geometric IB....................................................................................................................................................... 454 15.5.1 Geometric IB (Automatic Calculation of Two-arc Contact) ; G02/G03 P_Q_ /R_ ..................................... 455 15.5.2 Geometric IB (Automatic Calculation of Linear - Arc Intersection) ; G01 A_ , G02/G03 P_Q_H_ ............. 457 15.5.3 Geometric IB (Automatic Calculation of Linear - Arc Intersection) ; G01 A_ , G02/G03 R_H_................. 460 15.6 G Command Mirror Image ; G50.1,G51.1 .......................................................................................................... 462 15.7 Normal Line Control ; G40.1/G41.1/G42.1 (G150/G151/G152).......................................................................... 466 15.8 Manual Arbitrary Reverse Run Prohibition ; G127.............................................................................................. 486 15.9 Data Input by Program........................................................................................................................................ 492 15.9.1 Parameter Input by Program ; G10 L70/L100, G11 ................................................................................... 492 15.9.2 Compensation Data Input by Program ; G10 L2/L10/L11/L12/L13/L20, G11 ............................................ 495 15.9.3 Compensation Data Input by Program (Turning Tool) ; G10 L12/L13, G11............................................... 501 15.9.4 Tool Shape Input by Program ; G10 L100, G11......................................................................................... 503 15.9.5 R-Navi Data Input by Program ; G10 L110, G11, G68.2, G69................................................................... 506 15.10 Tool Life Management II ; G10 L3, G11 .......................................................................................................... 510 15.10.1 Allocation of The Number of Tool Life Management Sets to Part Systems ............................................. 510 15.11 Inputting The Tool Life Management Data ; G10,G11...................................................................................... 512 15.11.1 Inputting The Tool Life Management Data by G10 L3 Command ; G10 L3,G11 ..................................... 512 15.11.2 Inputting The Tool Life Management Data by G10 L30 Command ; G10 L30,G11 ................................. 515 15.11.3 Precautions for Inputting The Tool Life Management Data...................................................................... 518 15.11.4 Allocation of The Number of Tool Life Management Sets to Part Systems ............................................. 519 16 Multi-part System Control ..................................................................................................................... 521 16.1 Timing Synchronization Operation...................................................................................................................... 522 16.1.1 Timing Synchronization Operation (! code) !n (!m ...) L ............................................................................. 522 16.1.2 Timing Synchronization Operation with Start Point Designated (Type 1) ; G115 ...................................... 525 16.1.3 Timing Synchronization Operation with Start Point Designated (Type 2) ; G116 ...................................... 528 16.1.4 Timing Synchronization Operation Function Using M codes ; M*** ........................................................... 531 16.1.5 Time Synchronization When Timing Synchronization Ignore Is Set .......................................................... 535 16.2 Mixed Control...................................................................................................................................................... 538 16.2.1 Arbitrary Axis Exchange ; G140, G141, G142 ........................................................................................... 538 16.3 Sub Part System Control .................................................................................................................................... 541 16.3.1 Sub Part System Control I ; G122............................................................................................................. 541 17 High-speed High-accuracy Control ...................................................................................................... 557 17.1 High-speed Machining Mode .............................................................................................................................. 558 17.1.1 High-speed Machining Mode I, II ; G05 P1, G05 P2 .................................................................................. 558 17.2 High-accuracy Control ........................................................................................................................................ 567 17.2.1 High-accuracy Control ; G61.1, G08 .......................................................................................................... 567 17.2.2 SSS Control ............................................................................................................................................... 585 17.2.3 Tolerance Control....................................................................................................................................... 589 17.2.4 Variable-acceleration Pre-interpolation Acceleration/Deceleration ............................................................ 593 17.2.5 Initial High-accuracy Control ...................................................................................................................... 596 17.2.6 Multi-part System Simultaneous High-accuracy ........................................................................................ 597 17.3 High-speed High-accuracy Control..................................................................................................................... 599 17.3.1 High-speed High-accuracy Control I, II, III ; G05.1 Q1/Q0, G05 P10000/P0, G05 P20000/P0.................. 599 17.3.2 Fairing ........................................................................................................................................................ 615 17.3.3 Smooth Fairing........................................................................................................................................... 616 17.3.4 Acceleration Clamp Speed......................................................................................................................... 625 17.3.5 Corner Deceleration in High-speed Mode.................................................................................................. 626 17.3.6 Precautions on High-speed High-accuracy Control ................................................................................... 627 17.4 Spline Interpolation ; G05.1 Q2/Q0..................................................................................................................... 630 17.5 Spline Interpolation 2; G61.4 .............................................................................................................................. 639 17.6 High-accuracy Spline Interpolation ; G61.2 ........................................................................................................ 646 17.7 Machining Condition Selection I ; G120.1,G121................................................................................................. 648 18 Advanced Machining Control ............................................................................................................... 653 18.1 Tool Position Compensation; G43.7/G49 ........................................................................................................... 654 18.2 Tool Length Compensation in the Tool Axis Direction ; G43.1/G49 ................................................................... 661 18.3 Tool Center Point Control; G43.4, G43.5/G49.................................................................................................... 668 18.4 Inclined Surface Machining ; G68.2, G68.3/G69 ................................................................................................ 696 18.4.1 How to Define Feature Coordinate System Using Euler Angles ................................................................ 698 18.4.2 How to Define Feature Coordinate System Using Roll-Pitch-Yaw Angles................................................. 700 18.4.3 How to Define Feature Coordinate System Using Three Points in a Plane ............................................... 702 18.4.4 How to Define Feature Coordinate System Using Two Vectors ................................................................ 704 18.4.5 How to Define Feature Coordinate System Using Projection Angles ........................................................ 706 18.4.6 Define by Selecting The Registered Machining Surface............................................................................ 708 18.4.7 How to Define Feature Coordinate System Using Tool Axis Direction ...................................................... 709 18.4.8 Tool Axis Direction Control; G53.1/G53.6 .................................................................................................. 711 18.4.9 Details of Inclined Surface Machining Operation ....................................................................................... 719 18.4.10 Rotary Axis Basic Position Selection ....................................................................................................... 723 18.4.11 Relationship between Inclined Surface Machining and Other Functions ................................................. 729 18.4.12 Precautions for Inclined Surface Machining............................................................................................. 733 18.5 3-dimensional Tool Radius Compensation (Tool's vertical-direction compensation) ; G40/G41.2,G42.2 .......... 737 19 Coordinate System Setting Functions ................................................................................................. 749 19.1 Coordinate Words and Control Axes .................................................................................................................. 750 19.2 Types of Coordinate Systems............................................................................................................................. 751 19.2.1 Basic Machine, Workpiece and Local Coordinate Systems....................................................................... 751 19.2.2 Machine Zero Point and 2nd, 3rd, 4th Reference Position (Zero Point) .................................................... 752 19.2.3 Automatic Coordinate System Setting ....................................................................................................... 753 19.2.4 Coordinate System for Rotary Axis ............................................................................................................ 754 19.3 Basic Machine Coordinate System Selection ; G53 ........................................................................................... 757 19.4 Coordinate System Setting ; G92 ....................................................................................................................... 760 19.5 Local Coordinate System Setting ; G52............................................................................................................. 762 19.6 Workpiece Coordinate System Setting and Offset ; G54 to G59 (G54.1)........................................................... 766 19.7 Workpiece Coordinate System Preset ; G92.1 .................................................................................................. 776 19.8 3-dimensional Coordinate Conversion ; G68/G69 .............................................................................................. 781 19.9 Coordinate Rotation by Program ; G68/G69....................................................................................................... 799 19.10 Coordinate Rotation Input by Parameter ; G10 I_ J_/K_ .................................................................................. 806 19.11 Scaling ; G50/G51 ............................................................................................................................................ 823 19.12 Reference Position (Zero Point) Return ; G28,G29 .......................................................................................... 827 19.13 2nd, 3rd, and 4th Reference Position (Zero Point) Return ; G30...................................................................... 831 19.14 Tool Change Position Return ; G30.1 - G30.6.................................................................................................. 834 19.15 Reference Position Check ; G27 ...................................................................................................................... 837 20 Protection Function ............................................................................................................................... 839 20.1 Stroke Check before Travel ; G22/G23 .............................................................................................................. 840 20.2 Enable Interfering Object Selection Data; G186................................................................................................. 842 21 Measurement Support Functions ......................................................................................................... 845 21.1 Automatic Tool Length Measurement ; G37 ....................................................................................................... 846 21.2 Skip Function ; G31 ........................................................................................................................................... 850 21.3 Multi-step Skip Function 1 ; G31.n, G04............................................................................................................ 856 21.4 Multi-step Skip Function 2 ; G31 P .................................................................................................................... 858 21.5 Speed Change Skip ; G31 Fn............................................................................................................................ 860 21.6 Torque Limitation Skip ; G160 ............................................................................................................................ 864 21.7 Programmable Current Limitation ; G10 L14 ; .................................................................................................... 868 22 System Variables ................................................................................................................................... 869 22.1 System Variables List ......................................................................................................................................... 870 22.2 System Variables (G Command Modal) ............................................................................................................. 872 22.3 System Variables (Non-G Command Modal) ..................................................................................................... 873 22.4 System Variables (Modal Information at Macro Interruption) ............................................................................. 874 22.5 System Variables (Tool Information) .................................................................................................................. 876 22.6 System Variables (Tool Compensation) ............................................................................................................. 884 22.7 System Variables (Tool Life Management)......................................................................................................... 885 22.8 System Variables (Workpiece Coordinate Offset) .............................................................................................. 890 22.9 System Variables (Extended Workpiece Coordinate Offset) .............................................................................. 891 22.10 System Variables (External Workpiece Coordinate Offset) .............................................................................. 892 22.11 System Variables (Position Information)........................................................................................................... 893 22.12 System Variables (Alarm) ................................................................................................................................. 897 22.13 System Variables (Message Display and Stop)................................................................................................ 898 22.14 System Variables (Cumulative Time) ............................................................................................................... 898 22.15 System Variables (Time Read Variables)......................................................................................................... 899 22.16 System Variables (Machining Information) ....................................................................................................... 901 22.17 System Variables (Reverse Run Information) .................................................................................................. 902 22.18 System Variables (Number of Workpiece Machining Times) ........................................................................... 902 22.19 System Variables (Mirror Image) ...................................................................................................................... 902 22.20 System Variables (Coordinate Rotation Parameter)......................................................................................... 903 22.21 System Variables (Rotary Axis Configuration Parameter)................................................................................ 904 22.22 System Variables (Normal Line Control Parameter)......................................................................................... 905 22.23 System Variables (Parameter Reading) ........................................................................................................... 906 22.24 System Variables (Workpiece Installation Error Compensation Amount)......................................................... 910 22.25 System Variables (Macro Interface Input (PLC -> NC)).................................................................................... 911 22.26 System Variables (Macro Interface Output (NC -> PLC))................................................................................. 917 22.27 System Variables (R Device Access Variables) ............................................................................................... 923 22.28 System Variables (PLC Data Reading) ............................................................................................................ 929 22.29 System Variables (Interfering Object Selection) ............................................................................................... 933 22.30 System Variables (ZR Device Access Variables) [C80] ................................................................................... 936 23 Appx.1: Fixed Cycles ............................................................................................................................. 939 15 Program Support Functions 439 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15Program Support Functions 15.1 Corner Chamfering I /Corner Rounding I Function and purpose Chamfering at any angle or corner rounding is performed automatically by adding ",C_" or ",R_" to the end of the block to be commanded first among those command blocks which shape the corner with lines only. 15.1.1 Corner Chamfering I ; G01 X_ Y_ ,C Function and purpose This chamfers a corner by connecting the both side of the hypothetical corner which would appear as if chamfering is not performed, by the amount commanded by ",C_". Command format N100 G01 X__ Y__ ,C__ ; N200 G01 X__ Y__ ; ,C Length up to chamfering starting point or end point from hypothetical corner Corner chamfering is performed at the point where N100 and N200 intersect. Detailed description (1) The start point of the block following the corner chamfering is the hypothetical corner intersection point. (2) If there are multiple or duplicate corner chamfering commands in a same block, the last command will be valid. (3) When both the corner chamfer and corner rounding commands exist in the same block, the latter command is valid. (4) Tool compensation is calculated for the shape which has already been subjected to corner chamfering. (5) When the block following a command with corner chamfering does not contain a linear command, a corner chamfering/corner rounding II command will be executed. (6) Program error (P383) will occur when the movement amount in the corner chamfering block is less than the chamfering amount. (7) Program error (P384) will occur when the movement amount in the block following the corner chamfering block is less than the chamfering amount. (8) Program error (P382) will occur when a movement command is not issued in the block following the corner chamfering I command. IB-1501278-D 440 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Program example (1) G91 G01 X100. ,C10.; (2) X100. Y100.; Y (2) Y100.0 (c) (1) (a) (b) 10.0 10.0 X X100.0 X100.0 (a) Chamfering start point (b) Hypothetical corner intersection point (c) Chamfering end point 441 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.1.2 Corner Rounding I ; G01 X_ Y_ ,R_ Function and purpose The hypothetical corner, which would exist if the corner were not to be rounded, is rounded with an arc that has a radius commanded by ",R_" only when configured of linear lines. Command format N100 G01 X__ Y__ ,R__ ; N200 G01 X__ Y__ ; ,R Arc radius of corner rounding Corner rounding is performed at the point where N100 and N200 intersect. Detailed description (1) The start point of the block following the corner rounding is the hypothetical corner intersection point. (2) When both corner chamfering and corner rounding are commanded in the same block, the latter command will be valid. (3) Tool compensation is calculated for the shape which has already been subjected to corner rounding. (4) When the block following a command with corner rounding does not contain a linear command, a corner chamfering/corner rounding II command will be executed. (5) Program error (P383) will occur when the movement amount in the corner rounding block is less than the R value. (6) Program error (P384) will occur when the movement amount in the block following the corner rounding block is less than the R value. (7) Program error (P382) will occur if a movement command is not issued in the block following the corner rounding. IB-1501278-D 442 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Program example (1) G91 G01 X100. ,R10.; (2) X100. Y100.; Y (2) Y100.0 (b) (a) (1) R10.0 (c) X X100.0 (a) Corner rounding start point X100.0 (b) Corner rounding end point 443 (c) Hypothetical corner intersection point IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.1.3 Corner Chamfering Expansion/Corner Rounding Expansion Function and purpose Using an E command, the feedrate can be designated for the corner chamfering and corner rounding section. In this way, the corner section can be cut into a correct shape. Example F200. E100. (G94) G01Y70.,C30. F200.E100.; X-110.; F200. F200. E100. (G94) G01Y70.,R30. F200.E100.; X-110.; Y F200. X IB-1501278-D 444 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Detailed description (1) The E command is modal. It is also valid for the feed in the next corner chamfering/corner rounding section. Example (G94) G01Y30.,C10. F100.E50.; X-50.,C10.; Y50.,C10.; X-50.; F100. E50. F100. E50. F100. E50. Y F100. X (2) E command modal has separate asynchronous feedrate modal and synchronous feedrate modal functions. Which one is validated depends on the asynchronous/synchronous mode (G94/G95). (3) When the E command is 0, or when there has not been an E command up to now, the corner chamfering/corner rounding section feedrate will be the same as the F command feedrate. Example Y F100. F100. F100. E50. X F100. F100. F100. E50. F100. (G94) G01Y30.,C10. F100.E50.; X-50.,C10.; Y50.,C10. E0; X-50.; E50. F100. (G94) G01Y30.,C10. F100.; X-50.,C10.; Y50.,C10. E50; X-50.; F100. F100. F100. (4) E command modal is not cleared even if the reset button is pressed. It is cleared when the power is turned OFF. (In the same manner as F commands.) (5) All E commands except those shown below are at the corner chamfering/corner rounding section feedrate. - E commands during thread cutting modal - E commands during thread cutting cycle modal 445 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.1.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding Detailed description (1) Shown below are the operations of manual interruption during corner chamfering or corner rounding. With an absolute value command and manual absolute switch ON. Y N1 G28 XY; N2 G00 X120.Y20. ; N3 G03 X70. Y70.I-50. ,R20. F100 ; N4 G01 X20. Y20. ; 140. N4 N3 40. 20. 70. 120. (mm) X With an incremental value command and manual absolute switch OFF Y N1 G28 XY; N2 G00 X120. Y20. ; N3 G03 X-50. Y50. I-50. ,R20. F100 ; N4 G01 X-50. Y-50.; 140. N4 N3 40. 20. 70. 120. (mm) X Interrupt amount Path in interrupt case Path in non-interrupt case (2)With a single block during corner chamfering or corner rounding, the tool stops after these operations are executed. IB-1501278-D 446 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.2 Corner Chamfering II /Corner Rounding II Function and purpose Corner chamfering and corner rounding can be performed by adding ",C" or ",R" to the end of the block which is commanded first among the block that forms a corner with continuous arbitrary angle lines or arcs. 15.2.1 Corner Chamfering II ; G01/G02/G03 X_ Y_ ,C_ Function and purpose The corner is chamfered by commanding ",C" in the 1st block of the two continuous blocks containing an arc. For an arc, this will be the chord length. Command format N100 G03 X__ Y__ I__ J__ ,C__ ; N200 G01 X__ Y__ ; ,C Length up to chamfering starting point or end point from hypothetical corner Corner chamfering is performed at the point where N100 and N200 intersect. Detailed description (1) If this function is commanded while the corner chamfer or corner rounding command is not defined in the specifications, it causes a program error (P381). (2) The start point of the block following the corner chamfering is the hypothetical corner intersection point. (3) If there are multiple or duplicate corner chamfering commands in a same block, the last command will be valid. (4) When both corner chamfering and corner rounding are commanded in the same block, the latter command will be valid. (5) Tool compensation is calculated for the shape which has already been subjected to corner chamfering. (6) Program error (P385) will occur when positioning or thread cutting is commanded in the corner chamfering command block or in the next block. (7) Program error (P382) will occur when the block following corner chamfering contains a G command other than group 01 or another command. (8) Program error (P383) will occur when the movement amount in the block, commanding corner chamfering, is less than the chamfering amount. (9) Program error (P384) will occur when the movement amount is less than the chamfering amount in the block following the block commanding corner chamfering. (10) Even if a diameter is commanded, it will be handled as a radial command value during corner chamfering. (11) Program error (P382) will occur when a movement command is not issued in the block following the corner chamfering II command. 447 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Program example (1) Linear - arc Y (a) Absolute value command N1 G28 XY; N2 G90 G00 X100. Y100.; N3 G01 X50.Y150.,C20. F100; N4 G02 X0 Y100. I-50. J0; : Relative value command N1 G28 XY; N2 G91 G00 X100. Y100.; N3 G01 X-50.Y50.,C20. F100; N4 G02 X-50. Y-50. I-50. J0; : C20. 150. C20. N3 N4 100. 50. 100. (mm) X (a) Hypothetical corner intersection point (2) Arc - arc Y 130. 110. Absolute value command N1 G28 XY; N2 G91 G00 X140. Y10.; N3 G02 X60.Y50.I0 J100. ,C20. F100; N4 X0 Y30.I-60.J80.; : Relative value command N1 G28 XY; N2 G91 G00 X140. Y10.; N3 G02 X-80.Y40. R100. ,C20. F100; N4 X-60. Y-20. I-60. J80.; : (a) C20. 50. 30. C20. N4 N3 10. 60. (a) Hypothetical corner intersection point IB-1501278-D 448 140. (mm) X M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.2.2 Corner Rounding II ; G01/G02/G03 X_ Y_ ,R_ Function and purpose The corner is rounded by commanding ",R_" in the 1st block of the two continuous blocks containing an arc. Command format N100 G03 X__ Y__ I__ J__ ,R__ ; N200 G01 X__ Y__ ; ,R Arc radius of corner rounding Corner rounding is performed at the point where N100 and N200 intersect. Detailed description (1) If this function is commanded while the corner chamfer or corner rounding command is not defined in the specifications, it causes a program error (P381). (2) The start point of the block following the corner rounding is the hypothetical corner intersection point. (3) When both corner chamfering and corner rounding are commanded in a same block, the latter command will be valid. (4) Tool compensation is calculated for the shape which has already been subjected to corner rounding. (5) Program error (P385) will occur when positioning or thread cutting is commanded in the corner rounding command block or in the next block. (6) Program error (P382) will occur when the block following corner rounding contains a G command other than group 01 or another command. (7) Program error (P383) will occur when the movement amount in the corner rounding block is less than the R value. (8) Program error (P384) will occur when the movement amount is less than the R value in the block following the corner rounding. (9) Even if a diameter is commanded, it will be handled as a radial command value during corner rounding. (10) A program error (P382) will occur if a movement command is not issued in the block following corner rounding. 449 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Program example (1) Linear - arc Y (a) Absolute value command N1 G28 XY; N2 G90 G00 X100. Y30.; N3 G01 X50.Y80.,R10. F100; N4 G02 X0 Y30. I-50.J0; : Relative value command N1 G28 XY; N2 G91 G00 X100. Y30.; N3 G01 X-50.Y50.,R10. F100; N4 G02 X-50. Y-50. I-50.J0; : 80. R10. N3 N4 30. 50. 100. (mm) X (a) Hypothetical corner intersection point (2) Arc - arc Y Absolute value command N1 G28 XY; N2 G90 G00 X100. Y30.; N3 G02 X50.Y80. R50.,R10.F100; N4 X0 Y30. R50.; : Relative value command N1 G28 XY; N2 G91 G00 X100. Y30.; N3 G02 X-50.Y50. I0 J50.,R10.F100; N4 X-50. Y-50. I-50. J0; : (a) 80. R10. N4 N3 30. 50. 100. (mm) X (a) Hypothetical corner intersection point 15.2.3 Corner Chamfering Expansion/Corner Rounding Expansion For details, refer to "Corner Chamfering I / Corner Rounding" and "Corner Chamfering Expansion / Corner Rounding Expansion". 15.2.4 Interrupt during Corner Chamfering/Interrupt during Corner Rounding For details, refer to "Corner Chamfering I / Corner Rounding" and "Interrupt during Corner Chamfering Interrupt during / Corner Rounding". IB-1501278-D 450 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.3 Linear Angle Command ; G01 X_/Y_ A_/,A_ Function and purpose The end point coordinates are automatically calculated by commanding the linear angle and one of the end point coordinate axes. Command format N1 G01 Xx1(Yy1) Aa1; N2 G01 Xx2(Yy2) A-a2; (A-a2 can also be set as Aa 3. ) N1 G01 Xx1(Yy1) ,Aa1; N2 G01 Xx2(Yy2) ,A-a2; This designates the angle and the X or Y axis coordinates. Select the command plane with G17 to G19. Y ( x1,y1) y1 a2 N1 N2 a3 a1 y2 ( x2,y2) X Detailed description (1) The angle is set based on the positive (+) direction of the horizontal axis for the selected plane. The counterclockwise (CCW) direction is indicated by a positive sign (+), and the clockwise (CW) direction by a negative sign (-). (2) Either of the axes on the selected plane is commanded for the end point. (3) The angle is ignored when the angle and the coordinates of both axes are commanded. (4) When only the angle has been commanded, this is treated as a geometric command. (5) The angle of either the start point (a1) or end point (a2) may be used. (6) This function is valid only for the G01 command; it is not valid for other interpolation or positioning commands. (7) The range of slope "a" is between -360.000 and 360.000. When a value outside this range is commanded, it will be divided by 360 (degrees) and the remainder will be commanded. (Example) If 400 is commanded, 40° (remainder of 400/360) will become the command angle. (8) If an address A is used for the axis name or the 2nd miscellaneous function, use ",A" as the angle. (9) If "A" and ",A" are commanded in a same block, ",A" will be interpreted as the angle. Note A program error (P33) will occur if this function is commanded during the high-speed machining mode or highspeed high-accuracy mode. 451 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.4 Geometric ; G01 A_ Function and purpose When it is difficult to calculate the intersection point of two straight lines in a continuous linear interpolation command, the end point of the first straight line will be automatically calculated inside the CNC and the movement command will be controlled, provided that the slope of the first straight line as well as the end point coordinates and slope of the second straight line are commanded. Note (1) If the parameter (#1082 Geomet) is set to 0, geometric I will not function. Command format N1 G01 Aa1 (A-a2) Ff1; N2 Xx2 Yy2 A-a4 (A-a3) Ff2; Aa1, A-a2, A-a3, Aa4 Angle Ff1, Ff2 Speed Xx2, Yy2 Next block end point coordinates Y ? a3 N1 a2 X N2 a1 (C) a4 (x2,y2) (C) Current position Detailed description (1) Program error (P396) will occur when the geometric command is not on the selected plane. (2) The slope indicates the angle to the positive (+) direction of the horizontal axis for the selected plane. The counterclockwise (CCW) direction is indicated by a positive sign (+), and the clockwise (CW) direction by a negative sign (-). (3) The range of slope "a" is between -360.000 and 360.000. When a value outside this range is commanded, it will be divided by 360 (degrees) and the remainder will be commanded. (Example) If 400 is commanded, 40° (remainder of 400/360) will become the command angle. (4) The slope of the line can be commanded on either the start or end point side. Whether designated slope is the starting point or the end point will be automatically identified in NC. (5) The end point coordinates of the second block should be commanded with absolute values. If incremental values are used, program error (P393) will occur. (6) The feedrate can be commanded for each block. (7) When the angle where the two straight lines intersect is less than 1°, program error (P392) will occur. (8) Program error (P396) will occur when the plane is changed in the 1st block and 2nd block. (9) This function is ignored when address A is used for the axis name or as the 2nd miscellaneous function. (10) Single block stop is possible at the end point of the 1st block. (11) Program error (P394) will occur when the 1st and 2nd blocks do not contain the G01 or G33 command. IB-1501278-D 452 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Relationship with Other Functions (1) Corner chamfering and corner rounding can be commanded after the angle command in the 1st block. (x2,y2) N2 a2 (Example 1) N1 Aa1 ,Cc1 ; N2 Xx2 Yy2 Aa2 ; c1 ? a1 N1 c1 (x1,y1) (x2,y2) N2 a2 (Example 2) N1 Aa1 ,Rr1 ; N2 Xx2 Yy2 Aa2 ; r1 ? N1 a1 (x1,y1) (2) The geometric command I can be issued after the corner chamfering or corner rounding command. (x3,y3) N3 a2 ? N2 (Example 3) N1 Xx2 Yy2 ,Cc1 ; N2 Aa1 ; N3 Xx3 Yy3 Aa2 ; a1 c1 (x2,y2) N1 c1 (x1,y1) (3) The geometric command I can be issued after the linear angle command. (x3,y3) N3 a3 ? (Example 4) N1 Xx2 Aa1 ; N2 Aa2 ; N3 Xx3 Yy3 Aa3 ; N2 (x2,y2) a2 N1 a1 (x1,y1) 453 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.5 Geometric IB Function and purpose With the geometric IB function, the contact and intersection are calculated by commanding an arc center point or linear angle in the movement commands of two continuous blocks (only blocks with arc commands), instead of commanding the first block end point. Note (1) If the parameter (#1082 Geomet) is not set to 2, geometric IB will not function. Two-arc contact N2 r1 (??) r2 Y X N1 Linear - arc (arc - linear) intersection N1 r1 (??) Y r1 N2 (??) N1 N2 X Linear - arc (arc - linear) contact N2 r1 r1 N1 N1 (??) Y N2 X IB-1501278-D (??) 454 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.5.1 Geometric IB (Automatic Calculation of Two-arc Contact) ; G02/G03 P_Q_ /R_ Function and purpose When the contact of two continuous contacting arcs is not indicated in the drawing, it can be automatically calculated by commanding the 1st circular center coordinate value or radius, and the 2nd arc end point absolute value and center coordinate value or radius. Command format N1 G02(G03) Pp1 Qq1 Ff1; N2 G03(G02) Xx2 Yy2 Pp2 Qq2 Ff2; N1 G02(G03) Pp1 Qq1 Ff1; N2 G03(G02) Xx2 Yy2 Rr2 Ff2; N1 G02(G03) Rr1 Ff1; N2 G03(G02) Xx2 Yy2 Pp2 Qq2 Ff2; P,Q X and Y axes circular center coordinate absolute value (diameter/radius value command)The center address for the 3rd axis is commanded with A. R Arc radius (when a (-) sign is attached, the arc is judged to be 180° or more) * I and J (X and Y axes arc center coordinate incremental value) commands can be issued instead of P and Q. 1st block arc : Incremental amount from the start point to the center 2nd block arc : Incremental amount from the end point to the center (p1,q1) r2 (x2,y2) (p2,q2) r1 Y X 455 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Detailed description (1) Program error (P393) will occur before the 1st block if the 2nd block is not a coordinate absolute value command. (2) Program error (P398) will occur before the 1st block if there is no geometric IB specification. (3) Program error (P395) will occur before the 1st block if there is no R (here, the 1st block is designated with P, Q (I, J)) or P, Q (I, J) designation in the 2nd block. (4) Program error (P396) will occur before the 1st block if another plane selection command (G17 to G19) is issued in the 2nd block. (5) Program error (P397) will occur before the 1st block if two arcs that do not contact are commanded. (6) The contact calculation accuracy is ±1μm (fractions rounded up). (7) Single block operation stops at the 1st block. (8) When I or J is omitted, the values are regarded as I0 and J0. P and Q cannot be omitted. (9) The error range in which the contact is obtained is set in parameter "#1084 RadErr". Tool path "Arc error" (10) For an arc block perfect circle command (arc block start point = arc block end point), the R designation arc command finishes immediately, and there is no operation. Thus, use a PQ (IJ) designation arc command. (11) G codes of the G modal group 1 in the 1st/2nd block can be omitted. (12) Addresses being used as axis names cannot be used as command addresses for arc center coordinates or arc radius. (13) When the 2nd block arc inscribes the 1st block arc and the 2nd block is an R designation arc, the R+ sign becomes the inward turning arc command, and the R- sign becomes the outward turning arc command. N2 R- R+ N1 IB-1501278-D 456 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.5.2 Geometric IB (Automatic Calculation of Linear - Arc Intersection) ; G01 A_ , G02/G03 P_Q_H_ Function and purpose When the contact point of a shape in which contact between a line and an arc is not indicated in the drawing, it can be automatically calculated by commanding the following program. Command format (For G18 plane) N1 G01 Aa1 (A-a2) Ff1; N2 G02(G03) Xx2 Yy2 Pp2 Qq2 Hh2 Ff2 ; N1 G02(G03) Pp1 Qq1 Hh1 (,Hh1) Ff1 ; N2 G1 Xx2 Yy2 Aa3 (A-a4) Ff2 ; A Linear angle (-360.000° to 360.000°) P,Q X and Y axes circular center coordinate absolute value (diameter/radius value command)The center address for the 3rd axis is commanded with A. H (,H) Selection of linear - arc intersection 0: Intersection of the shorter line 1: Intersection of the longer line * I and J (X and Y axes arc center coordinate incremental value) commands can be issued instead of P and Q. 1st block arc : Incremental amount from the start point to the center 2nd block arc : Incremental amount from the end point to the center N2 H=0 (??) N1 H=1 H=1 (??) (??) N1 (??) (p2,q2) - a2 (p1,q1) (x2,y2) a1 H=0 - a4 N2 a3 (x2,y2) Y X 457 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Detailed description (1) When the 2nd miscellaneous function address is A, the 2nd miscellaneous function is validated and this function is invalidated. (2) Program error (P393) will occur before the 1st block if the 2nd block is not a coordinate absolute value command. (3) Program error (P398) will occur before the 1st block if there is no geometric IB specification. (4) In case of the 2nd block arc, a program error (P395) will occur before the 1st block if there is no P, Q (I, J) designation. A program error (P395) will also occur if there is no A designation for the line. (5) Program error (P396) will occur before the 1st block if another plane selection command (G17 to G19) is issued in the 2nd block. (6) Program error (P397) will occur before the 1st block if a straight line and arc that do not contact or intersect are commanded. (7) Single block operation stops at the 1st block. (8) When I or J is omitted, the values are regarded as I0 and J0. P and Q cannot be omitted. (9) When H is omitted, the value is regarded as H0. (10) The linear - arc contact is automatically calculated by designating R instead of P, Q (I, J). (11) The error range in which the intersect is obtained is set in parameter "#1084 RadErr". Tool path Arc error (12) As seen from the + direction of the horizontal axis of the selected plane, the counterclockwise (CCW) direction is considered to be + and the clockwise direction (CW) -. (13) The slope of the line can be commanded on either the start or end point side. Whether designated slope is the starting point or the end point will be automatically identified. (14) When the distance to the intersection from the line and arc is same (as in the figure below), the control by address H (short/long distance selection) is invalidated. In this case, the judgment is carried out based on the angle of the line. (p2,q2) a1 N1 G1 A a1 Ff1; N2 G2 Xx2 Yy2 Pp2 Qq2 Ff2 ; -a2 N1 G1 A –a2 Ff1; N2 G2 Xx2 Yy2 Pp2 Qq2 Ff2 ; (15) The intersect calculation accuracy is ±1μm (fractions rounded up). (16) In linear - arc intersections, the arc command can only be PQ (IJ) command. When the arc block start point and arc block end point are the same point, the arc is a perfect circle. IB-1501278-D 458 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (17) G codes of the G modal group in the 1st block can be omitted. (18) Addresses being used as axis names cannot be used as command addresses for angles, arc center coordinates or intersection selections. (19) When geometric IB is commanded, two blocks are pre-read. Relationship with other functions Command Tool path Geometric IB + corner chamfering N1 G02 P_ Q_ H_ ; N2 G01 X_ Y_ A_ ,C_ ; G01 X_ Y_ ; Y N2 X 459 N1 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.5.3 Geometric IB (Automatic Calculation of Linear - Arc Intersection) ; G01 A_ , G02/G03 R_H_ Function and purpose When the intersection of a shape in which a line and an arc intersect is not indicated in the drawing, it can be automatically calculated by commanding the following program. Command format (For G18 plane) N1 G01 Aa1 (A-a2) Ff1; N2 G03(G02) Xx2 Yy2 Rr2 Ff2; N1 G03(G02) Rr1 Ff1; N2 G01 Xx2 Yy2 Aa3 (A-a4) Ff2 ; A Linear angle (-360.000° to 360.000°) R Circular radius (??) N1 a1 Y - a2 r2 (??) N1 N2 r1 - a4 N2 a3 (x2,y2) (x2,y2) X Detailed description (1) When the 2nd miscellaneous function address is A, the 2nd miscellaneous function is validated and this function is invalidated. (2) Program error (P393) will occur before the 1st block if the 2nd block is not a coordinate absolute value command. (3) Program error (P398) will occur before the 1st block if there is no geometric IB specification. (4) Program error (P396) will occur before the 1st block if another plane selection command (G17 to G19) is issued in the 2nd block. (5) A program error (P397) will occur before the 1st block if a straight line and arc that do not contact are commanded. (6) In case of the 2nd block arc, a program error (P395) will occur before the 1st block if there is no R designation. A program error (P395) will also occur if there is no A designation for the line. (7) Single block operation stops at the 1st block. (8) The linear - arc contact is automatically calculated by designating R instead of P, Q (I, J). IB-1501278-D 460 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (9) The error range in which the contact is obtained is set in parameter "#1084 RadErr". Tool path Arc error (10) The line slope is the angle to the positive (+) direction of its horizontal axis. Counterclockwise (CCW) is positive (+). Clockwise (CW) is negative (-). (11) The slope of the line can be commanded on either the start or end point side. Whether the commanded slope is on the start or end point side is identified automatically inside the NC unit. (12) The intersect calculation accuracy is ±1μm (fractions rounded up). (13) In linear - arc contact, the arc command can only be an R command. Thus, when the arc block start point = arc block end point, the arc command finishes immediately, and there will be no operation. (Perfect circle command is impossible.) (14) G codes of the G modal group 1 in the 1st block can be omitted. (15) Addresses being used as axis names cannot be used as command addresses for angles or arc radius. (16) When geometric IB is commanded, two blocks are pre-read. Relationship with other functions Command Tool path Geometric IB + corner chamfering N1 G03 R_ ; N2 G01 X_ Y_ A_ ,C_ ; G01 X_ Y_ ; N2 Y N1 X Geometric IB + corner rounding N1 G03 R_ ; N2 G01 X_ Y_ A_ ,R_ ; G01 X_ Y_ ; N2 Y N1 X 461 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.6 G Command Mirror Image ; G50.1,G51.1 Function and purpose When cutting a shape that is symmetrical on the left and right, programming time can be shortened by machining one side and then using the same program to machine the other side. The mirror image function is effective for this. For example, when using a program as shown below to machine the shape on the left side (A), a symmetrical shape (B) can be machined on the right side by applying mirror image and executing the program. Y (A) (B) X Mirror axis Command format Mirror image ON G51.1 Xx1 Yy1 Zz1 x1, y1, z1 Mirror image center coordinates (Mirror image will be applied regarding this position as a center) Mirror image OFF G50.1 Xx2 Yy2 Zz2 x2, y2, z2 IB-1501278-D Mirror image cancel axis (The values of x2, y2, z2 will be ignored.) 462 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Detailed description (1) At G51.1, command the mirror image axis and the coordinate to be a center of mirror image with the absolute command or incremental command. (2) At G50.1, command the axis for which mirror image is to be turned OFF. The values of x2, y2, and z2 will be ignored. (3) If mirror image is applied on only one axis of the designated plane, the rotation direction and compensation direction will be reversed for the arc or tool radius compensation and coordinate rotation, etc. (4) This function is processed on the local coordinate system, so the center of the mirror image will change when the counter is preset or when the workpiece coordinates are changed. (5) Reference position return during mirror image If the reference position return command (G28, G30) is executed during the mirror image, the mirror image will be valid during the movement to the intermediate point, but will not be applied to the movement to the reference point after the intermediate point. Path on which mirror is applied Mirror center Programmed path Intermediate point when mirror is applied Intermediate point (6) Return from zero point during mirror image If the return command (G29) from the zero point is commanded during the mirror image, the mirror will be applied to the intermediate point. (7) The mirror image will not be applied to the G53 command. 463 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Relationship with other functions (1) Combination with radius compensation The mirror image (G51.1) will be processed after the radius compensation (G41, G42) is applied, so the following type of cutting will take place. Programmed path Path with mirror image applied Program path Path with only radius compensation applied Path with only mirror image applied Path with mirror image and radius compensation applied IB-1501278-D 464 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Precautions CAUTION Turn the mirror image ON and OFF at the mirror image center. If mirror image is not canceled at the mirror center, the absolute value and machine position will deviate as shown below. (This state will last until an absolute value command (positioning with G90 mode) is issued, or a reference position return with G28 or G30 is executed.) The mirror center is set with an absolute value, so if the mirror center is commanded again in this state, the center may be set to an unpredictable position. Cancel the mirror at the mirror center or position with the absolute value command after canceling. Absolute value (position commanded in program) Machine position When moved with the incremental command after mirror cancel Mirror cancel command Mirror axis command Mirror center 465 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.7 Normal Line Control ; G40.1/G41.1/G42.1 (G150/G151/G152) Function and purpose The C axis (rotary axis) turning will be controlled so that the tool constantly faces the normal line direction in respect to the movement of the axes in the selected plane during program operation. At the block seams, the C axis turning is controlled so that the tool faces the normal line direction at the next block's start point. C axis center (rotary axis) Tool end position C axis turning During arc interpolation, the rotary axis turning is controlled in synchronization with the operation of the arc interpolation. Rotation axis center (C axis) Tool end position The normal line control I and II can be used according to the C axis turning direction during normal line control. Which method is to be used depends on the MTB specifications (parameter "#1524 C_type"). Normal line control type Turning direction Turning speed Type I Direction that is 180° or less Parameter speed (#1523 C_feed) (#1524 C_type = 0) (shortcut direction) Type II As a principle, the com(#1524 C_type = 1) manded direction IB-1501278-D Feedrate 466 Turning speed in arc interpolation Speed when the program path follows the F command Speed when the tool nose follows the F command M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Command format Normal line control cancel G40.1 (G150)X__ Y__ F__ ; Normal line control left ON G41.1 (G151)X__ Y__ F__ ; Normal line control right ON G42.1 (G152)X__ Y__ F__ ; X X axis end point coordinate Y Y axis end point coordinate F Feedrate G41.1 Normal line control left side G42.1 Normal line control right side (a) (a) (b) (b) (a) Center of rotation (b) Tool end(b) Tool end Programmed path Tool end path The normal line control axis depends on the MTB specifications (parameter #1522 C_axis). Normal line control is carried out in respect to the movement direction of the axis which is selecting the plane. G17 plane I-J axes G18 plane K-I axes G19 plane J-K axes Whether the normal line control is canceled at resetting depends on the MTB specifications (parameter “#1210 RstGmd/ bitE”). 467 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Detailed description Definition of the normal line control angle The normal line control angle is 0° (degree) when the tool is facing the horizontal axis (+ direction) direction. The counterclockwise direction turning is + (plus), and the clockwise direction turning is - (minus). G17 plane (I - J axes) ... The axis angle is 0°(degree) when the tool is facing the +I direction. J+ 90 180 0 I+ 270 G18 plane (K - I axes) ...The axis angle is 0°(degree) when the tool is facing the +K direction. I+ 90 180 0 K+ 270 G19 plane (J - K axes) ... The axis angle is 0°(degree) when the tool is facing the +J direction. K+ 90 180 0 270 IB-1501278-D 468 J+ M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Normal line control turning operation in respect to movement command (1) Start-up After the normal line control axis turns to the right angle of the advance direction at the start point of the normal line control command block, the axis which is selecting the plane is moves. Note that the normal line control axis at the start up turns in the direction that is 180° or less (shortcut direction) in both the normal line control type I and II. G41.1 N1 : N3 N1 G01 Xx1 Yy1 Ff1 ; N2 G41.1 ; N3 (x1,y1) ... Independent block N3 Xx2 Yy2 ; : (x2,y2) N2 is fixed G41.1 N1 N2 : N1 G01 Xx1 Yy1 Ff1 ; N2 (x1,y1) N2 G41.1 Xx2 Yy2 ; ... Same block : (x2,y2) (2) During normal line control mode (a) Operation in block During interpolation of the linear command, the angle of the normal line control axis is fixed, and the normal line control axis does not turn. During the arc command, the normal line control axis turns in synchronization with the operation of the arc interpolation. : G41.1 ; N1 G02 Xx1 Yy1 Ii1 Jj1 ; : (i1,j1) N1 Programmed path Tool end path (x1,y1) 469 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (b) Block seam No tool radi- After the normal line control axis is turned to be at the right angle of the plane selecting us compen- movement in the next block, the operation moves to the next block. sation Liner - Liner Liner - Arc Arc - Arc Programmed path Tool end path With tool ra- If tool radius compensation is applied, normal line control is carried out along the path to dius com- which the tool radius compensation is applied. pensation Liner - Liner Liner - Arc Arc - Arc Programmed path Tool radius compensation path Tool end path (3) Cancel The normal line control axis will not turn, and the plane selecting axis will be moved by the program command. : G40.1 N1 G01 Xx1 Yy1 Ff1 ; N2 G40.1 ; N1 (x1,y1) ... Independent block N3 Xx2 Yy2 ; N3 : (x2,y2) N2 is fixed G40.1 N1 (x1,y1) : N1 G01 Xx1 Yy1 Ff1 ; N2 N2 G40.1 Xx2 Yy2 ; : (x2,y2) IB-1501278-D 470 ... Same block M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Normal line control temporary cancel During normal line control, the turning operation for the normal line control axis is not carried out at the seam between a block and the next block, in which the movement amount is smaller than that set with the parameter (#1535 C_leng). (1) For liner block; When the movement amount of the N2 block is smaller than the parameter(#1535 C_leng), the normal line control axis is not turned at the seam between the N1 block and N2 block. It stays the same direction as the N1 block. N2 block movement amount < Parameter(#1535 C_leng) N2 N1 N3 (2) For arc block; When the diameter value of the N2 block is smaller than the parameter(#1535 C_leng), the normal line control axis is not turned at the seam between the N1 block and N2 block. It stays the same direction as the N1 block. During arc interpolation of the N2 block, the normal line control axis does not turn in synchronization with the operation of arc interpolation. N2 block diameter value < Parameter (#1535 C_leng) N2 N1 (a) N3 (a) Diameter value Note Since operation fractions are created by calculating the intersection point of two segments, the turning operation may or may not be carried out when the parameter (#1535 C_leng) and the segment length are equal. 471 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Normal line control axis turning direction at block seam The normal line control axis turning direction at block seam differs according to the normal line control type I or II (parameter “#1524 C_type”). The turning angle is limited by the angle ε set with the parameter (#1521 C_min). These parameter settings depend on the MTB specifications. Item Normal line control type I Direction that is 180° or less. Normal line control axis turning direction at (shortcut direction) block seam When | θ | < ε, turning is not performed. Normal line control θ: Turning angle axis turning angle at ε: Parameter (#1521 C_min) block seam When the turning angle is 180 degrees, the turning direction is undefined regardless of the command mode. Normal line control type II G41.1: - direction (CW) G42.1: + direction (CCW) When | θ | < ε, turning is not performed. θ: Turning angle ε: Parameter (#1521 C_min) The operation error (0118) will occur in the following cases: [For G41.1] ε <= θ < 180° - ε [For G42.1] 180° + ε < θ <= 360° - ε [G41.1 When the normal line control axis [G41.1/G42.1 When the normal line control is at 0°] axis is at 0°] 90 90 (a) 180 180 0 - 180 0 - - (d) (c) (b) (e) (c) 270 270 [G42.1 When the normal line control axis (a) The normal line control axis turns coun- is at 0°] terclockwise. (d) (b) The normal line control axis turns clock90 wise. (c) The axis does not turn. 180 180 0 + - (c) (e) 270 (c) The axis does not turn. (d) The normal line control axis turns. (e) Operation error (0118) IB-1501278-D 472 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (1) Normal line control type I Normal line control axis turning angle at block seam: θ 1. -ε < θ < ε G41.1 G42.1 90 180 0 - No turning No turning Shortcut direction Shortcut direction 270 (-90 ) 2. ε <= θ < 180° 90 180 0 270 (-90 ) 3. 180° <= θ <= 360°- ε 90 180 0 360 - 270 (-90 ) 473 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (2) Normal line control type II Normal line control axis turning angle at block seam: θ 1. -ε < θ < ε G41.1 G42.1 90 180 0 - No turning No turning 270 (-90 ) 2. ε <= θ < 180°- ε 90 180 - 180 0 270 Operation error (0118) (*1) (-90 ) 3. 180°-ε <= θ <= 180°+ ε 90 180 - 180 180 0 + 270 (-90 ) 4. 180°+ ε < θ <= 360°- ε 90 180 180 0 + 360 - 270 Operation error (0118) (*1) (-90 ) (*1) If the axis turns into the command direction, it turns inside the workpiece, causing an operation error. IB-1501278-D 474 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Operation to be performed when the turning angle set before the circular interpolation starts falls below the minimum turning angle The turning angle falls to or below the minimum turning angle (parameter "#1521 C_min") before the circular interpolation starts; therefore, turning operation may not be inserted. In this case, it depends on the parameter "#12105 C_minTyp" whether to interpolate the turning angle which was not inserted before the tool reaches the end point of circular interpolation. These parameters depends on the MTB specifications. If the turning angle set before the linear interpolation starts falls to or below the minimum turning angle, turning is not carried out. [The turning angle is interpolated up to the end point of the arc (“#12105 C_minTyp” = 0).] The turning angle in the section in which the normal line control axis is not turned is interpolated up to the end point of the circular interpolation. The turning angle falls below the value of parameter #1521. (The control does not insert the turning movement) Tool end path N1 N2 Programmed path Circular center [The turning angle is not interpolated (“#12105 C_minTyp” = 1).] The turning angle in the section in which the normal line control axis is not turned is not interpolated during circular interpolation. The turning angle falls below the value of parameter #1521. (The control does not insert the turning movement) Tool end path N1 N2 Programmed path Circular center 475 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Therefore, an operation error will occur. Normal line control axis turning speed Turning speed at block seam (select from type I or type II) (1) Normal line control axis turning speed at block seam (a) Rapid traverse Normal line control type I Dry run OFF Normal line control type II Dry run OFF The rapid traverse rate (#2001 rapid) is applied. Normal line control axis turning speed f = Rapid traverse rate * (Rapid traverse override) (° / min) Normal line control axis turning speed f = F * 180 / (π * R) * (Rapid traverse override) (°/min) When R = 0, follow the formula below. Normal line control axis turning speed f = F * (Rapid traverse override) (° /min) F: Rapid traverse rate (#2001 rapid) (mm/min) R: Parameter (#8041 C-rot.R) (mm) (Length from normal line control axis center to tool nose) <Note> Dry run ON The manual feedrate is applied. Normal line control axis turning speed f = Manual feedrate * (Cutting feed override) (° /min) (1) If the normal line control axis turning speed exceeds the rapid traverse rate (#2001 rapid), the rapid traverse rate will be applied. Dry run ON Normal line control axis turning speed f = F * 180 / (π * R) * (Rapid traverse override) (°/min) When R = 0, follow the formula below. Normal line control axis turning speed f = F * (Rapid traverse override) (° /min) (1) When the manual override valid is ON, the cutting F: Rapid traverse rate (#2001 rapid) (mm/min) feed override is valid. R: Parameter (#8041 C-rot.R) (mm) (2) If the normal line control axis turning speed ex- (Length from normal line control axis center to tool ceeds the cutting feed clamp speed (#2002 nose) clamp), the cutting feed clamp speed will be ap- <Note> plied. (1) If the normal line control axis turning speed ex(3) When the rapid traverse is ON, the dry run is inceeds the cutting feed clamp speed (#2002 valid. clamp), the cutting feed clamp speed will be applied. <Note> (2) If the normal line control axis turning speed exceeds the rapid traverse rate (#2001 rapid), the rapid traverse rate will be applied. (3) When the rapid traverse is ON, the dry run is invalid. IB-1501278-D 476 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (b) Cutting feed Normal line control type I Dry run OFF Normal line control type II The feedrate at the tool nose is the F command. The normal line control axis turning speed is the normal The normal line control axis turning speed set with the line control axis speed that follows this F command. parameter (#1523 C_feed) is applied. Normal line control axis turning speed f Normal line control axis turning speed f = Parameter (#1523 C_feed) * (Cutting feed override) = F * 180 / (π * R) * (Cutting feed override) (°/min) (° /min) When R = 0, follow the formula below. Dry run ON (Rapid traverse ON) Normal line control axis turning speed f = F (° /min) F: Feedrate command (mm/min) The cutting feed clamp speed (#2002 clamp) is apR: Parameter (#8041 C-rot.R) (mm) plied. (Length from normal line control axis center to tool Normal line control axis turning speed f nose) = Cutting feed clamp speed (°/min) Dry run ON (Rapid traverse OFF) The manual feedrate is applied. Normal line control axis turning speed f = Manual feedrate * (Cutting feed override) (° /min) <Note> <Note> (1) When the manual override valid is ON, the cutting (1) If the normal line control axis turning speed exfeed override is valid. ceeds the cutting feed clamp speed (#2002 clamp), the cutting feed clamp speed will be ap(2) If the normal line control axis turning speed explied. ceeds the cutting feed clamp speed (#2002 clamp), the cutting feed clamp speed will be ap- (2) When the dry run is ON, the normal line control plied. axis turning speed is obtained by the same expression as the rapid traverse. (F) (R) (F) (f) =F*180/( (f) *R) F: Feedrate command f: Normal line control axis turning speed R: Parameter (#8041 C-rot.R) F: Feedrate command f: Normal line control axis turning speed 477 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (2) Normal line control axis turning speed during circular interpolation Normal line control type I Normal line control type II The normal line control axis turning speed is the rota- The feedrate at the tool nose is the F command. The tion speed obtained by feedrate F. normal line control axis turning speed is the rotation speed that follows this F command. Normal line control axis turning speed f = F * 180 / (π * r) (° /min) Normal line control axis turning speed f F : Feed command speed (mm/min) = F * 180 / (π * (R + r)) (° /min) r : Arc radius (mm) F : Feed command speed (mm/min) R : Parameter (#8041 C-rot. R) (mm) (Length from normal line control axis center to tool (F) nose) r : Arc radius (mm) (F) (r) (f) =F*180/( *r) (R) (r) (f) =F*180/( *(R+r)) Note (1) If the normal line control axis turning speed exceeds the cutting feed clamp speed (#2002 clamp), the speed will be as follows; - Normal line control axis turning speed = Cutting feed clamp speed. Normal line control axis turning speed = Cutting feed clamp speed Moving speed during arc interpolation = The speed according to the normal line control axis turning speed IB-1501278-D 478 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Automatic corner arc insertion function During normal line control, an arc is automatically inserted at the corner in the axis movement of the plane selection. This function is for the normal line control type I. The radius of the arc to be inserted is set with the parameter (#8042 C-ins.R). This parameter can be read and written using the macro variable #1901. Normal line control is performed also during the interpolation for the arc to be inserted. Parameter (#8042 C-rot. R) <Supplements> The corner arc is not inserted in the following cases: linear and arc, arc and arc, linear and moveless or moveless and linear blocks or when a line is shorter than the radius of the arc to insert. Corner R is not inserted. During the radius compensation, the radius compensation is applied to the path that the corner arc is inserted. Radius compensation path Parameter (#8042 C-rot. R) 479 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions The stop point of the single block and block start interlock is as follows. Stop point The stop point of the cutting start interlock is as follows. Stop point IB-1501278-D 480 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Program example Normal line control type I Main program O500 Sub program O501 G91X0Y0;G28C0; G90G92G53X0Y0; G00G54X25.Y-10.; G03G41.1X35.Y0.R10.F10.; #10=10; WHILE[#10NE0]DO1; M98P501; #10=#10-1; END1; G03X25.Y10.R10.; G40.1; G28X0Y0; M02; G03X8.Y9.R15.; G02X-8.R10.; G03Y-9.R-15.; G02X8.R10.; G03X35.Y0.R15.; M99; R10 R15 R10 (0,0) 20. 20. 481 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Normal line control type II (Example 1) Main program O500 Sub program O1001 G91X0Y0; G17G91G01Y20.,R10.Z-0.01; G28Z0; X-70.,R10.; G28C0; Y-40.,R10.; G90G92G53X0Y0Z0; X70.,R10.; G00G54G43X35.Y0.Z100.H Y20.; 1; M99; G00Z3.; G01Z0.1F6000; O1002 G42.1; G17G91G01Y20.,R10.; M98P1001L510; X-70.,R10.; M98P1002L2; Y-40.,R10.; G91G01Y10.Z0.05; X70.,R10.; G40.1; Y20.; G90G00Z100.; M99; G28X0Y0Z0; M02; (Corner chamfering/Corner R specifications are required) (Corner chamfering/Corner R specifications are required) (a) (b) 0.1 5. 10. R10 20. (0,0) 20. 35. 35. (a) C axis (b) Tool IB-1501278-D 482 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (Example 2) Main program O2000 Sub program O2001 G91G28Z0; G28X0Y0; G28C0; G90G92G53X0Y0Z0; G00G54X30.Y0.; G00Z3.; G41.1G01Z0.1F5000; M98P2001L510; M98P2002L2; G91G01X-30.Z0.05; G40.1; G90G00Z100.; G28X0Y0Z0; M02; G17G91G01X-60.Z-0.01; X60.; M99; O2002 G17G91G01X-60.; X60.; M99; (a) (b) 0.1 5. (0,0) 30. 30. (a) C axis (b) Tool 483 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Relationship with Other Functions Function name Notes Unidirectional positioning Normal line control is not applied. Helical cutting Normal line control is applied normally. Spiral interpolation As the start point and end point are not on the same arc, a normal line control will not be applied correctly. Exact stop check The operation will not decelerate and stop for the turning movement of the normal line control axis. Error detect Error detect is not applied to the turning movement of the normal line control axis. Override Override is applied to the turning movement by normal line control axis. Coordinate rotation by program Normal line control is applied to the shape after coordinate rotation. Scaling Normal line control is applied to the shape after scaling. Mirror image Normal line control is applied to the shape after mirror image. Thread cutting Normal line control is not applied. Geometric command Normal line control is applied to the shape after geometric command. Automatic reference position Normal line control is not applied. return Start position return Normal line control is not applied to the movement to the intermediate point position. If the base specification parameter "#1086 G0Intp" is OFF, normal line control is applied to the movement from the intermediate point to a position designated in the program. High-speed machining mode This cannot be commanded during normal line control. Program error (P29) will III occur. The normal line control command during high-speed machining mode III cannot be issued, either. Program error (P29) will occur. High-accuracy control This cannot be commanded during normal line control. Program error (P29) will occur. The normal line control command during high-accuracy control cannot be issued, either. Program error (P29) will occur. Spline This cannot be commanded during normal line control. Program error (P29) will occur. The normal line control command during spline cannot be issued, either. Program error (P29) will occur. High-speed High-accuracy control I/II This cannot be commanded during normal line control. Program error (P29) will occur. The normal line control command during high-speed High-accuracy control I/II cannot be issued either. Program error (P29) will occur. Cylindrical interpolation This cannot be commanded during normal line control. Program error (P486) will occur. The normal line control command during cylindrical interpolation cannot be issued, either. Program error (P481) will occur. Workpiece coordinate system offset The workpiece coordinate system cannot be changed during normal line control. Program error (P29) will occur. The program parameter input (G10L2) cannot be commanded either. Program error (P29) will occur. Local coordinate system off- The local coordinate system cannot be changed during normal line control. Proset gram error (P29) will occur. Program restart The program including the normal line control command cannot be restarted. "E98 CAN'T RESEARCH" will occur. Dry run The feedrate is changed by the dry run signal even in respect to the turning movement of the normal line control axis. IB-1501278-D 484 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Function name Notes Graphic check The section turned by normal line control is not drawn. The axes subject to graphic check are drawn. G00 non-interpolation Normal line control is not applied. Polar coordinate interpolation This cannot be commanded during normal line control. Program error (P486) will occur. The normal line control command during polar coordinate interpolation cannot be issued either. Program error (P481) will occur. Exponential interpolation If the normal line control axis is the same as the rotary axis of exponential interpolation, a program error (P612) will occur. If they are different, an error will not occur, but normal line control is not applied. Plane selection This cannot be commanded during normal line control. Program error (P903) will occur. Mixed control This cannot be commanded during normal line control. An operation error (M01 1035) will occur. System variable The block end coordinate (#5001 - ) for the normal line control axis during normal line control cannot obtain a correct axis position. Precautions (1) During normal line control, the program coordinates are updated following the normal line control axis movement. Thus, program the normal line control on the program coordinate system. (2) The normal line control axis will stop at the turning start position for the single block, cutting block start interlock and block start interlock. (3) If the movement command is issued to the normal line control axis (C axis) during normal line control, it is ignored. (4) The coordinate system preset command (G92 C_;) cannot be issued to the normal line control axis during C axis normal line control (during G41.1 or G42.1 modal). The program error (P901) will occur if commanded. (5) When a mirror image is applied to the axis in plane selection mode, normal line control is carried out for the shape processed with the mirror image. (6) The rotary axis must be designated as the normal line control axis (parameter "#1522 C_axis"). Designate so that the axis is not duplicated with the axis on the plane where normal line control is to be carried out. If an illegal axis is designated, the program error (P902) will occur when the program (G40.1, G41.1, G42.1) is commanded. The program error (P902) will also occur if the parameter "#1522 C_axis" is "0" when commanding a program. This parameter setting depends on the MTB specifications. (7) The movement of the normal line control axis is counted as one axis of number of simultaneous contouring control axes. If the number of simultaneous contouring control axes exceeds the specification range by movement of the normal line control axis, the program error (P10) will occur. 485 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.8 Manual Arbitrary Reverse Run Prohibition ; G127 Function and purpose The manual arbitrary reverse run function controls the feedrate, which is under automatic operation in memory or MDI mode, in proportion to the manual feedrate by the jog or the rotation speed by the manual handle, and manually carries out the reverse run. After the automatic operation has been stopped in a block, the reverse run can be carried out back through the blocks (up to 20 blocks) that were executed before the block. If necessary, it is possible to correct the program buffer and execute the fixed program after carrying out the reverse run up to the return position. This function (G127) is available to prevent the program from backing to blocks before the commanded block when carrying out the manual arbitrary reverse run. The detailed setting and operation vary depending on the machine specifications. Refer to the Instruction Manual issued by the MTB. "Forward run" means to execute blocks in the same order as for the automatic operation. "Reverse run" means to process the executed blocks backward. Whether the reverse run is prohibited for each part system depends on the MTB specifications (system variable #3004). Refer to "List of System Variables" for details. Command format All part system reverse run prohibit command G127 ; This command disables the program from running reverse to blocks before G127. In part systems that do not have this command executed, the program cannot run reverse before the timing with G127 commanded in any part system even if a block is in process. No commands in the machining program can be backed in the reverse run mode. For some G codes, the operation differs from the above. Refer to "Relationship with Other Functions". $1 G127 $2 $3 $4 The reverse run is disabled before the G127 block in the 2nd part system. The reverse run is canceled in the middle of a block in part systems other than the 2nd part system. IB-1501278-D 486 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Relationship with other functions The following shows the relationship between the manual arbitrary reverse run command and G code. Symbol in "Reverse run" column Operation ○ *1 Block with reverse run enabled ○ *2 Block with restricted-reverse run enabled Refer to the Remarks for restrictions. ∆ Block with reverse run ignored. This block is ignored in both the forward and reverse run modes. × *3 Block with reverse run prohibited. This is intended only for the command blocks. × *4 Block with reverse run prohibited. The reverse run is also prohibited for all blocks after the mode has been switched by this block. × *5 Prohibits the reverse run in all part systems. G Code G00 Function name Reverse run Remarks Positioning ○ *1 - G01 Linear interpolation ○ *1 - G02 Circular interpolation CW and spiral/conical × *3 interpolation CW (type2) - G03 Circular interpolation CCW and spiral/coni- × *3 cal interpolation CCW (type2) - G02.3 Exponential interpolation CW × *3 - G03.3 Exponential interpolation CCW × *3 - G02.4 3-dimensional circular interpolation × *3 - G03.4 3-dimensional circular interpolation × *3 - G04 Dwell ○ *1 Dwell skip is invalid. G05 High-speed high-accuracy control II/III / High-speed machining mode × *4 - G05.1 High-speed high-accuracy control I / Spline × *4 - G06.2 NURBS interpolation × *4 - G07 Hypothetical axis interpolation × *3 - G07.1 G107 Cylindrical interpolation × *4 - G08 High-accuracy control × *4 - G09 Exact stop check ○ *1 - G10 Program data input (Parameter / Compen- ∆ sation amount / Coordinate rotation by parameter data) / Life management data registration The reverse run is enabled, but data is not recovered. G10.6 Tool retract command × *3 - G11 Program parameter input / cancel ∆ The reverse run is enabled, but data is not recovered. G12 Circular cutting CW × *3 - G13 Circular cutting CCW × *3 - G12.1 G112 Polar coordinate interpolation ON × *4 - G13.1 G113 Polar coordinate interpolation cancel × *4 - G15 Polar coordinate command OFF × *4 - G16 Polar coordinate command ON × *4 - G17 X-Y plane selection ○ *2 Data is recovered using the modal information storage block. 487 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions G Code Function name Reverse run Remarks G18 Z-X plane selection ○ *2 Data is recovered using the modal information storage block. G19 Y-Z plane selection ○ *2 Data is recovered using the modal information storage block. G20 Inch command ○ *1 Switched with the movement command just after commanded. G21 Metric command ○ *1 Switched with the movement command just after commanded. G22 Stroke check before travel ON × *3 - G23 Stroke check before travel OFF × *3 - G27 Reference position check × *3 - G28 Automatic reference position return × *3 - G29 Start position return × *3 - G30 2nd, 3rd and 4th reference position return × *3 - G30.1 Tool change position return 1 × *3 - G30.2 Tool change position return 2 × *3 - G30.3 Tool change position return 3 × *3 - G30.4 Tool change position return 4 × *3 - G30.5 Tool change position return 5 × *3 - G30.6 Tool change position return 6 × *3 - G31 Skip/Multi-step skip function 2 × *3 - G31.1 Multi-step skip function 1-1 × *3 - G31.2 Multi-step skip function 1-2 × *3 - G31.3 Multi-step skip function 1-3 × *3 - G33 Thread cutting ○ *2 The reverse run is enabled, but the synchronous feed is invalid. Actual cutting mode available. G34 Special fixed cycle (bolt hole circle) × *4 - G35 Special fixed cycle (write at angle) × *4 - G36 Special fixed cycle (arc) × *4 - G37 Automatic tool length measurement × *3 - G37.1 Special fixed cycle (grid) × *4 - G38 Tool radius compensation vector designa- × *3 tion - G39 Tool radius compensation corner arc - G40 Tool radius compensation cancel / 3-dimen- ○ *2 sional tool radius compensation cancel Data is recovered using the modal information storage block. G41 Tool radius compensation left / 3-dimensional tool radius compensation left ○ *2 Data is recovered using the modal information storage block. G42 Tool radius compensation right / 3-dimensional tool radius compensation right ○ *2 Data is recovered using the modal information storage block. G40.1 G150 Normal line control cancel × *4 - G41.1 G151 Normal line control left ON × *4 - G42.1 G152 Normal line control right ON × *4 - G43 Tool length compensation (+) ○ *2 Data is recovered using the modal information storage block. G44 Tool length compensation (-) ○ *2 Data is recovered using the modal information storage block. G43.1 Tool length compensation along the tool axis × *3 - IB-1501278-D × *3 488 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions G Code G43.4 Function name Reverse run Tool center point control type1 ON × *4 Remarks - G43.5 Tool center point control type2 ON × *4 - G45 Tool position offset (expansion) ○ *2 Data is recovered using the modal information storage block. G46 Tool position offset (reduction) ○ *2 Data is recovered using the modal information storage block. G47 Tool position offset (double) ○ *2 Data is recovered using the modal information storage block. G48 Tool position offset (decreased by half) ○ *2 Data is recovered using the modal information storage block. G49 Tool length compensation cancel / Tool cen- ○ *1/ ter point control cancel × *3 If tool length compensation cancel is designated, reverse running is enabled. G50.2 Scaling cancel × *4 - G51.2 Scaling ON × *4 - G50.1 Mirror image by G code cancel × *3 - G51.1 G command mirror image ON × *3 - G52 Local coordinate system setting ○ *2 Data is recovered using the modal information storage block. G53 Machine coordinate system selection ○ *2 Data is recovered using the modal information storage block. G54 Workpiece coordinate system 1 selection ○ *2 Data is recovered using the modal information storage block. G55 Workpiece coordinate system 2 selection ○ *2 Data is recovered using the modal information storage block. G56 Workpiece coordinate system 3 selection ○ *2 Data is recovered using the modal information storage block. G57 Workpiece coordinate system 4 selection ○ *2 Data is recovered using the modal information storage block. G58 Workpiece coordinate system 5 selection ○ *2 Data is recovered using the modal information storage block. G59 Workpiece coordinate system 6 selection ○ *2 Data is recovered using the modal information storage block. G54.1 Workpiece coordinate system selection 48 ○ *2 / 96 sets extended Data is recovered using the modal information storage block. G60 Unidirectional positioning × *3 - G61 Exact stop check mode ○ *1 - G61.1 High-accuracy control ON × *4 - G61.2 High-accuracy spline × *4 - G62 Automatic corner override ○ *1 - G63 Tapping mode ○ *1 - G63.1 Synchronous tapping mode (Forward tapping) × *4 - G63.2 Synchronous tapping mode (Reverse tapping) × *4 - G64 Cutting mode ○ *1 - G65 Macro call Simple call ○ *1 - G66 User macro Modal call A ○ *1 - G66.1 User macro Modal call B ○ *1 - G67 User macro Modal call cancel ○ *1 - G68 Coordinate rotation by program mode ON / × *4 3-dimensional coordinate conversion mode ON - G68.2 Inclined surface machining command - 489 × *3 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions G Code Function name Reverse run Remarks G68.3 Inclined surface machining command (Based on tool axis direction) × *3 - G69 Coordinate rotation by program mode can- × *4 cel / 3-dimensional coordinate conversion mode cancel / Inclined surface machining command cancel - G70 User fixed cycle × *3 - G71 User fixed cycle × *3 - G72 User fixed cycle × *3 - G73 Fixed cycle (step) ○ *1 Data is created for each movement block in the fixed cycle. G74 Fixed cycle (reverse tap) ○ *2 The reverse run is enabled, but the synchronous feed is invalid. Actual cutting mode available. G75 Fixed cycle (circular cutting cycle) ○ *1 Data is created for each movement block in the fixed cycle. G76 Fixed cycle (Fine boring) ○ *1 Data is created for each movement block in the fixed cycle. G77 User fixed cycle × *3 - G78 User fixed cycle × *3 - G79 User fixed cycle × *3 - G80 Fixed cycle for drilling cancel ○ *1 - G81 Fixed cycle (drill/spot drill) ○ *1 Data is created for each movement block in the fixed cycle. G82 Fixed cycle (drill/counter boring) ○ *1 Data is created for each movement block in the fixed cycle. G83 Fixed cycle (deep drilling) ○ *1 Data is created for each movement block in the fixed cycle. G84 Fixed cycle (tapping) ○ *2 The reverse run is enabled, but the synchronous feed is invalid. Actual cutting mode available. G85 Fixed cycle (boring) ○ *1 Data is created for each movement block in the fixed cycle. G86 Fixed cycle (boring) ○ *1 Data is created for each movement block in the fixed cycle. G87 Fixed cycle (back boring) ○ *1 Data is created for each movement block in the fixed cycle. G88 Fixed cycle (boring) ○ *1 Data is created for each movement block in the fixed cycle. G89 Fixed cycle (boring) ○ *1 Data is created for each movement block in the fixed cycle. G90 Absolute value command ○ *2 Switched with the movement command just after commanded. G91 Incremental value command ○ *2 Switched with the movement command just after commanded. G92 Coordinate system setting ○ *1 - G92.1 Workpiece coordinate preset ○ *1 - G93 Inverse time feed ○ *1 - G94 Asynchronous feed (feed per minute ) ○ *1 - G95 Synchronous feed (feed per revolution) ○ *1 - G96 Constant surface speed control ON ○ *2 Switched with the movement command just after commanded. G97 Constant surface speed control OFF ○ *2 Switched with the movement command just after commanded. IB-1501278-D 490 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions G Code Function name Reverse run Remarks (G94) Asynchronous feed (feed per minute ) ○ *1 - (G95) Synchronous feed (feed per revolution) ○ *1 - G98 Fixed cycle (Initial level return) ○ *1 - G99 Fixed cycle R point level return ○ *1 - G115 Start point designation synchronization Type 1 ○ *1 - G116 Start point designation synchronization Type 2 ○ *1 - G118.2 Parameter switching (Spindle) × *3 - G119.2 Inertia Estimation (Spindle) × *3 - G100 to G225 User macro (G code call) Max. 10 ○ *1 - M98 Subprogram call ○ *1 - 491 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.9 Data Input by Program 15.9.1 Parameter Input by Program ; G10 L70/L100, G11 Function and purpose The parameters set from the setting and display unit can be changed in the machining programs. G10 L70 For commanding data with decimal point, and character string data. The data's command range conforms to the parameter setting range described in Setup Manual. G10 L100 For setting/changing the tool shape for 3D solid program check. Command format Data setting start command G10 L70 ; P__ S__ A__ H□__ ; Bit parameter P__ S__ A__ D__ ; Numerical value parameter P__ S__ A__ <character string> ; Character string parameter P Parameter No. S Part system No. A Axis No. H Bit type data D Numeric type data character string Character string data Data setting end command G11 ; Note (1) The sequence of addresses in a block must be as shown above. When an address is commanded two or more times, the last command will be valid. (2) The part system No. is set in the following manner. "1" for the 1st part system, "2" for 2nd part system, and so forth. If the address S is omitted, the part system of the executing program will be applied. As for the parameters common to part systems, the command of part system No. will be ignored. (3) The axis No. is set in the following manner. "1" for 1st axis, "2" for 2nd axis, and so forth. If the address A is omitted, the 1st axis will be applied. As for the parameters common to axes, the command of axis No. will be ignored. (4) Address H is commanded with the combination of setting data (0 or 1) and the bit designation □ (0 to 7). Hd0: Sets the dth bit OFF. (d: 0 to 7) Hd1: Sets the dth bit ON. (d: 0 to 7) (5) Only the decimal number can be commanded with the address D. The value that is smaller than the input setting increment (#1003 iunit) will be round off to the nearest increment. (6) The character string must be put in angled brackets "<" and ">". If these brackets are not provided, the program error (P33) will occur. Up to 63 characters can be set. IB-1501278-D 492 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (7) Issue "G10 L70" and "G11" commands in independent blocks. A program error (P33, P421) will occur if not commanded in independent blocks. (8) The parameter "#1078 Decimal pnt type 2" is disabled. (9) The following data cannot be changed with the G10 L70 command: Tool compensation data, workpiece coordinate data, PLC switch, and PLC axis parameter. (10) The settings of the parameters with (PR) in the parameter list will be enabled after the power is turned OFF and ON. Refer to the parameter list in your manual. Data setting start command G10 L100 ; P__ T__ K__ D__ H__ I__ J__ C__ ; Data setting end command G11 ; P Line No. of the tool set area 1 to 80 (Required to command) (*1) T Tool No. 0 to 99999999 (Required to command) K Command the tool type using a numerical value. 0: Default tool (3: Sets to drill.) 1: Ball end mill 2: Flat end mill 3: Drill 4: Bull nose end mill 5: Chamfer 6: Tap 7: Face mill D Tool diameter/radius (Decimal point input available) (*2) H Tool length (Decimal point input available) I Tool shape data 1 (Decimal point input available) J Tool shape data 2 (Decimal point input available) C Command the tool color using a numerical value. 0: Default color (2: Sets to red.) 1: Gray 2: Red 3: Yellow 4: Blue 5: Green 6: Light blue 7: Purple 8: Pink (*1) Line No. corresponds with a line No. in the tool shape set area (tool shape set screen). (*2) The setting of "#8117 OFS Diam DESIGN" determines tool diameter or tool radius. (*3) For details of the data, refer to the explanation of Instruction Manual "Program Check (3D)". (*4) Omitted addresses cannot be set or changed. (*5) When address T is set to 0, the designated line is deleted. (*6) In the following cases, the program error (P421) occurs and the parameter in the block is not changed. When a block contains an address whose data are out of range When there is an illegal address When P or T is omitted (*7) Issue G10 L70/L100 and G11 commands in independent blocks. A program error (P421) will occur if not commanded in independent blocks. (*8) The parameter "#1078 Decimal pnt type 2" is enabled. (*9) The parameter "#8044 Unit*10" is disabled. (*10) The display or operation at graphic check varies depending on the model or display unit. 493 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Precautions Parameter update timing The timing for updating the spindle parameter and the NC axis parameter settings depends on the MTB specifications (parameter "#1254 set26/bit3"). #1254 set26/bit3 Spindle parameter NC axis parameter Invalid The program updates the parameter settings, waiting for "all axes smoothing zero" in all part systems. Valid The program updates the parameter settings without waiting for "smoothing zero". (*1) The program updates the parameter settings, waiting for "all axes smoothing zero" in control part systems. (*2) (*1) The parameters of the target spindle are not updated while the functions below are active. The parameters are updated after the functions have been completed. Synchronous tapping cycle The spindle for spindle position control is in C axis mode and the C axis is in motion. (*2) The program updates the exchange axis under the arbitrary axis exchange control, waiting for "all axes smoothing zero" in all part systems. Program example (1) For G10 L70 G10 L70 ; P6401 H71 ; Sets "1" to "#6401 bit7". P8204 S1 A2 D1.234 ; Sets "1.234" to "#8204 of the 1st part system 2nd axis". P8621 <X> ; Sets "X" to "#8621". G11 ; (2) When G10 L100 command G10 L100; P1 T1 K3 D5. H20. I0 J0 C2 ; Set the data of Line 1 P2 T10 D10. ; Set "10." for the tool diameter/radius of Line 2 P8 T0 ; Clear the data of Line 8 G11 ; IB-1501278-D 494 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.9.2 Compensation Data Input by Program ; G10 L2/L10/L11/L12/L13/L20, G11 Function and purpose The tool compensation and workpiece offset can be set or changed by the program using the G10 command. During the absolute value (G90) mode, the commanded offset amount serves as the new offset, whereas during the incremental value (G91) mode, the currently set offset plus the commanded offset serves as the new offset. Command format Workpiece coordinate system offset input (L2) G90 (G91) G10 L2 P_ X_ Y_ Z_ ; P 0 : External workpiece 1 : G54 2 : G55 3 : G56 4 : G57 5 : G58 6 : G59 X, Y, Z Offset amount of each axis Note (1) The compensation amount in the G91 will be an incremental amount and will be cumulated each time the program is executed. Command G90 or G91 before the G10 as a cautionary means to prevent this type of error. Extended workpiece coordinate system offset input (L20) G10 L20 P_ X_ Y_ Z_ ; P n No. of G54.n (1 to 300) X, Y, Z Offset amount of each axis Offset input to the currently selected workpiece coordinate system (When the L command is omitted) G10 P_ X_ Y_ Z_ ; P (1) During G54 to G59 modal 0 : External workpiece offset (EXT) 1 to 6 : Workpiece offset input (G54 to G59) Other than 0 to 6 : Program error (P35) (2) During G54.n modal X, Y, Z 1 to 300 : Extended workpiece coordinate offset amount setting (G54.n) Other than 1 to 300 : Program error (P35) Offset amount of each axis 495 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Tool compensation input (L10/L11/L12/L13) Tool compensation memory type I G10 L10 P_ R_ ; P Compensation No. R Compensation amount Tool compensation memory type II G10 L10 P_ R_ ; Tool length compensation shape compensation G10 L11 P_ R_ ; Tool length compensation wear compensation G10 L12 P_ R_ ; Radius shape compensation G10 L13 P_ R_ ; Radius wear compensation Note (1) Type I is selected when parameter "#1037 cmdtyp" is set to "1", and type II is selected when set to "2". Compensation input cancel G11 ; Common to workpiece coordinate system offset, extended workpiece coordinate system offset, and tool compensation. IB-1501278-D 496 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Detailed description (1) Even if this command is displayed on the screen, the offset No. and variable details will not be updated until actually executed. (2) G10 is an unmodal command and is valid only in the commanded block. (3) The G10 command does not contain movement, but must not be used with G commands other than G54 to G59, G90 or G91. (4) Do not command G10 in the same block as the fixed cycle and sub-program call command. This will cause malfunctioning and program errors. (5) The workpiece offset input command (L2 or L20) should not be issued in the same block as the tool compensation input command (L10). (6) If an illegal L No. or compensation No. is commanded, the program errors (P172 and P170) will occur respectively. If the offset amount exceeds the maximum command value, the program error (P35) will occur. (7) Decimal point inputs can be used for the offset amount. (8) The offset amounts for the external workpiece coordinate system and the workpiece coordinate system are commanded as distances from the basic machine coordinate system zero point. (9) The workpiece coordinate system updated by inputting the workpiece coordinate system will follow the previous modal (G54 to G59) or the modal (G54 to G59) in the same block. (10) L2/L20 can be omitted when the workpiece offset is input. (11) When the P command is omitted for workpiece offset input, it will be handled as the currently selected workpiece compensation input. (12) If the G command that cannot be combined with G10 is issued in the same block, a program error (P45) will occur. (13) The setting range for the compensation amount is given below. Program error (P35) occurs for any value not listed in the table after command unit conversion. With an incremental value command, the setting range for the compensation amount is the sum of the present setting value and command value. Setting Compensation amount Metric system Inch system #1003=B ± 9999.999 (mm) ± 999.9999 (inch) #1003=C ± 9999.9999 (mm) ± 999.99999 (inch) #1003=D ± 9999.99999 (mm) ± 999.999999 (inch) #1003=E ± 9999.999999 (mm) ± 999.9999999 (inch) Program example (1) Input the compensation amount. ; G10 L10 P10 R-12.345 ; G10 L10 P05 R9.8765 ; G10 L10 P30 R2.468 ; H10=-12.345 H05=9.8765 H30=2.468 497 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (2) Updating of compensation amount (Example 1) Assume that H10 = -1000 is already set. N1 G01 G90 G43 Z-100000 H10 F100 ; (Z=-101000) N2 G28 Z0 ; N3 G91 G10 L10 P10 R-500 ; (The mode is the G91 mode, so -500 is added.) N4 G01 G90 G43 Z-100000 H10 ; (Z=-101500) (Example 2) Assume that H10 = -1000 is already set. Main program N1 G00 X100000 ; a N2 #1=-1000 ; N3 M98 P1111 L4 ; b1, b2, b3, b4 Subprogram O1111 N1 G01 G91 G43 Z0 H10 F100 ; c1, c2, c3, c4 G01 X1000 ; d1, d2, d3, d4 #1=#1-1000 ; G90 G10 L10 P10 R#1 ; M99 ; (b1) c1 d1 (b2) (b3) (b4) c2 d2 c3 d3 c4 d4 1000 1000 1000 1000 (a) 1000 1000 1000 1000 <Note> Final offset amount will be H10= -5000. (Example 3) The program for Example 2 can also be written as follows. Main program N1 G00 X100000 ; N2 M98 P1111 L4 ; Subprogram O1111 N1 G01 G91 G43 Z0 H10 F100 ; N2 G01 X1000 ; N3 G10 L10 P10 R-1000 ; N4 M99 ; IB-1501278-D 498 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (3) When updating the workpiece coordinate system offset amount Assume that the previous workpiece coordinate system offset amount is as follows. X=-10.000 Y=-10.000 N100 G00 G90 G54 X0 Y0 ; N101 G90 G10 L2 P1 X-15.000 Y-15.000 ; N102 X0 Y0 ; M02 ; -X - 20. M - 10. Basic machine coordinate system zero point N100 -X N101 (W1) - 10. G54 coordinate before change N102 -X W1 G54 coordinate after change -Y - 20. -Y -Y <Note> Changes of workpiece current position display in N101 The G54 workpiece position display data will change before and after the workpiece coordinate system is changed with G10 in N101. → X = +5.000 X=0 Y=0 Y = +5.000 When workpiece coordinate system offset amount is set in G54 to G59 G90 G10 L2 P1 X-10.000 Y-10.000 ; G90 G10 L2 P2 X-20.000 Y-20.000 ; G90 G10 L2 P3 X-30.000 Y-30.000 ; G90 G10 L2 P4 X-40.000 Y-40.000 ; G90 G10 L2 P5 X-50.000 Y-50.000 ; G90 G10 L2 P6 X-60.000 Y-60.000 ; 499 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (4) When using one workpiece coordinate system as multiple workpiece coordinate systems Main program : #1=-50. #2=10. ; M98 P200 L5 ; M02 ; % Sub program O200 N1 G90 G54 G10 L2 P1 X#1 Y#1 ; N2 G00 X0 Y0 ; N3 X-5. F100 ; N4 X0 Y-5. ; N5 Y0 ; N6 #1=#1+#2 ; N7 M99 ; % -X - 60. - 50. - 40. - 30. - 20. G54'' '' W G54'' ' W G54'' G54' G54 W W M - 10. W - 10. Basic machine coordinate system zero point 5 - 20. 4 - 30. 3 - 40. 2 - 50. 1 -Y Precautions (1) Even if this command is displayed on the screen, the offset No. and variable details will not be updated until actually executed. N1 G90 G10 L10 P10 R-100 ; N2 G43 Z-10000 H10 ; N3 G00 X-10000 Y-10000 ; N4 G90 G10 L10 P10 R-200 ; IB-1501278-D The H10 offset amount is updated when the N4 block is executed. 500 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.9.3 Compensation Data Input by Program (Turning Tool) ; G10 L12/L13, G11 Function and purpose If the tool compensation type is changed to type III by the compensation type selection function, it is possible to write the offset amount for three base axes, nose R compensation amount, and tool nose point (parameter "#1046 T-ofs disp type"). During the absolute value (G90) mode, the commanded tool compensation amount serves as a new one. During the incremental value (G91) mode, the currently set compensation amount plus the commanded compensation amount serves as the new compensation amount. Command format Turning tool compensation input (L12/L13) G10 L12 P__ X__ Y__ Z__ R__ Q__ ; (Shape compensation) P Tool shape compensation No. (1 to number of tool compensation sets) X, Y, Z Compensation amount for each axis R Nose R compensation amount Q Hypothetical tool nose point G10 L13 P__ X__ Y__ Z__ R__ Q__ ; (Wear compensation) P Wear compensation No. (1 to number of tool compensation sets) X, Y, Z Compensation amount for each axis R Nose R compensation amount Q Hypothetical tool nose point Compensation input cancel G11 ; 501 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Detailed description The commanded range and unit of the compensation amount are as follows. Program error (P35) occurs for any value not listed in the table after command unit conversion. With an incremental value command, the commanded range for the compensation amount is the sum of the present setting value and command value. Setting Compensation amount Metric system Inch system #1003=B ± 9999.999 (mm) ± 999.9999 (inch) #1003=C ± 9999.9999 (mm) ± 999.99999 (inch) #1003=D ± 9999.99999 (mm) ± 999.999999 (inch) #1003=E ± 9999.999999 (mm) ± 999.9999999 (inch) Precautions (1) The X, Y, and Z addresses are set to the axis names specified in the parameters for three base axes (parameters “#1026 base_I”, “#1027 base_J”, and “#1028 base_K”). The compensation data input by program of the tool offset is not available for an axis address that is not specified in the parameters for three base axes. Therefore, be sure to carry out compensation data input by program after specifying the parameters for three base axes. (2) The compensation data input by program is available using a command (G10 L10, L11, L12, or L13) in a normal machining center system, but only the compensation amount of the Z axis and nose R can be input as data. IB-1501278-D G10 L10 P__ R__; Z axis shape compensation G10 L11 P__ R__; Z axis wear compensation G10 L12 P__ R__; Nose R shape compensation G10 L13 P__ R__; Nose R wear compensation 502 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.9.4 Tool Shape Input by Program ; G10 L100, G11 Function and purpose This function sets tool shape data of the tool management screen by the machining program. Using this function saves having to execute the many steps required to input the tool shape from the screen when executing 3D checks. Command format Tool shape settings from the program G10 L100; Data setting start command P_ T_ K_ D_ H_ I_ J_ C_ ; Data setting command P Data No. Specify the data No. on the tool management screen. (Cannot be omitted.) The maximum value of data No. varies depending on the number of tool management data sets. T Tool No. Specify the tool No. (Cannot be omitted.) 0 to 99999999 When "0" is specified, all the tool shape data of data No. specified by address P will be "0". In this case, only the tool shape data is changed. K Type Designate the tool type using a numerical value. [Mill tool] 1: Ball end mill 2: Flat end mill 3: Drill 4: Radius end mill 5: Chamfer 6: Tap 7: Face mill [Turning tool] 51: Turning 52: Slotting 53: Thread cutting 54: Turning drill 55: Turning tap D Shape data 1 H Shape data 2 I Shape data 3 Designate shape data of the tool. (Decimal point input enabled) The setting details of shape data differ depending on the tool type. J Shape data 4 Refer to the following "Correspondence between tool types and shape data" for the settings for each tool type. C Tool color Specify the tool color. G11; 1: Gray 2: Red 3: Yellow 4: Blue 5: Green 6: Light blue 7: Purple 8: Pink Data setting end command 503 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions [Correspondence between tool types and shape data] [Mill tool] Shape data Item by tool type Ball end mill Flat end mill Drill Radius end mill Chamfer 1 Tool length 2 Tool radius (*1) Tap Face mill 3 - - Tool nose angle Corner rounding End angle Pitch Cutter length 4 - - - - End diame- Thread diter ameter Shank diameter 5 - - - - - - - 6 - - - - - - - [Turning tool] Shape data Item by tool type Turning Slotting Thread cutting 1 Turning drill Turning tap Tool length A 2 Tool length B Tool length B (*1) 3 Tool nose radius Tool nose radius - 4 Tool nose angle Tool nose width - - Thread diameter 5 Cutting edge an- Max. slot depth gle - - - 6 Tool width Tool width - - Tool width Tool nose angle Pitch (*1) When "#8968 Tool shape radius validity" is set to "0", input the diameter value. When it is set to "1", input the radius value. Note (1) Omitted addresses cannot be set. (2) If address "P" or "T" is omitted, a program error (P422) will occur. (3) For M80 Series, the tool shape data will be rewritten during the graphic check. (4) For M800W and M800S Series, this change is only reflected on the graphic check drawing. The tool shape data is not rewritten. IB-1501278-D 504 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Detailed description Tool shape settings from the program The 3D check switches the drawing of tools at the timing of a tool change command. Therefore, the machining program should be prepared to run a tool shape setting command prior to the tool change command being issued. Machining program Tool shape data O200 Tool A G10 L100; P1 T201 ...; (Change the shape of tool A.) P3 T203 ...; (Newly register the shape of Tool B G11; Tool management screen Tool C tool C.) (a) T201; (Replaced with tool A.) 3D check screen (b) T202; (Replaced with tool B.) (c) T203; (Replaced with tool C.) (a) The tool is drawn with the shape that has been changed by the machining program. (b) The tool is drawn with a shape that has been registered on the tool management screen. (c) The tool is drawn with a new shape that has been registered by the machining program. Program example (1) Tool shape settings from the program G10 L100 ; P1 T1 K3 D5. H20. I0 J0 C2 ; Sets the data of data No. 1. P2 T10 D10. ; Sets the tool diameter of data No. 2 to "10.". P8 T0 ; Sets the tool shape data of data No. 8 to "0". G11; Precautions (1) If the G10 or G11 command is not issued in an independent block, a program error (P422) will occur. (2) If a block contains an address whose data is out of range, a program error (P35) will occur. (3) If a block contains an illegal address, a program error (P32) will occur. (4) The parameter "#1078 Decimal pnt type 2" is valid for the position command. Other command addresses comply with the minimum input unit ("#1015 cunit"). (Based on the MTB specifications.) (5) The parameter "#8044 UNIT*10" is invalid. (6) The command unit of parameters to be input in mm/inch can be switched by G20/G21. 505 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.9.5 R-Navi Data Input by Program ; G10 L110, G11, G68.2, G69 Function and purpose The R-Navi setup parameters can be configured from a machining program. Command setting values with absolute values. The input unit conforms to the input setting unit of the 1st part system and the initial inch. In either case, the input unit depends on the MTB specifications (parameters "#1003 iunit" and "#1041 I_inch"). The parameter "#8044 UNIT*10" is invalid. Command format Workpiece registration and setting G69; Canceling the selected machining surface G10 L110 ; Start setting workpiece data Q_ <_> F_ C_ R_ X_ Y_ Z_ I_ J_ K_; Data setting G11; End data setting Command G10 and G11 in independent blocks. A program error (P423) will occur if not commanded in independent blocks. Address Q cannot be omitted. If omitted, a program error (P423) will occur. For the omitted addresses, data remains unchanged. Cancel the selected machining surface before data setting. If data is set to a machining workpiece including the selected machining surface, a program error (P423) will occur. Q Workpiece registration No.(1 to 10) <> Workpiece name Designate the name using up to 20 one-byte alphanumeric characters, including symbols. (If "0" is entered, the setting value is cleared.) F Workpiece shape 0: Rectangular parallelepiped 1: Circular cylinder C Basic coordinate system of machining workpiece 0 to 5: G54 to G59 6 to 305: G54.1P1 to G54.1P300 R Marked point No. When the workpiece shape is set to rectangular parallelepiped, designate the marked point to set the basic coordinate system zero point. (0 to 8) X, Y, Z, Workpiece size When the shape is set to circular cylinder, designate the diameter with X and the height with Y. (0.000 to 99999.999) I, J, K Workpiece shift Set the shift amount from the marked point to the basic coordinate system zero point. (-99999.999 to 99999.999) IB-1501278-D 506 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Symbols "\", "/", ",", "*", "?", """, "<", ">", "|", " " (space), “@”, and “~” cannot be used as one-byte symbols. If an available symbol is set, a program error (P35) or (P32) will occur. For details on each of input data, refer to the instruction manual. Machining surface registration and setting G69; Canceling the selected machining surface G10 L111 ; Start setting machining surface data P0 Q_ D_ <_> X_ Y_ Z_ A_; P1 M_ B_ C_ E_ F_ H_ I_; P2 M_ B_ C_ E_ F_ H_ I_; Machining surface setting (Refer to (1).) Designate the coordinate axis direction (1st axis). (Refer to (2).) Designate the coordinate axis direction (2nd axis). (Refer to (2).) G11; End data setting G68.2 P10 Q__ D__ ; Selecting the registered machining surface Command G10 and G11 in independent blocks. A program error (P423) will occur if not commanded in independent blocks. Addresses P, Q, and D cannot be omitted. If omitted, a program error (P423) will occur. For the omitted addresses, data remains unchanged. For the machining surface designated with P0, set the coordinate axis direction with P1 and P2. Be sure to first command P0. If P1 or P2 is commanded before P0, a program error (P423) will occur. The machining surface cannot be registered for an undefined workpiece. If the registration command is issued, a program error (P423) will occur. Cancel the selected machining surface before data setting. If data is set to the selected machining surface, a program error (P423) will occur. (1) Command address to register the machining surface P Machining surface registration (0) Q Workpiece registration No. (1 to 10) D Machining surface registration No. (2 to 17) <> Designate the name of the machining surface using up to 15 one-byte alphanumeric characters, including symbols. (If "0" is entered, the setting value is cleared.) X, Y, Z Designate the coordinate system zero point (feature coordinate system zero point) of the machining surface with the offset from the basic coordinate zero point. In this case, designate the coordinate axis direction of the basic coordinate system. (-99999.999 to 99999.999) A From three orthogonal axes (X, Y, and Z axes), select two coordinate axes to designate the coordinate axis direction along the machining surface. 0: Z/X axis 1: Y/Z axis 2: X/Y axis Symbols "\", "/", ",", "*", "?", """, "<", ">", "|", " " (space), “@”, and “~” cannot be used as one-byte symbols. If an available symbol is set, a program error (P35) or (P32) will occur. For details on each of input data, refer to the instruction manual. 507 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (2) Command address to designate the coordinate axis direction P Coordinate axis direction designation axis 1: 1st axis 2: 2nd axis M Coordinate axis direction designation method Designate the method to set the coordinate axis direction along the machining surface. 0: [Method 1] On-axis point (+) 1: [Method 2] Latitude/Longitude 2: [Method 3] Latitude / Projection angle 3: [Method 4] Start point / End point 4: [Method 5] Indexing angle (Z axis direction only) B, C, E, F, H, I Coordinate axis direction setting (*1) (-99999.999 to 99999.999) (*1) The setting details vary depending on the coordinate axis direction designation method (M address). [M address: 0 (On-axis point (+))] B, C, E: Coordinate value on X, Y, or Z axis F to I: Vacuous [M address: 1 (Latitude/Longitude)] B: Latitude (θ1) C: Longitude (θ2) E to I: Vacuous [M address: 2 (Latitude / Projection angle)] B: Latitude (θ1) C: Projection angle (θ2) E to I: Vacuous [M address: 3 (Start point / End point)] B: Start point coordinate value (X) C: Start point coordinate value (Y) E: Start point coordinate value (Z) F: End point coordinate value (X) H: End point coordinate value (Y) I: End point coordinate value (Z) [M address: 4 (Indexing angle)] B: 1st rotation angle (θ1) C: 2nd rotation angle (θ2) E to I: Vacuous Method 5 (indexing angle) in the coordinate axis direction designation method is only available in the Z axis direction. If a command is issued to an axis other than the Z axis designated by the coordinate axis selection command (P0Ax), a program error (P423) will occur. P0 A0 (Z/X axis) P0 A1 (Y/Z axis) P0 A2 (X/Y axis) P2 M4 setting causes an error. (Method 5 is not able to be selected on the 2nd axis.) P1M4 or P2M4 setting causes an error. (Method 5 is not able to be selected.) For details on each of input data, refer to the instruction manual. IB-1501278-D 508 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Operation example This function enables the R-Navi setup parameters to be configured from a machining program. After the parameters have been configured from the program, you can check the values or select the machining surface from the setup screen. Machining program O200 Canceling the selected machining surface G69; (Setting of workpiece) G10 L110; Q1 <WORK1> F0 C0 R1 X50.0 Y30.0 Z20.0 I0.0 J0.0 K0.0 ; Q2 <WORK2> F0 C0 R5 X50.0 Y30.0 Z20.0 I-10.0 J-5.0 K-40.0 ; ... G11; (Setting the machining surface) G10 L111; (Workpiece : 1, surface : 2) P0 Q1 D2 <SURFACE1_2> X50.0 Y-30.0 Z-20.0 A0; P1 M0 B1.0 C0.0 E1.732 F0.0 H0.0 I0.0; P2 M1 B90.0 C0.0 E0.0 F0.0 H0.0 I0.0; (Workpiece : 1, surface : 17) P0 Q1 D17 <SURFACE1_17> X20.0 Y20.0 Z10.0 A0; P1 M1 B0.0 C30.0 E0.0 F0.0 H0.0 I0.0; P2 M0 B0.0 C30.0 E0.0 F0.0 H0.0 I0.0; ... (Workpiece : 2, surface : 2) P0 Q2 D2 <SURFACE2_2> X20.0 Y20.0 Z10.0 A0; P1 M0 B1.0 C0.0 E1.732 F0.0 H0.0 I0.0; P2 M1 B90.0 C0.0 E0.0 F0.0 H0.0 I0.0; ... G11; Setup parameters WORK2 WORK1 BASE-SURFACE SURFACE1-2 Setup screen Restrictions (1) If the machining surface is selected or canceled while the block start interlock signal (*BSL) is turned OFF, an operation error (M01 0109) will occur. After this, if the block start interlock signal (*BSL) is turned ON, the machining surface is selected or canceled. The operation of the PLC signal depends on the MTB specifications. 509 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.10 Tool Life Management II ; G10 L3, G11 15.10.1 Allocation of The Number of Tool Life Management Sets to Part Systems Function and purpose The number of tool life management sets can be set per part system. This function is divided into following methods and which one is used depends on the MTB specifications (parameters "#1439 Tlife-SysAssign", "#12055 Tol-lifenum"). Arbitrary allocation: Arbitrarily allocates the number of tool life management sets to each part system. Fixed allocation: Automatically and evenly allocates the number of tool life management sets to each part system. The arbitrary allocation enables the efficient allocation because when a certain part system needs only a small number of tool life management sets, the rest can be allocated to another part system. If an auxiliary-axis part system does not need the tool life management sets at all, the number of tool life management sets can be set to "0" for the auxiliary-axis part system. Subsequent description is an example in the case where the number of tool life management sets in the system is 999 sets. (1) Arbitrary allocation (with #1439=1) The number of sets allocated to each part system depends on the MTB specifications (parameter "#12055 Tollifenum"). The following example shows the number of tool offset sets allocated when the lathe system is a 4-part system. (a) When the number of tool life management sets is increased for the 1st part system ($1) of 4-part system $1 250 $2 250 $3 250 $4 250 $1 400 $2 200 $3 200 $4 200 (b) When the number of tool life management sets is set to "0 sets" for the 3rd part system ($3) of 3-part system to use that part system as an auxiliary-axis part system IB-1501278-D $1 334 $2 333 $3 333 $1 500 $2 500 $3 0 510 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (2) Automatic and even allocation (with #1439=0) 1-part system 2-part system $1 $1 3-part system (Lathe system only) $1 500 999 (*1) $2 500 334 (*2) $2 333 $3 333 4-part system (Lathe system only) $1 250 $2 250 $3 250 $4 250 (*1)The maximum number of tool life management sets per part system is 999. (*2) If there is any remainder, the remainder is allocated to the 1st part system. Precautions (1) The maximum number of tool life management sets for 1-part system is 999. (2) For 1-part system, up to the number of tool life management sets in the system is available regardless of the parameter setting. (3) When the value of the parameter "#12055 Tol-lifenum" is equal to or lower than the number of tool life management sets in the system, the remainder is not allocated to any part system even if the specification allows arbitrary allocation. (4) When the value of the parameter "#12055 Tol-lifenum" is equal to or lower than the number of tool life management sets in the system, system alarm (Y05) is generated even if the specification allows arbitrary allocation. (5) Even if the specification allows arbitrary allocation, fixed allocation is applied if the parameter is "#12055 Tollifenum"= "0" for all part systems. (6) When entering data into the tool life management file, if the number of tool life management data exceeds that of current tool life management sets, the excess tool life management data cannot be entered. 511 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.11 Inputting The Tool Life Management Data ; G10,G11 15.11.1 Inputting The Tool Life Management Data by G10 L3 Command ; G10 L3,G11 Function and purpose Using the G10 command (unmodal command), the tool life management data can be registered, changed and added to, and preregistered groups can be deleted. There are three tool life management methods: I, II, and III. Which method is valid depends on the MTB specifications. Only group No. 1 can be used to register, change and add for the tool life management III. Command format Start of life management data registration G10 L3; P_ L_ Q_ ; (First group) T_ H_ D_; T_ H_ D_; P_ L_ Q_ ; (Next group ) T_ H_ D_; P Group No. L Life Q Control method T Tool No. The spare tools are selected in the order of the tool Nos. registered here. H Length compensation No. D Radius compensation No. Start of life management data change or addition G10 L3 P1; P_ L_ Q_ ; (First group) T_ H_ D_; T_ H_ D_; P_ L_ Q_ ; (Next group ) T_ H_ D_; P Group No. L Life Q Control method T Tool No. H Length compensation No. D Radius compensation No. IB-1501278-D 512 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Start of life management data deletion G10 L3 P2; P_ ; (First group) P_ ; (Second group) P Group No. End of life management data registration, change, addition or deletion G11 ; Detailed description Command range Item Command range Group No. (Pn) 1 to 99999999 (Only group No. 1 can be used for the tool life management III) Life (Ln) 0 to 65000 times (No. of times control method)0 to 4000 minutes (time control method) Control method (Qn) 1 to 3 1: Number of mounts control 2: Time control 3: Number of cutting times control Tool No. (Tn) 1 to 99999999 Length compensation No. (Hn) 0 to 999 (*) Radius compensation No. (Dn) 0 to 999 (*) (*) The setting range of the tool compensation No. differs according to the specification of the "number of tool offset sets". If a value exceeding each command range is issued, a program error (P35) will occur. 513 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Operation example Program example Operation Data registration G10 L3; P10 L10 Q1 ; T10 H10 D10 ; G11 ; M02 ; 1. After deleting all group data, the registration starts. 2. Group No. 10 is registered. 3. Tool No. 10 is registered in group No. 10. 4. The registration ends. 5. The program ends. Group change, addition G10 L3 P1; P10 L10 Q1 ; T10 H10 D10 ; G11 ; M02 ; 1. Changing and addition of the group and tool starts. 2. The change and addition operation takes place in the following manner. (1) When group No. 10 has not been registered.- Group No. 10 is additionally registered. - Tool No. 10 is registered in group No. 10. (2) When group No. 10 has been registered, but tool No. 10 has not been registered. - Tool No. 10 is additionally registered in group No. 10. (3) When group No. 10 and tool No. 10 have been both registered.- The tool No. 10 data is changed. 3. The group and tool change and addition ends. 4. The program ends. Group deletion G10 L3 P2; P10 ; G11 ; M02 ; 1. The group deletion starts. 2. The group No. 10 data is deleted. 3. The group deletion ends. 4. The program ends. IB-1501278-D 514 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.11.2 Inputting The Tool Life Management Data by G10 L30 Command ; G10 L30,G11 Function and purpose Using the G10 command (unmodal command), the tool life management data can be registered, changed and added to, and preregistered groups can be deleted. Only group No. 1 can be used to register, change and add for the tool life management III. To specify additional compensation amount or direct compensation amount by control method, the length compensation and diameter compensation can be registered/changed with the tool compensation amount format. Command format Start of life management data registration G10 L30; P_ L_ Q_ ; (First group) T_ H_ R_ ; T_ H_ R_ ; P_ L_ Q_ ; (Next group ) T_ H_ R_ ; P Group No. L Life Q Control method T Tool No. The spare tools are selected in the order of the tool Nos. registered here. H Length compensation No. or length compensation amount R Radius compensation No. or radius compensation amount L_, Q_, H_, and R_ cannot be omitted. If omitted, a program error (P33) occurs. Start of life management data change or addition G10 L30 P1; P_ L_ Q_ ; (First group) T_ H_ R_ ; T_ H_ R_ ; P_ L_ Q_ ; (Next group ) T_ H_ R_ ; P Group No. L Life Q Length compensation data format, radius compensation data format, control method T Tool No. H Length compensation No. or length compensation amount D Radius compensation No. or radius compensation amount L_, Q_, H_, and R_ cannot be omitted. If omitted, a program error (P33) occurs. 515 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Start of life management data deletion G10 L30 P2; P_ ; (First group) P_ ; (Second group) P Group No. End of life management data registration, change, addition or deletion G11 ; Detailed description Command range Item Command range Group No. (Pn) 1 to 99999999 (Only group No. 1 can be used for the tool life management III) Tool No. (Tn) 1 to 99999999 Control method (Qabc) abc:Three integer digits a. Tool length compensation data format 0: Compensation No. 1: Incremental value compensation amount 2: Absolute value compensation amount b. Tool radius compensation data format 0: Compensation No. 1: Incremental value compensation amount 2: Absolute value compensation amount c. Tool management method 0: Usage time 1: Number of mounts 2: Number of usages Life (Ln) 0 to 4000 minutes (usage time) 0 to 65000 times (number of mounts) 0 to 65000 times (number of usages) Length compensation (Hn) (No./amount) 0 to 999 (compensation No.) (*1) ±999.999 (incremental value compensation amount) (*2) ±999.999 (absolute value compensation amount) (*2) Radius compensation (Rn) (No./amount) 0 to 999 (compensation No.) (*1) ±999.999 (incremental value compensation amount) (*2) ±999.999 (absolute value compensation amount) (*2) (*1) The setting range of the tool compensation No. differs according to the specification of the "number of tool offset sets". (*2) Refer to (16) in "12.9.3 Precautions for Inputting the Tool Life Management Data" for the data range of compensation amount. IB-1501278-D 516 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions Operation example Program example Data registration G10 L30; P10 L10 Q001 ; T10 H10 R10 ; G11 ; M02 ; Group change, addition G10 L30 P1; P10 L10 Q122 ; T10 H0.5 R0.25 ; G11 ; M02 ; Operation 1. After deleting all group data, the registration starts. 2. Group No. 10 is registered. Tool management method is number of mounts Compensation No. method is applied to tool length compensation and tool radius compensation. 3. Tool No. 10 is registered in group No. 10. 4. The registration ends. 5. The program ends. 1. Changing and addition of the group and tool starts. 2. The change and addition operation takes place in the following manner. (1) When group No. 10 has not been registered: (a) Group No. 10 is registered additionally. About the change and addition tool Tool management method is number of usages, Tool length compensation is the incremental value compensation amount method, and Tool radius compensation is the absolute value compensation amount method. (b) For group No. 10, the incremental value compensation amount "0.5" is registered for the length compensation, and the absolute value compensation amount "0.25" is registered for the radius compensation. (2) When group No. 10 has been registered, but tool No. 10 has not been registered. - Tool No. 10 is additionally registered in group No. 10. (3) When group No. 10 and tool No. 10 have been both registered. - The tool No. 10 data is changed. 3. The group and tool change and addition ends. 4. The program ends. Group deletion G10 L30 P2; P10 ; G11 ; M02 ; 1. The group deletion starts. 2. The group No. 10 data is deleted. 3. The group deletion ends. 4. The program ends. 517 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.11.3 Precautions for Inputting The Tool Life Management Data Relationship with other functions (1)During the following operations, the tool usage data will not be counted. - Machine lock - Auxiliary axis function lock - Dry run - Single block - Skip Precautions (1) The tool life data is registered, changed, added to or deleted by executing the program in the memory or MDI mode. (2) The group No. and tool No. cannot be commanded in duplicate. The program error (P179) will occur. (3) When two or more addresses are commanded in one block, the latter address will be valid. (4) If the life data (L_) is omitted in the G10L3 command, the life data for that group will be "0". (5) If the control method (Q_) is omitted in the G10L3 command, the control method for that group will follow the base specification parameter "#1106 Tcount". Note that when carrying out the No. of cutting times control method, command the method from the program. (6) If the control method (Q_) is not designated with 3-digit by G10 L30 command, the omitted high-order are equivalent to "0". Therefore, "Q1" is equivalent to "Q001", and "Q12" is equivalent to "Q012". (7) If the length compensation No. (H_) is omitted in the G10L3 command, the length compensation No. for that group will be "0". (8) If the radius compensation No. (D_) is omitted in the G10L3 command, the radius compensation No. for that group will be "0". (9) Programming with a sequence No. is not possible between G10 L3 or G10 L30 and G11. The program error (P33) will occur. (10) If the usage data count valid signal (YC8A) is ON, G10 L3 or G10 L30 cannot be commanded. The program error (P177) will occur. (11) The registered data is held even if the power is turned OFF. (12) When G10 L3 or G10 L30 is commanded, the commanded group and tool will be registered after all of the registered data is erased. (13) The change and addition conditions in the G10L3P1 or G10 L30 P1 command are as follows. (a) Change conditions Both the commanded group No. and tool No. are registered. -> Change the commanded tool No. data. (b) Additional conditions Neither the commanded group No. nor tool No. is registered. -> Additionally register the commanded group No. and tool No. data. The commanded group No. is registered, but the commanded tool No. is not registered. -> Additionally register the commanded tool No. data to the commanded group No. (14) The setting range of the tool compensation No. depends on the MTB specifications. (15) Only group No. 1 can be used to register, change and add for the tool life management III. IB-1501278-D 518 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions 15.11.4 Allocation of The Number of Tool Life Management Sets to Part Systems Function and purpose The number of tool life management sets can be set per part system. This function is divided into following methods and which one is used depends on the MTB specifications (parameters "#1439 Tlife-SysAssign", "#12055 Tol-lifenum"). Arbitrary allocation: Arbitrarily allocates the number of tool life management sets to each part system. Fixed allocation: Automatically and evenly allocates the number of tool life management sets to each part system. The arbitrary allocation enables the efficient allocation because when a certain part system needs only a small number of tool life management sets, the rest can be allocated to another part system. If an auxiliary-axis part system does not need the tool life management sets at all, the number of tool life management sets can be set to "0" for the auxiliary-axis part system. Subsequent description is an example in the case where the number of tool life management sets in the system is 999 sets. (1) Arbitrary allocation (with #1439=1) The number of sets allocated to each part system depends on the MTB specifications (parameter "#12055 Tollifenum"). The following example shows the number of tool offset sets allocated when the lathe system is a 4-part system. (a) When the number of tool life management sets is increased for the 1st part system ($1) of 4-part system $1 250 $2 250 $3 250 $4 250 $1 400 $2 200 $3 200 $4 200 (b) When the number of tool life management sets is set to "0 sets" for the 3rd part system ($3) of 3-part system to use that part system as an auxiliary-axis part system $1 334 $2 333 $3 333 $1 500 $2 500 $3 0 519 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 15 Program Support Functions (2) Automatic and even allocation (with #1439=0) 1-part system 2-part system $1 $1 3-part system (Lathe system only) $1 500 999 (*1) $2 500 334 (*2) $2 333 $3 333 4-part system (Lathe system only) $1 250 $2 250 $3 250 $4 250 (*1)The maximum number of tool life management sets per part system is 999. (*2) If there is any remainder, the remainder is allocated to the 1st part system. Precautions (1) The maximum number of tool life management sets for 1-part system is 999. (2) For 1-part system, up to the number of tool life management sets in the system is available regardless of the parameter setting. (3) When the value of the parameter "#12055 Tol-lifenum" is equal to or lower than the number of tool life management sets in the system, the remainder is not allocated to any part system even if the specification allows arbitrary allocation. (4) When the value of the parameter "#12055 Tol-lifenum" is equal to or lower than the number of tool life management sets in the system, system alarm (Y05) is generated even if the specification allows arbitrary allocation. (5) Even if the specification allows arbitrary allocation, fixed allocation is applied if the parameter is "#12055 Tollifenum"= "0" for all part systems. (6) When entering data into the tool life management file, if the number of tool life management data exceeds that of current tool life management sets, the excess tool life management data cannot be entered. IB-1501278-D 520 16 Multi-part System Control 521 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control 16Multi-part System Control 16.1 Timing Synchronization Operation CAUTION When programming a multi-part system, carefully observe the movements caused by other part systems' programs. 16.1.1 Timing Synchronization Operation (! code) !n (!m ...) L Function and purpose The multi-axis, multi-part system complex control CNC system can simultaneously run multiple machining programs independently. The synchronization-between-part systems function is used in cases when, at some particular point during operation, the operations of 1st and 2nd part systems are to be synchronized or in cases when the operation of only one part system is required. When timing synchronization is executed in the 1st part system ($1) and the 2nd part system ($2), operations will be as follows. $1 $2 Simultaneous and independent operation Timing synchronization operation Simultaneous and independent operation Timing synchronization operation 2nd part system operation only 1st part system waiting Timing synchronization operation Simultaneous and independent operation % % Command format !n (!m ...) L_ ; ... timing synchronization operation !n, !m, ... Timing synchronization operation (!) and part system No. (n:1 - number of part system that can be used) Follows the settings of the parameter "#19419 Timing sync system" if part system number is omitted. L Timing Synchronization Operation No. 0 to 9999 IB-1501278-D 522 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Detailed description (1) Timing synchronization between part systems during automatic operation If !n L__ is commanded from a part system (i), operation of the part system i program will wait until !i L_ is commanded from the part system n program. When !i L_ is commanded, the programs for the two part systems will start simultaneously. Timing synchronization between 2 part systems $i $n Pi1 Pn1 !nL1 ; Timing synchronization Pi2 $i $n Pi1 waiting... !iL1; Pn2 Pi2 Simultaneously start Pn1 Pn2 (2) The timing synchronization operation is normally issued in a single block. However, if a movement command or M, S or T command is issued in the same block, whether to synchronize after the movement command or M, S or T command or to execute the movement command or M, S or T command after synchronization will depend on the MTB specifications (#1093 Wnvfin). #1093 Wmvfin 0 : Wait before executing movement command. 1 : Wait after executing movement command. (3) If there is no movement command in the same block as the timing synchronization operation, when the next block movement starts, synchronization may not be secured between the part systems. To synchronize the part systems when movement starts after waiting, issue the movement command in the same block as the timing synchronization operation. (4)The L command is the timing synchronization identification No. The same Nos. are waited but when they are omitted, the Nos. are handled as L0. (5) "SYN" will appear in the operation status section during timing synchronization operation. The timing synchronization operation signal will be output to the PLC I/F. (6) In a timing synchronization operation, other part system to be waited for is specified but the own part system can be specified with the other part system. (7) The timing synchronization operation of a specific part system can be ignored depending on the MTB specifications. Operation will be determined by the combination of the timing synchronization operation ignore signal and parameter "#1279 ext15/bit0". For setting combination, refer to "Time synchronization when timing synchronization ignore is set". For the specifications of the machine you are using, see the instructions issued by the MTB. 523 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Precautions (1) When the M code can be used, both the M code and ! code can be used. (2) While the timing synchronization operation M code is valid, if one part system is standing by with an M code, an alarm will occur if there is a ! code timing synchronization operation command in the other part system. (3) While the timing synchronization operation M code is valid, if one part system is standing by with a ! code, an alarm will occur if there is an M code timing synchronization operation command in the other part system. (4) When macro interruption is carried out in a part system waiting, the part system can stop while waiting even if the conditions for time synchronization are met. In this case, you will be able to continue the program, ignoring the timing synchronization with timing synchronization operation ignore signal. For details, contact the MTB. IB-1501278-D 524 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control 16.1.2 Timing Synchronization Operation with Start Point Designated (Type 1) ; G115 Function and purpose The part system can wait for the other part system to reach the start point before starting itself. The start point can be set in the middle of a block. Command format !n L__ G115 X__ Y__ Z__ ; !n Timing synchronization operation (!) and part system No. (n:1 - number of part system that can be used) Part systems follow the settings of the parameter "#19419 Timing sync system" if the number is omitted. L Timing Synchronization Operation No. 0 to 9999 (It will be regarded as "L0" when omitted.) G115 G command XYZ Start point (Command by axis and workpiece coordinate value) 525 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Detailed description (1)Designate the start point using the workpiece coordinates of the other part system (ex. $2). (2)The start point check is executed only for the axis designated by G115. (Example) !L2 G115 X100. ; Once the other part system reaches X100, the own part system (ex. $1) will start. The other axes are not checked. (3)The other part system starts first when timing synchronization operation is executed. (4)The own part system waits for the other part system to move and reach the designated start point, and then starts. $1 !2 G115 $2 !1 G00 X... !2 G115 $1 !1 $2 G00 X... Timing synchronization Designated start point (5) When the start point designated by G115 is not on the next block movement path of the other part system, the own part system starts once all the designated axis of the other part system has reach the designated start point. Movement Designated start point Actual start point (6) After waiting, if the start point cannot be obtained with movement command of the other timing synchronization block, the operations depend on the MTB specifications (parameter "#1229 set01/bit5"). (a) When the parameter is ON Wait till the own part system reaches the start point by moving after the next block. (b) When the parameter is OFF When the next block finishes moving, the own part system will start. IB-1501278-D 526 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control (7)The timing synchronization status continues when the G115 command has been duplicated between part systems. (Operations will not restart.) $1 !2 G115 Timing synchronizing $2 !1 G115 (8) The single block stop function does not apply for the G115 block. (9) A program error (P32) will occur if an address other than an axis is designated in G115 command block. (10) In the timing synchronization operation, other part system to be waited for is specified but the own part system can be specified with the other part system. (11) The timing synchronization operation of a specific part system can be ignored depending on the MTB specifications. Operation will be determined by the combination of the timing synchronization operation ignore signal (PLC signal) and parameter "#1279 ext15/bit0". For setting combination, refer to "Time synchronization when timing synchronization ignore is set". For the specifications of the machine you are using, see the instructions issued by the MTB. Precautions (1) Parameter "#1093 Wmvfin" that selects the timing of the timing synchronization operation and commands on the same block does not work for the start point command block (G115/G116). After synchronization. the start point check will be executed by G115/G116. (2) Be careful about the timing when interrupting during the time synchronization of G115/G116. For example, assume interruption with the macro interrupt type 1 while a part system is waiting for time synchronization with G116. In this case, if there is a movement command or MSTB command in the interrupt program, the program will continue after the interrupt program completes without waiting for the start point. (3)The L command is the timing synchronization identification No. The same Nos. are waited but when they are omitted, the Nos. are handled as L0. 527 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control 16.1.3 Timing Synchronization Operation with Start Point Designated (Type 2) ; G116 Function and purpose The own part system can make the other part system to wait until it reaches the start point. The start point can be set in the middle of a block. Command format !n L__ G116 X__ Y__ Z__ ; !n Timing synchronization operation (!) and part system No. (n:1 - number of part system that can be used) Part systems follow the settings of the parameter "#19419 Timing sync system" if the number is omitted. L Timing Synchronization Operation No. 0 to 9999 (It will be regarded as "L0" when omitted.) G116 G command XYZ Start point (Command by axis and workpiece coordinate value) IB-1501278-D 528 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Detailed description (1)Designate the start point using the workpiece coordinates of the own part system (ex. $1). (2)The start point check is executed only for the axis designated by G116. (Example) !L1 G116 X100. ; Once the own part system reaches X100, the other part system (ex. $2) will start. The other axes are not checked. (3)The own part system starts first when timing synchronization operation is executed. (4)The other part system waits for the own part system to move and reach the designated start point, and then starts. !2 G116 $1 G00 X... $2 !1 !2 G116 $1 $2 G00 X... !1 Timing synchronization Designated start point (5) When the start point designated by G116 is not on the next block movement path of own part system, the other part system starts once all the designated axes of the own part system has reach the designated start point. Movement Designated start point Actual start point (6) If the start point cannot be obtained with the movement of the own part system to the next block, the operations depend on the MTB specifications (parameter "#1229 set01/bit5"). (a) When the parameter is ON The own part system will have a program error (P511) before moving. (b) When the parameter is OFF When the next block finishes moving, the other part system will start. (7)The timing synchronization status continues when the G116 command has been duplicated between part systems. (Operations will not restart.) $1 !2 G116 Timing synchronizing $2 !1 G116 529 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control (8) The single block stop function does not apply for the G116 block. (9) A program error (P32) will occur if an address other than an axis is designated in G116 command block. (10) In the timing synchronization operation, other part system to be waited for is specified but the own part system can be specified with the other part system. (11) The timing synchronization operation of a specific part system can be ignored depending on the MTB specifications. Operation will be determined by the combination of the timing synchronization operation ignore signal (PLC signal) and parameter "#1279 ext15/bit0". For setting combination, refer to "Time synchronization when timing synchronization ignore is set". For the specifications of the machine you are using, see the instructions issued by the MTB. Precautions Refer to "Start point designation timing synchronization (Type 1) ; G115". IB-1501278-D 530 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control 16.1.4 Timing Synchronization Operation Function Using M codes ; M*** Function and purpose The timing synchronization operation function between part systems is conventionally commanded with the "!" code, but by using this function, the part systems can be waited with the M code commanded in the machining program. If the timing synchronization operation M code is commanded in either part system during automatic operation, the system will wait for the same M code to be commanded in the other part system before executing the next block. The timing synchronization operation M code is used to control the timing synchronization operation between the 1st part system and 2nd part system. Whether the timing synchronization operation M code can be used depends on the MTB specifications. Command format M*** ; *** Timing synchronization operation M code M code used for timing synchronization depends on the MTB specifications (parameter "#1310 WtMmin)", "#1311 WtMmax"). 531 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Detailed description (1) When the timing synchronization operation M code is commanded in the machining program, the two part systems will be waited and operation will start in the commanded block. If the timing synchronization operation M code is commanded in either part system during automatic operation, the system will wait for the same M code to be commanded in the other part system before executing the next block. $1 $2 P11 Simultaneous and independent operation on part system 1 and 2 P21 Timing synchronization M100 ; M100 ; P12 In simultaneous and independent operation P22 M101 ; M101 Waiting M101 ; M102 ; As M101 is commanded in part system 1, part system 2 starts operation. M102 Waiting P23 As M102 is commanded in part system 2, part system 1 and 2 start operation.independently. Simultaneous and independent operation M102 ; P14 P24 M30 ; M30 ; M102 Waiting P11 $1 P12 P21 $2 P14 P22 P23 P24 M101 Waiting (2) When the timing synchronization operation M code has been commanded in one part system, and the part system is standing by for waiting, an alarm will occur if a different M code is commanded in the other part system. $1 $2 P11 P21 M100 ; M100 Waiting M101 ; P12 IB-1501278-D Simultaneous and independent operation Alarm (Operation stops) P22 532 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control (3)The part systems are waited with the M code following the parameters below. These settings depend on the MTB specifications. Refer to these settings. For details, refer to the specifications of your machine. (a) M code range designation parameter (M code minimum value <= M code <= M code maximum value) # Item Details Setting range 1310 WtMmin Timing synchronization M code ABS. MIN. The minimum value of the M code. If the setting value 0, is "0", the timing synchronization operation M code will 100 ~ 99999999 be ignored. 1311 WtMmax Timing synchronization M code ABS. MAX. The maximum value of the M code. If the setting value 0, is "0", the timing synchronization operation M code will 100 ~ 99999999 be ignored. This function is invalid if either parameter is set to "0". The timing synchronization operation M code cannot be used if the M code maximum value is smaller than the minimum value. When the timing synchronization operation M code is valid, both the M code and ! code can be used for timing synchronization operation. (b) Timing synchronization operation method parameters # 1279 (PR) Item ext15 (bit0) Method for timing synchronization operation between part systems Details Setting range Select an operation for timing synchronization opera- 0 / 1 tion between part systems. 0: If one of the part systems is not in automatic operation, ignore the timing synchronization operation and execute the next block. 1: Operate according to the timing synchronization operation ignore signal. If the timing synchronization operation ignore signal is "1", the timing synchronization operation will be ignored. If "0", the part systems will be waited. Depending on the timing synchronization operation method selection parameter and timing synchronization operation ignore signal combination, the timing synchronization operation will be determined by the parameters, regardless of the command format ("!" code and M code). This parameter requires the CNC to be turned OFF after the settings. Turn the power OFF and ON to enable the parameter settings. # 1093 Item Wmvfin Method for timing synchronization operation between part systems Details Setting range Parameter to designate the timing synchronization op- 0 / 1 eration between part systems method when using multi-part systems. When there is a movement command in the timing synchronization operation (!, M) block: 0 : Wait before executing movement command. 1 : Wait after executing movement command. Relation with other functions Refer to "Timing Synchronization Operation (! code);!n (!m ...) L" 533 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Precautions For precautions for time synchronization, also refer to "Timing Synchronization (!code);!n (!m ...) L" (1) When timing synchronization operation with the M code, always command the M code in an independent block. (2) When standing by after commanding the timing synchronization operation M code in one part system, an alarm will occur if a different M code is commanded in the other part system. Operation will stop in both part systems. (3) The timing synchronization operation (! code, M code) in the machining program can be ignored with the timing synchronization operation ignore signal. (This depends on the MTB specifications. ) Operation with a single part system is possible without deleting the timing synchronization operation (! code, M code) in the machining program. (4) Unlike other M codes, the timing synchronization operation M code does not output code signals and strobe signals. (5) When the M code can be used, both the M code and ! code can be used. (6) While the timing synchronization operation M code is valid, if one part system is standing by with an M code, an alarm will occur if there is a ! code timing synchronization operation command in the other part system. (7) While the timing synchronization operation M code is valid, if one part system is standing by with a ! code, an alarm will occur if there is an M code timing synchronization operation command in the other part system. (8) If there is a timing synchronization operation with M code after the 3rd part system, an alarm will occur. (9) The G115 and G116 commands cannot be used when waiting with the M code. (10) If the M code command Nos. are overlapped, the order of priority will be M code macro, M command synchronous tapping, timing synchronization operation M code and normal M code. (11) When macro interruption is carried out in a part system waiting, the part system can stop while waiting even if the conditions for time synchronization are met. In this case, you will be able to continue the program, ignoring the timing synchronization with timing synchronization operation ignore signal. For details, contact the MTB. (12) "SYN" will appear in the operation status section during timing synchronization operation. IB-1501278-D 534 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control 16.1.5 Time Synchronization When Timing Synchronization Ignore Is Set Function and purpose Turning on the timing synchronization operation ignore signal makes it possible to ignore the timing synchronization operation of that part system. With a 2-part system, if the timing synchronization operation ignore signal of the other part system is ON, timing synchronization is not executed. In the following section, a 3-part system is used as an example to make it easier to understand the functions. This signal is also used in the following functions. Timing synchronization (! code, M code) Start point timing synchronization (G115, G116) Balance cut (G15) Lathe system only Note (1) For sub part system control function, refer to "16.3 Sub Part System Control". Timing synchronization operation ignore signal (PLC signal) OFF Parameter 0 (#1279 ext15/bit0) 1 ON (1) Ignores the timing synchronization with a part system not in automatic operation (2) Does not ignore the timing synchroniza- (3) Ignores the timing synchronization retion regardless of whether or not a part sys- gardless of whether or not a part system is tem is in automatic operation (the timing in automatic operation (ignores the timing synchronization is executed until the condi- synchronization command for the part systions for timing synchronization are estab- tem with the timing synchronization ignore lished.) signal ON and the timing synchronization operation for that part system) The following operation diagram gives an example of ! code. (1) A case that "Ignores the timing synchronization with a part system not in automatic operation" $i $n (Not in automatic operation) Ignore timing synchronization Pi1 $m Pm1 !n !m L _ ; Simultaneously start after timing synchronization block !i !n L _ ; Pm2 Pi2 $i Pi1 waiting... Pi2 $n $m Pm1 Pm2 Start simultaneously 535 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control (2) A case that "Does not ignore the timing synchronization regardless of whether or not in automatic operation" $i $n Pi1 $m Necessarily conduct timing synchronization !n !m L 1 ; Pm1 Timing synchronization !i !n L 1 ; Start the $n program. $i $n $m Pi1 Pm1 !n !m L 1 ; (Automatic start) !i !n L 1 ; Timing synchronization Simultaneously start after timing synchronization block Pi1 Pn2 waiting... Automatic start Pm1 Pn2 waiting... A Pm2 Pi2 Pn1 $n $m Timing synchronization !i !m L 1 ; Pi2 $i Pn1 Pm2 B A: When timing synchronization operation between part systems (parameter "#1279 ext15/bit0" = 1), the timing synchronization status continues until the conditions for timing synchronization are established. B: Part system n is automatically started. If the conditions for timing synchronization are established, the next block will start. IB-1501278-D 536 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control (3) A case that "Ignores the timing synchronization regardless of whether or not in automatic operation" $i $n Pi1 !n !m L 1 ; $i and $n start simultaneously in the next block after timing synchronization. Ignore timing Pn1 synchronization !i !n L 1 ; !i !m L1 ; Pn2 Ignore timing synchronization with part system m. $n $m $m timing synchronization ignore signal Pi1 Pm1 Timing synchronization Pi2 $i $m Timing synchronization operation ignore signal ON Pi2 waiting... !n !m Pn1 Ignore timing synchronization Pm2 Part system m does not conduct timing synchronization. Timing synchronization Pn2 !i !m Pm1 !i !n Part system m is in the timing synchronization ignore state, so timing synchronization is not conducted. 537 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control 16.2 Mixed Control 16.2.1 Arbitrary Axis Exchange ; G140, G141, G142 Function and purpose With this function, an arbitrary axis can be exchanged freely across part systems. The machining can be freer in the multiple part systems by exchanging an axis that can be commanded for machining programs in each part system. This makes it possible to perform operations which are not possible with regular axis configurations: for instance, tools which are provided only on the 1st part system can be used for machining on the 2nd part system. This chapter illustrates an example based on the placements of the basis axes below. X axis Y axis Z axis C axis 1st part system ($1) X1 Y1 Z1 - 2nd part system ($2) X2 Y2 - C2 Refer to "Programming Manual Lathe System" (IB-1501275, IB-1501276) for details of the arbitrary axis exchange. Command format When commanding the arbitrary axis exchange G140 command address = axis address ... ; Command Address It is a command address used in a movement or other command after arbitrary axis exchange command (G140). Designate the command address with one alphabetical character set to parameters ("#12071 adr_abs[1]"to "#12078 adr_abs[8]") . Axis address Set the axis name for arbitrary axis exchange. Designate the command with two alphanumeric characters set to the parameter "#1022 axname2". When returning the exchanged axis G141; Arbitrary axis exchange return Returns the control right of the axis, exchanged by the previous arbitrary axis exchange command (G140) in the commanded part system, to the state before the axis exchange. G142; Reference axis arrange return Returns the control right of the axis, exchanged by the arbitrary axis exchange command (G140) in the commanded part system, to the power-on state. IB-1501278-D 538 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Detailed description Arbitrary axis exchange command (G140) There are two methods for axis exchange operations with arbitrary axis exchange command (G140). The methods for your machine depends on the MTB specifications (parameter "#1434 G140Type2"). Method Operation Method for exchanging all axes Designates axes to be used in the part system with a command address. The ("#1434 G140Type2" = 0) command addresses axes that are not designated will be released as uncontrol axes. Method for exchanging command axes ("#1434 G140Type2" = 1) Designates axes to be used in the part system with a command address. The command addresses axes that are not designated will maintain the current state. (1) Operation example of the method for exchanging all axes ("#1434 G140Type2"=0) Below is the control axis of each part system when running the following machining programs (1st part system, 2nd part system) $1 $2 Machining program Machining program G140 X=X1 Y=Y1 Z=Z1; G00 X10.; G01 X5. F1; : (a) G140 X=X1 Y=Y2; G00 Y25.; G01 X8. F2; : (b) Control axes G140 X=X2 Y=Y2 C=C2; G00 X20.; G01 X15. F2; : $2 Uncontrol axes X Y Z X Y C X1 Y1 Z1 X2 Y2 C2 - X2 - C2 Y1,Z1 - Z1 - Y1,X2,C2 - - - X2,Y2,C2 X2 Y2 C2 - (d) (e) G140 Y=Z1; G00 Y10.; G01 Y8. F0.05; : G140 X=X1 Y=Y1 Z=Z1; G00 X20. Y15.; G01 X15. F5; : $1 X1 Y2 - (c) X1 G140 X=X2 Y=Y2 C=C2; G00 X0; : 1st part system ($1) (a),(c) (b) 2nd part system ($2) (d),(f) (e) Y1 Z1 (f) Declares the use of X1 axis, Y1 axis and Z1 axis. Declares the use of X1 axis and Y2 axis. The control right of Y2 axis shifts to the 2nd part system from the 1st part system. Y1 axis, exchanged for Z1 axis and Y2 axis which were not designated, will be an uncontrol axis. Declares the use of X2 axis, Y2 axis and C2 axis. Declares the use of Z1 axis. X2 axis and C2 axis which were not designated will be uncontrol axes. 539 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control (2) Operation example of the method for exchanging command axes ("#1434 G140Type2"=1) Below is the control axis of each part system when running the following machining programs (1st part system, 2nd part system) $1 $2 Machining program Machining program G140 X=X1 Y=Y1 Z=Z1; G00 X10.; G01 X5. F1; : (a) G140 Y=Y2; G00 Y25.; G01 X8. F2; : (b) Control axes G140 X=X2 Y=Y2 C=C2; G00 X20.; G01 X15. F2; : G140 Y=Y1; G00 Y10.; G01 Y8. F0.05; : G140 Y=Y1 ; G00 X20. Y15.; G01 X15. F5; : $1 $2 Uncontrol axes X Y Z X Y C X1 Y1 Z1 X2 Y2 C2 - X2 - C2 Y1 X2 Y1 C2 - X2 - C2 Y2 X2 Y2 C2 - (d) (e) X1 Y2 Z1 (c) X1 G140 X=X2 Y=Y2 C=C2; G00 X0; : 1st part system ($1) (a) Y1 Z1 (f) Declares the use of X1 axis, Y1 axis and Z1 axis. (b) Declares the use of Y2 axis. The control right of Y2 axis shifts to the 2nd part system from the 1st part system. Y1 axis which was exchanged for Y2 axis will be an uncontrol axis. (c) Declares the use of Y1 axis. The control right of Y1 axis shifts to the 2nd part system from the 1st part system. Y2 axis which was exchanged for Y1 axis will be an uncontrol axis. 2nd part system ($2) (d) Declares the use of X2 axis, Y2 axis and C2 axis. (e) Declares the use of Y1 axis. (f) Declares the use of X2 axis, Y2 axis and C2 axis. Unavailable state of axis exchange "Unavailable state of axis exchange" indicates a "condition in which a target axis for axis exchange is not available for exchange because the designated target axis for axis exchange is being used by other part systems or for other reasons" through the arbitrary axis exchange command (G140), the arbitrary axis exchange return command (G141), the reference axis arrange return command (G142). When the conditions for unavailable state of axis exchange fall through, no axis exchange mode will be cancelled. It will be cancelled when a reset signal or emergency stop is entered. IB-1501278-D 540 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control 16.3 Sub Part System Control 16.3.1 Sub Part System Control I ; G122 Function and purpose This function activates and operates any non-operating part system (sub part system) in the multi-part system. Sub part system control I can be used in the same manner as calling subprogram in a non-operating part system. An auxiliary axis machining program can be controlled in the sub part system by commanding Sub part system control I (G122) from the main part system. In the usage example below, the tool positioning starts to the machining start point at the same time (time T1) as the start of gantry retract by using Sub part system control I (G145) in the flow from feeding the workpiece to moving to cut start position in order to reduce the cycle time. Select whether main part system or sub part system for each part system in Sub part system control I. When using a part system as a sub part system, by setting the operation mode to "Sub part system I operation mode" with the PLC signal and commanding sub part system control I (G122) from an operating part system, it is possible to activate the part system in the sub part system I operation mode as a sub part system. Machining process when Sub part system control is OFF Main part system ($1) (1) Feed the workpiece (2) Clamp the workpiece (3) Retract gantry T1 (4) Move to cut start position T1: Time when gantry retract is started Machining process when Sub part system control is ON Sub part system ($2) (1)Feed the workpiece Main part system ($1) (2)Clamp the workpiece Wait for completion of sub part system Time T2 T2: Time when gantry retract is completed (3)Retract gantry (4)Move to cut start position Time Sub part system starts T1 T2 The following describes the meanings of the terms used in this chapter. Term Meaning Main part system Indicates a part system located on the uppermost stream side of a sub part system call flow. Sub part system Indicates a part system activated by the sub part system activation command. Calling part system Indicates a part system that issued the sub part system activation command. The examples below shows many part systems to provide an easy-to-understand explanation. The actually available number of part systems depends on your machine's specifications. 541 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Enabling conditions (1) This function can be used in multi-part systems of two or more part systems. (2) In order to activate a sub part system using the sub part system control I command, the following conditions must be satisfied. There are conditions to enable functions that are only applicable to the M80 series. [Condition 1] This condition must only be satisfied for the M80 series. The number of sub part systems has been set in the base common parameter "#1483 SBS1_sys num" (the number of part systems in sub part system I). (a) Part systems as many as the number specified in #1483, counted from the end of the valid part system (the part system for which "#1001 SYS_ON" is set to "1"), will be reserved as sub part systems. (b) If the number of sub part systems or main part systems exceeds the maximum number defined in the system specifications, an MCP alarm (Y05 1483) will occur. (c) If the values set for "#1483 SBS1_sys num" and "#1474 SBS2_sys num" are both "1" or more, an MCP alarm (Y05 1483) will occur. [Condition 2] The identification No. (B command value) used to activate a sub part system has been set in the base common parameter "#12049 SBS_no" (sub part system I identification No.) for sub part systems. (a) If an identification No. that is not set in the parameter "#12049 SBS_no" is specified when the sub part system control I command is issued, a program error (P650) (sub part system identification No. illegal) will occur. [Condition 3] The PLC signal SBSM (Sub part system I operation mode) of the sub part system is set to "1". (a) In a part system operating the sub part system I operation mode, the operation mode appears as "SUB" in the part system display of the operation screen. (b) If the sub part system control I command is issued to a part system that is not operating the sub part system I operation mode, an operation error (M01 1111) will occur. However, while the an operation error (M01 1111) is occurring, the operation can be started by setting SBSM to "1". IB-1501278-D 542 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Command format Call sub part system G122 A__P__Q__K__D__B__H__ (argument); G122 <file name> P__Q__K__D__B__H__ (argument); A Program No. (1 to 99999999 or 100010000 to 199999998) <File name> File name of the program (up to 32 characters) P Start sequence number (Head of the program if omitted.) Q End sequence number (To end (M99) of the program if omitted.) K Number of repetitions (1 to 9999) D Synchronization control (0/1) B Sub part system identification No. (1 to 7) H Sub part system reset type (0/1) Argument Argument of a sub part system local variable (Setting rage of local variable (decimal point command is valid)) Complete sub part system M99: (command of a sub part system side) Cancel the standby status for completion of sub part system G145; (command of a sub part system side that is issued when the D0 command is issued) Note (1) G145 is ignored in a sub part system activated in the parallel control method (D1 command). 543 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Detailed description This function can be used in multi-part systems of two or more part systems. Main part system and sub part system are switched according to the MTB specifications. Description of each address Address A Meaning Program No. Command range (unit) 1 to 99999999 or 100010000 to 199999998 (*1) Remarks Program No. or file name of the machining program operating in the sub part system. Programs in external device cannot be designated. If address A and <file name> are designated at the <File name> File name of the pro- Up to 32 characters. same time, precedence is given to address A. gram If designation of the program is omitted, the machining program defined by the MTB will be used (parameter "#12050 SBS_pro"). P Start sequence No. 1 to 99999999 Sequence No. to start the machining program operating in the sub part system. If there is no command, the operation will start from the head of the machining program. Q End sequence No. 1 to 99999999 Sequence No. to end the machining program operating in the sub part system. If there is no command, the program will run up to M99. K Number of repetitions 1 to 9999 The number of times to repeat the machining program for continuous operation in the sub part system. If there is no command, the program will run only once. (No repetition) D Synchronization control 0/1 Validity of synchronous control 0: The next block is processed after the sub part system operation completes. 1: The next block is processed at the same time as the start of a sub part system operation. If there is no command, it is handled in the same manner as 0 is designated. B Sub part system identification No. 1 to 7 Identification No. used for timing synchronization with sub part system, etc. The sub part system to be activated is designated by an identification No. The correspondence between identification No. and part system No. depends on the MTB specifications (parameter "#12049 SBS_no"). If there is no command, it is handled in the same manner as 1 is designated. H Sub part system re- 0 / 1 set type (*2) (Argument) Argument of a sub part system local variable IB-1501278-D 0: The G command modal is maintained by the reset when a sub part system is complete. 1: The G command modal is initialized by the reset when a sub part system is complete. If there is no command, it is handled in the same manner as 0 is designated. Setting range of lo- Argument is passed to the sub part system as a local variable (level 0). cal variable (Decimal point com- However, addresses A, B, D, G, H, K, O, P, and Q cannot be used as an argument. mand is possible.) For the correspondence between address and variable number, refer to the following table. 544 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control (*1) When the parameter "#1253 set25/bit0" is set to "1", the command range is "100010000 to 199999989". (*2) If a sub part system ends by M99 or the end sequence No., resetting processing is performed automatically in the sub part system. Correspondence of argument designation address and variable number in sub part system Argument designa- Variable number in sub tion address part system Argument designa- Variable number in sub tion address part system A - N #14 B - O - C #3 P - D - Q - E #8 R #18 F #9 S #19 G - T #20 H - U #21 I #4 V #22 J #5 W #23 K - X #24 L #12 Y #25 M #13 Z #26 Note (1) Addresses can be designated in an arbitrary order. (2) Addresses which do not need to be designated can be omitted. (3) Local variables in a sub part system are initialized every time the sub part system is activated. Default value is <empty>. (4) To use local variables in a sub part system, user macros must be available. For the available functions of each model, refer to the list. Operation mode of a sub part system (1) The operation mode of sub part systems is used as "sub part system I operation mode". If the memory mode/ MDI mode and the sub part system I operation mode are entered at the same time, the stop code (T01 0108) will be generated. (2) In a part system operating the sub part system I operation mode, the operation mode appears as "SUB" in the part system display of the operation screen. If an alarm or warning occurs in a sub part system, the part system No. appears as "SUB" in the alarm/warning message of the operation screen. (3) If the sub part system control I command is issued to a part system that is not operating the sub part system I operation mode, an operation error (M01 1111) will occur. Activation part system of a sub part system When issuing the sub part system control I command, designate the sub part system identification No. with command address B. (When there is no B command, it will be handled as the B1 command.) The sub part system identification No. and the sub part system No. to be called depend on the MTB specifications. (Parameter "#12049 SBS_no") (Example 1) and (Example 2) show the operations when parameters are set as shown below. The available number of part systems depends on your machine's specifications. #12049 SBS_no Sub part system I identification No. $1 $2 $3 $4 $5 $6 $7 $8 0 0 0 0 1 2 3 4 545 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control (Example 1) If the B command is omitted, $5 corresponding to B1 will be activated. Calling part system ($1) Sub part system ($5) : : G122 A100 D0; : : : : : M99; (Example 2) Sub part system identification No. (the part system No. to be activated and correspondence) can be specified with the B command. Calling part system ($1) Sub part system ($7) : : G122 A100 D0 B3; : : : : : M99; Operation program of a sub part system When issuing the sub part system control I command, designate the program No. or program name to be operated in the sub part system with command address A or <file name>. If designation of the program is omitted, the machining program set in parameter "#12050 SBS_pro" will be started. If a machining program is managed for each part system, the program of the part system designated as a sub part system will be operated (*1). If a machining program is commonly managed between part systems, the designated program will be operated. (*1) If the program of the part system No. for the sub part system is empty, the program of the 1st part system ($1) will be operated. If the program of the 1st part system is also empty, a program error (P461) will occur. (1) If program is managed for each part system O100 Caller part system ($1) O1 - $1 : : G122 A100 D0 B3㸹 : $7 is assumed to be started by B3 command. $1 $2 Sub part system ($7) O100 - $7 : : M99; When $7 is blank, $1 data will be called. $3 $4 $5 $6 $7 $8 IB-1501278-D 546 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control (2) If program is commonly managed between part systems Calling part system ($1) O1 : O100 : Sub part system ($7) G122 A100 D0 B3； O100 : : $7 is assumed to be started by B3 command. : M99; Sub part system activation with the completion wait method (D=0) If "0" is designated for command address D when the sub part system control I command is issued, or if command address D is omitted, the calling part system will wait for the called sub part system to complete (to M99 or the end sequence No.) before starting the next block. Meanwhile, if the completion wait cancel command (G145) is issued in a sub part system while the calling part system is in the sub part system completion standby state, the machine will shift to a parallel processing mode. The following shows the operation and the activation timing of each part system. Calling part system O1 : G122 A100 D0 B1; (a) Start Calling part system O2 : Sub part system O100 : : : Completion wait G00 X100.; : (c) Start G122 A200 D0 B1; Completion wait (d) Waiting canceled G00 X100.; : M99; Sub part system O200 : G145; : M99; (e) Completion (b) Completion (a) (b) O1 Calling part system O100 Sub part system (c) Calling part system (d) (e) O2 O200 Sub part system : Completion wait 547 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Activation of a sub part system with parallel processing mode (D=1) If "1" is designated for command address D when the sub part system control I command is issued, the following blocks of the calling part system and the first and the following blocks of the sub part system will be operated in parallel. The following shows the operation and the activation timing of each part system. Calling part system O1 : G122 A100 D1 B1; G00 X100.; : : (a) Start Sub part system O100 : : M99; (b) Completion (a) (b) O1 Calling part system O100 Sub part system Activation of multiple sub part systems Multiple sub part systems can be activated in parallel during separate processes by calling from a single part system. The number of sub part systems to be processed simultaneously depends on the model. The following shows the operation and the activation timing of each part system. Sub part system 1 O100 : : M99; (a) Start (Parallel processing method) (c) Completion Calling part system O1 : G122 A100 D1 B1; : G122 A200 D0 B2; (b) Start (Completion wait method) O200 (d) Completion M99; Completion wait G00 X100.; : (a) (b) O1 Calling part system O100 Sub part system 1 O200 Sub part system 2 : Completion wait IB-1501278-D 548 Sub part system 2 (c) (d) : : : M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Activate a sub part system from another sub part system A sub part system can be activated from another sub part system. The number of sub part systems to be processed simultaneously depends on the model. The following shows the operation and the activation timing of each part system. Calling part system O1 : G122 A100 D0 B1; (a) Start Sub part system 1 O100 : : G122 A200 D0 B2; (b) Start Sub part system 2 O200 Completion wait Completion wait : : (c) Completion M99; (d) Completion G00 X100.; : : : M99; (a) Calling part system (b) (c) (d) O1 O100 Sub part system 1 O200 Sub part system 2 : Completion wait 549 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Sub part system activation command to a sub part system being activated If G122 is commanded while a sub part system is being activated, using the same identification No. (B command), the machine will wait for the earlier sub part system to complete activation, before activating the next sub part system. Calling part system 1 Calling part system 2 O1 : G122 A100 D0 B1; (a) Start O100 G00 X100.; (d) Start M99; O200 : : : : : : (b) G122 A200 D1 B1; : : Completion wait (c) Completion O2 Sub part system (Identification No. 1) G00 X-20.; : (e) Completion M99; (a) (b) (c) (d) O1 Calling part system 1 O2 Calling part system 2 O100 O200 Sub part system : Completion wait IB-1501278-D : Standby 550 Wait for vacancy of sub part system (e) : : : M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Operation example In the following example, the machining start timing is accelerated by controlling auxiliary axis with a sub part system and operating the main part system and the sub part system in parallel. The tool positioning starts to the machining start point at the same time (time T1) as the start of gantry retract by using sub part system completion wait cancel command (G145) in the flow from mounting the workpiece to moving to cut start position, after feeding and mounting the workpiece with the gantry, in order to reduce the cycle time. (The machine configuration below is a sample only.) [Axis configuration] Main part system ($1) : X1 axis, Z1 axis => Tool Sub part system ($2) : X2 axis, Z2 axis => Workpiece feed gantry [Machining process] (a) Feed workpiece (b) Clamp workpiece (c) Retract gantry (d) Move to cut start position (1) Machining process when sub part system control is OFF Main part system ($1) O1 : G140 X=X2 Z=Z2; ... (a) G00 X50.; G00 Z20.; M20; ... (b) G00 X0. Z0. ; ... (c) G141; G140: Arbitrary axis exchange command G141: Arbitrary axis exchange return command G00 X30. Z-15.; ... (d) M20 : M code of workpiece mounting G01 Z-20. F10.; : Main part system ($1) (a) (b) (c) (d) Time Time when gantry retract is started Time when gantry retract is completed After the gantry is retracted, cut start position is determined. 551 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control (2) Machining process when sub part system control is ON Main part system ($1) Sub part system ($2) O1 O100 G00 X50.; ... (a) G00 Z20.; M20; ... (b) G145; G00 X0. Z0.; ... (c) : M99; : : G122 A100 D0 B1; G00 X30. Z-15.; ... (d) G01 Z-20. F10.; : : M20 : M code of workpiece mounting Sub part system ($2) (a) (b) Main part system ($1) (c) (d) Time Activation of a sub part system Start of gantry retract Completion of retract : Completion wait Processes after "(c) Retract gantry" and "(d) Move to cut start position" will be operated in parallel. IB-1501278-D 552 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Relationship with Other Functions Timing synchronization with sub part system While a sub part system is under control, timing synchronization between part systems can be issued with the "![Part system No.]" command. To synchronize timing between a main part system and a sub part system, or between sub part systems, it is also possible to designate a sub part system identification No. (B command) as shown below. However, the number of part systems that can be used is limited by the specifications. ![Sub part system identification No.] For example, to synchronize timing with the calling part system, command "![0]". Note that, designate the calling part system with "![0]", not the main part system. (Example 1) and (Example 2) shown below are examples of the timing synchronization operation between the main part system ($3), sub part system 1 ($5, identification No. 1), and sub part system 2 ($6, identification No. 2). (Example 1) Timing synchronization by designating a part system No. Main part system ($3) : G122 A100 D1 B1; G122 A200 D1 B2; : !5!6; G00 X100.; : : Timing synchronization with 5th and 6th part systems Sub part system 1 ($5) !3!6; : : : : : : : Timing synchronization with 3rd and 6th part systems Sub part system 2 ($6) !3!5; : : : : : : : Timing synchronization with 3rd and 5th part systems (Example 2) Timing synchronization by designating a sub part system identification No. Main part system ($3) : G122 A100 D1 B1; G122 A200 D1 B2; : ![1]![2]; G00 X100.; : Sub part system 1 ($5, identification No. 1) ![0]![2]; : : : : : : Sub part system 2 ($6, identification No. 2) ![0]![1]; : : : : : : Timing synchronization with the following part system Timing synchronization with the following part system Timing synchronization with the following part system Sub part system of identification No. 1 Sub part system of identification No. 2 Calling part system ($3) Sub part system of identification No. 2 Calling part system ($3) Sub part system of identification No. 1 553 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Timing synchronization operation ignore signal Whether to ignore the "![Sub part system identification No.]" command or not depends on the MTB specifications. (Settings of parameter "#1279 ext15/BIT0" and the following PLC signal) Operation PLC signal for ignor#1279 ing timing synchroni- If the other part system is be- If the other part system is not being ext15/BIT0 zation between part ing activated as a sub part activated as a sub part system systems system ON 0 OFF The timing synchronization operation is ignored when activation of a sub part system is completed for the other part system. ON Ignore the timing synchronization operation. OFF Execute the timing synchronization operation between part systems. 1 Program error (P35) Tool Functions If the tool No. is changed (T command) in the program run of a sub part system, the T code data will be changed for the sub part system only. The T code data will not be changed for the main part system or other sub part systems. Tool compensation When an axis in the main part system, for which the tool compensation has been commanded, is moved to a sub part system with the arbitrary axis exchange or other operation, the tool compensation will be maintained. Also, when an axis (*1) in a sub part system, for which tool compensation has been commanded, is moved to the main part system or another sub part system with the arbitrary axis exchange operation, tool compensation will be maintained. Whether the arbitrary axis exchange function is available depends on the specifications of your machine tool. (*1) If tools are managed for each part system, when the tool compensation command is issued in a sub part system, the offset data of the sub part system will be referenced as shown below. (The setting value of the main part system will not be referenced.) Main part system ($1) Sub part system ($2) O1 O100 : G28 Z0 T01; ...(a) G90 G92 Z0; G43 Z50. H01; ...(b) G01 Z-500. F500; : G122 A100 D0 B1; G00 X10. Z50.; ...(e) : G140 X=X1; G28 X0 T02; ...(c) G90 G92 X0; G43 X10. H02; ...(d) G01 X-100. F500; : G141; M99; G140: Arbitrary axis exchange command G141: Arbitrary axis exchange return command IB-1501278-D 554 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control T code data (a) Compensation amount $1 $3 Z1 X1 1 - : : (b) 1 - L(01_$1) : (c) 1 2 L(01_$1) : (d) 1 2 L(01_$1) L(02_$3) (e) 1 2 L(01_$1) L(02_$3) L(N_$M) indicates the compensation amount of compensation No. N in the Mth part system. User macro The sub part system control I command does not affect nesting in user macros and subprograms. It can be commanded from a subprogram nested at the deepest level. Resetting (1) If the NC reset signal is input to the main part system, the operation of the main part system will be reset and end immediately. However, the operation of sub part systems will continue. The reset operation of the sub part system follows the NC reset signal of the sub part system. (2) If the NC reset signal is input to an operating sub part system, the operation of the sub part system will end immediately. Therefore, if the calling part system is in the sub part system completion standby state, the sub part system is reset, and at the same time, the calling part system cancels the standby state, and the following block will be executed. Buffer correction If both of the following conditions (1) and (2) are satisfied, the buffer correction is disabled. (The buffer correction window will not open even if the program correction key is pressed.) (1) The next block is G122 command (including "macro statement + G122 command"). (2) The program designated by G122 is the same as that of the calling part system. O100 : G00 Z50.; Buffer correction possible G00 X100.; Buffer correction impossible G122 A100 P77 D0 B1; Designated program is the program of its own part system (O100) G00 Y30.; Buffer correction possible : N77 : Program operated in sub part system M99; Machining time computation The completion wait time of the sub part system control I command (G122) will not be added to the machining time computation for the main part system. Program restart If the restart search from the block of the G122 command is attempted, a program error (P49) will occur. 555 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 16 Multi-part System Control Illegal modal of a sub part system control I command If the sub part system control I (G122) is commanded during the following G command modal, a program error (P652) will occur. User macro modal call (G66, G66.1) Fixed cycle modal High-speed machining mode (G05P1, G05P2) High-speed high-accuracy mode (G05.1Q1, G05P10000, G05P20000) Manual arbitrary reverse run The sub part system control I (G122) is ignored at the reverse run or the forward run after the reverse run. Because the sub part systems are in a mode in which reverse run is prohibited, reverse run cannot be carried out in sub part systems. Precautions (1) The sub part system control I command (G122) is a G code that must be issued alone. If it is commanded in the same block together with another G code, a program error (P651) or (P32) will occur. If another G code is commanded prior to G122 (for example, G00 G122), a program error (P651) will occur. If another G code is commanded following G122 (for example, G122 G00), a program error (P32) will occur. (2) While the sub part system I operation mode is in operation, even if the sub part system is not being activated, automatic operation cannot be started with the automatic operation start signal (ST). The stop code (0146) will be generated. However, when a sub part system is being activated, automatic operation is started with the automatic operation start signal (ST). (3) If a sub part system identification No. of its own part system is designated for the B command with the sub part system control I command (G122), a program error (P650) will occur. (4) The PLC signal of the sub part system references the state of the sub part system. (The signal state of the main part system will not be taken over.) (5) Parameters per part system of the sub part system follow the setting in the sub part system. Therefore, parameters must also be set in the sub part system. (6) If the sub part system completion wait cancel command (G145) is issued in the main part system, the program error (P34) will occur. (7) Operation executed by M80 is as follows. These parameter settings depend on the MTB specifications. Activation of a sub part system is only possible in sub part systems that are reserved using the parameter "#1483 SBS1_sys num". If the sub part system activation command is issued to a main part system (*1), an operation error (M01 1111) will occur. (*1) This refers to a case in which the Sub part system I operation mode is established (SBSM: ON) using the PLC signal before G122 is commanded. Operation searches cannot be carried out in sub part systems that are reserved using the parameter "#1483 SBS1_sys num". If the values set for the parameters "#1483 SBS1_sys num" and "#1474 SBS2_sys num" are both "1" or more, an MCP alarm (Y05 1483) will occur. IB-1501278-D 556 17 High-speed High-accuracy Control 557 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17High-speed High-accuracy Control 17.1 High-speed Machining Mode 17.1.1 High-speed Machining Mode I, II ; G05 P1, G05 P2 Function and purpose This function runs a machining program for which a freely curved surface has been approximated by fine segments at high speed. A higher fine segment processing capability leads to a faster cutting speed, resulting in a shorter cycle time and a better machining surface quality. The high-speed high-accuracy control I/II/III enable not only the high-speed machining mode but also the high-accuracy control mode. Use the high-speed high-accuracy control I/II/III for machining which needs to make an edge at a corner or reduce an error from an inner route of curved shape. This function can be used simultaneously for up to two part systems depending on the MTB specifications. kBPM, the unit for the fine segment processing capability, is an abbreviation of "kilo blocks per minute" and refers to the number of machining program blocks that can be processed per minute. In the main text, the axis address refers to the address of an axis that exits on the machine. It corresponds to the address designated in the parameters "#1013 axname" and "#1014 incax". These parameter settings depend on the MTB specifications. For one part system G01 block fine segment capacity for 1mm segment (unit: kBPM) Mode Command Maximum feedrate when 1mm segment G01 block is executed (kBPM) M850 / M830 M80 Type A Type B High-speed machining mode I G05 P1 33.7 33.7 16.8 High-speed machining mode II G05 P2 168 67.5 - Note (1) The above performance applies under the following conditions. 6-axis system (including spindle) or less 1-part system 3 axes or less commanded simultaneously in G01 The block containing only the axis name and movement amount (Macro and variable command are not included.) In the "G61.1" high-accuracy control mode or cutting mode (G64) During tool radius compensation cancel (G40) (only in the high-speed machining mode II) The parameter "#1259 set31/bit1" is set to "1". (The number of machining blocks per unit time is set to "low-speed mode".) When the above conditions are not satisfied, the given feedrate may not be secured. (2) The performance in the table may vary depending on the combination with other function. IB-1501278-D 558 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Multi-part system (high-speed machining mode II) G01 block fine segment capacity for 1mm segment (unit: kBPM) Maximum feedrate when 1mm segment G01 block is executed (kBPM) M850 / M830 M80 Type A Type B 1-part system 1 part systems 168 67.5 - (*2) 2-part system 1 part system only 100 67.5 - (*2) Two part systems simultaneously 67.5 33.7 - (*2) 4-part system Up to 16 axes 1 part system only - (*1) - (*1) - (*2) Two part systems simultaneously - (*1) - (*1) - (*2) 5 part systems or more or 17 axes or more 1 part system only - (*1) - (*1) - (*2) Two part systems simultaneously - (*1) - (*1) - (*2) (*1) This system cannot be used for this model. (*2) There are no high-speed machining mode II specifications. Note (1) The above performance applies under the following conditions. 3 axes commanded simultaneously in G01 The block containing only the axis name and movement amount (Macro and variable command are not included.) Tool radius compensation cancel (G40) mode The parameter "#1259 set31/bit1" is set to "1". (The number of machining blocks per unit time is set to "low-speed mode".) When the above conditions are not satisfied, the given feedrate may not be secured. (2) The performance in the table may vary depending on the combination with other function. (3) The number of part systems and axes that can be used depends on the specifications of your machine tool. 559 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Command format High-speed machining mode I ON G05 P1 ; High-speed machining mode II ON G05 P2 ; High-speed machining mode I/II OFF G05 P0 ; In addition to the G05 P0 command, the high-speed machining mode I is canceled when the high-speed machining mode II (G05 P2) is commanded. In reverse, the high-speed machining mode II is canceled when the high-speed machining mode I (G05 P1) is commanded. Command G05 in an independent block. A program error (P33) will occur if a movement or other command is additionally issued in a G05 command block. A program error (P33) will also occur if there is no P command in a G05 command. In addition to cancel the high-speed machining mode II, a G05 P0 command is also used to cancel the high-speed high-accuracy control II/III. Refer to "17.3 High-speed High-accuracy Control" for details. IB-1501278-D 560 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Detailed description (1) The override, maximum cutting speed clamp, single block operation, dry run, manual interruption and graphic trace and high-accuracy control mode are valid even during the high-speed machining mode I/II. For a part system that uses the high-speed machining mode II, "1" must be set for the parameter "#8040 HighSpeedAcc". By default, the high-speed machining mode II can only be used in the first part system. (2) When using the high-speed machining mode II, setting to eliminate the speed fluctuation at the seams between the arc and the straight line, or between arcs depends on the MTB specifications (parameter "#1572 Cirorp/ bit1"). (3) Combination with high-accuracy control The high-speed machining mode and high-accuracy control can be used simultaneously by taking the following steps: (a) Set "1" for the parameter "#8040 High-SpeedAcc". (b) Command "G05 P2" and "G08 P1" or "G61.1" from the machining program. The parameter "#8040 High-SpeedAcc" can be set to "1" for up to two part systems. If "0" is set for all part systems, the first and second part systems can use the high-speed machining mode and high-accuracy control simultaneously. Also refer to the following for the description of each function: High-accuracy control: "17.2 High-accuracy Control" Simultaneous usage of the high-speed machining mode and high-accuracy control: "17.3 High-speed Highaccuracy Control" (4) While high-speed machining mode II is valid, the following variable commands or operation commands can be designated following the axis address. When other variable commands or operation commands are issued, highspeed machining mode II is canceled temporarily. (a) Referencing common variables or local variables Common variables or local variables can be referenced (example: X#500, Y#1, Z##100, A#[#101], etc.). (b) Four basic arithmetic rule Four basic arithmetic rule (+, -, *, /) operations are available, and also the operation priority can be designated using parentheses ( ) ([#500+1.0]*#501, etc.). Program example High-speed machining mode I G28 X0. Y0. Z0. ; G91 G00 X-100. Y-100. ; G01 F10000 ; G05 P1 ; High-speed machining mode I ON : X0.1 Y0.01 ; X0.1 Y0.02 ; X0.1 Y0.03 ; : G05 P0 ; High-speed machining mode I OFF M30 ; 561 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Relationship with other functions Relationship between the high-speed machining mode II and G code functions Column A: Operation when the additional function is commanded while the high-speed machining mode II is enabled Column B: Operation when the high-speed machining mode II (G05P2) is commanded while the additional function is enabled ○: The high-speed machining mode II and the additional function are both enabled ∆: The high-speed machining mode II is temporarily canceled, while the additional function is enabled x: Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination □: Others Group 0 IB-1501278-D G code Function name A B G04 Dwell ∆ - G05P0 High-speed machining mode II OFF High-speed high-accuracy control II OFF High-speed high-accuracy control III OFF □ (*1) □ (*2) G05P2 High-speed machining mode II ON □ (*3) □ (*3) G05P10000 High-speed high-accuracy control II ON □ (*2) □ (*2) G05P20000 High-speed high-accuracy control III ON □ (*2) □ (*3) G05.1Q0 High-speed high-accuracy control I OFF Spline interpolation OFF □ (*3) □ (*2) G05.1Q1 High-speed high-accuracy control I ON □ (*2) □ (*2) G05.1Q2 Spline interpolation ON ○ ○ G07 Hypothetical axis interpolation ∆ ∆ G08P0 High-accuracy control OFF □ (*3) □ (*2) G08P1 High-accuracy control ON □ (*4) □ (*4) G09 Exact stop check ∆ - G10 I_J_ G10 K_ Parameter coordinate rotation input ∆ - G10 L2 Compensation data input by program ∆ - G10 L70 G10 L50 Parameter input by program ∆ - G27 Reference position check ∆ - G28 Reference position return ∆ - G29 Start position return ∆ - G30 2nd to 4th reference position return ∆ - G30.1G30.6 Tool change position return ∆ - G31 Skip Multiple-step skip 2 ∆ - G31.1G31.3 Multi-step skip ∆ - G34-G36 G37.1 Special Fixed Cycle ∆ - G37 Automatic tool length measurement ∆ - G38 Tool radius compensation vector designation ∆ - G39 Tool radius compensation corner circular command - 562 ∆ M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Group 0 1 G code Function name A B G52 Local coordinate system setting ∆ - G53 Machine coordinate system selection ∆ - G60 Unidirectional positioning ∆ - G65 User macro simple call □ (*5) □ (*6) G92 Coordinate system setting ∆ - G92.1 Workpiece coordinate preset ∆ - G122 Sub part system control I X (P652) □ (*7) G00 Positioning ∆ ∆ G01 Linear interpolation ○ ○ G02 G03 Circular interpolation ○ ○ G02.1 G03.1 Spiral interpolation ∆ ∆ G02.3 G03.3 Exponential interpolation ∆ ∆ G02.4 G03.4 3-dimensional circular interpolation ∆ ∆ G06.2 NURBS interpolation ○ ○ G33 Thread cutting ∆ ∆ 2 G17 to G19 Plane selection ○ ○ 3 G90 Absolute value command ○ ○ G91 Incremental value command ○ ○ G22 Stroke check before travel ON ∆ ∆ G23 Stroke check before travel OFF ○ ○ G93 Inverse time feed ∆ ∆ G94 Asynchronous feed (feed per minute) ○ ○ 4 5 G95 Synchronous feed (feed per revolution) ∆ ∆ 6 G20 Inch command ○ ○ G21 Metric command ○ ○ 7 G40 Tool radius compensation cancel ○ ○ G41 G42 Tool radius compensation ○ ○ G43 G44 Tool length offset ○ ○ G43.1 Tool length compensation along the tool axis ○ ○ G43.4 G43.5 Tool center point control ○ ○ G49 Tool length offset cancel ○ ○ G80 Fixed cycle cancel ○ ○ ∆ ∆ 8 9 Group 9 Fixed cycle Other than G80 563 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Group 10 11 12 13 14 G code Function name A B G98 Fixed cycle initial level return ○ ○ G99 Fixed cycle R point return ○ ○ G50 Scaling cancel ○ ○ G51 Scaling ON ∆ ∆ G54 to G59 G54.1 Workpiece coordinate system selection ○ ○ G61 Exact stop check mode ∆ ∆ G61.1 High-accuracy control ○ ○ G61.2 High-accuracy spline ○ ○ G62 Automatic corner override ∆ ∆ G63 Tapping mode ∆ ∆ G64 Cutting mode ○ ○ G66 G66.1 User macro modal call ∆ ∆ G67 User macro modal call ○ ○ Cancel 15 16 17 18 19 21 24 27 G40.1 Normal line control cancel ○ ○ G41.1 G41.2 Normal line control X (P29) X (P29) G68 Coordinate rotation by program ON ∆ ∆ G68.2 G68.3 Inclined surface machining command ○ ○ G69 Coordinate rotation cancel ○ ○ G96 Constant surface speed control ON ○ ○ G97 Constant surface speed control OFF ○ ○ G15 Polar coordinate command OFF ○ ○ G16 Polar coordinate command ON ∆ ∆ G50.1 Mirror image OFF ○ ○ G51.1 Mirror image ON ○ ○ G07.1 Cylindrical interpolation X (P34) X (P481) G12.1 Polar coordinate interpolation ON X (P34) X (P481) G13.1 Polar coordinate interpolation OFF ○ ○ G188 Dynamic M/L program changeover ○ ○ G189 Dynamic M/L program changeover cancel ○ ○ G54.4P0 Workpiece installation error compensation ○ cancel ○ G54.4 P1 to P7 Workpiece installation error compensation ○ ○ (*1) Disables the high-speed machining mode II. (*2) Enables the high-speed machining mode II. (*3) High-speed machining mode II continues. (*4) Enables the high-speed machining mode II and high-accuracy control. (*5) Enables the high-speed machining mode II in a macro program. (*6) Enables the high-speed machining mode II if G05P2 is commanded in a macro program. (*7) Enables the high-speed machining mode II if G05P2 is commanded in a sub part system. IB-1501278-D 564 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Relationship between the high-speed machining mode II and functions other than G codes Column A: Operation when the additional function is commanded while the high-speed machining mode II is enabled Column B: Operation when the high-speed machining mode II (G05P2) is commanded while the additional function is enabled ○: The high-speed machining mode II and the additional function are both enabled ∆: The high-speed machining mode II is temporarily canceled, while the additional function is enabled x: Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination □: Others Function name A B SSS ON - ○ Mirror image by parameter setting ON - ∆ PLC mirror image ON - ∆ Coordinate rotation by parameter - ∆ Subprogram call (M98) □ (*8) □ (*9) Figure rotation (M98 I_J_K_) □ (*15) □ (*16) Timing synchronization between part sys- □ (*10) tems - MTB macro □ (*11) □ (*12) Macro interruption □ (*13) □ (*14) Corner chamfering/Corner R ∆ - Linear angle command ∆ - Geometric command ∆ - Chopping ○ ○ Fairing/ smooth fairing ON ○ ○ Optional block skip ○ - (*8) Enables the high-speed machining mode II in a subprogram. (*9) Enables the high-speed machining mode II if G05P2 is commanded in a subprogram. (*10) Enables timing synchronization. (*11) Enables the high-speed machining mode II in a MTB program. (*12) Enables the high-speed machining mode II if G05P2 is commanded in a MTB program. (*13) Enables the high-speed machining mode II in an interrupt program. (*14) Enables the high-speed machining mode II if G05P2 is commanded in an interrupt program. (*15) Disables the high-speed machining mode II in a figure rotation subprogram. (*16) The high-speed machining mode II is disabled even if G05P2 is commanded in a figure rotation subprogram. 565 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Precautions (1) If "G05 P1(P2)" is commanded when the high-speed machining mode I/(II) specifications are not provided, a program error (P39) will occur. (2) The automatic operation process has priority in high-speed machining mode I/II, and as a result, the screen display may slow down. (3) The speed will decelerate once at the G05 command block, so turn ON and OFF when the tool separates from the workpiece. (4) When carrying out operations in high-speed machining mode I/II by communication or tape mode, the machining speed may be suppressed depending on the program transmission speed limit. (5) Command G05 in an independent block. (6) A decimal point is invalid for the P address in the G05 command block. (7) The P addresses, which are valid in the G05 command block, are P0, P1 and P2 only. If other P addresses are commanded, a program error (P35) will occur. If there is no P command, a program error (P33) will occur. (8) The machining speed may be suppressed depending on the number of characters in one block. IB-1501278-D 566 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.2 High-accuracy Control 17.2.1 High-accuracy Control ; G61.1, G08 Function and purpose Machining errors caused by delays in control systems can be inhibited. This function is useful for machining which needs to make an edge at a corner or reduce an error from an inner route of curved shape. In high-accuracy control, acceleration/deceleration is performed not to cause machining error by pre-reading blocks and acceleration/deceleration is automatically performed according to a machining shape so that the machining error is inhibited with minimizing an extension of machining time. High-accuracy control OFF NC command High-accuracy control ON NC command Corner shape Machining program commanded shape Machining program commanded shape Machining program commanded shape Machining program commanded shape NC command NC command Curve shape Commands to enable high-accuracy control are as follows: High-accuracy control command (G08P1/G61.1) High-speed high-accuracy control I command (G05.1Q1) High-speed high-accuracy control II/III command (G05P10000/G05P20000) High-accuracy spline interpolation command (G61.2) This function uses the following functions to minimize the increase in machining time while reducing the shape error. (1) Acceleration/deceleration before interpolation (2) Optimum speed control (3) Vector accuracy interpolation (4) Feed forward (5) S-pattern filter control In the main text, the axis address refers to the address of an axis that exits on the machine. It corresponds to the address designated in the parameters "#1013 axname" and "#1014 incax". These parameter settings depend on the MTB specifications. 567 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Command format High-accuracy control valid G61.1 ; or, G08 P1; High-accuracy control invalid G08 P0 ; or, G command in G code group 13 except G61.1 High-accuracy control can be canceled with either command regardless of the command that has enabled the control. Note (1) After "G08 P1" is commanded, G code group 13 is automatically switched to the G61.1 modal. If the high-accuracy control mode is canceled by the "G08 P0" command, G code group 0 is switched to the "G08P0" modal and G code group 13 becomes the "commanded mode". IB-1501278-D 568 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Detailed description (1) Feedrate command F is clamped with the "#2110 Clamp (H-precision)" (Cutting feed clamp speed for high-accuracy control mode) set with parameter. (2) Rapid traverse rate enables "#2109 Rapid(H-precision)" (Rapid traverse rate during high-accuracy control mode) set by the parameter. (3) When the "#2109 Rapid(H-precision)" is set to "0", the movement follows "#2001 rapid" (rapid traverse rate) set by the parameter. Also, when "#2110 Clamp (H-precision)" is set to "0", the speed will be clamped with "#2002 clamp" (Cutting clamp speed) set with parameter. (4) The modal holding state of the high-accuracy control mode depends on the MTB specifications (combination of the parameters "#1151 rstint" (reset initial) and "#1148 I_G611" (initial high-accuracy)). Parameter Default state Resetting Reset initial (#1151) Initial highaccuracy (#1148) Power ON Reset 1 OFF OFF OFF Hold ON Reset 2 Reset & rewind OFF OFF OFF ON ON Hold ON ON ON Parameter Emergency stop Emergency stop cancel Reset initial (#1151) Initial highaccuracy (#1148) Emergency stop switch or external emergency stop Emergency stop switch or external emergency stop OFF OFF Hold Hold ON OFF OFF ON Hold Hold ON ON Parameter Reset initial (#1151) Initial highaccuracy (#1148) OFF OFF Block interruption Block stop NC alarm OT Mode changeover (automatic/manual) or feed hold Single block Servo alarm H/W OT Hold ON OFF ON ON Hold: Modal hold ON: Switches to the high-accuracy control mode As for G61.1, the mode is switched to the high-accuracy mode, even if the other modes (G61 to G64) are valid. OFF: The status of the high-accuracy control mode is OFF. 569 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Acceleration/deceleration before interpolation Acceleration/deceleration control is carried out for the movement commands to suppress the impact and to smooth out the velocity waveform when the machine starts or stops moving. However, if high-accuracy control is disabled, the corners at the block seams are rounded, and path errors occur regarding the command shape because acceleration/deceleration is performed after interpolation. In the high-accuracy control function mode, acceleration/deceleration is carried out before interpolation to solve the above problems. This acceleration/deceleration before interpolation enables machining with a faithful path to the commanded shape of the machining program. Furthermore, the acceleration/deceleration time can be reduced because the constant inclination acceleration/deceleration is performed for the acceleration/deceleration before interpolation. (1) Basic patterns of acceleration/deceleration control in linear interpolation commands Acceleration/deceleration waveform pattern Normal mode (F) clamp (T) G1tL (a) Because of the acceleration/deceleration that controls the acceleration/deceleration time to achieve the commanded speed at a constant level (constant time constant acceleration/deceleration), the acceleration/deceleration becomes more gentle as the command speed becomes slower (the acceleration/deceleration time does not change). (b) The time to achieve the commanded speed (G1tL) can be set independently for each axis. Note, however, that an arc shape will be distorted if the time constant differs among the base axes. G1tL: G1 time constant (linear) (MTB-specified parameter #2007) High-accuracy control mode (F) clamp G1bF G1bF/2 (T) G1btL/2 G1btL (F) Combined speed (T) Time (a) Because of the acceleration/deceleration that controls the acceleration/deceleration time to achieve the maximum speed (G1bF) set by a parameter at a constant level (constant inclination type linear acceleration/deceleration), the acceleration/deceleration time is reduced as the command speed becomes slower. (b) Only one acceleration/deceleration time constant (common for each axis) exists in a system. G1bF: Maximum speed (MTB-specified parameter #1206) G1btL: Time constant (MTB-specified parameter #1207) <Note> G1bF and G1btL are values for specifying the inclination of the acceleration/deceleration time. The actual cutting feed maximum speed is clamped by the "#2002 clamp" value. IB-1501278-D 570 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (2) Path control in circular interpolation commands When commanding circular interpolation with the conventional post-interpolation acceleration/deceleration control method, the path itself that is output from the NC to the servo runs further inside the commanded path, and the circle radius becomes smaller than that of the commanded circle. This is due to the influence of the smoothing course droop amount for NC internal acceleration/deceleration. With the pre-interpolation acceleration/deceleration control method, the path error is eliminated and a circular path faithful to the command results, because interpolation is carried out after the acceleration/deceleration control. Note that the tracking lag due to the position loop control in the servo system is not the target here. The following shows a comparison of the circle radius reduction error amounts for the conventional post-interpolation acceleration/deceleration control and pre-interpolation acceleration/deceleration control in the high-accuracy control mode. Machining program commanded shape R Actual tool path R F R : Commanded radius (mm) ∆R: Circle radius reduction error amount (mm) F: Cutting feedrate (mm/min) If an arc is commanded by a machining program as shown above, the error ∆R occurs for the commanded shape on the actual tool path. In the normal mode (acceleration/deceleration after interpolation), ∆R is caused by acceleration/deceleration of NC and lag of servo system. High-accuracy control (acceleration/deceleration before interpolation), however, can eliminate errors caused by acceleration/deceleration of NC. By additionally using the feed forward control, it is also possible to reduce errors caused by lag of servo system. The compensation amount of the circle radius reduction error (∆R) is theoretically calculated as shown in the following table. Post-interpolation acceleration/deceleration con- Pre-interpolation acceleration/deceleration control (normal mode) trol (high-accuracy control mode) Linear acceleration/deceleration 1 1 F ∆R = 2R 12 Ts 2 + Tp2 60 Linear acceleration/deceleration 2 1 ∆R = 2R Tp2 1 - Kf 2 Exponential function acceleration/deceleration 1 ∆R = 2R Ts2 + Tp2 F 60 2 F 60 2 (a) Because the item Ts can be ignored by using the pre-interpolation acceleration/deceleration control method, the radius reduction error amount can be reduced. (b) Item Tp can be negated by making Kf = 1. Ts: Acceleration/deceleration time constant in the NC (s) Tp: Servo system position loop time constant (s) (inverse number to "#2203 PGN1") Kf: Feed forward coefficient Kf = fwd_g / 1000 (fwd_g: #2010 Feed forward gain) 571 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Optimum speed control When the moving direction is changed on the corner, arc, etc., acceleration corresponding to the amount of change and the feedrate is generated. When the acceleration is large, there is a possibility of machine vibration and it may leave stripes on the machining surface. In the high-accuracy control mode, the deceleration control (optimum speed control) is performed to keep the generated acceleration under the allowance that has been designed with the parameter so that the problem mentioned above can be solved. The optimum speed control suppresses the machine vibration and enables highly accurate machining while minimizing the extension of cycle time. Corner deceleration Consists of optimum corner deceleration and tolerable acceleration control for each axis. Arc speed clamp Controls deceleration so that the combined acceleration on an arc is kept below the tolerable acceleration common to all axes. This can suppress path errors (circle radius reduction error amount) on an arc to a certain level. (1) Optimum corner deceleration Highly accurate edge machining can be achieved by controlling deceleration so that the combined acceleration at the seam between blocks is kept under the tolerable acceleration common to all axes, which is determined by "#1206 G1bF (maximum speed)", "#1207 G1btL (time constant)", and accuracy coefficient. When entering in a corner, optimum speed for the corner (optimum corner speed) is calculated from the angle with the next block (corner angle) and the tolerable acceleration common to all axes. The machine decelerates to the speed in advance, and then accelerates back to the command speed after passing the corner. Y axis When a corner with the corner angle θ is passed F : Speed before entering the corner at speed F, the acceleration ∆F occurs according F : Speed after passing to θ and F. corner F : Acceleration at the corner X axis The corner speed F is controlled so that ∆F generated above does not exceed the tolerable acceleration common to all axes. The speed pattern is as shown on the left. Synthesis rate F0 = F0x2 + F0y2 Time X-axis speed F0x2 Time Y-axis speed F0y2 Time IB-1501278-D 572 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Optimum corner deceleration is not carried out when blocks are smoothly connected, because deceleration is not necessary. The criteria for whether the connection is smooth or not can be designated by the machining parameter "#8020 DCC ANGLE". If the corner angle is equal to or less than the corner deceleration angle, the connection is judged to be smooth and optimum corner deceleration is not carried out. The edge accuracy can be further improved by setting a greater accuracy coefficient. A greater accuracy coefficient, however, reduces the optimum corner speed, which may increase the cycle time. Setting a negative accuracy coefficient can increase the optimum corner speed and reduce the cycle time. As shown below, different accuracy coefficients can be used depending on the parameter "#8021 COMP_CHANGE", and the tolerable acceleration common to all axes can be obtained with the following formula: #8021 COMP CHANGE Accuracy coefficient used 0 #8019 R COMP 1 #8022 CORNER COMP Tolerable acceleration for all axes (mm/s2) = G1bF(mm/min) G1btL(ms) * 60 * 1000 * 100 - R COMP 100 The corner speed V0 can be maintained at more than a certain speed so that the corner speed does not drop too far. Set "#2096 crncsp (corner deceleration minimum speed)" for each axis, and make a combined speed so that the moving axis does not exceed this setting. Speed is not clamped Speed is clamped (a) (c) V (a) (b) (a) Corner deceleration speed (b) Clamp value according to X axis (c) Y axis setting value (d) X axis setting value (d) Note that the speed is controlled with the optimum corner deceleration speed in the following cases. When the combined corner deceleration speed is equal to or less than the optimum corner deceleration speed When the corner deceleration minimum speed parameter setting for the moving axes is set to "0" for even one axis. 573 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (2) Tolerable acceleration control for each axis (optimum acceleration control) The acceleration to be generated at a seem between blocks is evaluated for each axis to control deceleration so that the seam is passed at the optimum speed. This enables highly accurate edge machining. The optimum deceleration speed is calculated so that the acceleration of each axis to be generated at the seam is equal to or less than the tolerable acceleration for each axis, which is determined by "#2157 G1bFx" (maximum speed for each axis), "#2158 G1btLx" (time constant for each axis), and the accuracy coefficient. The machine decelerates to the speed in advance, and then accelerates back to the command speed after passing the corner. This control enables deceleration at an appropriate speed for the characteristics of each axis even when machine vibrations may easily occur due to a low tolerable acceleration for a specific axis (rotary axis). This means that the deceleration speed can be raised at a corner where acceleration is generated only for an axis with a high tolerable acceleration, leading to a reduced cycle time. If acceleration is generated for the X axis (linear axis) as shown in Figure (a) below or for the C axis (rotary axis) as shown in Figure (b), the corner speed F is controlled so that the acceleration to be generated at the X or C axis does not exceed the tolerable acceleration for the X or C axis, respectively. If the tolerable acceleration for the X axis is higher than that for the C axis, a higher deceleration speed can be used for a path where acceleration is generated only for the X axis than where acceleration is generated only for the C axis. In this case, the speed patterns are as shown in Figures (c) and (d) below: C axis F : Speed after passing the corner F: Acceleration at the corner C axis F : Speed before entering the corner F : Speed after passing the corner F : Speed before entering the corner F : Acceleration at the corner X axis X axis (a) Corner shape which generates the acceleration on X axis (linear axis) Synthesis rate (b) Corner shape which generates the acceleration on C axis (rotary axis) Synthesis rate F0 = F0x2 + F0c2 F0 = F0x2 + F0y2 Time X-axis speed Time Controls the acceleration generated on X-axis speed X axis to be the X-axis tolerable acceleration or less. F0x2 Time F0x2 C-axis speed C-axis speed F0c2 F0c2 Time Controls the acceleration generated on C axis to be the C-axis tolerable acceleration or less. Time Time (c) Speed pattern which generates the acceleration on X axis (linear axis) IB-1501278-D (d) Speed pattern which generates the acceleration on C axis (rotary axis) 574 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Deceleration is not carried out when blocks are smoothly connected (when the acceleration to be generated for each axis is equal to or lower than the tolerable acceleration for each axis). The edge accuracy can be further improved by setting a greater accuracy coefficient. A greater accuracy coefficient, however, reduces the optimum corner speed, which may increase the cycle time. Setting a negative accuracy coefficient can increase the optimum corner speed and reduce the cycle time. As shown below, different accuracy coefficients can be used depending on the parameter "#8021 COMP_CHANGE". Also, the tolerable acceleration can be adjusted for each axis using "#2159 compx" (accuracy coefficient for each axis), and the tolerable acceleration for each axis can be obtained with the following formula. It is necessary, however, to set the same tolerable acceleration for all base axes because an arc shape is distorted if it differs among them. If G1bFx is 0 (not set), the tolerable acceleration is calculated using "#2001 rapid" (rapid traverse rate). And if G1btLx is 0 (not set), the tolerable acceleration is calculated using "#2004 G0tL" (G0 time constant (linear)). If G1bFx and G1btLx are 0 for all base axes, the tolerable accelerations for the base axes are unified to the lowest one. #8021 COMP CHANGE Accuracy coefficient used 0 #8019 R COMP 1 #8022 CORNER COMP Tolerable acceleration for each axes (mm/s2) = G1bFx(mm/min) G1btLx(ms) * 60 * 1000 * 575 100 - R COMP 100 * 100 - compx 100 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (3) Arc speed clamp During circular interpolation, even when moving at a constant speed, acceleration is generated as the advance direction constantly changes. When the arc radius is large enough in relation to the commanded speed, control is carried out at the commanded speed. However, when the arc radius is relatively small, the speed is clamped so that the generated acceleration does not exceed the tolerable acceleration/deceleration speed before interpolation, calculated with the parameters. This allows arc cutting to be carried out at an optimum speed for the arc radius. The figure below shows the acceleration ∆F (mm/s²) for movement at the constant speed F (mm/min) on an arc shape with the radius R (mm). Here, the arc clamp speed F' (mm/min) that makes the acceleration ∆F lower than the tolerable acceleration common to all axes Ac (mm/s²) can be obtained with the following formula: F : Commanded speed (mm/min) R : Commanded arc radius (mm) F ∆θ : Angle change per interpolation unit F ∆F : Speed change per interpolation unit F R F F The tool is fed with the arc clamp speed F' so that ∆F does not exceed the tolerable acceleration common to all axes Ac (mm/s²). R*Ac*60 F' F' = G1bF(mm/min) G1btL(ms) When the above F' expression is substituted with F in the expression for the maximum logical arc radius reduction error amount ∆R, explained in the section "Pre-interpolation acceleration/deceleration", the commanded radius R is eliminated, and ∆R does not rely on R. Here, Tp is the servo system position loop time constant (s) and Kf is the feed forward coefficient. Tp is the inverse number to "#2203 PGN1" (position loop gain) (Tp = 1 / PGN1) and Kf is a ratio of "#2010 fws_g" (feed forward gain) (Kf = fwd_g / 100), both of which depend on the MTB specifications. ∆R : Arc radius reduction error amount 2 1 F Tp : Position loop gain time constant of servo system 2 2 R 2R Tp 1 - Kf 60 Kf : Feed forward coefficient F : Cutting feedrate AC 2 2 Tp 1 Kf 2 In other words, with an arc command to be clamped at the arc clamp speed, in logical terms regardless of the commanded radius R, machining can be carried out with a radius reduction error amount within a constant value. The roundness can be further improved by setting a greater accuracy coefficient. A greater accuracy coefficient, however, reduces the arc clamp speed, which may increase the cycle time. Setting a negative accuracy coefficient can increase the arc clamp speed and reduce the cycle time. As shown below, different accuracy coefficients can be used depending on the parameter "#8021 COMP_CHANGE", and the tolerable acceleration common to all axes can be obtained with the following formula: #8021 COMP CHANGE Accuracy coefficient used 0 #8019 R COMP 1 #8023 CURVE COMP Tolerable acceleration for all axes (mm/s2) IB-1501278-D = G1bF(mm/min) G1btL(ms) 576 * 60 * 1000 * 100 - R COMP 100 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Vector accuracy interpolation When a fine segment is commanded and the angle between the blocks is extremely small (when not using optimum corner deceleration), interpolation can be carried out more smoothly using the vector accuracy interpolation. Vector accuracy interpolation Commanded path Feed forward control This function reduces path errors caused by delay of servo systems. Path errors caused by acceleration/deceleration of NC can be eliminated by acceleration/deceleration before interpolation, however errors caused by delay of servo systems cannot be eliminated by acceleration/deceleration before interpolation. Therefore, when the arc shape of radius R (mm) is machined at speed F (mm/min) as the figure (a)below, for instance, the lag time occurs between the NC commanded speed and the actual tool speed in amount of the servo system time constant and the path error ∆R (mm) occurs. Feed forward control generates the command value taking the delay of servo systems as shown in figure (b)below so that the path error caused by delay of servo systems can be inhibited. Speed NC commanded shape F R Delay of servo ΔR NC commanded speed Actual tool speed Time Actual tool path (a) NC command and actual tool movement during Feed forward control OFF Speed NC commanded speed is set forward according to a expected delay. (Feed forward control) NC commanded shape Time Actual tool path Actual tool speed (corresponding to original NC commanded speed) 577 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (b) NC command and actual tool movement during Feed forward control ON R= 1 2R 1 - Kf Tp F 60 Here, Tp is the servo system position loop time constant (s) and Kf is the feed forward coefficient. Tp is the inverse number to "#2203 PGN1" (position loop gain) (Tp = 1 / PGN1) and Kf is a ratio of "#2010 fws_g" (feed forward gain) (Kf = fwd_g / 100), both of which depend on the MTB specifications. Combination with the smooth high gain (SHG) control function Feed forward control can inhibit path errors more effectively by increasing the feed forward coefficient. In some cases, however, the coefficient cannot be increased because a greater coefficient may cause machine vibrations. In this case, use this function together with the smooth high gain (SHG) control function to stably compensate path errors caused by lag of servo system. To enable the SHG control, it is also necessary to set "#2204 PGN2" (position loop gain 2) and "#2257 SHGC SHG" (control gain) in addition to "#2203 PGN1" (position loop gain 1), all of which depend on the MTB specifications. By enabling the SHG control, it is possible to inhibit path errors, for example, for an arc shape equivalently as with conventional control (SHG control OFF) using the equivalent feed forward gain fwd_g as shown in the following formula. This means that setting fwd_g = 50 (%) for the SHG control is as effective as setting fwd_g = 100 (%) for conventional control in inhibiting path errors. fwd _ g' = 100 1- 1- fwd _ g 100 1 2 S-pattern filter control S-pattern filter (soft acceleration/deceleration filter) is the function that inhibits the machine vibration by smoothing a velocity waveform. There are following types of S-pattern filters: G01/G00 S-pattern filter G01/G00 jerk filter S-pattern filter 2 Smoothing velocity waveform of inclination-constant linear acceleration/deceleration inclination-constant linear acceleration/ deceleration Making velocity waveform of S-pattern filter even smoother S-pattern filter Interpolation (axis distribution) Jerk filter Axis speed Synthesis rate Synthesis rate Time IB-1501278-D Synthesis rate Time Axis speed Time 578 Smoothing each axis speed after interpolation S-pattern filter 2 Axis speed Time Time Time Time Axis speed M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (1) G01/G00 S-pattern filter This function inhibits the machine vibration by smoothing a velocity waveform generated by inclination-constant linear acceleration/deceleration. Inclination-constant linear acceleration/deceleration generates continuous velocity waveforms, but makes the acceleration discontinuous. As a result, machine vibrations may easily occur when there are discontinuities in acceleration, which may cause scratches or streaks on the machining surface. The S-pattern filter can make the velocity waveform even smoother and eliminate acceleration discontinuities to inhibit machine vibrations. The Spattern filter does not impair machining accuracy because it makes the combined speed smoother before interpolation. A greater S-pattern filter time constant, however, may increases the cycle time. To the S-pattern filter time constant, "#1568 SfiltG1" is applied during cutting feed (G01) or "#1569 SfiltG0" during rapid traverse (G00), each of which can be set in the range of 0 to 200 (ms). (2) G01/G00 jerk filter The jerk filter function inhibits machine vibrations by eliminating jerk discontinuities when the S-pattern filter alone cannot inhibit such vibrations. Through the S-pattern filter, continuous velocity waveforms can be obtained up to acceleration, but jerk discontinuities remain. The jerk filter further filters the velocity waveform smoothed by the S-pattern filter to smooth jerk as well to inhibit machine vibrations. The jerk filter does not impair machining accuracy because it makes the combined speed smoother before interpolation. To the jerk filter time constant, "#12051 Jerk_filtG1" is applied during cutting feed (G01) or "#12052 Jerk_filtG0" during rapid traverse (G00), each of which can be set in the range of 0 to 50 (ms). Even if a jerk filter time constant is set, the S-pattern filter time constant is the time to achieve the target acceleration. As a result, the time constant for S-pattern filter processing is "S-pattern filter time constant" - "Jerk filter time constant". If the jerk filter time constant is greater than the S-pattern filter time constant, an MCP alarm (Y51 0030) will occur. Constant inclination linear acceleration/deceleration Speed Machine vibration is likely to occur Acceleration Time S-pattern filter Jerk filter Speed Speed Acceleration Time Time Acceleration Time Time Tsfilt - Tjerk Jerk Time Tsfilt Jerk Jerk Time Time Time Tjerk Tsfilt: S-pattern filter time constant Tjerk: Jerk filter time constant 579 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (3) S-pattern filter 2 This function inhibits machine vibrations by smoothing slight speed fluctuation caused when the combined speed is distributed to each axis element. S-pattern filter 2 can inhibit machine vibrations by smoothing slight speed fluctuation on each axis. The function, however, may impair machining accuracy because it filters each axis speed after interpolation. A greater S-pattern filter 2 time constant, however, may increases the cycle time. To the S-pattern filter 2 time constant, "#1570 Sfilt2" is applied, which can be set in the range of 0 to 200 (ms). (4) How to adjust parameters (a) The table below shows typical initial values for each filter time constant. If your machine's natural angular frequency fn (Hz) is known, vibrations can be inhibited effectively by setting the vibration period Tn (ms) obtained with the following formula for the S-pattern filter time constant: Tn = 1000 (ms) fn S-pattern filter Jerk filter (SfiltG1/SfiltG0) 50ms S-pattern filter (Jerk_filtG1/Jerk_filtG0) 0ms (Sfilt2) 10ms (b) If vibrations cannot be inhibited properly with the above initial values, increase the S-pattern filter time constant. Or, decrease the S-pattern filter time constant to reduce the cycle time. (c) If vibrations occur at a corner or other section and stripes remain on the machining surface even after the Spattern filter time constant is increased, increase the S-pattern filter 2 time constant. The maximum S-pattern filter 2 time constant, however, should be 20 to 25 ms because a greater S-pattern filter 2 time constant may impair machining accuracy. (d) If high-frequency machine vibrations remain even after the S-pattern filter/S-pattern filter 2 are applied, set the jerk filter time constant. If a shorter cycle time has a priority over the machining accuracy, it is possible to inhibit vibrations at a corner by reducing the corner accuracy coefficient to increase the corner deceleration speed and increasing the S-pattern filter 2 time constant. IB-1501278-D 580 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Relationship with other functions (1) The modal must be set as shown below when commanding G08 P1/G61.1. Function G code Cylindrical interpolation cancel (*1) G07.1 Polar coordinate interpolation cancel (*1) G15 Tool radius compensation mode cancel G40 Tool length compensation cancel G49 Normal line control cancel G40.1 Programmable mirror image OFF G50.1 Mirror image with settings Cancel Mirror image with signals Cancel No macro modal call G67 Feed per revolution cancel G94 Constant surface speed control mode cancel G97 Interruption type macro mode cancel M97 (*1) These functions can be commanded if the tolerable acceleration control for each axis (optimum acceleration control) or variable-acceleration pre-interpolation acceleration/deceleration specifications are valid. (2) A program error will occur if high-accuracy control is commanded in the following modes. During milling -> Program error (P481) During cylindrical interpolation -> Program error (P481) (*2) During polar coordinate interpolation -> Program error (P481) (*2) During normal line control -> Program error (P29) (3) A program error (P29) will occur if the following commands are issued during the high-accuracy control mode. Milling Cylindrical interpolation (*2) Polar coordinate interpolation (*2) Normal line control (*2) An error will not occur if the tolerable acceleration control for each axis (optimum acceleration control) or variable-acceleration pre-interpolation acceleration/deceleration specifications are valid. 581 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Operation when high-accuracy control-related G commands are combined The table below shows operations when following high-accuracy control-related commands are combined: G61.1, G8P1 : High-accuracy control G64 : Cutting mode G61 : Exact stop check mode G62 : Automatic corner override G63 : Tapping mode G61.2 : High-accuracy spline interpolation G08P0 : High-accuracy control cancel (cutting mode) G05.1Q1 : High-speed high-accuracy control I G05.1Q2 : Spline interpolation G05P2 : High-speed machining mode II G05P10000 : High-speed high-accuracy control II G05P20000 : High-speed high-accuracy control III A G61.1/G08P1 G61.2 IB-1501278-D B Operation when B is commanded during A command G61.1 Continues high-accuracy control. G61, G62, G63, G64 Cancels high-accuracy control and operates in the commanded mode. G61.2 Operates in the high-accuracy spline interpolation mode. G8P1 Continues high-accuracy control. G8P0 Cancels high-accuracy control. (Changes G code group 13 to G64.) G05.1Q1 Operates in the high-speed high-accuracy control I mode. G05.1Q2 A program error (P34) will occur. G05P2 Operates in high-accuracy control + high-speed machining mode II. G05P10000 Operates in the high-speed high-accuracy control II mode. G06.2 A program error (P34) will occur. G61.1 Operates in the high-accuracy control mode. G61, G62, G63, G64 Operates in the commanded mode. G61.2 Continues high-accuracy spline interpolation. G08P1 Operates in the high-accuracy control mode. G08P0 A program error (P29) will occur. G05.1Q1 A program error (P29) will occur. G05.1Q2 A program error (P34) will occur. G05P2 Operates in high-accuracy spline interpolation + high-speed machining mode II. G05P10000 A program error (P29) will occur. G06.2 A program error (P34) will occur. 582 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control A G05.1Q1 G05P10000 B G61.1 Operation when B is commanded during A command Continues the high-speed high-accuracy control I mode. G64 Continues the high-speed high-accuracy control I mode. G61, G62, G63 Operates in the high-speed high-accuracy control I + commanded mode. G61.2 A program error (P29) will occur. G08P1 Continues the high-speed high-accuracy control I mode. G08P0 Continues the high-speed high-accuracy control I mode. G05.1Q1 Continues the high-speed high-accuracy control I mode. G05.1Q2 A program error (P34) will occur. G05P2 Operates in the high-speed machining mode II. G05P10000 A program error (P34) will occur. G06.2 A program error (P34) will occur. G61.1 Continues the high-speed high-accuracy control II mode. G64 Continues the high-speed high-accuracy control II mode. G61, G62, G63 Operates in the high-speed high-accuracy control II + commanded mode. G61.2 A program error (P29) will occur. G08P1 Continues the high-speed high-accuracy control II mode. G08P0 Continues the high-speed high-accuracy control II mode. G05.1Q1 A program error (P34) will occur. G05.1Q2 Operates in the high-speed high-accuracy control II mode + spline interpolation G05P2 Operates in the high-speed machining mode II. G05P10000 Continues the high-speed high-accuracy control II mode. G06.2 Operates in the NURBS interpolation mode. 583 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Precautions (1) The "high-accuracy control" specifications are required to use this function If G61.1 is commanded when there are no specifications, a program error (P123) will occur. (2) The high-accuracy control function is internally enabled by the high-speed high-accuracy I/II/III (G5.1Q1/ G5P10000) command. If the high-speed high-accuracy I/II/III is commanded in the high-accuracy control mode, the high-speed high-accuracy I/II/III mode is enabled. Then, if the high-speed high-accuracy I/II/III mode is canceled, the high-accuracy control mode is restored. (3) In the high-accuracy control mode, feedrate command F is clamped with the "#2110 Clamp (H-precision)" (Cutting feed clamp speed for high-accuracy control mode) set with parameter. When the cutting feed clamp speed for the high-accuracy control mode is 0, however, it is clamped with the "#2002 clamp" cutting clamp speed set by the parameter. (4) In the high-accuracy control mode, rapid traverse rate conforms to "#2109 Rapid(H-precision)" (Rapid traverse rate during high-accuracy control mode) set by the parameter. When the rapid traverse rate during the high-accuracy control mode is set to "0", however, the movement follows "#2001 rapid" set by the parameter. (5) If the specifications for the multi-part system simultaneous high-accuracy control are not provided, the "#1205 G0bdcc" (G0 pre-interpolation) can be used with only one part system. If the 2nd or later part system is set to the G0 pre-interpolation acceleration/deceleration, an MCP alarm (Y51 0017) will occur. (6) "#1568 SfiltG1", "#1569 SfiltG0" and "#1570 Sfilt2" cannot be changed from the screen during program mode. If these parameters is changed by "parameter input by program", these parameters become valid from the next block. (7) If Reset or Emergency signal is input during axis travel, it takes a time equal to the time constant to recover from the reset or emergency stop state. (8) When there are high-accuracy acceleration/deceleration time constant expansion specifications, the sampling buffer area may be smaller. (9) The high-accuracy control time constant expansion specifications can only be used for a 1-part system. In a multi-part system, the high-accuracy acceleration/deceleration time constant expansion specifications are disabled even when they are set to ON. (10) For a part system where high-accuracy control is to be commanded, set the number of axes in the part system to 8 or less. If high-accuracy control is commanded for a part system that has 9 or more axes, an operation error (M01 0135) will occur. The error will not occur, however, if the number of axes in the part system excluding the master axis/slave axis is 8 or less during the synchronous control/control axis synchronization between part systems. (11) Even if the parameter "#1210 RstGmd" (modal G code reset setting) is set to "not to initialize group 13 at reset", group 13 is initialized according to the setting of "#1148 I_G611" (Initial hi-precis) if it is enabled. To retain group 13 at reset, set "#1148 I_G611" to "0". These parameters depend on the MTB specifications. (12) If the parameter "#1205 G0bdcc" (G0 acceleration/deceleration before interpolation) is set to "1", the value set with the parameter "#2224 SV024" (in-position detection width) will be used as the in-position width. The setting of the parameter "#2077 G0inps" (G0 in-position width) and the programmable in-position check with ",I" address are disabled. IB-1501278-D 584 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.2.2 SSS Control Function and purpose This function runs a machining program that approximates a freely curved surface with fine segment lines at high speed and with high-level accuracy. This function enables machining with less scratches and streaks on the cutting surface compared to the conventional high-accuracy control function. With conventional high-accuracy control, the angle between two blocks is compared with the corner deceleration angle to determine whether to execute corner deceleration between the blocks. This can cause the speed to suddenly change between the blocks with an angle close to the corner deceleration angle, resulting in scratches or streaks. The SSS (Super Smooth Surface) control uses information on not only the angle but also global paths between two blocks to provide optimum speed control that is not significantly affected by minute stepping or waviness. The favorable effects of this control include a reduction in the number of scratches or streaks on cutting surfaces. The SSS control has the following features: (1) This function is effective at machining smooth-shaped dies using a fine segment program. (2) This function provides speed control that is not susceptible to errors in paths. (3) Even if corner deceleration is not required, the speed is clamped if the predicted acceleration is high. (The clamp speed can be adjusted using the parameter "#8092 ClampCoeff".) The length of the path direction recognized with SSS control can be adjusted with the machining parameter "#8091 reference length". The range is increased as the setting value increases, and the effect of the error is reduced. If the multi-part system simultaneous high-accuracy specification is provided, up to two part systems can be used at the same time. Note (1) The use of this function requires the following functions, in addition to the SSS control specifications. Make sure that these specifications are enabled before using this function. High-accuracy control (G61.1/G08P1) High-speed high-accuracy control I (G05.1 Q1) High-speed high-accuracy control II (G05 P10000) High-speed high-accuracy control III (G05 P20000) 585 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Detailed description When the parameters are set as below, each of the following high-accuracy control commands is activated under SSS control. <Parameter> "#8090 SSS ON" ON <Command format of the modes activated under SSS control>" [High-accuracy control] G61.1 ; or G08P1; High-accuracy control ON G08P0; or, G command in group 13 except G61.1 High-accuracy control OFF [High-speed high-accuracy control I] G05.1 Q1 ; High-speed high-accuracy control I ON G05.1 Q0 ; High-speed high-accuracy control I OFF [High-speed high-accuracy control II] G05 P10000 ; High-speed high-accuracy control II ON G05 P0 ; High-speed high-accuracy control II OFF [High-speed high-accuracy control III] G05 P20000 ; High-speed high-accuracy control III ON G05 P0 ; High-speed high-accuracy control III OFF "SSS" is displayed on the modal display screen under SSS control. However "SSS" is not displayed when a command being executed is out of the scope of SSS control. Adjustment of accuracy coefficient The clamp speed at a corner and arc can be adjusted using "#8022 CORNER COMP" and "#8023 CURVE COMP" (If "#8021 COMP_CHANGE" is set to "0", use "#8019 R COMP" to adjust the clamp speed at a corner and arc). When "#8096 Deceler. coeff. ON" is set to "1", "#8097 Corner decel coeff" and "#8098 Arc clamp spd coef" become valid during SSS control. Using these parameters, you can use different corner deceleration speeds and clamp speeds at arcs according to whether or not the SSS control is enabled. For parameters #8097 and #8098, respectively, set a percentage ratio to the level of the relevant speed that is applied when the SSS control is disabled. Parameter Item to be adjusted #8097 Corner decel coeff Corner deceleration speed to be applied when the SSS control is enabled #8098 Arc clamp spd coef Arc clamp speed to be applied when the SSS control is enabled (Example) When "#8097 Corner decel coeff" is set to 200 (%), the corner deceleration speed that is applied when the SSS control is enabled becomes twice the corner deceleration speed that is applied when the SSS control is disabled. When setting the parameters, adjust the values within the range in which the machine does not vibrate. IB-1501278-D 586 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Parameter standard values The standard values of the parameters related to SSS control are shown below. (1) User parameters # Item Standard value 8090 SSS ON 8091 StdLength 1 8092 ClampCoeff 8093 StepLeng 8094 DccWaitAdd 0 8096 Deceler. coeff. ON 1 8097 Corner decel coeff 300 8098 Arc clamp spd coef 100 8019 R COMP 0 8020 DCC ANGLE 10 1.000 1 0.005 8021 COMP CHANGE 1 8022 CORNER COMP 0 8023 CURVE COMP -20 8034 AccClampt ON 0 8036 CordecJudge 0 8037 CorJudgeL 0 <Note> Reference items for adjusting the parameter The relationship between each parameter, accuracy and speed is shown below. The accuracy and speed required for machining can be adjusted with these settings. When setting the parameters, adjust the values within the range in which the machine does not vibrate. Parameter Adjustment target Effect #8022 CORNER COMP Accuracy at corner section Large setting = Accuracy increases, speed drops #8023 CURVE COMP Accuracy at curve section Large setting = Accuracy increases, speed drops #8092 ClampCoeff Accuracy at curve section Large setting = Accuracy drops, speed increases <Note> Usually use the standard value and adjust with "#8023". (2) Basic specification parameters (depend on the MTB specifications) # Item Standard value 1148 I_G611 Initial high-accuracy 0 1206 G1bf Acceleration/deceleration before interpolation Maximum speed - 1207 G1btL Acceleration/deceleration before interpolation Time constant - 1571 SSSdis SSS control adjustment coefficient fixed value selection 0 1572 Cirorp Arc command overlap 0 1568 SfiltG1 G1 soft acceleration/deceleration filter 0 1569 SfiltG0 G0 soft acceleration/deceleration filter 0 1570 Sfilt2 Soft acceleration/deceleration filter 2 0 (3) Axis specification parameters (depend on the MTB specifications) # Item Standard value 2010 fwd_g Feed forward gain 70 2068 G0fwdg G00 feed forward gain 70 2096 crncsp Minimum corner deceleration speed 0 587 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control SSS control parameter [Range for recognizing the shape] #1571 SSSdis #8091 StdLength Movement command [Measure for step] #8093 StepLeng Set the value approximately the same as the CAM path difference (tolerance) for the parameter. #8093 StepLeng [Acceleration/deceleration process] Feedrate Seam between blocks Clamp speed = theory deceleration speed (after adding accuracy coefficient)×√#8092 ClampCoeff Time #8094 DccWaitAdd Able to wait for deceleration by setting the extra time when the speed feedback does not drop to the clamp speed. Precautions (1) Pre-reading is executed during SSS control, so a program error could occur before the block containing the error is executed. (2) Buffer correction is not guaranteed during SSS control. (3) If automatic/manual simultaneous or automatic handle feed interrupt are used during SSS control, the machining accuracy will not be guaranteed. (4) If a fine arc command is issued during SSS control, it may take longer to machine. (5) The same path as single block operation will be used during graphic check. (6) The line under the cutting feedrate and arc command block are subjected to the speed control in the SSS control. The command blocks that are not subjected to speed control, decelerate first and automatically switch the SSS control ON and OFF. (7) SSS control is temporally disabled in the following modal: NURBS interpolation Polar coordinate interpolation Cylindrical interpolation User macro interruption enable (M96) Feed per revolution (synchronous feed) Inverse time feed Constant surface speed control Fixed cycle 3-dimensional coordinate conversion Hypothetical axis interpolation Automatic tool length measurement Tool length compensation along the tool axis (8) There are some restrictions for each high-accuracy control. Refer to each section for restrictions. "17.2 High-accuracy Control" "17.3 High-speed High-accuracy Control" (9) Fairing is disabled during the SSS control. IB-1501278-D 588 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.2.3 Tolerance Control Function and purpose This function obtains the optimum clamp speed for corners or curves based on the designated tolerance to perform operations. It also ensures smooth passing within the tolerance range in corner sections, which suppresses machine vibrations. This means that the clamp speed can be increased to reduce the cycle time. This function allows the machine to operate with the optimum tool path and speed, simply by specifying the tolerance, so an operator can easily carry out high quality machining. The tolerance refers to the allowable error amount between the path commanded in the machining program and the path output by NC. The validity of this function depends on the MTB specifications. This function also requires the SSS control specifications because it can only be used under SSS control. Program command path Path commanded by NC to drive unit Tool path Tolerance control: Invalid Tolerance control: Valid This function is enabled when the following conditions are satisfied: (1) The tolerance control specification is valid. (Based on the MTB specifications.) (2) The parameter "#8090 SSS ON" is set to "1". (3) The parameter "#12066 Tolerance ctrl ON" is set to "1". (*1)(*2) (4) High-accuracy control (G61.1/G08P1), spline interpolation (G61.2/G05.1Q2), spline interpolation 2 (G61.4), or high-speed high-accuracy control I/II/III (G05.1Q1/G05P10000/G05P20000) is valid. (*1) Even if conditions (1) and (3) are satisfied, an operation error (M01 0139) will occur and the cycle start cannot be performed automatically if the parameter "#8090 SSS ON" is set to "0". In this case, enable SSS control and reset the alarm to start the cycle automatically. (*2) A setting error will occur if "1" is set when this specification is invalid. 589 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Command format Set the tolerance with the parameter "#2659 tolerance" or the ",K" address following the G code (G61.1 or G61.4 command). When the setting value is "0", this function runs with "0.01(mm)". Tolerance specification G61.1 or G61.4 ,K__ ; ,K Tolerance (mm) The range of the command value is 0.000 to 100.000. If a value exceeding the range is commanded, a program error (P35) will occur. The tolerance designated by ",K" is applied to all axes in the part system. When "0" is designated or ",K" is omitted, the program runs based on the value of the parameter "#2659 tolerance". The tolerance designated by ",K" is not held after reset. Therefore, if ",K" is not designated in the G61.1 or G61.4 command after reset, the axis runs based on the value of the parameter "#2659 tolerance". Note (1) The G61.4 command requires the specifications of spline interpolation 2. Detailed description The axis moves in the designated tolerance range during tolerance control. The tolerance on the corner shape is as shown on the right. Speed control The clamp speed is obtained from the tolerance in the corner or curve section during tolerance control. As the designated tolerance is lower, the axis speed decelerates. Tolerance: High Tolerance: Low Command path Synthesis rate Time IB-1501278-D 590 Time M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Parameters valid during tolerance control The parameters valid and invalid during tolerance control are as follows. Some parameters depend on the MTB specifications. (1) Valid parameters No. Parameter name 1206 G1bF 1207 G1btL 1568 SfiltG1 12051 Jerk_filtG1 2659 tolerance Supplements When combining with the variable-acceleration pre-interpolation acceleration/deceleration or tolerable acceleration control for each axis, specify parameters "#2157 G1bFx" and "#2158 G1btLx". (2) Invalid parameters (Parameters with no setting required) No. 1570 Parameter name Supplements Sfilt2 Ignored even if the value is entered. 2159 compx 8019 R COMP Ignored even if the value is entered. The clamp speed is obtained from the tolerance during tolerance control; therefore, parameters for adjusting the clamp speed are not required. 8020 DCC ANGLE 8021 COMP CHANGE 8022 CORNER COMP 8023 CURVE COMP 8096 Deceler. coeff. ON 8097 Corner decel coeff 8098 Arc clamp spd coef Program example : G91 ; G61.1 ,K0.02; Designate tolerance 0.02 (mm). G01 X0.1 Z0.1 F1000 ; X0.1 Z-0.2 ; Y0.1 ; Tolerance: 0.02 (mm) G61.1 ,K0; Designate tolerance 0 (mm). X-0.1 Z-0.05 ; X-0.1 Z-0.3 ; Tolerance: Follows parameter "#2659 tolerance". G64 ; : 591 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Precautions (1) While tolerance control is valid, tolerance control may be canceled temporarily depending on some commands. If tolerance control is canceled temporarily, the axis moves to the commanded position without taking an inner route in a corner section. After this, when a temporary cancel cause is removed, tolerance control restarts. The temporary cancel conditions are as follows. (a) Modal in which the group 1 command is not G01 (linear interpolation) or G02/G03 (circular interpolation). (b) Under single block operation (c) Modal in which SSS control is disabled temporarily (Modal shown below) NURBS interpolation Polar coordinate interpolation Cylindrical interpolation User macro interruption enable (M96) Feed per revolution (Synchronous feed) Inverse time feed Constant surface speed control Fixed cycle 3-dimensional coordinate conversion Hypothetical axis interpolation Automatic tool length measurement Tool length compensation along the tool axis Normal line control Unidirectional positioning Exponential interpolation 3-dimensional circular interpolation (2) The stored stroke limit's prohibited range is determined based on the program command path. As a result, machining may not be stopped even if the command moved inward by tolerance control enters the prohibited range. (3) If a feed hold signal is turned ON at a corner, machining stops on the program command path. This means that it does not stop at point A in the figure below but at point B. Program command path Path without a feed hold signal Path when a feed hold signal is turned ON at a corner A IB-1501278-D B 592 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.2.4 Variable-acceleration Pre-interpolation Acceleration/Deceleration Function and purpose This function is useful when each axis differs in the characteristics (responsiveness) (4-axis/5-axis machine, etc.). The normal acceleration/deceleration before interpolation performs the acceleration/deceleration by setting acceleration common to all axes. Therefore, if the high responsiveness and low responsiveness coexist in axes, the acceleration needs to be set to suit the axis with low responsiveness. On the other hand, the variable-acceleration pre-interpolation acceleration/deceleration can perform the acceleration/deceleration by setting diverse acceleration to each axis. This means that it is possible to set a higher acceleration for axes with high responsiveness than before. Therefore, the acceleration for the axis with high responsiveness can be larger than before so that cycle time can be reduced especially in the indexing machining. (Refer to following figure.) The validity of this function depends on the MTB specifications. This function also requires the SSS control specifications because it can only be used under SSS control. Synthesis rate Variable-acceleration pre-interpolation acceleration/deceleration Acceleration/deceleration before interpolation Time Rotary axis Linear axis Shortened This function is enabled when the following conditions are satisfied: (1) The variable-acceleration pre-interpolation acceleration/deceleration specification is valid. (Based on the MTB specifications.) (2) The MTB-specific parameter has been set (#12060 VblAccPreInt). (*1) (3) Under SSS control (*2) (*1) A setting error will occur if "1" is set when this specification is invalid. (*2) The validity of the SSS control function depends on the MTB specifications. To enable SSS control, it is necessary to set the parameter "#8090 SSS ON" to "1" to command high-accuracy control. (*3) Even if conditions (1) and (2) are satisfied, an operation error (M01 0136) will occur and the cycle start cannot be performed automatically if the parameter "#8090 SSS ON" is set to "0". In this case, enable SSS control and reset the alarm to start the cycle automatically. "VAC" is displayed on the operation screen and modal display under variable-acceleration pre-interpolation acceleration/deceleration. 593 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Detailed description The acceleration for each axis is determined in the MTB specifications (parameters "#2157 G1bFx" (maximum speed for each axis) and "#2158 G1btLx" (axis time constant)). For an axis with G1bFx = 0 (not set), the acceleration is calculated using "#1206 G1bF" (maximum speed). And for an axis with G1btLx = 0 (not set), the acceleration is calculated using "#1207 G1btL" (time constant). Therefore, if G1bFx and G1btLx are 0 (not set) for all axes, the normal acceleration/deceleration before interpolation is performed. The following shows examples of settings. Set linear axis acceleration for "#1206 G1bF" and "#1207 G1btL". #1206 G1bF 10000 (mm/min) #1207 G1btL 100 (ms) It is assumed that only the acceleration for the rotary axis is set for "#2157 G1bFx" and "#2158 G1btLx". ("#1206 G1bF" and "#1207 G1btL" are used by not setting the acceleration for the linear axis.) X Y Z C #2157 G1bFx 0 (not set) 0 (not set) 0 (not set) 10000 (mm/min) #2158 G1btLx 0 (not set) 0 (not set) 0 (not set) 500 (ms) The figure below shows movements with the above settings. (1) If only the X axis moves, acceleration/deceleration is performed at the acceleration set for the X axis. ... (a) (2) If only the C axis moves, acceleration/deceleration is performed at the acceleration set for the C axis. ... (d) (3) If both of the X and C axes move, acceleration/deceleration is performed at the optimum acceleration calculated within the range that the acceleration of each axis does not exceed the setting. If the movement of the X axis is dominant ... (b) If the movement of the C axis is dominant ... (c) (a) (b) (c) (d) Acceleration : Large Synthesis rate Acceleration : Small Synthesis rate Time Synthesis rate Time Synthesis rate Time X-axis speed X axis speed X-axis speed X axis speed Time C-axis speed Time C-axis speed Time C-axis speed Time Time Time IB-1501278-D 594 Time C-axis speed Time Time M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Precautions (1) Under variable-acceleration pre-interpolation acceleration/deceleration, corner deceleration is realized with tolerable acceleration control for each axis. Corner deceleration patterns and acceleration/deceleration patterns are as follows with each parameter setting: #12060 VblAccPreInt 0 0 1 1 0 1 0 1 Variable-acceleration Pre-interpolation Acceleration/Deceleration ON #12053 EachAxAccCntrl Tolerable acceleration control for each axis ON Corner deceleration pattern Optimum corner Tolerable acceleration control for each axis deceleration Acceleration/deceleration pattern Acceleration/deceleration before interpolation Variable-acceleration pre-interpolation acceleration/deceleration (2) This function can only be used under SSS control. This means that variable-acceleration pre-interpolation acceleration/deceleration is also disabled during a modal that temporarily disables SSS control. As a result, the tool is under tolerable acceleration control for each axis. In this mode, the acceleration is determined by "#1206 G1bF" and "#1207 G1btL". Out of #2157 and #2158, set the longer one for #1206 and #1207. (Make a note of the original values and restore them as necessary.) Refer to "17.2.2 SSS Control" for modals that temporarily disable SSS control. (3) Basically, set the same acceleration for base axes I, J, and K. A different acceleration causes a distorted shape against an arc command. The figure below shows an example where the acceleration in the Y direction is greater than that in the X direction. Actual tool path Machining program commanded shape Y X 595 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.2.5 Initial High-accuracy Control If "#1148 I_G611" (Initial high-accuracy) is set by the MTB specifications, high-accuracy control-related functions can be enabled when the power is turned ON. At power ON, the modes set by this parameter are enabled, but each mode can be changed to a different one by commanding as follows in the machining program. #1148 setting value Modes enabled at power ON 0 G08P0/G64 (cutting mode) command 1 G08P1/G61.1 (high-accuracy control mode) command 2 G05.1Q1 (high-speed high-accuracy control I mode) command 3 G05P10000 (high-speed high-accuracy control II mode) command 4 G05P20000 (high-speed high-accuracy control III mode) command It is impossible, however, to shift to the high-speed high-accuracy control II/high-speed high-accuracy control III mode during the high-speed high-accuracy control I. Likewise, it is also impossible to shift to the high-speed highaccuracy control I mode during the high-speed high-accuracy control II/high-speed high-accuracy control III mode. To shift to either mode, cancel the current high-speed high-accuracy control mode using "G05.1 Q0" or "G05 P0" first and then command the target mode. If any function set by this parameter is not included in your machine's specifications, an available high-accuracy function with a number smaller than the parameter setting is enabled. IB-1501278-D 596 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.2.6 Multi-part System Simultaneous High-accuracy Function and purpose High-accuracy control and high-speed machining mode are available respectively in all part systems, however, the simultaneous usage of high-accuracy control and high-speed machining mode (including High-speed high-accuracy control I/II/III) are available only in part systems which are limited by the parameter "#8040 High-SpeedAcc". While high-accuracy control and high-speed machining mode are available simultaneously in a part system where this parameter is set to "1", a program error (P129) will occur in those where the parameter is set to "0" when commanded. Also, for part systems where "#8040 High-SpeedAcc" is set to "0", "#1148 I_G611" must be set to "0" (Cutting mode when the power is turned ON) or "1" (High-accuracy control mode when the power is turned ON). If the parameter "#1148 I_G611" is set to a value other than "0" and "1", the parameter is regarded as being set to "1". Note that up to two part systems can be set to use high-accuracy control and high-speed machining mode simultaneously. If three or more part systems are set as such, an MCP alarm (Y51 0032) will occur. If the parameter "#8040 High-SpeedAcc" is set to "0" for all part systems, the simultaneous usage of high-accuracy control and high-speed machining mode is available in the 1st and 2nd part systems. Up to 2 part systems can be set to "1" $1 High-speed high-accuracy enabled part system = 1 $2 High-speed high-accuracy enabled part system = 1 G28 X0 Y0; G08P0 G05P0 G28 X0 Y0; G08P0 G05P0 G08 P1; G08P1 G05 P10000; G08P1 G05P2 G05 P2; G91 G01 F3000; G05P2 G91 G01 F3000; X1.; : High-speed high-accuracy : : : : : : G05P0; G08 P0; High-speed high-accuracy : : G05P0 G08P0 G05P0; M02; G08P0 G05P0 M02; $3 High-speed high-accuracy enabled part system = 0 $4 High-speed high-accuracy enabled part system = 0 G28 X0 Y0; G08P0 G05P0 G28 X0 Y0; G08P0 G05P0 G08 P1; G08P1 G05 P10000; G08P1 G05P2 Alarm : G08 P0; G91 G01 F3000; G08P0 G05 P2; X1.; : G05P2 : G08 P1; : G08P1 Alarm : : : G08 P0; : G05 P0; G05P0; M02; M02; (Note) It is limited also in G61.1 command. 597 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Although some MTB specifications support the high-accuracy acceleration/deceleration time constant expansion specifications, only one part system can be used. Multi-part systems cannot be used even if the high-accuracy acceleration/deceleration time constant expansion specifications are valid. For multi-part systems, "#1207 G1btL" must be set to a value within the setting range that is applicable when there are no high-accuracy acceleration/deceleration time constant expansion specifications. Refer to the following chapters for details of each high-accuracy control. "17.2 High-accuracy Control" "17.3 High-speed High-accuracy Control" Detailed description (1) When "#1148 I_G611" (Initial hi-precis) is enabled, the initial modal state after power ON will be the high-accuracy control mode. Refer to "17.2.5 Initial High-accuracy Control" for details. In this case, the high-accuracy control mode is enabled if the multi-part system simultaneous high-accuracy specification is provided. Otherwise, the 1st part system enters the high-accuracy control mode, but the 2nd part system enters the cutting mode. (2) If you use the high-accuracy acceleration/deceleration time constant expansion function together with the multipart system simultaneous high-accuracy function, an MCP alarm (Y51 0020) will occur. Make sure to disable the high-accuracy acceleration/deceleration time constant extension function when you use the multi-part system simultaneous high-accuracy function. IB-1501278-D 598 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.3 High-speed High-accuracy Control It depends on the MTB specifications whether the modal state at power ON is high-speed high-accuracy control I, II, III, or OFF. It also depends on the specifications whether to hold the modal state at reset. Refer to the specifications of your machine. In the main text, the axis address refers to the address of an axis that exits on the machine. It corresponds to the address designated in the parameters "#1013 axname" and "#1014 incax". These parameter settings depend on the MTB specifications. 17.3.1 High-speed High-accuracy Control I, II, III ; G05.1 Q1/Q0, G05 P10000/P0, G05 P20000/P0 Function and purpose This function runs a machining program that approximates a freely curved surface with fine segments at high speed and with high-level accuracy. This is effective in increasing the speed of machining dies of a freely curved surface. This function is useful for machining which needs to make an edge at a corner or reduce an error from an inner route of curved shape. A higher fine segment processing capability leads to a faster cutting speed, resulting in a shorter cycle time and a better machining surface quality. kBPM, the unit for the fine segment processing capability, is an abbreviation of "kilo blocks per minute" and refers to the number of machining program blocks that can be processed per minute. Fine segment capacity for 1-part system G01 block fine segment capacity for 1mm segment (unit: kBPM) The performance below applies under the following conditions. 6-axis system (including spindle) or less 1-part system 3 axes or less commanded simultaneously in G01 The block containing only the axis name and movement amount (Macro and variable command are not included.) Tool radius compensation cancel mode (G40) The parameter "#1259 set31/bit1" is set to "1". (The number of machining blocks per unit time is set to for "low-speed mode".) When the above conditions are not satisfied, the given feedrate may not be secured. Fine segment capacity M850 / M830 Restriction in the program M80 Type A Type B High-speed high-accuracy function I mode 67.5 33.7 16.8 Yes High-speed high-accuracy function II mode 168 (*1) 67.5 - Yes High-speed high-accuracy function III mode 270 (*1) 135 - Yes (*1) When the fairing is valid (When the parameter "#8033" is set to "1"), and the fairing is executed successively, depending on machining programs, the performance of fine segment execution may decelerate more than the value described in the above table. In the network connection, the value described in the above table may not be guaranteed depending on the state. 599 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Fine segment capacity for multi-part system G01 block fine segment capacity for 1mm segment (unit: kBPM) The fine segment processing capability below applies under the following conditions. 3 axes or less commanded simultaneously in G01 The block containing only the axis name and axis movement amount (Macro and variable command are not included.) Tool radius compensation OFF (G40) The parameter "#1259 set31/bit1" is set to "1". (The number of machining blocks per unit time is set to for "low-speed mode".) When the above conditions are not satisfied, the given feedrate may not be secured. (1) High-speed high-accuracy control I Number of part systems/num- Number of part systems ber of axes M850 / M830 (#8040=1) 67.5 M80 Type A Type B 33.7 16.8 1-part system 1 part systems 2-part system 1 part systems 67.5 33.7 16.8 2 part systems 33.7 33.7 16.8 4-part system 1 part systems - (*1) - (*1) - (*1) Up to 16 axes 2 part systems - (*1) - (*1) - (*1) 5 part systems or more or 17 axes or more 1 part systems - (*1) - (*1) - (*1) 2 part systems - (*1) - (*1) - (*1) (2) High-speed high-accuracy control II Number of part systems/num- Number of part systems ber of axes M850 / M830 (#8040=1) M80 Type A Type B 1-part system 1 part systems 168 (*3) 67.5 - (*2) 2-part system 1 part systems 100 67.5 - (*2) 2 part systems 67.5 67.5 - (*2) 4-part system 1 part systems - (*1) - (*1) - (*2) Up to 16 axes 2 part systems - (*1) - (*1) - (*2) 5 part systems or more or 17 axes or more 1 part systems - (*1) - (*1) - (*2) 2 part systems - (*1) - (*1) - (*2) (3) High-speed high-accuracy control III Number o\f part systems/num- Number of part systems ber of axes M850 / M830 (#8040=1) 1-part system 1 part systems 2-part system 1 part systems 2 part systems M80 Type A Type B 135 - (*2) 168 135 - (*2) 100 67.5 - (*2) 270 4-part system 1 part systems - (*1) - (*2) - (*2) Up to 16 axes 2 part systems - (*1) - (*2) - (*2) 5 part systems or more or 17 axes or more 1 part systems - (*1) - (*2) - (*2) 2 part systems - (*1) - (*2) - (*2) (*1) This system cannot be used for this model. (*2) There are no corresponding high-speed high-accuracy control specifications. (*3) 100 kBPM for a time constant expansion system. (The time constant expansion system is available when its specifications are enabled and it is a 1-part system.) IB-1501278-D 600 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control High-speed high-accuracy control simultaneously for two part systems High-speed high-accuracy control I, II, III can be used simultaneously in up to two part systems. High-speed high-accuracy control I, II, III can be used in a part system where "1" is set for the parameter "#8040 High-SpeedAcc". A program error occurs (P129) if this is commanded for a part system where "0" is set for the parameter. If the parameter "#8040 High-SpeedAcc" is set to "0" for all part systems, only the first part system is handled as the one with the parameter set to "1". Also, a part system where the parameter "#1148 Initial hi-precis" is set to "2" to "4" is handled as the one with the parameter "#8040 High-SpeedAcc" set to "1". The parameter "#8040 High-SpeedAcc" can be set to "1" for up to two part systems. If 3 or more part systems are set to "1", an MCP alarm (Y51 0032) occurs. When "1" is set for two part systems, the fine segment processing capability decreases compared to when "1" is set only for one part system. Command format G05.1 Q1 ; High-speed high-accuracy control I ON G05.1 Q0 ; High-speed high-accuracy control I OFF G05 P10000 ; High-speed high-accuracy control II ON G05 P20000 ; High-speed high-accuracy control III ON G05 P0 ; High-speed high-accuracy control II/III OFF Note (1) The high-speed high-accuracy mode II and III cannot be used at the same time. (2) These commands are valid regardless of the parameter "#1267 ext03/bit0" setting if the specifications are available. (3) High-speed high-accuracy control III can also be used by setting a parameter instead of a G code. If the parameter "#8131 High-speed high-accuracy control 3" is set to "1", the high-speed high-accuracy control II command can be handled as the III command. This also enables the high-speed high-accuracy control III mode in the machining program using "G05P10000". Likewise, the G05P2 command issued during a high-accuracy control mode can be handled as the high-speed high-accuracy control III command. Furthermore, by setting "#1148 Initial hi-precis" to "4", the high-speed high-accuracy control III mode can be set as the initial modal state after power ON. 601 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Detailed description (1) The high-speed high-accuracy control I / II / III can be used during tape, MDI, SD card or memory modes. (2) The override, maximum cutting speed clamp, single block operation, dry run, handle interrupt and graphic trace are valid even during the high-speed high-accuracy control I / II / III modal. (3) The machining speed may drop depending on the number of characters in one block. (4) The high-speed high-accuracy control I / II / III function automatically turns the high-accuracy control mode ON. For high-accuracy control function, refer to "17.3 High-speed High-accuracy Control". (5) Turn the tool radius compensation command ON and OFF during the high-speed high-accuracy control I/II/III mode. If the high-speed high-accuracy control I/II/III mode is turned OFF without turning the tool radius compensation OFF, a program error (P34) will occur. (6) Turn the high-speed high-accuracy control I / II / III mode OFF before commanding data other than those that can be commanded. (7) When using the high-speed high-accuracy control II / III mode, it is necessary to set the parameter "#1572 Cirorp" to eliminate the speed fluctuation at the seams between arc and straight line or arc and arc. This parameter, however, depends on the MTB specifications. (8) Feedrate command F is clamped with the "#2110 Clamp (H-precision)" (Cutting feed clamp speed for high-accuracy control mode) set with parameter. (9) Rapid traverse rate enables "#2109 Rapid(H-precision)" (Rapid traverse rate during high-accuracy control mode) set by the parameter. (10) When the "#2109 Rapid(H-precision)" is set to "0", the movement follows "#2001 rapid" (rapid traverse rate) set by the parameter. Also, when "#2110 Clamp (H-precision)" is set to "0", the speed will be clamped with "#2002 clamp" (Cutting clamp speed) set with parameter. Enabling conditions To enable each high-speed high-accuracy control function, it is necessary to satisfy the following conditions respectively: (1) The specification of each function is valid. (*1) (2) Each function is in a valid modal state. (Refer to "Relationship with other functions".) (3) Each function is enabled by one of the following procedures: Command each in the machining program. (*2) Set each for the parameter "#1148 Initial hi-precis". (The modal at power ON corresponds to each highspeed high-accuracy control function.) #1148 setting High-speed high-accuracy control I 2 High-speed high-accuracy control II 3 High-speed high-accuracy control III 4 (*1) The following conditions are additionally required to enable high-speed high-accuracy control III. The time constant expansion system is invalid. The SSS control specifications are valid, and the parameter "#8090 SSS ON" is set to "1". If high-speed high-accuracy control III is commanded when the SSS control mode is set to OFF, high-speed high-accuracy control II is enabled. (*2) High-speed high-accuracy control III is also enabled by the following commands. While the parameter "#8131 High-speed high-accuracy control III" is set to "1", command "G05 P10000" (highspeed high-accuracy control II) from the machining program. IB-1501278-D 602 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Relationship with other functions Relationship between the high-speed high-accuracy control I and other functions (1) Relationship between the high-speed high-accuracy control I and G code functions Column A: Operation when the additional function is commanded while the high-speed high-accuracy control I is enabled Column B: Operation when the high-speed high-accuracy control I (G05.1Q1) is commanded while the additional function is enabled ○: The high-speed high-accuracy control I and the additional function are both enabled ∆: The high-speed high-accuracy control I is temporarily canceled, while the additional function is enabled X: Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination □: Others Group 0 G code Function name A B G04 Dwell ∆ - G05P0 High-speed machining mode II OFF High-speed high-accuracy control II OFF High-speed high-accuracy control III OFF X (P34) □ (*2) G05P2 High-speed machining mode II ON □ (*4) □ (*2) G05P10000 High-speed high-accuracy control II ON X (P34) X (P34) G05P20000 High-speed high-accuracy control III ON X (P34) X (P34) G05.1Q0 High-speed high-accuracy control I OFF Spline interpolation OFF □ (*1) □ (*2) G05.1Q1 High-speed high-accuracy control I ON □ (*3) □ (*3) G05.1Q2 Spline interpolation ON X (P34) X (P34) G07 Hypothetical axis interpolation ∆ ∆ G08P0 High-accuracy control OFF □ (*3) □ (*2) G08P1 High-accuracy control ON □ (*3) □ (*2) G09 Exact stop check ∆ - G10 I_J_ G10 K_ Parameter coordinate rotation input ∆ - G10 L2 Compensation data input by program ∆ - G10 L70 G10 L50 Parameter input by program ∆ - G27 Reference position check ∆ - G28 Reference position return ∆ - G29 Start position return ∆ - G30 2nd to 4th reference position return ∆ - G30.1G30.6 Tool change position return ∆ - G31 Skip Multiple-step skip 2 ∆ - G31.1G31.3 Multi-step skip ∆ - G34-G36 G37.1 Special Fixed Cycle ∆ - 603 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Group 0 1 G code Function name B G37 Automatic tool length measurement ∆ - G38 Tool radius compensation vector designation ∆ - G39 Tool radius compensation corner circular command ∆ - G52 Local coordinate system setting ∆ - G53 Machine coordinate system selection ∆ - G60 Unidirectional positioning ∆ - G65 User macro simple call □ (*5) □ (*6) G92 Coordinate system setting ∆ - G92.1 Workpiece coordinate preset ∆ - G122 Sub part system control I X (P652) □ (*7) G00 Positioning ∆ ∆ G01 Linear interpolation ○ ○ G02 G03 Circular interpolation □ When SSS is enabled: ○ When SSS is disabled: ∆ □ When SSS is enabled: ○ When SSS is disabled: ∆ G02.1 G03.1 Spiral interpolation ∆ ∆ G02.3 G03.3 Exponential interpolation ∆ ∆ G02.4 G03.4 3-dimensional circular interpolation ∆ ∆ G06.2 NURBS interpolation X (P34) X (P34) G33 Thread cutting ∆ ∆ 2 G17-G19 Plane selection ○ ○ 3 G90 Absolute value command ○ ○ G91 Incremental value command ○ ○ G22 Stroke check before travel ON ○ ○ G23 Stroke check before travel OFF ○ ○ G93 Inverse time feed X (P125) X (P125) G94 Asynchronous feed (feed per minute) ○ ○ G95 Synchronous feed (feed per revolution) ○ ○ G20 Inch command ○ ○ G21 Metric command ○ ○ G40 Tool radius compensation cancel ○ ○ G41 G42 Tool radius compensation ○ X (P29) G43 G44 Tool length offset ○ X (P29) G43.1 Tool length compensation along the tool axis ○ X (P29) G43.4 G43.5 Tool center point control ○ X (P29) G49 Tool length offset cancel ○ ○ G80 Fixed cycle cancel ○ ○ ∆ ∆ 4 5 6 7 8 9 Group 9 Fixed cycle Other than G80 IB-1501278-D A 604 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Group 10 11 12 13 14 15 16 17 18 19 21 24 27 G code Function name A B G98 Fixed cycle initial level return ○ ○ G99 Fixed cycle R point return ○ ○ G50 Scaling cancel ○ ○ G51 Scaling ON ○ X (P34) G54-G59 G54.1 Workpiece coordinate system selection ○ ○ G61 Exact stop check mode □ (*8) □ (*9) G61.1 High-accuracy control □ (*3) □ (*2) G61.2 High-accuracy spline X (P29) X (P29) G62 Automatic corner override □ (*3) □ (*2) G63 Tapping mode □ (*3) □ (*2) G64 Cutting mode □ (*3) □ (*2) G66 G66.1 User macro modal call □ (*5) □ (*6) G67 User macro modal call cancel ○ ○ G40.1 Normal line control cancel ○ ○ G41.1 G41.2 Normal line control X (P29) X (P29) G68 Coordinate rotation by program ON ○ X (P34) G68.2 G68.3 Inclined surface machining command ○ ○ G69 Coordinate rotation cancel ○ ○ G96 Constant surface speed control ON ○ ○ G97 Constant surface speed control OFF ○ ○ G15 Polar coordinate command OFF ○ ○ G16 Polar coordinate command ON X (P34) X (P34) G50.1 Mirror image OFF ○ ○ G51.1 Mirror image ON ○ X (P34) G07.1 Cylindrical interpolation X (P485) ∆ G12.1 Polar coordinate interpolation ON X (P485) ∆ G13.1 Polar coordinate interpolation OFF ○ ○ G188 Dynamic M/L program changeover ○ ○ G189 Dynamic M/L program changeover cancel ○ ○ G54.4P0 Workpiece installation error compensation cancel ○ ○ G54.4 P1-P7 Workpiece installation error compensation ○ ○ (*1) Disables the high-speed high-accuracy control I. (*2) Enables the high-speed high-accuracy control I. (*3) High-speed high-accuracy control I continues. (*4) Enables the high-speed machining mode II. (*5) Enables the high-speed high-accuracy control I in a macro program. (*6) Enables the high-speed high-accuracy control I if G05.1Q1 is commanded in a macro program. (*7) Enables the high-speed high-accuracy control I if G05.1Q1 is commanded in a sub part system. (*8) Enables the exact stop check mode. (*9) Exact stop check mode continues. 605 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (2) Relationship between the high-speed high-accuracy control I and functions other than G codes Column A: Operation when the additional function is commanded while the high-speed high-accuracy control I is enabled Column B: Operation when the high-speed high-accuracy control I (G05.1Q1) is commanded while the additional function is enabled ○: The high-speed high-accuracy control I and the additional function are both enabled ∆: The high-speed high-accuracy control I is temporarily canceled, while the additional function is enabled X: Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination □: Others Function name A B SSS ON - ○ Mirror image by parameter setting ON - X (P34) PLC mirror image ON - X (P34) Coordinate rotation by parameter - ∆ Subprogram call (M98) □ (*10) □ (*11) Figure rotation (M98 I_J_K_) □ (*17) □ (*18) Timing synchronization between part systems □ (*12) - MTB macro □ (*13) □ (*14) Macro interruption □ (*15) □ (*16) PLC interruption □ (*15) □ (*16) Corner chamfering/Corner R ∆ - Linear angle command ○ - Geometric command ○ - Chopping ○ ○ Optional block skip ○ - (*10) Enables the high-speed high-accuracy control I in a subprogram. (*11) Enables the high-speed high-accuracy control I if G05.1Q1 is commanded in a subprogram. (*12) Enables timing synchronization. (*13) Enables the high-speed high-accuracy control I in a MTB program. (*14) Enables the high-speed high-accuracy control I if G05.1Q1 is commanded in a MTB program. (*15) Enables the high-speed high-accuracy control I in an interrupt program. (*16) Enables the high-speed high-accuracy control I if G05.1Q1 is commanded in an interrupt program. (*17) Disables the high-speed high-accuracy control I in a figure rotation subprogram. (*18) The high-speed high-accuracy control I is disabled even if G05.1Q1 is commanded in a figure rotation subprogram. IB-1501278-D 606 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Relationship between the high-speed high-accuracy control II and other functions (1) Relationship between the high-speed high-accuracy control II and G code functions Column A: Operation when the additional function is commanded while the high-speed high-accuracy control II is enabled Column B: Operation when the high-speed high-accuracy control II (G05P10000) is commanded while the additional function is enabled ○: The high-speed high-accuracy control II and the additional function are both enabled ∆: The high-speed high-accuracy control II is temporarily canceled, while the additional function is enabled X: Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination □: Others Group 0 G code Function name A ∆ B G04 Dwell - G05P0 High-speed machining mode II OFF □ (*1) High-speed high-accuracy control II OFF High-speed high-accuracy control III OFF □ (*2) G05P2 High-speed machining mode II ON □ (*4) □ (*2) G05P10000 High-speed high-accuracy control II ON □ (*3) □ (*3) G05P20000 High-speed high-accuracy control III ON □ (*2) □ (*2) G05.1Q0 High-speed high-accuracy control I OFF Spline interpolation OFF □ (*3) □ (*2) G05.1Q1 High-speed high-accuracy control I ON X (P34) X (P34) G05.1Q2 Spline interpolation ON ○ ○ G07 Hypothetical axis interpolation ∆ ∆ G08P0 High-accuracy control OFF □ (*3) □ (*2) G08P1 High-accuracy control ON □ (*3) □ (*2) G09 Exact stop check ∆ - G10 I_J_ G10 K_ Parameter coordinate rotation input ∆ - G10 L2 Compensation data input by program ∆ - G10 L70 G10 L50 Parameter input by program ∆ - G27 Reference position check ∆ - G28 Reference position return ∆ - G29 Start position return ∆ - G30 2nd to 4th reference position return ∆ - G30.1G30.6 Tool change position return ∆ - G31 Skip Multiple-step skip 2 ∆ - G31.1G31.3 Multi-step skip ∆ - G34-G36 G37.1 Special Fixed Cycle ∆ - G37 Automatic tool length measurement ∆ - G38 Tool radius compensation vector designa- ∆ tion - G39 Tool radius compensation corner circular command - ∆ G52 Local coordinate system setting ∆ - G53 Machine coordinate system selection ∆ - G60 Unidirectional positioning ∆ - 607 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Group 0 1 G code Function name B G65 User macro simple call □ (*5) □ (*6) G92 Coordinate system setting ∆ - G92.1 Workpiece coordinate preset ∆ - G122 Sub part system control I X (P652) □ (*7) G00 Positioning ∆ ∆ G01 Linear interpolation ○ ○ G02 G03 Circular interpolation ○ ○ G02.1 G03.1 Spiral interpolation ∆ ∆ G02.3 G03.3 Exponential interpolation ∆ ∆ G02.4 G03.4 3-dimensional circular interpolation ∆ ∆ G06.2 NURBS interpolation ○ ○ G33 Thread cutting ∆ ∆ 2 G17-G19 Plane selection ○ ○ 3 G90 Absolute value command ○ ○ G91 Incremental value command ○ ○ G22 Stroke check before travel ON ∆ ∆ G23 Stroke check before travel OFF ○ ○ G93 Inverse time feed ∆ ∆ G94 Asynchronous feed (feed per ○ minute) ○ G95 Synchronous feed (feed per revolution) ∆ ∆ G20 Inch command ○ ○ G21 Metric command ○ ○ G40 Tool radius compensation cancel ○ ○ G41 G42 Tool radius compensation ○ ○ G43 G44 Tool length offset ○ ○ G43.1 Tool length compensation along the tool axis ○ ○ G43.4 G43.5 Tool center point control ○ ○ G49 Tool length offset cancel ○ ○ G80 Fixed cycle cancel ○ ○ ∆ ∆ Fixed cycle initial level return ○ ○ 4 5 6 7 8 9 Group 9 Fixed cycle Other than G80 10 G98 G99 Fixed cycle R point return ○ ○ 11 G50 Scaling cancel ○ ○ G51 Scaling ON ∆ ∆ 12 G54-G59 Workpiece coordinate system ○ selection ○ G54.1 IB-1501278-D A 608 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Group 13 14 15 16 17 18 19 21 24 27 G code Function name A B G61 Exact stop check mode ∆ ∆ G61.1 High-accuracy control □ (*3) □ (*2) G61.2 High-accuracy spline X (P29) X (P29) G62 Automatic corner override ∆ ∆ G63 Tapping mode ∆ ∆ G64 Cutting mode □ (*3) □ (*2) G66 G66.1 User macro modal call ∆ ∆ G67 User macro modal call cancel ○ ○ G40.1 Normal line control cancel ○ ○ G41.1 G41.2 Normal line control X (P29) X (P29) G68 Coordinate rotation by program ON ∆ ∆ G68.2 G68.3 Inclined surface machining command ○ ○ G69 Coordinate rotation cancel ○ ○ G96 Constant surface speed con- ○ trol ON ○ G97 Constant surface speed con- ○ trol OFF ○ G15 Polar coordinate command OFF ○ ○ G16 Polar coordinate command ON ∆ ∆ G50.1 Mirror image OFF ○ ○ G51.1 Mirror image ON ○ ○ G07.1 Cylindrical interpolation X (P34) X (P481) G12.1 Polar coordinate interpolation X (P34) ON X (P481) G13.1 Polar coordinate interpolation ○ OFF ○ G188 Dynamic M/L program changeover ○ ○ G189 Dynamic M/L program changeover cancel ○ ○ G54.4P0 Workpiece installation error compensation cancel ○ ○ G54.4 P1-P7 Workpiece installation error compensation ○ ○ (*1) Disables the high-speed high-accuracy control II. (*2) Enables the high-speed high-accuracy control II. (*3) High-speed high-accuracy control II continues. (*4) Enables the high-speed machining mode II. (*5) Enables the high-speed high-accuracy control II in a macro program. (*6) Enables the high-speed high-accuracy control II if G05P10000 is commanded in a macro program. (*7) Enables the high-speed high-accuracy control II if G05P10000 is commanded in a sub part system. (*8) Enables the exact stop check mode. (*9) Exact stop check mode continues. 609 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (2) Relationship between the high-speed high-accuracy control II and functions other than G codes Column A: Operation when the additional function is commanded while the high-speed high-accuracy control II is enabled Column B: Operation when the high-speed high-accuracy control II (G05P10000) is commanded while the additional function is enabled ○: The high-speed high-accuracy control II and the additional function are both enabled ∆: The high-speed high-accuracy control II is temporarily canceled, while the additional function is enabled X: Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination □: Others Function name A B SSS ON - ○ Mirror image by parameter setting ON - ∆ PLC mirror image ON - ∆ Coordinate rotation by parameter - ∆ Subprogram call (M98) □ (*10) □ (*11) Figure rotation (M98 I_J_K_) □ (*17) □ (*18) Timing synchronization between part systems □ (*12) - MTB macro □ (*13) □ (*14) Macro interruption □ (*15) □ (*16) PLC interruption □ (*15) □ (*16) Corner chamfering/Corner R ∆ - Linear angle command ∆ - Geometric command ∆ - Chopping ○ ○ Fairing/smooth fairing ON ○ ○ Optional block skip ○ - (*10) Enables the high-speed high-accuracy control II in a subprogram. (*11) Enables the high-speed high-accuracy control II if G05P10000 is commanded in a subprogram. (*12) Enables timing synchronization. (*13) Enables the high-speed high-accuracy control II in a MTB program. (*14) Enables the high-speed high-accuracy control II if G05P10000 is commanded in a MTB program. (*15) Enables the high-speed high-accuracy control II in an interrupt program. (*16) Enables the high-speed high-accuracy control II if G05P10000 is commanded in an interrupt program. (*17) Disables the high-speed high-accuracy control II in a figure rotation subprogram. (*18) The high-speed high-accuracy control II is disabled even if G05P10000 is commanded in a figure rotation subprogram. (*19) Enables the normal mode (G05P0). IB-1501278-D 610 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Relationship between the high-speed high-accuracy control III and other functions (1) Relationship between the high-speed high-accuracy control III and G code functions Column A: Operation when the additional function is commanded while the high-speed high-accuracy control III is enabled Column B: Operation when the high-speed high-accuracy control III (G05P20000) is commanded while the additional function is enabled ○: The high-speed high-accuracy control III and the additional function are both enabled ∆: The high-speed high-accuracy control III is temporarily canceled, while the additional function is enabled X: Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination □: Others Group 0 G code Function name A B G04 Dwell ∆ - G05P0 High-speed machining mode II OFF High-speed high-accuracy control II OFF High-speed high-accuracy control III OFF □ (*1) □ (*2) G05P2 High-speed machining mode II ON □ (*3) □ (*2) G05P10000 High-speed high-accuracy control II ON □ (*4) □ (*2) G05P20000 High-speed high-accuracy control III ON □ (*3) □ (*3) G05.1Q0 High-speed high-accuracy control I OFF Spline interpolation OFF □ (*3) □ (*2) G05.1Q1 High-speed high-accuracy control I ON X (P34) X (P34) G05.1Q2 Spline interpolation ON □ (*2) □ (*2) G07 Hypothetical axis interpolation ∆ ∆ G08P0 High-accuracy control OFF □ (*3) □ (*2) G08P1 High-accuracy control ON □ (*3) □ (*2) G09 Exact stop check ∆ - G10 I_J_ G10 K_ Parameter coordinate rotation input ∆ - G10 L2 Compensation data input by program ∆ - G10 L70 G10 L50 Parameter input by program ∆ - G27 Reference position check ∆ - G28 Reference position return ∆ - G29 Start position return ∆ - G30 2nd to 4th reference position return ∆ - G30.1G30.6 Tool change position return ∆ - G31 Skip Multiple-step skip 2 ∆ - G31.1G31.3 Multi-step skip ∆ - G34-G36 G37.1 Special Fixed Cycle ∆ - G37 Automatic tool length measurement ∆ - G38 Tool radius compensation vector designation ∆ - G39 Tool radius compensation corner circular command ∆ - G52 Local coordinate system setting ∆ - 611 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Group 0 1 G code Function name B G53 Machine coordinate system selection ∆ - G60 Unidirectional positioning ∆ - G65 User macro simple call □ (*5) □ (*6) G92 Coordinate system setting ∆ - G92.1 Workpiece coordinate preset ∆ - G122 Sub part system control I X (P652) □ (*7) G00 Positioning □ (*2) □ (*2) G01 Linear interpolation ○ ○ G02 G03 Circular interpolation □ (*2) □ (*2) G02.1 G03.1 Spiral interpolation ∆ □ (*19) G02.3 G03.3 Exponential interpolation ∆ □ (*19) G02.4 G03.4 3-dimensional circular interpolation ∆ □ (*19) G06.2 NURBS interpolation □ (*2) □ (*2) G33 Thread cutting ∆ □ (*19) 2 G17-G19 Plane selection ○ ○ 3 G90 Absolute value command ○ ○ G91 Incremental value command ○ ○ G22 Stroke check before travel ON ∆ □ (*19) G23 Stroke check before travel OFF ○ ○ G93 Inverse time feed ∆ □ (*19) G94 Asynchronous feed (feed per minute) ○ ○ G95 Synchronous feed (feed per revolution) ∆ □ (*19) G20 Inch command ○ ○ G21 Metric command ○ ○ G40 Tool radius compensation cancel ○ ○ G41 G42 Tool radius compensation □ (*2) □ (*2) G43 G44 Tool length offset ○ ○ G43.1 Tool length compensation along the tool axis □ (*2) □ (*2) G43.4 G43.5 Tool center point control □ (*2) □ (*2) G49 Tool length offset cancel ○ ○ G80 Fixed cycle cancel 4 5 6 7 8 9 10 11 12 ○ ○ Group 9 Fixed cycle Other than G80 ∆ □ (*19) G98 Fixed cycle initial level return ○ ○ G99 Fixed cycle R point return ○ ○ G50 Scaling cancel ○ ○ G51 Scaling ON ∆ □ (*19) G54-G59 Workpiece coordinate system selection ○ ○ G54.1 IB-1501278-D A 612 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Group 13 14 15 16 G code Function name A B G61 Exact stop check mode ∆ □ (*19) G61.1 High-accuracy control □ (*3) □ (*2) G61.2 High-accuracy spline X (P29) X (P29) G62 Automatic corner override ∆ □ (*19) G63 Tapping mode ∆ □ (*19) G64 Cutting mode □ (*3) □ (*2) G66 G66.1 User macro modal call ∆ □ (*19) G67 User macro modal call cancel ○ ○ G40.1 Normal line control cancel ○ ○ G41.1 G41.2 Normal line control X (P29) X (P29) G68 Coordinate rotation by program ON ∆ □ (*19) G68.2 G68.3 Inclined surface machining command □ (*2) □ (*2) G69 Coordinate rotation cancel ○ ○ 17 G96 Constant surface speed control ON ○ ○ G97 Constant surface speed control OFF ○ ○ 18 G15 Polar coordinate command OFF ○ ○ 19 21 24 27 G16 Polar coordinate command ON ∆ □ (*19) G50.1 Mirror image OFF ○ ○ G51.1 Mirror image ON □ (*2) □ (*2) G07.1 Cylindrical interpolation X (P34) X (P481) G12.1 Polar coordinate interpolation ON X (P34) X (P481) G13.1 Polar coordinate interpolation OFF ○ ○ G188 Dynamic M/L program changeover ○ ○ G189 Dynamic M/L program changeover cancel ○ ○ G54.4P0 Workpiece installation error compensation can- ○ cel ○ G54.4P1-P7 Workpiece installation error compensation □ (*2) □ (*2) (*1) Disables the high-speed high-accuracy control III. (*2) Enables the high-speed high-accuracy control III. (*3) High-speed high-accuracy control III continues. (*4) Enables the high-speed high-accuracy control II. (*5) Enables the high-speed high-accuracy control III in a macro program. (*6) Enables the high-speed high-accuracy control III if G05P20000 is commanded in a macro program. (*7) Enables the high-speed high-accuracy control III if G05P20000 is commanded in a sub part system. (*8) Enables the exact stop check mode. (*9) Exact stop check mode continues. 613 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (2) Relationship between the high-speed high-accuracy control III and functions other than G codes Column A: Operation when the additional function is commanded while the high-speed high-accuracy control III is enabled Column B: Operation when the high-speed high-accuracy control III (G05P20000) is commanded while the additional function is enabled ○: The high-speed high-accuracy control III and the additional function are both enabled ∆: The high-speed high-accuracy control III is temporarily canceled, while the additional function is enabled X: Alarm generation (the text in parentheses refers to the number of the program error to be generated.) -: No combination □: Others Function name A SSS ON B - ○ SSS OFF - □ (*4) Mirror image by parameter setting ON - ∆ PLC mirror image ON - ∆ Coordinate rotation by parameter - ∆ Subprogram call (M98) □ (*10) □ (*11) Figure rotation (M98 I_J_K_) □ (*17) □ (*18) Timing synchronization between part systems □ (*12) - MTB macro □ (*13) □ (*14) Macro interruption □ (*15) □ (*16) PLC interruption □ (*15) □ (*16) Corner chamfering/Corner R ∆ - Linear angle command ∆ - Geometric command ∆ - Chopping ○ ○ Fairing/smooth fairing ON □ (*4) □ (*4) Optional block skip □ (*4) - (*10) Enables the high-speed high-accuracy control III in a subprogram. (*11) Enables the high-speed high-accuracy control III if G05P20000 is commanded in a subprogram. (*12) Enables timing synchronization. (*13) Enables the high-speed high-accuracy control III in a MTB program. (*14) Enables the high-speed high-accuracy control III if G05P20000 is commanded in a MTB program. (*15) Enables the high-speed high-accuracy control III in an interrupt program. (*16) Enables the high-speed high-accuracy control III if G05P20000 is commanded in an interrupt program. (*17) Disables the high-speed high-accuracy control III in a figure rotation subprogram. (*18) The high-speed high-accuracy control III is disabled even if G05P20000 is commanded in a figure rotation subprogram. (*19) Enables the normal mode (G05P0). IB-1501278-D 614 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.3.2 Fairing Function and purpose This function is an additional function when the high-speed high-accuracy control II mode is ON If there is a protrusion in a path (zigzagging path) in a machining program generated with a CAM, etc., this function can be used to eliminate the protruding path smaller than the setting value so that the protruding path is smoothly connected with the previous and the next paths. This function is valid only for continuous linear commands (G01). Related parameter Details #8033 Fairing ON 0 : Fairing invalid 1 : Execute fairing for the protruding block 2 : Smooth fairing valid #8029 Fairing L Execute fairing for the shorter block than this setting value Before fairing After fairing Path before/after fairing execution If there is any protruding path after fairing, fairing is repeated. Before fairing After first fairing After final fairing Path in repetitive fairing executions 615 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.3.3 Smooth Fairing Function and purpose This function is an additional function when the high-speed high-accuracy control II mode is ON A path can be smoothen by compensating commanded positions of a machining program. This function is useful when executing a fine segment program to machine smoothly at low speed or a rough machining program with long segment to machine smoothly. This function is enabled while high-speed high-accuracy control II is ON or while high-accuracy control is ON in highspeed machining mode II, and performs compensation on consecutive G01 command during this time. The validity of this function depends on the MTB specifications. To use this function, the high-speed high-accuracy control II specification, or the high-speed machining mode II and high-accuracy control specifications are required. Commanded path G90 G00 X0.271 Y0.161; G01; N01 X0.319 Y0.249; N02 X0.415 Y0.220; N03 X0.475 Y0.299; N04 X0.566 Y0.256; N05 X0.638 Y0.325; N06 X0.720 Y0.268; N07 X0.803 Y0.325; N08 X0.875 Y0.256; N09 X0.965 Y0.299; N10 X1.026 Y0.220; N11 X1.122 Y0.249; N12 X1.169 Y0.161; Commanded position N03 N01 N02 N07 N05 N04 N06 N09 N11 N08 N10 Smooth fairing OFF N12 Smooth fairing ON Compensated position Tool path Tool path Commanded position Commanded position Faring and smooth faring differ as follows: Fairing Smooth fairing Operation - Eliminating blocks shorter than designated length Usage - Eliminating minute steps to occur at fillet and - Smooth machining at low speed for a fine other sections segment program - Eliminating noises on commanded paths - Smooth machining for a rough machining program IB-1501278-D 616 - Compensating commanded positions across multiple blocks M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control When a minute step exists on a commanded path, for instance, the path after compensation differs between fairing and smooth fairing as follows: Commanded path Commanded position N07 N01 N02 N03 N04 N05 N08 N09 N10 G01; N06 Path after compensation by fairing G90 G00 X0 Y0; N01 X0.100 Y0.000; Eliminates blocks shorter than designated length. N02 X0.200 Y0.000; N03 X0.300 Y0.000; N04 X0.400 Y0.000; Path after compensation by smooth fairing Path after compensation N05 X0.500 Y0.000; N06 X0.500 Y0.010; N07 X0.600 Y0.010; N08 X0.700 Y0.010; N09 X0.800 Y0.010; Compensates commanded positions in blocks around a step. N10 X0.900 Y0.010; Refer to "Relationship with Other Functions" for the relationship between smooth fairing and other functions. Detailed description Enabling conditions To enable smooth fairing, it is necessary for the following conditions to be satisfied respectively: (a) The smooth fairing option is set to ON. (b) One of the following modes is set to ON. - G05 P20000 (*1) - G05 P10000 - G05 P2 and the high-accuracy function (G61.1/G08P1 or G61.2) are used simultaneously. (c) At least one of the following conditions is satisfied. - The parameter "#8033 Fairing ON" is set to "2". - The G05 P20000, R1 / G05 P10000, R1 / G05 P2, or R1 command is issued. (*1) This command functions as G05 P10000 while smooth fairing is ON. 617 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Enabling smooth fairing Two methods are available to enable smooth fairing: "G05 Pp,Rr command" and parameter "#8033 Fairing ON" ((c) of fairing enable conditions). Relationship between ",R" address and parameter "#8033 Fairing ON" Parameter "#8033 Fairing ON" 0 Both OFF G05 P20000 G05 P10000 G05 P2 Command 1 Fairing ON 2 Smooth fairing ON No ,R × ○ ● ,R0 × × × ,R1 ● ● ● ●: Smooth fairing ON, ○: Fairing ON, X: Both OFF (1) When the ",R" address is set to the G05 command, the operation shown in the table below is performed regardless of the setting value of the parameter "#8033". Smooth fairing ON Smooth fairing OFF G05 P20000,R1 G05 P10000,R1 G05 P2,R1 Smooth fairing is ON regardless of the setting value of the parameter "#8033". G05 P20000,R0 G05 P10000,R0 G05 P2,R0 Both fairing and smooth fairing are OFF regardless of the setting value of the parameter "#8033". G05 P0,Rr (r=0,1) G05 P1,Rr (r=0,1) (Program error(P33)) G05 P20000,Rr (r=0,1) G05 P10000,Rr (r=0,1) G05 P2,Rr (r=0,1) G05 P1,Rr (r=0,1) G05 P0,Rr (r=0,1) Program error (P39) (2) The ",R" address is unmodal information. The ",R" address value designated by previous G05 command is not inherited to the next and subsequent G05 commands. Each time the G05 command is issued, the fairing function is switched as shown in the table above. Machining program Operation N01 G05 P10000,R1; ... In this period, the program runs with G05 P10000,R1. N02 G05 P0; N03 G05 P10000; The ",R" address of the N01 G05 command is not inherited. ... In this period, the program runs with G05 P10000 (without the ",R" address). N04 G05 P0; (3) To switch smooth fairing and fairing, insert the G05P0; command between them. If this switching is commanded without inserting the G05P0 command, a program error (P560) will occur. Machining program Operation N01 G05 P10000,R1; Set the parameter "#8033" to "1". ... In this period, the program runs with smooth fairing. N03 G05 P10000; Issuing this command switches to fairing, which causes an error. IB-1501278-D 618 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (4) To enable smooth fairing without setting the ",R" address to the G05 command, set the parameter "#8033 Fairing ON" to "2". The following operation is performed. G05 P20000 G05 P10000 G05 P2 Smooth fairing ON G05 P1 G05 P0 Both fairing and smooth fairing are OFF Details of Operation An operation example is as follows. (In this figure, symbol ○ indicates the compensated position, and symbol ● indicates the commanded position.) (1) Smooth fairing smoothens the path by compensating the positions designated by successive G01 commands. This function recognizes the paths before and after each commanded position, and compensates commanded positions that cause a path to become unsmooth. [Commanded path] (indicated by dashed lines) NO5 NO3 NO2 NO6 NO7 NO8 NO9 NO10 NO11 NO12 NO1 [Path after compensation] (indicated by solid lines) The smooth parts Only the unsmooth parts are compensated. are not targeted for compensation. G90 G00 X0.322 Y0.234; G01; N01 X0.413 Y0.276; N02 X0.507 Y0.311; N03 X0.603 Y0.338; N04 X0.701 Y0.357; N05 X0.798 Y0.399; N06 X0.900 Y0.343; N07 X1.003 Y0.399; N08 X1.095 Y0.328; N09 X1.205 Y0.367; N10 X1.284 Y0.282; N11 X1.399 Y0.304; N12 X1.465 Y0.207; : Compensated position : Commanded position 619 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (2) The path recognition range is determined by the parameter "#8038 Path recog. range". Determine the setting value to include multiple G01 commands in the path recognition range. When the setting value is "0", the range is set to "1.0 (1 mm)". When the path recognition range is set to 0.5 mm: 0.11mm 0.1mm 0.1mm 0.11mm 0.1mm 0.1mm 0.1mm 0.1mm 0.1mm 0.1mm 0.1mm 0.1mm The path is recognized in the range of 0.5 mm forward and 0.5 mm backward of the commanded position. G90 G00 X0.322 Y0.234; G01; N01 X0.413 Y0.276; N02 X0.507 Y0.311; N03 X0.603 Y0.338; N04 X0.701 Y0.357; N05 X0.800 Y0.369; N06 X0.900 Y0.423; N07 X1.000 Y0.369; N08 X1.099 Y0.357; N09 X1.198 Y0.338; N10 X1.294 Y0.311; N11 X1.388 Y0.276; N12 X1.478 Y0.234; (3) The upper limit of the compensation distance can be determined so that the compensated position does not deviate from the commanded position significantly. Designate this upper limit in the parameter "#8039 Comp. range limit". Ordinarily, designate the tolerance that is designated when generating the machining program with CAM. When the setting value is "0", the range is set to "0.005 (5 microns)". (a) When the compensation distance tolerance is high: NO6 Desirable compensation position NO7 Compensation range tolerance Actual compensation position G90 G00 X0.322 Y0.234; G01; N01 X0.413 Y0.276; N02 X0.507 Y0.311; N03 X0.603 Y0.338; N04 X0.701 Y0.357; N05 X0.800 Y0.369; N06 X0.900 Y0.423; N07 X1.000 Y0.369; N08 X1.099 Y0.357; N09 X1.198 Y0.338; N10 X1.294 Y0.311; N11 X1.388 Y0.276; N12 X1.478 Y0.234; (b) When the compensation distance tolerance is low: Compensation range tolerance Desirable compensation position IB-1501278-D Actual compensation position 620 G90 G00 X0.322 Y0.234; G01; N01 X0.413 Y0.276; N02 X0.507 Y0.311; N03 X0.603 Y0.338; N04 X0.701 Y0.357; N05 X0.800 Y0.369; N06 X0.900 Y0.423; N07 X1.000 Y0.369; N08 X1.099 Y0.357; N09 X1.198 Y0.338; N10 X1.294 Y0.311; N11 X1.388 Y0.276; N12 X1.478 Y0.234; M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (4) While smooth fairing is ON, the modal or mode status is changed, and smooth fairing may be set to OFF. While smooth fairing is OFF, the commanded position is not compensated, and the axis moves as commanded. For details on the modal or mode status that causes smooth fairing to be set to OFF, refer to "Relationship with other functions". While smooth fairing is OFF, the axis moves to the commanded posi- G90 G00 X0.0 Y0.0; tion. G01; N01 G01 X0.039 Y0.077; N02 G01 X0.139 Y0.080; N03 G01 X0.172 Y0.174; N04 G01 X0.271 Y0.161; NO6 N05 G01 X0.319 Y0.249; N06 G02 X1.122 Y0.249 R0.5; N07 G01 X1.169 Y0.161; N08 G01 X1.268 Y0.174; N09 G01 X1.301 Y0.080; N10 G01 X1.401 Y0.077; N11 G01 X1.441 Y0.000; Valid Invalid Valid Compensation restarts from the block in which smooth fairing enable conditions are satisfied again. (5) While smooth fairing is ON, it may be canceled temporarily depending on commands when: - there is a block that contains only a sequence number; - the modal status of the absolute value/incremental value command is changed by the G90 or G91 command; and - the movement command is issued to an axis other than the three basic axes. If a command that triggers a temporary cancel is inserted, the axis moves to the commanded position once. For the list of commands that trigger a temporary cancel, refer to "Relationship with other functions". G90 G00 X0.322 Y0.234; G90 G01; N01 X0.413 Y0.276; N02 X0.507 Y0.311; N03 X0.603 Y0.338; N04 X0.701 Y0.357; N05 X0.798 Y0.399; If a block that triggers a temporary cancel is in- N06 X0.900 Y0.343; serted, the axis moves to the commanded posi- N07; N08 X1.003 Y0.399; tion once. N09 X1.095 Y0.328; N10 X1.205 Y0.367; N11 X1.284 Y0.282; N12 X1.399 Y0.304; N13 X1.465 Y0.207; 621 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Relationship with other functions (1) Relationship between smooth fairing and other G code functions A Shows if smooth fairing is valid or not when the G code function on the left is enabled. ○ (Valid): Compensates for the commanded position X (invalid): Does not compensate the commanded position B Shows operation when the G code on the left is commanded together with a movement command (XYZ address command)(*) while smooth fairing is ON. ○ (continuation): Compensates for the commanded position X (temporary cancel): Temporarily suspends compensation to move to the commanded position (*) Temporary cancel for blocks with no movement commands (example: When G90; is commanded independently). G code group 0 Function name G05 High-speed machining mode/high-speed high-accuracy control G08 High-accuracy Control A B (*1) - ○ × G command in group 0 except the above - × 1 G01 Linear interpolation ○ ○ G command in group 1 except the above × × 2 G17/G18/G19 Plane selection ○ (*2) 3 G90/G91 Absolute value command/incremental value command ○ (*2) 4 G23 Stroke check before travel OFF ○ × G command in group 4 except the above × × 5 G94 Asynchronous feed (feed per minute ) ○ ○ G command in group 5 except the above × × 6 G20/G21 Inch/Metric command ○ × 7 G40 Tool radius compensation cancel/3-dimentional tool radius compensation cancel ○ ○ G41/G42 Tool radius compensation/3-dimensional tool radius compensation ○ ○ G command in group 7 except the above × × G43/G44 Tool length offset + /tool length offset - ○ × G43.1 Tool length compensation along the tool axis ○ × G49 Tool length offset cancel ○ × G command in group 8 except the above × × 8 9 G80 Fixed cycle cancel ○ × G command in group 9 except the above × × 10 G98/G99 Fixed cycle initial level return/R point level return ○ × 11 G50 Scaling cancel ○ × G command in group 11 except the above × × 12 G54-G59/G54.1 Workpiece coordinate system selection ○ × 13 IB-1501278-D G Code G61.1 High-accuracy control ON ○ × G61.2 High-accuracy spline ○ × G command in group 13 except the above × × 14 G67 User macro modal call cancel ○ × G command in group 14 except the above × × 15 G40.1/G150 Normal line control cancel ○ × G command in group 15 except the above × × 622 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control G code group 16 G Code G69 Function name A B Coordinate rotation cancel/3-dimensional coordinate conversion cancel ○ × G command in group 16 except the above × × 17 G96/G97 Constant surface speed control ON/OFF ○ × 18 G15 Polar coordinate command OFF ○ × G command in group 18 except the above × × 19 G50.1 Mirror image by G code OFF ○ ○ G command in group 19 except the above × × 21 G13.1/G113 Cylindrical interpolation/polar coordinate interpolation OFF ○ ○ G command in group 21 except the above × × 24 G188/G189 Dynamic M/L program changeover/cancel ○ × 27 G54.4 Workpiece installation error compensation (*3) × (*1) ○ (valid) for G05P2/G05P10000/G05P20000 and X (invalid) for the others. (*2) ○ (continuation) if the modal state does not change before and after the command and X (temporary cancel) otherwise. (*3) ○ (Valid) for G54.4P0 and X (invalid) for the others. (2) Relationship between smooth fairing and functions other than G codes A Shows if smooth fairing is valid or not when the function on the left is enabled. ○ (Valid): Compensates for the commanded position X (invalid): Does not compensate the commanded position B Shows operation when the function on the left is commanded while smooth fairing is ON. ○ (continuation): Compensates for the commanded position X (temporary cancel): Temporarily suspends compensation to move to the commanded position Function other than G code A B Block containing only EOB(;) - (*1) Block containing only comment - ○ Block containing only sequence number - × Block containing only MSTB command - × Block containing only F command - × If there is an axis movement command for other than three base axes - × Block without movement command - × During single block operation × × Subprogram call (M98 P_) ○ × Figure rotation subprogram call (M98 P_I_J_K_) × × Macro interruption (M96, UIT) ○ × User macro simple call ○ × User macro modal call × × MTB macro × × PLC interruption (PIT) (*2) Coordinate rotation by parameter (G10 I_J_/K_) × × Mirror image by parameter setting (#8211 Mirror image) × × Mirror image with PLC signals ON × × (*1) When there is a block containing only EOB, compensation is not temporarily canceled. However, in such a case, the path slightly changes compared to when there are no blocks containing only EOB. (*2) PLC interruption is not allowed during high-speed high-accuracy control II/III. 623 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control The table below shows which fairing functions are enabled according to the combination of the parameter "#8033 Fairing ON" setting and G command: "#8033 Fairing ON" 0 1 2 Both OFF Fairing ON Smooth fairing ON G05 P0 G61.1 × × × G61.2 ○ ○ ○ G05 P2 G61.1 × × ● G61.2 ○ ○ ● G5.1 Q0 × ○ ● G5.1 Q2 × × ● G05 P10000 G05 P20000 ●: Smooth fairing ON, ○: Fairing ON, X: Both OFF IB-1501278-D 624 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.3.4 Acceleration Clamp Speed Function and purpose This function is an additional function when the high-speed high-accuracy control II mode is ON The cutting feed clamp speed during the high-speed high-accuracy control II / III mode, when the following parameter is set to "1", is clamped so that the acceleration generated by each block movement does not exceed the tolerable value. This function clamps the speed optimally even at a section where "angle change at each block is small but entire curvature is large" such as shown below. The tolerable acceleration value is calculated from the parameter "#1206 G1bF" and "#1207 G1btL" setting values. (Tolerable acceleration = #1206/#1207) #8034 Related parameter Details AccClampt ON 0 : Clamp the cutting speed with parameter "#2002 clamp" (*1) or the corner deceleration function. 1: Cutting speed clamp determined by acceleration reference is also executed. R If the tool moves along the large curvature section without deceleration, a large acceleration is generated resulting in a path error by curving inward. Speed control by curvature (*1) When a speed is set in "#2109 Clamp(H-precision)", clamp is executed at that speed. When the setting value is "0", clamp is executed with "#2002 clamp". 625 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.3.5 Corner Deceleration in High-speed Mode Function and purpose This function is an additional function when high-speed high-accuracy control II mode is ON. During high-accuracy control, if the angle between the adjacent blocks in the machining program is large, this function, conventionally, automatically decelerates the machining so that the acceleration generated when passing through the corner is maintained within the tolerable value. If a fine block is inserted at the corner section in the machining program generated with the CAM, etc., the corner passing speed will not match the periphery. This can affect the machining surface. In the corner deceleration in the high-speed mode, even when this type of fine block is inserted, the corner will be judged from a vantage point by setting the below parameter. The fine block is excluded at the judgment of an angle, but is not excluded from the actual movement command. Related parameter Details #8036 CordecJudge 0 : Judge the corner from the angle of the neighboring block. 1 : Judge the corner from the angle of the neighboring block, excluding the minute blocks. #8027 CorJudgeL Exclude shorter block than this setting value. (a) High-speed mode corner deceleration (a) When"#8036 CordecJudge" is set to "1", corner deceleration is realized without an influence of fine blocks. IB-1501278-D 626 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.3.6 Precautions on High-speed High-accuracy Control Precautions Common precautions on high-speed high-accuracy control I/II/III (1) The validity of each high-speed high-accuracy control function depends on the MTB specifications. If any of the above is commanded when the corresponding specification is not available on the machine, a program error (P39) will occur. (2) The machining speed may drop depending on the number of characters in one block. (3) Feedrate command F is clamped with the "#2110 Clamp (H-precision)" (Cutting feed clamp speed for high-accuracy control mode) set with parameter. (4) The rapid traverse rate conforms to "#2109 Rapid(H-precision)" (Rapid traverse rate during high-accuracy control mode) set by the parameter. (5) When "#2109 Rapid(H-precision)" (high-accuracy control mode rapid traverse rate) is set to "0", however, the movement follows "#2001 rapid" (Rapid traverse rate) set with the parameter. Also, when "#2110 Clamp (H-precision)" (Cutting feed clamp speed for high-accuracy control mode) is set to "0", the speed will be clamped with "#2002 clamp" (Cutting clamp speed) set with parameter. (6) The automatic operation processing has priority in the high-speed high-accuracy control I/II/III modal, so the screen display, etc., may be delayed. (7) The speed will decelerate once at the high-speed high-accuracy control I command (G05.1 Q1), high-speed high-accuracy control I OFF command (G05.1 Q0), high-speed high-accuracy control II command (G05P10000), high-speed high-accuracy control III command (G05P20000), and high-speed high-accuracy control II/III OFF command (G05P0), so turn ON and OFF when the tool separates from the workpiece. (8) When carrying out high-speed high-accuracy control I/II operation during tape mode, the machining speed may be suppressed depending on the program transmission speed and the number of characters in one block. (9) If the parameter "#1205 G0bdcc" (G0 acceleration/deceleration before interpolation) is set to "1", the value set with the parameter "#2224 SV024" (in-position detection width) will be used as the in-position width. "#2077 G0inps" (G0 in-position width) and the ",I" command (programmable in-position check) are disabled. Common precautions on high-speed high-accuracy control II/III (1) While high-speed high-accuracy control II/III is enabled, the following variable commands or operation commands can be designated following the axis address. When other variable commands or operation commands are issued, high-speed high-accuracy control II/III is canceled temporarily. (a) Referencing common variables or local variables Common variables or local variables can be referenced (example: X#500, Y#1, Z##100, A#[#101], etc.). (b) Four basic arithmetic rule Four basic arithmetic rule (+, -, *, /) operations are available, and also the operation priority can be designated using parentheses ( ) ([#500 + #501] * #502, etc.). Precautions on high-speed high-accuracy control I (1) Command G05.1Q0 after turning the tool radius compensation OFF. If G05.1Q0 is commanded without turning the tool radius compensation OFF, a program error (P29) will occur. (2) G05.1Q1; and G05.1Q0; are independent commands. If a sequence number other than "N" is commanded, the program error (P33) will occur. (3) The program error (P33) will occur if the G05.1 command block does not contain a Q command. (4) If the high-speed high-accuracy control I command is issued in the high-speed high-accuracy control II modal, a program error (P34) will occur. 627 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Precautions on high-speed high-accuracy control II (1) G05P10000; and G05P0; are independent commands. If a sequence number other than "N" is commanded, the program error (P33) will occur. (2) The program error (P33) will occur if the G05 command block does not contain a P command. (3) The fairing function is valid for the continuous linear command (G01). Fairing is not possible in the case below. G02 G02 G01 (4) In a single block mode, operation stops at the end point of each block. (5) When using the high-speed high-accuracy control II mode, set parameter "#1572 Cirorp/Bit0" to "1" to eliminate the speed fluctuation at the seams between the arc and the straight line, or between arcs. (6) A program error (P33) will occur if the geometric command is issued during the high-speed high-accuracy control II. (7) If the high-speed high-accuracy control II command is issued in the high-speed high-accuracy control I modal, a program error (P34) will occur. Precautions on high-speed high-accuracy control III (1) If high-speed high-accuracy control III is commanded while its specifications are invalid, a program error (P39) will occur. (2) G05P20000; and G05P0; are independent commands. If a sequence number other than "N" is commanded, the program error (P33) will occur. (3) The program error (P33) will occur if the G05 command block does not contain a P command. (4) A program error (P33) will occur if the geometric command is issued during high-speed high-accuracy control III. (5) If the high-speed high-accuracy control III command is issued in the high-speed high-accuracy control I modal, a program error (P34) will occur. (6) If the high-speed high-accuracy control II mode is valid when high-speed high-accuracy control III is commanded, follow the precautions on high-speed high-accuracy control II. (7) High-speed high-accuracy control III can be enabled by commanding the G code from the machining program. (a) High-speed high-accuracy control III command with the high-speed high-accuracy control III enable conditions satisfied If all modal conditions in each G code group and each mode condition shown in "Fine segment capacity for multi-part system" are satisfied when G05P20000; is commanded, the high-speed high-accuracy control III mode is enabled, and "G05P20000" is displayed on the modal screen. If conditions are not satisfied after G05P20000; has been commanded, the high-speed high-accuracy control III mode is enabled, but the fine segment capacity is not guaranteed. Machining program High-speed high-accuracy control III enable conditions G05 P20000; ...High-speed high-accuracy control Enable conditions are satisIII command fied. Enable mode G05 P20000 G41 XxYyDd; ...Tool radius compensation ON Enable conditions are not sat- G05P20000 (*1) isfied. G40 XxYy; ...Tool radius compensation OFF Enable conditions are satisfied. G05 P20000 (*1) High-speed high-accuracy control III is enabled, but the fine segment capacity shown in "Fine segment capacity for multi-part system" is not guaranteed. IB-1501278-D 628 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (b) High-speed high-accuracy control III command with no high-speed high-accuracy control III enable conditions satisfied If the conditions shown in "Fine segment capacity for multi-part system" are not satisfied when G05P20000; is commanded, the high-speed high-accuracy control II mode is enabled, and "G05P10000" is displayed on the modal screen. In this case, even if all the conditions shown in "Fine segment capacity for multi-part system" are satisfied after G05P20000; has been commanded, the high-speed high-accuracy control III mode is not enabled. To enable the high-speed high-accuracy control III mode, command G05P20000; again. Machining program High-speed high-accuracy control III enable conditions Enable mode G41 XxYyDd; ...Tool radius compensation ON Enable conditions are not satG05 P10000 G05 P20000; ...High-speed high-accuracy control isfied. III command G40 XxYy; ...Tool radius compensation OFF 629 Enable conditions are satisfied. G05 P10000 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.4 Spline Interpolation ; G05.1 Q2/Q0 Function and purpose This function automatically generates a spline curve that passes through a sequence of points commanded by the fine segment machining program, and interpolates the path along this curve. This enables high-speed and high-accuracy machining to be achieved. G64/G61.1 G61.2/G05.1Q2 There are two types of spline interpolation command format: G61.2 and G05.1Q2. Both formats can be used regardless of the parameter "#1267 ext03/bit0" setting if the spline interpolation specifications are available to the machine. This section describes the G05.1Q2 command. For G61.2, refer to "17.6 High-accuracy Spline Interpolation ; G61.2". The G05.1Q2 command can be issued when the machining parameter "#8025 SPLINE ON" is set to "1" in the highspeed high-accuracy control function II mode (between G05 P10000 and G05 P0) The following explanation is limited to the spline function in the high-speed high-accuracy control function II mode. Difference between G61.2 and G05.1Q2 Conditions under which the command can be issued and functions that are valid during a specific modal differ between G61.2 and G05.1Q2. Functions that become valid Conditions under Command format which the command Spline interpolation Fairing High-accuracy concan be issued trol (*2) G61.2 None G05.1 Q2 When the system is Valid in the high-speed high-accuracy control II mode and "#8025 SPLINE ON" is set to "1" (*1) Valid (*3) (*4) Valid Valid Can be turned ON and OFF using "#8033 Fairing ON" Valid (Because the system is in the high-speed high-accuracy control II mode) (*1) The validity of the high-speed high-accuracy control II function depends on the MTB specifications. A program error (P34) will occur if the conditions under which the command can be issued are not satisfied. (*2) The spline interpolation smoothly connects a sequence of points commanded by program. As a result, the glossy machining surface can be obtained, and the machining time can be reduced because the frequency of the corner deceleration decreases compared with conventional linear interpolation. (*3) Super-fine blocks often included in the data generated with CAM are deleted. Such a super-fine block may scratch the machining surface, and increase machining time because of acceleration/deceleration. This function prevents these problems. IB-1501278-D 630 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (*4) The following shows the functions and their operations included in the high-accuracy control described in this section. Functions of high-accuracy control Details Acceleration/deceleration before The process is the same as that performed in the high-accuracy interpolation (Constant inclination control mode (G61.1/G08P1). acceleration/deceleration, S-pattern filter) Optimum corner deceleration As is done in the high-accuracy control mode (G61.1/G08P1), optimum corner deceleration is performed at points where the angle between blocks exceeds the spline cancel angle or points at the boundary between G01 and G00, because spline interpolation is temporarily canceled to make corners. Arc speed clamp (For spline interpolation, curvature speed clamp) Clamp speed is calculated based on the spline curvature radius. The process for arc blocks is the same as that performed in the high-accuracy control mode (G61.1/G08P1). Curvature radius speed clamp Clamp speed is calculated based on the spline curvature radius. Arc entrance/exit deceleration control The process for arc blocks is the same as that performed in the high-accuracy control mode (G61.1/G08P1). SSS Control Optimum speed control is performed so that the process is not affected by steps or reverse runs. Feed forward control The process is the same as that performed in the high-accuracy control mode (G61.1/G08P1). The validity of the SSS control function depends on the MTB specifications. Command format Spline interpolation mode ON G05.1 Q2 X0 Y0 Z0 ; Spline interpolation mode OFF G05.1 Q0 ; 631 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Detailed description Temporary cancellation of spline interpolation Normally, once the spline function is activated, one curve is generated by smoothly connecting all points until it is canceled. However, if a corner edge should be created, or if the segment length is long and spline interpolation should not to be carried out, the function can be canceled temporarily with the parameters. (1) Cancel angle If the angle θ of two consecutive blocks exceeds the value set in parameter "#8026 CANCEL ANG.", the spline function will be temporarily canceled, and optimum corner deceleration will be applied. When this parameter is not set (=0), the spline interpolation will be constantly applied. The corner deceleration angle of the high-accuracy control function is valid during the temporary cancellation, and the optimum corner deceleration will be applied. (Example 1) Cancel angle = 60° Programmed command Spline interpolation path (Example 2) Cancel angle = 0° Programmed command Spline interpolation path <Note> If the section to be a corner is smooth when actual machining is carried out, lower the "CANCEL ANG.". If a smooth section becomes a corner, increase the "CANCEL ANG.". If "CANCEL ANG." >= "DCC ANGLE", the axis will decelerate at all corners where the angle is larger than the "CANCEL ANG." . If the "CANCEL ANG." < "DCC ANGLE", corner deceleration will not be applied if the corner angle is equal to or less than "DCC ANGLE" even if the spline interpolation is canceled. IB-1501278-D 632 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (2) Fine segment length If the movement amount in a block is longer than the parameter "#8030 MINUTE LENGS", the spline function will be temporarily canceled, and the linear interpolation will be executed. When this parameter is not set (= 0), the fine segment length will be 1mm. When the segment length in a block > fine segment length (#8030 MINUTE LENGS), the linear interpolation will be executed. Linear interpolation If the fine segment length is set to "-1", the spline interpolation will not be canceled according to the block length. (3) When a block without movement exists If a block without movement exists during the spline function is operating, the spline interpolation will be canceled temporarily. Note that blocks containing only ";" will not be viewed as a block without movement. Block without movement (4) When a block markedly longer than other blocks exists in spline function Given that the i-th block length is Li in the spline interpolation mode and if the following condition is met, the block will be interpreted as a linear section, and the spline interpolation mode will be temporarily canceled: Li > Li-1 x 8 or Li > Li+1 x 8 However, if the parameter "#8030 MINUTE LENGS" is set to "-1", the mode will not be canceled. Li > Li-1 × 8 or Li > Li + 1 × 8 Li - 1 Li+1 633 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Spline interpolation curve shape correction Normally, once the spline function is enabled, one curve is generated by connecting all points smoothly until the function is canceled. But if the spline curve shape should be corrected, the spline curve shape can be corrected with the parameters. (1) Chord error of block containing inflection point When changing the CAD curve data into fine segments with the CAM, normally, the tolerance (chord error) of the curve is approximated in segments that are approx. 10μm. If there is an inflection point in the curve, the length of the block containing the inflection point may lengthen. (Because the tolerance is applied at both ends near the inflection point.) If the block lengths with this block and the previous and subsequent blocks are unbalanced, the spline curve in this block may have a large error in respect to the original curve. At sections where the tolerance (chord error) of the fine segment block and spline curve in a block containing this type of inflection point, if the chord error in the corresponding section is larger than the value set in parameter (#8027 Toler-1), the spline curve shape is automatically corrected so that the error is within the designated value. However, if the maximum chord error of the corresponding section is more than five times larger than the parameter "#8027" setting value, the spline function will be temporarily canceled. The curve is corrected only in the corresponding block. The corrections are carried out under the following conditions for each block in the spline interpolation mode. There is an inflection point in the spline curve, and the maximum error of the spline curve and linear block is larger than parameter "#8027". (Distance between P3-P4 in Fig. 1) When the above conditions are satisfied, the spline curve will be corrected so that the error between P3-P4 in Fig. 2 is within the designated value. Tolerance (chord error) Spline curve P2 P1 P3 Inflection point P0 Fine segment P7 P4 P6 P5 Fig. 1 Spline curve before error correction IB-1501278-D 634 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Chord error designated in the parameter "Toler" P3 Spline curve before correction Spline curve after correction P4 Fig. 2 Spline curve after error correction In parameter "#8027 Toler-1", set the tolerance when developed into fine segments with the CAM. Set a smaller value if the expansion (indentation) is apparent due to the relationship with the adjacent cutting paths. (2) Chord error of block not containing inflection point Even in blocks that do not contain an inflection point, if the block lengths are not matched, the tolerance of the spline curve may increase. The curve may also expand due to the effect of relatively short blocks. At sections where the tolerance (chord error) between the fine segment block and spline curve in a block without an inflection point becomes large, if the chord error in the corresponding section is larger than the value set in parameter (#8028 Toler-2), the spline curve shape is automatically corrected so that the error is within the designated value. However, if the maximum chord error of the corresponding section is more than five times larger than the parameter "#8028" setting value, the spline function will be temporarily canceled. The curve is corrected only in the corresponding block. The corrections are carried out under the following conditions for each block in the spline interpolation mode. There is no inflection point in the spline curve, and the maximum error of the spline curve and linear block is larger than parameter "#8028". (Distance between P2-P3 in Fig. 3) When the above conditions are satisfied, the spline curve will be corrected so that the error between P2-P3 in Fig. 4 is within the designated value. Spline curve Fine segment P2 P3 Tolerance (chord error) P1 P4 P5 Fig. 3 Spline curve before error correction 635 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Chord error designated in the parameter "Toler-2" Spline curve before correction P2 P3 Spline curve after correction P1 P4 P5 Fig. 4 Spline curve after error correction In parameter "Toler-2", set the tolerance when developed into fine segments with the CAM. Curvature speed clamp The commanded speed F for the spline function during a segment linear arc will be the speed commanded in the previously set modal. However, if the axis is fed with the same speed, excessive acceleration may occur at the sections where the curvature is large (where curvature radius is small) as shown below. Thus, the speed clamp will be applied. (a) F (c) (b) F (d) (a) Curvature small (b) Acceleration small (c) Acceleration large (d) Curvature large F: Feed command speed (mm/min) Acceleration and curvature With the spline function, the high-accuracy control function is always valid. Thus, even if the curvature changes such as in this curve, the speed will be clamped so that the tolerable value for pre-interpolation acceleration/deceleration, which is calculated with the parameters, is not exceeded. The clamp speed is set for each block, and the smaller of the curvature radius Rs at the curve block start point and the curvature radius Re at the end point of the block will be used as the main curvature radius R. Using this main curvature radius R, the clamp speed F' will be calculated with expression (1). The smaller of this clamp speed F' and the commanded speed F will be incorporated for the actual feedrate. This allows cutting with an adequate feedrate corresponding the curvature radius along the entire curve. F' Rs Rs : Block start point curvature radius (mm) Re : Block end point curvature radius (mm) R : Block main curvature radius (mm) (smaller one of Rs and Re) ∆V : Tolerable value of pre-interpolation acceleration/deceleration F : Clamp speed (mm/min) Re F' = R V= IB-1501278-D V 60 1000 100- Ks 100 (1) G1bF(mm/min) G1btL(ms) 636 G1bF : Target pre-interpolation acceleration/deceleration G1btL : Acceleration/deceleration time to reach the target speed Ks : Accuracy coefficient M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Program example : G91; G05 P10000 ; High-speed high-accuracy control function II mode ON : G05.1 Q2 X0 Y0 Z0; Spline interpolation mode ON G01 X1000 Z-300 F1000; X1000 Z-200 ; Y1000; X-1000 Z-50 ; X-1000 Z-300 ; G05.1 Q0 ; Spline interpolation mode OFF : G05 P0 ; High-speed high-accuracy control function II mode OFF : (1) The spline function carries out spline interpolation when the following conditions are all satisfied. If the following conditions are not satisfied, the spline function will be canceled once, and the judgment whether to carry out new spline from the next block will be made. It is the movement only of three axes set to the basic axes I, J and K. When the block length is smaller than the value of the machining parameter "#8030 MINUTE LENGS". When the movement amount is not 0. When one of the following modes is entered. G01: Linear interpolation, G40: Tool compensation cancel, G64: Cutting mode, G80: Fixed cycle cancel, G94: Feed per minute When only an axis commanded with G05.1Q2 is commanded. A single block is not being executed. (2) Graphic check will draw the shape of when the spline interpolation OFF. (3) During the spline function mode, the command to the axis must be issued after G05.1 Q2 in the same block. For example, if the X axis and Y axis are to be commanded in the spline function mode, command "G05.1 Q2 X0 Y0;". The command block containing an axis not designated with this command (G05.1 Q2 X0 Y0) in the spline function mode will carry out linear interpolation instead of spline interpolation. (4) If G05.1 Q2 is commanded when not in the high-speed high-accuracy control function II mode (between G05 P10000 and G05 P0), the program error (P34) will occur. (5) If the machining parameter "#8025 SPLINE ON" is "0" in the high-speed high-accuracy control function II mode (between G05 P10000 and G05 P0) and G05.1 Q2 is commanded, the program error (P34) will occur. (6) Up to three axes set as the basic axes I, J and K can be commanded for the spline function. Relationship with other functions Refer to Relationship with other functions in "17.2 High-accuracy Control". 637 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Precautions (1) If this function are not provided and "G05.1 Q2" is commanded, the program error (P39) will occur. (2) Even if "-1" is set for parameter "#8030 MINUTE LENGS", the spline function will be temporarily canceled by the cancel conditions (cancel angle, non-movement block, excessive chord error, etc.) other than the block length. (3) Command "G05.1 Q2" and "G05.1 Q0" commands in independent blocks. A program error (P33) will occur if not commanded in independent blocks. (4) The program error (P33) will occur if the G05.1 command block does not contain a Q command. (5) A program error (P34) will occur if the number of axis in the part system does not exceed 3. IB-1501278-D 638 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.5 Spline Interpolation 2; G61.4 Function and purpose This function automatically generates a curve that smoothly passes through within the tolerable error range. The tool is able to move along the curve, providing smooth machining. This function allows the machine to operate with the optimum tool path and speed, simply by specifying the tolerance, so an operator can easily attain high quality machining. This function also requires the tolerance control specifications because it can only be used under tolerance control. The tolerance refers to the allowable error amount between the path commanded in the machining program and the path output by NC. Tolerance Tool path Commanded position This function is enabled when the following three conditions are satisfied: (1) Tolerance control is valid. (2) The specifications of spline interpolation 2 are valid. (3) "G61.4" is commanded from the machining program. If G61.4 is commanded while tolerance control is invalid, a program error (P34) will occur. If G61.4 is commanded while the specifications of spline interpolation 2 are not defined, a program error (P39) will occur. Command format Spline interpolation 2 mode ON G61.4 (,K__); , K: Tolerance (mm) Spline interpolation 2 mode with command G61.4 will be cancelled by designating any one of G code group 13. G61 (Exact stop check mode) G61.1 (High-accuracy control mode) G61.2 (Spline interpolation command) G62 (Automatic corner override) G63 (Tapping mode) G64 (Cutting mode) G08P1 (High-accuracy control mode start) G08P0 (High-accuracy control mode end) 639 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Detailed description Tolerance specification method Designate the tolerance using one of the following methods. Designate the tolerance using the parameter "#2659 tolerance". When the setting value is "0", this function runs with "0.01(mm)". Designate the numeric value following the ",K" address in the G61.4 command. (a) The range of the command value is 0.000 to 100.000 (mm). If a value exceeding the range is commanded, a program error (P35) will occur. (b) The tolerance designated by ",K" is applied to all axes in the part system. (c) When "0" is set to ",K" or ",K" is omitted, the program runs using the setting value of the parameter "#2659 tolerance" as the tolerance. (d) The tolerance designated by ",K" is not held after reset. Therefore, if ",K" is not designated in the G61.4 command after reset, the setting value of the parameter "#2659 tolerance" is enabled. [Program example] : G91 ; G61.4 ,K0.02; Designate tolerance 0.02 (mm). G01 X0.1 Z0.1 F1000 ; X0.1 Z-0.2 ; Y0.1 ; Tolerance: 0.02 (mm) G61.4 ,K0; Designate the tolerance 0 [mm]. X-0.1 Z-0.05 ; X-0.1 Z-0.3 ; Tolerance: Follows parameter "#2659 tolerance". G64 ; : Details of Operation Basic operations Spline interpolation 2 interpolates a command point row of the machining program with a smooth curve. The following figures show the command points and paths. Program command point Program command path Interpolated path IB-1501278-D 640 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Since the path is interpolated with a smooth curve, the interpolated path is different from that of the commanded path of the machining program. Set the tolerance between the interpolated path and commanded path in the parameter "#2659 tolerance". [For curve] [For corner] Tolerance amount Tolerance amount The interpolated path varies depending on the tolerance as shown below. For curve For corner Tolerance: High Tolerance: Low 641 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Temporary cancel While spline interpolation 2 is enabled, it may be canceled temporarily depending on commands. If spline interpolation 2 is canceled temporarily, the axis moves to the commanded position. After this, when a temporary cancel cause is removed, spline interpolation 2 restarts. The temporary cancel conditions are as follows. (1) The group 1 modal is not G01, G02, or G03. (2) The block has a G code other than G90, G91, G01, G02, or G03 commanded. (3) The block has M (miscellaneous function command value), S (spindle command rotation speed), T (tool command value), or B (2nd miscellaneous function command value) designated. (4) Under single block operation (For details, refer to "Single Block Operation".) (5) Modal in which SSS control is disabled temporarily (Modal shown below) NURBS interpolation Polar coordinate interpolation Cylindrical interpolation User macro interruption enable (M96) Feed per revolution (synchronous feed) Inverse time feed Constant surface speed control Fixed cycle 3-dimensional coordinate conversion Hypothetical axis interpolation Automatic tool length measurement Tool length compensation along the tool axis Normal line control Unidirectional positioning Exponential function interpolation 3-dimensional circular interpolation Path without temporary cancel Block without movement by temporary cancel Path without temporary cancel Block with movement by temporary cancel IB-1501278-D 642 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Feed hold Feed hold allows a deceleration stop in the middle of a curve. However, no interrupt operation can be performed. If the mode is switched to the manual mode or MDI mode during the feed hold, an operation error (M01 0180) will occur and the interrupt operation will be prohibited. After the program has been stopped by the feed hold, the movement on the curve can be restarted by the cycle start. The tool path specified just after the program has restarted is different from that specified when the program is not stopped by the feed hold, and the tool passes an area near the program-commanded shape. Program commanded shape NC commanded shape (Not stopped by the feed hold) NC commanded shape (Stopped by the feed hold) Single block operation During single block operation, spline interpolation 2 is canceled temporarily. In this period, linear interpolation is carried out at the commanded position. If single block is set to ON during continuous operation, the currently processed block stops on a curve, and the next and subsequent blocks stop on the commanded points. (c) Block stop at commanded position (a) Sets the single block signal ON. (d) Sets the single block signal OFF. (b) Block stop on curve (e) Restarts spline interpolation 2. 643 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Relationship with other functions Smooth fairing Spline interpolation 2 and smooth fairing can be used together. A spline interpolation 2 curve is generated along the points that are compensated by smooth fairing. Compensation by smooth fairing Smooth fairing OFF Smooth fairing ON Tool radius compensation Spline interpolation 2 and tool radius compensation can be combined. A spline curve is generated along the path for which the radius is compensated. High-speed high-accuracy control III Spline interpolation 2 and high-speed high-accuracy control III can be combined. However, the fine segment processing capacity is limited. Spline interpolation Spline interpolation 2 (G61.4) and spline interpolation (G61.2/G05.1Q2) cannot be combined. The following differences are between spline interpolation 2 (G61.4) and spline interpolation (G61.2/G05.1Q2). Feature of spline curve Parameter for adjusting the curve shape Spline interpolation 2 (G61.4) Passes near the commanded points. (*1) #2659 tolerance Spline interpolation (G61.2/G05.1Q2) Passes on the commanded points. #8026 CANCEL ANG. #8027 Toler-1 #8028 Toler-2 #8029 FairingL #8030 MINUTE LENGS #8033 Fairing ON (*1) The axis passes through the commanded points at the start and end points. The following shows differences between the spline interpolation 2 path and spline interpolation path. Spline interpolation 2 IB-1501278-D Spline interpolation 644 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Others G code Function name When the G codes shown on When spline interpolation 2 is enthe left are commanded while abled while the functions shown on spline interpolation 2 is enthe left are enabled abled G43.4 G43.5 Tool center point control Program error (P941) Program error (P942) G68.2 G68.3 Inclined surface machin- Program error (P953) ing command Program error (P951) G54.4 P1 to P7 Workpiece installation error compensation Program error (P545) Program error (P546) Precautions (1) The graphic check drawing is not carried out during spline interpolation 2 (the period from G61.4 to the cancel command). (2) PLC interrupt is not available during spline interpolation 2. If an PLC interrupt is performed during spline interpolation 2, the operation error (M01 0180) will occur. 645 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.6 High-accuracy Spline Interpolation ; G61.2 Function and purpose This function automatically generates a spline curve that passes through a sequence of points commanded by the fine segment machining program, and interpolates the path along this curve. This enables high-speed and high-accuracy machining to be achieved. This function has two functions; fairing function to delete unnecessary fine blocks, and spline interpolation function to connect smoothly a sequence of points commanded by the program. The high-accuracy control function G61.1 is also valid. The high-accuracy spline Interpolation is valid only for the first part system. G61.2 cannot be commanded in the 2nd part system even when the multi-part system simultaneous high-accuracy specifications are available. There are two types of spline interpolation command format: G61.2 and G05.1Q2. Both formats can be used regardless of the parameter "#1267 ext03/bit0" setting if the spline interpolation specifications are available to the machine. This section describes the G61.2 command. For information about differences between G05.1Q2 and G61.2 or features of spline interpolation, refer to "Spline Interpolation ; G05.1Q2". Command format G61.2 X__ Y__ Z__ F__ ; or G61.2 ; ... Spline mode ON X X axis end point coordinate Y Y axis end point coordinate Z Z axis end point coordinate F Feedrate The "G61.2" high-accuracy spline interpolation mode is canceled when any of the functions of G code group 13 is commanded. Detailed description (1) Fairing Refer to "Additional functions when high-speed high-accuracy control II mode is ON" in "High-speed high-accuracy control". (2) Spline interpolation Refer to "Detailed description" of "Spline Interpolation". IB-1501278-D 646 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Program example : G91 ; G61.2 ; G01 X0.1 Z0.1 F1000 ; X0.1 Z-0.2 ; Y0.1 ; X-0.1 Z-0.05; X-0.1 Z-0.3; G64 ; : ...... Spline interpolation mode ON ...... Spline interpolation mode OFF (1) The spline interpolation is available when the following conditions are all satisfied. If the following conditions are not satisfied, the spline function will be canceled once, and the judgment whether to carry out new spline from the next block will be made. - It is the movement only of three axes set to the basic axes I, J and K. - When the block length is smaller than the value of the machining parameter "#8030 MINUTE LENGS". - When the movement amount is not 0. - The group 1 command is G01 (linear interpolation). - Operation in fixed cycle modal - It is not during hypothetical axis interpolation mode. - It is not during 3-dimensional coordinate conversion modal. - It is not in a single block mode. (2) The spline function is a modal command of group 13. This function is valid from G61.2 command block. (3) The spline function is canceled by group 13 commands (G61 to G64). (4) The spline function is canceled by NC reset 2, reset & rewind, NC reset 1 (the setting which does not hold modal when NC is reset) or power ON/OFF. Precautions (1) If this function are not provided and G61.2 is commanded, the program error (P39) will occur. (2) Even if "-1" is set for parameter "#8030 MINUTE LENGS", the spline function will be temporarily canceled by the cancel conditions (cancel angle, non-movement block, excessive chord error, etc.) other than the block length. (3) Graphic check will draw the shape of when the spline interpolation OFF. (4) A program error (P34) will occur if the number of axis in the part system does not exceed 3. 647 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control 17.7 Machining Condition Selection I ; G120.1,G121 Function and purpose After initializing the machining condition parameter groups with the machining condition selection I function, the machining condition parameter groups can be switched by G code command. Switching is also possible on the machining condition selection screen. In that case, however, the machining conditions selected on the screen are applied to all part systems. Command format G120.1 P_ Q_ ; ... Machining condition selection I P Machining purpose 0: Reference parameter 1: Usage 1 2: Usage 2 3: Usage 3 Q Condition 1: Condition 1 2: Condition 2 3: Condition 3 When omitted, Q1 will be applied G121 ; ... Machining condition selection I cancel Detailed description (1) G120.1 and G121 commands are unmodal commands of G code group 0. (2) Switching of the machining condition parameter group using the G120.1 or G121 command is only applied to the commanded part system. (3) Command G120.1 and G121 in an independent block. If not, a program error (P33) will occur. (4) Address P in G120.1 command cannot be omitted. If omitted, a program error (P33) will occur. (5) Address Q in G120.1 command can be omitted. If omitted, it will be handled as "Q1 (condition 1)" is commanded. (6) When address P and Q in G120.1 command is commanded with a decimal point, the digit after the decimal point is ignored. (7) If other than "0 to 3" is set to address P in G120.1 command or other than "1 to 3" is set to address Q, a program error (P35) will occur. (8) When address P is set to "0" and address Q is omitted or set between "1" and "3" in G120.1 command, it will be switched to the reference parameter. (9) It will be switched to the machining condition parameter group selected in "Machining cond" screen by the G121 command. (10) When the emergency stop and reset (reset 1, reset 2, and reset & rewind) are performed while running the machining program whose machining condition parameter group is switched by G120.1 command, it will be switched to the selected condition parameter group machining in "Machining cond" screen. (11) Because the parameters are switched after being decelerated by G120.1 and G121 commands, the workpiece may be damaged. Make sure to keep the tool away from the workpiece when commanding G120.1 and G121. (12) When the machining condition parameter group is switched by G120.1 command more than once, the parameter group commanded last becomes valid. IB-1501278-D 648 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (13) It is switched to the selected machining condition parameter group in the "Machining cond" screen by program end (M02 and M30). (14) If G120.1 and G121 are commanded without initializing the machining condition parameter group, a program error (P128) will occur. (15) If the restart search from the block of the G120.1 or G121 command is attempted, a program error (P49) will occur. Program example "Machining cond" (setting) screen The displayed machining condition parameter group is switched depending on whether tolerance control is enabled or disabled. High-speed setting (for rough cutting machining) 649 Standard setting (for medium finishing machining) High-accuracy setting (for finishing machining) IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control (1) When "machine usage 1" and "condition 1" from the machining condition parameter group are selected in "Machining cond" (selecting) screen before running the program. N1 G91; G28 Z0; Operate with the machining condition parameter group N2 G28; X0 Y0; (machining usage 1/condition 1) N3 G90 G54 G00 X2. Y2.; N4 G43 H1 Z50.; N5 G90 G01 Z-5. F3000; N6 M3 S10000; N7 F2000; N8 G05 P10000; N9 G01; X2.099 Y1.99; N10 X2.199 Y1.990; : N1499 G05 P0; N1500 G91; G28 Z0; N1501 G28; X0 Y0; N1502 M5; N1503 G120.1 P1 Q3; N1504 G90 G54 G00 X2. Y2.; N1505 G43 H1 Z50.; ... The machining condition parameter groups are switched. Operate with the machining condition parameter group (machining usage 1/condition 3) N1506 G90 G01 Z-8. F3000; N1507 M3 S10000; N1508 F1200; N1509 G05 P10000; N1510 G01; X2.099 Y1.997; N1511 X2.199 Y1.990; : N2999 G05 P0; N3000 G91; G28 Z0; N3001 G28; X0 Y0; N3002 M5; N3003 M30; IB-1501278-D ... Return to the selected machining condition parameter group in "Machining cond" screen at the program end. 650 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control Relationship with other functions (1) G code modal that cause a program error when commanding G120.1 and G121 are listed below. G Code Function Program error when G120.1 and G121 are commanded G02.3, G03.3 Exponential interpolation P128 G06.2 NURBS interpolation P32 G07.1 Cylindrical interpolation P128 G12.1 Polar coordinate interpolation P128 G10 Parameter input by program P421 Tool compensation input by program G33 Thread Cutting G38 Tool radius compensation (vector P128 designation) P128 G39 Tool radius compensation (corner P128 arc) G41, G42 Tool radius compensation P128 3-dimensional tool radius compensation G41.1/G151 Normal line control Left P128 G42.1/G152 Normal line control Right P128 G43 Tool length compensation (+) P128 G44 Tool length compensation (-) P128 G43.1 Tool length compensation along the tool axis P128 G43.4, G43.5 Tool center point control P942 G66, G66.1 User macro (modal call A, B) P128 G68.2, G68.3 Inclined surface machining P951 G73/G74/G76/G81/G82/G83/ G84/G85/G86/G87/G88/G89 Fixed cycle P33(When G120.1 command is issued) P128(When G121 command is issued) Precautions (1) Because the parameters are switched after being decelerated once G120.1 or G121 is commanded, the workpiece may be damaged. Make sure to keep the tool away from the workpiece when commanding G120.1 and G121. (2) For the parameters "#8033 Fairing ON" and "#8090 SSS ON", the switched machining condition parameter group is effective only after it has been switched on the machining condition selection screen. (3) It is switched to the reference parameter by turning the power ON again. (4) The machining condition parameter cannot be switched on the "Machining cond" screen and cannot be set on the "Machining cond" screen during automatic operation. (5) When the machining condition parameter group is switched by the G120.1 command in the machining program during displaying the "Machining cond" screen, the selected machining condition parameter being displayed will not be switched unless the display screen is transited to the other screen once. (6) When G120.1 and G121 are commanded, parameters are switched when smoothing for NC axes in all part systems become "0". (7) The machining condition parameter group neither set the parameter setting from the program by G10 command nor read the parameters by system variables (from #100000). (8) When the machining condition parameter group is switched, the same values are used for all NC axes which belong to the switched part system to the parameter "#2010 Feed forward gain" and "#2659 Tolerance". 651 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 17 High-speed High-accuracy Control IB-1501278-D 652 18 Advanced Machining Control 653 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18Advanced Machining Control 18.1 Tool Position Compensation; G43.7/G49 Function and purpose The position compensation of a turning tool is executed when turning is performed in a machine of machining center system. Use of the tool position compensation enables the three base axes (X, Y and Z axes) to be compensated from the tool base position (base point). To set the compensation amount of the three base axes, switch the tool compensation display type to tool compensation type III. The validity of this parameter depends on the MTB specifications (parameter "#1046 T-ofs disp type"). Y axis tool compensation amount (base axis J) X axis tool compensation amount (base axis I) Z(+) Z axis tool compensation amount (base axis K) Y(+) Base position (base point) X(+) The tool position compensation function is valid for machining center compensation type II. This setting depends on the MTB specifications (parameter "#1037 cmdtyp"). Command format Tool position compensation start G43.7 H__; H Compensation No. (H0 cancels tool position compensation.) Tool position compensation cancel G49; The valid range of the compensation No. will differ according to the specifications (No. of compensation sets). If the commanded compensation No. exceeds the specification range, the program error (P170) will occur. The H address can be omitted. If omitted, the previously specified compensation No. is used. Note (1) Do not omit the H address. If the H address is omitted, an unintended operation may be performed by the H address that is input using a command other than G43.7. (2) Even if the H command is issued independently, the compensation amount corresponding to the compensation No. does not become valid. The compensation amount designated by the previous command is applied continuously. (3) If G43.7 is commanded with a type other than tool compensation type II of the machining center, the program error (P39) will occur. IB-1501278-D 654 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Detailed description Three base axes The tool position compensation function compensates the tool position for the axis specified in the parameter using the offset specified by the compensation No. The three base axes are determined by the following parameters. #1026 base_I (Base axis I) #1027 base_J (Base axis J) #1028 base_K (Base axis K) Differences between tool length compensation and tool position compensation [Tool length compensation (G43/G44)] Tool length compensation amount Z [Tool position compensation (G43.7)] X axis direction compensation amount Y axis direction compensation amount Base position (Base point) Z(+) X Y(+) X(+) The H address is used to compensate only one axis. Z axis direction compensation amount The H address is used to compensate three axis directions. 655 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Start-up and cancel operations When G43.7 is commanded in the program, tool position compensation is enabled, and the axis moves using the coordinate position, which is obtained by adding the compensation amount specified by the compensation No. to the end point coordinates specified in the movement command of the block, as the end point. This process is executed regardless of the absolute value command or incremental value command. Then, the compensation amount is added to the end point coordinates specified in the program until tool position compensation is canceled with a G49 command. Even except when the power is turned ON, G49 mode is set after M02 and M30 have been executed or after resetting has been performed. When no movement command is included in the same block as for G43.7 or G49, the operation depends on the MTB specifications (parameter "#1247 set19/bit0" (Movement by tool length offset)). For details, refer to "Movement by tool length compensation". For absolute command R N1 G91 G28 X0 Y0 Z0 ; N2 G00 G90 ; N3 G43.7 X-20. Y0. Z-40. H01 ; N4 Z-80. N5 G01 X-50. F500 ; N3 N4 For incremental command N1 G91 G28 X0 Y0 Z0 ; N2 G00 G91 ; N3 G43.7 X-20. Y0. Z-40. H01 ; N4 Z-40. N5 G01 X-30. F500 ; N5 Workpiece Program path Compensation No. (1) The compensation No. commanded in the same block as G43.7 will be valid for the following modals. G43.7 Hh1 ; : Used as the tool compensation amount of (lh1). G49; : Tool length compensation is canceled. G43.7; : Used again as the tool compensation amount of (lh1). (2) When G43.7 is further commanded in G43.7 mode, the compensation is applied by the tool compensation amount commanded later. G43.7 Hh1 ; : Used as the tool compensation amount of (lh1). G43.7 Hh2 ; : Used as the tool compensation amount of (lh2). (3) When the H command is issued independently during G43.7 modal, the compensation amount in modal mode is applied continuously. IB-1501278-D G43.7 Hh1 ; : Used as the tool compensation amount of (lh1). G43.7 Hh2 ; : Used as the tool compensation amount of (lh2). Hh3 ; : The compensation amount designated in (lh2) is applied continuously. 656 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Tool compensation cancel at reference position return operation If the reference position return operation is performed, the tool length compensation amount is canceled when the reference position return is completed. However, for the manual high-speed reference position return, the axis can be returned to the coordinates that are shifted by the tool length compensation amount again when the axis is moved after it has reached the reference position, using the parameter. (Parameter "#8122 Keep G43 MDL M-REF") Automatic reference position return (G28/G30) When the axis reached the reference position: Manual reference position return Dog type High-speed type Cancel Cancel Cancel When the axis moves af- Cancel ter the above: Cancel #8122 = 0: Cancel #8122 = 1: Reactivates tool length compensation amount that is applied before the axis reaches the reference position. (Example 1) Automatic reference position return operation G43.7 Xx1 Zz1 Hh1 ; : G28 Xx2 Zz2 ; Canceled when reference position is reached. (Same as when G49 is commanded.) G01 Xx3 Zz3 Ff3 ; : Performs the same operation as that in G49 mode. (Example 2) Manual dog-type reference position return operation (The same operation is also performed when "#8122" is set to "0" and manual high-speed reference position return is valid.) G43.7 Xx1 Zz1 Hh1 ; : (Interrupted by manual Canceled when reference position is reached. dog-type reference position return.) G01 Xx2 Zz2 Ff2 ; : Performs the same operation as that in G49 mode. (Example 3) When "#8122" is set to "1" and manual high-speed reference position return is valid: G43.7 Xx1 Zz1 Hh1 ; : (Interrupted by manual Canceled when reference position is reached. high-speed reference position return.) G01 Xx2 Zz2 Ff2 ; : The end point is set for the coordinates that are shifted by the compensation amount specified by compensation No. h1. The movement is commanded to the G53 machine coordinate system, the axis will move to the machine position when the tool compensation amount is canceled. If the movement command is issued first after G53, the axis returns to the coordinates that are shifted by the tool length compensation amount. 657 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Movement by tool length compensation If no movement command is included in the same block as for the G43.7 or G49 command, whether the axis moves to the current position by the specified compensation amount when the G43.7 command block is executed is determined depending on the MTB specifications (parameter "#1247 set19/bit0"). G43.7/G49 Independent command Not moved. (#1247 set19/bit0=1) ： G00 Xx Yy Zz ; G43.7 H1 ; (*1) ： G49 ; (*2) ： Moved. (#1247 set19/bit0=0) (*1) (*2) ： G00 Xx Yy Zz ; G43.7 H1 ; (*3) ： G49 ; (*4) ： (*3) (*4) (*1) Not moved. (*3) Movement by compensation amount (+) (*2) Not moved. (*4) Movement by compensation amount (-) If tool position compensation is commanded in- If tool position compensation is commanded independently, the axis does not move, but the dependently, the axis moves by the tool length tool compensation amount is applied to the pro- compensation amount. gram position counter. Movement command included ： G00 Xx Yy Zz ; G43.7 H1 X10.; (*3) ： G49 X5. ; (*4) ： (*3) (*4) (*3) Movement by compensation amount (+) (*4) Movement by compensation amount (-) If the tool position compensation and axis movement command are issued in the same block, the axis moves to the end point that is obtained by adding the tool length compensation amount to the movement command. IB-1501278-D 658 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Relationship with other functions Relationship between tool position compensation command and G code function Column A : Operation to be performed when the tool position compensation command (G43.7/G49) and another G command are issued to the same block Column B :Operation to be performed when another command is issued in G43.7 mode Column C : Operation to be performed when G43.7 is commanded in non-G43.7 mode ○ : Can be executed. - : The G43.7 command is ignored. P(xx) : The program error will occur. Modal group 0/1 1 G code G04 Function A Dwell P45 (*1) B ○ C ○ G05 High-speed high-accuracy II P33 ○ ○ G05.1 High-speed high-accuracy I P34 ○ ○ G07 Hypothetical axis interpolation P33 ○ ○ G08 High-accuracy control P33 ○ ○ G10 Parameter input by program / Compensation data P45 (*1) input by program ○ ○ G11 Parameter input by program cancel - ○ ○ G12/G13 Circular cut P32 (H command only) ○ ○ G27 Reference position check P45 (*1) ○ (*5) ○ G28 Reference position return P45 (*1) ○ ○ G29 Start position return P45 (*1) ○ ○ G30 2nd to 4th reference position return P45 (*1) ○ ○ G30.1 - G30.6 Tool change position return - ○ ○ G37 Automatic tool length measurement P801 P801 ○ G52 Local coordinate system setting P45 (*1) ○ ○ G53 Machine coordinate system selection P45 (*1) ○ ○ G53.1/G53.6 Tool Axis Direction Control P953 ○ ○ G65 User macro simple call P231 (*1) ○ ○ G115/G116 Start point timing synchronization P32 ○ ○ G120.1/G121 Machining condition selection I P33 ○ ○ G122 Activate sub part system I P651, P32 (*2) ○ ○ G02/G03 Circular interpolation P33 (*1) ○ G2.3/G3.3 Exponential function interpolation ○ ○ P33 G2.4/G3.4 3-dimensional circular interpolation P75 P75 P75 P33 ○ G06.2 NURBS interpolation ○ P32 7 G41.2/G42.2 3-dimensional tool radius compensation (Tool's ver- P163 tical-direction compensation) ○ P162 8 G43 Tool length compensation (+) ○ (*3) P801 P801 G43.1 Tool length compensation along the tool axis ON ○ (*3) P801 P930 G43.4/G43.5 Tool center point control ○ (*3) P941 P942 G44 Tool length compensation (-) ○ (*3) P801 P801 G49 Tool length compensation cancel ○ (*3) ○ ○ 9 G73 - G76 G81 - G89 Fixed cycle for drilling P801 ○ P801 14 G66 User macro modal call - (*4) ○ ○ 659 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Modal group G code Function A 16 G68 3-dimensional coordinate conversion mode ON G68.2/G68.3 19 G50.1 G51.1 21 G7.1/G107 G12.1/G112 Polar coordinate interpolation ON G13.1/G113 Polar coordinate interpolation cancel B C P923 ○ ○ Inclined surface machining command P954 ○ ○ G command mirror image cancel P801 ○ ○ G command mirror image ON P801 P801 P801 Cylindrical interpolation P33 ○ P481 P33 ○ P481 P33 ○ ○ 24 G188/G189 G code switch of program format P33 P29 ○ 27 G54.4 Workpiece installation error compensation P546 P546 ○ (*1) When the parameter "#1241 set13" is set to "1", G43.7 is ignored. (*2) If G122 is called before G43.7, the program error (P651) will occur. If it is called after G43.7, the program error (P32) will occur. (*3) When "G43.7 G43 H1;" is commanded, the G43 commanded later is enabled. (*4) Only the modal is updated. (*5) If the reference position return (G28) is commanded during the G43.7 modal, the G43.7 modal is canceled when the return is completed. Circular interpolation When the compensation by tool position compensation command G43.7 or G49 is applied to the circular movement axis, compensation movement is superimposed with circular movement if the axis moves by the specified compensation amount in the circular command block. Z Z axis tool compensation amount (Reference axis K) Uncompensated path Circular movement amount Path compensated by tool position compensation X Graphic check If the tool position compensation command G43.7 is issued during graphic check, the program error (P803) will occur. IB-1501278-D 660 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.2 Tool Length Compensation in the Tool Axis Direction ; G43.1/G49 Function and purpose (1) Changes in the tool length compensation in the tool axis direction and compensation amount The tool length can be compensated for in the tool axis direction even when the rotary axis rotates and the tool axis direction becomes other than the Z axis direction. By using this function, and setting the deviation between the tool length amount set in the program and the actual tool length as the compensation amount, a more flexible program can be created. This is especially valid for programs in which many axis movement commands are present. The tool length compensation amount in the tool axis direction can be changed by rotating the manual pulse generator when the tool length compensation amount in the tool axis direction is being changed during the tool length compensation in the tool axis direction mode. (2) Machine configuration The compensation using the tool length compensation in the tool axis direction function is applied to the direction of the tool tip axis (rotary axis). As for the axes that determine the compensation direction, a combination of the C axis (spindle) for Z axis rotation and the A axis for X axis rotation or B axis for Y axis rotation is designated using a parameter. (d) C A (e) (d) A/B (e) Z (f) B (f) C X (g) Y Axis A or B B A Axis B or C (d) Rotation center (e) Tool (f) Axis direction (compensation direction) (g) Workpiece 661 (g) Axis A or B IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Command format Tool length compensation along the tool axis ON G43.1 X__ Y__ Z__ H__ ; Tool length compensation cancel G49 X__ Y__ Z__ ; X, Y, Z Movement data H Tool length compensation No. (If the compensation No. exceeds the specification range, a program error (P170) will occur.) Detailed description (1) G43, G44 and G43.1 are in the same G code group. Therefore, it is not possible to designate more than one of these commands simultaneously for compensation. G49 is used to cancel the G43, G44 and G43.1 commands. (2) If the G43.1 command is designated when the specification for the tool length compensation in the tool axis direction is not provided, the program error (P930) will occur. (3) If reference position has not been completed for any of the X, Y, Z, A or B and C axes in the G43.1 block, the program error (P430) will occur. However, the error does not apply to the following cases. When mechanical axes have been selected The error does not apply to the A, B and C axes. When "1" has been set for the "#2031 noref" zero point return parameter The error does not apply to the axis for which "noref" is set to "1" because it is considered that the reference position return of the axis has already completed. IB-1501278-D 662 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Changing the amount of tool length compensation in the tool axis direction (1) When the following conditions have been met, the handle movement amount is added to the tool length compensation amount in the tool axis direction by rotating the manual pulse generator. When the operation mode is MDI, memory or tape operation mode and the state is "during single block stop", "during feed hold" or "during cutting feed movement". Note that compensation amount cannot be changed during error or warning. During tool length compensation in the tool axis direction (G43.1). In the tool length compensation amount in the tool axis direction changing mode (YC92/1). In the tool handle feed & interruption mode (YC5E/1). The 3rd axis (tool axis) is selected for the handle selection axis. (2) The change amount is canceled when the compensation No. is changed. Note The coordinate value in the tool length compensation amount in the tool axis direction change mode operates in the same manner as that when the manual ABS is ON, regardless of manual ABS switch (YC28) or base axis specification parameter "#1061 intabs". If compensation amount is changed during continuous operation, single block stop, or feed hold, the compensation amount will be effective immediately in the next block. (Example) When changing compensation amount during continuous operation. (b) (c) (d) (a) (Example) When changing compensation amount during single block stop. (b) (b) (c) (d) (a) (e) (a) Compensation amount before change (b) Changed compensation amount (c) Path after compensation (d) Program path (e) Single block stop When changing compensation amount, the compensation amount corresponding to the actual compensation No. will be changed. However, when executing the NC reset or tool length compensation in the direction of tool axis cancel (G49), the compensation amount will be returned to the original. 663 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Tool length compensation in the tool axis direction vector The vectors representing the tool length compensation in the tool axis direction are as follows. (1) When the A and C axes are set as the rotary axes: Vx = L * sin(A) * sin(C) Vy = -L * sin(A) * cos(C) Vz = L * cos(A) (2) When the B and C axes are set as the rotary axes: Vx = L * sin(B) * cos(C) Vy = L * sin(B) * sin(C) Vz = L * cos(B) Vx, Vy, Vz : Tool length compensation along the tool axis vectors for X, Y and Z axes L : Tool length compensation amount (1h) A, B, C : Rotation angle (machine coordinate position) of A, B and C axes (a) (c) (b) (d) (a) Path after tool length compensation in the tool axis di- (b) G43.1 command rection (c) Program path (d) G49 command (3) Rotary axis angle command The value used for the angle of the rotary axis (tool tip axis) differs according to the type of rotary axis involved. When servo axes are used: The machine coordinate position is used for the rotation angles of the A, B and C axes. When mechanical axes are used: Instead of the machine coordinate position of the axes, the values read out from the R registers (R2628 to R2631) are used for the rotation angles of the A, B and C axes. Compensation amount resetting Tool length compensation in the tool axis direction is cleared in the following cases. (1) When manual reference position return is completed. (2) When reset 1, reset 2 or reset & rewind has been executed. (3) When the G49 command has been designated. (4) When the offset No. 0 command has been executed. (5) When NC reset has been executed with "1" set for the basic system parameter "#1151 rstint". (6) When the G53 command is designated while the compensation status is still established, the compensation is temporarily canceled, and the tool moves to the machine position designated by G53. IB-1501278-D 664 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Program example Example of arc machining Shown below is an example of a program for linear -> arc -> arc -> linear machining using the B and C rotary axes on the ZX plane. Machining program X N01 G91 G28 X0 Y0 Z0 ; Compensation amount H01 = 50 mm N07 N02 G28 B0 C0 ; N08 N03 G90 G54 G00 X400. Y0 ; H01 = 50mm N09 N04 Z-150 ; N05 B90 ; B axis: 90° N06 G18 ; N07 G43.1; X250 H01; Tool length compensation in the tool axis direction ON N10 Z N08 G01 Z0 F200 ; N09 G02 X0 Z250. I-250. K0 B0 ; Top right arc, B axis: 0° N10 G02 X-250. Z0 I0 K-250. B90. ; N12 N11 G01 Z-150.; N12 G00 G49 X-400. ; N11 Bottom right arc, B axis: -90° Tool length compensation in the tool axis direction OFF N13 G91 G28 B0 C0 ; N14 G28 X0 Y0 Z0 ; N15 M02 ; Tool with no compensation Program path Path after compensation 665 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Relationship with other functions Relationship with 3-dimensional coordinate conversion (1) A program error (P931) will occur if 3-dimensional coordinate conversion is carried out during tool length compensation in the tool axis direction. (2) A program error (P921) will occur if the tool length is compensated for in the tool axis direction during 3-dimensional coordinate conversion. (3) A program error (P923) will occur if the tool length compensation in the tool axis direction is commanded in the same block as the 3-dimensional coordinate conversion. Relationship with automatic reference position return (1) A program error (P931) will occur if a command from G27 to G30 is issued during tool length compensation in the tool axis direction. Relationship with manual reference position return (1) Reference position return of orthogonal axis Tool length compensation along the tool axis will be canceled, as well as the dog-type reference position return and the high-speed reference position return. <Y axis Manual reference position return> N1 G90 G00 G54 X0 Y0 Z0 ; Z Positioning to the workpiece origin N2 45◦ N1 M N2 G00 A45.; Y Rotating the rotary axis by 45° N3 G43.1 H1 ; Tool length compensation along the tool axis ON W N3 N4 G19 G03 Y-5.858 Z-14.142 J14.142 K-14.142 A90. ; N4 Circular cutting Manual dog-type reference position return (a) N5 G00 Y0.; (a) N6 Z0 ; : : <Movement after Y axis Manual reference position return> N5 G00 Y0. ; Z Positioning to the position where tool length compensation along the tool axis was canceled. Y M N6 Z0. ; -> Positioning to the position where tool length compensation along the tool axis was canceled. W : : N6 N5 IB-1501278-D 666 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (2) Reference position return of rotary axis Tool length compensation along the tool axis will be canceled, as well as the dog-type reference position return and the high-speed reference position return. <A axis Manual reference position return> N1 G90 G00 G54 X0 Y0 Z0 ; Z Positioning to the workpiece origin N2 G00 A45.; N2 M Y Rotating the rotary axis by 45° N3 G43.1 H1 ; 45° Tool length compensation along the tool axis ON W N3 N3 N4 G19 G03 Y-5.858 Z-14.142 J14.142 K-14.142 A90. ; N4 Circular cutting Manual dog-type reference position return (a) 90° N5 G00 Y0.; (a) N6 Z0 ; : : <Movement after A axis Manual reference position return> N5 G00 Y0.; Z M Positioning to the position where tool length compensation in the tool axis direction was canceled. Y N6 Z0 ; Positioning to the position where tool length compensation in the tool axis direction was canceled. W : : N6 N5 Relationship with graphic check (1) Graphic check draws a path after compensation. 667 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.3 Tool Center Point Control; G43.4, G43.5/G49 Function and purpose The tool center point control function controls a commanded position described in the machining program to be the tool center point in the coordinate system that rotates together with a workpiece (table coordinate system). This function can be applied for the three types of machine as below. (1) A tool tilt type: a machine with two rotary axes set on the head. (2) A table tilt type: a machine with two rotary axes set on the table. (3) A combined type: a machine with one rotary axis set on the tool and another on the table. With this function, in the case of using tool tilt type, the tool center point is controlled so that it moves on the programmed path specified on the workpiece coordinate system. In the case of using the table tilt type, the tool center point is controlled so that it moves on the programmed path specified on the table coordinate system (a coordinate system which rotates together with a workpiece). (1) Tool tilt type Tool center point control OFF and tool length compensation along the tool axis ON Rotation center Tool Center Point Control ON Program path Rotation center Path of the tool center point Controls so that the path of the tool holder center point Controls so that the tool center point draws a straight draws a straight line. line. (2) Table tilt type Tool center point control OFF and tool length compensation along the tool axis ON Tool Center Point Control ON Path of the tool center point Z(+) Z(+) X(+) X(+) B(- ) X'(+) Z''(+) Rotation center B(- ) X''(+) Rotation center Controls so that the tool holder center point positions on Controls so that the tool center point positions on the tathe workpiece coordinate system. ble coordinate system. IB-1501278-D 668 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (3) Combined type Tool center point control OFF and tool length compensation along the tool axis ON Tool center point control ON Path of the tool center point Z(+) Z(+) Z'(+) X(+) X(+) B(- ) Z''(+) Rotation center X'(+) B(- ) X''(+) Rotation center Controls so that the tool holder center point positions on Controls so that the tool center point positions on the tathe workpiece coordinate system. ble coordinate system. If the tool center point control is commanded without the specifications of this function, a program error (P940) will occur. In addition, 3 orthogonal axes must be commanded first and 2 rotary axes alter. When the number of simultaneous contouring control axes is 4 When the number of simultaneous contouring control axes is 4, the tool center point control is only available for the simultaneous movement of 4 axes or less. Using this function allows you to designate the tool center point position on the table coordinate system (which rotates as the workpiece rotates); therefore, you can easily create a machining program without calculating the workpiece rotation or spindle end point position. [Restrictions] 5 or more simultaneous contour control axes Command type G43.4/G43.5 G43.4 only (*1) Limitations when com- None (Format error, etc. only) manded Interpolation mode A single rotary axis can be commanded in the same block. (*2) Joint interpolation / Single axis rotation in- Joint interpolation only terpolation (*3) Type of passing singu- Type 1 / type 2 (*3) lar point Program coordinate system selection 4 simultaneous contour control axes Invalid (*4) Table coordinate system / workpiece coordinate system (selected by parameter) (*3) Rotary axis basic posi- Zero degree position basis / start position standard (*3) tion selection Rotary axis prefiltering Select whether this function is valid or invalid with a parameter. Designate the time constant with a parameter. (*1) If G43.5 is commanded, a program error (P34) will occur. (*2) If two rotary axes are commanded, a program error (P10) occurs. However, if a single rotary axis only moves even when two rotary axes are commanded, it is not judged to be erroneous. (*3) Selected by a parameter. (*4) Only the joint interpolation is available in G43.4; therefore, the singular point type is invalid. 669 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control [Restrictions in movement command] o: Can be commanded, x: Alarm 3 orthogonal axes or less 1 rotary axis 2 rotary axes o o × 3 orthogonal axes 3 orthogonal axes or less + 1 rotary or less + 2 rotary axis axes o × Command format There are two command formats: <Type 1>, where tool angle is commanded by the rotary axis; and <Type 2>, where tool angle is commanded by the vectors of the workpiece surface, I, J, and K. Tool center point control ON G43.4 (X__ Y__ Z__ A__ C__) H__ ; G43.5 (X__ Y__ Z__) I__ J__ K__ H__ ; Type 1 ON Type 2 ON (*1) X,Y,Z Orthogonal coordinate axis movement command A,C Rotary axis movement command I,J,K Workpiece surface angle vector H Tool length compensation No. (*1) Can only be commanded when the number of simultaneous contouring control axes is 5 or more. Note (1) When orthogonal coordinate axis movement command or rotary axis movement command is not issued in the same block, start-up will be applied without axis movement (No movement for the compensation amount). (2) Commands to I, J, and K will be ignored during the tool center point control type 1. (3) Rotary axis movement command cannot be issued during the tool center point control type 2. If commanded, a program error (P33) occurs. (4) If I, J, or K is omitted when issuing the tool center point control type 2 command, the omitted address will be considered as "0". Tool center point control cancel G49 (X__ Y__ Z__ A__ C__); Note (1) Instead of using G49, other G codes in G code group 8 can be used for canceling. (2) If orthogonal coordinate axis command and rotary axis command are issued in the same block as G49, the tool center point control modal will be canceled on the spot. Then, commanded axis movement will be performed. If the cancel command is issued alone, the modal will be canceled on the spot, and yet no axis movement (movement for the compensation amount) will be performed. IB-1501278-D 670 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Detailed description Programming coordinate system Specify the end position of each block looking from the programming coordinate system in the tool center point control mode. In the program, specify the position of the tool center point. The programming coordinate system is a coordinate system used for the tool center point control, and whether to use the table coordinate system or the workpiece coordinate system depends on the MTB specifications (parameter "#7908 SLCT_PRG_COORD"). (1) Table coordinate system When "0" is set to the programming coordinate system selection parameter, the table coordinate system, which is the valid workpiece coordinate system at that time fixed to the table, is specified as the programming coordinate system. Table coordinate system rotates along the table rotation. And it does not rotate along the tool axis rotation. The X,Y,Z addresses are considered to have been issued on the table coordinate system. When a rotary axis movement is commanded in a block prior to G43.4/G43.5 command, the angle generated by rotary axis movement is regarded as an initial setting at G43.4/G43.5 command. (2) Workpiece coordinate system When "1" is set to the programming coordinate system selection parameter, the valid workpiece coordinate system at that time is specified as the programming coordinate system. The coordinate system in this case does not rotate along the table rotation. A linear movement is carried out for the table (workpiece) when the X,Y,Z addresses are issued. The end position looking from the workpiece coordinate system after table rotation is specified to the X, Y and Z. 671 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Rotary axis basic position selection When the table coordinate system, the workpiece coordinate system fixed to the table, is to be defined as a programming coordinate system, the appropriate rotary axis angle for fixing the workpiece coordinate system to the table depends on the MTB specifications (parameter "#7911 SLCT_STANDARD_POS"). Rotary axis standard selection The timing to be fixed to the table Operation example 1 (Workpiece coordinate offset 0°) Y Start position standard (#7911=1) Zero degree position standard (#7911=0) The position of rotary axis holding the work- When the position of rotary axis holding the piece at the start of tool center point control workpiece is at 0 degree on the workpiece coordinate system : G90G54G0C0 C-15. ; G43.4 Hh; : C90. ; : Workpiece coordinate 0° : G90G54C0 C-15. ; G43.4 Hh; : C90. ; : Y X Workpiece coordinate 0° Y X 0° 0° X M achine coordinate Machine coordinate Machine coordinate Machine coordinate Machine coordinate system position fixed at -15° position 90° by C90. position -15° by C-15. position 90° by C90. command command command Y Y Y -15° X Y X -15° Operation example 2 (Workpiece coordinate offset 45°) Y : G90G54G0C0 C-15. ; G43.4 Hh; : C90. ; : 90° -90° X Workpiece coordinate 0° : G90G54C0 C-15. ; G43.4 Hh; : C90. ; : Y X X X Workpiece coordinate 0° Y X 45° 45° Machine coordinate Fixed at machine co- Machine coordinate Machine coordinate Machine coordinate system ordinate position 30° position 135° by C90. position 30° by C-15. position 135° by C90. command command command Y Y X 30° IB-1501278-D Y 135° X 672 Y X 30° 135° X M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Start-up (1) Independent start-up command (a) Tool center point control type 1, type 2 When the tool center point control is ON, no axis movement is performed (including movement for the compensation amount). <Tool tilt type> : G43.4 Hh; : or : G43.5 Hh; <Table tilt type> : G43.4 Hh; : or : G43.5 Hh; A (+) Z Z Y A (+) Y (b) Tool center point control type 2 "G43.5 Ii Jj Kk Hh ; " performs the same movement as the tool center point control type 1 in (2). (2) Start-up with movement command (When orthogonal coordinate axis command is issued in the same block) (a) Tool center point control type 1, type 2 When the tool center point control is ON, the tool center point moves only as much as it is ordered under the incremental value command. <Tool tilt type> : G91; (Incremental value) G43.4 Yy Zz Hh; : or : G43.5 Yy Zz Hh; : <Table tilt type> : G91; (Incremental value) G43.4 Yy Zz Hh; : or : G43.5 Yy Zz Hh; : A (+) Z Z Y Y Z Z Y Y A (+) Under the absolute value command, the tool center point moves to y1, z1. <Tool tilt type> : G90; (Absolute value) G00 Yy0 Zz0; G43.4 Yy Zz Hh; : or : G43.5 Yy Zz Hh; : <Table tilt type> A (+) (y0,z0) (y1,z1) h z1- z0 Z y1- y0 Y : G90; (Absolute value) G00 Yy0 Zz0; G43.4 Yy Zz Hh; : or : G43.5 Yy Zz Hh; : (y0,z0) (y1,z1) h Z y1- y0 Y 673 z1- z0 A (+) IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (b) Tool center point control type 2 The rotary axis moves toward the commanded workpiece surface vector (I,J,K) direction along the movement command issued. <Tool tilt type> : G91; (Incremental value) G43.5 Yy Zz Ii Jj Kk Hh; : <Table tilt type> : G91; (Incremental value) G43.5 Yy Zz Ii Jj Kk Hh; : A (+) Z y z (i,j,k) (i,j,k) y Z z Y Y A (+) (3) Start-up with movement command (When rotary axis command is issued in the same block) (a) Tool center point control type 1 In the case of using the tool tilt type, the orthogonal axis moves according to the rotary axis angle while fixing the tool center point to the center. In the case of using the table tilt type, the orthogonal axis moves so that the tool center point locates on the rotated table workpiece coordinate system. <Tool tilt type> : G43.4 Aa Hh; : a Z <Table tilt type> A (+) : G43.4 Aa Hh; : z Z a Y Y (b) Tool center point control type 2 A program error (P33) will occur. IB-1501278-D A (+) 674 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Cancel (1) Independent cancel command (a) Tool center point control type 1, type 2 Canceling the movement for the compensation amount is not performed regardless of absolute/incremental value command. On the other hand, the tool center point control modal will be canceled. <Tool tilt type> : G49; : <Table tilt type> : G49; : A (+) Z Z A (+) Y Y The tool will not move. (2) Cancellation with movement command (When orthogonal coordinate axis command is issued in the same block) (a) Tool center point control type 1, type 2 Canceling the movement for the compensation amount is not performed regardless of absolute/incremental value command. Orthogonal coordinate axis movement command is executed upon cancellation of the tool center point control modal. <Tool tilt type> : G91; (Incremental value) G49 Yy Zz ; : <Table tilt type> : G91; (Incremental value) G49 Yy Zz ; : A (+) Z z z Z y A (+) Y y Y (3) Cancellation with movement command (When rotary axis command is issued in the same block) (a) Tool center point control type 1, type 2 Canceling the movement for the compensation amount is not performed regardless of absolute/incremental value command. Rotary axis movement command is executed upon cancellation of the tool center point control modal. <Tool tilt type> : G49 Aa Hh; : <Table tilt type> A (+) : G49 Aa Hh; : Z Y Z a A (+) a Y 675 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control During tool center point control (1) Tool center point control type 1 (a) When executing the movement command to the orthogonal coordinate axis and rotary axis. : A (+) Z G90 ; G43.4 Yy1 Zz1 Aa1 Hh ; a1 a2=0 a3 Yy2 Aa2 ; Yy3 Aa3 ; : The tool center point moves along the programmed path. z1 y1 y2 Y y3 (b) When executing the movement command to the rotary axis only. : A (+) G90 ; G43.4 Yy1 Zz1 Aa1 Hh ; a1 a2 Yy2 ; Aa2 ; Yy3 Aa3 ; : a3 z1 When executing the movement command to the rotary axis only, the orthogonal axis moves without moving the tool center point. y1 y2 y3 (2) Tool center point control type 2 (a) When executing the movement command to the orthogonal coordinate axis and the workpiece surface angle vector command. : A (+) (i3,j3,k3) Z G43.5 Yy1 Zz1 Ii1 Jj1 Kk1 Hh ; (i1,j1,k1) Yy2 Ii2 Jj2 Kk2 ; Yy3 Ii3 Jj3 Kk3 ; : Tool center point moves along the programmed path. (i2,j2,k2) z1 y1 y2 y3 (b) When executing the workpiece surface angle vector command only. : A (+) G43.5 Yy1 Zz1 Ii1 Jj1 Kk1 Hh ; (i1, j1, k1) Yy2 ; Ii2 Jj2 Kk2 ; Yy3 Ii3 Jj3 Kk3 ; : When executing the workpiece surface angle vector command only, the orthogonal axis moves without moving the tool center point. IB-1501278-D a3 (i3, j3, k3) z1 y1 676 y2 y3 Y M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Feedrate during tool center point control Feedrate during the tool center point control is controlled so that the tool center point moves according to the commanded speed. Interpolation method There are two methods of interpolation: single axis rotation interpolation and joint interpolation, which are selected by parameter. (1) Single axis rotation interpolation When transforming from a start-point angle vector "r1" into an end-point angle vector "r2", interpolate so that the angular rate of the rotary "φ" around the vector "k" axis, which is vertical to "r1"-"r2" plane, will be constant. (r1) Start-point command vector "r1" (k) (r2) End-point command vector "r2" (k) Unit vector vertical to r1-r2 plane Y(- ) (r1) O Y’( - ) (r2) Z( - ) Z’( - ) (a) Features Tool angle vector always exists on the plane consisting of "O", "r1" and "r2". The angular rates of each rotary axis will not be constant. (b) Operations (Example) Current position: Aa° , C0° When commanding "G90 Yy A-a. C45. ;" or "G90 Yy Ii Jj Kk ;" <Tool tilt type> <Table tilt type> Y(- ) Z’’ (+) Z(+) Z’(+) Y(+) Y’’ (+) Z(- ) Y’(+) Z(+) Y(+) <Combined type> Z(+) Z(+) Y(+) Z(+) Y(+) Z(+) Y(+) 677 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (2) Joint interpolation A movement from a start-point angle vector "r1" to an end-point angle vector "r2" is interpolated to keep the angular rates of each axis constant. (a) Features The angular rates of each rotary axis become constant. As this control aims to keep the angular rates of each rotary axis constant, a tool angle vector may not exist on the plane consisting of "O", "r1" and "r2". (r1) Start-point command vector "r1" C(+) (r2) End-point command vector "r2" Y(- ) A(+) O (r1) Z(- ) (r2) Passing singular point When passing the singular point (singular position (*1)), there are two kinds of movements to be followed from the singular point. When using an A-C axis tilt type machinery, there are two different movements (Fig. b, c) to be followed. In those movements, the rotation angles of the A axis are the same absolute value but different in signs (+/-). The rotation angles of the C axis corresponding the two movements are differed by 180 degrees one another. Determine which one of the two movements are to be selected with parameter. The figures below are the example of movements seen during tool center point control type 2. When the tool-centerpoint-side rotary axis moves in the sign (+) direction from the starting position (Fig. a), (Fig. b) is representing "passing singular point type 1". When the tool-center-point-side rotary axis moves in the sign (-) direction from the starting position (Fig. a), (Fig. c) is representing "passing singular point type 2". <Starting position> Y(- ) Movement in sign (+) Y(- ) C0 C0 Z(- ) (b) (a) Z(- ) Movement in sign (-) Y(- ) C0 Z(- ) (c) (*1) The position in which the tool-center-point-side rotary axis or the table-base-side rotary axis is 0. IB-1501278-D 678 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (1) Passing singular point type 1 Select the same direction as the start point of the tool-base-side rotary axis or table-workpiece-side rotary axis in the block where a singular point passing is carried out. When the rotation angle of the start point is 0°, select the wider stroke limit. When the stroke limits are the same, select the one with a minus-coded rotation angle. <Tool tilt type> X(- ) Y(- ) (c) (a) (b) Z(- ) <Table tilt type> (a) (b) Z'(+) Z(+) Z"(+) Y(+) Y'( - ) Y"( - ) (c) <Combined type> (a) (b) Z(+) Z(+) Z(+) Y(- ) Y(- ) Y(+) (c) (a) Singular point (b) When passing near the singular point, C axis rotates 180° within the parameter "#7907 CHK_ANG" (Near the singular judgment angle). (c) C axis rotates 180° 679 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (2) Passing singular point type 2 Select the one with the smaller rotary movement amount of the tool-base-side rotary axis or the table-workpieceside rotary axis on the singular point. When the tool-base-side rotary axis and the table workpiece have the same rotary movement amount, select the one with the tool-base-side rotary axis or the table-workpiece-side rotary axis that are to be rotated in the minus-coded direction. <Tool tilt type> X(- ) Y(- ) (a) Z(- ) <Table tilt type> (a) Z'(+) Z(+) Z"(+) Y'(+) Y(+) Y"(+) <Combined type> (a) Z(+) Z(+) Z(+) Y(+) Y(+) Y(+) (a) C axis does not rotate 180° when passing near the singular point. IB-1501278-D 680 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (3) Operation near the singular point in each interpolation method Interpolation method Command Single axis G43.4 rotation in- (Rotary axis terpolation command) G43.5 (I/J/K command) Joint inter- G43.4 polation (Rotary axis command) G43.5 (I/J/K command) Passing sin- Command from a singular point Command to pass a singular gular point to a non-singular point point type Type 1 Type 2 As designated in the command value. However, in the case where the signs at the start point and end point of either tool-center-pointside rotary axis or table-base-side rotary axis differ, if tool-base-side rotary axis or table-workpiece-side rotary axis rotates in the same block, the tool will not pass the singular point, resulting in a program error (P943). Type 1 Select the one with the wider stroke range. When the stroke range is the same, select a minus direction of the tool-center-point-side rotary axis or the table-base-side rotary axis. Type 2 Select the one with the smaller movement amount of the tool-baseside rotary axis or the table-workpiece-side rotary axis. Type 1 As designated in the command value. Select the one with the samecoded end point as the start point of the tool-center-pointside rotary axis or the tablebase-side rotary axis. Type 2 Type 1 Select the one with the wider stroke range. When the stroke range is the same, select a minus direction of the tool-center-point-side rotary axis or the table-base-side rotary axis. Type 2 Select the one with the smaller movement amount of the tool-baseside rotary axis or the table-workpiece-side rotary axis. 681 Select the one with the samecoded end point as the start point of the tool-center-pointside rotary axis or the tablebase-side rotary axis. IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Machine speed fluctuation suppression during high-accuracy control In tool center point control during high-accuracy control, if there is no change in a center point speed command (F command), and also if a rotary axis moves with each block's segment length short, the machine end speed (speed of a motor that drives the tool/table) may fluctuate sharply. By enabling the parameter "#7913 MCHN_SPEED_CTRL" (Machine speed fluctuation suppression), fluctuation can be suppressed. (1) When "#7913 = 0", the machine end speed is awaited to decelerate down to the machine end speed command (*1). Select this setting when a machining is desired to closely follow the movement commands. (2) When "#7913 = 1", the next block movement command is output to the machine immediately after a movement command output of the currently processed block is completed. Select this setting in such a case as an execution of a machining program with non-continuous rotary axis movement commands, where a smooth movement is desired preventing a sudden deceleration of the machine end speed between blocks. Nevertheless, if any of the conditions below is satisfied, deceleration is awaited regardless of the parameter setting. When judged to be a corner When the machining program's F command is changed When the speed is clamped When the override is changed (*1) A machine end speed command value means a speed command value that is output to the machine end so that the center point speed becomes the F command value. Nevertheless, depending on the machining program, enabling the parameter "#7913 MCHN_SPEED_CTRL" (Machine speed fluctuation suppression) may generate a machine vibration without deceleration. <Machining program example> Discontinuous rotary axis movement commands (a block is skipped between the movement commands) : G61.1; G43.4 Hh; G1 Ff; : N10 Xx1 Yy1 Zz1 Aa1; N20 Xx2 Yy2 Zz2; N30 Xx3 Yy3 Zz3 Aa3; N40 Xx4 Yy4 Zz4; : IB-1501278-D <Note> Center point block lengths are even. A machine end block length is longer when it has a rotary axis movement command. (In this case, the machine end speed is faster in a block with rotary axis movement than in a block without rotary axis movement.) When SSS control is enabled, a machine speed fluctuation suppression is disabled. 682 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (1) Speed when "#7913 = 0" Tool center point speed (F) 䊶䊶 N10 N20 N30 N40 䊶䊶 (T) Machine end speed (F) 䊶䊶 N10 N20 N30 N40 䊶䊶 (T) Center point command speed Machine end command speed (F) Actual speed (T) Time Awaited to decelerate down to the machine end speed of the next block. Thus, the speed changes sharply. (2) Speed when "#7913 = 1" Tool center point speed (F) 䊶䊶 N10 N20 N30 N40 䊶䊶 (T) Machine end speed (F) 䊶䊶 N10 N20 N30 N40 䊶䊶 Center point command speed (T) Machine end command speed (F) Actual speed (T) Time Not awaited to decelerate down to the machine end command speed of the next block. Thus, the speed does not change sharply, and the movement is smooth. In (2), because the control does not wait for the deceleration to the machine end command speed of the next block, the actual center point speed exceeds the command speed. In such a case, by adjusting (increasing) the setting value of "#1570 Sfilt2" (Soft acceleration/deceleration filter 2), a range of the excess of the center point speed can be suppressed even when it exceeds the command speed. <Note> When SSS control is enabled, a machine speed fluctuation suppression is disabled. 683 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Rotary axis prefiltering Rotary axis prefiltering means smoothing (prefiltering) the rotary axis command (tool angle shift) process, which moves the rotary axis smoothly and produces smoother cutting surface. Tool center point moves on the tracks as programmed by the rotary axis command while the command process is smoothed with this function. This function is available for the programs which have intermittent rotary axis commands (tool angle shifts) or the programs with inconstant shift amount of rotary axis angle (or tool angle) per unit time. Set the filter time constant for this function with parameters. When the rotary axis prefiltering is disabled, the tool center point shift speed may be sharply fluctuated due to the intermittent rotary axis command, as the figure below. (a) Q3 Q1 (b) Q5 Q4 Q6 Q7 Q8 (c) Q2 P0 Q9 P1 P2 P3 P4 P5 P6 P7 P8 P9 P10 (d) Q10 P11 (e) (a) Without tool angle shift (b) With tool angle shift (c) Machine position (rotation center) (d) Tool center point needs to be shifted at constant speed in spite of the tool angle shift. (e) Tool center point As shown below, the rotary axis prefiltering reduces speed fluctuation of tool center point by smoothing the rotary axis command process. (c) (a) Q1 P1 Q5 Q4 Q3 Q2 P0 (e) (b) P2 P3 P4 P5 Q6 P6 Q7 P7 P9 (d) Q9 P10 (g) (f) (a) Tool angle before smoothing (b) Tool angle after smoothing (c) With tool angle shift (d) Machine position (rotation center) (e) Without tool angle shift (f) Tool center point needs to be shifted at constant speed (g) Tool center point IB-1501278-D P8 Q8 684 P11 Q10 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Note (1) This function is available only when SSS control is enabled. (Not available together with a machine speed fluctuation suppression.) (2) This function is disabled at G00 command. (3) The actual angle of the tool may be deviated from the commanded one in the program. (4) Even if a rotary axis prefiltering is enabled for a program without an angle shift, it does not affect the machining quality. However, it may extend cycle time, so when executing such a machining, it is recommended that the rotary axis prefiltering is disabled. Mounting the rotary axis on the left-hand orthogonal coordinate system When tool center point control is used on the machine in which the rotary axis is mounted on the left-hand orthogonal coordinate system, all the following three conditions must be satisfied. (1) Use tool center point control type 1 (G43.4). (Normal operation is not assured in tool center point control type 2 (G43.5).) (2) Set the parameter "#7910 SLCT_INT_MODE" (interpolation mode selection) to the joint interpolation method. (Normal operation is not assured in single axis interpolation mode.) (3) Set the rotary axis configuration parameter "rotation direction" of the rotary axis mounted on the left-hand orthogonal coordinate system to CCW. The target "rotation direction" parameters are as follows. "#7923 DIR_T1" (Rotation direction of the tool rotating type base-side rotary axis) "#7933 DIR_T2" (Rotation direction of the tool rotating type / composite type tool axis) "#7943 DIR_W1" (Rotation direction of the table rotating type base-side rotary axis) "#7953 DIR_W2" (Rotation direction of the table rotating type / composite type workpiece axis) 685 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Circular command in tool center point control (G43.4/G43.5) When the following conditions are met, circular command will be executed on the selected plane in tool center point control. <Tool tilt type> Programming coordinate system Rotary axis reference position selection Start position standard (#7911=1) 0° position standard (#7911=0) Table coordinate system Rotary axis machine coordinate position in circular command is at 0°. (1) (2) (#7908=0) Workpiece coordinate system (#7908=1) <Table tilt type> Programming coordinate system Rotary axis reference position selection Start position standard (#7911=1) 0° position standard (#7911=0) Table coordinate system Rotary axis workpiece coordinate posi- Rotary axis workpiece coordinate po(#7908=0) tion at the start of tool center point con- sition in circular command is at 0°. (3) trol coincides with that of the circular command. (4) Workpiece coordinate sys- Rotary axis about the I/J/K axis workpiece coordinate position in circular comtem (#7908=1) mand is at 0°. (5) <Combined type> Programming coordinate system Rotary axis reference position selection Start position standard (#7911=1) Table coordinate system Table-side rotary axis workpiece coor(#7908=0) dinate position at the start of tool center point control coincides with that of the circular command, and also, tool-side rotary axis machine coordinate position in circular command is at 0°. 0° position standard (#7911=0) Table-side rotary axis workpiece coordinate position in circular command is at 0° and tool-side rotary axis machine coordinate position is at 0°. Workpiece coordinate sys- Tool-side rotary axis machine coordinate position in circular command is at 0° tem (#7908=1) and table-side rotary axis workpiece coordinate position is at 0°. <Note> (a) A program error (P942) will occur in the following cases. During tool center point control type 2 (G43.5) Rotary axis command is issued in the same block During the inclined surface machining and the workpiece installation error compensation (b) If the circular command is issued without positioning three orthogonal axes after tool center point control has been started independently, a program error (P70) or (P71) may occur. IB-1501278-D 686 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (1) Tool tilt type (Rotary axis machine coordinate 0°) <Machining program> : G18 G43.4 H1 : G02 Xx Zz Ii Kk : (a) Z(+) Y(+) Z(+) X(+) Y(+) X(+) (2) Tool tilt type (Rotary axis machine coordinate - 30°) <Machining program> : G18 G43.4 H1 A-30. : G02 Xx Zz Ii Kk : A-30 A0° Z(+) A(-) Y(+) Z(+) X(+) Y(+) (P) X(+) (3) Table tilt type (0° position standard) <Machining program> : G18 G43.4 H1 : G02 Xx Zz Ii Kk : Z(+) (a) Y(+) Z(+) X(+) Y(+) A(+) X(+) (a) Arc operations (P) Program error 687 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (4) Table tilt type (Start position standard) <Machining program> : G19 A-45. G43.4 H1 : G02 Xx Yy Ii Jj : Z(+) (a) A-45° :(s) Y(+) A0° Z(+) Y(+) X(+) A(+) X(+) (5) Table tilt type (Programming coordinate system = workpiece coordinate system) <Machining program> : G18 G43.4 H1 : G02 Xx Zz Ii Kk : Z(+) (a) Y(+) A0°:(s) Z(+) (I) X(+) Y(+) X(+) (a) Arc operations IB-1501278-D (s) Start position 688 (I) About I axis M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Relationship with other functions (1) F1-digit Feed Controls so that the tool center point moves at the commanded speed. Note that speed cannot be changed with the manual handle. (2) Buffer correction Buffer correction cannot be performed during tool center point control. (3) Miscellaneous function (MSTB) Miscellaneous function (MSTB) command can be executed during tool center point control. (When passing the singular point, strobe signal is output at the block start and the completion wait at the block end.) (Example) (b) Z : A (+) (a) (c) G90 Aa1 ; G43.4 Yy1 Aa2 Mm Hh ; a2 a : C (+) y1 (a) M strobe output Y (b) Passing singular point (c) M completion wait (4) Spindle/C Axis Control Axes unrelated to the tool tilt or table tilt can be controlled. (5) Manual reference position return Do not perform manual reference position return during tool center point control. If performed, the tool moves off the programmed track. (6) Machining time computation Machining time calculation is not performed accurately on the machining program in which the tool center point control mode is commanded. (7) Graphic trace Graphic trace during the tool center point control is always traced with the tool center point. (8) Graphic check Graphic check during the tool center point control is always check the graphic with the tool center point. (9) Program restart Restart search cannot be performed during the tool center point control. If attempted, a program error (P49) occurs. (10) Reset modal retention Canceled during the tool center point control. (11) Collation stop Position in the tool center point control can be collated and stopped. (12) Automatic operation handle interruption Do not perform the automatic operation handle interruption during the tool center point control. If performed, the tool moves off the programmed track. (13) Manual / Automatic simultaneous Manual / Automatic simultaneous cannot be executed to the axes related to the tool center point control during the tool center point control. (14) Tool handle feed & interruption Do not perform the tool handle feed & interruption during the tool center point control. If performed, the tool moves off the programmed track. (15) Corner chamfering/Corner R When the corner chamfering/corner R is performed during the tool center point control, the tool center point control becomes valid to the track after the corner chamfering/corner R. 689 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (16) Mirror image by parameter setting / external mirror image input When the tool center point control command is issued during the mirror image by parameter/external Input, a program error (P941) occurs. Also, do not turn the mirror image by parameter/external input ON during the tool center point control. (17) Linear angle command When A axis is used as a rotary axis, the linear angle command cannot be executed. When A axis is not used as a rotary axis, tool center point control becomes valid to the shape after the linear angle command. (18) Geometric command When A axis is used as a rotary axis, the geometric command cannot be executed. When A axis is not used as a rotary axis, tool center point control becomes valid to the shape after the geometric command. (19) Figure rotation The tool center point control becomes valid to the shape after the figure rotation. (20) Coordinate rotation by parameter When the tool center point control command is issued during the coordinate rotation by parameter, a program error (P941) occurs. Also, do not turn the coordinate rotation by parameter ON during the tool center point control. (21) Chopping Chopping operation for the 3 orthogonal axes and 2 rotary axes cannot be performed during the tool center point control. (22) Macro interruption If the macro interruption command is executed during the tool center point control, a program error (P942) occurs. (23) Tool life management The compensation amount of the tool center point control during the tool life management is equal to the compensation amount of the tool subjected to the tool life management. (24) G00 non-interpolation Functions as "G00 interpolation". (25) Actual feedrate display The final combined feedrate is displayed here. (26) Manual interruption When the manual interruption is executed during the feed hold or single block stop, the movement will be the one to be observed when the manual ABS is OFF when rebooting regardless of whether an absolute/incremental value command is selected. (27) Machine lock The each axis machine lock becomes valid to the motor axis. (28) Remaining distance counter Remaining distance at the tool center point on the programming coordinate system is displayed. (29) Interlock Interlock is applied for the motor axis. (30) Cutting feed / Rapid traverse override Override is applied to the feedrate at the tool center point. When the feedrate is clamped, the override is applied to the clamp speed. (31) Manual reference position return If the manual reference position return is performed during the tool center point control, the tool moves off the programmed track after that. (32) Dry run Dry run is applied to the speed at the tool center point. (33) NC reset Immediately decelerates to stop when the NC reset is executed during the tool center point control. The tool center point control will be canceled even if NC reset 1 and the modal retention. (34) Emergency stop Immediately stops if the emergency stop is applied during the tool center point control. (35) Stored stroke limit limit Stored stroke limit will be valid at the motor axis for all IB, IIB and IC. IB-1501278-D 690 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (36) MDI interruption When the MDI interruption is performed during the tool center point control, an operation error (M01 0170) occurs. (37) High-accuracy control function The acceleration at rapid traverse (G00) during the high-accuracy control is same as that at cutting feedrate (G01). Combination with arbitrary axis exchange When performing tool center point control in combination with an arbitrary axis exchange (G140) command, you need to set the rotary axis configuration parameters using the 2nd axis name. Set the parameter "#1450 5axis_Spec/bit0" to "1" (setting by the 2nd axis name), and assign the axis configuration for executing tool center point control to the rotary axis configuration parameter (#7900 or later) using the 2nd axis name (example: A1, B2). If the G43.4/G43.5 command is issued after arbitrary tool exchange has been completed while the parameter "#1450 5axis_Spec/bit0" is not designated, a program error (P941) will occur. You can set the configurations up to the number of valid part systems (up to four part systems) in the rotary axis configuration parameter. With multiple configurations set, you can perform tool center point control in different axis configurations. Tool center point control can be performed using the axis configuration in the part system with axis exchange completed by applying the rotary axis configuration parameter in the configuration in which all axes included in the part system are set. 691 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Relation with other G codes Pxxx in the list indicates the program error Nos. Column A: Operation to be carried out when the G command in the list is issued while this function is modal Column B: Operation to be carried out when this function is commanded while the G command in the list is modal Column C: Operation to be carried out when the G command in the list and this function are commanded for the same block All the G codes not listed above cannot be used. Format Function A B C G00 Positioning G01 Linear interpola- Switched to a cutting Perform tool center point Perform tool center point tion feedrate, and then per- control with cutting feed. control with cutting feed. form tool center point control. G02/G03 P941 Circular interpo- Available when some lation conditions are met. Refer to "Tool Center Point Control; G43.4/G43.5". P941 Helical interpola- P942 tion P941 P941 G02.1/G03.1 Spiral Interpola- P942 tion P941 P941 G02.3/G03.3 Exponential P942 function interpolation P941 P941 G04 Dwell - Tool center point control is ignored as dwell function takes precedence over the tool center point control function. G05 Switched to a rapid tra- Perform tool center point Perform tool center point verse feedrate, and then control at a rapid tracontrol at a rapid traperform tool center point verse feedrate. verse feedrate. control. Dwelling is performed. P1 (*1) High-speed ma- Max. feedrate is 16.8 m/ chining mode min when 1 mm segment G1 block is commanded with 5 axes simultaneously Max. feedrate is 16.8 m/ P33 min when 1 mm segment G1 block is commanded with 5 axes simultaneously P2 (*1) Max. feedrate is 100 m/ min when 1 mm segment G1 block is commanded with 5 axes simultaneously Max. feedrate is 100 m/ P33 min when 1 mm segment G1 block is commanded with 5 axes simultaneously P1000 High-speed high- Max. feedrate is 100 m/ 0 accuracy control min when 1 mm seg(*2) II ment G1 block is commanded with 5 axes simultaneously Max. feedrate is 100m/ P33 min when 1mm segment G1 block is commanded with 5 axes simultaneously G05.1 (*2) High-speed high- Max. feedrate is 33.7 m/ accuracy control min when 1 mm segI ment G1 block is commanded with 5 axes simultaneously Max. feedrate is 33.7 m/ P33 min when 1 mm segment G1 block is commanded with 5 axes simultaneously G06.2 NURBS interpo- P942 lation P*** NURBS general er- P941 ror G07.1 G107 Cylindrical inter- P942 polation P941 IB-1501278-D 692 P941 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Format G08 (*2) P0 Function High-accuracy control P1 A B C Perform tool center point Perform tool center point P33 control in cutting mode. control in cutting mode. Tool center point control Tool center point control P33 is performed in the high- is performed in the highaccuracy control mode. accuracy control mode. G09 Exact stop check G10/G11 - Deceleration check is performed at the block end. Parameter input P942 by program - P941 G10 Compensation data input by program P942 - P941 G12/G13 Circular cut P942 - Tool center point control is ignored as the circular cutting takes precedence over the tool center point control function. G12.1/G13.1 G112/G113 Polar coordinate P942 interpolation P941 P941 G15/G16 Polar coordinate P942 command P941 P941 G17 to G19 Plane selection The modal is switched to the specified plane. G20/G21 Inch/ Metric P942 G22/G23 Stroke check be- P942 fore travel P941 P941 G27 Reference posi- P942 tion Check - The tool center point control is ignored as the reference position check becomes valid. G28 Reference posi- P942 tion Return - The tool center point control is ignored as the reference position return becomes valid. G29 Start position re- P942 turn - The tool center point control is ignored as the start position return becomes valid. G30 2nd to 4th refer- P942 ence position return - The tool center point control is ignored as the 2nd, 3rd, 4th reference position return becomes valid. G30.1 to G30.6 Tool change po- P942 sition return 1 to 6 - P941 G31 Skip Deceleration check is performed at the block end. The modal is switched to the specified plane. Tool center point control P941 is performed according to the inch / metric modal. P942 - P941 G31.1 to G31.3 Multi-step skip P942 - P941 G33 Thread cutting P942 P941 P941 G34 to G36/ G37.1 Special Fixed Cycle P942 - P941 G37 Automatic tool P942 length measurement - P941 693 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Format Function A B C G38 Tool radius com- P942 pensation vector designation - P941 G39 Tool radius com- P942 pensation corner circular command - P941 G40/G41/G42 Tool radius com- P942 pensation P941 P941 G40.1/G41.1/ G41.2/G150/ G151/G152 Normal line con- P942 trol P941 P941 G43/G44/G49 Tool length com- Tool length compensapensation tion can be performed upon tool center point control cancellation. Tool center point control The subsequently comcan be performed upon manded modal takes tool length compensa- precedence. tion cancellation. G43.1/G49 Tool length com- Tool length compensapensation along tion along the tool axis the tool axis can be performed upon tool center point control cancellation. Tool center point control The subsequently comcan be performed upon manded modal takes tool length compensa- precedence. tion along the tool axis cancellation. G45/G46/ G47/G48 Tool position off- P942 set - P941 G50/G51 Scaling P942 P941 P942 G50.1/G51.1 Mirror image P942 P941 P941 G52 Local coordinate P942 system Setting - The tool center point control is ignored as the local coordinate system setting becomes valid. G53 Machine coordi- P942 nate system selection - The tool center point control is ignored as the machine coordinate system selection becomes valid. G54 to G59/ G54.1 Workpiece coor- P942 dinate system selection Tool center point control P941 is performed in the currently selected workpiece coordinate system. G60 Unidirectional positioning - The tool center point control is ignored as the unidirectional positioning becomes valid. G61 Exact stop check Deceleration check is mode performed at the block end. Deceleration check is performed at the block end. Deceleration check is performed at the block end. G61.1 High-accuracy control G61.2 High-accuracy P942 spline interpolation 1 P941 P941 G62 Automatic corner P942 override P941 P941 G63 Tapping mode P942 P941 P941 G64 Cutting mode Perform tool center point Perform tool center point Perform tool center point control in cutting mode. control at a cutting fee- control in cutting mode. drate. IB-1501278-D P942 Tool center point control Tool center point control Tool center point control is performed in the high- is performed in the high- is performed in the highaccuracy control mode. accuracy control mode. accuracy control mode. 694 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Format Function A B C Tool center point control Tool center point control Tool center point control becomes valid even in becomes valid even in is ignored as the user the user macro program. the user macro program. macro takes precedence over the tool center point control function. G65 to G67/ G66.1 User macro - User macro sub- User macro subprogram program termi- is terminated. nation Tool center point control will be ignored. - End position er- The end position error ror check cancel- check cancellation belation comes valid. - The end position error check cancellation, too, becomes valid. G68/G69 Coordinate rota- P942 tion P941 P941 G68IiJjKk/ G69 3-dimensional P922 coordinate conversion P941 P923 G70 to G89 Fixed cycle P942 The tool center point control is ignored as the start fixed cycle becomes valid. The tool center point control is ignored as the start fixed cycle becomes valid. G90/G91 Absolute/Incremental value command The modal is switched to the specified absolute / incremental value command, and then tool center point control is performed. Tool center point control is performed following the absolute / incremental modal. Tool center point control is performed under the specified absolute / incremental value command. G92 Machine coordi- P942 nate system setting - P941 G94 Feed per minute Tool center point control Tool center point control Tool center point control is performed in the feed- is performed in the feed- is performed in the feedperminute mode. perminute mode. perminute mode. G95 Feed per revolu- P942 tion P941 P941 G96/G97 Constant surface P942 speed control P941 P941 G98 Fixed cycle Initial The modal is switched to level return G98 and tool center point control becomes valid. The modal is switched to G98 and tool center point control becomes valid. The modal is switched to G98 and tool center point control becomes valid. G99 Fixed cycle (R The modal is switched to point level return) G99 and tool center point control becomes valid. The modal is switched to G99 and tool center point control becomes valid. The modal is switched to G99 and tool center point control becomes valid. G114.1 Spindle synchro- P942 nization P941 P941 (*1) It is valid when the parameter "#1267 ext03/bit0" is OFF. If it is commanded when this parameter is ON, the program error (P34) will occur. (*2) It is valid when the parameter "#1267 ext03/bit0" is ON. If it is commanded when the parameter is OFF, the program error (P34) will occur. 695 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.4 Inclined Surface Machining ; G68.2, G68.3/G69 Function and purpose Inclined surface machining function enables defining a new coordinate system (feature coordinate system) which is obtained by rotating and parallel translating the origin of the present coordinate system (X, Y, Z) (a coordinate system that existed before the inclined surface machining command was issued). With this function, you can define an arbitrary plane in a space and issue normal program commands to this plane in machining. It's possible to automatically control the tool axis to be in the + Z direction of the newly defined feature coordinate system. The feature coordinate system is redefined in accordance with the tool axis direction, thus there is no need to mind the feature coordinate system's direction and tool axis' rotation direction in making machining programs. If the inclined surface machining is commanded while this function is not defined in the specifications, it causes a program error (P950). Y Z Z X Y Original coordinate system Feature coordinate system X When workpiece installation error compensation is valid, the workpiece coordinate system is set to the workpiece installation coordinate system. In M830/M80, if the linear axis and two rotary axes are commanded to the same block, a program error (P10) will occur. (Example) When the following machining program is executed with machine configuration X-Y-Z-A-C : G68.2 X10. Y20, I0. J-45. K0.; : X20. A10 C20; Program error (P10) : G69; The feature coordinate system is defined using the following method. G Code G68.2 P0 Command method Define using Euler angles G68.2 P1 Define using roll-pitch-yaw angles G68.2 P2 Define using three points in a plane G68.2 P3 Define using two vectors G68.2 P4 Define using projection angles G68.2 P10 Define by selecting the registered machining surface G68.3 Define using tool axis direction G69 Cancel inclined surface machining command IB-1501278-D 696 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control If address P is omitted when G68.2 is commanded, it is assumed that G68.2 P0 is designated (define using Euler angles). If address P is not set to "0" to "4" or "10" when G68.2 is commanded, a program error (P954) will occur. If address P or Q of the G68.2 command includes a decimal point, it is rounded to an integer. Make sure to command G68.2, G68.3, and G69 in an independent block. If they are commanded in the same block as for other G codes or a motion command, etc., a program error (P954) will occur. The G69 command cannot be issued during circular interpolation or fixed cycle mode. If issued, a program error (P952) will occur. 697 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.4.1 How to Define Feature Coordinate System Using Euler Angles Command format Inclined surface machining mode ON (define using Euler angles) (P0 can be omitted.) G68.2 P0 X__ Y__ Z__ I__ J__ K__ ; X, Y, Z Feature coordinate system's origin Command by the absolute values with respect to the coordinate system before issuing the inclined surface machining command. I, J, K Euler angles (-360.0° to 360.0°) Note (1) If the address X, Y or Z is omitted, the address will be regarded as zero. When all of addresses X, Y, and Z are set to "0", the feature coordinate system's origin will be the same as that of the coordinate system before the inclined surface machining command is issued. (2) If the address I, J or K is omitted, the address will be regarded as zero. (3) If any address other than P, X, Y, Z, I, J and K is included, a program error (P954) will occur. Detailed description By commanding G68.2 P0 (define using Euler angles), the feature coordinate system (a coordinate system made by rotating and shifting the origin of the coordinate system before inclined surface machining) is defined. Coordinate system rotation is commanded using the Euler angles. (Example) When "G68.2 Xx Yy Zz Ia Jb Kc;" is commanded, the feature coordinate system is established as below. (a) Define a point (x, y, z) in the coordinate system before issuing the inclined surface machining command, as the feature coordinate system's origin. (b) Rotate the coordinate system, which was defined by shifting the origin in (a), by angle a about its Z axis. (c) Rotate the coordinate system, which was defined by rotation in (b), by angle b about its X axis. (d) Rotate the coordinate system, which was defined by rotation in (c), by angle c about its Z axis. (e) The coordinate system created in the above steps is the feature coordinate system. IB-1501278-D 698 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control If coordinate system's rotation is counter clockwise when viewing from the positive ends of the rotation center axis, this rotation will be considered as forward rotation. The relationship between the coordinate system before issuing the inclined surface machining command and the feature coordinate system is as shown below. (a) WZ (c) (b) Z b z Y Z Y WY x WX X a y X FY WZ (e) (d) FZ Y Z X FX WY z c x WX 699 y IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.4.2 How to Define Feature Coordinate System Using Roll-Pitch-Yaw Angles Command format Inclined surface machining mode ON (define using roll-pitch-yaw angles) G68.2 P1 Q__ X__ Y__ Z__ I__ J__ K__ ; X, Y, Z Feature coordinate system's origin Command by the absolute values with respect to the coordinate system before issuing the inclined surface machining command. Q Rotation order (q: Setting value for address "Q") q First Second Third 123 X Y Z 132 X Z Y 213 Y X Z 231 Y Z X 312 Z X Y 321 Z Y X If address Q is omitted, "q" will be handled as "123". I Rotation angle about the X axis (roll angle) (the setting range is from -360.0° to 360.0°) J Rotation angle about the Y axis (pitch angle) (the setting range is from -360.0° to 360.0°) K Rotation angle about the Z axis (yaw angle) (the setting range is from -360.0° to 360.0°) Note (1) If the address X, Y or Z is omitted, the address will be regarded as zero. When all of addresses X, Y, and Z are set to "0", the feature coordinate system's origin will be the same as that of the coordinate system before the inclined surface machining command is issued. (2) If the address I, J or K is omitted, the address will be regarded as zero. (3) If any address other than P, Q, X, Y, Z, I, J and K is included, a program error (P954) will occur. (4) A program error (P954) will occur if "q" is a value other than those listed above. IB-1501278-D 700 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Detailed description (Example) The feature coordinate system is established by the machining program as shown below. G68.2 P1 Q123 Xx Yy Zz Ia Jb Kc; (When q=123 [rotations in the order of WX, WY and WZ]) (a) Designate the feature coordinate system's origin by x, y and z (coordinates that existed before the inclined surface machining command was issued). (b) Rotate the shifted coordinate system by angle "a" about the X axis of the coordinate system before issuing the inclined surface machining command. (Roll angle) (c) Rotate the coordinate system, which was defined after rotation in (b), by angle "b" about the Y axis of the coordinate system before issuing the inclined surface machining command. (Pitch angle) (d) Rotate the coordinate system, which was defined after rotation in (c), by angle "c" about the Z axis of the coordinate system before issuing the inclined surface machining command. (Yaw angle) (e) The coordinate system created in the above steps is the feature coordinate system. (a) (b) FZ FY (c) a FY FX WZ WY FZ FX (x, y, z) WX (d) FZ (e) FZ FX c FY FX FY FZ FX b FY 701 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.4.3 How to Define Feature Coordinate System Using Three Points in a Plane Command format Inclined surface machining mode ON (define using three points in a plane) G68.2 P2 Q0 X__ Y__ Z__ R__ ; Shift amount setting G68.2 P2 Q1 X__ Y__ Z__ ; 1st point coordinate setting G68.2 P2 Q2 X__ Y__ Z__ ; 2nd point coordinate setting G68.2 P2 Q3 X__ Y__ Z__ ; 3rd point coordinate setting Q Designate the points Designate from the 1st to the 3rd points, or specify by the shift distance. 0: Shift distance 1: The 1st point 2: The 2nd point 3: The 3rd point X, Y, Z Shift amount between the 1st point and the feature coordinate system's origin (Shift amount setting) Command by the incremental value with respect to the feature coordinate system before parallel shift. R The angle to rotate the feature coordinate system about the Z axis (the setting range is from -360.0° to 360.0°) X, Y, Z (The 1st point) Designate the feature coordinate system's origin using with the workpiece coordinate system's position. (*1) X, Y, Z (The 2nd point) Designate a point on the feature coordinate system's X axis (+ direction) using with the workpiece coordinate system's position. (*1) X, Y, Z (The 3rd point) Designate a point on the feature coordinate system's Y axis using with the workpiece coordinate system's position. (*1) (*1) Command by the absolute values with respect to the coordinate system before issuing the inclined surface machining command. Note (1) If the address Q is omitted, the address will be regarded as zero. (2) If the address X, Y or Z in Q0 to Q3 is omitted, the address will be handled as zero. (3) If the address R is omitted, the address will be regarded as zero. (4) If any address other than P, Q, X, Y, Z and R is included, a program error (P954) will occur. (5) A program error (P954) will occur in the following cases. When any other command is included among G68.2 P2 Q0 to Q3. When any of G68.2 P2 Q1 to Q3 is lacked. When G68.2 P2 Q0 to Q3 are overlapped. When a value other than 0 to 3 is commanded in the address Q. When R is commanded in more than one block. (6) A program error (P955) will occur in the following cases. When the same point was designated for two or more points among the 1st to the 3rd points. When the three points exist on a straight line. The distance between one of the three points and the straight line connecting the other two points is less than 0.1 (mm). IB-1501278-D 702 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Detailed description (1) Designate the points Q1, Q2 and Q3 with respect to the coordinate system before issuing the inclined surface machining command. The point Q1 will be the origin of the feature coordinate system. (2) Define the X, Y and Z axes' directions of the feature coordinate system in the following procedure. Feature coordinate system's X axis is in the direction from the 1st point (Q1) to the 2nd point (Q2). Normally, designate a point on Y axis (+ direction) as Q3. (If the commanded X axis and Y axis are not at perfect right angles, the Y axis will be automatically compensated to be at right angles to the X axis.) Feature coordinate system's Z axis is in the direction of the cross product of (Q2-Q1)×(Q3-Q1). Feature coordinate system's Y axis is determined with respect to the right-handed system. (3) When shift distance (x0, y0, z0) of the feature coordinate system's origin is commanded, the feature coordinate system's origin is further parallel translated by (x0, y0, z0). Command the parallel translation distance with respect to the feature coordinate system before parallel translation. Always specify x0, y0 and z0 by incremental value. (4) When the rotation angle a is commanded in the address R, the feature coordinate system is rotated by the angle "a" about the Z axis of the feature coordinate system. (Example) The feature coordinate system is established by the machining program as shown below. G68.2 P2 Q0 Xx0 Yy0 Zz0 Ra ; G68.2 P2 Q1 Xx1 Yy1 Zz1 ; G68.2 P2 Q2 Xx2 Yy2 Zz2 ; G68.2 P2 Q3 Xx3 Yy3 Zz3 ; FZ (=FZ1) (4) FZ1 FY a Q3 FY1 (3) a FX (x0,y0,z0) WZ (1) Q1 Q2 (x1,y1,z1) FX1 (2) WY WX Coordinate system before issuing the inclined surface machining command (Workpiece coordinate system) 703 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.4.4 How to Define Feature Coordinate System Using Two Vectors Command format Inclined surface machining mode ON (define using two vectors) G68.2 P3 Q1 X__ Y__ Z__ I__ J__ K__ ; G68.2 P3 Q2 I__ J__ K__ ; Q Designate vectors Select the X axis direction vector or the Z axis direction vector. 1: X axis direction vector 2: Z axis direction vector X, Y, Z Feature coordinate system's origin Command by the absolute values with respect to the coordinate system before issuing the inclined surface machining command. I, J, K The feature coordinate system's X or Z axis direction vector When Q1 is commanded, the X axis direction vector is set. When Q2 is commanded, the Z axis direction vector is set. Command the direction with respect to the coordinate system before issuing the inclined surface machining command. The setting range is the same as the axis setting range, and the unit is dimensionless. Note (1) If the address X, Y or Z is omitted, the address will be regarded as zero. When all of addresses X, Y, and Z are set to "0", the feature coordinate system's origin will be the same as that of the coordinate system before the inclined surface machining command is issued. (2) If the address I, J or K in G68.2 P3 Q1 and Q2 is omitted, the omitted value will be handled as zero. (3) If any address other than P, Q, I, J and K is included, a program error (P954) will occur. (X, Y and Z are possible to command in G68.2 P3 Q1) (4) A program error (P954) will occur in the following cases. When any other command is included between G68.2P3 Q1 and Q2. When either G68.2 P3 Q1 or Q2 is lacked. When G68.2 P3 Q1 and Q2 are overlapped. When a value other than 1 to 2 is commanded in the address Q. When the address Q is omitted (5) A program error (P955) will occur in the following cases. When all of addresses I, J, and K are set to "0": When the angle formed by the feature coordinate system's X and Z vectors is not a right angle, and the deviation is 5 degrees or more. IB-1501278-D 704 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Detailed description (1) Designate the feature coordinate system's origin by x, y and z (coordinates that existed before the inclined surface machining command was issued). (2) Define the X, Y and Z axes' directions of the feature coordinate system in the following procedure. Feature coordinate system's X axis positive direction is rx = (ix, jx, kx). Feature coordinate system's Y axis positive direction is that of the cross product of (iz, jz, kz)×(ix, jx, kx). The feature coordinate system's Z axis is determined with respect to the right-handed system. The direction of rx=(ix, jx, kx) is the X axis of the feature coordinate system. Normally, the direction of rz=(iz, jz, kz) is the Z axis (positive direction) of the feature coordinate system. (If rx and rz are not at perfect right angle to each other, they will be automatically compensated so that they are at right angle to the X axis.) (Example) The feature coordinate system is established by the machining program as shown below. G68.2 P3 Q1 Xx Yy Zz Iix Jjx Kkx ; G68.2 P3 Q2 Iiz Jjz Kkz ; rz=(iz,jz,kz) rx=(ix,jx,kx) FZ FX FY (x,y,z) Y X WZ Z WY WX Coordinate system before issuing the inclined surface machining command (Workpiece coordinate system) 705 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.4.5 How to Define Feature Coordinate System Using Projection Angles Command format Inclined surface machining mode ON (define using projection angles) G68.2 P4 X__ Y__ Z__ I__ J__ K__ ; X, Y, Z Feature coordinate system's origin Command by the absolute values with respect to the coordinate system before issuing the inclined surface machining command. I The angle to rotate the X axis about the Y axis of the coordinate system before issuing the inclined surface machining command (the setting range is from -360.0° to 360.0°) J The angle to rotate the Y axis about the X axis of the coordinate system before issuing the inclined surface machining command (the setting range is from -360.0° to 360.0°) K The rotation angle about the Z axis of the feature coordinate system (the setting range is from -360.0° to 360.0°) Note (1) If the address X, Y or Z is omitted, the address will be regarded as zero. When all of addresses X, Y, and Z are set to "0", the feature coordinate system's origin will be the same as that of the coordinate system before the inclined surface machining command is issued. (2) If the address I, J or K is omitted, the omitted value will be handled as zero. (3) If any address other than P, X, Y, Z, I, J and K is included, a program error (P954) will occur. (4) A program error (P955) will occur when the angle formed by the X axis after rotating by the angle designated with address I about the Y axis, and the Y axis after rotating by the angle designated with address J about the X axis is 1 degree or less. Detailed description (1) Designate the feature coordinate system's origin by x, y and z (coordinates that existed before the inclined surface machining command was issued). (2) Define the X, Y and Z axes' directions of the feature coordinate system in the following procedure. The direction in which the X axis of the coordinate system before issuing the inclined surface machining command is rotated by angle a about the Y axis is defined as "ra". The direction in which the Y axis of the coordinate system before issuing the inclined surface machining command is rotated by angle b about the X axis is defined as "rb". Feature coordinate system's Z axis is in the direction of the cross product of (ra × rb). Feature coordinate system's X axis is in the direction determined by rotating "ra" by the angle "c" about the feature coordinate system's Z axis. Feature coordinate system's Y axis is determined with respect to the right-handed system. Note If "ra" and "rb" are considered to be parallel (or if the angle formed by the two vectors is 1 degree or less), a program error (P955) will occur. Except XZ and YZ plane, it is not possible to designate a plane that is in parallel with Z axis. IB-1501278-D 706 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (Example) The feature coordinate system is established by the machining program as shown below. G68.2 P4 Xx Yy Zy Ia Jb Kc ; FZ FZ rb FY b FY FX a FX c ra (x, y, z) Y WY WZ WX X Z Coordinate system before issuing the inclined surface machining command (Workpiece coordinate system) 707 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.4.6 Define by Selecting The Registered Machining Surface Command format Inclined surface machining mode ON (define R-Navi machining surface) G68.2 P10 Q__ D__ ; Q Workpiece No. designated by R-Navi or workpiece name designated by R-Navi D Machining surface No. designated by R-Navi or machining surface name designated by R-Navi Note (1) When address Q is omitted, select workpiece No. 1 if Q0,Q1 is commanded. (2) When address D is omitted, select machining surface No. 1 (BASE-SURFACE) if D0,D1 is commanded. (3) If any address other than P, Q, and D is designated when G68.2 P10 is commanded, a program error (P954) will occur. (4) A program error (P954) will occur when: a value other than 0 to 10 is commanded in address Q or an undefined workpiece name is designated; a value other than 0 to 17 is commanded in address D or an undefined machining surface name is designated; the workpiece name does not include a character string (command represented by "Q<>"); and the machining surface name does not include a character string (command represented by "D<>"). (5) If no feature coordinate system can be defined for the selected machining surface, a program error (P956) will occur. (6) If there are multiple workpieces or machining surfaces of the same name when the workpiece name or machining surface name is designated, a lower number is selected. (7) When the machining surface is called from the program, [SEL] or [*] is not displayed on the screen. Various PLC signals are not set to ON. (R-Navi machining surface selecting signal (XD28), R-Navi selecting workpiece No. signal (R660), R-Navi selecting machining surface No. signal (R661)) (8) When the machining surface is called from the program, the basic coordinate system designated by R-Navi for each workpiece is not selected. Before "G68.2 P10" is commanded, select a workpiece coordinate system from the program. (9) If you have defined a workpiece No. in address Q, define a machining surface No. in address D. If you have defined a workpiece name in address Q, define a machining surface name in address D. IB-1501278-D 708 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.4.7 How to Define Feature Coordinate System Using Tool Axis Direction Command format Inclined surface machining mode ON (define using tool axis direction) G68.3 X__ Y__ Z__ R__; X, Y, Z Feature coordinate system's origin Command by the absolute values with respect to the coordinate system before issuing the inclined surface machining command. R The angle to rotate the feature coordinate system about Z axis (the setting range is from -360.0° to 360.0°) Note (1) If the address X, Y or Z is omitted, the address will be regarded as zero. When all of addresses X, Y, and Z are set to "0", the feature coordinate system's origin will be the same as that of the coordinate system before the inclined surface machining command is issued. (2) If the address R is omitted, the omitted value will be handled as zero. (3) If any address other than X, Y, Z and R is included, a program error (P954) will occur. Detailed description (1) Designate the feature coordinate system's origin by x, y and z (coordinates that existed before the inclined surface machining command was issued). (2) Define the X, Y and Z axes' directions of the feature coordinate system in the following procedure. Feature coordinate system's Z axis is in the tool axis direction. Feature coordinate system's X axis is in the direction of the X axis of the coordinate system before issuing the inclined surface machining command after rotating with the tool. (When all the tool-side rotary axes are at 0 degrees (machine value), the feature coordinate system's X axis will be in the same direction as the X axis of the coordinate system before issuing the inclined surface machining command.) Feature coordinate system's Y axis is in the direction of the Y axis of the coordinate system before issuing the inclined surface machining command after rotating with the tool. (When all the tool-side rotary axes are at 0 degrees (machine value), the feature coordinate system's Y axis will be in the same direction as the Y axis in the coordinate system before issuing the inclined surface machining command.) Feature coordinate system is finally established by rotating the commanded angle with address R about the Z axis. 709 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (Example) The feature coordinate system is established by the machining program as shown below. G68.3 Xx Yy Zy Ra; FY a FZ FX a WZ WY WX Coordinate system before issuing the inclined surface machining command (Workpiece coordinate system) IB-1501278-D 710 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.4.8 Tool Axis Direction Control; G53.1/G53.6 Function and purpose A rotary axis is automatically moved so that the tool axis direction (direction from the tool's tip to the bottom) will be the feature coordinate system's +Z axis direction. For table tilt type and compound type machines, feature coordinate system may change in accordance with the rotation of the table rotary axis. The following two types of tool axis direction control can be utilized: Type 1 (G53.1 command) Only the rotary axis is moved. Type 2 (G53.6 command) The rotary axis and the orthogonal axis are moved by fixing the tool center point position in the view from the workpiece. Command format Tool axis direction control (type 1): Only the rotary axis is moved. G53.1 P__ ; Tool axis direction control (type 2): The rotary axis and the orthogonal axis are moved by fixing the tool center point position in the view from the workpiece. G53.6 P__ Q__ H__ ; P Select a solution for the rotary axis 0: Select a default solution for each machine type 1: Select a solution so that the primary rotary axis rotation is positive. 2: Select a solution so that the primary rotary axis rotation is negative. Q Select the rotation order of the rotary axes when the number of simultaneous contouring control axes is 4 axes or less and the operation at the time of G53.6 command is limited to simultaneous 4 axes (3 orthogonal axes + 1 rotary axis) or less. (In the following example, there are 2 rotary axes.) 0: The axes operate in the order set in the "#7917 SLCT_G53_6_ROTAX" parameter. 1: The axes operate in the order of primary rotary axis and secondary rotary axis. 2: The axes operate in the order of secondary rotary axis and primary rotary axis. Even if the number of simultaneous contouring control axes is 5 axes or more, the number can be limited to the simultaneous 4 axes (3 orthogonal axes + 1 rotary axis) or fewer by address Q command. However, when address Q command is "0", 5 axes operate simultaneously regardless of the parameter settings. H Tool length offset No. G53.1/G53.6 are group 00. Note (1) Command G53.1/G53.6 during inclined surface machining mode. If commanded in any other mode, a program error (P953) will occur. (2) Make sure to command G53.1/G53.6 surely in a block. If this command is issued in the same block as of other G codes or travel command etc., a program error (P953) will occur. (3) The travel speed when G53.1 is commanded follows the G group 1 modal (such as G00/G01) during the tool axis direction control command. (4) The travel speed on the feature coordinate system when G53.6 is commanded follows G group 1 modal (such as G00/G01). The travel speed of each axis may exceed the command speed as the tool tip position is fixed in the view from workpiece. However, rapid traverse (G00) is clamped by the parameter "#2001 rapid", and the cutting feed (G01) is clamped by the parameter "#2002 clamp". (These parameters depend on the MTB specifications.) 711 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (5) If the address P is omitted, the omitted value will be handled as zero. If any other value than 0, 1, and 2 is command, a program error (P35) will occur. (6) If any address other than P/N is commanded while commanding G53.1, a program error (P953) will occur. (7) When address Q is omitted at the time of G53.6 command, it is regarded that 0 is commanded. If any other value than 0, 1, and 2 is command, a program error (P35) will occur. (8) If any address other than P/H/N is commanded while commanding G53.6, a program error (P953) will occur. (9) When the address H is omitted, H modal commanded before G53.6 command will be applied. If H modal is not commanded, a program error (P953) will occur. (Example 1) (Example 2) : G43 H1 : G53.6 ← Use H1 : : G53.6 ← Error (P953) : (10) If the tool length offset No. is changed by address H command, a program error (P953) will occur. (Example 1) : G43 H1 ← Command the tool offset No.1 : G53.6 H2 ← If tool length offset No.2 is commanded, a program error (P953) will occur. : (11) If the offset amount for the tool No. that the address H is commanded is "0", a program error (P957) will occur. (Example 1) When "H1 = 0" (Example 2) When "H1 ≠ 0" (Example 3) When "0" is commaned to address H : G43 H1 : G53.6 ← Error (P957) : IB-1501278-D : : G43 H1 G53.6 ← Error (P957) : : H0 ← Tool length offset is "0" : while it remains G43 modal. G53.6 ← Error (P957) : 712 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Detailed description The operation of type 1 (G53.1) For the G53.1 command, the 3 orthogonal axes (X, Y, and Z axes) do not move, however, only the 2 rotary axes rotate simultaneously so that the tool axis direction is in line with the +Z direction of the feature coordinate system. (1) For compound type B-C axes When the G53.1 command is issued for a compound type (B-C axes) machine, the B axis of the tool and the C axis of the table rotate simultaneously. WZ B B WY FY FZ WX G53.1 FX C C (2) For table tilt type A-C axes When the G53.1 command is issued for a table tilt type (A-C axes) machine, the A and C axes of the table rotate simultaneously. WZ FZ G53.1 WY FY FX WX A A C C (3) For tool tilt type B-C axes When the G53.1 command is issued for a tool tilt type (B-C axes) machine, the B and C axes of the tool rotate simultaneously. C C WZ B WY FY B WX G53.1 FZ 713 FX IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Type 2 (G53.6) command For G53.6 command, the tool axis end position of the tool axis direction seen from workpiece is fixed to be in +Z direction in the feature coordinate system, and up to 3 orthogonal axes (x axis, Y axis, and Z axis) and 2 rotary axes moves simultaneously. The number of axes to be moved simultaneously is limited by the number of simultaneous contouring control axes. If the number of simultaneous contouring control axes is 4 axes or fewer, the rotary axes move separately. The order of rotary axes moving separately can be specified with address Q command. When the number of simultaneous contouring control axes is 5 axes or more, the rotary axes can also be moved separately by issuing the address Q command. [When the number of simultaneous contouring control axes is 5 axes or more] For G53.6 command, up to 3 orthogonal axes(X axis, Y axis, and Z axis) and 2 rotary axes can be moved simultaneously. (1) For compound type B-C axes When the G53.6 command is issued for a compound type (B-C axes) machine, the X, Y, Z, and B axes of the tool and the C axis of the table move simultaneously. WZ B WY WX FY B FZ G53.6 FX C C (2) For table tilt type A-C axes When the G53.6 command is issued for a table tilt type (A-C axes) machine, the X, Y, and Z axes of the tool and the A and C axes of the table move simultaneously. WZ FZ WY G53.6 FY WX FX A A C IB-1501278-D C 714 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (3) For tool tilt type B-C axes When the G53.6 command is issued for a tool tilt type (B-C axes) machine, the X, Y, Z, B, and C axes of the tool rotate simultaneously. C C WZ WY B FY WX G53.1 B FZ FX [When the number of simultaneous contouring control axes is 4 axes or fewer] Up to 3 orthogonal axes (X, Y, Z axes) and a rotary axis move simultaneously with G53.6 command. When 2 rotary axes move, the order of rotary axes to move is specified with the parameter “#7917 SLCT_G53_6_ROTAX” or address Q. When specifying "1" to the address Q, the axis moves in the order of primary rotary axis and secondary rotary axis. When setting "2" to the address Q, the axis moves in the order of the secondary axis and the primary axis. When executing the single block operation, either performing the block stop or not at the movement completion for each rotary axis can also be specified with parameter “#8132 G53.6 block stop”. (1) Compound type B-C axis (a) When moving in the order of primary rotary axis and secondary rotary axis First, the B axis ("B" in the figure below) of the tool rotates, and then the X, Y, and Z axes of the tool also move to fix the tool center position. Next, the C axis ("C" in the figure below) of the table rotates, and then the X, Y, and Z axes of the tool also move as if the tool follows the workpiece movement. WZ FY WY FZ WX B G53.6 FY B FZ FX FX C C WY WX FY FY FX FX 715 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (b) When moving in the order of secondary rotary axis and primary rotary axis First, the C axis ("C" in the figure below) of the table rotates, and then the X, Y, and Z axes of the tool also move as if the tool follows the workpiece movement. Next, the B axis ("B" in the figure below) of the tool rotates, and then the X, Y, and Z axes of the tool also move to fix the tool center position. WZ WY B FY FZ WX FY FZ B G53.6 FX C F X FX C WY WX F Y FY FY FX FX (2) For table tilt type A-C axes (When moving in the order of secondary rotary axis and primary rotary axis) First, the C axis ("C" in the figure below) of the table rotates, and then the X, Y, and Z axes of the tool also move as if the tool follows the workpiece movement. Next, the A axis ("A" in the figure below) of the table rotates, and then the X, Y, and Z axes of the tool also move as if the tool follows the workpiece movement. WZ WY FZ WX G53.6 FX A A C FY C WY WX FX FX FY FY IB-1501278-D 716 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (3) For tool tilt type B-C axis (When moving in the order of primary rotary axis and secondary rotary axis) First, the B axis ("B" in the figure below) of the tool rotates, and then the X, Y, and Z axes of the tool also move to fix the tool center position. Next, the C axis ("C" in the figure below) of the tool rotates, and then the X, Y, and Z axes of the tool also move to fix the tool center position. C WZ FY WX B G53.6 FY C WY FZ FZ B FX FX X F FY FY F X WY WX FX FX Select rotary axis' solution When G53.1 is commanded, there are normally two types of solutions for the rotary axis' calculated angle; one is to rotate the primary rotary axis positively, and the other negatively. Use the address P (P=0, 1 or 2) in G53.1 command to select either one of the solutions. These are the default solutions for each machine type. When P is "0": Selects a default solution for each machine type When P is "1": Selects a solution so that the primary rotary axis rotation is positive When P is "2": Selects a solution so that the primary rotary axis rotation is negative When the address P is omitted, P will be regarded as zero, so the default solution for each machine type is selected. If any other value than 0,1, and 2 is command, a program error (P35) will occur. These are the default solutions for each machine type. Machine type Primary rotary axis Solution selected by default Tool tilt type Tool-side 2nd rotary axis Selects a solution so that the primary rotary axis rotation is positive (same as when P is "1") Table tilt type Table-side 2nd rotary axis Selects a solution so that the primary rotary axis rotation is negative (same as when P is "2") Compound type Tool-side rotary axis Selects a solution so that the primary rotary axis rotation is positive (same as when P is "1") 717 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Primary rotary axis is the rotary axis which serves as the criteria for selecting the solution in G53.1 command. WZ WX WY FY FZ FX (*1) G53.1 P0 G53.1 P1 (*3) B>0 G53.1 P2 B<0 FY FZ FY FZ FX (*2) (*2) FX C C (*1) Indicates the 1st feature coordinate system. (*2) Indicates the 2nd feature coordinate system. (*3) For compound type machines, a solution that makes the primary rotary axis rotation positive is selected as a result of issuing the G53.1P0 command. IB-1501278-D 718 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.4.9 Details of Inclined Surface Machining Operation Detailed description Operation during inclined surface machining mode When inclined surface machining is commanded, the above-mentioned feature coordinate system is defined. By setting the parameters #8901 to #8906 to "23", you can display the coordinates of the feature coordinate system on the counter (no machine motion). The travel commands during inclined surface machining mode are handled with respect to the feature coordinate system. In the counter display of the feature coordinate system, whether the machining position on the program command that does not include the tool length compensation/tool radius compensation can be selected depends on the MTB specifications (parameter "#1287 ext23/bit1, bit2 (inclined surface coordinate display)". Tool Axis Direction Control When G53.1 is commanded, the rotary axis moves so that the tool axis direction will be + Z direction of the feature coordinate system. At this time, the rotary axis moves, but X, Y and Z axes won't move. The rotary axis' travel speed is determined based on the modal when G53.1 is commanded. CAUTION Depending on the feature coordinate system setting, rotary axis may move greatly in response to G53.1 command. Thus, before commanding G53.1, move the tool far enough away from the table. Cancel inclined surface machining mode The command G69 cancels the inclined surface machining. When this mode is canceled, the feature coordinate system setting will be canceled, the coordinate system will change back to the workpiece coordinate system when inclined surface machining was commanded, and workpiece coordinate position counter will change back to the previous workpiece coordinate system's coordinates (no machine motion). By inputting Reset, the inclined surface machining is also canceled. (If the parameter "#1151 rstint" is set to "0", however, the inclined surface machining mode is kept even when Reset 1 is input.) 719 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Program example Program example 1 The machining program #10 is for machining an identical shape on each face of the hexagonal column using a compound type machine. Feature coordinate systems on each face are defined in the blocks N1 to N6, and then same machining is performed using the subprogram (Machining program #100). The workpiece origin is deemed to be at the center of the hexagonal column's end-face. Machining program #10 N1 G68.2 X86.6025 Y50. Z0. I-90. J-45. K0.; M98 P100; G69; G00 Z200.; Machining on the face (1) N2 G68.2 X86.6025 Y-50. Z0. I-150. J-45. K0.; M98 P100; G69; G00 Z200.; Machining on the face (2) N3 G68.2 X0. Y-100. Z0. I-210. J-45. K0.; M98 P100; G69; G00 Z200.; Machining on the face (3) N4 G68.2 X-86.6025 Y-50. I-270. J-45. K0.; M98 P100; G69; G00 Z200.; Machining on the face (4) N5 G68.2 X-86.6025 Y50. I-330. J-45. K0; M98 P100; G69; G00 Z200.; Machining on the face (5) N6 G68.2 X0. Y100. I-30. J-45. K0.; M98 P100; G69; G00 Z200.; Machining on the face (6) M30 Machining program #100 G53.1; G90 G00 X0. Y0. Z5.; G01 Z-5. F500 ; G01 Y20. F1000; G02 X20. Y0. R20. F1000; G01 X0. F1000; M99 ; FY FY (1) FZ FX (6) 86.6025 50. (2) WX G WY (5) (3) (4) G: Feature coordinate system's origin IB-1501278-D 720 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Program example 2 The machining program #10 to #15 are for machining a shape on an inclined surface of the cube as shown in the figure next page. The feature coordinate system is defined by designating the inclined surface in each main program, and then same machining is done using the subprogram (Machining program #100). Machining program #10 Euler angles N1 G28XYZBC ; G54X0Y0Z0 ; M200 ; G68.2 X33.3333 Y 33.3333 Z66.6666 I-45 J54.7356 K0; M98 P100; G69; Machining program #11 Roll-pitch-yaw angles N2 G28XYZBC ; M200 ; G68.2 P1 Q321 X33.3333 Y 33.3333 Z66.6666 I45 J-35.2644 K-30; M98 P100; G69; M30 ; Machining program #12 Three points in a plane N3 G28XYZBC ; G54X0Y0Z ; M200 ; G68.2 P2 Q0 X0 Y-18.7503 Z0 R0; G68.2 P2 Q1 X50 Y50 Z100; G68.2 P2 Q2 X50 Y0 Z50; G68.2 P2 Q3 X50 Y50 Z100; M98 P100; G69; M30 ; Machining program #13 Two vectors N4 G28XYZBC ; G54X0Y0Z0 ; M200 ; G68.2 P3 Q1 X33.3333 Y 33.3333 Z66.6666 J-100 K0; G68.2 P3 Q2 I-100 J-100 K100; M98 P100; G69; M30 ; 721 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Machining program #14 Projection angles N5 G28XYZBC ; G54X0Y0Z0 ; M200 ; G68.2 P4 X33.3333 Y 33.3333 Z66.6666 I-45 J45 K-60; M98 P100; G69; M30 ; Machining program #15 Tool axis direction basis N6 G28XYZBC ; G54X0Y0Z0 ; M200 ; B-45. C45.; G68.3 X33.3333 Y33.3333 Z66.6667 R0.; M98 P100; M69 ; M30 ; Machining program #100 G53.1; G90G00X0.Y0.Z0.B0.C0.; G00X0Y0Z0; G01 Y50. F1000; G02 X50. Y0. R50. F1000; G01 X0. F1000; M99 ; WZ FY B C FZ FX 100 WX WY 100 A 100 FY FX B C G A (X0, Y0, Z0) = (33.3333, 33.3333, 66.6667) G: Feature coordinate system's origin IB-1501278-D 722 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.4.10 Rotary Axis Basic Position Selection Detailed description When inclined surface machining is commanded, the basic position for establishing the feature coordinate system's origin can be set with the parameter (#7915 Rotary axis basic position in inclined surface machining). There are two types of basic position selection. One is to set the feature coordinate system in view from the workpiece coordinate system independently of the rotary axis' position when inclined surface machining is commanded (Start position basis), and the other is to set the feature coordinate system in view from a workpiece coordinate system which is determined regardless of the rotary axis position when inclined surface machining is commanded (Zero degree position basis). Rotary axis basic position in inclined surface machining Start position basis (#7915=1) When workpiece is placed in the workpiece coordinate system direction: Workpiece coordinate offset A0. C0. ： ： G90 G54 A0. C0. G68.2XxYyZz Rotary axis basic position in inclined surface machining Zero degree position basis (#7915=0) G90 G54 A0. C0. G68.2XxYyZz WZ G53.1 WZ G53.1 WY FY ： WY FY ： FZ FZ FX FX WX C0° WX WZ C0° WY C0° WX When G68.2 is commanded: When G68.2 is commanded: Feature coordinate system is defined at Feature coordinate system is defined at a position in view from a workpiece co- a position in view from a workpiece coordinate system. ordinate system regardless of rotary axis position. C0° C0° FZ FZ WZ WZ FY FY WY WY FX FX WX WX When G53.1 is commanded: When G53.1 is commanded: The tool axis direction matches the Z axis direction of the feature coordinate system, which has been defined with G68.2. The tool axis direction matches the Z axis direction of the feature coordinate system, which has been defined with G68.2. 723 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Rotary axis basic position in inclined surface machining Start position basis (#7915=1) When workpiece is placed deviated from the workpiece coordinate system: Workpiece coordinate offset A0. C30. ： ： G90 G54 A0. C30. G68.2XxYyZz Rotary axis basic position in inclined surface machining Zero degree position basis (#7915=0) G90 G54 A0. C30. WZ G53.1 G68.2XxYyZz WZ WY G53.1 WY FY ： ： FZ FZ FY FX C0° WX C0° WX WZ FX WY 30° 30° C0° WX 30° When G68.2 is commanded: When G68.2 is commanded: Feature coordinate system is defined at Feature coordinate system is defined at a position in view from a workpiece co- a position in view from a workpiece coordinate system. ordinate system regardless of rotary axis position. FZ FZ C0° WZ FY WY FX WX WZ C0° FY WY FX WX When G53.1 is commanded: When G53.1 is commanded: The tool axis direction does not match the Z axis direction of the feature coordinate system, which has been defined with G68.2 command. The tool axis direction matches the Z axis direction of the feature coordinate system, which has been defined with G68.2. Example) Polygon machining: (Subprogram) (Main program) : Machining an identical shape : on each of the six surfaces. G68.2 Xx Yy Zz Ii Jj Kk G68.2 Xx Yy Zz Ii Jj Kk G53.1 G53.1 WZ G01 Xx Ff M98 Pp WY : G69 G69 : (4) (5) (3) M99 (Subprogram) (6) (2) WX Create a machining shape in the sub- G01 Xx Ff (1) program using inclined surface machin- : ing and tool axis direction control. Need M99 to consider the rotary axis' angle before Carry out inclined surface machining calling the subprogram. and tool axis direction control in the main program and create a machining shape in the subprogram. No need to consider the rotary axis' angle before calling the subprogram. IB-1501278-D 724 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Combination with tool center point (TCP) control When inclined surface machining control is commanded together with the TCP control (G43.4), define the table-interlocked feature coordinate system by setting the parameter (#7911 Rotary axis basic position selection) for TCP control. When zero degree position basis (#7911=0) is selected, it is possible to define the table-interlocked feature coordinate system at an arbitrary rotary axis angle. For the start position basis (#7911=1), the table-interlocked feature coordinate system can be defined on an inclined surface only when the TCP control is commanded at the same rotary axis angle as of the inclined surface machining command (G68.2) or tool axis direction control command (G53.1). When workpiece is placed in the workpiece coordinate system direction: Rotary axis basic position selection Workpiece coordinate system zero point for a basis (#7911 = 0) Inclined surface machining command Zero degree position basis (#7915 =0) Workpiece coordinate offset A 0. C0. Rotary axis basic position selection The position when the tool center point is commanded for a basis (#7911 = 1) ： G90 G54 A0. C0. G68.2XxYyZz WZ G53.1 WY FY G43.4 FZ ： FX C0° WZ WX WY C0° WX When G68.2 is commanded: Feature coordinate system is defined at a position in view from a workpiece coordinate system regardless of rotary axis position. C0° FZ WZ FY WY FX WX When G53.1 is commanded: The tool axis direction matches the Z axis direction of the feature coordinate system, which has been defined with G68.2. C0° C0° *FZ *FZ WZ WZ *FY *FY WY WY *FX *FX WX When G43.4 is commanded: WX When G43.4 is commanded: Feature coordinate system is fixed to Feature coordinate system is fixed to the table at 0 degree of the coordi- the table at a position in view from a nate system. workpiece coordinate system regardless of rotary axis position. 725 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control When workpiece is placed deviated from workpiece coordinate system (1) When TCP control (G43.4) is commanded at the same angle as of tool axis direction control (G53.1) Rotary axis basic position selection Workpiece coordinate system zero point for a basis (#7911 = 0) Inclined surface machining command Zero degree position basis (#7915 =0) Workpiece coordinate offset A 0. C30. Rotary axis basic position selection The position when the tool center point is commanded for a basis (#7911 = 1) ： G90 G54 A0. C0. WZ G68.2XxYyZz WY G53.1 FY G43.4 FZ ： FX WZ C-30° WX WY WX C0° 30° When G68.2 is commanded: Feature coordinate system is defined at a position in view from a workpiece coordinate system regardless of rotary axis position. C-30° FZ WZ FY WY FX WX When G53.1 is commanded: The tool axis direction matches the Z axis direction of the feature coordinate system, which has been defined with G68.2. C-30° C-30° *FZ WZ *FZ WZ *FY WY *FY WY *FX *FX WX WX When G43.4 is commanded: When G43.4 is commanded: Feature coordinate system is fixed to Feature coordinate system is fixed the table at a position in view from a to the table at the position of the workpiece coordinate system regard- present feature coordinate system. less of rotary axis angle. IB-1501278-D 726 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (2) When TCP control (G43.4) is commanded at a different angle from tool axis direction control (G53.1). Rotary axis basic position selection Workpiece coordinate system zero point for a basis (#7911 = 0) Inclined surface machining command Zero degree position basis (#7915 =0) Workpiece coordinate offset A 0. C30. Rotary axis is rotated before tool center point control command Rotary axis basic position selection The position when the tool center point is commanded for a basis (#7911 = 1) ： G90 G54 A0. C0. WZ G68.2XxYyZz G53.1 WY FY G00 A30. FZ G43.4 FX ： C-30° WX WZ WY When G68.2 is commanded: Feature coordinate system is defined at a position in view from a workpiece coordinate system regardless of rotary axis position. WX C0° C-30° 30° FZ WZ FY WY FX WX When G53.1 is commanded: The tool axis direction matches the Z axis direction of the feature coordinate system, which has been defined with G68.2. FZ FY WZ FX WY C-30° WX When G00 A30 is commanded: The tool axis direction does not match the Z axis direction of the feature coordinate system, which has been defined with G68.2 command. FZ WZ *FY FY *FZ WY *FX C-30° WZ FX WY C-30° WX WX When G43.4 is commanded: When G43.4 is commanded: Feature coordinate system is fixed to Feature coordinate system is fixed the table at a degree determined to the table at the position of the based on the rotary axis position. present feature coordinate system. 727 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Start position based inclined surface machining command (#7915=1) If the Z axis of the feature coordinate system defined on an inclined surface matches the tool axis direction, the tableinterlocked feature coordinate system can be defined by commanding the tool center point (TCP) control. However, if the TCP control start position basis is selected (#7911=1), the table-interlocked feature coordinate system can be defined on an inclined surface only when TCP control is commanded at the same angle as of the inclined surface machining command (G68.2) or tool axis direction control command (G53.1). IB-1501278-D 728 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.4.11 Relationship between Inclined Surface Machining and Other Functions Relationship with other functions Commands Available in Inclined Surface Machining Mode If commanded in any other mode, a program error (P951) will occur. Command G00, G01 G02, G03 G02.1, G03.1 Function Positioning, Linear Interpolation Circular interpolation, Helical interpolation Spiral interpolation G04 Dwell G05 P0, P1, P2, P10000 High-speed machining mode, high-speed high-accuracy control II G05.1 Q0, Q1 High-speed high-accuracy control I G08 P1 High-accuracy control G09 Exact stop check G10, G11 Parameter input by program / cancel, Compensation data input by program G12, G13 Circular cut G17, G18, G19 Plane selection G22/G23 Stroke check before travel ON / cancel G28 Automatic 1st reference position return G29 Start position return G30 2nd to 4th reference position return G30.1 to G30.6 Tool exchange position return G31 Skip (*1) G31.1 to G31.3 Multi-step skip (*1) G34, G35, G36, G37.1 Special Fixed Cycle G40, G41, G42 Tool radius compensation cancel/left/right G43, G44, G49 G43.1 G43.4, G43.5 Tool length compensation plus/minus/cancel Tool length compensation along the tool axis Tool center point control types I/II G45,G46,G47,G48 Tool position offset G50, G51 Scaling cancel/ON G50.1, G51.1 G command mirror image cancel/ON G53 Machine coordinate system selection G53.1 Tool Axis Direction Control G61 G61.1 G62 G64 Exact stop check mode High-accuracy control Automatic corner override Cutting mode G65 User macro simple call G66, G66.1, G67 User macro modal call A/B/cancel G69 Coordinate rotation cancel, Inclined surface machining cancel G70 to G76, G80 to G89 Fixed cycle for drilling (Including synchronous tapping) G90, G91 Absolute value command, Incremental value command G93 G94 G95 Inverse time feed Feed per minute Feed per revolution G98, G99 Fixed cycle initial level return, R point level return M98, M99 Subprogram call, main program return F Feedrate command M,S,T,B M, S, T, B command 729 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Command Macro command Function Local variable, Common variable, Arithmetic Commands (such as four basic arithmetic rule, trigonometric functions, square root) Control Commands (IF-GOTO- and WHILE-DO-) (*1) Only the three orthogonal axes designated by the rotary axis configuration parameter can be commanded. If two rotary axes are commanded, a program error (P951) will occur Modes where inclined surface machining (including cancel command) is available If inclined surface machining (G68.2 or G68.3) is commanded in a mode other than those listed below, a program error (P952) will occur. Mode Function G00, G01 Positioning, Linear Interpolation G05 P0, P1, P2 High-speed machining mode G05.1 Q0, Q1 High-speed high-accuracy control I G08 P1 High-accuracy control G13.1 Polar coordinate interpolation cancel G15 Polar coordinate command cancel G17, G18, G19 Plane selection G20, G21 Inch command, Metric command G22/G23 Stroke check before travel ON/cancel G40 Tool radius compensation cancel G40.1 Normal line control cancel G43, G44 G49 Tool length compensation Tool length compensation cancel G50 Scaling cancel G50.1 Mirror image by G code OFF G54 to G59, G54.1 Workpiece coordinate system selection, Extended workpiece coordinate system selection G54.4 Pp Workpiece installation error compensation G61 G61.1 G64 Exact stop check mode High-accuracy control Cutting mode G67 User macro modal call OFF G69 Coordinate rotation cancel, 3-dimensional coordinate conversion cancel G80 Fixed cycle cancel G90, G91 Absolute value command, Incremental value command G93 G94 G95 Inverse time feed Feed per minute Feed per revolution G97 Constant surface speed control OFF G98, G99 Fixed cycle initial level return, R point level return IB-1501278-D 730 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Modes where tool axis direction control (G53.1/G53.6) is available If tool axis direction control is commanded in a mode other than those listed below, a program error (P953) will occur. Mode Function G00, G01 Positioning, Linear Interpolation G05 P0, P1, P2 High-speed machining mode G05.1 Q0, Q1 High-speed high-accuracy control I G08 High-accuracy control G13.1 Polar coordinate interpolation cancel G15 Polar coordinate command cancel G17, G18, G19 Plane selection G20, G21 Inch command, Metric command G23 Stroke check before travel OFF G40 Tool radius compensation cancel G40.1 Normal line control cancel G43, G44 Tool length compensation G49 Tool length compensation cancel G50 Scaling cancel G50.1 Mirror image by G code OFF G54 to G59, G54.1 Workpiece coordinate system selection, Extended workpiece coordinate system selection G54.4 P Workpiece installation error compensation G61 Exact stop check mode G61.1/G08P1 High-accuracy control G64 Cutting mode G67 User macro modal call OFF G68.2 to G68.9 Inclined surface machining G80 Fixed cycle cancel G90, G91 Absolute value command, Incremental value command G93 Inverse time feed G94 Feed per minute G95 Feed per revolution G97 Constant surface speed control OFF G98, G99 Fixed cycle initial level return, R point level return 731 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Skip during inclined surface machining command A skip operation during the inclined surface machining command is the same as the normal skip operation. The axis moves on the feature coordinate system. Machining program N1 G68.2 Xx Yy Zz Ii Jj Zz ; N2 G53.1; N3 G90 G31 Z0. F100; Wz Wy Fy Fx Fz Wz The axis moves to the Z axis direction of the feature coordinate system in the N3 block. For the skip function, refer to each chapter in "21 Measurement Support Functions". Combination with arbitrary axis exchange If you use simple inclined surface machining in combination with an arbitrary axis exchange (G140) command, you need to set the rotary axis configuration parameters using the 2nd axis name. Set the parameter "#1450 5axis_Spec/bit0" to "1" (setting by the 2nd axis name), and assign the axis configuration for executing inclined surface machining to the rotary axis configuration parameter (#7900 or later) using the 2nd axis name (example: A1, B2). If the inclined surface machining is commanded after the arbitrary axis exchange has been completed while the parameter "#1450 5axis_Spec/bit0" is not designated, a program error (P952) will occur. You can set the configurations up to the number of valid part systems (up to four part systems) in the rotary axis configuration parameter. With multiple configurations set, you can perform inclined surface machining in different axis configurations. Inclined surface machining can be performed using the axis configuration in the part system with axis exchange completed by applying the rotary axis configuration parameter in the configuration in which all axes included in the part system are set. IB-1501278-D 732 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.4.12 Precautions for Inclined Surface Machining Precautions (1) A rotary axis moves at G53.1 command. Thus, move the tool far enough away from the table before commanding G53.1. (2) When inclined surface machining is commanded, the coordinates of the feature coordinate system are set in the system variables #5001 to #5100+n (excluding #5021 to #5021+n), which are used to read the position information. But, the coordinates of the machine coordinate system are set in the variables #5021 to #5021+n (machine coordinate values) even when inclined surface machining is commanded. n: varies depending on the number of control axes. (3) When Reset signal is input during inclined surface machining command, the inclined surface machining mode will be canceled, and the modal G code will be G69. (However, when the parameter "#1151 rsint" is set to "0", the inclined surface machining mode will be kept even if Reset 1 is input.) (4) When the external deceleration signal is input, the signal is not input to the axes of the feature coordinate system, but to the axes of the machine coordinate system that is actually operating. (5) If G28 or G30 is commanded after the inclined surface machining command has been issued, the control is carried out with respect to the inclined surface coordinate system up to the intermediate point, and then carried out with respect to the machine coordinate system from the intermediate point. (6) Tool radius compensation, mirror image by G code, fixed cycle command, tool center point control, scaling, and tool length compensation along the tool axis should be nested in the inclined surface machining command. Thus, these commands need to be commanded between the inclined surface machining command (G68.2, etc) and G69. G68.2 X_Y_Z_I_J_K_ G41 D1 : Inclined surface machining In tool radius compensation : G40 : G69 (7) If inclined surface machining (G68.2) is commanded while tool length compensation is active, the actual tool tip position does not match the current position. In such case, command G53.1 to align the tool axis direction with the Z axis of the feature coordinate system, which will make the tool tip position the same as the current position. Before commanding G68.2, the current position and actual tool tip are the same. Z X When feature coordinate system is defined in G68.2, a point obtained by compensating the tool length direction to be in the feature coordinate axis' Z direction is deemed as the current position. Thus, the current position doesn't match with the actual tool tip position. Z X Z The actual tool tip point becomes the same as the current position by commanding G53.1 to align the tool axis direction with the feature coordinate system's Z direction. X 733 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (8) Coordinate conversion is not carried out upon manual interruption, so travel, by a distance equivalent to the manual interruption amount, is carried out with respect to the machine coordinate system. When manual interruption with ABS ON, or tool center point control has been performed during inclined surface machining, return to the position before interruption, and then restart automatic operation. If you restart automatic operation in a different position from the one prior to the interruption, operation error (M01 0185) will occur. An interruption to a rotary axis during inclined surface machining will also cause an operation error (M01 0185). If automatic handle interruption is attempted during inclined surface machining, an operation error (M01 0185) will occur. (9) MDI interruption, PLC interruption and macro interruption are disabled during inclined surface machining. If MDI interruption or PLC interruption is attempted during inclined surface machining, an operation error (M01 0185) will occur. If macro interruption is enabled during inclined surface machining, a program error (P951) will occur. Also when inclined surface machining is commanded while macro interruption is active, a program error (P952) will occur. (10) When inclined surface machining is commanded during MDI interruption, PLC interruption, or macro interruption, a program error (P952) will occur. (11) When a circular command is graphically traced under the inclined surface machining command, circular tracing is performed if the feature coordinate system matches the machine coordinate system. If the systems are unmatched, a linear tracing is performed instead. (12) Tracing is carried out using the machine coordinate values. (13) When this function is used together with tool center point control or the workpiece installation error compensation function, inclined surface machining is subject to the restraints of each function. For details, refer to each chapter. (14) Program restart from the block after the inclined surface machining command is issued cannot be implemented. If commanded, a program error (P49) occurs. Program example N10 G00 X_Y_Z_; Restart from the block N10 or N11 is possible. N11 G00 X_Y_Z_B_C; : N20 G68.2 X_Y_Z_I_J_K; Restart from the block N20 or later is not possible. N21 G01 X_Y_Z_F_; Attempting to do so will cause an alarm. N22 G01 X_Y_Z_F_; N23 G69 N30 G90 G00 X_Y_; N31 G90 G00 Z_; (15) If you want to display the coordinates on the position screen during inclined surface machining, enter "23" in the parameters #8901 to #8906. Then, the corresponding counter is shown with respect to the feature coordinate system. In the inclined surface coordinate counter display, whether the machining position on the program command that does not include the tool length compensation/tool radius compensation can be selected depends on the MTB specifications (parameter "#1287 ext23/bit1, bit2 (inclined surface coordinate display)". When tool tip coordinate display is enabled, inclined surface coordinates' counter can be displayed on the window by selecting the inclined surface for the counter selections 1, 2 and 3. (16) The movement that occurs in response to the G00 command is always the interpolation type. (Non-interpolation type is not available.) (17) In the case of table rotation type machines, the tool axis direction is not changed in G68.3. Thus, a feature coordinate system is defined with respect to the Z axis of the coordinate system before the inclined surface machining command is issued. But, designation of feature coordinate system's origin, and the rotation R about Z axis are enabled. (18) When inclined surface machining is commanded during inclined surface machining, a program error (P951) will occur. (19) In the parameters #7900 to #7902, #7922, #7932, #7942, and #7952, designate the axes of the first part system. If you command inclined surface machining in a part system where any of the designated axes is not ready, a program error (P932) will occur. IB-1501278-D 734 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (20) The feature coordinate system is defined with respect to the coordinate system (workpiece coordinate system), which is independent of the table rotary axis' rotation angle, so it is dependent on the table rotary axis' angle before the inclined surface machining command is issued. (21) A linear axis command during inclined surface machining is carried out using the coordinates of the feature coordinate system. And a rotary axis command is done using the coordinates (machine values) of the workpiece coordinate system. (22) If the address R, I, J or K has exceeded the setting range, a program error (P35) will occur. (23) Buffer correction cannot be implemented during inclined surface machining command. (24) If the operation mode is switched to "reference position return" during inclined surface machining command, an operation error (M01 0185) will occur. (25) If a linear angle command, geometric command, or figure rotation command is issued during inclined surface machining command, a program error (P951) will occur. (26) If arbitrary axis exchange (G140) is issued during inclined surface machining modal, the program error (P951) will occur. (27) When the axis during inclined surface machining control is the target for axis exchange, the operation error (M01 1101) will occur. The alarm will be cancelled by reset. (28) The part system in which inclined surface machining is being carried out does not cancel mixed control regardless of the setting for the parameter "#1280 ext16/bit1" (Cancellation of mixed control by resetting) even if a reset operation that does not reset the modal ("#1151 rstint" = "0" and NC reset 1) is carried out. If an axis in a part system in which inclined surface machining is being carried out is specified as the axis to be exchanged in the part system, the axis exchange will not be possible and an operation error (M01 1101) will occur regardless of whether the automatic operation mode has been established. (29) When the number of simultaneous contouring control axes is four or less and the indexing is performed with the indexing type 2 of R-navi on the selected machining surface, the block stop due to the completion of each axis travel will not be performed regardless of whether the parameter "#G53.6 block stop" has been set. (30) The axis configuration of applicable machines is as follows. The function is effective for the machine configuration with the right-hand orthogonal coordinate system defined in ISO standard. (a) This function applies to three types of machine configuration as below. Type Description Example of machines Tool tilt type Two rotary axes on tool head side Table tilt type Compound type Two rotary axes on table side One rotary axis each on tool head side and table side (B) (B) (A) (A) (A) (B) Primary rotary Tool-side 2nd rotary axis axis (A) (B) Tool-side 1st rotary axis Table-side 2nd rotary axis Tool-side rotary axis Table-side 1st rotary axis Table-side rotary axis In this manual, the following axes are called as primary rotary axis: the tool-side 2nd rotary axis (tool tilt type), the table-side 1st rotary axis (table tilt type), and the tool side rotary axis (compound type). 735 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (b) This function is not applicable to machines as below. Description Example of machines A machine whose rotary axis’s rotation center axis is not parallel to any orthogonal coordinate axis. A machine whose direction from the tool tip to the tool base is not parallel to Z axis (Z axis positive direction) when machine positions of the rotary axes are all 0°. 0° Tool axis direction A machine in which three linear axes do not form a right-handed orthogonal coordinate system. (31) If any of the orthogonal axes of all the active part systems is under machine lock during inclined surface machining, normal synchronous tapping is applied even though the high-speed tapping specification is provided. IB-1501278-D 736 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control 18.5 3-dimensional Tool Radius Compensation (Tool's vertical-direction compensation) ; G40/G41.2,G42.2 Function and purpose This function realizes the tool radius compensation for the machine with 2 rotary axes by calculating the change in the direction of a workpiece and the inclination of the tool caused by the move of the rotary axes. Tool radius compensation is carried out three-dimensionally by calculating the tool path on the surface of a workpiece from the program command and obtaining the compensation vector on a plane (compensation plane) perpendicular to the tool direction (offset plane). (b) (a) r r : Compensation amount : Tool center path r Z : Program path Y (a) Tool direction (b) Offset plane X If the specification is not provided, when 3-dimensional tool radius compensation (tool's vertical-direction compensation) is commanded, a program error (P161) will occur. Command format 3-dimensional tool radius compensation (Tool's vertical-direction compensation) left G41.2 (X_ Y_ Z_ A_ B_ C_) D_; 3-dimensional tool radius compensation (Tool's vertical-direction compensation) right G42.2 (X_ Y_ Z_ A_ B_ C_) D_; 3-dimensional tool radius compensation (Tool's vertical-direction compensation) cancel G40 (X_ Y_ Z_ A_ B_ C_); or D0; X,Y,Z Orthogonal coordinate axis movement command (can be omitted) A,B,C Rotary axis movement command (can be omitted) D Compensation No. "D0;" refers to a D command of compensation number "0". Note (1) All the G codes in the above command format belong to the modal group 7. 737 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Detailed description This function calculates the change in the direction of a workpiece and the inclination of the tool caused by the move of the rotary axes, and converts the programmed tool path onto the offset plane (perpendicular to the tool direction at the compensation point) to conduct the tool radius compensation for 5-axis machining. (Refer to "How to calculate the compensation vector" for the details of offset plane.) The operations at the start/cancel and in compensation mode on the offset plane conform to the normal tool radius compensation. Refer to Chapter "12.3 Tool Radius Compensation ; G38,G39/G40/G41,G42" for the operations which are not explained in this section. Tool radius compensation start (startup) The type of compensation start can be selected from type A and type B by the parameter "#8157 Radius comp type B", like the conventional tool radius compensation. Refer to "12.3 Tool Radius Compensation ; G38,G39/G40/ G41,G42" for the descriptions of type A/type B. The startup must be carried out in the G code modal listed in "Modes in which G41.2/G42.2 command is issued" in "Relation with other functions". If commanded in an unlisted modal, a program error (P163) will occur. Tool radius compensation operation For usable functions during the compensation, refer to "Commands which can be issued while G41.2/G42.2 is executed" in "Relation with other functions". If an unavailable function is commanded, a program error (P162) will occur. Interference check is not available for this function. Tool radius compensation cancel When any of the following condition is met, the tool radius compensation for 5-axis machining will be canceled. (1) After the compensation cancel command (G40) is executed (2) A command of offset number D00 is issued (3) NC reset 1 (*1) (4) NC reset 2 or Reset &Rewind is commanded The type of compensation cancel can be selected from type A and type B by the parameter "#8157 Radius comp type B", as well as the startup. (*1) The compensation is canceled when "#1151 rstint" is ON. IB-1501278-D 738 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control How to calculate the compensation vector The compensation vectors for tool radius compensation are obtained as shown below. (1) Table coordinate system Convert the program command into the path on the surface of the table coordinate system. Table coordinate system rotates with the workpiece (the figure below) as the table rotates. The command path on this coordinate system is the relative command path of the tool against the workpiece. <Default state> <When the table rotates> Z Z Y Y X XX (2) Conversion into the points on the offset plane Reflect the obtained path on the table coordinate system onto the offset plane (vertical to the tool axis direction at the compensation point) and calculate the points (A' and C' in the figure below) on the offset plane. (b) Z Y X A’ C (a) BB C’ (a) Tool direction at point A (b) Tool direction at point B A A Offset plane at point A Offset plane at point B Path on the table coordinate system 739 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (3) Compensation on the offset plane Perform the conventional tool radius compensation on the offset plane and calculate the compensation vector on the offset plane. Z Y A’ X C B C’ A Path on the table coordinate system on the offset plane Compensation vector on the offset plane IB-1501278-D 740 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control When a block is inserted When a block is inserted while cutting a corner, the direction of the tool at the single block stop is equal to that of the previous block. (Like a feedrate and other modal data, the rotation angle of the previous block is kept.) (b) A Z Y A’ X C’ B B (b) Tool direction at point B C Path on the table coordinate system Offset plane at point B If the program moves from A, B to C as shown in the figure above, the offset plane at point B is as the figure below. The block between the points B2 and B3 is inserted, the tool direction between B2-B3 is same as at point B2 and the tool moves on the offset plane which is created at point B. A’ C’ B B1 B4 (S) B3 B2 Path on the table coordinate system on the offset plane (S) Single block stop point 741 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Program example N1 G28 Z N2 G28 BC N3 G28 XY N4 G90 G54 G00 X-60. Y0. N5 G00 B30. N6 G43.4 H1 Z-50. N7 G42.2 G01 X-50. D1 N8 G01 X-49.990 Y-1.000 C 1.15 N9 G01 X-49.960 Y-1.999 C 2.29 N10 G01 X-49.910 Y-2.998 C 3.44 : : N200 G01 X50. Y0. C180. N201 G01 Z0. N202 G40 N203 G49 N204 G28 Z N205 G28 BC N206 G28 X M30 (D1 =5.0, H1=50.0) Z Y G54 Compensation amount -50.0 50.0 -50.0 X Programmed path Tool center path IB-1501278-D 742 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Relationship with other functions Commands which can be issued in a same block as G41.2/G42.2 Function G00 Positioning G01 Linear interpolation G90 Absolute value command G91 Incremental value command F Feedrate command N Sequence No. If unlisted commands are issued in a same block with 3-dimensional tool radius compensation (tool's vertical-direction compensation) (G41.2/G42.2), a program error (P163) will occur. Commands which can be issued while G41.2/G42.2 is executed Function G00 Positioning G01 Linear interpolation G04 Dwell G05 P0, G05 P1, G05 P2 High-speed machining mode G05 P0, G05 P10000 High-speed high-accuracy control II G08 P0, G08 P1 High-accuracy control G09 Exact stop G20, G21 Inch/metric command (*1) G22, G23 Stroke check before travel ON/OFF G40 Tool radius compensation cancel G41.2, G42.2 3-dimensional tool radius compensation (tool's vertical-direction compensation) right/left G61 Exact stop check mode G61.1 High-accuracy control ON G64 Cutting mode G65 User macro simple call G66 User macro modal call A G66.1 User macro modal call B G67 User macro modal call cancel G90, G91 Absolute value command, Incremental value command G93 Inverse time feed G94 Feed per minute G95 Feed per revolution G96, G97 Constant surface speed control ON/OFF M98, M99 Subprogram call, main program return F Feedrate command M, S, T, B M, S, T, B command Macro command Local variables and common variables Operation commands (four basic arithmetic rule, trigonometric functions, square root) Control commands (IF - GOTO -, WHILE - DO -) N Sequence No. (*1) If the inch/metric command switches during 3-dimensional tool radius compensation (tool's vertical-direction compensation), a program error (P162) will occur. 743 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Modes in which G41.2/G42.2 command can be issued Function G00, G01 Positioning, Linear Interpolation G17, G18, G19 Plane selection G20, G21 Inch/Metric command G22, G23 Stroke check before travel ON/OFF G40 Tool radius compensation cancel G40.1, G150 Normal line control cancel G41.2, G42.2 3-dimensional tool radius compensation (tool's vertical-direction compensation) left/right G43, G44 Tool length compensation (+/-) G43.1 Tool length compensation along the tool axis G43.4, G43.5 Tool center point control type I/II G49 Tool length compensation cancel G50 Scaling cancel G50.1 G command mirror image cancel G54, G55, G56, G57, G58, G59, G54.1 Workpiece coordinate system selection, extended workpiece coordinate system selection G54.4Pn Workpiece installation error compensation G61 Exact stop check mode G61.1 High-accuracy control ON G64 Cutting mode G67 User macro modal call cancel G68.2 Inclined surface machining G68.3 Inclined surface machining command (Define using tool axis direction) G69 3-dimensional coordinate conversion cancel G80 Fixed cycle cancel G90, G91 Absolute value command, Incremental value command G93 Inverse time feed G94 Feed per minute G95 Feed per revolution G96, G97 Constant surface speed control ON/OFF G98, G99 Fixed cycle initial level return, R point level return G15, G13.1, G113 Polar coordinate command cancel Combination with arbitrary axis exchange control When performing 3-dimensional tool radius compensation (tool's vertical-direction compensation) in combination with an arbitrary axis exchange (G140) command, you need to set the rotary axis configuration parameters using the 2nd axis name. Set the parameter "#1450 5axis_Spec/bit0" to "1" (setting by the 2nd axis name), and assign the axis configuration for executing 3-dimensional tool radius compensation (tool's vertical-direction compensation) to the rotary axis configuration parameter (#7900 or later) using the 2nd axis name (example: A1, B2). If the G41.2/G42.2 command is issued after the arbitrary tool exchange has been completed while the parameter "#1450 5axis_Spec/bit0" is not designated, a program error (P163) will occur. You can set up to four valid part systems in the rotary axis configuration parameter. With multiple configurations set, you can perform 3-dimensional tool radius compensation (tool's vertical-direction compensation) in different axis configurations. 3-dimensional tool radius compensation (tool's vertical-direction compensation) can be performed using the axis configuration in the part system with axis exchange completed by applying the rotary axis configuration parameter in the configuration in which all axes included in the part system are set. IB-1501278-D 744 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control Precautions (1) Interference check is not available for 3-dimensional tool radius compensation (tool's vertical-direction compensation). The parameter "#8103 COLL. CHK OFF" to turn ON/OFF the interference check, available for conventional tool radius compensation, is invalid in 3-dimensional tool radius compensation (tool's vertical-direction compensation). (2) Tool radius compensation vector designation (G38) and Tool radius compensation corner arc (G39) are not available. If commanded, a program error (P162) will occur. (3) Corner Chamfering/Corner Rounding, Linear Angle Command and Geometric Command are not available. If commanded, a program error (P162) will occur. (4) Manual interruption, automatic operation handle interruption, manual / automatic simultaneous, manual speed command, manual reference position return, tool handle feed & interruption, and manual arbitrary feed mode will cause an operation error (M01 0232) when the manual mode is ON. (5) Macro interruption cannot be used. If 3-dimensional tool radius compensation (tool's vertical-direction compensation) is commanded when macro interruption is valid, a program error (P163) will occur. If macro interruption valid (M96) is commanded in 3-dimensional tool radius compensation (tool's vertical-direction compensation), a program error (P162) will occur. (6) Tool escape and return is not available. Turning ON the tool escape and return transit point designation signal and the manual mode will cause an operation error (M01 0232). (7) Switching from a mode to MDI mode or from MDI mode to another mode in 3-dimensional tool radius compensation (tool's vertical-direction compensation) will cause an operation error (M01 0232). (8) Turning ON on the PLC interruption signal in 3-dimensional tool radius compensation (tool's vertical-direction compensation) will cause an operation error (M01 0232). (9) Mirror image by the external input is not available for the target axis (*1) of 5-axis machining. If mirror image by the external input is set to ON in the 3-dimensional tool radius compensation (tool's vertical-direction compensation), a program error (P162) will occur. Also, if the 3-dimensional tool radius compensation (tool's verticaldirection compensation) is commanded during mirror image by the external input, a program error (P163) will occur. (*1) Axes here are the axes designated with the parameters "#7900 RCDAX_I", "#7901 RCDAX_J", "#7902 RCDAX_K", "#7922 ROTAXT1", "#7932 ROTAXT2", "#7942 ROTAXW1", and "#7952 ROTAXW2". These settings depend on the MTB specifications. (10) If 3-dimensional tool radius compensation (tool's vertical-direction compensation) is commanded in the reverse run control mode, or if the reverse run control mode signal is set to ON in 3-dimensional tool radius compensation (tool's vertical-direction compensation), a program error (P163) will occur. (11) This function can be combined with the tool center point control (G43.4,G43.5/G49). However, the ON/OFF of the 3-dimensional tool radius compensation (tool's vertical-direction compensation) must be nested in the ON/ OFF of the tool center point control and it must be commanded in the tool center point control. If the tool center point control is commanded in 3-dimensional tool radius compensation (tool's vertical-direction compensation), a program error (P162) will occur. This function can also be combined with tool length compensation along the tool axis (G43.1/G49) in the same conditions as the above. During tool center point control G43.4 H1 ･･･ G41.2 D1 ･･･ ･･･ ･･･ ･･･ G49 3-dimensional tool radius compensation (Tool's vertical-direction compensation) G40 (12) When used with the tool center point control, the compensation is applied to the tool center point path. (13) The restart search from the block in 3-dimensional tool radius compensation (tool's vertical-direction compensation) is possible while the restart search from the block concurrently using the tool center point control is impossible. (14) Fairing in high-speed machining mode/high-speed high-accuracy control is not available. The parameter "#8033 Fairing ON" to turn ON/OFF the fairing function in high-speed machining mode/high-speed high-accuracy control is invalid in 3-dimensional tool radius compensation (tool's vertical-direction compensation). 745 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (15) As shown in the figure below, we recommend that the tool approach to the surface of the workpiece at an angle. The tool radius compensation amount may not be correctly reflected on the cutting when the direction of the approach is opposite to the cutting direction. So the tool must shift to the surface of the workpiece at the start of the cutting at an angle to the tool axis direction. ×: Tool radius compensation amount may not be correctly reflected because there is no movement on the offset plane and the tool radius compensation amount is not re-calculated. ○: Tool radius compensation amount is correctly reflected. Offset plane (perpendicular to the tool axis direction) Movement on the offset plane. (16) The buffer correction is not available in 3-dimensional tool radius compensation (tool's vertical-direction compensation). Pressing the menu [Prg correct] will display an error message. (17) Also, if 3-dimensional tool radius compensation (tool's vertical-direction compensation) is commanded during mirror image by parameter setting or coordinate rotation by parameter, a program error (P163) will occur. If the parameter is turned on in 3-dimensional tool radius compensation (tool's vertical-direction compensation), a program error (P162) will occur at the next start. IB-1501278-D 746 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control (18) The axis configuration of applicable machines is as follows: The function is effective for the machine configuration with the right-hand orthogonal coordinate system defined in ISO standard. (a) This function applies to three types of machine configurations as below: Type Tool tilt type Description Two rotary axes on tool head side Example of machines Table tilt type Compound type Two rotary axes on table side One rotary axis each on tool head side and table side (B) (A) (B) (A) (A) (B) Primary rota- Tool-side 2nd rotary axis ry axis (A) (B) Tool-side 1st rotary axis Table-side 2nd rotary axis Tool-side rotary axis Table-side 1st rotary axis Table-side rotary axis In this manual, the following axes are called as primary rotary axis: the tool-side 2nd rotary axis (tool tilt type), the table-side 1st rotary axis (table tilt type), and the tool side rotary axis (compound type). (b) This function is not applicable to machines as below: Description Example of machines A machine whose rotary axis's rotation center axis is not parallel to any orthogonal coordinate axis. A machine whose direction from the tool tip to the tool base is not parallel to Z axis (Z axis positive direction) when machine positions of the rotary axes are all 0°. 0° Tool axis direction A machine in which three linear axes do not form a righthanded orthogonal coordinate system. <Note> This cannot be applied to a machine on which the rotary axis's rotation center axis is not parallel to any orthogonal coordinate axis. This cannot be applied to a machine of which the direction from the tool tip to the tool base is not parallel to Z axis (Z axis positive direction) when machine positions of the rotary axes are all 0°. 747 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 18 Advanced Machining Control IB-1501278-D 748 19 Coordinate System Setting Functions 749 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19Coordinate System Setting Functions 19.1 Coordinate Words and Control Axes Function and purpose The number of control axes is set to "3" in the standard specifications; however, up to eight axes can be controlled if an additional axis is added. To specify each machining direction, use alphabetical coordinate words that are predefined appropriately. X-Y table +Z +Z +Y +X Program coordinates Workpiece Table +X +Y Direction of table movement Bed X-Y and rotating table +Z Workpiece +X Direction of table +Y movement IB-1501278-D +Y +C +X Program coordinates +C Direction of table revolution 750 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.2 Types of Coordinate Systems 19.2.1 Basic Machine, Workpiece and Local Coordinate Systems Function and purpose The basic machine coordinate system is fixed in the machine and it denotes that position which is determined inherently by the machine. The workpiece coordinate systems are used for programming and in these systems the basic point on the workpiece is set as the coordinate zero point. The local coordinate systems are created on the workpiece coordinate systems and they are designed to facilitate the programs for parts machining. Upon completion of the reference position return, the basic machine coordinate system and workpiece coordinate systems (G54 to G59) are automatically set with reference to the parameters. The basic machine coordinate system is set so that the first reference position is brought to the position specified by the parameter from the basic machine coordinate zero point (machine zero point). X1 M Y1 R#1 Y X W3 W4 L W1 W2 X1 M Z1 W1 W2 R#1 Z X M: Basic machine coordinate system W: Workpiece coordinate system L: Local coordinate system The local coordinate systems (G52) are valid on the coordinate systems designated by workpiece coordinate systems 1 to 6. The hypothetical machine coordinate system can be set on the basic machine coordinate system using a G92 command. At this time, the workpiece coordinate system 1 to 6 is also simultaneously shifted. Also refer to "Coordinate Systems and Coordinate Zero Point symbols". 751 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.2.2 Machine Zero Point and 2nd, 3rd, 4th Reference Position (Zero Point) Function and purpose The machine zero point serves as the reference for the basic machine coordinate system. It is inherent to the machine and is determined by the reference (zero) position return. 2nd, 3rd and 4th reference positions relate to the position of the coordinates that have been set beforehand by parameter from the zero point of the basic machine coordinate system. (M) (R2) x y (R1) (X2,Y 2) y (R3) (X1,Y 1) x (R4) y G52 (W) x (M) Basic machine coordinate system (G52) Local coordinate system (W) Workpiece coordinate systems (G54 to G59) (R1) 1st reference position (R2) 2nd reference position (R3) 3rd reference position (R4) 4th reference position IB-1501278-D 752 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.2.3 Automatic Coordinate System Setting Function and purpose This function creates each coordinate system according to the parameter values input beforehand from the setting and display unit when the first manual reference position return or the reference position is reached with the dogtype reference position return when the NC power is turned ON. The actual machining program is programmed over the coordinate systems that have been set above. (M) x1 y3 y2 y1 (R1) (G56) (G55) (G54) x2 x3 y4 (G59) (G58) (G57) x4 (M) Basic machine coordinate system (R1) 1st reference position (G54) Workpiece coordinate system 1 (G55) Workpiece coordinate system 2 (G56) Workpiece coordinate system 3 (G57) Workpiece coordinate system 4 (G58) Workpiece coordinate system 5 (G59) Workpiece coordinate system 6 Detailed description (1) The coordinate systems created by this function are as follow: - Basic machine coordinate system - Workpiece coordinate systems (G54 to G59) (2) The parameters related to the coordinate system all provide the distance from the zero point of the basic machine coordinate system. Therefore, after deciding at which position the first reference position should be set in the basic machine coordinate system and then set the zero point positions of the workpiece coordinate systems. (3) When the automatic coordinate system setting function is executed, shifting of the workpiece coordinate system with G92, setting of the local coordinate system with G52, shifting of the workpiece coordinate system with origin set, and shifting of the workpiece coordinate system with manual interrupt will be canceled. (4) The dog-type reference position return will be executed when the first time manual reference position return or the first time automatic reference position return is executed after the power has been turned ON. It will be also executed when the dog-type is selected by the parameter for the manual reference position return or the automatic reference position return for the second time onwards. CAUTION If the workpiece coordinate offset amount is changed during automatic operation (including during single block operation), it will be validated from the next block or after multiple blocks of the command. 753 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.2.4 Coordinate System for Rotary Axis Function and purpose The axis designated as the rotary axis with the parameters is controlled with the rotary axis' coordinate system. The rotary axis includes the rotating type (short-cut valid/invalid) and linear type (workpiece coordinate position linear type and all coordinate position linear type). The workpiece coordinate position range is 0 to 359.999° for the rotating type, and 0 to ± 99999.999° for the linear type. The machine coordinate value and relative position differ according to the parameters. The rotary axis is commanded with a degree (°) unit regardless of the inch or metric designation. The rotary axis type can be set with the parameter "#8213 rotation axis type" for each axis. Rotary axis Rotating type rotary axis #8213 setting value Short-cut invalid Short-cut valid 0 1 Linear type rotary axis Workpiece coordi- All-coordinate posinate position linear tion linear type type 2 Workpiece coordi- Displayed in the range of 0° to 359.999°. nate position Machine coordinate Displayed in the range of 0° to 359.999°. position/relative position Linear axis 3 - Displayed in the range of 0° to ± 99999.999°. Displayed in the range of 0° to ± 99999.999°. ABS command The incremental Moves with a shortamount from the end cut to the end point. point to the current position is divided by 360 degrees, and the axis moves by the remainder amount according to the sign. INC command Moves in the direction of the commanded sign by the commanded incremental amount starting at the current position. In the same manner as the normal linear axis, it moves according to the sign by the amount obtained by subtracting the current position from the end point (without rounding up to 360 degrees). Reference position Depends on the absolute command or the incremental command during the movement to the interreturn mediate point. Returns with movement within 360 degrees. IB-1501278-D 754 Moves and returns in the R point direction for the difference from the current position to the R point. M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Operation example Examples of differences in the operation and counter displays according to the type of rotation coordinate are given below. (The workpiece offset is set as 0°.) Rotary type (short-cut invalid) (1) The machine coordinate position, workpiece coordinate position and relative position are displayed in the range of 0° to 359.999°. (2) For the absolute position command, the axis moves according to the sign by the remainder amount obtained by dividing by 360°. Program 90 Workpiece Machine G28 C0. 45 N3 N1 G90 C-270. 90.000 N2 C405. 45.000 45.000 225.000 225.000 N3 G91 C180. N1 90.000 0 N2 Rotary type (short-cut valid) (1) The machine coordinate position, workpiece coordinate position and relative position are displayed in the range of 0° to 359.999°. (2) For the absolute position command, the axis rotates to the direction having less amount of movement to the end point. Program 90 N1 G90 C-270. 45 N3 Workpiece Machine G28 C0. N2 C405. N2 N3 G91 C180. 90.000 90.000 45.000 45.000 225.000 225.000 N1 0 755 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Linear type (workpiece coordinate position linear type) (1) The coordinate position counter other than the workpiece coordinate position is displayed in the range of 0° to 359.999°. The workpiece coordinate position is displayed in the range of 0 to ±99999.999°. (2) The movement is the same as the linear axis. (3) During reference position return, the axis moves in the same manner as the linear axis until the intermediate point is reached. The axis returns with a rotation within 360° from the intermediate point to the reference position. (4) During absolute position detection, even if the workpiece coordinate position is not within the range of 0 to 359.999°, the system will start up in the range of 0 to 359.999° when the power is turned ON again. Program Workpiece Machine 90 Relative position G28 C0. 45 N1 G90 C-270. N3 N2 C405. N3 G91 C180. -270.000 90.000 90.000 405.000 45.000 45.000 585.000 225.000 225.000 After the power is turned ON again 0 N1 Workpiece 225.000 N2 Machine 225.000 Linear type (all coordinate position linear type) (1) The workpiece coordinate position counter is displayed in the range of 0 to ±99999.999°. (2) The movement is the same as the linear axis. (3) During reference position return, the axis moves in the same manner as the linear axis until the intermediate point is reached. The axis rotates by the difference from the intermediate point to the reference position and returns to the reference position. (4) During absolute position detection, the system starts up at the position where the power was turned OFF when the power is turned ON again. Program Workpiece Machine 90 G28 C0. 45 N1 G90 C-270. N3 N2 C405. N3 G91 C180. -270.000 -270.000 -270.000 405.000 405.000 405.000 585.000 585.000 585.000 After the power is turned ON again 0 N1 Workpiece 585.000 N2 IB-1501278-D Relative position 756 Machine 585.000 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.3 Basic Machine Coordinate System Selection ; G53 Function and purpose The basic machine coordinate system is the coordinate system that expresses the position (tool change position, stroke end position, etc.) that is characteristic to the machine. The tool is moved to the position commanded on the basic machine coordinate system with the G53 command and the coordinate command that follows. Command format (G90)G53 X__ Y__ Z__ α__ ; α Additional axis Detailed description (1) When the power is switched on, the basic machine coordinate system is automatically set as referenced to the reference (zero) position return position, which is determined by the automatic or manual reference (zero) position return. (2) The basic machine coordinate system is not changed by the G92 command. (3) The G53 command is valid only in the designated block. (4) In the incremental value command mode (G91), the G53 command provides movement with the incremental value in the coordinate system being selected. (5) Even if G53 is commanded, the tool radius compensation amount for the commanded axis will not be canceled. (6) The 1st reference coordinate position indicates the distance from the basic machine coordinate system zero point to the reference position (zero point) return position. (7) The G53 command will move with cutting feedrate or rapid traverse following command modal. (8) If the G53 command and G28 command (reference position return) are issued in the same block, the command issued last will be valid. (500,500) -X (M) R1 (M) Basic machine coordinate system (R1) 1st reference position -Y 1st reference position coordinate value: X=+500 and Y=+500 (9) If the G53 command and G28 command (reference position return) are issued in the same block, the command issued last will be valid. (10) Even if G53 is commanded, the tool radius compensation amount for the commanded axis will not be canceled. 757 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (11) Depending on the MTB specifications, all movement commands in the G53 command block may run in rapid traverse mode (parameter "#1253 set/bit5"). (a) When the movement method of the G53 command block follows the command modal [Example in which the G53 block is executed during G01 modal) Program G group 01 modal Cutting or Rapid traverse N01 G01 X100. Z100. F1000; G01 Cutting N02 G53 X200. Z200.; G01 Cutting N03 X300. Z300.; G01 Cutting [Example in which the G53 block is executed during G00 modal] Program G group 01 modal Cutting or Rapid traverse N01 G00 X100. Z100.; G00 Rapid traverse N02 G53 X200. Z200.; G00 Rapid traverse N03 X300. Z300.; G00 Rapid traverse (b) When all the movement methods of the G53 command block are set to rapid traverse [Example in which the G53 block is executed during G01 modal) Program G group 01 modal Cutting or Rapid traverse N01 G01 X100. Z100. F1000; G01 Cutting N02 G53 X200. Z200.; G01 Rapid traverse N03 X300. Z300.; G01 Cutting The G group 01 modal does not change in the G53 command block; only the operation is set to rapid traverse. Relationship with Other Functions (1) Tool Compensation Functions When the G53 command is issued, the tool compensation amount of the axis with the movement command designated is canceled temporarily. (2) Machine coordinate system selection, Feedrate designation If an ",F" command is specified when there are no specifications for the feedrate command for G53, a program error (P39) will occur. (3) Inclined surface machining When the G53 command is issued during inclined surface machining, a program error (P951) occurs. (4) Polar coordinate interpolation Do not issue the G53 command during the polar coordinate interpolation mode. (5) Polar coordinate command The axis command with the G53 command is not interpreted as the polar coordinate command during the polar coordinate command mode. (6) Tool length compensation along the tool axis When the G53 command is designated while the compensation status is still established, the compensation is temporarily canceled, and the tool moves to the machine position designated by G53. (7) G command mirror image The mirror image will not be applied to the G53 command. (8) High-speed High-accuracy Control A program error will occur if the G53 command is issued during the high-speed high-accuracy control II mode. (9) 3-dimensional coordinate conversion Coordinate conversion will not be carried out for the machine coordinate system even if G53 command is issued in the 3-dimensional coordinate conversion modal. (10) Tool center point control A program error (P942) will occur if the G53 command is issued during the tool center point modal. (11) Workpiece installation error compensation A program error (P545) will occur if the G53 command is issued during workpiece installation error compensation. IB-1501278-D 758 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Precautions (1) In the machine with the specifications in which all the movement commands of the G53 command block run in rapid traverse mode, if the G53 and G01 commands are issued in the same block, the block is set to rapid traverse. However, the G group 01 modal is switched; therefore, the movement commands in the next and subsequent blocks run in cutting feed mode. [Example in which the G53 and G01 commands are issued in the same block] Program N01 G00 X100. Z100.; G group 01 modal Cutting or Rapid traverse G00 Rapid traverse N02 G53 G01 X200. Z200. F1000; G01 Rapid traverse N03 X300. Z300.; Cutting G01 759 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.4 Coordinate System Setting ; G92 Function and purpose By commanding G92, the absolute value coordinate system and current position display value can be newly preset according to the command value without moving the machine. Command format G92 X__ Y__ Z__ α__ ; α Additional axis Detailed description After the power is turned on, the first reference position return will be done with dog-type, and when completed, the coordinate system will be set automatically. (Automatic coordinate system setting) Reference position return completed R (b) R,M (a) (a) The basic machine coordinate system and workpiece coordinate system are created at the preset position. (a) Power ON position (b) Basic machine coordinate system (c) Workpiece coordinate system 100. (c) WG54 100. 200. [Relative position] X 0.000 Y 0.000 [Workpiece] X 300.000 Y 200.000 By commanding G92, the absolute value (workpiece) coordinate system and current position display value can be preset in the command value without moving the machine. Coordinate system setting R,M 200. For example, if G92 X0 Y0; is commanded, the workpiece coordinate system will be newly created. 100. (d) 50. WG54 100. [Relative position] X -200.000 Y -150.000 IB-1501278-D 200. 100. -100. (d) WG54' 100. - 50. 200. WG54 300. [Workpiece] X 100.000 Y 50.000 R,M (d) Tool position 760 [Relative position] X 0.000 Y 0.000 [Workpiece] X 0.000 Y 0.000 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Note (1) If the workpiece coordinate system deviated because the axis is moved manually when the manual absolute position switch is OFF, etc., the workpiece coordinate system can be corrected with the following steps. Execute reference position return while the coordinate system is deviated. After that, command G92G53X0Y0Z0;. With this command, the workpiece coordinate position and current position will be displayed, and the workpiece coordinate system will be preset to the offset value. Precautions (1) If the parameter "#1279 ext15/bit5" is set to "1", the coordinate systems setting (G92) shift amount is cleared when the axis reaches to the manual reference position. 761 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.5 Local Coordinate System Setting ; G52 Function and purpose The local coordinate systems can be set on the G54 through G59 workpiece coordinate systems using the G52 command so that the commanded position serves as the programmed zero point. The G52 command can also be used instead of the G92 command to change the deviation between the zero point in the machining program and the machining workpiece zero point. Command format G54(G54 to G59) G52 X__ Y__ Z__ α__ ; α Additional axis Detailed description (1) The G52 command is valid until a new G52 command is issued, and the tool does not move. This command, G52, comes in handy for employing another coordinate system without changing the zero point positions of the workpiece coordinate systems (G54 to G59). (2) The local coordinate system offset will be cleared by the dog-type manual reference (zero) point return or reference (zero) point return performed after the power has been switched ON. (3) The local coordinate system is canceled by (G54 to G59) G52 X0 Y0 Z0 α0;. (4) Coordinate commands in the absolute value (G90) cause the tool to move to the local coordinate system position. (G91) G52 X_Y_; Incremental value Ln Absolute value Local coordinate system Absolute value Ln Ln Reference position R M (G90) G52 X_Y_; Workpiece Wn(n=1 6) coordinate system Workpiece coordinate system offset (Screen setting, G10 L2 P__X__ Y__ ; ) External workpiece coordinate system offset (Screen setting, G10 P0 X__ Z__ ; ) Machine coordinate system <Note> If the program is executed repeatedly, the workpiece coordinate system will deviate each time. Thus, when the program is completed, the reference position return operation must be commanded. IB-1501278-D 762 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (Example 1) Local coordinates for absolute value mode (The local coordinate system offset is not cumulated) (1) G28 X0 Y0 ; (8) (9) (2) G00 G90 X1. Y1. ; Y 2500 (3) G92 X0 Y0 ; (4) G00 X500 Y500 ; (5) G52 X1. Y1. ; (6) G00 X0 Y0 ; (7) G01 X500 F100 ; (8) Y500 ; (9) G52 X0 Y0 ; (6) 2000 1500 W1 L1 (3) (2) 1000 (1) New coordinate system created by (3) Matched with local coordinate system by (9). (10) W1 500 (10) G00 X0 Y0 ; (7) Local coordinate system created by (5). (5) (4) 500 1000 1500 2000 2500 3000 R#1 W1 X Current position The local coordinate system is created by (5), canceled (9) and matched with the coordinate system for (3). <Note> If the program is executed repeatedly, the workpiece coordinate system will deviate each time. Thus, when the program is completed, the reference position return operation must be commanded. (Example 2) Local coordinates for incremental value mode (The local coordinate system offset is cumulated.) <Main program> (1) G28 X0 Y0 ; (2) G92 X0 Y0 ; (3) G91 G52 X500 Y500 ; (4) M98 P100 ; (5) G52 X1. Y1. ; (6) M98 P100 ; (7) G52 X-1.5 Y-1.5 ; (8) G00 G90 X0 Y0 ; Y' Y 2500 2000 (B) <Subprogram> 500 (3) (2) (B) G90 G00 X0 Y0 ; (C) G01 X500 ; (D) Y500 ; (E) G91 ; (F) M99 ; (6) (C) W1 L2 1000 O100 ; (D) 1500 M02 ; (A) Y" (4) X' Local coordinate system created by (3). (C) (8) W1 L1 500 R#1 W1 Local coordinate system created by (5). (D) (B) (1) X" 1000 1500 Current position 2000 2500 3000 X (Matched with local coordinate system by (7). The local coordinate system X'Y' is created at the XY coordinate system (500,500) position by (3). The local coordinate system X"Y" is created at the X'Y' coordinate system (1000,1000) position by (5). The local coordinate system is created at the X"Y" coordinate system (-1500, -1500) position by (7). In other words, the same occurs as when the local coordinate system and XY coordinate system are matched and the local coordinate system is canceled. 763 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (Example 3) When used together with workpiece coordinate system (1) G28 X0 Y0 ; G54 G55 (2) G00 G90 G54 X0 Y0 ; X 1000 1000 (3) G52 X500 Y500 ; Y 500 2000 (4) M98 P200 ; (5) G00 G90 G55 X0 Y0 ; (6) M98 P200 ; (7) G00 G90 G54 X0 Y0 ; Workpiece coordinate system offset (parameter setting value) Y 3000 : M02 ; (A) O200 ; (B) G00 X0 Y0 ; (C) G01 X500 F100 ; (D) Y500 ; (E) M99 ; (D) 2500 (B) 2000 G55 (C) (5) W2 1500 (D) (B) 1000 (7) (C) W1 L1 (3) (2) 500 Local coordinate system created by (3) G54 W1 (1) 500 R#1 1000 1500 Current position 2000 2500 3000 X The local coordinate system is created at the G54 coordinate system (500,500) position by (3), but the local coordinate system is not created for the G55 coordinate system. During the movement for (7), the axis moves to the G54 local coordinate system's reference position (zero point). The local coordinate system is canceled by G90G54G52X0Y0;. IB-1501278-D 764 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (Example 4) Combination of workpiece coordinate system G54 and multiple local coordinate systems (1) G28 X 0 Y0 ; G54 (2) G00 G90 G54 X0 Y0 ; X 500 (3) M98 P300 ; Y 500 (4) G52 X1. Y1. ; (5) M98 P300 ; (6) G52 X2. Y2. ; (7) M98 P300 ; (8) G52 X0 Y0 ; : Workpiece coordinate system offset (parameter setting value) 3000 (7) 2500 M02 ; (A) O300 ; (B) G00 X0 Y0 ; (C) G01 X500 F100 ; (D) Y500 ; (E) X0 Y0 ; (F) M99 ; W1 L2 Local coordinate system created by (6) 2000 (5) 1500 W1 L1 (D) 1000 % 500 (8) (2) (3) G54 (E) (C) (B) W1 500 R#1 Local coordinate system created by (4) 1000 1500 2000 2500 3000 Current position The local coordinate system is created at the G54 coordinate system (1000,1000) by (4). The local coordinate system is created at the G54 coordinate system (2000,2000) by (6). The G54 coordinate system and local coordinate system are matched by (8). 765 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.6 Workpiece Coordinate System Setting and Offset ; G54 to G59 (G54.1) Function and purpose (1) The workpiece coordinate systems facilitate the programming on the workpiece, serving the reference position of the machining workpiece as the zero point. (2) These commands enable the tool to move to the positions in the workpiece coordinate system. There are extended workpiece coordinate systems (G54.1) in addition to 6 workpiece coordinate systems, which are used by the programmer for programming (G54 to G59). The number of the extended workpiece coordinate systems varies depending on the MTB specifications. (3) Among the workpiece coordinate systems currently selected by these commands, any workpiece coordinate system with coordinates that have been commanded by the current position of the tool is reset. (The "current position of the tool" includes the compensation amounts for tool radius, tool length and tool position compensation.) (4) A hypothetical machine coordinate system with coordinates that have been commanded by the current position of the tool is set by these commands. (The "current position of the tool" includes the compensation amounts for tool radius, tool length and tool position compensation.) (G54,G92) Workpiece coordinate system (G90) G54 to G59 ; Workpiece coordinate system selection (G54 to G59) G92 X__ Y__ Z__ α__ ; Set workpiece coordinate system α Additional axis Extended workpiece coordinate system G54.1 Pn ; Extended workpiece coordinate system selection (P1 to P300) (*1) G54.1 Pn ; G92 X__ Y__ Z__ ; Workpiece coordinate system setting (P1 to P300) (*1) G10 L20 Pn X__ Y__ Z__ ; Extended workpiece coordinate system offset amount setting (P1 to P300) (*1) When the offset amount of the currently designated workpiece coordinate system is rewritten G10 G54.1 Pn X__ Y__ Z__ ; Extended workpiece coordinate system offset amount setting (P1 to P300) (*1) When the extended workpiece coordinate system is selected, and the offset amount is rewritten (*1) The maximum number of coordinate systems depends on the specifications. IB-1501278-D 766 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Detailed description (1) With any of the G54 through G59 commands or G54.1P1 through G54.1P300 commands, the tool radius compensation amounts for the commanded axes will not be canceled even if workpiece coordinate system selection is commanded. (2) The G54 workpiece coordinate system is selected when the power is turned ON. (3) Commands G54 through G59 and G54.1P1 through G54.1P300 are modal commands (group 12). (4) The coordinate system will move with G92 in a workpiece coordinate system. (5) The offset setting amount in a workpiece coordinate system denotes the distance from the basic machine coordinate system zero point. (#1)Reference position (zero point) return position R#1 M -X Basic machine coordinate system zero point - X(G54)(- 500, - 500) - X(G55)(- 2000, - 1000) W2 W1 -Y (G54) G54 reference position (zero point) - Y(G55) G55 reference position (zero point) -Y G54 X = -500 Y = -500 G55 X = -2000 Y = -1000 (6) The offset settings of workpiece coordinate systems can be changed any number of times. (They can also be changed by G10 L2 Pp1 Xx1 Yy1 Zz1.) [Handling when L or P is omitted] G10 L2 Pn Xx Yy Zz ; n=0 : Set the offset amount in the external workpiece coordinate system. n=1 to 6 : Set the offset amount in the designated workpiece coordinate system. Others : The program error (P35) will occur. G10 L2 Xx Yy Zz ; Set the offset amount in the currently selected workpiece coordinate system. When in G54.1 modal, the program error (P33) will occur. G10 L20 Pn Xx Yy Zz n=1 to maximum number of coordinate systems : Set the offset amount in the desig; nated workpiece coordinate system. (The number of extended workpiece coordinate systems under the specifications) Others : Program error (P35) will occur. G10 L20 Xx Yy Zz ; Set the offset amount in the currently selected workpiece coordinate system. When in G54 to G59 modal, the program error (P33) will occur. G10 Pn Xx Yy Zz ; Set the offset amount in the designated coordinate system No. by P code. When the currently selected coordinate system is G54 to G59, P1 to P6 corresponds to G54 to G59 respectively. When the external coordinate system is selected, P No. corresponds to G54.1 P1 to P300. If other values are set, the program error (P35) will occur. G10 Xx Yy Zz ; Set the offset amount in the currently selected coordinate system. G10 G54.1 Xx Yy Zz ; When there is no P code in the same block as G54.1, the program error (P33) will occur. (7) A new workpiece coordinate system 1 is set by issuing the G92 command in the G54 (workpiece coordinate system 1) mode. At the same time, the other workpiece coordinate systems 2 to 6 (G55 to G59) will move in parallel and new workpiece coordinate systems 2 to 6 will be set. 767 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (8) A hypothetical machine coordinate system is formed at the position that deviates from the new workpiece reference position (zero point) by an amount equivalent to the workpiece coordinate system offset amount. (R1) M -X M -X (a) - X(G54) - X(G55' ) W2 (b) W1 - X(G55) (c) W2 - X(G54' ) W1 (d) - Y(G55) - Y(G54) (e) -Y - Y(G54 ' ) - Y(G55 ' ) -Y (R1) Reference position 1 (a) Hypothetical machine coordinate system based on G92 (b) Old workpiece 1 (G54) coordinate system (c) Old workpiece 2 (G55) coordinate system (d) New workpiece 1 (G54) coordinate system (e) New workpiece 2 (G55) coordinate system After the power has been switched on, the hypothetical machine coordinate system is matched with the basic machine coordinate system by the first automatic (G28) or manual reference position (zero point) return. (9) By setting the hypothetical machine coordinate system, the new workpiece coordinate system will be set at a position that deviates from that hypothetical machine coordinate system by an amount equivalent to the workpiece coordinate system offset amount. (10) When the first automatic (G28) or manual reference position (zero point) return is completed after the power has been turned ON, the basic machine coordinate system and workpiece coordinate systems are set automatically in accordance with the parameter settings. (11) If G54 X- Y-; is commanded after the reference position return (both automatic or manual) executed after the power is turned ON, the program error (P62) will occur. (A speed command is required as the movement will be controlled with the G01 speed.) (12) Do not command a G code for which a P code is used in the same block as G54.1 or G10L20. If a G code is commanded, a P code is used for a prior G command or the program error occurs (P33). (13) If there are no specifications for the extended workpiece coordinate system selection, a program error (P35) will occur when the G54.1 command is executed. This error will also occur when one of P49 to P300 is commanded although the specifications allow up to the 48 sets. Command 6 sets Standard 48 sets 96 sets 300 sets 6 sets ○ ○ ○ ○ 48 sets × ○ ○ ○ 96 sets × × ○ ○ 300 sets × × × ○ ○ : Movable × : P35 Setting value range over (14) If there are no specifications for the extended workpiece coordinate system selection, the program error (P172) will occur when the G10 L20 command is executed. (15) A new workpiece coordinate system P1 can be set by commanding G92 in the G54.1 P1 mode. However, the workpiece coordinate system of the other workpiece coordinate systems G54 to G59, G54.1, and P2 to P96 will move in parallel with it, and a new workpiece coordinate system will be set. IB-1501278-D 768 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (16) The offset amount of the extended workpiece coordinate system is assigned to system variables #7001 onwards. The system variables #7001 to #890n are available up to the valid number of sets. (You can use them for the 300-set specification also, but there are system variables corresponding to up to 96 sets only.) The system variables #101001 to #11595n are available when the 300-set specification is enabled. If you use the system variables #101001 to #11595n when the 300-set specification is disabled, the program error (P241) will occur. CAUTION If the workpiece coordinate system offset amount is changed during single block stop, the new setting will be valid from the next block. (17) When the "#1151 Reset ini" parameter is OFF, the modal of G54.1 command will be retained even if the reset 1 is carried out. (18) The P address of the G54.1 command cannot be commanded alone even in G54.1 modal. Even if commanded, the designated extended workpiece coordinate system cannot be selected. (Ex) P54.1 P5 ; Changed to P5 workpiece coordinate system. P3 ; Ignored. G92 X0 Y0 Z0 ; The current position becomes the zero point of P5 workpiece coordinate system. (19) When G92 is commanded in the extended workpiece coordinate system, the coordinate system will be sifted. Program example (Example 1) (1) G28 X0 Y0 ; (R1) (2) G53 X-1000 Y-500 ; (3) G53 X0 Y0 ; (1) (2) M (3) When the coordinate value of the 1st reference position (R1) is zero, the basic machine coordinate system zero point (M) and reference position (zero point) return position (#1) will coincide. (Example 2) (1) G28 X0 Y0 ; (R1) (2) G90 G00 G53 X0 Y0 ; (1) (3) G54 X-500 Y-500 ; (2) (4) G01 G91 X-500 F100 ; M -X (G54) - 1000 - 500 (5) Y-500 ; (6) X+500 ; -X (G55) (7) Y+500 ; (9) (10) (8) G90 G00 G55 X0 Y0 ; (3) W2 W1 -500 (8) (5) (11) (4) (6) -500 -1000 (7) -1000 -1500 (9) G01 X-500 F200 ; (10) X0 Y-500 ; -Y (G55) (11) G90 G28 X0 Y0 ; 769 -Y (G54) IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (Example 3) When workpiece coordinate system G54 (-500, -500) has deviated in Example 2. (It is assumed that (3) to (10) in Example 2 have been entered in subprogram 1111.) (1) G28 X0 Y0 ; (2) G90 G00 G53 X0 Y0 ; (This is not required when there is no G53 offset.) (3) G54 X-500 Y-500 ; Amount by which workpiece coordinate system deviates (4) G92 X0 Y0 ; New workpiece coordinate system is set. (5) M98 P1111 ; (R1) (1) (2) -X (c) - X(G55) M - X(G54) -X (G54') (d) (a) (3) (4) - X(G55') (b) W1 -Y (G54) W2 -Y (G55) -Y (G54') - Y(G55') -Y (R1) Reference position return position (a) Old G54 coordinate system (b) New G54 coordinate system (c) Old G55 coordinate system (d) New G55 coordinate system Note (1) The workpiece coordinate system will deviate each time steps (3) to (5) shown in the above figure are repeated. The reference position return (G28) command should therefore be issued upon completion of the program. IB-1501278-D 770 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (Example 4) When six workpieces are placed on the same coordinate system of G54 to G59, and each is to be machined with the same machining. (1) Setting of workpiece offset data Workpiece 1 X = -100.000 Y = -100.000.....G54 Workpiece 2 X = -100.000 Y = -500.000.....G55 Workpiece 3 X = -500.000 Y = -100.000.....G56 Workpiece 4 X = -500.000 Y = -500.000.....G57 Workpiece 5 X = -900.000 Y = -100.000.....G58 Workpiece 6 X = -900.000 Y = -500.000.....G59 (2) Machining program (subprogram) O100; N1 G90 G00 G43 X-50. Y-50. Z-100. H10 ; Positioning N2 G01 X-200. F50 ; Surface cutting Y-200. ; Surface cutting X-50. ; Surface cutting Y-50. ; Surface cutting N3 G28 X0 Y0 Z0 ; N4 G98 G81 X-125. Y-75. Z-150. R-100. F40 ; : Drilling 1 X-175. Y-125. ; Drilling 2 X-125. Y-175. ; Drilling 3 X- 75. Y-125. ; Drilling 4 G80 ; N5 G28 X0 Y0 Z0 ; : N6 G98 G84 X-125. Y-75. Z-150. R-100. F40 ; Tapping 1 X-175. Y-125. ; Tapping 2 X-125. Y-175. ; Tapping 3 X- 75. Y-125. ; Tapping 4 G80 ; M99 ; (3) Positioning program (main) G28 X0 Y0 Z0 ; At power ON N1 G90 G54 M98 P100 ; N2 G55 M98 P100 ; N3 G57 M98 P100 ; N4 G56 M98 P100 ; N5 G58 M98 P100 ; N6 G59 M98 P100 ; N7 G28 X0 Y0 Z0 ; N8 M02 ; % 771 IB-1501278-D -X IB-1501278-D -X -X G59 G58 772 -Y W6 -Y W5 -X -X G57 G56 -Y W4 -Y W3 900mm -X -X 2 3 1 G55 4 G54 W1 200mm 175 125 75 500mm 100mm 0 M -Y W2 -Y -Y 175 125 200mm 50 75 50mm 100mm 500mm M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (Example 5) Program example when continuously using 48 sets of added workpiece coordinate system offsets. In this example, the offsets for each workpiece are set beforehand in P1 to P48 when 48 workpieces are fixed on a table, as shown in the drawing below. P8 P6 P7 P3 P11 P9 P24 P14 P22 P23 P19 P30 P38 P40 P35 P43 P41 P42 P32 P34 P36 P37 P39 P17 P31 P29 P28 P26 P16 P18 P20 P21 P27 P25 P1 P15 P13 P12 P10 P2 P4 P5 P47 P45 P44 P33 P46 01000 01001 G28 XYZ ; Reference position return G43 X-10.Y-10.Z-100.H10.; #100=1 ; Initialize added workpiece coordinate system P No. G01 X-30.; G90 ; Absolute value mode Y-30.; WHILE [#100LE48]D01 ; Repeat P No. to 48 X-10.; G54.1 P#100 ; Set workpiece coordinate system Y-10.; M98 P1001 ; Call sub-program G00 G40 Z10.; #100=#100+1 ; P No. +1 G98 G81 X-20.Y-15.Z150.R5.F40; Return to reference position X-20.Y-25.; END1 ; G28 Z ; P48 Contour Drilling X-25.Y-20.; G28 XY ; X-15.Y-20.; M02 ; G80 ; M99 ; 773 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (Example 6) Program example when the added workpiece coordinate system offsets are transferred to the standard workpiece coordinate system offsets and used. In this example, the workpiece coordinate system offsets for each workpiece are set beforehand in P1 to P24 when the workpiece is fixed on a rotating table, as shown in the drawing below. P3 P19 P20 P22 P23 P21 P24 P1 Z P2 P5 P6 P4 X B 020000 (Main) G28 XYZB ; Reference position return G90 ; Absolute value mode G00 B0 ; Position table to face 1 G65 P2001 A1 ; Load workpiece offsets M98 P2002 ; Drilling G00 B90 ; Position table to face 2 G65 P2001 A7 ; M98 P2002 ; G00 B180 ; Position table to face 3 G65 P2001 A13 ; M98 P2002 ; G00 B270 ; Position table to face 4 G65 P2001 A19 ; M98 P2002 ; G28 XYB ; Return to reference position M02 ; % IB-1501278-D 774 Y M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 02001 (Transmission of workpiece offsets) #2=5221 ; Leading No. of workpiece coordinate system variables #3=[#1-1]*20+7001 ; Leading No. of added workpiece coordinate system variables #5=0 ; No. of sets counter clear WHILE [#5 LT 6] DO1 ; Check No. of sets #6=#6+1 ; Set transmission source 1st axis variable No. #7=#7+1 ; Set transmission destination 1st axis variable No. #4=#4+1 ; Clear No. of axes counter WHILE [#4 LT 6] DO2 ; Check No. of axes #[#6]=#[#7] ; Transmit variable data #6=#6+1 ; Set transmission source next axis #7=#7+1 ; Set transmission destination next axis #4=#4+1 ; No. of axes counter +1 END2 ; #2=#2+20 ; Transmission source Set lead of next variable set. #3=#3+20 ; Transmission destination Set lead of next variable set. #5=#5+1 ; No. of sets counter +1 END1 ; M99 ; % O2002 (Drilling) G54 M98 H100 ; Drilling in G54 coordinate system G55 M98 H100 ; G55 G56 M98 H100 ; G56 G57 M98 H100 ; G57 G58 M98 H100 ; G58 G59 M98 H100 ; G59 G28 Z0 ; M99 ; N100 G98 G81 X-20. Y-15. Z-150. R5. F40 ; Fixed cycle for drilling X-25. Y-20. ; X-20. Y-25. ; X-15. Y-20. ; G80 ; G28 Z ; M99 ; % 775 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.7 Workpiece Coordinate System Preset ; G92.1 Function and purpose This function presets the workpiece coordinate system shifted with the program command during manual operation to the workpiece coordinate system offset from the machine zero point by the workpiece coordinate offset amount by the program command (G92.1). The workpiece coordinate system, which is set when the following type of operation or program command is executed, will be shifted from the machine coordinate system. When manual interrupt is executed while manual absolute is OFF When movement command is issued in machine lock state When axis is moved with handle interrupt When operation is carried out with mirror image When local coordinate system is set with G52 Shifting the workpiece coordinate system with G92 This function presets the shifted workpiece coordinate system to the workpiece coordinate system offset from the machine zero point by the workpiece coordinate offset amount. This takes place in the same manner as manual reference position return. Whether to preset the relative coordinate depends on the MTB specifications (parameter "#1228 aux12/bit6"). Command format G92.1 α0 X0. Y0. Z0. α0 ; Additional axis (1) Command the address of the axis to be preset. The axis will not be preset unless commanded. (2) A program error (P35) will occur if a value other than "0" is commanded. (3) Command G92.1 in an independent block. (4) Whether to conduct an error check when the coordinate system preset command (G92.1) is independently issued depends on the MTB specifications (parameter "#1242 set14/bit1"). IB-1501278-D 776 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Detailed description (1) When manual operation is carried out when manual absolute is set to OFF, or if the axis is moved with handle interrupt. Y Y (Wx) (C) (C) (a) W1’ (Wy) W1 X W1 X M (a) Manual movement amount (C) Current position (Wx) Workpiece coordinate x after preset (Wy) Workpiece coordinate y after preset If manual operation is carried out when manual absolute is set to OFF, or if the axis is moved with handle interrupt, the workpiece coordinate system will be shifted by the manual movement amount. This function returns the shifted workpiece coordinate zero point W1' to the original workpiece coordinate zero point W1, and sets the distance from W1 to the current position as the workpiece coordinate system's current position. (2) When movement command is issued in machine lock state Y Y (a) (Wx) (C) (b) (C) (Wy) (W1) (W1) X X (a) Movement amount during machine lock (b) Workpiece coordinate system coordinate value (Wx) Workpiece coordinate x after preset (Wy) Workpiece coordinate y after preset (C) Current position (W1) Workpiece coordinate zero point If the movement command is issued in the machine lock state, the current position will not move, and only the workpiece coordinates will move. This function returns the moved workpiece coordinates to the original current position, and sets the distance from W1 to the current position as the workpiece coordinate system's current position. 777 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (3) When operation is carried out with mirror image Y Y (Wx) (C) (C) (a) (b) (Wy) (W1) (W1) X (d) (a) Actual operation (b) Program command (C) Current position (d) Mirror image center (Wx) Workpiece coordinate x after preset (Wy) Workpiece coordinate y after preset X (W1) Workpiece coordinate zero point If operation is carried out with mirror image, only the NC internal coordinates are used as the program command coordinates. The other coordinates are the current position coordinates. This function sets the NC internal coordinates as the current position coordinates. (4) Setting local coordinate system with G52 Y Y (a) (Wx) (C) (C) (b) (L1) (Wy) (W1) (W1) X (a) Local coordinates x (b) Local coordinates y (Wx) Workpiece coordinate x after preset (Wy) Workpiece coordinate y after preset (C) Current position (L1) Local coordinate zero point X (W1) Workpiece coordinate zero point The local coordinate system is set with the G52 command, and the program commands, etc., are issued with the local coordinate system. With this function, the set local coordinate system is canceled, and the program commands, etc., use the workpiece coordinate system which has W1 as the zero point. The canceled local coordinate system is only the selected workpiece coordinate system. IB-1501278-D 778 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (5) Shifting the workpiece coordinate system with G92 Y Y (a) (Wx) (C) (C) (b) (W1') (Wy) (W1) (W1) X X (a) Local coordinates x (b) Local coordinates y (Wx) Workpiece coordinate x after preset (Wy) Workpiece coordinate y after preset (C) Current position (W1) Workpiece coordinate zero point (W1') Workpiece zero point after G92 command The workpiece coordinate system shifts with the G92 command, and the distance between W1' and the current position is set as the current position of the workpiece coordinate system. This function returns the shifted workpiece coordinate zero point to W1, and sets the distance from W1 to the current position as the workpiece coordinate system's present position. This is valid for all workpiece coordinate systems. Program example The workpiece coordinate system shifted with G92 is preset with G92.1. Y Y (5) (4) 1500 1500 (3) (2) 1000 1000 (W1') 500 500 (1) (W1) 500 1000 1500 X (W1) (mm) 500 1000 1500 X (mm) (W1) Workpiece coordinate zero point (W1') Workpiece zero point after G92 command (Example) G28 X0 Y0 ; G00 G90 X1. Y1. ; G92 X0 Y0 G00 X500 Y500 ; G92.1 X0 Y0 ; ... (1) ... (2) ... (3) ... (4) ... (5) 779 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Relationship with other functions Tool No./Tool Compensation No. (T Code)/tool length compensation If the error check is enabled when the workpiece coordinate system preset is independently commanded (*1), command all the tool compensation axes when commanding "G92.1" during the tool compensation. When commanding "G92.1" during the tool length compensation, designate the tool length compensation axis. If those axes are not commanded, a program error (P29) will occur. (*1) The setting depends on the MTB specifications (parameter "#1242 set14/bit1"). Tool nose radius compensation / Tool radius compensation Cancel the tool nose radius compensation or the tool radius compensation, and command the workpiece coordinate system preset (G92.1). When the workpiece coordinate system preset (G92.1) is commanded during the tool nose radius compensation or the tool radius compensation, a program error (P29) will occur if none of the tool compensation axes are commanded. 3-dimensional coordinate conversion If the workpiece coordinate system preset (G92.1) is commanded in 3-dimensional coordinate conversion, a program error (P921) will occur. Other G code commands If the workpiece coordinate system preset (G92.1) is commanded during the modal shown below, a program error (P34) will occur. (1) Scaling (2) Coordinate rotation by program (3) G command mirror image (4) Tool length compensation along the tool axis Precautions (1) Cancel tool length compensation, tool nose radius compensation, tool radius compensation, and tool position offset when using this function. If this function is executed without canceling them, the workpiece coordinates will be at a position obtained by subtracting the workpiece coordinate offset amount from the machine value. Thus, the compensation vector will be temporarily canceled. (2) This function cannot be executed while the program is being resumed. IB-1501278-D 780 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.8 3-dimensional Coordinate Conversion ; G68/G69 Function and purpose With the 3-dimensional coordinate conversion function, a new coordinate system can be defined by shifting the zero point and rotating in respect to the X, Y and Z axes of the currently set workpiece coordinate system. By using this function, an arbitrary spatial plane can be defined, and machining on that plane can be carried out with normal program commands. The validity of this function depends on the MTB specifications. Refer to the specifications of your machine tool. Y Y' (P) Z' (W) X' Z (M) X (M) Machine coordinate system (P) G68 Program coordinate system (W) Workpiece coordinate system When the G68 command is issued, the zero point is shifted by the command value (x, y, z) in respect to the current local coordinate system. A new G68 program coordinate system rotated by the designated rotation angle "r" in respect to the commanded rotation center direction (i, j, k) is created. The local coordinate system is the same as the workpiece coordinate system when the local coordinate system offset is not ON. Command format 3-dimensional coordinate conversion mode command G68 X__ Y__ Z__ I__ J__ K__ R__ ; X,Y,Z Rotation center coordinates Designate with the absolute position of the local coordinate system. I,J,K Rotation center axis direction (1: Designated 0: Not designated) Note that "1" is designated for only one of the three axes. "0" is designated for the other two axes. R Rotation angle The counterclockwise direction looking at the rotation center from the rotation center axis direction is positive (+). The setting range is -360 to 360°, and the unit follows the minimum command unit. 3-dimensional coordinate conversion mode cancel command G69 ; 781 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Detailed description (1) Command the rotation center coordinates with absolute values. (2) If the rotation center coordinates are omitted, the zero point of the currently set coordinate system will be the rotation center coordinates. (3) Designate values for all of I, J and K. If any of the I, J, K is not designated, program coordinate rotation command will be valid. (4) Set "1" in only one of I, J and K, and set "0" for the other two. The program error (P33) will occur if "1" is set in two or more. (5) The program error (P33) will also occur if "0" is set for all I, J and K. (6) When addresses I, J and K are not designated, this will be handled as the program coordinate rotation. (7) If a number other than "0" (including numbers of two or more digits) is designated for addresses I, J and K, this will be handled as "1". If a blank is designated, this will be handled as "0". (8) If a G code that cannot be commanded in the 3-dimensional coordinate conversion modal is issued, the program error (P921) will occur. When 3-dimensional coordinate conversion is commanded during the modal where 3-dimensional coordinate conversion cannot be carried out, the program error (P922) or program error (P923) will also occur. For details, refer to "Relationship with Other Functions". (9) Command G68 in an independent block. If another G code command is issued to the same block as for the G68 command, a program error (P923) will occur. (10) The 3-dimensional coordinate conversion command for the rotary axis will result in the program error (P32). (11) If a 3-dimensional coordinate conversion command is issued when there are no specifications for 3-dimensional coordinate conversion, the program error (P920) will occur. Coordinate system (1) By issuing the 3-dimensional coordinate conversion command, a new coordinate system (G68 program coordinate system) will be created on the local coordinate system. (2) The coordinate system for the 3-dimensional coordinate conversion rotation center coordinates is the local coordinate system. Thus, these coordinate systems are affected by the following coordinate system offset and coordinate system shift amount. When local coordinate system is set with G52 G92 shift amount by G92 command Coordinate system offset corresponding to the workpiece coordinate system selected with the command External workpiece coordinate offset Manual interruption amount or manual feed amount when manual ABS is OFF (3) If 3-dimensional coordinate conversion is commanded again during the 3-dimensional coordinate conversion modal, a G68 program coordinate system is created on the current G68 program coordinate system, and is used as a new G68 program coordinate system. (4) The local coordinate system cannot be created (G52) on the G68 program coordinate system. (If G52 is issued, the program error (P921) will occur.) (5) G68 program coordinate system can be reset either by G69 command or reset inputting. (Exclude reset 1 when "0" is set to the parameter "#1151 rsint") (6) Whether to run the manual operation during the 3-dimensional coordinate conversion modal in the G68 program coordinate system can be designated by switching the manual feed coordinate for 3-dimensional coordinate conversion. (7) Even if the 3-dimensional coordinate conversion modal state is canceled by reset, etc., the manual operation is possible in the G68 program coordinate system before the 3-dimensional coordinate conversion modal is canceled, until the G69 command is issued. In the same way as during the 3-dimensional coordinate conversion modal, the target coordinate can be designated by switching the manual feed coordinate for 3-dimensional coordinate conversion. IB-1501278-D 782 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Rotation angle (1) For the rotation angle, the counterclockwise direction looking at the rotation center from the plus direction of the rotation center axis is the plus (+) direction. (2) The rotation angle command unit with no decimal point depends on the parameter "#1078 Decpt2" (Decimal pnt type 2). (3) If the rotation angle is omitted, the rotation angle will be handled as 0°. Rotation center coordinates (1) The G68 rotation center coordinate system is commanded with the local coordinate system (G68 program coordinate system during the 3-dimensional coordinate conversion modal). (2) The rotation center coordinate designation is handled as an absolute value command whether or not an absolute/ incremental modal (G90/G91) is currently being executed. (3) If the rotation center coordinate is omitted, it will be handled as if the zero point of the current local coordinate (G68 program coordinate system during the 3-dimensional coordinate conversion modal) is designated for the omitted address's axis. (The same as when "0" is just set.) G68 multiple commands By commanding 3-dimensional coordinate conversion during the 3-dimensional coordinate conversion modal, two or more multiple commands can be issued. (1) The 3-dimensional coordinate conversion command in the 3-dimensional coordinate conversion modal is combined with the conversion in the modal. (2) If 3-dimensional coordinate conversion is overlapped during the 3-dimensional coordinate conversion modal, the overlapped 3-dimensional coordinate conversion will be created on the coordinate system (G68 program coordinate system) created with 3-dimensional coordinate conversion in the modal. Thus, the rotary axis and coordinates must be designated with this G68 program coordinate system. If creating a 90° rotated coordinate system for X axis and Y axis each, commands must be issued as in Example 2, not Example 1. <Example 1> G68 X0. Y0. Z0. I1 J0 K0 R90.; X axis rotation 90° G68 X0. Y0. Z0. I0 J1 K0 R90.; Y axis rotation 90° (The Y axis designated here is the same as the Z axis in the original coordinate system.) <Example 2> G68 X0. Y0. Z0. I1 J0 K0 R90.; X axis rotation 90° G68 X0. Y0. Z0. I0 J0 K1 R-90.; Z axis rotation 90° (The Z axis -90 rotation designated here is the same as the Y axis +90 rotation in the original coordinate system.) 783 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Conversion method for 3-dimensional coordinate conversion The coordinate values (Xp, Yp, Zp) in the newly set G68 program coordinate system and the coordinate values (Xm, Ym, Zm) in the reference workpiece coordinate system are converted as shown below. First G68 command [Xm, Ym, Zm, 1]=[Xp, Yp, Zp, 1]R1 T1 -1 (Forward row) (Reverse row) -1 [Xp, Yp, Zp, 1]=[Xm, Ym, Zm, 1](T1 )(R1 ) Second G68 command [Xm, Ym, Zm, 1]=[Xp, Yp, Zp, 1]R2 T2 R1 T1 [Xp, Yp, Zp, 1]=[Xm, Ym, Zm, 1](T1-1)(R1-1)(T2-1)(R2-1) R1, R2 : Rotation row calculated from first and second G68 parameter T1, T2 : Movement row calculated from first and second G68 parameter The conversion rows Rn and Tn (n = 1, 2) are as follow. Rn conversion row I designation (rotation around X J designation (rotation around Y K designation (rotation around Z axis) axis) axis) 1 0 0 0 cosR 0 - sinR 0 cosR sinR 0 0 0 cosR sinR 0 0 1 0 0 - sinR cosR 0 0 0 - sinR cosR 0 sinR 0 cosR 0 0 0 1 0 0 0 0 1 0 0 0 1 0 0 0 1 Tn conversion row 1 0 0 0 0 1 0 0 0 0 1 0 x y z 1 x, y, z : Rotation center coordinates (parallel movement amount) I, J, K : Rotation axis selection R : Rotation angle Manual operation in G68 program coordinate system Whether to run manual operations (jog feed, incremental feed, and manual handle feed) during the 3-dimensional coordinate conversion modal in the coordinate system (G68 program coordinate system) after the 3-dimensional coordinate conversion command was issued can be designated by switching the manual feed coordinate for 3-dimensional coordinate conversion. When the axis stops during machining, operations such as a pulling operation by manual feed can be performed in the G68 program coordinate system. (1) Coordinate switching enable conditions A manual operation coordinate change by switching the manual feed coordinate for 3-dimensional coordinate conversion is available only when the output signal that enables the manual feed for 3-dimensional coordinate conversion is set to ON. (The operation of the PLC signal depends on the MTB specifications.) The manual operation coordinate change by switching the manual feed coordinate for 3-dimensional coordinate conversion becomes valid after three basic axes have stopped. When the manual feed coordinate for 3-dimensional coordinate conversion is switched while even one of three basic axes is moving, a coordinate change is performed after three basic axes have stopped. The output signal that enables the manual feed for 3-dimensional coordinate conversion is set to ON when all of the following conditions are satisfied. (a) One of the jog, incremental, or handle feed modes is selected. (b) G68 (3-dimensional coordinate conversion command) is commanded once. However, if the signal is canceled by the G69 command, it is not turnd ON until G68 is commanded again. IB-1501278-D 784 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (2) Operation example The absolute coordinate positions are displayed in the G68 program coordinate system with a parameter. This depends on the MTB specifications (parameter "#1561 3Dcdc"). The machine zero point is used as the workpiece coordinate zero point. Also, the manual ABS is set to ON to return to the position commanded by the machining program with the absolute command after a manual interruption. <Operation procedure> (1) Set mode selection to automatic operation (memory, MDI, tape, etc.) mode. (2) Execute the following machining program, then perform single block stop after the N03 block has been completed... (a) N01 G68 X0. Z0. Y0. I0 J1 K0 R45. ; Set the G68 program coordinate system (X’Y’Z’) which has been rotated +45°in the Y axis direction around the (X0, Z0). N02 G00 X1.; N03 G00 Z-10.; Position the axis near the hole position in the G68 program coordinate system. N04 G01 Z-20.; Cutting in G68 program coordinate system (3) Set the handle mode, then select the Z axis with the 1st handle. Then, check that the output signal that enables the manual feed for 3-dimensional coordinate conversion is set to ON. (4) Set to ON the signal that switches the manual feed coordinate for 3-dimensional coordinate conversion. (5) Move the axis by -5. with the handle in the Z' direction of the G68 program coordinate, then check the hole position... (b) (6) Move the axis by +7. with the handle in the Z' direction to retract the tool... (c) (7) After executing an automatic start, execute the N04 block... (d) X X’ Z’ (a) Z (b) (c) (d) Absolute coordinate (a) Positioning (b) Hole position check (c) Retract (d) Cutting Machine coordinate X 1.000 -6.364 Z -10.000 -7.778 X 1.000 -9.900 Z -15.000 -11.314 X 1.000 -4.950 Z -8.000 -6.364 X 1.000 -13.435 Z -20.000 -14.849 785 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (3) Precautions (a) When the automatic and manual operation modes are selected simultaneously, the manual feed for 3-dimensional coordinate conversion cannot be commanded. However, manual operation is available only for the axis for which the manual automatic simultaneous valid axis signal is set to ON. (b) The speed limit is applied so that the speed distributed to the movement amount in the machine axis direction does not exceed the clamp speed of each axis. (c) If even one axis satisfies the external deceleration conditions, the speed limit is applied so that the movement speed in each axis direction does not exceed the external deceleration speed. (d) The movement amount by handle feed conforms to that on the G68 program coordinate system. If clamp ("#1281 ext17/bit4=1") is commanded with the number of handle input pulses, the movement amount on the G68 program coordinate system becomes the integral multiple of the handle magnification. (e) When clamp ("#1281 ext17/bit4=1") is commanded with the number of handle input pulses, if the one-scale movement amount by manual feed for 3-dimensional coordinate conversion exceeds the movement amount for the specified time at clamp speed, the operation error (M01 0060) occurs at the time of pulse occurrence, not at the time of handle axis selection, and movement will fail. To move, reduce the handle magnification. (f) The manual feed operation for 3-dimensional coordinate conversion is not available in manual reference position return mode. If it is started, an operation error (M01 0060) will occur. To use the manual reference position return mode, set to OFF the signal that switches the manual feed coordinate for 3-dimensional coordinate conversion. (g) The manual feed operation for 3-dimensional coordinate conversion is not available in tool retract and return mode. If it is started, an operation error (M01 0060) will occur. To use the tool escape mode, set to OFF the signal that switches the manual feed coordinate for 3-dimensional coordinate conversion. (h) This function is not compatible with the manual tool length measurement function, workpiece position measurement function, and manual skip based on the manual feed for 3-dimensional coordinate conversion. If it is started, an operation error (M01 014) will occur. While the manual tool length measurement function or workpiece position measurement function is active or when manual skip is valid, set to OFF the signal that switches the manual feed coordinate for 3-dimensional coordinate conversion. (i) When the manual automatic simultaneous valid axis signal is set to ON for any of three basic axes, operation is performed in the same way as when the manual automatic simultaneous valid axis signal for three basic axes is set to ON. (j) When the manual machine lock signal is set to ON for any of three basic axes, operation is performed in the same way as when the manual machine lock signal for three basic axes is set to ON. (k) When a factor such as manual interlock that triggers the stop of the axis under manual movement occurs at any of three basic axes, execute deceleration stop on the three basic axes. (l) When the 3-dimensional coordinate conversion modal state is canceled by reset, etc., the manual feed for 3dimensional coordinate conversion is possible; however, the absolute coordinate position display function and other functions conform to the 3-dimensional coordinate conversion modal state and parameter setting. The coordinate cannot be changed by switching the manual feed coordinate for 3-dimensional coordinate conversion. (m) If the G69.1 command exists up to the block to be restart-searched at program restart, it also cancels the state that enables the manual feed in 3-dimensional coordinate conversion as the G69.1 command does. IB-1501278-D 786 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Program example Program example 1 N1 G68 X10.Y0. Z0. I0 J1 K0 R-30.; N2 G68 X0. Y10. Z0. I1 J0 K0 R45.; : N3 G69 ; +Z +Y" +Y 45 +Z" +Y' +X" P"(0,10,0) (B) +X' P(0,0,0) (L) - 30 P'(10,0,0) (A) +X (1) With N1, the zero point is shifted by (x, y, z) = (10, 0, 0) in respect to the currently set local coordinate system (L). The new G68 program coordinate system (A) rotated -30° in the counterclockwise direction using the Y axis as the center, is set. (2) With N2, the zero point is shifted by (x, y, z) = (0, 10, 0) in respect to the newly set G68 program coordinate system (A). The new G68 program coordinate system (B) rotated +45° in the counterclockwise direction using the X axis as the center, is set. (3) With N3, the G68 program coordinate systems that have been set are all canceled, and the state prior to where the first G68 has been commanded is resumed. 787 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Program example 2 This is only a sample program to explain about the operations. (To actually proceed with the machining by using this program, the dedicated tools and the tool change functions are required.) (1) Example of machining program using arc cutting in the following program example, the arc cutting (N3 block) carried out on the top of the workpiece is also carried out on the side of the workpiece. By using 3-dimensional coordinate conversion, the side can be cut using the same process (N8 block). N01 G17 G90 G00 X0 Y0 Z0; Position to the workpiece zero point P. N02 G00 X100. Y200. Z200.; Move to (100, 200, 200) with rapid traverse. N03 G02 X100. Y400. J100. F1000; Carry out arc cutting on workpiece top. N04 G00 Z300.; Escape +100 in +Z direction at rapid traverse rate. N05 G68 X0 Y0 Z200. I0 J1 K0 R90.; Set the G68 program coordinate system (X’Y’Z’) which has been rotated +90°in the Y axis direction around the (0,0,200). N06 G17 G90 G00 X0 Y0 Z0; Position to the new program zero point P'. N07 G00 X100. Y200. Z200.; Move to G68 program coordinate system (100, 200, 200) and workpiece coordinate system (200, 200, 100) at rapid traverse rate. N08 G02 X100. Y400. J100. F1000; Carry out arc cutting on workpiece side. N09 G00 Z300.; Move +100 in + Z' direction of G68 program coordinate system at rapid traverse rate. N10 G69 ; N11 M02 ; +Y' +Z +Y N4 N6 N3 N9 N7 P ’(0,0,200) N8 N1 N2 P (0,0,0) +Z' +X +X' IB-1501278-D 788 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (2) Example of machining program using fixed cycle In the following program, the bolt hole circle (N08 block) executed on the top of the workpiece is also carried out on the side of the workpiece. By using 3-dimensional coordinate conversion, the side can be cut using the same process (N18 block). N01 G90 G00 X0 Y0 Z0; Position to the workpiece coordinate system's 1st workpiece zero point. N02 F2000 ; N03 G00 X100. Y100. Z-600.; Move to (100, 100, -600) with rapid traverse. N04 G52 X100. Y100. Z-600.; Set the local coordinate system (X'Y'Z') to the (100, 100, -600). N05 G00 X100. Y10. Z 200.; Move to (100, 10, 200) position in the local coordinate system at a rapid traverse. N06 G91 ; Incremental value command N07 G81 Z-10. R5. L0 F2000; Drilling cancel N08 G34 X100. Y200. I90. J270. K10.; Bolt hole circle N09 G80 ; Drilling cancel N10 G91 G00 X-200.; Move -200 from machining end point in X axis direction at rapid traverse rate. N11 G90 G52 X0 Y0 Z0; Cancel local coordinate system. N12 G90 G00 X0 Y0 Z0; Position to workpiece zero point. N13 G00 X100. Y100. Z-400.; Move to (100, 100, -400) with rapid traverse. N14 G68 X100. Y100. Z-400. I0 J1 K0 R90.; Set G68 program coordinate system (X",Y",Z") rotated +90° in Y axis direction using (100, 100, -400) position as center. N15 G00 X100.Y10. Z200.; Move to (100, 10, 200) position in the G68 program coordinate system at a rapid traverse rate. N16 G91 ; Incremental value command N17 G81 Z-10. R5. L0 F200; Drilling cancel N18 G34 X100.Y200. I90. J270. K10.; Bolt hole circle N19 G80 ; Drilling cancel N20 G91 G00 X-200.; Move -200 from machining end point in X axis direction at rapid traverse rate. N21 G69 ; Cancel 3-dimensional coordinate conversion modal. N22 M02 ; End program. +Y N1 (0,0,0) N12 +X N20 N13 -Z +Y’’ N10 +Z’ N7 N9 N3 +Y’ ’’ (100,100, - 400) N5 N17 N19 N15 ’ (100,100, - 600) +Z’’ +X’’ +X’ 789 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Relationship with Other Functions (1) Circular interpolation Circular interpolation in the 3-dimensional coordinate conversion modal operates according to the coordinate value resulting from 3-dimensional coordinate conversion. With G17, G18 and G19 commands, circular interpolation functions normally for all the planes in which 3-dimensional coordinate conversion has been executed. (2) Fine spline Designation of a spline axis should be done to the movement axis after the 3-dimensional coordinate conversion. When a movement occurs to the axis in which spline cannot be designated, spline will be in the pause status. (3) Reference position check The 3-dimensional coordinate conversion is applied for the positioning commanded by G27 in the 3-dimensional coordinate conversion modal. (4) Reference point return The 3-dimensional coordinate conversion is applied for the mid-point commanded by G28 and G30 in the 3-dimensional coordinate conversion modal. However, reference position return will be carried out without the 3-dimensional coordinate conversion. (5) Tool change position return 3-dimensional coordinate conversion is not carried out for the tool change position even if a command from G30.1 to G30.6 is issued in the 3-dimensional coordinate conversion modal. The returning order and position will be on the machine coordinate system. (6) Tool compensation When executing the tool length/radius/position compensation in the 3-dimensional coordinate conversion modal, the 3-dimensional coordinate conversion is carried out after the compensation value has been applied. (7) Machine coordinate system selection Coordinate conversion will not be carried out for the machine coordinate system even if G53 command is issued in the 3-dimensional coordinate conversion modal. (8) Mirror image When issuing the mirror image command in the 3-dimensional coordinate conversion modal, as well as when executing the 3-dimensional coordinate conversion in the mirror image modal, 3-dimensional coordinate conversion will be executed for the coordinate value, which is calculated by the mirror image. (9) User macro When a user macro call command is issued in the 3-dimensional coordinate conversion modal, the 3-dimensional coordinate conversion will be valid after the macro execution. (10) Fixed cycle for drilling The fixed cycle in the 3-dimensional coordinate conversion can be executed in an oblique direction for the orthogonal coordinate system. In the same manner, synchronous tapping cycle can also be executed. However, the fixed cycle hole drilling rapid traverse speed during the 3-dimensional coordinate conversion modal is switched as shown below by the settings of the parameters "#15663 DselctDrillaxMode" and "#1564 3Dspd". (This depends on the MTB specifications.) Fixed cycle rapid traverse speed during 3-dimensional coordinate conversion #1566 0 (Rapid traverse mode) 1 (Cutting mode) #1564 - 0 Rapid traverse speed The "#2001 rapid" value for The "#2002 clamp" value each machine axis is con- for each machine axis is verted to the speed in the converted to the speed in composite movement direc- the composite movement tion, and the slowest speed direction, and the slowest is applied. speed is applied. 1 to 1000000 The value (mm/min) set to "#1564 3Dspd" is applied. <Note> The speed of operation 1 in the table above conforms to the "#2001 rapid" value regardless of the parameter setting above. When a macro interruption, MDI interruption, or PLC interruption is carried out in the fixed cycle during 3dimensional coordinate conversion, the rapid traverse speed in the interrupt machining program conforms to the "#2001 rapid" value regardless of the parameter setting above. IB-1501278-D 790 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (I) (1) (2) (5) (R) (3) (4) [Operation] (1) Position to the initial position at the rapid traverse rate. (2) Position to the R point at the rapid traverse rate. (3) Hole machining is conducted by cutting feed. (4) Escape to the R point. Cutting feed or rapid traverse depending on the fixed cycle mode. (5) The tool is returned to the initial point at the rapid traverse rate. (I) Initial point (R) R point Parameter "#1566" becomes valid when each fixed cycle is set to rapid traverse mode. The operation numbers in the table below correspond to those in the figure above. Relationships between fixed cycles and parameter "#1566" G Code G73 [Operation] (2) ○ [Operation] (3) × [Operation] (4) ○ [Operation] (5) ○ G74 ○ × × ○ G75 ○ × ○ ○ G76 ○ × ○ ○ G81 ○ × ○ ○ G82 ○ × ○ ○ G83 ○ × ○ ○ G84 ○ × × ○ G85 ○ × × ○ G86 ○ × ○ ○ G87 ○ ○ × ○ G88 ○ × ○ ○ G89 ○ × × ○ o: "#1566" is valid (rapid traverse). x: "#1566" is irrelevant (cutting feed). For G87, the movement completion position in operation 3 is set to R point. Parameter "#1566" is also valid for rapid traverse operation at G76 or G87 shift. Parameter "#1566" is also valid for G73 or G83 return operation. (11) Synchronous tapping cycle The synchronous tapping cycle in the 3D coordinate conversion can be executed in an oblique direction for the orthogonal coordinate system. The Synchronous tapping cycle in the 3-dimensional coordinate conversion modal will not function even if "#1223 aux07/bit3" (synchronous tapping in-position check expansion valid)" is valid. Set the synchronous tapping cycle to invalid. (This parameter setting depends on the MTB specifications.) The rapid traverse rate in synchronous tapping cycle always follows the value of #2001(rapid traverse rate) during the 3D coordinate conversion mode, regardless of the values of #1566(switch drill axis's mode from rapid traverse during 3D) and #1564(hole drilling cycle during 3D coordinate conversion). If any of the orthogonal axes of all the active part systems is under machine lock during 3-dimensional coordinate conversion, normal synchronous tapping is applied even though the high-speed synchronous tapping specification is enabled. 791 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (12) Geometric command Geometric command can be issued in the 3-dimensional coordinate conversion modal. However, if the geometric command is issued in the same block as in the 3-dimensional coordinate conversion command (G68, G69), "the program error (P32) will occur. (13) Init const sur spd When the 3-dimensional coordinate conversion command is issued while the parameter initial constant surface speed is valid, the program error (P922) will occur. This is the same consequence as in the case where the 3dimensional coordinate conversion command is issued in the constant surface speed (G96) modal. (14) Machine lock The machine lock in the 3-dimensional coordinate conversion modal will be valid for the movement axis for the coordinate value after executing the 3-dimensional coordinate conversion. (15) Interlock The interlock in the 3-dimensional coordinate conversion modal will be valid for the movement axis for the coordinate value after executing the 3-dimensional coordinate conversion. (16) Coordinate read variable When reading the workpiece coordinate system/skip coordinate system during the 3-dimensional coordinate conversion modal, local coordinate system and G68 program coordinate system can be switched with the parameter "#1563 3Dcdrc". (17) Workpiece coordinate display Whether to display the workpiece coordinate system position in the 3-dimensional coordinate conversion modal, in the workpiece coordinate system or in the G68 program coordinate system can be switched with the parameter "#1561 3Dcdc". In the same manner, absolute value can be displayed on the special display. <Note> 1um of display deviation may occur during the 3-dimensional coordinate conversion; however, this is normal. (18) Remaining command display Whether to display the remaining commands in the 3-dimensional coordinate conversion modal, in the workpiece coordinate system or in the G68 program coordinate system can be switched with the parameter "#1562 3Dremc". <Note> 1um of display deviation may occur during the 3-dimensional coordinate conversion; however, this is normal. (19) Graphic check Linear tracing is applied to circular interpolation (including corner R) during 3-dimensional coordinate conversion in graphic check mode. (20) Manual operation in G68 program coordinate system Refer to "Manual Operation in G68 Program Coordinate System" in Detailed description. (21) Others G41, G42, and the fixed cycle commands G73 to G89 have to be nested inside the G68/G69 commands. For the block next to G68, a movement command in the G90 (Absolute value command) mode has to be issued. (Example) G68 X50. Y100. Z150. I1 J0 K0 R60. ; G90 G00 X0 Y0 Z0 ; G41 D01 ; G40 ; G69 ; G00 command during 3-dimensional coordinate conversion modal is the interpolation type regardless of settings of the basic parameter "#1086 G0Intp (G00 non-interpolation)" Origin zero cannot be executed during the 3-dimensional coordinate conversion modal. When in a G68/G69 block during tool compensation, the program position counter indicates a position shifted by the tool length offset. IB-1501278-D 792 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Relation with other G codes Pxxx in the list indicates the program error Nos. Column A: Operation to be carried out when the G command in the list is issued during 3-dimensional coordinate conversion Column B: Operation to be carried out when 3-dimensional coordinate conversion is commanded while the G command modal in the list is established Column C: Operation to be carried out when the G command in the list and 3-dimensional coordinate conversion are commanded for the same block G command Function A B C G00 Positioning ○ ○ P923 G01 Linear interpolation ○ ○ P923 G02 Circular interpolation CW ○ ○ P923 Helical interpolation CW P921 P922 P923 G03 Circular interpolation CCW ○ ○ P923 Helical interpolation CCW P921 P922 P923 G02.3 Exponential interpolation CW P921 P922 P923 G02.4 3-dimensional circular in- P921 terpolation CW P922 P923 G03.3 Exponential interpolation CCW P921 P922 P923 G03.4 3-dimensional circular in- P921 terpolation CCW P922 P923 G04 Dwell ○ - G04 valid, G68 ignored G05 P0 High-speed machining mode cancel ○ - P923 G05 P1,2 High-speed machining mode I, II P34 P34 P923 G05 P10000 High-speed high-accura- P34 cy control II P34 P923 G05.1 Q0 High-speed machining ○ mode/High-speed highaccuracy control cancel ○ P923 G05.1 Q1 High-speed high-accura- ○ cy control I ○ P923 G05.1 Q2 Fine spline P34 P34 P923 G07.1/ G107 Cylindrical interpolation P921 P481 P923 G09 Exact stop check ○ - P923 G10 Parameter input by pro- ○ gram P421 P923 Program tool compensa- ○ tion input - G10 valid, G68 ignored G11 Parameter input by pro- ○ gram cancel - P923 G12 Circular cutting CW - P923 G12.1 Polar coordinate interpo- P921 lation P481 P923 G13 Circular cutting CCW ○ - P923 G13.1 Polar coordinate interpo- ○ lation cancel - P923 ○ 793 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions G command Function A B C G15 Polar coordinate command cancel ○ - P923 G16 Polar coordinate command ○ ○ P923 G17 Plane selection X-Y ○ ○ ○ G18 Plane selection Z-X ○ ○ ○ G19 Plane selection Y-Z ○ ○ ○ G20 Inch command ○ ○ ○ G21 Metric command ○ ○ ○ G27 Reference position check ○ - G27 valid, G68 ignored G28 Reference position return ○ - G28 valid, G68 ignored G29 Start position return ○ - G29 valid, G68 ignored G30 2nd to 4th reference po- ○ sition return - G30 valid, G68 ignored G30.1 Tool change position re- ○ turn 1 - G30.1 valid, G68 ignored G30.2 Tool change position re- ○ turn 2 - G30.2 valid, G68 ignored G30.3 Tool change position re- ○ turn 3 - G30.3 valid, G68 ignored G30.4 Tool change position re- ○ turn 4 - G30.4 valid, G68 ignored G30.5 Tool change position re- ○ turn 5 - G30.5 valid, G68 ignored G30.6 Tool change position re- ○ turn 6 - G30.6 valid, G68 ignored G31 Skip ○ - P923 G31.1 Multi-step skip 1 ○ - P923 G31.2 Multi-step skip 2 ○ - P923 G31.3 Multi-step skip 3 ○ - P923 G33 Thread cutting P921 P922 P923 G34 Special fixed cycle (bolt hole circle) ○ - P923 G35 Special fixed cycle (line at angle) ○ - P923 G36 Special fixed cycle (arc) ○ - P923 G37.1 Special fixed cycle (grid) ○ - P923 G37 Automatic tool length measurement - G37 valid, G68 ignored G38 Tool radius compensa- ○ tion (vector designation) - P923 G39 Tool radius compensation (corner arc) ○ - P923 G40 Tool radius compensation cancel ○ - ○ G41 Tool radius compensation ○ P922 P923 3-dimensional tool radius ○ compensation P922 P923 IB-1501278-D P921 794 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions G command G42 Function Tool radius compensation A B C ○ P922 P923 3-dimensional tool radius ○ compensation P922 P923 G40.1/ G150 Normal line control can- P921 cel - P923 G41.1/ G151 Normal line control Left P921 P922 P923 G42.1/ G152 Normal line control Right P921 P922 P923 G43 Tool length compensation (+) ○ ○ P923 G44 Tool length compensation (-) ○ ○ P923 G45 Tool position compensa- ○ tion increase - P923 G46 Tool position compensa- ○ tion decrease - P923 G47 Tool position compensa- ○ tion 2-fold increase - P923 G48 Tool position compensa- ○ tion 2-fold decrease - P923 G49 Tool length compensation cancel ○ - P923 G43.1 Tool length compensation along the tool axis P927 P931 P923 G43.4 Tool center point control P941 type1 ON P922 P923 G43.5 Tool center point control P941 type2 ON P922 P923 G50 Scaling cancel P921 - P923 G51 Scaling ON P921 ○ P923 G50.1 Mirror image cancel ○ - P923 G51.1 Mirror image ON ○ ○ P923 G52 Local coordinate system P921 setting - G52 valid, G68 ignored G53 Machine coordinate sys- ○ tem setting - G53 valid, G68 ignored G54 Workpiece coordinate system 1 selection P921 ○ P923 G55 Workpiece coordinate system 2 selection P921 ○ P923 G56 Workpiece coordinate system 3 selection P921 ○ P923 G57 Workpiece coordinate system 4 selection P921 ○ P923 G58 Workpiece coordinate system 5 selection P921 ○ P923 G59 Workpiece coordinate system 6 selection P921 ○ P923 G54.1 Extended workpiece co- P921 ordinate system selection ○ P923 795 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions G command G60 Function A B C Unidirectional positioning P921 - G60 valid, G68 ignored Unidirectional positioning P921 (Modal designation) P922 P923 G61 Exact stop check mode ○ ○ P923 G61.1 High-accuracy control ○ ○ P923 G62 Automatic corner override ○ ○ P923 G63 Tapping mode P921 P922 P923 G64 Cutting mode ○ ○ ○ G65 User macro simple call ○ - Update modal only (Coordinate rotation by program) G66 User macro Modal call A ○ ○ Update modal only (Coordinate rotation by program) G66.1 User macro modal call B ○ Update modal only (Coordinate rotation by program) Update modal only (Coordinate rotation by program) G67 User macro modal call cancel ○ ○ Update modal only after macro (Coordinate rotation by program) G68 Coordinate rotation by program ON P921 P922 - 3-dimensional coordinate conversion ON ○ ○ - Coordinate rotation by program cancel ○ (3-dimensional co- ordinate conversion cancel) - 3-dimensional coordinate conversion cancel ○ - - G73 Fixed cycle (step) ○ P922 P923 G74 Fixed cycle (reverse tap- ○ ping) (including synchronous tapping) P922 P923 G76 Fixed cycle (fine boring) ○ P922 P923 G80 Fixed cycle cancel ○ - P923 G81 Fixed cycle (drill/spot drill) ○ P922 P923 G82 Fixed cycle (drill/counter boring) ○ P922 P923 G83 Fixed cycle (deep drilling) ○ P922 P923 G84 Fixed cycle (tapping) (including synchronous tapping) ○ P922 P923 G85 Fixed cycle (boring) ○ P922 P923 G86 Fixed cycle (boring) ○ P922 P923 G87 Fixed cycle (back boring) ○ P922 P923 G88 Fixed cycle (boring) ○ P922 P923 G89 Fixed cycle (boring) ○ P922 P923 G90 Absolute value command ○ ○ ○ G69 IB-1501278-D 796 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions G command Function A B C G91 Incremental value com- ○ mand ○ ○ G92 Coordinate system setting - P923 G94 Asynchronous feed (feed ○ per minute ) ○ ○ G95 Synchronous feed (feed ○ per revolution) ○ ○ G96 Constant surface speed P921 control ON P922 P923 G97 Constant surface speed P921 control OFF - P923 G98 Fixed cycle (Initial level return) ○ ○ ○ G99 Fixed cycle (R point level return) ○ ○ ○ P921 Note (1) None of the G codes not listed above can be used. 797 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Precautions Precautions related to arc command If the first command after the 3-dimensional coordinate conversion command is an arc shape, and the center of the arc did not change before and after the 3-dimensional coordinate conversion, an arc is drawn. However, an error will occur in the following cases: (1) For the arc in which the arc center is specified with I and J, if the center coordinate has deviated by 3-dimensional coordinate conversion, a program error (P70 Major arc end position deviation) will occur. G90 G28 X0 Y0 Z0 ; F3000 G17 ; G68 X100. Y0. Z0. I0 J0 K1 R0. ; G02 X100. I50. ; Y Y Y' (Err.) (a) (E) (X50, Y0) (C) X (X100, Y0) (a) X X' (X'50, Y'0) (C) (X'100, Y'0) No 3-dimensional coordinate conversion (a) Arc center (C) Current position (E) (X100, Y0) In 3-dimensional coordinate conversion (E) End point (Err.) Program error (2) For the arc in which the arc radius is specified with R, if the center coordinate has deviated by 3-dimensional coordinate conversion, a program error (P71 Arc center calculation disabled) will occur. G90 G28 X0 Y0 Z0 ; F3000 G17 ; G68 X100. Y0. Z0. I0 J0 K1 R0. ; G02 X100. R50. ; Y Y Y' (r) = 50 (r) X (C) 50 (E) (X100, Y0) (C) (X100, Y0) (E) (X'100, Y'0) (Err.) No 3-dimensional coordinate conversion (a) Arc center IB-1501278-D In 3-dimensional coordinate conversion (C) Current position (E) End point 798 (r) Radius (Err.) Program error X X' M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.9 Coordinate Rotation by Program ; G68/G69 Function and purpose When machining a complicated shape located in a rotated position in respect to the coordinate system, this function enables to machine the rotated shape with the program for the shape before rotation on the local coordinate system and with the rotation angle designated by the program coordinate rotation command. Command format Coordinate rotation ON G68 X__ Y__ R__; X,Y Rotation center coordinates Two axes (X, Y or Z) corresponding to the selected plane are designated with absolute positions. R Rotation angle The counterclockwise direction is +. Coordinate rotation cancel G69; Select the command plane with G17 to G19. Y r1 (x1,y1) y1 Y' X' x1 W X W' W : Original local coordinate W' : Rotated local coordinate system r1 : Rotation angle (x1, y1) Rotation center 799 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Detailed description (1) Always command the rotation center coordinate (x1, y1) with an absolute value. Even if commanded with an incremental address, it will not be handled as an incremental value. The rotation angle "r1" depends on the G90/ G91 modal. (2) If the rotation center coordinates (x1, y1) are omitted, the position where the G68 command was executed will be the rotation center. (3) The rotation takes place in the counterclockwise direction by the angle designated in rotation angle r1. (4) The rotation angle r1 setting range is -360.000 to 360.000. If a command exceeding 360 degrees is issued, the remainder divided by 360 degrees will be the command. (5) Since the rotation angle "r1" is modal data, if once commanded, it will not be changed until the new angle is commanded. Thus, the command of rotation angle "r1" can be omitted. If the rotation angle is omitted in spite that G68 is commanded for the first time, "r1" will be regarded as “0”. (6) The program coordinate rotation is a function used on the local coordinate system. The relationship of the rotated coordinate system, workpiece coordinate system and basic machine coordinate system is shown below. (R) Rotation angle (L) (R) (L) (x1,y1)=(0,0) Local coordinate system (W) Workpiece coordinate system (M) Basic machine coordinate system (W) (M) (7) The coordinate rotation command during coordinate rotation is processed as the changes of center coordinates and rotation angle. (8) If M02 or M30 is commanded or the reset signal is input during the coordinate rotation mode, the coordinate rotation mode will be canceled. (9) G68 is displayed on the modal information screen during the coordinate rotation mode. When the mode is canceled, the display changes to G69. (The modal value is not displayed for the rotation angle command R.) (10) The program coordinate rotation function is valid only in the automatic operation mode. IB-1501278-D 800 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Program example Program coordinate rotation by absolute command N01 G28 X0. Y0.; X' N02 G54 G52 X200. Y100. ; Local coordinate designation Y' N03 T10 ; N04 G68 X-100. Y0. R60. ; Coordinate rotation ON Y N05 M98 H101 ; Subprogram execution N06 G69 ; Coordinate rotation cancel N07 G54 G52 X0 Y0 ; Local coordinate system cancel N08 M02 ; End Subprogram (Shape programmed with original coordinate system) 60 (a) 100. (W) - 100. N104 N103 X - 100. 100. 200. N101 N102 (b) N101 G00 X-100. Y-40.; N102 G83 X-150. R-20. Q-10.F100 ; N103 G00 Y40. ; N104 G83 X-150. R-20. Q-10.F100 ; N105 M99 - 100. (a) Actual machining shape (b) Program coordinate (W) Local coordinates (before rotation) 801 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Operation when only one axis was commanded by the first movement command Command basically two axes in the rotation plane by an absolute value immediately after the coordinate rotation command. When commanding one axis only, the following two kinds of operations can be selected by the parameter "#19003 PRG coord rot type". (1) When "#19003 PRG coord rot type" is "1", the operation is the same as when "N04" is "X50.Y0.". The end point is calculated on the assumption that the start point rotates along with the coordinates' rotation. N01 G17 G28 X0. Y0.; N03 G68 X40. Y0. R90.; X’ Y N02 G90 G92 G53 X0. Y0.; Coordinate rotation ON N04 X50.; Y=10 N05 (X’,Y’)=(50,50) X= -10 (X’,Y’)=(40,40) N05 Y50.; N06 G69 ; Coordinate rotation cancel N07 M02 ; End X’ =50 N04 (a) X (W) (b) (W1) Y’ Y’ =50 (S) (X’ ,Y’)=(0,0) (S) Start point Machine movement path (a) Center of rotation (b) The start point is rotated virtually (W) Local coordinate system before rotation (W1) Local coordinate system after rotation (2) When "#19003 PRG coord rot type" is "0", only axis commanded in N04 (X' Axis) is moved. The start point does not rotate along with the coordinate rotation; therefore the end position is calculated based on the current position on the local coordinate system before rotation. N01 G17 G28 X0. Y0.; Y N02 G90 G92 G53 X0. Y0.; N03 G68 X40. Y0. R90.; Coordinate rotation ON (X’,Y’)=(50,50) N05 N04 X50.; X= -10 N05 Y50.; N06 G69 ; N07 M02 ; Coordinate rotation cancel End X' Y=10 N04 (W) X' =50 (a) X (S) (X̉,Ỷ)=(40,40) (W1) Y' Y'=50 (X',Y')=(0,0) (S) Start point Machine movement path IB-1501278-D (a) Center of rotation (b) The start point is rotated virtually (W) Local coordinate system before rotation (W1) Local coordinate system after rotation 802 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Local coordinate designation during program coordinate rotation (1) When "#19003 PRG coord rot type" is "0", the position commanded on the rotated coordinate system is set as the local coordinate zero point. (2) When "#19003 PRG coord rot type" is "1", the position commanded on the coordinate system before it is rotated, is set as the local coordinate zero point and the local coordinate will be rotated. N01 G17 G28 X0. Y0.; N02 G90 G92 G53 X0. Y0.; N03 G68 X20. Y0. R90.; Coordinate rotation ON N04 G52 X10. Y10.; Local coordinate setting N05 X20.; N06 Y10.; N07 G69 ; Coordinate rotation cancel W: Workpiece coordinate system N08 M02 ; End L : Local coordinate system (1) Operation of #19003 = 0 (2) Operation of #19003 = 1 N03 X' Y Y,Y' X X=20 (Workpiece coordinate system is rotated virtually.) Y' (Rotation center) (Workpiece coordinate systm after rotation) W Y=-20 X,X' W,W ' W' Workpiece coordinate system is rotated virtually. Workpiece coordinate system is not rotated. N04 Y Y,Y' X' X" X=30 Y" W Y=-10 Y' (X,Y)=(0,0) X" (Local coordinate designation) X LX=30 W,W' L X,X' Y= -10 Y" (X,Y)=(10,10) (Rotation center) (Local coordinate designation) The workpiece coordinate zero point after rotation Designate the local coordinate system on the is considered as (X,Y)=(0,0). The position after workpiece coordinate system. shifted by 10 each in the X and Y directions is set as the local coordinate zero point. The direction of the shift is not the direction of X' and Y'. N05 (X",Y")=(20,30) Start point:(X",Y")=(10,30) Y Y=10 Y Y=10 (X",Y")=(10,30) X" Y" L (X",Y")=(20,-10) X X=40 W X W (Rotation center) X" Y" L (The start point is rotated virtually.) Start point: (X",Y")=(-10,-10) The commanded axis moves on the rotation coor- The commanded axis moves on the rotation coordinate system. dinate system. Axis without movement command does not move. Axis without movement command moves to the position on rotation coordinate system. N06 (X",Y")=(20,30) Y Y=10 X" (X",Y")=(20,10) Y X=30 X=20 X W Y" (X" ,Y" )=(20,10) X" Y=10 (X" ,Y" )=(20, - 10) X=40 X W L Y" 803 L IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Coordinate system designation during program coordinate rotation When the coordinate system setting (G92) is executed during program coordinate rotation (G68), this program operates same as "Local coordinate designation during program coordinate rotation". (1) When "#19003 PRG coord rot type" is "0", the position is preset to the current position commanded on the rotated coordinate system. (Ex.) Designation on the coordinate system (X'-Y') after rotation Y Y Y' Y' G68 X0 Y0 R30. G00 X10. Y10. G92 X0. Y0. X' (a) X' (b) 10. 10. (c) 10. X G54(0, 0) (a) Position after rotation 10. X G54(0, 0) (b) Commanded position (c) G92 shift amount (2) When "#19003 PRG coord rot type" is "1", the position is preset to the current position commanded on the coordinate system before rotation. The coordinate system is rotated after the position is commanded. (Ex.) Setting on the coordinate system (X-Y) after rotation Y Y Y' Y' G68 X0 Y0 R30. G00 X10. Y10. G92 X0. Y0. X' (a) X' (b) 10. 10. (c) 10. G54(0, 0) (a) Position after rotation X G54(0, 0) (b) Commanded position 10. X (c) G92 shift amount <Note> When "#19003 PRG coord rot type" is "1"and the coordinate system setting (G92) is executed during coordinate rotation mode, the rotation center of the program coordinate rotation is not shifted. (It stays at the same position in respect to the basic machine coordinate system.) IB-1501278-D 804 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Relationship with Other Functions (1) Program error (P111) will occur if the plane selection code is commanded during the coordinate rotation mode. (2) Program error (P485) will occur if polar coordinate interpolation is commanded during the coordinate rotation mode. (3) Program error (P481) will occur if coordinate rotation is commanded during the polar coordinate interpolation mode. (4) Program error (P485) will occur if cylindrical interpolation is commanded during the coordinate rotation mode. (5) Program error (P481) will occur if coordinate rotation is commanded during the cylindrical interpolation mode. (6) Program error (P34) will occur if the workpiece coordinate system preset (G92.1) is commanded during the coordinate rotation mode. (7) Program error (P34) will occur if high-accuracy control mode, high-speed machining mode, high-speed high-accuracy I or II is commanded during the coordinate rotation mode. (8) Program coordinate rotation and figure rotation cannot be carried out simultaneously. If the coordinate rotation is commanded during the figure rotation and vice versa, a program error (P252) will occur. (9) If the tool position offset is commanded during the coordinate rotation mode, a program error (P141) will occur. Precautions (1) Always command an absolute value for the movement command immediately after G68 and G69. (2) If the manual absolute is ON and interrupted the coordinate rotary axis, then, do not use automatic operation for the following absolute value command. (3) The intermediate point during reference position return is the position after the coordinates are rotated. (4) If the workpiece coordinate system offset amount is changed during the coordinate rotation mode, the rotation center for the program coordinate rotation will be shifted. (The center will follow the coordinate system.) (5) If the workpiece coordinates are changed during the coordinate rotation mode (ex. from G54 to G55), the rotation center of the program coordinate rotation will be the position on the coordinate system which the command was issued. (It stays at the same position in respect to the basic machine coordinate system.) (6) If coordinate rotation is executed to the G00 command for only one axis, two axes will move. If G00 non-interpolation (parameter "#1086 G0Intp" = 1) is set, each axis will move independently at the respective rapid traverse rates. If the axis must be moved linearly (interpolated) from the start point to the end point (such as during the hole machining cycle), always turn G00 non-interpolation OFF (parameter "#1086 G0Intp" = 0). The feedrate in this case is the composite speed of each axis' rapid traverse rate, so the movement speed will be faster than when moving only one axis (before coordinate rotation). (7) If the coordinate rotation specifications are not provided, a program error (P260) will occur when coordinate rotation is commanded. (8) The compensation during the coordinate rotation mode is carried out to the local coordinate system after coordinate rotation. The compensation direction is the coordinate system before rotation. (9) Mirror image during the coordinate rotation mode is applied to the local coordinate system after coordinate rotation. (10) On the display, the positions after rotation is always displayed on the local coordinate system before rotation. (11) When the coordinate value variables are read, the positions are all on the coordinate system before rotation. (12) The coordinates can also be rotated for the parallel axis. Select the plane that contains the parallel axis before issuing the G68 command. The plane cannot be selected in the same block as the G68 command. (13) The coordinates can be rotated for the rotary axis. The angle will be interpreted as the length when rotating. 805 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.10 Coordinate Rotation Input by Parameter ; G10 I_ J_/K_ Function and purpose If a deviation occurs between the workpiece alignment line and machine coordinate system's coordinate axis when the workpiece is mounted, the machine can be controlled by rotating the machining program coordinates according to the workpiece alignment line deviation. The coordinate rotation amount is set with the parameters. The parameters can also be set with the G10 command. Ym G57 G56 (a) W4' ǰ(b) W3' W2 W1 G55 W2' G54 M W1' Xm (a) Center of rotation (b) Rotation angle To enable this function, the following conditions must be satisfied: (1) The parameter "#8116 CoordRotPara invd" is set to "0". (2) The parameter "#8627 Coord rot angle" is set. Alternatively, "#8625 Coord rot vctr(H)" and "#8626 Coord rot vctr(V)" are set. IB-1501278-D 806 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Command format G10 I__ J__ ; G10 K__ ; I Horizontal vector. Command a value corresponding to the parameter "#8625 Coord rot vctr(H)". Command range: -99999.999 to 99999.999 The value of "#8627 Coord rot angle" is automatically calculated when commanding vector contents. J Vertical vector. Command a value corresponding to the parameter "#8626 Coord rot vctr(V)". Command range: -99999.999 to 99999.999 The value of "#8627 Coord rot angle" is automatically calculated when commanding vector contents. K Rotation angle Command a value corresponding to the parameter "#8627 Coord rot angle". Command range: -360.000 to 360.000 "#8625 Coord rot vctr(H)" and "#8626 Coord rot vctr(V)" are set to "0" when commanding the coordinate rotation angle. Parameters specified in the parameter setting screen can be changed from the machining program. Refer to the Instruction Manual for settings and contents of the parameters. 807 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Detailed description (1) As for the coordinate rotation center position, designate the position on the machine coordinate system. (2) All workpiece coordinate systems from G54 to G59, G54.1 rotate with the rotation command. While the machine coordinate system does not rotate, it can be understood that there is a hypothetical machine coordinate system in the coordinate system after rotation. (3) When parameter settings are configured, their setting values become valid at the following timings. Automatic operation: The setting values become valid from the next block after parameter settings have been configured. Manual operation: The setting values become valid if the PLC signal (manual feed coordinate switching for coordinate rotation by parameter) is set to ON after parameter settings have been configured. Concept of coordinate system (1) Set the parameters "#8623 Coord rot centr(H)" and "#8624 Coord rot centr(V)" at the position of the machine coordinate system. (2) The workpiece coordinate system set on the orthogonal coordinate system rotates around the rotation center. (3) The machine coordinate system does not rotate. G54 G55 Workpiece coordinate zero point G92 (Coordinate system shift) #8624 Rotation center EXT (External workpiece coordinate offset) #8623 Basic machine coordinate zero point Workpiece coordinate system setting Workpiece coordinate system after coordinate rotation by parameter Coordinate rotation start The coordinate rotation starts when the following parameters are changed. (When the same value is reset to the parameter, it is not considered as change) When the parameter "#8116 CoordRotPara invd" is "1" or the parameter "#8627 coordinate rotation angle" is "0", coordinate rotation will not start. #8621 Coord rot plane(H) #8622 Coord rot plane(V) #8623 Coord rot centr(H) #8624 Coord rot centr(V) #8625 Coord rot vctr(H) #8626 Coord rot vctr(V) #8627 Coord rot angle #8116 CoordRotPara invd (*1) (*1) The parameter "#8116 CoordRotPara invd" is common to all part systems. Therefore, before designating this parameter, set "0" to the parameter "#8627 Coord rot angle" in part systems in which "coordinate rotation by parameter" is not used. IB-1501278-D 808 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Coordinate rotation stop (cancel) When coordinate rotation is enabled, setting the parameter "#8116 CoordRotPara invd" to "1" or "#8627 Coord rot angle" to "0", and then issuing the following movement command cancels the parameter coordinate rotation. Coordinate rotation temporary cancel The coordinate rotation by parameter is temporarily canceled when in (1) or (2) as follows. (1) Reference position return command (G28, G30) If reference position return is performed on any of the axes in the rotated coordinate system (horizontal axis or vertical axis), both of the two axes will temporarily cancel the coordinate rotation. However moving to the intermediate point will not be temporarily canceled, but it will keep operating. (2) Basic machine coordinate system selection (G53) Only the commanded axis of basic machine coordinate system selection (G53) will be temporarily cancel the coordinate rotation. In items (1) and (2) above, when the coordinate rotation by parameter is canceled temporarily, the counter display follows the setting of the parameter "#11086 PRM coordinate rotation counter". 809 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Operation example First movement command after coordinate rotation start/end/temporary cancel When issuing a movement command for the first time after coordinate rotation has been started, ended, reset, or returned from temporary cancel, issue the command in G00 or G01 mode by designating the two axes configuring the rotation plane using absolute values. [Parameters] [Machining program] #8621 Coord rot plane(H) = X N01 G17 G28 X0. Y0.; #8622 Coord rot plane(V) = Y N02 G54 G90 X0. Y0.; #8623 Coord rot centr(H) = 30.0 N03 G10 K90.; (Coordinate rotation start) #8624 Coord rot centr(V) = 60.0 N04 G54 G90 G00 X20. Y10.;(Absolute value com#8627 Coord rot angle = 0.0 mand to two axes) [G54 workpiece coordinate system offset] : X = 10.0 Y = 10.0 <0 I D ;: <: ;0<0 ;0<0 : ;: G : <: <: H F ;: <: ;: 0 E ;:<: ;0 (W): Workpiece coordinate system before rotation (W1): Workpiece coordinate system after rotation (a): Rotation center (b): Actual axis position (c): Workpiece coordinate system zero point after coordinate rotation (d): N04 Commanded path (e): N04 Actual movement path (f): N04 End point Note that, if the command that is issued for the first time after coordinate rotation has been started, ended, or returned from temporary cancel is any of the following, the operation differs depending on the setting of the parameter "#19008 PRM coord rot type". (1) Command to an axis configuring the rotation plane by the absolute value (2) Command by incremental value (3) Circular interpolation command IB-1501278-D 810 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Operation when an axis configuring the rotation plane is commanded by the absolute value The operation can be selected from the following 2 types by setting of the parameter "#19008 PRM coord rot type". (1) When the parameter "#19008 PRM coord rot type" is "0". The end point is calculated by virtually rotating the start point along with the coordinate rotation. For that reason, the operation is the same as when "N04" is "G00 X20. Y0." in the following example. [Parameters] [Machining program] #8621 Coord rot plane(H) = X N01 G17 G28 X0. Y0.; #8622 Coord rot plane(V) = Y N02 G54 G90 X0. Y0.; #8623 Coord rot centr(H) = 30.0 N03 G10 K90.; (Coordinate rotation start) #8624 Coord rot centr(V) = 60.0 N04 G54 G90 G00 X20.; (Absolute value command #8627 Coord rot angle = 0.0 to an axis) [G54 workpiece coordinate system offset] : X = 10.0 Y = 10.0 <0 I D ;: <: ;0<0 ;0<0 : ;: : G <: <: H F ;: <: ;: 0 E ;:<: ;0 (W): Workpiece coordinate system before rotation (W1): Workpiece coordinate system after rotation (a): Rotation center (b): Actual axis position (c): Start point rotated virtually along with the coordinate rotation (d): N04 Commanded path (e): N04 Actual movement path (f): N04 End point 811 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (2) When the parameter "#19008 PRM coord rot type" is "1". The start point does not rotate along with the coordinate rotation; therefore the end point position is calculated based on the current position on the local coordinate system before rotation. For that reason, only the axis commanded in N04 (X' axis) is moved. [Parameters] [Machining program] #8621 Coord rot plane(H) = X N01 G17 G28 X0. Y0.; #8622 Coord rot plane(V) = Y N02 G54 G90 X0. Y0.; #8623 Coord rot centr(H) = 30.0 N03 G10 K90.; (Coordinate rotation start) #8624 Coord rot centr(V) = 60.0 N04 G54 G90 G00 X20.; (Absolute value command #8627 Coord rot angle = 0.0 to an axis) [G54 workpiece coordinate system offset] : X = 10.0 Y = 10.0 <0 I ;: <: ;0<0 D ;0<0 : ;: : <: G H ;: 0 E ;:<: ;0 (W): Workpiece coordinate system before rotation (W1): Workpiece coordinate system after rotation (a): Rotation center (b): The actual axis position and start point position are the same (d): N04 Commanded path (e): N04 Actual movement path (f): N04 End point IB-1501278-D 812 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Operation when incremental value commands are given The operation can be selected from the following 2 types by setting of the parameter "#19008 PRM coord rot type". (1) When the parameter "#19008 PRM coord rot type" is "0". The end point is calculated by virtually rotating the start point along with the coordinate rotation. For that reason, the commanded path and actual movement path differs in N04. [Parameters] [Machining program] #8621 Coord rot plane(H) = X N01 G17 G28 X0. Y0.; #8622 Coord rot plane(V) = Y N02 G54 G90 X0. Y0.; #8623 Coord rot centr(H) = 30.0 N03 G10 K90.; (Coordinate rotation start) #8624 Coord rot centr(V) = 60.0 N04 G54 G91 G00 X20. Y10.;(Incremental value #8627 Coord rot angle = 0.0 command to two axes) [G54 workpiece coordinate system offset] : X = 10.0 Y = 10.0 <0 I D ;: <: ;0<0 ;0<0 : ;: : G <: <: H F ;: <: ;: 0 E ;:<: ;0 (W): Workpiece coordinate system before rotation (W1): Workpiece coordinate system after rotation (a): Rotation center (b): Actual axis position (c): Start point rotated virtually along with the coordinate rotation (d): N04 Commanded path (e): N04 Actual movement path (f): N04 End point 813 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (2) When the parameter "#19008 PRM coord rot type" is "1". The start point does not rotate along with the coordinate rotation; therefore the end point position is calculated based on the current position on the local coordinate system before rotation. For that reason, the commanded path and actual movement path are the same in N04. [Parameters] [Machining program] #8621 Coord rot plane(H) = X N01 G17 G28 X0. Y0.; #8622 Coord rot plane(V) = Y N02 G54 G90 X0. Y0.; #8623 Coord rot centr(H) = 30.0 N03 G10 K90.; (Coordinate rotation start) #8624 Coord rot centr(V) = 60.0 N04 G54 G91 G00 X20. Y10.;(Incremental value #8627 Coord rot angle = 0.0 command to two axes) [G54 workpiece coordinate system offset] : X = 10.0 Y = 10.0 I <0 ;: <: D ;0<0 ;0<0 : ;: : <: <: G H ;: 0 E ;:<: ;0 (W): Workpiece coordinate system before rotation (W1): Workpiece coordinate system after rotation (a): Rotation center (b): The actual axis position and start point position are the same (d): N04 Commanded path (e): N04 Actual movement path (f): N04 End point IB-1501278-D 814 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Operation when circular interpolation is commanded The operation can be selected from the following 2 types by setting of the parameter "#19008 PRM coord rot type". (1) When the parameter "#19008 PRM coord rot type" is "0". The end point of an arc is calculated from the position to which the start point is virtually rotated along with the coordinate rotation. In this case, the start point of an arc is not rotating but the end point of an arc is rotating, so it may cause "P70: Arc end point deviation large" due to the difference in radius between the start and end points. [Parameters] [Machining program] #1084 Arc error = 0.1 N01 G17 G28 X0. Y0.; #8621 Coord rot plane(H) = X N02 G54 G90 X0. Y0.; #8622 Coord rot plane(V) = Y N03 G10 K90.; (Coordinate rotation #8623 Coord rot centr(H) = 30.0 start) #8624 Coord rot centr(V) = 60.0 N04 G54 G91 G03 X20. R10. F500;(Circular interpo#8627 Coord rot angle = 0.0 lation command) [G54 workpiece coordinate system offset] : X = 10.0 Y = 10.0 <0 D I ;0<0 ;: <: : ;0<0 ;: K G : <: <: J ;: 0 F ;: <: E ;:<: ;0 (W): Workpiece coordinate system before rotation (W1): Workpiece coordinate system after rotation (a): Rotation center (b): Actual axis position (c): Start point rotated virtually along with the coordinate rotation (d): N04 Commanded path (f): End point calculated from the virtually rotated start point (g): Start point radius (h): End point radius As the difference in radius between the start and end points is bigger than "#1084 RadErr", it causes program error (P70). 815 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (2) When the parameter "#19008 PRM coord rot type" is "1". The start point and end point of an arc are calculated from the current position on the workpiece coordinate system before the coordinate rotation and the circular interpolation is performed from the current position to the end point. [Parameters] [Machining program] #1084 Arc error = 0.1 N01 G17 G28 X0. Y0.; #8621 Coord rot plane(H) = X N02 G54 G90 X0. Y0.; #8622 Coord rot plane(V) = Y N03 G10 K90.; (Coordinate rotation #8623 Coord rot centr(H) = 30.0 start) #8624 Coord rot centr(V) = 60.0 N04 G54 G91 G03 X20. R10. F500;(Circular interpo#8627 Coord rot angle = 0.0 lation command) [G54 workpiece coordinate system offset] : X = 10.0 Y = 10.0 <0 D ;0<0 : ;: : I ;: <: ;0<0 <: <: G H ;: 0 E ;:<: ;0 (W): Workpiece coordinate system before rotation (W1): Workpiece coordinate system after rotation (a): Rotation center (b): The actual axis position and start point position are the same (d): N04 Commanded path (e): N04 Actual movement path (f): N04 End point IB-1501278-D 816 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions First movement command after coordinate rotation cancel When rotation angle "0" is commanded during coordinate rotation, it will be canceled by next movement command regardless of G90 and G91. The calculation of the end point will be different by setting of the parameter "#19008 PRM coord rot type". (1) When the parameter "#19008 PRM coord rot type" is "0". The end point is calculated on the assumption that the start point rotates along with the coordinate rotation cancel. Program the first movement command after coordinate rotation cancel either G00 or G01 mode. [Parameters] [Machining program] #8621 Coord rot plane(H) = X N01 G54 G90 X50.Y50.; #8622 Coord rot plane(V) = Y N02 G54 G90 X0. Y0.; #8623 Coord rot centr(H) = 30.0 N03 G10 K0.; (Coordinate rotation cancel) #8624 Coord rot centr(V) = 60.0 N04 G91 G00 X20. Y10.;(Incremental value com#8627 Coord rot angle = 90.0 mand to two axes) [G54 workpiece coordinate system offset] : X = 10.0 Y = 10.0 <0 I D ;:<: ;0<0 ;0<0 : ;: : <: <: H G ;: 0 F ;:<: E ;: <: ;0<0 ;0 (W): Workpiece coordinate system before rotation (W1): Workpiece coordinate system after rotation (a): Rotation center (b): Actual axis position (c): Start point rotated virtually along with the coordinate rotation cancel (d): N04 Commanded path (e): N04 Actual movement path (f): N04 End point 817 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (2) When the parameter "#19008 PRM coord rot type" is "1". The start point does not rotate along with the coordinate rotation cancel; therefore the end point position is calculated based on the current position on the local coordinate system before rotation. [Parameters] [Machining program] #8621 Coord rot plane(H) = X N01 G54 G90 X50.Y50.; #8622 Coord rot plane(V) = Y N02 G54 G90 X0. Y0.; #8623 Coord rot centr(H) = 30.0 N03 G10 K0.; (Coordinate rotation cancel) #8624 Coord rot centr(V) = 60.0 N04 G91 G00 X20. Y10.;(Incremental value com#8627 Coord rot angle = 90.0 mand to two axes) : [G54 workpiece coordinate system offset] X = 10.0 Y = 10.0 <0 : D ;0<0 I ;:<: ;0<0 ;: : G H <: <: ;: E ; : < : ; 0< 0 ;0 0 (W): Workpiece coordinate system before rotation (W1): Workpiece coordinate system after rotation (a): Rotation center (b): The actual axis position and start point position are the same (d): N04 Commanded path (e): N04 Actual movement path (f): N04 End point First movement command after temporary coordinate rotation cancel The operation of the first movement command issued after the program coordinate rotation is returned from temporary cancel is the same as the operation that occurs when the parameter "#19008 PRM coord rot type" is set to "0" in "First movement command after coordinate rotation". IB-1501278-D 818 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Presetting the workpiece coordinate and counter in the rotation coordinate system The workpiece coordinate and counter can be preset in the same way as for the orthogonal coordinate system by commanding G92/G92.1 in the rotation coordinate system. Figures (1) to (3) show the operations to be performed when the machining program is executed while the parameters and workpiece coordinate system offset are set as follows: [Parameters] [Machining program] #19008 PRM coord rot type = 0 (1) N01 G54 G17 G28 X Y; (Case where the start point is virtually rotated with the coN02 G90 G00 X0. Y0. ordinate rotation) N03 G10 K90. ; #8621 Coord rot plane(H) = X N04 G00 X0. Y0.; #8622 Coord rot plane(V) = Y N05 G00 X10. Y10.; #8623 Coord rot centr(H) = 20.0 (2) N06 G92 X0. Y0.; #8624 Coord rot centr(V) = 40.0 N07 G00 X10. Y10.; #8627 Coord rot angle = 0.0 (3) N08 G92.1 X0. Y0.; [G54 workpiece coordinate system offset] N09 G00 X0. Y0.; X = 10.0 N10 G00 X-10. Y10.; Y = 10.0 (1) (2) YM N04 (E) (XW',YW')=(10,10) (XM,YM)=N04 (E)(40,40) (a) (XM,YM)=(20,40) YM Xw’’ Xw ’ N07 G00 X10. Y10. N04 G00 X0. Y0. N06 (E) (XW'',YW'')=(10,10) (XM,YM)=(30,50) Xw ’ (XM,YM)=(40,40) N05 G00 X10. Y10. N06 G92 X0. Y0. YW’’ YW (XM,YM)=(50,30) Y ’ W YW’ (b) N02 G00 X0. Y0. (W) (XM,YM)=(50,30) N03 G10 K90. XW (W) (XM,YM)=(10,10) XM M M XM (3) Xw’’ YM Xw’ N09 G00 X0. Y0. (W) (XM,YM)=(40,40) YW’’ N08 G92.1 X0. Y0. YW’ (XM,YM)=(50,30) N10 G00 X-10. Y10. N09 (E) (XW'',YW'')=(-10,10) (XM,YM)=(40,20) M (W): Workpiece coordinate zero point (a): Rotation center (b): Axis position before coordinate rotation (E): End point ("N04 (E)" refers to the end point of the N04 block.) XM 819 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Program example (1) When used for compensating positional deviation of pallet changer. + Y G57 + G56 + + G55 (a) G54 M X (a) Rotation movement (15 degree) N01 G28 X0 Y0 Z0 ; N02 M98 P9000 ; Pallet deviation measurement N03 G90 G53 X0 Y0 ; Parallel movement amount shift N04 G92 X0 Y0 ; Parallel movement amount definition N05 G10 K15. ; Rotation amount definition N06 G90 G54 G00 X0 Y0 ; G54 workpiece machining N07 M98 H101 ; N08 G90 G55 G00 X0 Y0 ; G55 workpiece machining N09 M98 H101 ; N10 G90 G56 G00 X0 Y0 ; G56 workpiece machining N11 M98 H101 ; N12 G90 G57 G00 X0 Y0 ; G57 workpiece machining N13 M98 H101 ; N14 G27 X0 Y0 Z0 ; N15 M02 ; Machining shape program N101 G91 G01 G42 D01 F300 ; N102 X100 ; N103 G03 Y50. R25. ; N104 G01 X-100.; N105 G03 Y-50. R25. ; N106 G01 G40 ; N107 M99 ; IB-1501278-D 820 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Relationship with other functions (1) To use any of the following functions together with the coordinate rotation by parameter, start the coordinate rotation by parameter first and command the following function later. Tool radius compensation Mirror image (2) The coordinate rotation by parameter cannot be used together with the coordinate rotation by program and the 3-dimensional coordinate conversion. If they are used at the same time the coordinate position will not be calculated right. (3) The following high-speed high-accuracy processes are temporarily canceled during coordinate rotation by parameter. No program errors occur; however, the processing capacity is the same as when the high-speed high-accuracy processes are set off. High-speed machining mode I / high-speed machining mode II High-speed high-accuracy control I / High-speed high-accuracy control II / High-speed high-accuracy control III (4) If the figure rotation is commanded during the coordinate rotation by parameter, a program error (P252) will occur. (5) If the inclined surface machining command (G68.2/G68.3) is commanded during the coordinate rotation by parameter, a program error (P952) will occur. (6) The following functions can be used together with the coordinate rotation by parameter. Classification Control axes Function Number of basic control axes (NC axes) Memory mode Input command Inch/Metric changeover Positioning/Interpolation Positioning Linear interpolation Circular interpolation (Center/Radius designation) Feed Manual rapid traverse Jog feed Incremental feed Handle feed Manual feedrate B Manual speed clamp Dwell (Time-based designation) Tool compensation Tool length offset Tool position offset Tool radius compensation Tool radius compensation diameter designation Coordinate system Coordinate system setting Workpiece coordinate system selection External workpiece coordinate offset Workpiece coordinate system preset (G92.1) Plane selection Operation support functions Single block Graphic trace Manual interruption Automatic operation handle interruption Manual absolute switch Program support functions Subprogram control High-accuracy control (G61.1/G08) Multi-part system simultaneous high-accuracy control Machine support functions Custom API library 821 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Precautions (1) If rotation angle zero is commanded while carrying out coordinate rotation, it will be canceled at the next movement command regardless of the G90 or G91. (2) Command the first movement after this command with the G00 or G01 mode. If an arc command is issued, the arc start point will not be rotated. However, only the arc end point will rotate. This will cause the start point radius and end point radius to differ, and the program error (P70) will occur. (3) When data has been input using the data input/output function, it is recognized that the parameter "#8627 Coord rot angle" has been input, and automatic calculation from the values of "#8625 Coord rot vctr(H)" and "#8626 Coord rot vctr(V)" is not carried out. (4) Do not use this command with G54 to G59 and G90, G91. If used, the command will not be reflected correctly. (5) If both vertical / horizontal vectors (I,J) and rotation angle are commanded, the rotation angle will be given the priority. IB-1501278-D 822 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.11 Scaling ; G50/G51 Function and purpose By multiplying the moving axis command values within the range specified under this command by the factor, the shape commanded by the program can be enlarged or reduced to the desired size. Command format Scaling ON (set the common scaling factor to the three basic axes) G51 X__ Y__ Z__ P__ ; X,Y,Z Scaling center coordinates P Scaling factor Y y1 sc p1 s1 s3 s2 p2 p3 x1 X sc : Scaling center p1,p2,p3: Program shape s1,s2,s3: Shape after scaling Scaling ON (When setting the scaling factor to each of the three basic axes) G51 X__ Y__ Z__ I__ J__ K__ ; X,Y,Z Scaling center coordinates I Scaling factor of basic 1st axis J Scaling factor of basic 2nd axis K Scaling factor of basic 3rd axis Scaling cancel G50 ; 823 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Detailed description Specifying the scaling axis, scaling center and its factor Commanding G51 selects the scaling mode. The G51 command only specifies the scaling axis, its center and factor, and does not move the axis. Though the scaling mode is selected by the G51 command, the axis actually valid for scaling is the axis where the scaling center has been specified. (1) Scaling center - Specify the scaling center in accordance with the then absolute/incremental mode (G90/G91). - The scaling center must be specified also when the current position is defined as a center. - As described above, the axis valid for scaling is only the axis whose center has been specified. (2) Scaling factor - Use the address P or I, J, K to specify the scaling factor. - Minimum command unit : 0.000001 - Command range: Both -99999999 to 99999999 (-99.999999 to 99.999999 times) and -99.999999 to 99.999999 is valid, but the decimal point command is valid only after the G51 command. - When the factor is not specified in the same block as G51, the factor set with the parameter "#8072 SCALING P" is used. - When the address P and the address I, J, K are commanded in a same block, a factor specified by the address I, J, K is applied for the basic three axes. And a factor specified by the address P is applied for other axes. - If changed during the scaling mode, the value of this parameter will not become valid. Scaling is performed with the setting value that was used when G51 was commanded. - When the factor is not specified in either the program nor parameter, it is calculated as 1. (3) A program error will occur in the following cases. - Scaling was commanded though there was no scaling specification.(P350) - The upper limit of the factor command range was exceeded in the same block as G51.(P35) (When using the machining parameter scaling factor, the factor is calculated as 1, when -0.000001 < factor < 0.000001, or the factor is more than 99.999999 or less than -99.999999.) Scaling cancel When G50 is commanded, scaling is canceled. IB-1501278-D 824 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Program example (Example 1) Scaling center Y -200. -150. -100. N09 -50. X -50. N11 N03 -100. N08 N06 D01=25.000 N07 -150. Program path after 1/2 scaling Tool path after 1/2 scaling Program path when scaling is not applied Tool path when scaling is not applied <Program> N01 G92 X0 Y0 Z0 ; N02 G90 G51 X-100. Y-100. P0.5; N03 G00 G43 Z-200. H02; N04 G41 X-50. Y-50. D01; N05 G01 Z-250. F1000; N06 Y-150. F200; N07 X-150.; N08 G02 Y-50. J50.; N09 G01 X-50.; N10 G00 G49 Z0; N11 G40 G50 X0 Y0; N12 M02; 825 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Relationship with other functions (1) G27 reference position check command When G27 is commanded during scaling, scaling is canceled at completion of the command. (2) Reference position return command (G28, G29, G30) When the G28, G30 or reference position return command is issued during scaling, scaling is canceled at the intermediate point and the axis returns to the reference position. When the midpoint is to be ignored, the axis returns to the reference point directly. When G29 is commanded during scaling, scaling is applied to the movement after the midpoint. (3) G60 (unidirectional positioning) command If the G60 (unidirectional positioning) command is given during scaling, scaling is applied to the final positioning point and is not applied to the creep amount. Namely, the creep amount is uniform regardless of scaling. (4) Workpiece coordinate system switching When the workpiece coordinate system is switched during scaling, the scaling center is shifted by the difference between the offset amounts of the new and old workpiece coordinate systems. (5) During figure rotation When figure rotation is commanded during scaling, scaling is applied to the center of the figure rotation and the rotation radius. (6) Scaling command in figure rotation subprogram By commanding the scaling in the subprogram of the figure rotation, scaling can be applied only to the shape designated by the subprogram, not to the rotation radius of the figure rotation. (7) During coordinate rotation When scaling is commanded during coordinate rotation, the scaling center rotates. Scaling is executed at that rotated scaling center. (8) G51 command When the G51 command is issued during the scaling mode, the axis whose center was newly specified is also made valid for scaling. Also, the factor under the latest G51 command is made valid. Precautions (1) Scaling is not applied to the compensation amounts of tool radius compensation, tool position compensation, tool length compensation and the like. (Compensation is calculated for the shape after scaling.) (2) Scaling is valid for only the movement command in automatic operation. It is invalid for manual movement. (3) For X, Y and Z, scaling is valid for only the specified axes and is not applied to unspecified axes. (4) When an arc is commanded and scaling is valid for one of the two axes configuring the arc plane, a program error (P70) will occur. (5) When M02 or M30 is commanded, or when NC reset is carried out during the scaling mode, the mode switches to a cancel mode. (6) When the coordinate system is shifted (G92, G52 command) during scaling, the scaling center is also shifted by the difference amount. (7) If manual interruption is made during scaling, manual ABS selection is ignored for the movement followed by an incremental value command and operation performed is the same as in manual ABS OFF. IB-1501278-D 826 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.12 Reference Position (Zero Point) Return ; G28,G29 Function and purpose After the commanded axes have been positioned by G00, they are returned respectively at rapid traverse to the first reference position when G28 is commanded. By commanding G29, the axes are first positioned independently at high speed to the G28 or G30 intermediate point and then positioned by G00 to the commanded position. (R2) (0,0,0,0) (R1) (x 3 ,y 3 ,z 3 , 3 ) G30P2 G28 G28 G29 (x 1 ,y 1 ,z 1 , (S) 1 ) (CP) G30 G30P3 (x 2 ,y 2 ,z 2 , 2 G30P4 ) G29 (R3) (R4) (R1) 1st reference position (R2) 2nd reference position (R3) 3rd reference position (R4) 4th reference position (S) Start point (CP) Intermediate point Command format G28 Xx1 Yy1 Zz1 αα1; ... Automatic reference position return X, Y, Z, α Coordinate value of the intermediate point (α is an additional axis) G29 Xx2 Yy2 Zz2 αα2; ... Start point return X, Y, Z, α Coordinate value of the end point (α is an additional axis) 827 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Detailed description (1)The G28 command is equivalent to the following: G00 Xx1 Yy1 Zz1 α α1; G00 Xx3 Yy3 Zz3 α α3; where Xx3 Yy3 Zz3 α3 are the coordinate values of the reference position that are set in parameters "#2037 G53ofs" for the distance from the basic machine coordinate system zero point as specified by the MTB. (2)After the power has been switched on, the axes that have not been subject to manual reference position return are returned by the dog type of return just as with the manual type. In this case, the return direction is regarded as the command sign direction. If the return type is straight-type return, the return direction will not be checked. For the second and subsequence returns, the return is made at high speed to the reference (zero) position that was stored at the first time and the direction is not checked. (3)When reference position return is completed, the zero point arrival output signal is output and also #1 appears at the axis name line on the setting and display unit screen. (4)The G29 command is equivalent to the following: G00 Xx1 Yy1 Zz1 α α1; G00 Xx2 Yy2 Zz2 α α2; Rapid traverse (non-interpolation type) applies independently to each axis for the positioning from the reference position to the intermediate point. In this case, x1 y1 z1 and α1 are the coordinate value of the G28 or G30 intermediate point. (5)Program error (P430) occurs when G29 is executed without executing automatic reference position (zero point) return (G28) after the power has been turned ON. (6)When the Z axis is canceled, the movement of the Z axis to the intermediate point will be ignored, and only the position display for the following positioning will be executed. (The machine itself will not move.) (7)The intermediate point coordinates (x1, y1, z1, α1) of the positioning point are assigned by the position command modal. (G90, G91). (8)G29 is valid for either G28 or G30 but the commanded axes are positioned after a return has been made to the latest intermediate point. (9)The tool compensation will be canceled during reference position return unless it is already canceled, and the compensation amount will be cleared. (10)The intermediate point can be ignored by parameter "#1091 Ignore middle point" setting. (11)Control from the intermediate point to the reference position is ignored for reference position return in the machine lock status. When the designated axis reaches as far as the intermediate point, the next block will be executed. (12)Mirror image is valid from the start point to the intermediate point during reference position return in the mirror image mode and the tool will move in the opposite direction to that of the command. However, mirror image is ignored from the intermediate point to the reference position and the tool will move to the reference position. (13)When G28/G29/G30 is commanded in single block mode, if "#1279 ext15/bit6 Enable single block stop at middle point" is set to "1", single block stop at middle point will be performed; single block stop at middle point will not be performed if set to "0". (14)If the mode is switched to MDI mode or reference position return mode while in a single block stop at the intermediate point, an operation error (M01 0013) occurs. (15)If the NC is reset while in a single block stop at middle point, the intermediate point for G29 start position return will not be updated. (16) If a miscellaneous function is commanded in the same block, the miscellaneous function completion waiting point will be the end of commanded movement, instead of the intermediate point. (17) If the PLC interrupt operation is operated while in a single block stop at the intermediate point, an operation error (M01 0129) occurs. IB-1501278-D 828 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Program example (Example 1) G28 Xx1 Zz1 ; (R1) (F) G0Xx3Zz3; (R1) (CP) (x1,z1) G0Xx1Zz1; (S) 1st operation after power has been turned ON 2nd and subsequent operations Near-point dog (S) Return start position (CP) Intermediate point (R1) Reference position (#1) (F) Rapid traverse rate (Example 2) G29 Xx2, Zz2 ; R (C) (G00)Xx1 Zz1; (CP) (x1,z1) (G00)Xx2 Zz2; (x2,z2) (C) Current position (CP) G28, G30 Intermediate point 829 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (Example 3) G28 : : G30 : : G29 Xx1 Zz1 ; (From point A to 1st reference position) Xx2 Zz2 ; (From point B to 2nd reference position) Xx3 Zz3 ; (From point C to point D) (R1) A (CP2) (x2,z2) G30 G28 B G29 (CP1) (x1,z1) D (x3,z3) (R2) C IB-1501278-D (CP1) Old intermediate point (CP2) New intermediate point (R1) Reference position (#1) (R2) 2nd reference position (#2) 830 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.13 2nd, 3rd, and 4th Reference Position (Zero Point) Return ; G30 Function and purpose The tool can return to the second, third, or fourth reference position by specifying G30 P2 (P3 or P4). (R2) G30P2 G28 G28 G29 (x1,y1,z1, 1) (CP) (S) G30 G30P3 G30P4 G29 (R3) (R4) (S) Start point (CP) Intermediate point (R2) 2nd reference position (R3) 3rd reference position (R4) 4th reference position Command format G30 P2(P3,P4)Xx1 Yy1 Zz1 αα1; X, Y, Z, α Coordinate value of the intermediate point (α is an additional axis) P Reference position No. P2: 2nd reference position return P3: 3rd reference position return P4: 4th reference position return 831 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Detailed description (1)The 2nd, 3rd, or 4th reference position return is specified by P2, P3, or P4. A command without P or with other designation method will return the tool to the 2nd reference position. (2) In the 2nd, 3rd, or 4th reference position return mode, as in the 1st reference position return mode, the tool returns to the 2nd, 3rd, or 4th reference position via the intermediate point specified by G30. (3) The 2nd, 3rd, and 4th reference position coordinates refer to the positions specific to the machine, and these can be checked with the setting and display unit. (4) If G29 is commanded after completion of returning to the 2nd, 3rd, and 4th reference position, the intermediate position used last is used as the intermediate position for returning by G29. (R1) -X (CP) (x1,y1) G30 Xx1 Yy1; G29 Xx2 Yy2; (R2) (x2,y2) (CP) Intermediate point -Y (R1) 1st reference position (R2) 2nd reference position (5) With reference position return on a plane during compensation, the tool moves without tool radius compensation from the intermediate point as far as the reference position. With a subsequent G29 command, the tool move without tool radius compensation from the reference position to the intermediate point and it moves with such compensation until the G29 command from the intermediate point. (R2) -X (CP) (a) (b) G30 Xx1Yy1; (x1,y1) -Y G29 Xx2Yy2; (x2,y2) (a) Tool nose center path (b) Program path (CP) Intermediate point (R1) 1st reference position (R2) 2nd reference position IB-1501278-D 832 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions (6) The tool length compensation amount for the axis involved is canceled after the 2nd, 3rd and 4th reference position return. (7) With second, third and fourth reference position returns in the machine lock status, control from the intermediate point to the reference position will be ignored. When the designated axis reaches as far as the intermediate point, the next block will be executed. (8) With second, third and fourth reference position returns in the mirror image mode, mirror image will be valid from the start point to the intermediate point and the tool will move in the opposite direction to that of the command. However, mirror image is ignored from the intermediate point to the reference position and the tool moves to the reference position. (R2) -X (a) -Y G30 P2 Xx1Yy1; (b) (a) X-axis mirror image (b) No mirror image (R2) 2nd reference position (9) If the 2nd, 3rd or 4th reference position is changed while G30 zero point return operation is in pause due to an interlock, "M01 Operation Error" occurs. (10) When G28/G29/G30 is commanded in single block mode, if "#1279 ext15/bit6 Enable single block stop at middle point" is set to "1", single block stop at middle point will be performed; single block stop at middle point will not be performed if set to "0". (11) If the mode is switched to MDI mode or reference position return mode while in a single block stop at the intermediate point, an operation error (M01 0013) occurs. (12) If the NC is reset while in a single block stop at middle point, the intermediate point for G29 start position return will not be updated. (13) If a miscellaneous function is commanded in the same block, the miscellaneous function completion waiting point will be the end of commanded movement, instead of the intermediate point. (14) If the PLC interrupt operation is operated while in a single block stop at the intermediate point, an operation error (M01 0129) occurs. 833 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.14 Tool Change Position Return ; G30.1 - G30.6 Function and purpose By specifying the tool change position in a parameter "#8206 tool change" and also specifying a tool change position return command in a machining program, the tool can be changed at the most appropriate position. The axes that are going to return to the tool change position and the order in which the axes begin to return can be changed by commands. Command format Tool change position return G30.n ; n = 1 to 6 Specify the axes that return to the tool change position and the order in which they return. Detailed description Commands and return order are given below. Command Return order G30.1 Z axis -> X axis - Y axis (-> additional axis) G30.2 Z axis -> X axis -> Y axis (-> additional axis) G30.3 Z axis -> Y axis -> X axis (-> additional axis) G30.4 X axis -> Y axis - Z axis (-> additional axis) G30.5 Y axis -> X axis - Z axis (-> additional axis) G30.6 X axis - Y axis - Z axis (-> additional axis) <Note> An arrow ( ->) indicates the order of axes that begin to return. A hyphen ( - ) indicates that the axes begin to return simultaneously. (Example: "Z axis -> X axis - Y axis" indicates that the Z axis returns to the tool change position, then the X axis and Y axis do at the same time.) (1) Whether the tool exchange position return for the additional axis is enabled or disabled depends on the MTB specifications (parameter "#1092 Tchg_A"). For the order for returning to the tool change position, the axes return after the standard axis completes the return to the tool change position (refer to above table). The additional axis alone cannot return to the tool change position. (2) If the axis address is commanded in the same block as the tool change position return command, a program error (P33) will occur. (3) After all necessary tool change position return is completed by a G30.n command, tool change position return complete signal TCP (XC93) is turned ON. When an axis out of those having returned to the tool change position by a G30.n command leaves the tool change position, the TCP signal is turned OFF. With a G30.1 command, for example, the TCP signal is turned on when the Z axis has reached the tool change position after the X and Y axes have reached the tool change position (in addition, after the additional axis has reached the tool change position if additional axis tool change position return is valid). The TCP signal is then turned OFF when the X, Y, or Z axis leaves the position. If tool change position return for added axes is on with parameter "#1092 Tchg_A", the TCP signal is turned ON when the added axis or axes have reached the tool change position after the standard axes did. It is then turned OFF when one of the X, Y, Z, and added axes leaves the position. IB-1501278-D 834 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions [TCP signal output timing chart] (G30.3 command with tool change position return for additional axes set ON) Machining program G30.1; T02; G00X - 100. Arrival of X axis to tool change position Arrival of Z axis to tool change position Arrival of additional axis to tool change position Tool change position return complete signal (TCP) (4) When a tool change position return command is issued, tool offset data such as for tool length offset and tool radius compensation for the axis that moved is canceled. (5) This command is executed by dividing blocks for every axis. If this command is issued during single-block operation, therefore, a block stop occurs each time one axis returns to the tool change position. To make the next axis tool change position return, therefore, a cycle start needs to be specified. 835 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions Operation example The figure below shows an example of how the tool operates during the tool change position return command. (Only operations of X and Y axes in G30.1 to G30.3 are figured.) Y G30.3 (TCP) G30.1 G30.2 X TCP : Tool change position (1) G30.1 command: The Z axis returns to the tool change position, then the X and Y axes simultaneously do the same thing. (If tool change position return is on for an added axis, the added axis also returns to the tool change position after the X, Y and Z axes reach the tool change position.) (2) G30.2 command: The Z axis returns to the tool change position, then the X axis does the same thing. After that, the Y axis returns to the tool change position. (If tool change position return is on for an added axis, the added axis also returns to the tool change position after the X, Y and Z axes reach the tool change position.) (3) G30.3 command: The Z axis returns to the tool change position, then the Y axis does the same thing. After the Y axis returns to the tool change position, the X axis returns to the tool change position. (If tool change position return is on for an added axis, the added axis also returns to the tool change position after the X, Y and Z axes reach the tool change position.) (4) G30.4 command : The X axis returns to the tool change position, then the Y axis and Z axis simultaneously do the same thing. (If tool change position return is on for an added axis, the added axis also returns to the tool change position after the X, Y and Z axes reach the tool change position.) (5) G30.5 command : The Y axis returns to the tool change position, then the X and Z axes return to the tool change position simultaneously. (If tool change position return is on for an added axis, the added axis also returns to the tool change position after the X, Y and Z axes reach the tool change position.) (6) G30.6 command :The X, Y and Z axes return to the tool change position simultaneously. (If tool change position return is on for an added axis, the added axis also returns to the tool change position after the X, Y and Z axes reach the tool change position.) IB-1501278-D 836 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions 19.15 Reference Position Check ; G27 Function and purpose This command first positions the tool at the position assigned by the program and then, if that positioning point is the 1st reference position, it outputs the reference position arrival signal to the machine in the same way as with the G28 command. Therefore, when a machining program is prepared so that the tool will depart from the 1st reference position and return to the 1st reference position, it is possible to check whether the tool has returned to the reference position after the program has been run. Command format X__ Y__ Z__ P__ ; ... Check command XYZ Return control axis P Check No. P1: 1st reference position check P2: 2nd reference position check P3: 3rd reference position check P4: 4th reference position check Detailed description (1) If the P command has been omitted, the 1st reference position will be checked. (2) The number of axes whose reference positions can be checked simultaneously depends on the number of axes which can be controlled simultaneously. Note that the display shows one axis at a time from the final axis. (3) An alarm will occur if the reference position is not reached after the command is completed. 837 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 19 Coordinate System Setting Functions IB-1501278-D 838 20 Protection Function 839 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 20 Protection Function 20Protection Function 20.1 Stroke Check before Travel ; G22/G23 Function and purpose By commanding the boundaries from the program with coordinate values on the machine coordinate system, machine entry into that boundary can be prohibited. This can be set only for the three basic axes. While the normal stored stroke limit stops entry before the prohibited area, this function causes a program error before movement to the block if a command exceeding the valid movement area is issued. Command format Stroke check before travel ON G22 X__ Y__ Z__ I__ J__ K__ ; Stroke check before travel cancel G23 ; XYZ Coordinates of upper point (basic axis name and its coordinate position) IJK Coordinates of lower point (I,J,K address and its coordinate position) Note (1) In the following command format, the basic axes are X, Y and Z. If the basic axis name differs, issue the command address of upper position coordinates with the basic axis name. Detailed description (1) The inner side of the boundary commanded with the upper position coordinate and the lower position coordinate is the prohibited area. (2) If the command is omitted, "0" will be set for the address. (3) The area designated with this function is different from the area designated with the stored stroke limit. However, the area enabled by both functions will be the actual valid movement range. Z Y (x, y, z) Upper point designated coordinate X (i, j, k) Lower point designated coordinate Prohibited range <Note> The upper point and lower point are commanded with coordinate on the machine coordinate system. IB-1501278-D 840 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 20 Protection Function Precautions (1) This function is valid only when starting the automatic operation. When interrupted with manual absolute OFF, the prohibited area will also be shifted by the interrupted amount. (2) An error will occur if the start point or end point is in the prohibited area. (3) Stroke check will not be carried out for the axes having the same coordinates set for the upper point and the lower point. (4) The stroke check is carried out with the tool center coordinate values. (5) If G23X_Y_Z_; etc., is commanded, the command will be interpreted as G23;X_Y_Z;(2 blocks) . Thus, the stroke check before travel will be canceled, then movement will take place with the previous movement modal. (6) During automatic reference position return, the check will not be carried out from the intermediate point to the reference position. With G29, when moving from the start point to intermediate point, the check will not be carried out. (7) If there is an address that is not used in one block, a program error will occur. (8) When the rotary-type rotary axis is set as a basic axis, the prohibited area will be converted to the range of from 0° to 360° in the same manner as the movement command. If the setting extends over "0°", the side containing "0°" will be the check area. (Example) (a) G22 Z45. K315. Stroke check area 45. <= Z <= 315. (b) G22 Z-115. K-45. Stroke check area 225. <= Z <= 315. (c) G22 Z45. K-45. Stroke check area 0. <= Z <=45., 315. <= Z <= 360. (a) (C) (b) 45 45 0 360 315 - 115 225 - 45 315 0 360 - 45 315 Shaded area: check area 841 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 20 Protection Function 20.2 Enable Interfering Object Selection Data; G186 Function and purpose Sixteen interfering objects to be checked in the interference check III are preset by the MTB (R register or system variables). The interfering object selection is enabled by the "Interference check III: Enable interfering object selection data" signal (Y769) or the "Enable interfering object selection data" command (G186) after the target interfering object has been selected. When the "Interference check III mode" signal (Y76A) is set to ON after the interfering object selection has been enabled, the interference check starts. Refer to the PLC Interface Manual (IB-1501258) for the R register and commands issued by the PLC device. For details on the system variables, refer to "22.29 System Variables (Interfering Object Selection)". This section describes the "Enable interfering object selection data" command (G186). Command format "Enable interfering object selection data" command G186; Detailed description Consistency check between interfering object definition and interfering object selection (1) When the "Enable interfering object selection data" command (G186) or the "interference check III: Enable interfering object selection data" signal is set to ON, the consistency between the interfering object definition and interfering object selection is checked. (2) If the consistency check causes an operation error, all axes in all part systems will stop. An operation error can be remedied by redefining the interfering object data (*1) or resetting all part systems (except for sub part system 2). (*1) After correcting the interfering object data, issue the "Enable interfering object selection data" signal or "Enable interfering object selection data" command (G186). (3) The manual operation and automatic operation are not available until all the part systems (except for subpart system 2) are reset. (4) In the case the alarm occurs due to the consistency check, the interfering data will not be updated. For the interference check between interfering objects, the interfering data enabled last time is continuously used. Interference check III mode enable command While the interference check III mode signal is set to ON after the "Enable interfering object selection data" signal or the "Enable interfering object selection data" command (G186) has been executed, the interference between interfering objects is checked. While the interference check III is being executed, the interference check III mode active signal is turned ON. After the NC power is turned ON, if the interference check III mode signal is turned ON without executing the "Enable interfering object selection data" signal or the "Enable interfering object selection data" command (G186) even once, an operation error (M03 1001) will occur. IB-1501278-D 842 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 20 Protection Function Timing chart at execution of G186 G186 command Interference check III mode enable signal G186 G186 (*1) (*2) Interference check III mode active signal Status of interference check III (*3) (*1) (*2) (*3) (*1) The first interfering data pattern is set by the G186 command. The interference check III function executes check processing based on the first data pattern setting. (*2) The second interfering data pattern is set by the G186 command. The interference check III function executes check processing based on the second data pattern setting. (*3) The interference check III function is not executed. Relationship with other functions Manual arbitrary reverse run The program cannot be run backward prior to the "Enable interfering object selection data" command (G186). Arbitrary reverse run If the "Enable interfering object selection data" command (G186) is run backward, the interference data at the reverse run is enabled, instead of returning to the interference data at forward run. 843 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 20 Protection Function Precautions (1) The high-speed high-accuracy control function (high-speed machining mode, high-accuracy control, spline interpolation, etc.) generates a path appropriate for the tolerance amount to execute a machining program commanded with fine segments at high speed and smoothly. Thus, a difference arises between the path on which the interference check III is performed and the path on which the tool actually passes. When using the interference check III together with the high-speed high-accuracy control (high-speed machining mode, high-accuracy control, spline interpolation, etc.), define an interfering object (solid) with the clearance amount to suit the path difference that occurs depending on the tolerance amount. (2) The axis that is stopped when an operation error (M03 0001) or (M03 0002) is detected depends on the MTB specifications (parameter "#1444 otsys" (OT all-part-system stop enable/disable selection). When "0" is set, all the axes in the part system which controls the axes set to "interfering object I/J/K control axis" and "I/J/K rotary control axis" in the interfering object definition will stop. When "1" is set, all axes in all part systems will stop. (3) If an operation error (M03 0002) is detected between the fixed interfering objects (*1), an alarm will be output to part system 1. (*1) These refer to the interfering objects for which "interfering object I/J/K control axis" and "I/J/K rotary control axis" are not set in the interfering object definition. (4) If you perform the interference check III during the high-speed simple program check, an operation error (M03 0001) may occur at a position different from the actual operation. (5) If multiple interfering objects including the rotary axis setting are set as one interfering object using the interfering check III: designation of disabled interference object, only the interfering object in which a rotary axis is set will be in rotating operation, checking the interference between the interfering objects. (6) If an operation error (M03 0001) occurs, cancel the alarm by moving the interfering object to the retracting direction with the linear axis. (7) The PLC axis is not available for the interference check III. However, it is available when NC axis/auxiliary axis switching is enabled. (8) In the interference check III, the interference is checked in 0.1μm units regardless of the control unit. (9) At the occurrence of the operation error (M03 0001), all the axes in the part system in which the alarm has occurred will stop. If the entry to the interference alarm area is not detected by the subsequent axis travel command (manual operation/automatic operation), the operation error (M03 0001) will be cancelled and the axes will travel. Depending on the relative positional relation between the interfering objects or the feedrate of axes, the axis can travel further to the interfering direction from the stopped position (a direction to which the interfering objects interfere). Even if the axis moves toward the interfering direction, it will stop before entering the interference alarm area. IB-1501278-D 844 21 Measurement Support Functions 845 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions 21Measurement Support Functions 21.1 Automatic Tool Length Measurement ; G37 Function and purpose These functions issue the command values from the measuring start position as far as the measurement position, move the tool in the direction of the measurement position, stop the machine once the tool has arrived at the sensor, cause the NC system to calculate automatically the difference between the coordinate values at that time and the coordinate values of the commanded measurement position and provide this difference as the tool offset amount. When offset is already being applied to a tool, it moves the tool toward the measurement position with the offset still applied, and if a further offset amount is generated as a result of the measurement and calculation, it provides further compensation of the present compensation amount. If there is one type of offset amount at this time, and the offset amount is distinguished between tool length offset amount and wear offset amount, the wear amount will be automatically compensated. Command format Automatic tool length measurement command G37 Z__ R__ D__ F__ ; Z Measuring axis address and coordinates of measurement position -------- X,Y,Z,α (α is the additional axis.) R This commands the distance between the measurement position and point where the movement is to start at the measuring speed. D This commands the range within which the tool is to stop. F This commands the measuring feedrate. When R_, D_ or F_ is omitted, the value set in the parameter is used instead. <Parameter> ("Automatic tool length measurement" on the machining parameter screen) #8004 SPEED: 0 to 1000000 [mm/min] #8005 ZONE r: 0 to 99999.999 [mm] #8006 ZONE d: 0 to 99999.999 [mm] IB-1501278-D 846 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions Detailed description (1) Operation with G37 command (F1) (f2) (a) D (d) D (d) F (fp) R (r) (d1) (b) 1R 1R 1R 1R (c) Op1 : Normal completion as it is measurement within the allowable range. Op2 : Alarm stop (P607) as it is outside of the measurement allowable range. Op3 : Alarm stop (P607) as the sensor is not detected. Op4 : Alarm stop (P607) as it is outside of the measurement allowable range. However if there is no (c) area, normal completion will occur. (a) Measurement allowable range (b) Compensation amount (d1) Distance (F1) Speed (f2) Feedrate (d) Measurement range (r) Deceleration range Measuring position Stop point Sensor output (2) The sensor signal (measuring position arrival signal) is used in common with the skip signal. (3) The feedrate will be 1mm/min if the F command and parameter measurement speed are 0. (4) An updated offset amount is valid unless it is assigned from the following Z axis (measurement axis) command of the G37 command. (5) Excluding the delay at the PLC side, the delay and fluctuations in the sensor signal processing range from 0 to 0.2ms. As a result, the measuring error shown below is caused. Maximum measuring error [mm] = Measuring speed [mm/min] * 1/60 * 0.2 [ms]/1000 (6) The machine position coordinates at that point in time are read by sensor signal detection, and the machine will overtravel and stop at a position equivalent to the servo droop. Maximum overtravel [mm] = Measuring speed [mm/min] * 1/60 * 1/Position loop gain [1/s] The standard position loop gain is 33 (1/s). 847 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions Operation example For new measurement [mm] G28 Z0; T01; M06 T02; G90 G00 G43 Z0 H01; G37 Z-400. R200. D150. F1; (Z0) 0 (a) - 100 Coordinate value when reached the measurement position = -300. -300.-(-400.)=100. 0+100.=100. H01=100. (b) - 200 F - 300 R (a) Tool length (b) Movement amount by tool length measurement (c) Measuring device D - 400 (c) D Note (1) A new measurement is applied when the current tool length compensation amount is zero. Thus, length will be compensated whether or not length dimension by tool compensation memory type and length wear are differentiated. When tool compensation is applied [mm] G28 Z0; T01; M06 T02; G43 G00 Z0 H01; G37 Z-400. R200. D50. F10; (Z0) 0 - 100 (d) Coordinate value when reached the measurement position = -305. -305.-(400.)=95. Thus, H01=95. - 200 F R - 300 (c) Measuring device (d) Wear amount D - 400 (c) D Note (1) A measurement for the wear amount is applied when the current tool length compensation amount is other than zero. Thus, length wear will be compensated if length dimension by tool compensation memory type and length wear are differentiated. If not differentiated, length dimension will be compensated. IB-1501278-D 848 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions Precautions (1) Program error (P600) occurs if G37 is commanded when the automatic tool length measurement function is not provided. (2) Program error (P604) will occur when no axis has been commanded in the G37 block or when two or more axes have been commanded. (3) Program error (P605) will occur when the H code is commanded in the G37 block. (4) Program error (P606) will occur when G43_H code is not commanded prior to the G37 block. (5) Program error (P607) will occur when the sensor signal is input outside the allowable measuring range or when the sensor signal is not detected even upon arrival at the end point. (6) When a manual interrupt is applied while the tool is moving at the measuring speed, a return must be made to the position prior to the interrupt and then operation must be resumed. (7) The data commanded in G37 or the parameter setting data must meet the following conditions: | Measurement point start point | > R command or parameter r > D command or parameter d (8) When the D address and parameter d in (7) above are zero, the operation will be completed normally only when the commanded measurement point and sensor signal detection point coincide. Otherwise, program error (P607) will occur. (9) When the R and D addresses as well as parameters r and d in (7) above are all zero, program error (P607) will occur regardless of whether the sensor signal is present or not after the tool has been positioned at the commanded measurement point. (10) When the measurement allowable range is larger than the measurement command distance, it becomes the measurement allowable range for all axes. (11) When the measurement speed movement distance is larger than the measurement command distance, all axes move at the measurement speed. (12) When the measurement allowable range is larger than the measurement speed movement distance, the axis moves in the measurement allowable range at the measurement speed. (13) The automatic tool length measurement command (G37) must be commanded together with the G43H_ command that designates the offset No. G43 H_; G37 Z_ R_ D_ F_; (14) If an axis other than Z is specified for the measuring axis in G37 while the parameter "#1080 Dril_Z" is set to "1", the program error(P606) occurs. 849 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions 21.2 Skip Function ; G31 Function and purpose When the skip signal is input externally during linear interpolation based on the G31 command, the machine feed is stopped immediately, the coordinate value is read, the remaining distance is discarded and the command in the following block is executed. Command format G31 X__ Y__ Z__ α__ R__ F__ ; X,Y,Z,α Axis coordinate value; they are commanded as absolute or incremental values according to the G90/G91 modal when commanded. α is the additional axis. R Acceleration/deceleration command R0: Acceleration/deceleration time constant=0 (No automatic acceleration/deceleration after interpolation.) R1: Acceleration/deceleration time constant valid. Accelerate/decelerate with the time constant set with the parameters "#2102 skip_tL" and "#2103 skip_t1". R0 is applied when it is omitted. F Feedrate (mm/min) IB-1501278-D 850 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions Detailed description (1) If an F command is programmed in the same block as G31, the commanded speed is set as the skip speed. If an F 1-digit feed command is issued to program the feedrate, F 1-digit feed is disabled. Note that, in the following cases, the skip speed and operations depend on the MTB specifications (parameter "#12022 skipF_spec/bit2"). #12022/bit2 = 0 #12022/bit2 = 1 Skip speed if an F command is The value of parameter "#1174 not programmed in the G31 skip_F" is used as the skip speed. block The skip speed is determined based on the modality of F when G31 is executed. A program error (P603) will also occur A program error (P62) will also occur if if the value of parameter "#1174 the value of F modality is "0". skip_F" is "0". Mode of commanded speed Only feed per minute mode is avail- Follows the mode (Feed per minute/ able. Feed per minute mode is enabled Feed per revolution) that is active even in feed per revolution mode. when G31 is executed. Modality of F command The F modal is not updated even if the The F modal that is updated by an F G31 block contains an F command. command in the G31 block varies depending on the mode (Feed per minute/Feed per revolution) that is active when G31 is executed. (2) The maximum speed of G31 command is determined by the machine specification. (3) When R0 is commanded or the R command is omitted, the step acceleration/deceleration will be applied to G31 block after the interpolation without performing the automatic acceleration/deceleration. When R1 is commanded, the automatic acceleration/deceleration will be performed according to the cutting feed acceleration/deceleration mode set by the parameter "#2003 smgst" with the time constant set by the parameter "#2102 skip_tL" and "#2103 skip_t1". Even if G1 constant inclination acceleration/deceleration (the parameter "#1201 G1_acc" is set to "1") is valid, the time constant acceleration and deceleration will be performed. (4) When the R1 is commanded with the acceleration and deceleration command, the automatic acceleration and deceleration will be performed after the interpolation even if the skip single is input. Note that if the value of the parameter "#2102 skip_tL" and "#2103 skip_t1" are large, the movement will not stop immediately. Acceleration/deceleration when R0 is commanded or R is omitted sk1 f t Acceleration/deceleration when R1 is commanded sk1 f (tL) (sk1) Skip signal (tL) t (tL) Skip time constant (5) Command the acceleration/deceleration command (R0/R1) whenever G31 is commanded. If R0/R1 has not been commanded, or anything other than R0/R1 has been commanded, the acceleration/deceleration time constant is assumed to "0" (R0), and automatic acceleration/deceleration after interpolation will not be performed. 851 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions (6) When G31 is commanded, the stop conditions (feed hold, interlock, override zero and stroke end) are valid. External deceleration is also valid. For the validity of the following various functions, refer to the MTB specifications. Cutting feed override (parameter "#12022 skipF_spec/bit0") Dry run (parameter "#12022 skipF_spec/bit1") (7) The G31 command is unmodal and it needs to be commanded each time. (8) If the skip command is input at the start of the G31 command, the G31 command will be completed immediately. When a skip signal has not been input until the completion of the G31 block, the G31 command will also be completed upon completion of the movement commands. (9) If the G31 command is issued during tool radius compensation or nose R compensation, program error (P608) will occur. (10) When there is no F command in the G31 command and the parameter speed is also zero, the program error (P603) will occur. (11) With machine lock or with the Z axis cancel switch ON when only the Z axis is commanded, the skip signal will be ignored and execution will continue as far as the end of the block. Readout of skip coordinates The coordinate positions for which the skip signal is input are stored in the system variables #5061 (1st axis) to #506n (n-th axis), so these can be used in the user macros. : G90 G00 X-100. ; G31 X-200. F60 ; (Skip command) #101=#5061 ; Skip signal input coordinate position (workpiece coordinate system) is readout to #101. : Note (1) Depending on the MTB specifications (parameter "#1366 skipExTyp"), the skip coordinate value may be "0" even if the G31 command is given in a 1-part system or in only a part of a multi-part system. G31 coasting The amount of coasting from when the skip signal is input during the G31 command until the machine stops differs according to the parameter "#1174 skip_F" or F command in G31. The time to start deceleration to stop after responding to the skip signal is short, so the machine can be stopped precisely with a small coasting amount. The coasting amount can be calculated from the following formula. 0= F 60 Tp+ = F 60 (Tp+t1) 1 F 60 (t1 t2) F 60 t2 2 δ0 : Coasting amount (mm) F : G31 skip speed (mm/min) Tp : Position loop time constant (s) = (position loop gain)-1 t1 : Response delay time (s) = (time taken from the detection to the arrival of the skip signal at the controller via PC) t2 : Response error time 0.001 (s) When G31 is used for calculation, the value calculated from the section indicated by δ1 in the above equation can be compensated for, however, δ2 results in calculation error. IB-1501278-D 852 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions Stop pattern with skip signal input is shown below. F (a) F: Feedrate (a) Skip signal input (T) Time Coasting amount ț0 (T) t1 t2 Tp The relationship between the coasting amount and speed when Tp is 30ms and t1 is 5ms is shown in the following figure. (a) Maximum value Tp=0.03 (b) Average value t1=0.005 0.050 (c) Minimum value (a) F: Feedrate (b) δ: Coasting amount 0.040 (c) 0.030 (mm) 0.020 0.010 0 10 20 30 40 50 60 70 F (mm/min) Readout error of skip coordinates mm (1) Skip signal input coordinate readout The coasting amount based on the position loop time constant Tp and cutting feed time constant Ts is not included in the skip signal input coordinate values. Therefore, the workpiece coordinate values applying when the skip signal is input can be readout within the error range in the following formula as the skip signal input coordinate values. However, coasting based on response delay time t1 results in a measurement error and so compensation must be provided. ε : Readout error ε=±(F/60)×t 2 (µm) F : Feedrate +1 t2 : Response error time 0.001 (s) 0 60 F (mm/min) Measurement value -1 Readout error of skip signal input coordinates Readout error with a 60mm/min feedrate is as shown below and the measurement value is within readout error range of ±1μm: ε= ± (60/60) x 0.001 = ± 0.001 (mm) (2) Readout of other coordinates The readout coordinate values include the coasting amount. Therefore, when coordinate values at the time of skip signal input is required, reference should be made to the section on the G31 coasting amount to compensate the coordinate value. As in the case of (1), the coasting amount based on the delay error time t2 cannot be calculated, and this generates a measuring error. 853 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions Examples of compensating for coasting (1) Compensating for skip signal input coordinates : G31 X100.F100 ; Skip command G04 ; Machine stop check #101=#5061 ; Skip signal input coordinate readout #102=#110*#111/60 Coasting based on response delay time ; #105=#101-#102 ; Skip signal input coordinates : #110 = Skip feedrate; #111 = Response delay time t1; (2) Compensating for workpiece coordinates : G31 X100.F100 ; Skip command G04 ; Machine stop check #101=#5061 ; Skip signal input coordinate readout #102=#110*#111/60 Coasting based on response delay time ; #103=#110*#112/60 Coasting based on position loop time constant ; #105=#101-#102#103 ; Skip signal input coordinates : #110 = Skip feedrate; #111 = Response delay time t1; #112 = Position loop time constant Tp; Operation to be carried out when the skip command is executed on multiple part systems at the same time The operation resulting from the G31 command executed simultaneously on multiple part systems depends on the MTB specifications (parameter "#1366 skipExTyp"). #1366 Operation 0 When any part system is executing the G31 command, the G31 command issued for other part systems is subjected to a block interlock state, and such G31 command will be executed after the current G31 command execution is completed. (No error is displayed.) In a single-block operation, for example, where the G31 block is started in multiple part systems at the same time, it is executed in the smallest part system first. 1 The G31 command is executed on multiple part systems at the same time. However, the skip coordinate position is not read and is set to "0" in all part systems. (*1) (*1) The skip coordinate position is also set to "0" when the G31 command is executed on a single part system. Furthermore, it is set to "0" when the G31 command is executed on one part system in a multiple part system configuration. When the G31 command is used for measuring purposes, "#1366 skipExTyp" must be "0". IB-1501278-D 854 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions Operation example G90 G00 G31 G01 G31 X-100000 Y0; X-500000 F100; Y-100000; X-0 F100; Y-200000; G31 X-500000 F100; Y-300000; X0; G31 - 500000 - 100000 0 Y W G01 G31 X - 100000 G01 G31 - 200000 G01 G01 - 300000 855 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions 21.3 Multi-step Skip Function 1 ; G31.n, G04 Function and purpose The setting of combinations of skip signals to be input enables skipping under various conditions. The actual skip operation is the same as G31. The G commands which can specify skipping are G31.1, G31.2, G31.3, and G04, and the correspondence between the G commands and skip signals and settings for each parameter depend on the MTB specifications. Command format G31.1 X__ Y__ Z__ α__ R__ F__ ; X,Y,Z,α Target coordinates R Acceleration/deceleration command R0: Acceleration/deceleration time constant=0 (No automatic acceleration/deceleration after interpolation.) R1: Acceleration/deceleration time constant valid. Accelerate/decelerate with the time constant set in the parameters "#2102 skip_tL" and "#2103 skip_t1". R0 is applied when it is omitted. F Feedrate (mm/min) Same with G31.2 and G31.3; Ff is not required with G04. As with the G31 command, this command executes linear interpolation and when the preset skip signal conditions have been met, the machine is stopped, the remaining commands are canceled, and the next block is executed. Detailed description (1) The skip speed is specified by program command or parameter. Feedrate G31.1 set with the parameter corresponds to "#1176 skip1f", G31.2 corresponds to "#1178 skip2f", G31.3 corresponds to "#1180 skip3f", and G04 corresponds to "#1173 dwlskp". Note that the F modal is not updated in each case. (2) A command is skipped if it meets the specified skip signal condition. (3) The feedrates corresponding to the G31.1, G31.2, and G31.3 commands can be set by parameters. (4) The skip conditions (logical sum of skip signals that have been set) corresponding to the G31.1, G31.2, G31.3 and G04 commands can be set by parameters. Parameter setting Valid skip signal 1 1 2 2 ○ 3 ○ ○ 4 ○ 5 ○ 6 7 ○ ○ ○ ○ ○ ○ (5) Details other than the above are the same as those on G31 (Skip function). IB-1501278-D 3 ○ 856 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions Operation example (1) The multi-step skip function enables the following control, thereby improving measurement accuracy and shortening the time required for measurement. [Parameter settings] Skip condition Skip speed G31.1 :7 20.0 mm/min(f1) G31.2 :3 5.0 mm/min(f2) G31.3 :1 1.0 mm/min(f3) [Program example] N10 G31.1 X200.0 ; N20 G31.2 X40.0 ; N30 G31.3 X1.0 ; f (f1) N10 (a) (a) Measurement distance (F) Skip speed (sk1) Input of skip signal 1 (sk2) Input of skip signal 2 (sk3) Input of skip signal 3 (F) (f2) N20 (f3) N30 t (sk3) (sk2) (sk1) <Note> If skip signal 1 is input before skip signal 2 in the above operation, N20 is skipped at that point and N30 is also ignored. f (sk3) (sk2) (f1) (sk1) N10 (f2) (f3) N20 (tL) (sk1) Skip signal (tL) (tL) N30 (tL) t (tL) Skip time constant (2) If a skip signal with the condition set during G04 (dwell) is input, the remaining dwell time is canceled and the following block is executed. 857 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions 21.4 Multi-step Skip Function 2 ; G31 P Function and purpose During linear interpolation by the skip command (G31), operation can be skipped according to the conditions of the skip signal parameter Pp. If multi-step skip commands are issued simultaneously in different part systems as shown in the left figure, both part systems perform skip operation simultaneously if the input skip signals are the same, or they perform skip operation separately if the input skip signals are different as shown in the right figure. The skip operation is the same as a normal skip command (G31 without P command). Y1 Y1 (sk1) ($1) (sk1) ($1) X1 X1 Y2 Y2 (sk1) ($2) (sk2) ($2) X2 X2 [Same skip signals input in both 1st and 2nd part systems] [Different skip signals input in 1st and 2nd part systems] ($1) 1st part system ($2) 2nd part system (sk1) Skip signal 1 (sk2) Skip signal 2 If the skip condition specified by the parameter "#1173 dwlskp" (indicating external skip signals 1 to 4) is met during execution of a dwell command (G04), the remaining dwell time is canceled and the following block is executed. Command format G31 X__ Y__ Z__ α__ P__ R__ F__ ; XYZα Target coordinates P Skip signal command R Acceleration/deceleration command R0: Acceleration/deceleration time constant=0 (No automatic acceleration/deceleration after interpolation.) R1: Acceleration/deceleration time constant valid. Accelerate/decelerate with the time constant set in the parameters "#2102 skip_tL" and "#2103 skip_t1". R0 is applied when it is omitted. F Feedrate (mm/min) IB-1501278-D 858 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions Detailed description (1) The skip speed is specified by program command or parameter. The feedrate by the parameter is set by "#1174 skip_F". Note that the F modal is not updated in each case. (2) The skip signal is specified by skip signal command p. The command range of "p" is from 1 to 255. If outside the range is commanded, program error (P35) will occur. Skip signal command P Valid skip signal 8 7 6 5 4 3 2 1 1 ○ 2 ○ 3 ○ 4 ○ 5 ○ 6 ○ ○ ○ ○ 7 8 ○ ○ ○ ○ : : : 253 ○ ○ ○ ○ ○ ○ ○ 254 ○ ○ ○ ○ ○ ○ ○ 255 ○ ○ ○ ○ ○ ○ ○ ○ (3) The specified skip signal command is a logical sum of the skip signals. (Example) G31 X100. P5 F100 ; Operation is skipped if skip signal 1 or 3 is input. (4) If skip signal parameter Pp is not specified, it works as a skip function (G31), not as a multi-step skip function. If speed parameter Ff is not specified, the skip speed set by the parameter "#1174 skip_F" will apply. [Relations between skip and multi-step skip] Skip specifications × Condition ○ Speed Condition Speed G31 X100 ;(Without P and F) Program error (P601) Skip 1 #1174 skip_F G31 X100 P5 ;(Without F) Program error (P602) Command val- #1174 skip_F ue G31 X100 F100 ;(Without P) Program error (P601) Skip 1 G31 X100; P5 F100; Program error (P602) Command val- Command value ue Command value (5) If skip specification is effective and P is specified as an axis address, skip signal parameter P will be given a priority. The axis address "P" will be ignored. (Example) G31 X100. P500 F100 ; This is regarded as a skip signal. (The program error (P35) will occur.) (6) Other than above, the same detailed description as "Skip function; G31" applies. 859 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions 21.5 Speed Change Skip ; G31 Fn Function and purpose When the skip signal is detected during linear interpolation by the skip command (G31), the feedrate is changed. Command format G31 X__ (Y__) Z__ α__ R__ F__ F1 = __ ... Fn = __ ; ("n" is the skip signal 1 to 8) ... Skip command X, (Y,) Z, α Target coordinates R Acceleration/deceleration command R0: Acceleration/deceleration time constant=0 When the movement is stopped by the skip signal detection, the step stop will occur. R1: Acceleration/deceleration time constant valid. When the movement is stopped by the skip signal detection, it will decelerate with the time constant set in the parameter "#2102 skip_tL" and "#2103 skip_t1". When omitted, R0 will be applied. F Feedrate when starting the cutting feed (mm/min) Fn= Feedrate after detecting the skip signal (mm/min) Fn = 0: Movement stop Fn ≠ 0 :Changing the feedrate to fn F1 = Feedrate after inputting the skip signal 1 : F8 = Feedrate after inputting the skip signal 8 IB-1501278-D 860 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions Detailed description (1) When the skip signal for which the feedrate fn≠0 is commanded, the speed is changed to the command speed corresponding to the skip signal. (2) When the skip signal for which the feedrate fn=0 is commanded, the movement is stopped. If R0 is commanded or R command is omitted, the skip stop will occur when the movement is stopped by the skip signal detection without performing the automatic acceleration/deceleration by the skip time constant. When R1 is commanded, the automatic acceleration/deceleration will be performed with the skip time constant after the interpolation even if the movement is stopped by the skip signal detection. Note that if the value of the parameter "#2102 skip_tL" and #2103 skip_t1" are large, it will not stop immediately. After the movement is stopped, the remaining movement commands are canceled and the following block will be executed. (3) When a skip signal has not been input until the completion of the G31 block, the G31 command will also be completed upon completion of the movement commands. (4) When the skip return is valid, the return operation by the skip signal detection is executed after the movement is stopped. (5) Even if G1 constant inclination acceleration/deceleration (#1201 G1_acc) is valid, the speed change skip will be the operation of the time constant acceleration and deceleration. (6) When the feedrate command (Fn=fn) is not specified after detecting the skip signal, the normal G31 skip operation will be applied. (7) If a skip signal (one of sk1 to sk4) are input during the deceleration (area (A) in the figure) after a move command has finished: (a) A skip signal (sk2 in the figure) for changing speed is ignored. (b) A skip signal (sk1 in the figure) for stopping the movement is executed and the speed is set to "0". Speed F (mm/min) (sk4) f (sk3) f4 f3 (sk1) (sk2) f2 f1 Time T (min) 0 (A) (8) The skip signal without commanding the feedrate in the program will be ignored. 861 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions (9) The speed change or the movement stop is performed when detecting the rising edge of the skip signal. Note that if several rising edges are input at 3.5ms intervals or less, they may be judged as the simultaneous input. When they are judged as the simultaneous input, the smaller value will be valid. Shown below are changes in time (T) and speed (F) when skip signals, 1 (sk1) to 4 (sk4), are input. Speed F (mm/min) (sk3+sk4) f (sk2) f4 f3 (sk1) f2 f1 Time T (min) 0 (sk4) (sk3) (sk2) (sk1) Time T (min) (10) If the G31 block is started with the skip signal input, that signal is considered to rise at the same time as the block starts. (11) If the skip signals for changing the speed and for stopping the movement are simultaneously input, the skip signal for stopping the movement will be valid regardless of the size of the number. (12) If the skip time constant "#2102 skip_tL" is illegal, an MCP alarm (Y51 15) will occur. If the "#2103 skip_t1" is illegal, an MCP alarm (Y51 16) will occur. (13) Other than above, the same detailed description as "Skip function; G31" applies. IB-1501278-D 862 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions Operation example The following shows the operations when a skip time constant and skip signals, 1 (sk1) to 4 (sk4), are input. (1) Example of when R is not commanded Skip time constant ((a) in the figure) and position loop time constant ((b) in the figure) G31 X100. Ff F1=0 F2=f2 F3=f3 F4=f4 ; Speed F (mm/min) (sk4) f (sk3) (sk2) f4 f3 (sk1) f2 f1 Time T (min) 0 (a) (a) (b) (2) Example of when R1 is commanded Skip time constant ((tL) in the figure) G31 X100. R1 Ff F1=0 F2=f2 F3=f3 F4=f4; Speed F (mm/min) (sk4) f (sk3) (sk2) f4 f3 (sk1) f2 f1 Time T (min) 0 (tL) (tL) (tL) 863 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions 21.6 Torque Limitation Skip ; G160 Function and purpose Axis movement is performed in the torque limited status, and the axis movement command is suspended to proceed to the next block when the current command value reaches the designated torque skip value and the torque skip turns ON. In addition to the torque, the droop value can be add to the condition of the skip ON (Droop skip). This function enables measurement without a sensor. Command format Torque limitation skip G160 X/Y/α__ Q__ D__ F__ ; The G160 command is unmodal (group 00). When executing the G160 command continuously, it must always be command for each block separately. X/Y/α Axis address and coordinate value command (mm/inch) (Decimal point command is possible) Q Torque skip value (0 to 500 (%)) D Droop skip value (0 to 99999.999 mm, 0 to 9999.9999 inch) F Skip speed Set it in the range of feedrates. (mm/min, inch/min, mm/rev, inch/rev) Note (1) Designate an axis that exits in the part system for the axis address. If an axis that does not exist in the part system, a program error (P32) will occur. (2) Only one axis can be commanded with the axis address. If no axis is specified or if two or more axes are specified in the same block, a program error (P595) will occur. (3) For spindle/C axis (C axis command), a Q command is specified with 121 to 500 %, the axis is clamped at 120%. (4) If a Q command is omitted, torque skip function is performed as specified by the MTB (parameter shown below). NC axis (servo axis): SV014 lLMTsp (current limit value in special control) Spindle/C axis (C axis command): For the normal spindle, SP065 TLM1 (torque limit 1) For spindle-mode servo, SV014 ILMTsp (current limit value in special control) (5) If D command is omitted, a skip operation is performed using the torque skip value only. (6) D command must be programmed within the excessive error width shown below. NC axis (servo axis): SV023 OD1 (detected excessive error width when servo is on) Spindle/C axis: SP023 OD1 (detected excessive error width (interpolation mode)) (7) If an F command is omitted, the feedrate depends on the MTB specifications (parameter "#1174 skip_F"). (8) A program error (P603) will occur if the skip speed in F command is 0. IB-1501278-D 864 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions Detailed description Acceleration/deceleration when G160 is commanded Follow the acceleration/deceleration pattern for linear interpolation (G01). Even if G01 constant inclination acceleration/deceleration is valid, the time constant acceleration and deceleration will be performed. Skip speed If F command is programmed in the same block as G160, the commanded speed is set as the skip speed. If an F 1-digit feed command is issued to program the feedrate, F 1-digit feed is disabled. Note that, in the following cases, the skip speed and operations depend on the MTB specifications (parameter "#12022 skipF_spec/bit2"). #12022/bit2 = 0 Skip speed if F command is not The value of parameter "#1174 programmed in the G160 block skip_F" is used as the skip speed. #12022/bit2 = 1 The skip speed is determined based on the modality of F when G160 is executed. A program error (P603) will also occur A program error (P62) will also occur if if the value of parameter "#1174 the value of F modality is "0". skip_F" is "0". Mode of commanded speed Only feed per minute mode is avail- Follows the mode (Feed per minute/ able. Feed per minute mode is enabled Feed per revolution) that is active when G160 is executed. even in feed per revolution mode. Modality of F command F modal is not updated even if the The F modal that is updated by F comG160 block contains an F command. mand in the G160 block varies depending on the mode (Feed per minute/Feed per revolution) that is active when G160 is executed. Control signals regarding speed control and stop (1) For the validity of the following various functions, refer to the MTB specifications. Cutting feed override valid/invalid (parameter "#12022 skipF_spec/bit0") Dry run valid/invalid (parameter "#12022 skipF_spec/bit1") (2) An operation error (M01 0102) occurs if 0% cutting feed override is performed when cutting feed override is invalid. (3) The stop conditions (feed hold, interlock, override zero and stroke end) and external deceleration are valid when torque limitation skip is used. (4) The machine lock signal is valid. (The counter is updated until the program reaches the end point of the block.) Processing when the torque skip turns on (1) If the current value for the specified axis exceeds the torque skip value, the torque limit is reached and droop exceeds the droop skip value, the torque skip turns on. If there is no D command, the torque skip turns on when the torque limit is reached. (2) The current position when the torque skip turns on is regarded as the block end point and the remaining distance (command value - actual movement distance) is discarded. 865 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions Completion of skip command (1) If the torque skip turns on during G160 command, the program completes the current block before moving on to the next block. (2) If the torque skip does not turn on until G160 command reaches the end point, the skip command completes at the end of the block and then the program moves on to the next block. (3) Set the skip coordinate values (workpiece coordinate values) to system variables (#5061 and onwards). When the tool has moved to the end point, set the end point position. Droop Droop skip value Torque skip on Time Current value Droop skip value Time Commanded speed Block end point Actual movement distance Remaining distance Program command position Interference object Axis movement target Program example : : Workpiece radius measurement tool G28 Z200. T01; Tool selection for measurement G00 X50. Y50. Z100. ; G160 Z40. Q80 F20; Torque skip command #100=#5061; Completion of skip command (Coordinate position (workpiece value) read) : 50. 40. 0. IB-1501278-D 866 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions Relationship with Other Functions Manual arbitrary reverse run The skip speed is controlled with the manual arbitrary reverse run speed. Torque skip command block cannot be executed in the reverse run. Manual interruption When a manual interrupt is applied during execution of torque skip, calculate the position shifted by the amount of the manual interruption as the skip position. Skip variables The torque skip position is common to skip variables (#5061 and onwards) for G31 skip function. Geometric, Corner Rounding, Corner Chamfering Geometric, Corner Rounding, and Corner Chamfering are not available for torque skip blocks. Program error (P595) will occur. Torque limit Torque skip command, if executed on the axis to which torque limits are applied, is based on the torque skip value in the G160 command. Functions for which torque skip command is not available Torque skip command (G160) cannot be commanded when any of the following functions is in use. (An error will occur.) Function name Error Tool radius compensation (G40, G41, G42, G46) Program error (P608) Synchronous control (G114.1) Program error (P595) High-speed high-accuracy control (G05.1/G05) Program error (P34) Precautions (1) Decreasing the torque limit value may cause a torque limit to be applied during acceleration/deceleration. (2) When the reset button is pressed while torque skip is active, an axis moving with G160 stops. After the axis has stopped, the original torque is restored. (3) Writing parameters via a PLC or other host controller during execution of torque skip causes the torque limit value to be the setting value of servo parameter SV014, possibly causing it to be no longer correct torque skip value. (The PLC signal operations and setting values of the servo parameters are based on the MTB specifications.) (4) When using D command (droop skip value), command a value that does not exceed the excessive error width. (5) After a torque skip, the droop is canceled. (6) The droop is displayed in interpolation increments on the drive monitor. They are different from the command increments of D command. 867 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 21 Measurement Support Functions 21.7 Programmable Current Limitation ; G10 L14 ; Function and purpose This function allows the current limit value of the NC axis to be changed to a desired value in the program, and is used for the workpiece stopper, etc. "#2214 SVO14(current limit value in special control)” can be changed. The commanded current limit value is designated with a ratio of the limit current to the rated current. Command format G10 L14 Xn ; L14 Current limit value setting (+ side/- side) X Axis address n Current limit value (%) Setting range: 1 to 999 Precautions (1) If the current limit value is reached when the current limit is valid, the current limit reached signal is output. (2) The following two modes can be used with external signals as the operation after the current limit is reached. The external signal determines which mode applies. [Normal mode] The movement command is executed in the current state. During automatic operation, the movement command is executed until the end, and then move to the next block with the droops still accumulated. [Interlock mode] During the occurrence of the droops, it enters to the internal interlock state and the next movement will not be carried out. During automatic operation, the operation stops at the corresponding block, and the next block is not moved to. During manual operation, the following same direction commands are ignored. (3) The position droop generated by the current limit can be canceled when the current limit changeover signal of external signals is canceled. (Note that the axis must not be moving.) (4) The setting range of the current limit value is 1% to 999%. Commands that exceed this range will cause a program error (P35). (5) If a decimal point is designated with the G10 command, only the integer will be valid. Example) G10 L14 X10.123 ; The current limit value will be set to 10%. (6) For the axis name "C", the current limit value cannot be set from the program (G10 command). To set from the program, set the axis address with an incremental axis name, or set the axis name to one other than "C". IB-1501278-D 868 22 System Variables 869 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22System Variables 22.1 System Variables List The M800/M80 series provides the following system variables. Note that the available types and numbers vary depending on the machine specifications and whether the machine is intended for use by a user or MTB. No. ○: Available -: Unavailable Reading Setting #1000 - #1035, #1200 - #1295 Signal input from PLC to NC ○ (*1) - 22.25 #1100 - #1135 #1300 - #1395 Signal output from NC to PLC ○ (*1) ○ (*1) 22.26 #1900, #1901 Used for normal line control. ○ ○ 22.22 #2001 - #2000+n #2201 - #2200+n #2401 - #2400+n #2601 - #2600+n Tool offset data ○ Also refer to the variables #10001, #135001 and #230001 or larger. ○ 22.6 #2501, #2601 External workpiece coordinate offset ○ ○ 22.10 #3000 Used to forcibly set to the alarm mode. Designate the number and message. - ○ 22.12 #3001, #3002 Cumulative time (integrating time) ○ - 22.14 #3001, #3002 #3011, #3012 Time read variables ○ ○ 22.15 #3003 ○ ○ 22.16 ○ ○ #3006 Inhibition of single block stop Inhibition of miscellaneous function finish signal waiting Prohibition of program check reverse run Automatic operation pause OFF Cutting override OFF G09 check OFF Dry run invalid Used to display and stop a message. - ○ 22.13 #3007 Mirror image ○ - 22.19 #3901, #3902 Number of machining processes / Maximum number of machining ○ processes ○ 22.18 #4001 - #4021 #4201 - #4221 G command modal information ○ - 22.2 #4101 - #4120 #4301 - #4320 Non-G command modal information ○ - 22.3 #4401 - #4421 #4507 - #4520 Modal information at macro interruption ○ - 22.4 #5001 - #5160+n Position information End point coordinate position of the previous block Machine coordinate position Workpiece coordinate position Skip coordinate position Tool position compensation amount Servo deviation amount Macro interruption stop block coordinate position Workpiece coordinate offset data ○ - 22.11 #3004 #5201 - #5320+n Data type or use Section ○ ○ 22.8 #7001 - #8900+n Extended workpiece coordinate offset data (48- or 96-set specifi- ○ cation) ○ 22.9 #10001 - #10000+n #11001 - #11000+n #16001 - #16000+n #17001 - #17000+n Tool offset data ○ Also refer to the variables #2001, #135001 and #230001 or larger. ○ 22.6 #26000 - #26077 Workpiece installation error compensation amount ○ 22.24 IB-1501278-D 870 ○ M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables No. #30060 - #30068 Reading Setting Coordinate Rotation Parameter Data type or use ○ - Section 22.20 #31001 - #31023 Rotary axis configuration parameter ○ - 22.21 #31100, #31101 Number of reverse run enable blocks, reverse run enable counter ○ - 22.17 #40000 - #40097 Specification of the selected interfering object and interfering model coordinate system offset ○ ○ 22.29 #50000 - #50749 #51000 - #51749 #52000 - #52749 Data of user backup area for R device ○ (*1) ○ (*1) 22.27 #50000 - #51199 ZR device access variables (C80 series only) ○ ○ 22.30 #60000 - #64700 Tool life management ○ ○ (*2) 22.7 #68000 - #68003 Tool management ○ ○ (*2) 22.5 #68011 - #68023 Basic information ○ ○ (*2) #68031 - #68040 Shape information ○ ○ #68051 - #68054 Cutting conditions ○ ○ #68061 - #68072 Additional information ○ ○ #68081 - #68088 Tool life ○ ○ #68101 - #68113 Compensation amount ○ ○ #100000 Parameter No. designation - ○ #100001 Part system No. designation - ○ #100002 Axis No./spindle No. designation - ○ #100010 Parameter value read ○ - #100100 Device type designation - ○ #100101 Device No. designation - ○ #100102 Number of read bytes designation - ○ #100103 Read bit designation - ○ 22.23 22.28 #100110 Reading PLC data ○ - #101001 - #115950+n Extended workpiece coordinate offset data (300-set specification) ○ ○ 22.9 #135001 - #135000+n #136001 - #136000+n #137001 - #137000+n #138001 - #138000+n Tool offset data ○ Also refer to the variables #2001, #10001 and #230001 or larger. ○ 22.6 #230001 - #230000+n Tool offset data ○ Also refer to the variables #2001, #10001 and #135001 or larger. ○ 22.6 (*1) Only for MTB. This cannot be designated by the user. (*2) Some numbers are not available depending on the contents. 871 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.2 System Variables (G Command Modal) Detailed description Using variable Nos. #4001 to #4021, it is possible to read the modal commands which have been issued in previous blocks. Similarly, it is possible to read the modals in the block being executed with variable Nos. #4201 to #4221. Variable No. Function Pre-read block Execution block #4001 #4201 Interpolation mode G00 : 0, G01 : 1, G02 : 2, G03 : 3, G33 : 33 #4002 #4202 Plane selection G17 : 17, G18 : 18, G19 : 19 #4003 #4203 Absolute/incremental G90 : 90, G91 : 91 #4004 #4204 No variable No. #4005 #4205 Feed designation G94 : 94, G95 : 95 #4006 #4206 Inch/metric G20 : 20, G21 : 21 #4007 #4207 Tool radius compensation G40 : 40, G41 : 41, G42 : 42 #4008 #4208 Tool length compensation G43:43, G44:44, G49:49 #4009 #4209 Fixed cycle G80 : 80, G73-74 : 73-74, G76 : 76, G81-89 : 8189 #4010 #4210 Return level G98 : 98, G99 : 99 #4011 #4211 #4012 #4212 Workpiece coordinate system G54-G59 : 54-59, G54.1:54.1 #4013 #4213 Acceleration/deceleration G61-G64 : 61-64, G61.1 : 61.1 #4014 #4214 Macro modal call G66 : 66, G66.1 : 66.1, G67 : 67 #4015 #4215 Normal line control G40.1 : 40.1, G41.1 : 41.1, G42.1 : 42.1 #4016 #4216 #4017 #4217 Constant surface speed G96 : 96, G97 : 97 #4018 #4218 No variable No. #4019 #4219 Mirror image #4020 #4220 #4021 #4221 G50.1:50.1, G51.1:51.1 No variable No. Example: G28 X0 Y0 Z0; G90 G1 X100. F1000; G91 G65 P300 X100. Y100.; M02; O300; #1=#4003; -> Group 3G modal (pre-read) #1=91.0 #2=#4203; -> Group 3G modal (active) #2=90.0 G#1 X#24 Y#25; M99; % IB-1501278-D 872 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.3 System Variables (Non-G Command Modal) Detailed description Using variable Nos. #4101 to #4120, it is possible to read the modal commands which have been issued in previous blocks. Similarly, it is possible to read the modals in the block being executed with variable Nos. #4301 to #4320. Variable No. Modal information Variable No. Modal information Pre-read block Execution block Pre-read Execution #4101 #4301 #4111 #4311 #4102 #4302 #4112 #4312 #4103 #4303 #4113 #4313 Miscellaneous function M #4104 #4304 #4114 #4314 Sequence number N #4105 #4305 #4115 #4315 Program number O (*1) #4106 #4306 #4116 #4316 #4107 #4307 #4117 #4317 #4108 #4308 #4118 #4318 #4109 #4309 #4110 #4310 Tool radius compensation No. D Feedrate F Tool length compensation No. H #4119 #4319 Spindle function S #4120 #4320 Tool function T #4130 #4330 Extended workpiece coordinate system No. P (*1) Programs are registered as files. When the program No. (file name) is read with #4115, #4315, the character string will be converted to a value. (Example 1) The file name "123" is the character string 0×31, 0×32, 0×33, so the value will be (0×31-0×30)*100 + (0×32-0×30)*10 + (0×33-0×30) = 123.0. Note that if the file name contains characters other than numbers, it will be "blank". (Example 2)If the file name is "123ABC", it contains characters other than numbers, so the result will be "blank". 873 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.4 System Variables (Modal Information at Macro Interruption) Detailed description Modal information when control passes to the user macro interruption program can be known by reading system variables #4401 to #4520. The unit specified with a command applies. System variable Modal information #4401 : #4421 G code (group01) : G code (group21) #4507 D code #4509 F code #4511 H code #4513 M code #4514 Sequence number N #4515 Program number O (*1) #4519 S code #4520 T code Some groups are not used. The above system variables are available only in the user macro interrupt program. If they are used in other programs, program error (P241) will occur. (*1) Programs are registered as files. When the program No. (file name) is read with #4515, the character string will be converted to a value. (Example 1) The file name "123" is the character string 0×31, 0×32, 0×33, so the value will be (0×31-0×30)*100 + (0×320×30)*10 + (0×33-0×30) = 123.0. Note that if the file name contains characters other than numbers, it will be "blank". (Example 2) If the file name is "123ABC", it contains characters other than numbers, so the result will be "blank". IB-1501278-D 874 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Modal information affected by user macro interruption If modal information is changed by the interrupt program, it is handled as follows after control returns from the interrupt program to the main program. Returning with M99; The change of modal information by the interrupt program is invalidated and the original modal information is restored. With interrupt type 1, however, if the interrupt program contains a move or miscellaneous function (MSTB) command, the original modal information is not restored. Returning with M99P__ ; The original modal information is updated by the change in the interrupt program even after returning to the main program. This is the same as in returning with M99P__; from a program called by M98, etc. Main program being executed Interrupt program M96Pp1 ; Op1 ; User macro interruption signal (UIT) (Modal change) Modal before interrupt is restored. M99(p2) ; (With Pp2 specified) Np2 ; Modal modified by interrupt program remains effective. Modal information affected by user macro interruption 875 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.5 System Variables (Tool Information) Tool management (#68000 - #68003) Variable No. Item / Description Data range #68000 Tool designation method Method to designate the tool to be read or written 1 to 3 1: In-use tool designation 2: Tool number designation 3: Tool management screen registration number designation #68001 Tool selection No. Designate the tool selection number that matches the setting of "#68000". #68003 #68000 Details of "#68001" Data range 1 ATC magazine num- 0 to 5 ber (Used only when the ATC is added.) 2 Tool No. (T No.) (Tool No. and compensation No. for lathe system) 1 to 99999999 3 Tool management screen registration number 1 to Number of managed tools Top vacant registra- The tool number indicates a vacant line number. tion number on tool 0: No vacant registration number management screen 1 to 999: Vacant registration number Attribute -/W Refer to -/W the "Description" column. 0 to 999 R/- If you command to read data to a write only variable or write to a read only variable, a program error (P241) will occur. If a value exceeding the allowable range is issued, a program error (P35) will occur. (1) Tool designation method (#68000), Tool selection number (#68001) Substitute a value to the parameters "#68000" and "#68001" to designate the tool to be read and written with the parameters "#68011" to "#68111". The tool designation methods are classified into three types as shown below. Tool designation method Details "#68000" setting value In-use tool desig- Reads or writes tool management data of the 1 nation tool in use. ATC magazine No. Tool number designation Tool No. (T No.) Reads or writes tool management data desig- 2 nated with the tool number. Tool manageReads or writes tool management data desig- 3 ment screen reg- nated with the registration number. istration number designation IB-1501278-D "#68001" setting value 876 Tool management screen registration number M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables (a) In-use tool designation (#68000=1) For the in-use tool, when the R register is checked in the order from "1" to "3" shown below, if the value designated in the R register is other than "0", it is judged to be the in-use tool number. Tool life management spindle tool number in machining center system (R12200: 1st part system to R12270: 8th part system) ATC spindle tool number (R10620: magazine 1 to R10660: magazine 5) T code data (R536) "#68001" designates the ATC magazine number. If ATC is not used, this item does not need to be designated. The "#68001" setting value has the meanings shown below. "#68001" setting value Meaning "0" or no "#680001" command Magazine 1 1 to 5 Magazine 1 to magazine 5 Note The in-use tool is determined when "#68000=1" or "#68001" is commanded. To designate the tool which is exchanged after the in-use tool has been determined as an in-use tool, command "#68000=1" or "#68001" again. (b) Tool number designation (#68000=2) "#68001" designates the tool number. In the lathe system, designate the T code (tool number and tool compensation number). (c) Tool management screen registration number designation (#68000=3) "#68001" designates the tool management screen registration number (line number). Note If "#68000" is commanded multiple times, the last designation method will be valid. "#68000" and "#68001" are valid until they are reset. When the power is turned ON or when the system is reset, "0" is set. When #68000 is 2, and when there are multiple tools which have the same tool number and the same tool compensation number as the ones designated by "#68001", the tool that has been found first will be selected. A program error (P245) will occur when: "#68000" is not designated; "#68000=1 ;" is commanded while the in-use tool number is set to "0"; "#68000=1 ;" is commanded while the in-use tool number is not registered on the tool management screen; "#68000=2 ;" is commanded while a read/write command is issued using "#68011" to "#68111" without commanding "#68001"; a tool not registered on the tool management screen with "#68011" is designated during the "#68000=2 ;" command; a write command is issued with "#68011" during the "#68000=2 ;" command; "#68000=3 ;" is commanded while a read/write command is issued using "#68011" to "#68111" without commanding "#68001"; "#68001=0 ;" is commanded. 877 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables (2) Top vacant registration number on tool management screen (#68003) Designating this value reads the top vacant registration number on the tool management screen with "#68003". Use example: Follow the procedure below to measure the compensation amount with the measurement macro, etc. and search for and register a vacant registration number when registering a new tool. 999 [Measurement macro program] : #68000 = 3 ; : Measurement #68001=#68003 ; Searches for a vacant registration number (No.3 in the example above), and designates registration number 3. #68011=999 ; Sets "999" to the tool management data "tool number" of tool management screen registration number 3. Note If no vacant registration number is found because all numbers are registered, "0" is set when "#68003" is read out. When "#68001=#68003;", "#68001" is set to "0", and a program error (P245) will occur. IB-1501278-D 878 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Basic information ("#68011" to "#68023") Variable No. Item / Description Data range Attribute #68011 Tool No. 0 to 99999999 #68012 Name Eight one-byte alphanu- R/W meric characters R/W #68013 Type 0: No setting 1: Ball end mill 2: Flat end mill 3: Drill 4: Radius end mill 5: Chamfering 6: Tapping 7: Face mill 51: Turning 52: Slotting 53: Thread cutting 54: Turning drill 55: Turning tap 0 to 7, 51 to 55 R/W #68014 Usage 0: No setting 1: External diameter 2: Internal diameter 3: Face 0 to 3 R/W #68015 Direction: hand/ro- <Mill tool, turning drill, turning tap> tation 0: CW 1: CCW 2: CW 3 :CW <Turning, slotting, thread cutting> 0: Right hand / Front 1: Left hand / Front 2: Right hand / Rear 3: Left hand / Rear 0 to 3 R/W #68016 Call 0.0 to 999.9 (mm) 0.00 to 99.99 (inch) R/W #68017 Number of blades 0 to 9 R/W #68018 Tool ID Eight one-byte alphanu- R/W meric characters #68019 Supplementary information 0 to 65535 R/W #68020 Conditions 0 to 65535 R/- #68021 Mounting angle 0.0 to 359.999 (degree) R/W #68023 Comb-shaped cutter offset J ±9999.999 (mm) ±999.9999 (inch) R/W If a value exceeding the allowable range is issued, a program error (P35) will occur. 879 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables (1) Tool No. ("#68011") The registered tool cannot be registered. If a tool is registered, the operation will be performed as shown below. Type Operation performed when a registered tool is designated Machining center sys- Life management I tem Life management II Program error (P245) Life management III Program error (P245) The life management specifications are invalid. Program error (P245) Life management I Program error (P245) Lathe system Program error (P245) Life management II Can be registered. The life management specifications are invalid. Can be registered. Example: When an attempt is made to change tool management data "tool number" of No.3 (3rd line) from "11" to "1" in life management II of the machining center system, the setting is as follows. #68000=3 Tool management screen registration number designation #68001=3 Designates No. 3 (3rd line) #68013=1 Tool No. 1 is already registered with No. 1 (1st line), causing a program error (P245). (2) Tool name ("#68012"), Tool ID ("#68018"), Material ("#68053") (a) Read Reads data only with the variable No. designation of the DPRNT command. Example 1: DPRNT [#68012] ; The tool name is read. Example 2: #100=#68012 ; A program error (P243) will occur. (b) Write A string can be designated by enclosing it in parentheses ( ). Example 1: #68012=(MTOOL1) ; Data is written up to the number of valid characters, and the rest is ignored. Example 2: #68012=#0 ; A string is cleared by writing "null" characters. Example 3: #68012= MTOOL1 ; If parentheses are omitted, a program error will occur. (3) Type ("#68013") to tool nose point P ("#68111") A program error will occur in the following case. Operation Operation result Type ("#68013") to tool nose point P ("#68111") is read Program error (P245) or written for the registration number with the tool number unspecified. (4) Compensation amount ("#68103" to "#68111") A program error will occur in the following case. Operation Operation result The compensation amount ("#68103" to "#68111") is Program error (P170) read or written for the tool with the compensation number unspecified. IB-1501278-D 880 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables (5) Tool life ("#68082" to "#68086") A program error will occur in the following case. Operation Operation result The tool life ("#68082" to "#68086") is read or written for Program error (P179) the tool with the tool life group number unspecified in tool life management I and II of the machining center system, or in tool life management II of the lathe system. Shape information ("#68031" to "#68040") Variable No. Item / Description #68031 to #68039 Tool shapes A to I #68040 Tool color 1: Gray 2: Red 3: Yellow 4: Blue 5: Green 6: Light blue 7: Purple 8: Pink Data range Attribute Length: 0 to 9999.999 (mm) 0 to 999.9999 (inch) Angle: 0 to 180.000 (degree) R/W 1 to 8 R/W If a value exceeding the allowable range is issued, a program error (P35) will occur. Cutting conditions ("#68051" to "#68054") Variable No. Item / Description Data range Attribute #68051 Spindle rotation speed S 0 to 99999999 R/W #68052 Feedrate F 0 to 1000000 (mm/min) 0 to 100000 (inch/min) R/W #68053 Material Four one-byte alphanumeric characters R/W #68054 Coolant M code 0 to 99999999 R/W If a value exceeding the allowable range is issued, a program error (P35) will occur. Additional information ("#68061" to "#68072") Variable No. Item / Description Data range Attribute #68061 to #68066 Customize 1 to 6 ±999999999 (*1) R/W #68067 to #68072 Customize 7 to 12 ±9999.999 (*1) R/W (*1) For customize data 1 to 12, the data range varies depending on the data format. If a value exceeding the allowable range is issued, a program error (P35) will occur. 881 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Tool life ("#68081" to "#68088") Variable No. Item / Description Life management I #68081 Group No. (0 to 99999999) #68082 Status (0 to 2) Life management II Attribute Life management III (Not used) R/W R/W #68083 Method (Ones digit: 0 to 2, 10,100s digit: 1 to 2) R/W #68084 Miscellaneous (0 to 65535) R/W #68085 Life time / Number of uses until life limit (0 to 4000 min. / 0 to 65000 sets) R/W #68086 Usage time / Number of uses (0 to 4000 min. / 0 to 65000 sets) R/W #68087 (Not used) (Not used) (Not used) -/- #68088 (Not used) (Not used) (Not used) -/- If an unused variable is commanded, a program error (P241) will occur. If a value exceeding the allowable range is issued, a program error (P35) will occur. IB-1501278-D 882 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Compensation amount ("#68101" to "#68113") Variable No. Item / Description Compensation type I Compensation type II Compensation type III Attribute #68101 No. H (0 to number of tool offset sets) No. H (0 to number of tool offset sets) Tool length compensation No. (0 to number of tool offset sets) R/W #68102 (Not used) No. D (0 to number of tool offset sets) Wear compensation No. (0 to number of tool offset sets) R/W #68103 Tool length (±9999.999999 (mm) ±999.9999999 (inch)) Length dimension (±9999.999999 (mm) ±999.9999999 (inch)) Tool length X (±9999.999999 (mm) ±999.9999999 (inch)) R/W #68104 (Not used) (Not used) Tool length Z (±9999.999999 (mm) ±999.9999999 (inch)) R/W #68105 (Not used) (Not used) Additional axis tool length (±9999.999999 (mm) ±999.9999999 (inch)) R/W #68106 (Not used) Length wear (±9999.999999 (mm) ±999.9999999 (inch)) Wear X (±9999.999999 (mm) ±999.9999999 (inch)) R/W #68107 (Not used) (Not used) Wear Z (±9999.999999 (mm) ±999.9999999 (inch)) R/W #68108 (Not used) (Not used) Additional axis wear (±9999.999999 (mm) ±999.9999999 (inch)) R/W #68109 (Not used) Radius dimension (±9999.999999 (mm) ±999.9999999 (inch)) Tool nose radius (±9999.999999 (mm) ±999.9999999 (inch)) R/W #68110 (Not used) Radius wear (±9999.999999 (mm) ±999.9999999 (inch)) Radius wear (±9999.999999 (mm) ±999.9999999 (inch)) R/W #68111 (Not used) (Not used) Tool nose point P (0 to 9) R/W #68112 (Not used) (Not used) 2nd additional axis tool length (±9999.999999 (mm) ±999.9999999 (inch)) R/W #68113 (Not used) (Not used) 2nd additional axis wear (±9999.999999 (mm) ±999.9999999 (inch)) R/W If an unused variable is commanded, a program error (P241) will occur. If a value exceeding the allowable range is issued, a program error (P35) will occur. 883 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.6 System Variables (Tool Compensation) Detailed description Tool compensation data can be read and set using the variable Nos. Type 1 Type 2 #10001 to #10000+n Variable number range #2001 to #2000+n ○ ○ (*1) ○ Z axis shape (*1) Type 3 #11001 to #11000+n #2201 to #2200+n × ○ (*2) ○ Z axis wear (*2) #16001 to #16000+n #2401 to #2400+n × ○ (*3) ○ Tool nose radius shape (*3) #17001 to #17000+n #2601 to #2600+n × ○ (*4) ○ Tool nose radius wear (*4) #135001 to #135000+n - × × ○ X axis wear #136001 to #136000+n - × × ○ Y axis wear #137001 to #137000+n - × × ○ X axis shape #138001 to #138000+n - × × ○ Y axis shape #230001 to #230000+n - × × ○ Tool nose point (*1) Length dimension (*2) Length wear (*3) Radius dimension (*4) Radius wear "n" in the table corresponds to the tool No. Maximum "n" value is the number of tool compensation sets. The #10000s and #2000s are equivalent functions, however, the maximum value of "n" for #2000 order is "200". When the number of tool offset sets is larger than "200", use the variables of #10000s. The tool compensation data is configured as data with a decimal point in the same way as other variables. When "# 10001=100;" is programmed, "100.000" is set in tool compensation data. Programming example Common variable Tool compensation data #101=100; #10001=#101; #102=#10001; #101=100.0 H1=100.000 #102=100.0 (Example 1) Calculation and tool offset data setting G28 Z0 T01. ; Reference position return #1 M06; Tool change (Spindle T01) #1=#5003 ; Start point memory G00 Z-500 ; Rapid traverse to safe position G31 Z-100. F100.; Skip measurement #10001=#5063-#1 ; G00 H1 G31 Measurement distance calculation and tool compensation data setting #5063 Sensor Note (1) In (Example 1), no consideration is given to the delay in the skip sensor signal. #5003 is the Z axis start point position and #5063 indicates the position at which the skip signal is input while G31 is being executed in the Z axis skip coordinates. IB-1501278-D 884 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.7 System Variables (Tool Life Management) Detailed description Definition of variable Nos. (1) Group number designation #60000 Assign the value to this variable No. to designate the group number of the tool life management data to be read with parameters "#60001" to "#64700". If a group No. is not designated, the data of the group registered first is read. This is valid until reset. When the tool life management III are provided, the group No. other than 1 cannot be used. (2) Tool life management system variable No. (Read) #60001 to #64700 #|a|b|c|d|e| | a | : "6" Fix (Tool life management) | b | c | : Details of data classification Data class Details Remarks 00 For control Refer by data types 05 Group No. Refer by registration No. 10 Tool No. Refer by registration No. 15 Tool data flag Refer by registration No. 20 Tool status Refer by registration No. 25 Life data Refer by registration No. 30 Usage data Refer by registration No. 35 Tool length compensation data Refer by registration No. 40 Tool radius compensation data Refer by registration No. 45 Auxiliary data Refer by registration No. The group No. and life data are common for the group. | d | e | : Registration No. or data type Registration No. 1 to 200 Data type Type Details 1 Number of registered tools 2 Life current value 3 Tool selection No. 4 Number of remaining registered tools 5 Execution signal 6 Cutting time cumulative value (min) 7 Life end signal 8 Life prediction signal 885 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables List of variables Variable No. Item Type Details 60001 Number of regis- Common to systered tools tem Total number of tools registered in each 0 to 200 group. 60002 Life current value For each group (*1) In-use tool usage time / number of uses 0 to 4000min. Usage data of the spindle tool or in-use 0 to 65000 sets tool (#60003) 60003 Tool selection No. In-use tool registration number 0 to 200 Registration number of the spindle tool (the first tool of ST:1 when the spindle tool is not data of the designated group, the first tool of ST:0 when ST:1 is not defined, or the last tool when all tools have reached the end of their lives) 60004 Number of remaining registered tools No. of first registered tool that has not reached its life. 60005 Execution signal "1" when this group is used in the pro0/1 gram being executed. "1" when the group number of spindle tool data matches that of the designated group 60006 Cutting time cumulative value (min) Indicates the time that this group is used (Not used) in the program being executed. 60007 Life end signal 0/1 "1" when lives of all tools in this group have expired. "1" when all registered tools in the designated group reach the end of their lives. 60008 Life prediction signal "1" when a new tool is selected with the 0/1 next command in this group. "1" when there are no tools in use (ST: 1) while there is an unused tool (ST: 0) in the designated group. (*1) Designate group number "#60000". IB-1501278-D Data range 886 0 to 200 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Variable No. Item Type Details For each group / This group's No. registration number (*2) Tool No. of the designated tool Data range 60500 +*** Group No. 1 to 99999999 61000 +*** Tool No. 61500 +*** Tool data Flag Parameters such as usage data count 0 to FF (H) method, length compensation method, tool radius compensation method bit0,1: Tool length compensation data format bit2,3: Tool radius compensation data format 0: Compensation number method 1: Incremental value compensation amount method 2: Absolute value compensation amount method bit4,5: Tool life management method 0: Usage time 1: Number of mounts 2: Number of uses 62000 +*** Tool status Tool usage state 0: Unused tool 1: In-use tool 2: Normal life tool 3: Tool error 1 4: Tool error 2 0 to 4 62500 +*** Life data Life time or No. of lives for each tool 0 to 4000 min. 0 to 65000 sets 63000 +*** Usage data Usage time or No. of uses for each tool 0 to 4000 min. 0 to 65000 sets 63500 +*** Tool length compensation Data Length compensation data set as com- Compensation No. 0 pensation No., absolute value compensa- and after Number of tool comtion amount or increment value pensation sets compensation amount method. Absolute value compensation amount ±999.999 (*1) Incremental value compensation amount ±999.999(*1) 64000 +*** Tool radius compensation data Radius compensation data set as com- Compensation No. 0 pensation No., absolute value compensa- and after tion amount or increment value Number of tool comcompensation amount method. pensation sets Absolute value compensation amount ±999.999 (*1) Incremental value compensation amount ±999.999(*1) 64500 +*** Auxiliary data Spare data 1 to 99999999 0 to 65535 (*2) Designate group number "#60000" / registration number***. However, group number / method / life is data common to groups. 887 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Program example (1) Normal commands #101 = #60001 ; Reads the number of registered tools. #102 = #60002 ; Reads the life current value. #103 = #60003 ; Reads the tool selection No. #60000 = 10 ; Designates the group No. of the life data to be read. Designated group No. is valid until reset. #104 = #60004 ; Reads the remaining number of registered tools in group 10. #105 = #60005 ; Reads the signal being executed in group 10. #111 = #61001 ; Reads the group 10, #1 tool No. #112 = #62001 ; Reads the group 10, #1 status. #113 = #61002 ; Reads the group 10, #2 tool No. % (2) When the group number is not designated: #104 = #60004 ; Reads the remaining number of registered tools in the first registered group. #111 = #61001 ; Reads the #1 tool No. in the first registered group. % (3) When an unregistered group number is designated (group 9999 does not exist): #60000 = #9999 ; Designates the group No. #104 = #60004 ; #104 = -1. (4) When an unused registration number is designated (15 tools for group 10): #60000 = 10 ; Designates the group No. #111 = #61016 ; #111 = -1. (5) When a registration number not defined in the specifications is designated: #60000 = 10 ; #111 = #61017 ; Program error (P241) (6) When tool life management data is registered with G10 command after group No. is designated. #60000 = 10 ; Designates the group No. G10 L3 ; Starts the life management data registration. The group 10 life data is registered through the commands from G10 to G11. P10 LLn NNn ; 10 is the group No., Ln is the life per tool, Nn is the method. TTn ; "Tn" is the tool No. : G11; Registers data in group 10 with the G10 command. #111 = #61001 ; Reads the group 10, #1 tool No. G10 L3 ; Starts the life management data registration. The life data other than group 10 is registered from G10 to G11. P1 LLn NNn ; 1 is the group No., "Ln" is the life per tool, "Nn" is the method. TTn ; "Tn" is the tool No. : IB-1501278-D G11; Registers the life data with the G10 command. (The registered data is deleted.) #111 = #61001 ; Group 10 does not exist. #111 = -1. 888 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Precautions (1) If the tool life management system variable is commanded without designating a group No., the data of the group registered at the head of the registered data will be read. (2) If a non-registered group No. is designated and the tool life management system variable is commanded, "-1" will be read as the data. (3) If an unused registration No. tool life management system variable is commanded, "-1" will be read as the data. (4) Once commanded, the group No. is valid until NC reset. (5) When the tool life management III are provided, the group No. other than 1 cannot be used. 889 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.8 System Variables (Workpiece Coordinate Offset) Detailed description By using variable Nos #5201 to #532n, it is possible to read out the workpiece coordinate system compensation data or to substitute values. Note (1) The number of controllable axes varies depending on the specifications. The last digit of the variable No. corresponds to the control axis No. Coordinate name 1st axis External workpiece offset #5201 2nd axis #5202 3rd axis 4th axis #5203 ..... nth axis #5204 Remarks ..... #520n External workpiece offset specifications are required. G54 #5221 #5222 #5223 #5224 ..... G55 #5241 #5242 #5243 #5244 ..... #522n Workpiece coordinate system offset #524n specifications are required. G56 #5261 #5262 #5263 #5264 ..... #526n G57 #5281 #5282 #5283 #5284 ..... #528n G58 #5301 #5302 #5303 #5304 ..... #530n G59 #5321 #5322 #5323 #5324 ..... #532n Y (Example 1) N1 - 90. N1 G28 X0 Y0 Z0 ; N2 #5221=-20. #5222=-20. ; N3 G90 G00 G54 X0 Y0 ; - 20. W1 N10 #5221=-90. #5222=-10. ; N11 G90 G00 G54 X0Y0 ; X N3 N11 - 10. - 20. W1 G54 workpiece coordinate system defined by N10 G54 workpiece coordinate system defined by N2 M02 ; Basic machine coordinate External workpiece offset (Example 2) G55 Coordinate system before change G54 W2 (G55) W1 (G54) N100 #5221=#5221+#5201 ; #5222=#5222+#5202 ; #5241=#5241+#5201 ; #5242=#5242+#5202 ; #5201=0 #5202=0; Basic machine coordinate system M G55 G54 Coordinate system after change W2 (G55) W1 (G54) This is an example where the external workpiece compensation values are added to the workpiece coordinate (G54, G55) system compensation values without changing the position of the workpiece coordinate systems. IB-1501278-D 890 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.9 System Variables (Extended Workpiece Coordinate Offset) Detailed description #7001 to #890n (48- or 96-set specification) By using variable Nos #7001 to #890n, it is possible to read out the extended workpiece coordinate system compensation data or to substitute values. Note (1) The system variables #7001 to #890n are available up to the valid number of sets. (You can use them for the 300-set specification also, but there are system variables corresponding to up to 96 sets only.) The last digit of the variable No. corresponds to the control axis No. Table 1 of syst to em variables for extended workpiece coordinate system compensation (n=1 to 8) 1st axis to nth axis 1st axis to nth axis 1st axis to nth axis 1st axis to nth axis P1 #7001 to #700n P25 #7481 to #748n P49 #7961 to #796n P73 #8441 to #844n P2 #7021 to #702n P26 #7501 to #750n P50 #7981 to #798n P74 #8461 to #846n P3 #7041 to #704n P27 #7521 to #752n P51 #8001 to #800n P75 #8481 to #848n P4 #7061 to #706n P28 #7541 to #754n P52 #8021 to #802n P76 #8501 to #850n P5 #7081 to #708n P29 #7561 to #756n P53 #8041 to #804n P77 #8521 to #852n P6 #7101 to #710n P30 #7581 to #758n P54 #8061 to #806n P78 #8541 to #854n P7 #7121 to #712n P31 #7601 to #760n P55 #8081 to #808n P79 #8561 to #856n P8 #7141 to #714n P32 #7621 to #762n P56 #8101 to #810n P80 #8581 to #858n P9 #7161 to #716n P33 #7641 to #764n P57 #8121 to #812n P81 #8601 to #860n P10 #7181 to #718n P34 #7661 to #766n P58 #8141 to #814n P82 #8621 to #862n P11 #7201 to #720n P35 #7681 to #768n P59 #8161 to #816n P83 #8641 to #864n P12 #7221 to #722n P36 #7701 to #770n P60 #8181 to #818n P84 #8661 to #866n P13 #7241 to #724n P37 #7721 to #772n P61 #8201 to #820n P85 #8681 to #868n P14 #7261 to #726n P38 #7741 to #774n P62 #8221 to #822n P86 #8701 to #870n P15 #7281 to #728n P39 #7761 to #776n P63 #8241 to #824n P87 #8721 to #872n P16 #7301 to #730n P40 #7781 to #778n P64 #8261 to #826n P88 #8741 to #874n P17 #7321 to #732n P41 #7801 to #780n P65 #8281 to #828n P89 #8761 to #876n P18 #7341 to #734n P42 #7821 to #782n P66 #8301 to #830n P90 #8781 to #878n P19 #7361 to #736n P43 #7841 to #784n P67 #8321 to #832n P91 #8801 to #880n P20 #7381 to #738n P44 #7861 to #786n P68 #8341 to #834n P92 #8821 to #882n P21 #7401 to #740n P45 #7881 to #788n P69 #8361 to #836n P93 #8841 to #884n P22 #7421 to #742n P46 #7901 to #790n P70 #8381 to #838n P94 #8861 to #886n P23 #7441 to #744n P47 #7921 to #792n P71 #8401 to #840n P95 #8881 to #888n P24 #7461 to #746n P48 #7941 to #794n P72 #8421 to #842n P96 #8901 to #890n 891 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables #101001 to #11595n (300-set specification) By using variable Nos #101001 to #11595n, it is possible to read out the extended workpiece coordinate system compensation data or to substitute values. Note (1) The system variables #101001 to #11595n are available when the 300-set specification is enabled. If you use the system variables #101001 to #11595n when the 300-set specification is disabled, the program error (P241) will occur. The last digit of the variable No. corresponds to the control axis No. Table 2 of syst to em variables for extended workpiece coordinate system compensation (n=1 to 8) 1st axis to nth axis P1 #101001 to #10100n P2 #101051 to #10105n P3 #101101 to #10110n P4 #101151 to #10115n P5 #101201 to #10120n P6 #101251 to #10125n P7 #101301 to #10130n P8 #101351 to #10135n : : : : P298 #115851 to #101585n P299 #115901 to #101590n P300 #118951 to #101595n 22.10 System Variables (External Workpiece Coordinate Offset) Detailed description The workpiece coordinate system compensation amount can be read using variables #2501 and #2601. By substituting a value in these variable Nos., the workpiece coordinate system compensation amount can be changed. System variable No. IB-1501278-D External workpiece coordinate system offset amount #2501 1st axis #2601 2nd axis 892 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.11 System Variables (Position Information) Detailed description Using variable Nos. #5001 to #5160+n, it is possible to read the end point coordinates, machine coordinates, workpiece coordinates, skip coordinates, tool position compensation amount and servo deviation amounts in the last block. Position information Axis No. 1 2 3 ... n Reading during movement End point coordinate of the last block #5001 #5002 #5003 ... #5000+n Valid Machine coordinate #5021 #5022 #5023 ... #5020+n Invalid Workpiece coordinate #5041 #5042 #5043 ... #5040+n Invalid #5061 #5062 #5063 ... #5060+n Valid #5161 #5162 #5163 ... #5160+n Skip coordi- Parameter 0 nate "#8713" Workpiece coordinate system 1 Feature coordinate / Workpiece installation coordinate Feature coordinate/Workpiece installation coordinate Tool position compensation amount #5081 #5082 #5083 ... #5080+n Invalid Servo deviation amount #5101 #5102 #5103 ... #5100+n Valid Macro interruption stop Start point coordinates #5121 #5122 #5123 ... #5120+n Valid Macro interruption stop End point coordinates #5141 #5142 #5143 ... #5140+n Valid Note The number of axes which can be controlled differs according to the specifications. The last digit of the variable No. corresponds to the control axis No. Basic machine coordinate system M Workpiece coordinate system W G00 G01 Read command [End point coordinates] Workpiece coordinate system W [Workpiece coordinates] [Machine coordinates] M 893 Machine coordinate system IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables (1) The position of the end point coordinates is position in the workpiece coordinate system. (2) The end point coordinates, skip coordinates and servo deviation amounts can be read even during movement. However, it must first be checked that movement has stopped before reading the machine coordinates and the workpiece coordinates. (3) The skip coordinates indicates the position where the skip signal is turned ON in the G31 block. If the skip signal does not turn ON. they will be the end point position. (For further details, refer to the section on Automatic Tool Length Measurement.) Read Command Gauge, etc. Skip coordinates value (4) The end point coordinates indicate the tool nose position regardless of the tool compensation and other such factors. On the other hand, the machine coordinates, workpiece coordinates and skip coordinates indicate the tool reference point position with consideration given to tool compensation. Skip signal G31 F (feedrate) Workpiece coordinate system W [Input coordinates of skip signal] [Workpiece coordinates] M [Machine coordinates] For "●", check stop and then proceed to read. For "○", reading is possible during movement. IB-1501278-D 894 Machine coordinate system M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Note Skip coordinate value is the position on the workpiece coordinate system, feature coordinate system, or workpiece installation coordinate system. For #5061 to #5060+n, when the parameter "#8713 Skip coord. Switch" is set to "0", it is the position on the workpiece coordinate system, and when set to "1", it is the position on the feature coordinate system or workpiece installation coordinate system. For #5161 to #5160+n, it is the position on the workpiece coordinate system while the inclined surface machining command or workpiece installation compensation is OFF. For feature coordinate system, the skip coordinate value is on "the actual position where the tool length compensation is included " regardless of the setting of the parameter "#1287 ext23/bit1, bit2 (inclined surface coordinate display)". The values in the work installation coordinate system can be read for the orthogonal axes for 5-axis machining that have been set by the rotary axis configuration parameters. For the other axes, the values in the workpiece coordinate system are read. When the workpiece installation error compensation is OFF, the values in the skip coordinate system are read for all the axes. The coordinate value in variable Nos. #5061 to #5060+n or #5161 to #5160+n memorize the moments when the skip input signal during movement was input and so they can be read at any subsequent time. For details, refer to "21.2 Skip Function ; G31". When the parameter "#1366 skipExTyp" (Multi-part system simultaneous skip command) is set to "1", the skip coordinate value will be "0", even if G31 command is given in one-part system or G31 command is given in only one of the multiple part systems. (Example 1) Example of workpiece position measurement An example to measure the distance from the measured reference position to the workpiece edge is shown below. Argument <Local variable> O9031 F(#9) 200 X(#24)100.000 Y(#25)100.000 Z(#26) - 10.000 Main program G65 P9031 X100. Y100. Z-10. F200; To subprogram <Common variable> #101 87.245 #102 87.245 #103 123.383 Skip input Start point N3 Z N8 N4 N1 #180=#4003; N2 #30=#5001 #31=#5002; N3 G91 G01 Z#26 F#9; N4 G31 X#24 Y#25 F#9; N5 G90 G00 X#30 Y#31; N6 #101=#30- #5061 #102=#31- #5062; N7 #103=SQR #101*#101+#102*#102 ; N8 G91 G01Z - #26; N9 IF #180 EQ 91 GOTO 11; N10 G90; N11 M99; #102 #103 N5 #101 Y X #101 X axis measurement amount N1 G90/G91 modal recording #102 Y axis measurement amount N2 X, Y start point recording #103 Measurement linear segment N3 amount Z axis entry amount N4 X, Y measurement (Stop at skip input) #5001 X axis measurement start point N5 Return to X, Y start point #5002 Y axis measurement start point N6 X, Y measurement incremental value calculation N7 Measurement linear segment calculation #5061 X axis skip input point N8 Z axis escape #5062 Y axis skip input point N9,N10 G90/G91 modal return N11 Main program return 895 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables (Example 2) Reading of skip input coordinates (a) Skip signal -X - 150 - 25 - 75 N1 G91 G28 X0 Y0; N2 G90 G00 X0 Y0; N3 X0 Y- 100.; N4 G31 X - 150. Y - 50. F80; N5 #111=#5061#112=#5062; N6 G00 Y0; N7 G31 X0; N8 #121=#5061#122=#5062; N9 M02; Y X - 50 - 75 - 100 -Y (a) #111=-75.+ε #112=-75.+ε #121=-25.+ε #122=-75.+ε ε is the error caused by response delay. (For details, refer to "21.2 Skip Function ; G31".) #122 is the N4 skip signal input coordinates as there is no Y command at N7. IB-1501278-D 896 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.12 System Variables (Alarm) Detailed description The NC unit can be forcibly set to the alarm state by using variable No. #3000. #3000= 70 (CALL #PROGRAMMER #TEL #530) ; 70 Alarm No. CALL #PROGRAMMER #TEL #530 Alarm message Any alarm number from 1 to 9999 can be specified. The alarm message must be written in 31 or less characters. NC alarm 3 signal (program error) is output. The "P277: MACRO ALM MESG" appears in the <ALARM> column on "DIAG 1." screen and the alarm message " (CALL #PROGRAMMER #TEL #530)" and the alarm No. (70) will appear in the <Operator massage>. Example of program (alarm when #1 = 0) <ALARM> DIAG 1. IF[#1 NE 0]GOTO 100 ; #3000=70 ( CALL #PROGRAMMER #TEL #530 ); Stops with NC alarm N100 P277: MACRO ALM MESG <Operator message> CALL #PROGRAMMER #TEL #530 70 Note (1) If zero or any number greater than 9999 is specified for the alarm No., the number will be invalid and it will not display. However, the operation will be in the alarm status, and the specified alarm message will appear. (2) Specify the alarm message by enclosing it in round parentheses after the alarm number. If there is any character string between the number and the alarm message enclosed in round parentheses, the alarm message will be invalid and it will not display. However, the operation will be in the alarm status, and the specified alarm No. will appear. (3) When 32 or more characters are specified for the alarm message, characters after the 32nd character will not display. (4) Spaces included in an alarm message character string are ignored, and will not display. To split the character string insert a character such as "." (period). 897 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.13 System Variables (Message Display and Stop) Detailed description By using variable No. #3006, the operation stops after the previous block is executed and, if message display data is commanded, the corresponding message and the stop No. will be indicated on the operator message area. #3006 = 1( TAKE FIVE ); 1 to 9999 Stop No. (When Nos. other than 1 - 9999 are set, the command will be invalidated.) TAKE FIVE Message (Nothing will be displayed if no message is designated.) The message should be written in 31 or less characters and should be enclosed by round parentheses. 22.14 System Variables (Cumulative Time) Detailed description The integrating time during the power is turned ON or the automatic start is running, can be read or values can be substituted by using variable Nos. #3001 and #3002. Type Variable No. Unit Power-on 3001 1ms Automatic start 3002 Contents when power Initialization of conis switched on tents Same as when power is switched off Substitute values to variables Count condition At all times while power is ON In-automatic start The cumulative time is reset to "0" at approximately 2.44 × 1011ms (approximately 7.7 years). O9010 G65P9010T (allowable time) ms ; To sub-program #3001=0 ; WHILE #3001LE#20 DO1 ; END1 : M99 ; Entered in local variable #20 Local variable T#20 IB-1501278-D 898 Allowable time portion: DO1 to END1 is repeated and when allowable time is reached, operations jumps to M99. M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.15 System Variables (Time Read Variables) Detailed description The following operations can be carried out using the system variable extension for the user macro time. (1) By adding time information system variable #3011 and #3012, the current date (#3011) and current time (#3012) can be read and written. (2) By adding parameter #1273/bit1, the unit (millisecond unit/hour unit) of the system variable "#3002" (cumulative time during automatic start) can be changed. Variable No. Details #3001 The cumulative time during power ON can be read and the value can be substituted. The unit is millisecond. #3002 The cumulative time during automatic start can be read and the value can be substituted. The unit can be changed between millisecond and hour with parameter #1273/bit1. #3011 The current date can be read and written. YYYY/MM/DD is read as a YYYYMMDD value. If a value "YYYYMMDD" is written, it is set to YY/MM/DD (the year is indicated by the last two digits). Command range for year/ Year (YYYY): 2000 to 2099 month/day setting Month (MM): 1 to 12 Day (DD): 1 to maximum number of days in one month #3012 The current time can be read and written. HH/MM/SS is read as a value "HHMMSS". When a value "HHMMSS" is written in, it will be set as HH/MM/SS. Command range for time setting Hour (HH): 0 to 23 (24-hour system) Minute (MM): 0 to 59 Second (SS): 0 to 59 (3) The cumulative time is reset to "0" at approximately 2.44 × 1011ms (approximately 7.7 years). (4) If a negative value or a value exceeding 244335917226 milliseconds (67871.08811851 hours for #3002 time designation) is set for the cumulative time, a program error (P35) will occur. (5) If a value exceeding the command range is set for the date or time, a program error (P35) will occur. (6) Always set the month/date/hour/minute/second as a two-digit value when setting the date and time. If the value only has one digit, always add 0. (February 14, 2001 => #3011= 20010214 ;, etc.) 899 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Program example Example of use (#3011, #3012) (Example 1) To read the current date (February 14, 2001) in common variable #100 #100 = #3011 ; (20010214 is inserted in #100) (Example 2) To write current time (18 hours, 13 minutes, 6 seconds) into system variable #3012 #3012 = 181306 ; (The command value cumulative time #2: time is set to 18:13:06.) (Example 3) By setting the following program example, the machining start/end time (year/month/date/hour/minute/ second) can be viewed. #100=#3011 ; => Machining start year/month/date #101=#3012 ; => Machining start hour/minute/second G28 X0 Y0 Z0 ; G92 ; G0 X50. ; : : : #102=#3011 ; #103=#3012 ; M30 ; => Machining end year/month/date => Machining end hour/minute/second Precautions Limits and precautions for using time reading variable (1) #3011 reads the date as an eight-digit value, so the difference between the two dates read in will not be the difference of days. (2) #3012 reads the time as a six-digit value, so the difference between the two times read in will not be the difference of hours. IB-1501278-D 900 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.16 System Variables (Machining Information) Detailed description Contents of variable No. "#3003" By substituting the values below in variable No. #3003, it is possible to suppress single block stop in the subsequent blocks or to advance to the next block without waiting for the miscellaneous function (M, S, T, B) finish (FIN) signal. #3003/bit Function Set to "1" Inhibits stop. Set to "0" 0 Inhibition of single block stop 1 Inhibition of miscellaneous function Does not wait for the signal. Waits for the signal. complete signal waiting 2 Prohibition of program check reverse run Prohibits reverse run. Does not inhibit stop. Allows reverse run. 3 (Not used) - - 4 (Not used) - - 5 (Not used) - - 6 (Not used) - - 7 (Not used) - - Note (1) Variable No. #3003 is set to zero by reset. Contents of variable No. "#3004" By substituting the values below in variable No. #3004, it is possible to make the feed hold, feedrate override and G09 functions either valid or invalid in the subsequent blocks. #3004/bit Function Set to "1" Set to "0" 0 Automatic operation pause OFF Invalid Valid 1 Cutting override OFF Invalid Valid 2 G09 check OFF Invalid Valid 3 (Not used) - - 4 Dry run invalid Invalid Valid 5 (Not used) - - 6 (Not used) - - 7 (Not used) - - Note (1) Variable No. #3004 is set to zero by reset. (2) The functions are valid when the above bits are 0, and invalid when they are 1. (3) When the feed hold is set to invalid with #3004, the following will occur when the feed hold switch is pressed. During thread cutting, block stop will be carried out at the end of the next block of the block where thread cutting is completed. During tapping with tap cycle, block stop will be carried out after the operation of R point return. In the case other than above, block stop will be carried out after the termination of the currently executing block. 901 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.17 System Variables (Reverse Run Information) Detailed description Variable No. Details Range #31100 Number of available blocks for reverse run Usage +1 added number of the blocks that retained the reverse run information while the "Reverse run control mode" signal was ON 0 to 201 #31101 Counter of available blocks for reverse run Number of available blocks for reverse run (value of #31100) when the "Reverse run" signal is turned ON to start. Turns "0" when the forward run has been executed for all the blocks. Displays "0" during normal operation. 0 to 201 22.18 System Variables (Number of Workpiece Machining Times) Detailed description The number of workpiece machining times can be read using variables #3901 and #3902. By substituting a value in these variable Nos., the number of workpiece machining times can be changed. Variable No. Type Data setting range #3901 Number of workpiece machining times 0 to 999999 #3902 Maximum workpiece value Note (1) The number of workpiece machining times must be a positive value. 22.19 System Variables (Mirror Image) Detailed description By reading variable No. #3007, it is possible to ascertain the status of mirror image of the each axis at the point. The axis corresponds to each bit of "#3007" as shown below. 0: Mirror image invalid 1: Mirror image valid The number of axes varies depending on your machine's specifications. #3007 Bit 15 14 13 12 11 10 9 8 nth axis IB-1501278-D 902 7 6 5 4 3 2 1 0 8 7 6 5 4 3 2 1 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.20 System Variables (Coordinate Rotation Parameter) Detailed description The following variables can be read by the system variables of the variable command. When an arbitrary axis is exchanged, this data is read in the axis arrangement that is set after the axis exchange has been completed. Note that writing is not possible onto these variables. Variable No. Parameter No. Description #30060 #8621 Control axis No. on the coordinate rotation plane (horizontal axis) #30061 #8622 Control axis No. on the coordinate rotation plane (vertical axis) #30062 #8623 Coordinate rotation center (horizontal axis) #30063 #8624 Coordinate rotation center (vertical axis) #30064 #8627 Coordinate rotation angle #30065 - SIN data for the coordinate rotation angle [SIN(Coordinate rotation angle)] #30066 - COS data for the coordinate rotation angle [COS(Coordinate rotation angle)] #30067 #8625 Coordinate rotation vector (horizontal axis) #30068 #8626 Coordinate rotation vector (vertical axis) 903 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.21 System Variables (Rotary Axis Configuration Parameter) Detailed description The following rotary axis configuration parameters can be read by the system variables of the variable command. By substituting a value in these variables, the setting value of rotary axis configuration parameter can be changed. Variable No. IB-1501278-D Parameter #31001 #7903 G92_CRD Origin zero set coordinate selection #31002 #7904 NO_TIP Tool handle feed function selection #31003 #7920 SLCT_T1 Rotary axis selection (Base-side rotary axis of tool rotation type) #31004 #7923 DIR_T1 Rotation direction (Base-side rotary axis of tool rotation type) #31005 #7924 COFST1H Horizontal axis rotation center offset (Base-side rotary axis of tool rotation type) #31006 #7925 COFST1V Vertical axis rotation center offset (Base-side rotary axis of tool rotation type) #31007 #7926 COFST1T Height axis rotation center offset (Base-side rotary axis of tool rotation type) #31008 #7930 SLCT_T2 Rotary axis selection (Tool-side rotary axis of tool rotation type) #31009 #7933 DIR_T2 Rotation direction (Tool-side rotary axis of tool rotation type) #31010 #7934 COFST2H Horizontal axis rotation center offset (Tool-side rotary axis of tool rotation type) #31011 #7935 COFST2V Vertical axis rotation center offset (Tool-side rotary axis of tool rotation type) #31012 #7936 COFST2T Height axis rotation center offset (Tool-side rotary axis of tool rotation type) #31013 #7940 SLCT_W1 Rotary axis selection (Base-side rotary axis of table rotation type) #31014 #7943 DIR_ W1 Rotation direction (Base-side rotary axis of table rotation type) #31015 #7944 COFSW1H Horizontal axis rotation center offset (Base-side rotary axis of table rotation type) #31016 #7945 COFSW1V Vertical axis rotation center offset (Base-side rotary axis of table rotation type) #31017 #7946 COFSW1T Height axis rotation center offset (Base-side rotary axis of table rotation type) #31018 #7950 SLCT_W2 Rotary axis selection (Workpiece-side rotary axis of table rotation type) #31019 #7953 DIR_W2 Rotation direction (Workpiece-side rotary axis of table rotation type) #31020 #7954 COFSW2H Horizontal axis rotation center offset (Workpiece-side rotary axis of table rotation type) #31021 #7955 COFSW2V Vertical axis rotation center offset (Workpiece-side rotary axis of table rotation type) #31022 #7956 COFSW2T Height axis rotation center offset (Workpiece-side rotary axis of table rotation type) #31023 #7912 NO_MANUAL Selection of manual feed for 3-dimensional 904 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.22 System Variables (Normal Line Control Parameter) Detailed description The normal line control parameter can be read or written using variable Nos. "#1900" and "#1901". Variable No. Details #1900 #8041 C-rot.R (Data with decimal point) #1901 #8042 C-ins.R (Data with decimal point) 905 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.23 System Variables (Parameter Reading) Function and purpose Parameter data can be read in with the system variables. Variable No. Application #100000 Parameter No. designation #100001 Part system No. designation #100002 Axis No./spindle No. designation #100010 Parameter value read Detailed description The parameter values are read in with the following four blocks using these four system variables. #100000 = 1001 ; Designates the parameter No. #100001 = 1 ; Designates the part system No. #100002 = 1 ; Designates the axis No./spindle No. #100 = #100010; Reads the parameter value. Parameter No. designation (#100000) The parameter to be read in is designated by substituting the parameter No. in this system variable. If the parameters are read without designating this No., the parameters will be read in the same manner as if the minimum parameter No. (#1) is designated. Once designated, the setting is held until the parameter No. is designated again or until it is reset. A program error (P39) will occur if a nonexistent parameter No. is set. Part system No. designation (#100001) (1) System variable for part system No. designation The part system No. of the parameter to be read in is designated by substituting an index value for this system variable. This designation will be ignored when reading in parameters that are not in a specific part system. If the parameters are read without designating this No., the parameters will be read in the same manner as if the index value 0 (part system in running program) is designated. Once designated, the setting is held until the part system No. is designated again or until it is reset. A program error (P39) will occur if a nonexistent part system No. is set. (2) Index values IB-1501278-D Index values Parameters per part system 0 Running part system 1 1st part system 2 2nd part system 3 - : - 9 - 10 PLC axis 906 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Axis No. /spindle No. designation (#100002) (1) System variable for axis or spindle No. designation The axis or spindle No. of the parameter to be read in is designated by substituting an index value for this system variable. This designation will be ignored when reading in parameters that are neither for a specific axis nor spindle. The axis parameter index value is the value set in the part system designated with #100001. Thus, when reading parameters that are not in the designated part system, the part system No. must be designated again. The spindle parameter's index value is not affected by the part system designation. If the parameters are read without designating this number, the parameters will be read in the same manner as when the index value 1 (1st axis/1st spindle in the designated part system) is designated. Once designated, the setting is held until the index value is designated again or until it is reset. A program error (P39) will occur if a nonexistent axis/spindle No. is set. (2) Index values Index values Axis parameter Spindle parameter 1 1st axis 1st spindle 2 2nd axis 2nd spindle 3 3rd axis 3rd spindle 4 4th axis 4th spindle 5 5th axis - 6 6th axis - Reading the parameters (#100010) The designated parameter data is read with this system variable. Data to be read as follows, depending on the parameter type. Type Read in data Numeric value The values displayed on the Parameter screen are output. Text ASCII codes are converted into decimal values. 907 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Program example (1) To read the parameter "#1002 axisno (number of axes)" for each part system: #100000 = 1002 ; Designates [#1002]. #100001 = 1 ; Designates [1st part system]. #101 = #100010; Reads the number of axes in 1st part system. #100000 = 1002 ; Designates [#1002]. (can be omitted since parameter No. is same) #100001 = 2 ; Designates [2nd part system]. #102 = #100010; Reads the number of axes in 2nd part system. #100001 = 5 ; Designates [5th part system]. (The program error (P39) will occur.) #100001 = 10 ; Designates [PLC axis]. #110 = #100010; Reads the number of PLC axes. (2) To read the axis parameter "#2037 G53ofs (#1 reference position)": [Conditions] #2037 G53ofs 1 part systems 2 part systems <1st axis> <2nd axis> <1st axis> <2nd axis> 100.000 200.000 300.000 400.000 [1st part system program] #100002 = 1 ; Designates [1st axis]. #100000 = 2037 ; Designates [#2037]. #101 = #100010; Reads the [#1 reference point] for the 1st axis. (#101=100.000) #100002 = 2 ; Designates [2nd axis]. #102 = #100010; Reads the [#2 reference point] for the 1st axis. (#102=200.000) #100001 = 2 ; Designates [2nd part system]. #100002 = 1 ; Designates [1st axis]. #201 = #100010; Reads the [#2 reference position] for the 1st axis in the 1st part system. (#201=300.000) [2nd part system program] #100002 = 1 ; Designates [1st axis]. IB-1501278-D #100000 = 2037 ; Designates [#2037]. #101 = #100010; Reads the [#1 reference point] for the 1st axis. (#101=300.000) #100002 = 2 ; Designates [2nd axis]. #102 = #100010; Reads the [#2 reference point] for the 1st axis. (#102=400.000) #100001 = 1 ; Designates [1st part system]. #100002 = 1 ; Designates [1st axis]. #201 = #100010; Reads the [#1 reference position] for the 1st axis in the 1st part system. (#201=100.000) 908 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables (3) To read the parameter for each part system, axis, or spindle: #100002 = 1 ; Designates [1st spindle]. #100000 = 3001 ; Designates [#3001]. #101 = #100010; Reads the [#3001 slimt1 (Number of limit rotation gears 00)] for 1st spindle. #100000 = 3002 ; Designates [#3002]. #102 = #100010; Reads the [#3002 slimt2 (Number of limit rotation gears 01)] for 1st spindle. #100002 = 2 ; Designates [2nd spindle]. #100000 = 3001 ; Designates [#3001]. #201 = #100010 ; Reads the [#3001 slimt1 (Number of limit rotation gears 00)] for 2nd spindle. #100000 = 3002 ; Designates [#3002]. #202 = #100010; Reads the [#3002 slimt2 (Number of limit rotation gears 01)] for 2nd spindle. (4) To read the text type parameter "#1169 system name" (part system name): [Conditions] <1st part system> <2nd part system> #1169 system name SYS1 SYS2 #100000 = 1169 ; Designates #1169. #100001 = 1 ; Designates 1st part system. #101 = #100010; This will be #101 = 1398362929 (0x53595331). Precautions (1) The number of part systems, axes and spindles is set at the maximum number specified by the model. (2) The inch/metric changeover function for the setting and display is valid for the readout data. (3) The machining condition parameter group cannot set the parameters from the program using the G10 command, and cannot read the parameters using the system variables ("#100000" and later). 909 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.24 System Variables (Workpiece Installation Error Compensation Amount) Detailed description Using the system variables below, read/write of the workpiece installation error compensation amounts is enabled. Common No.01 No.02 No.03 No.04 No.05 No.06 No.07 Workpiece installation error compensation amount ∆x #26000 #26010 #26020 #26030 #26040 #26050 #26060 #26070 Workpiece installation error compensation amount ∆y #26001 #26011 #26021 #26031 #26041 #26051 #26061 #26071 Workpiece installation error compensation amount ∆z #26002 #26012 #26022 #26032 #26042 #26052 #26062 #26072 Workpiece installation error compensation amount ∆a - #26013 #26023 #26033 #26043 #26053 #26063 #26073 Workpiece installation error compensation amount ∆b - #26014 #26024 #26034 #26044 #26054 #26064 #26074 Workpiece installation error compensation amount ∆c - #26015 #26025 #26035 #26045 #26055 #26065 #26075 Primary rotary axis position #26006 #26016 #26026 #26036 #26046 #26056 #26066 #26076 Secondary rotary axis position #26007 #26017 #26027 #26037 #26047 #26057 #26067 #26077 (Note 1) The primary rotary axis position corresponds with the axis set by the parameter #7942, and the secondary rotary axis position corresponds with the axis set by the parameter #7952. (Note 2) If the primary and secondary rotary axis positions are not of the table-side rotary axes, the set values are ignored. (Note 3) The setting ranges are the same as those set in the workpiece installation error setting screen. (Note 4) If the system variables #26000 to #26077 are written during workpiece installation error compensation, the program error (P545) will occur. IB-1501278-D 910 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.25 System Variables (Macro Interface Input (PLC -> NC)) Function and purpose The status of the interface input signals can be ascertained by reading out the values of variable Nos. #1000 to #1035, #1200 to #1295. Note The interface output signals can be sent by substituting values in variable Nos. #1100 to #1135, #1300 to #1395. (For details of the system variables for the output signals, refer to "22.26 System Variables (Macro Interface Output (NC -> PLC))".) Example of 1st part system (a) #1032 (R6436, R6437) #1132 (R6372, R6373) #1000 #1100 #1031 #1131 (c) #1033 (R6438, R6439) #1133 (R6374, R6375) #1200 #1300 #1231 #1331 #1134 (R6376, R6377) #1034 (R6440, R6441) #1232 #1332 #1263 #1363 #1135 (R6378, R6379) #1035 (R6442, R6443) (a) Input signal (b) #1264 #1364 #1295 #1395 (b) Output signal 911 (c) Macro instructions IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Detailed description Variable Nos. #1000 to #1035, #1200 to #1295 are for readout only, and nothing can be placed in the left side member of their operation formula. Input here refers to input to the NC. Whether it is per part system or common between part systems depends on the MTB specifications (parameter "#1230 set02/bit07"). Data unit (32 bits) All the input signals from #1000 to #1031 can be read at once by reading out the value of variable No. #1032. The input signals from #1200 to #1231, #1232 to #1263, and #1264 to #1295 can be read by reading out the values of variable Nos. #1033 to #1035. The data of the 1st part system ($1) to the 8th part system ($8) is as follows. Interface input signal System variable No. of points $1 $2 $3 $4 $5 $6 $7 $8 #1032 32 R6436, R6437 R6444, R6445 R6452, R6453 R6460, R6461 R6468, R6469 R6476, R6477 R6484, R6485 R6492, R6493 #1033 32 R6438, R6439 R6446, R6447 R6454, R6455 R6462, R6463 R6470, R6471 R6478, R6479 R6486, R6487 R6494, R6495 #1034 32 R6440, R6441 R6448, R6449 R6456, R6457 R6464, R6465 R6472, R6473 R6480, R6481 R6488, R6489 R6496, R6497 #1035 32 R6442, R6443 R6450, R6451 R6458, R6459 R6466, R6467 R6474, R6475 R6482, R6483 R6490, R6491 R6498, R6499 IB-1501278-D 912 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Bit unit The input signal has only two values: "0" and "1". Part system $1 $2 $3 $4 $5 $6 $7 $8 R device R6436R6443 R6444R6451 R6452R6459 R6460R6467 R6468R6475 R6476R6483 R6484R6491 R6492R6499 If the value is common between part systems, refer to the column of the 1st part system ($1). Interface input signal register System variable No. of points $1 $2 $3 $4 $5 $6 $7 $8 #1000 1 R6436/ bit0 R6444/ bit0 R6452/ bit0 R6460/ bit0 R6468/ bit0 R6476/ bit0 R6484/ bit0 R6492/ bit0 #1001 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1002 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1003 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1004 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1005 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1006 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1007 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1008 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1009 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1010 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1011 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1012 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1013 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1014 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1015 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 #1016 1 R6437/ bit0 R6445/ bit0 R6453/ bit0 R6461/ bit0 R6469/ bit0 R6477/ bit0 R6485/ bit0 R6493/ bit0 #1017 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1018 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1019 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1020 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1021 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1022 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1023 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1024 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1025 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1026 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1027 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1028 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1029 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1030 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1031 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 913 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables IB-1501278-D Interface input signal register System variable No. of points $1 $2 $3 $4 $5 $6 $7 $8 #1200 1 R6438/ bit0 R6446/ bit0 R6454/ bit0 R6462/ bit0 R6470/ bit0 R6478/ bit0 R6486/ bit0 R6494/ bit0 #1201 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1202 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1203 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1204 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1205 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1206 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1207 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1208 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1209 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1210 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1211 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1212 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1213 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1214 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1215 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 #1216 1 R6439/ bit0 R6447/ bit0 R6455/ bit0 R6463/ bit0 R6471/ bit0 R6479/ bit0 R6487/ bit0 R6495/ bit0 #1217 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1218 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1219 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1220 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1221 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1222 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1223 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1224 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1225 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1226 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1227 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1228 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1229 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1230 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1231 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 914 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Interface input signal register System variable No. of points $1 $2 $3 $4 $5 $6 $7 $8 #1232 1 R6440/ bit0 R6440/ bit0 R6448/ bit0 R6456/ bit0 R6472/ bit0 R6480/ bit0 R6488/ bit0 R6496/ bit0 #1233 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1234 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1235 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1236 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1237 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1238 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1239 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1240 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1241 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1242 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1243 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1244 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1245 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1246 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1247 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 #1248 1 R6441/ bit0 R6441/ bit0 R6449/ bit0 R6457/ bit0 R6473/ bit0 R6481/ bit0 R6489/ bit0 R6497/ bit0 #1249 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1250 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1251 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1252 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1253 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1254 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1255 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1256 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1257 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1258 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1259 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1260 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1261 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1262 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1263 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 915 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables IB-1501278-D Interface input signal register System variable No. of points $1 $2 $3 $4 $5 $6 $7 $8 #1264 1 R6442/ bit0 R6450/ bit0 R6458/ bit0 R6466/ bit0 R6474/ bit0 R6482/ bit0 R6490/ bit0 R6498/ bit0 #1265 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1266 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1267 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1268 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1269 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1270 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1271 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1272 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1273 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1274 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1275 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1276 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1277 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1278 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1279 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 #1280 1 R6443/ bit0 R6451/ bit0 R6459/ bit0 R6467/ bit0 R6475/ bit0 R6483/ bit0 R6491/ bit0 R6499/ bit0 #1281 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1282 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1283 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1284 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1285 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1286 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1287 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1288 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1289 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1290 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1291 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1292 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1293 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1294 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1295 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 916 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.26 System Variables (Macro Interface Output (NC -> PLC)) Function and purpose The interface output signals can be sent by substituting values in variable Nos. #1100 to #1135, #1300 to #1395. Note The status of the interface input signals can be ascertained by reading out the values of variable Nos. #1000 to #1035, #1200 to #1295. (For details of the system variables for the output signals, refer to "22.25 System Variables (Macro Interface Input (PLC -> NC))".) Example of 1st part system (a) #1032 (R6436, R6437) #1132 (R6372, R6373) #1000 #1100 #1031 #1131 #1033 (R6438, R6439) (c) #1133 (R6374, R6375) #1200 #1300 #1231 #1331 #1134 (R6376, R6377) #1034 (R6440, R6441) #1232 #1332 #1263 #1363 #1135 (R6378, R6379) #1035 (R6442, R6443) (a) Input signal (b) #1264 #1364 #1295 #1395 (b) Output signal 917 (c) Macro instructions IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Detailed description The status of the writing and output signals can be read in order to compensate the #1100 to #1135, #1300 to #1395 output signals. Output here refers to the output from the NC side. Whether it is per part system or common between part systems depends on the MTB specifications (parameter "#1230 set02/bit07"). Note (1) The last values of the system variables #1100 to #1135, #1300 to #1395 sent are retained as 1 or 0. (They are not cleared even by resetting.) (2) The following applies when any number except 1 or 0 is substituted into #1100 to #1131, #1300 to #1395. <Blank> is treated as 0. All values other than <blank> or "0" are treated as 1. Any value less than 0.00000001 is indefinite. Data unit (32 bits) All the output Nos. from #1100 to #1131 can be sent at once by substituting a value in variable No. #1132. The output signals from #1300 to #1331, #1332 to #1363, and #1364 to #1395 can be sent by substituting a value in variable Nos. #1133 to #1135. (20 to 231) The data of the 1st part system ($1) to the 8th part system ($8) is as follows. Interface output signal System variable No. of points $1 $2 $3 $4 $5 $6 $7 $8 #1132 32 R6372, R6373 R6380, R6381 R6388, R6389 R6396, R6397 R6404, R6405 R6412, R6413 R6420, R6421 R6428, R6429 #1133 32 R6374, R6375 R6382, R6383 R6390, R6391 R6398, R6399 R6406, R6407 R6414, R6415 R6422, R6423 R6430, R6431 #1134 32 R6376, R6377 R6384, R6385 R6392, R6393 R6400, R6401 R6408, R6409 R6416, R6417 R6424, R6425 R6432, R6433 #1135 32 R6378, R6379 R6386, R6387 R6394, R6395 R6402, R6403 R6410, R6411 R6418, R6419 R6426, R6427 R6434, R6435 IB-1501278-D 918 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Bit unit The output signal has only two values: "0" and "1". Part system $1 $2 $3 $4 $5 $6 $7 $8 R device R6372R6379 R6380R6387 R6388R6395 R6396R6403 R6404R6411 R6412R6419 R6420R6427 R6428R6435 If the value is common between part systems, refer to the column of the 1st part system ($1). Interface output signal register System variable No. of points $1 $2 $3 $4 $5 $6 $7 $8 #1100 1 R6372/ bit0 R6380/ bit0 R6388/ bit0 R6396/ bit0 R6404/ bit0 R6412/ bit0 R6420/ bit0 R6428/ bit0 #1101 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1102 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1103 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1104 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1105 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1106 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1107 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1108 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1109 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1110 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1111 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1112 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1113 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1114 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1115 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 #1116 1 R6373/ bit0 R6381/ bit0 R6389/ bit0 R6397/ bit0 R6405/ bit0 R6413/ bit0 R6421/ bit0 R6429/ bit0 #1117 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1118 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1119 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1120 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1121 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1122 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1123 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1124 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1125 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1126 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1127 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1128 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1129 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1130 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1131 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 919 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables IB-1501278-D Interface output signal register System variable No. of points $1 $2 $3 $4 $5 $6 $7 $8 #1300 1 R6374/ bit0 R6382/ bit0 R6390/ bit0 R6398/ bit0 R6406/ bit0 R6414/ bit0 R6422/ bit0 R6430/ bit0 #1301 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1302 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1303 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1304 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1305 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1306 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1307 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1308 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1309 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1310 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1311 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1312 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1313 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1314 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1315 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 #1316 1 R6375/ bit0 R6383/ bit0 R6391/ bit0 R6399/ bit0 R6407/ bit0 R6415/ bit0 R6423/ bit0 R6431/ bit0 #1317 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1318 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1319 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1320 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1321 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1322 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1323 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1324 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1325 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1326 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1327 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1328 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1329 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1330 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1331 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 920 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Interface output signal register System variable No. of points $1 $2 $3 $4 $5 $6 $7 $8 #1332 1 R6376/ bit0 R6384/ bit0 R6392/ bit0 R6400/ bit0 R6408/ bit0 R6416/ bit0 R6424/ bit0 R6432/ bit0 #1333 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1334 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1335 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1336 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1337 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1338 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1339 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1340 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1341 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1342 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1343 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1344 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1345 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1346 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1347 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 #1348 1 R6377/ bit0 R6385/ bit0 R6393/ bit0 R6401/ bit0 R6409/ bit0 R6417/ bit0 R6425/ bit0 R6433/ bit0 #1349 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1350 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1351 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1352 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1353 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1354 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1355 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1356 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1357 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1358 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1359 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1360 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1361 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1362 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1363 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 921 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables IB-1501278-D Interface output signal register System variable No. of points $1 $2 $3 $4 $5 $6 $7 $8 #1364 1 R6378/ bit0 R6386/ bit0 R6394/ bit0 R6402/ bit0 R6410/ bit0 R6418/ bit0 R6426/ bit0 R6434/ bit0 #1365 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1366 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1367 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1368 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1369 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1370 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1371 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1372 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1373 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1374 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1375 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1376 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1377 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1378 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1379 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 #1380 1 R6379/ bit0 R6387/ bit0 R6395/ bit0 R6403/ bit0 R6411/ bit0 R6419/ bit0 R6427/ bit0 R6435/ bit0 #1381 1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 bit1 #1382 1 bit2 bit2 bit2 bit2 bit2 bit2 bit2 bit2 #1383 1 bit3 bit3 bit3 bit3 bit3 bit3 bit3 bit3 #1384 1 bit4 bit4 bit4 bit4 bit4 bit4 bit4 bit4 #1385 1 bit5 bit5 bit5 bit5 bit5 bit5 bit5 bit5 #1386 1 bit6 bit6 bit6 bit6 bit6 bit6 bit6 bit6 #1387 1 bit7 bit7 bit7 bit7 bit7 bit7 bit7 bit7 #1388 1 bit8 bit8 bit8 bit8 bit8 bit8 bit8 bit8 #1389 1 bit9 bit9 bit9 bit9 bit9 bit9 bit9 bit9 #1390 1 bit10 bit10 bit10 bit10 bit10 bit10 bit10 bit10 #1391 1 bit11 bit11 bit11 bit11 bit11 bit11 bit11 bit11 #1392 1 bit12 bit12 bit12 bit12 bit12 bit12 bit12 bit12 #1393 1 bit13 bit13 bit13 bit13 bit13 bit13 bit13 bit13 #1394 1 bit14 bit14 bit14 bit14 bit14 bit14 bit14 bit14 #1395 1 bit15 bit15 bit15 bit15 bit15 bit15 bit15 bit15 922 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.27 System Variables (R Device Access Variables) Function and purpose By using variable Nos. #50000 to #50749, #51000 to #51749, #52000 to #52749, it is possible to read data (R8300 to R9799, R18300 to R19799, R28300 to R29799) and substitute value in the R device user backup area. Variable No. R device #50000 R8300, R8301 #50001 R8302, R8303 User backup area (1500 points) : #50749 R9798, R9799 Variable No. R device #51000 R18300, R18301 #51001 R18302, R18303 User backup area (1500 points) : #51749 R19798, R19799 Variable No. R device #52000 R28300, R28301 #52001 R28302, R28303 User backup area (1500 points) : #52749 R29798, R29799 Detailed description These variables read and write the two words of R device. Data range of these variables is -2147483648 to 2147483647. Depending on the setting of the PLC bit selection parameter "#6455/ bit0 to 2", these variables can be changed between decimal point valid or invalid for each user backup area. The position of the decimal point when decimal point valid is selected, varies according to the parameters "#1003 iunit" (inupt setting unit) and "#1041 I_inch" (initial inch). (This depends on the MTB specifications.) #1041 I_inch #1003 iunit B 0: Metric 1: Inch Three digits after the decimal point C D E Four digits after the dec- Five digits after the dec- Six digits after the deciimal point imal point mal point Four digits after the dec- Five digits after the dec- Six digits after the deciimal point imal point mal point Seven digits after the decimal point These variables are retained even when the power is off. These are common among part systems. 923 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Access from a machining program to R device [Reading variables] When the variable #50000 is used in a machining program as shown below, the data set in device R8300 and R8301 will be referred. G0 X#50000 ; R8300,R8301 Device Value #50000 R8301 0x0001 R8300 0xe240 0x1e240 (Hex.) = 123456 (Decimal) (1) When decimal point invalid is selected: Regardless of the setting of the parameter "#1003 iunit" (input setting unit) and "#1041 I_inch" (initial inch), the data set in the R device will be the command value. In case of the above example, the command value will be "X123456.". (2) When decimal point valid is selected: The data set in the R device will be read as a data with a decimal point. The position of the decimal point will be as follows, according to the settings of the parameters "#1003 iunit" (inupt setting unit) and "#1041 I_inch" (initial inch). #1041 I_inch #1003 iunit B C D E 0: Metric X123.456 X12.3456 X1.23456 X0.123456 1: Inch X12.3456 X1.23456 X0.123456 X0.0123456 [Substitution into variables] When substituting a value to the variable #50001 in a machining program as shown below, data will be set in the device R8302 and R8303. #50001 = 123 ; R8302,R8303 (1) When decimal point invalid is selected: Regardless of the setting of the parameter "#1003 iunit" (inupt setting unit) and "#1041 I_inch" (initial inch), substituted value will be set in the R device. #50001 Device Value 123 (Decimal) = 0x7b (Hex.) R8303 0x0000 R8302 0x007b When a value with a decimal point is substituted to a variable like "#50001 = 123.456 ;", the numbers after the decimal point will be truncated and "123" will be set. IB-1501278-D 924 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables (2) When decimal point valid is selected: According to the settings of the parameter "#1003 iunit" (inupt setting unit) and "#1041 I_inch" (initial inch), values which are shifted for the number of decimals will be set in the R device, as shown below. #1041 I_inch 0: Metric #1003 iunit B C D E #50001 123000 (Decimal) = 0x1e078 (Hex.) 1230000 (Decimal) = 0x12c4b0 (Hex.) 12300000 (Decimal) = 0xbbaee0 (Hex.) 123000000 (Decimal) = 0x754d4c0 (Hex.) R8303 0x0001 0x0012 0x00bb 0x0754 R8302 0xe078 0xc4b0 0xaee0 0xd4c0 Device #1041 I_inch 1: Inch #1003 iunit B C D E #50001 1230000 (Decimal) = 0x12c4b0 (Hex.) 12300000 (Decimal) = 0xbbaee0 (Hex.) 123000000 (Decimal) = 0x754d4c0 (Hex.) 1230000000 (Decimal) = 0x49504f80 (Hex.) Device R8303 0x0012 0x00bb 0x0754 0x4950 R8302 0xc4b0 0xaee0 0xd4c0 0x4f80 When a value with a decimal point is substituted to a variable like "#50001 = 123.456 ;", the value will directly be set. #1041 I_inch 0: Metric #1003 iunit B C D E #50001 123456 (Decimal) = 0x1e240 (Hex.) 1234560 (Decimal) = 0x12d680 (Hex.) 12345600 (Decimal) = 0xbc6100 (Hex.) 123456000 (Decimal) = 0x75bca00 (Hex.) R8303 0x0001 0x0012 0x00bc 0x075b R8302 0xe240 0xd680 0x6100 0xca00 #1003 iunit B C D E #50001 1234560 (Decimal) = 0x12d680 (Hex.) 12345600 (Decimal) = 0xbc6100 (Hex.) 123456000 (Decimal) = 0x75bca00 (Hex.) 1234560000 (Decimal) = 0x4995e400 (Hex.) R8303 0x0012 0x00bc 0x075b 0x4998 R8302 0xd680 0x6100 0xca00 0xe400 Device #1041 I_inch Device 1: Inch If the number of decimals of the substituted data exceeds the number of significant figures, the value will be rounded off to the number of significant figures and will be set. When "#50001 = 123.4567899 ;". #1041 I_inch 0: Metric #1003 iunit B C D E #50001 123457 (Decimal) = 0x1e241 (Hex.) 1234568 (Decimal) = 0x12d688 (Hex.) 12345679 (Decimal) = 0xbc614f (Hex.) 123456790 (Decimal) = 0x75bcd16 (Hex.) R8303 0x0001 0x0012 0x00bc 0x075b R8302 0xe241 0xd688 0x614f 0xcd16 #1003 iunit B C D E #50001 1234568 (Decimal) = 0x12d688 (Hex.) 12345679 (Decimal) = 0xbc614f (Hex.) 123456790 (Decimal) = 0x75bcd16 (Hex.) 1234567899 (Decimal) = 0x499602db (Hex.) R8303 0x0012 0x00bc 0x075b 0x4996 R8302 0xd688 0x614f 0xcd16 0x02db Device #1041 I_inch Device 1: Inch 925 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Use of R device access variables in control command These variables can be used in control command. However, note that the variable value and the condition of true/false differ between decimal point valid variables and invalid variables. IF [#50003 EQ 1] GOTO 30 ; G00 X100 ; N30 (1) When decimal point invalid is selected: Regardless of the setting of the parameter "#1003 iunit" (input setting unit) and "#1041 I_inch" (initial inch), R device value of #50003 whose condition is true, will be "1". #50003 Device Value 1 (Decimal) = 0x01 (Hex.) R8307 0x0000 R8306 0x0001 (2) When decimal point valid is selected: The condition is true when #50003 is "1". So the R device value of #50003 will be as follows depending on the setting of the parameter "#1003 iunit" (inupt setting unit) and "#1041 I_inch" (initial inch). #1041 I_inch 0: Metric #1003 iunit B C D E #50003 1000 (Decimal) = 0x3e8 (Hex.) 10000 (Decimal) = 0x2710 (Hex.) 100000 (Decimal) = 0x186a0 (Hex.) 1000000 (Decimal) = 0xf4240 (Hex.) R8307 0x0000 0x0000 0x0001 0x000f R8306 0x03e8 0x2710 0x86a0 0x4240 #1003 iunit B C D E #50003 10000 (Decimal) = 0x2710 (Hex.) 100000 (Decimal) = 0x186a0 (Hex.) 1000000 (Decimal) = 0xf4240 (Hex.) 10000000 (Decimal) = 0x989680 (Hex.) R8307 0x0000 0x0001 0x000f 0x0098 R8306 0x2710 0x86a0 0x4240 0x9680 Device #1041 I_inch Device IB-1501278-D 1: Inch 926 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Substitution between R device access variable and other variables. [Substitution into R device access variables] Common variables and coordinates variables can be substituted to the R device access variables. (Example 1) Common variables #101 = -123.456 ; #50004 = #101 ; (Example 2) #5063 : Skip coordinates #5063 #50004 = #5063 ; (1) When decimal point invalid is selected: Regardless of the settings of the parameter "#1003 iunit" (inupt setting unit) and "#1041 I_inch" (initial inch), the value which is rounded off will be set. When the common variable and coordinate variable in the above example are "-123.456": #50004 Device Value -123 (Decimal) = 0xffffff85 (Hex.) R8309 0xffff R8308 0x0085 (2) When decimal point valid is selected: Substitution will be as follows according to the settings of the parameter "#1003 iunit" (inupt setting unit) and "#1041 I_inch" (initial inch). #1041 I_inch 0: Metric #1003 iunit B C D E #50004 -123456 (Decimal) = 0xfffe1dc0 (Hex.) -1234560 (Decimal) = 0xffed2980 (Hex.) -12345600 (Decimal) = 0xff439f00 (Hex.) -123456000 (Decimal) = 0xf8a43600 (Hex.) Device R8309 0xfffe 0xffed 0xff43 0xf8a4 R8308 0x1dc0 0x2980 0x9f00 0x3600 #1003 iunit B C D E #50004 -1234560 (Decimal) = 0xffed2980 (Hex.) -12345600 (Decimal) = 0xff439f00 (Hex.) R8309 0xffed 0xff43 0xf8a4 0xb66a R8308 0x2980 0x9f00 0x3600 0x1c00 #1041 I_inch Device 1: Inch 927 -123456000 (Decimal) = -1234560000 (Decimal) = 0xf8a43600 (Hex.) 0xb66a1c00 (Hex.) IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables [Substitution of R device access variables] #50005 = 123.456789 ; #102 = #50005 ; (1) When decimal point invalid is selected: Regardless of the settings of the parameter "#1003 iunit" (inupt setting unit) and "#1041 I_inch" (initial inch), #102 will be "123". (2) When decimal point valid is selected: Substitution will be as follows according to the settings of the parameter "#1003 iunit" (inupt setting unit) and "#1041 I_inch" (initial inch). #1041 I_inch 0: Metric #1003 iunit B C D E #102 123.4570 123.4568 123.4568 123.4568 #1041 I_inch 1: Inch #1003 iunit B C D E #102 123.4568 123.4568 123.4568 123.4568 Precautions (1) The position of a decimal point changes depending on the settings of the parameter "#1003 iunit" (input setting unit) and "#1041 I_inch" (initial inch). Fix the decimal point position while considering these parameter settings when setting a number to an R device. (2) These variables do not handle <Blank>. If #0<Blank> is substituted, it will be converted into "0". Therefore, when comparing this variable after substituting #0<Blank> and #0<Blank> with a conditional expression (EQ), it will not be formed. (3) If a value exceeding the allowable range is substituted into this variable, a program error (P35) will occur. (4) When these values are used as decimal point invalid, the settings of "#1078 Decpt2" (Decimal point type 2) and "#8044 UNIT*10" will not be applied. (5) When a graphic is being checked, writing into R device will not be executed even if a value is substituted into these variables. For reading of these variables (reference to the R device value) during a graphic check, "0" is always read. IB-1501278-D 928 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.28 System Variables (PLC Data Reading) Function and purpose PLC data can be read in with the system variables. Variable No. Application #100100 Device type designation #100101 Device No. designation #100102 Number of read bytes designation #100103 Read bit designation #100110 Reading PLC data Note (1) These can be used only with some models. (2) The readable devices are limited. Detailed description The PLC data is read in with the following five blocks using these five system variables. #100100 = 1 ; Designates the device type. #100101 = 0 ; Designates the device No. #100102 = 1 ; Designates the number of bytes. #100103 = 2 ; Designates the bit. (Valid only when reading word device bits.) #100=#100110; Reads in the PLC data. Device designation (#100100) (1) System variable for device designation The type of device to be read in can be designated by substituting the device designation value in this system variable. If the data is read without designating this variable, the data will be read in the same manner as when the minimum value (0: M device) of the device designation value is designated. Once designated, the setting is held until the device is designated again or until it is reset. A program error (P39) will occur if a nonexistent device is set. (2) Device designation value [M800/M80 series] Device designation value Device 0 M Unit Device No. Device designation value Device F Bit F0 to F2047 Bit M0 to M61439 10 Unit Device No. 1 D Word D0 to D4095 13 L Bit L0 to L1023 2 C Bit C0 to C511 18 V Bit V0 to V511 4 X (*1) Bit X0 to X1FFF 19 ST Bit ST0 to ST127 5 Y (*1) Bit Y0 to Y1FFF 20 SD Word SD0 to SD2047 6 R Word R0 to R32767 21 SB (*1) Bit SB0 to SB3FF 7 T Bit T0 to T2047 22 SW (*1) Word SW0 to SW3FF 9 SM Bit SM0 to SM2047 23 B (*1) Bit B0 to BDFFF 24 W (*1) Word W0 to W2FFF 929 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables [C80 series] Device designation value Device Unit Device No. Device designation value Device Unit Device No. 0 M Bit M0 to M61439 10 F Bit F0 to F2047 1 D Word D0 to D8191 13 L Bit L0 to L1023 2 C Bit C0 to C511 18 V Bit V0 to V511 4 X (*1) (*2) Bit X0 to X1FFF 19 ST Bit ST0 to STI27 5 Y (*1) (*2) Bit Y0 to Y1FFF 20 SD Word SD0 to SD4095 6 R (*2) Word R0 to R32767 21 SB (*1) Bit SB0 to SB3FF 7 T Bit T0 to T2047 22 SW (*1) Word SW0 to SW1023 9 SM (*2) Bit SM0 to SM4095 23 B (*1) Bit B0 to BDFFF 24 W (*1) Word W0 to W2FFF The unit indicates the amount of data per device No. "Word" is 16 bits, and "Bit" is one bit. (*1) Device of which the device number is indicated in hexadecimal notation. (*2) The device marked by an asterisk (*) in the Device column has the determined use; therefore, do not use the undefined device number even for a vacant device. Device No. designation (#100101) The device to be read in is designated by substituting the device No. in this system variable. Convert a device expressed as a hexadecimal into a decimal when designating. If the data is read without designating this number, the data will be read in the same manner as when the minimum device No. (0) is designated. Once designated, the setting is held until the device No. is designated again or until it is reset. A program error (P39) will occur if a nonexistent device No. is set. Number of bytes designation (#100102) (1) System variable for number of bytes designation The reading size is designated by substituting the number of bytes designation value in this system variable. If the data is read without designating this number, the data will be read in the same manner as when the minimum device designation value (0: M device) is designated. Once designated, the setting is held until the number of bytes is designated again or until it is reset. A program error (P39) will occur if a number of bytes that does not exist in the specifications is set. (2) Number of bytes designation value Number of bytes designation value Read in data Size 0 1 bit 1 1 bytes 101 2 2 bytes 102 4 104 Sign Range - 0 to 1 No 0 to 255 Yes -128 to 127 No 0 to 65535 Yes 4 bytes Operation No Yes Word device Bit device The number of bits des- The bits for the designated device ignated is read in. No. are read in. The low-order byte is read in. 8 bits are read in from the designated device No. Two bytes are read in. 16 bits are read in from the designated device No. -32768 to 32767 0 to 4294967295 The designated device 32 bits are read in from the desig-2147483648 (L) and next device (H) nated device No. to 2147483647 are read in. 0 to 4 are designated without a sign, and 101 to 104 are designated with a sign. IB-1501278-D 930 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Bit designation (#100103) (1) System variable for bit designation The bit to be read in is designated by substituting the bit designation value in this system variable. This designation is valid only when reading the bits for a 16-bit device, and is invalid for the others. If the data is read without designating this number, the data will be read in the same manner as if the minimum bit designation value (0: bit 0) is designated. Once designated, the setting is held until the bit is designated again or until it is reset. A program error (P39) will occur if a nonexistent bit is set. (2) Bit designation value Bit designation value Read in bit 0 Bit 0 1 Bit 1 : : 15 Bit 15 Reading PLC data (#100110) The data for the designated device is read in with this system variable. Refer to the table for number of bytes designation for details on the range of data read in. Program example (1) To read a bit device #100100 = 0 ; Designates [M device]. #100101 = 0 ; Designates [Device No. 0]. #100102 = 0 ; Designates [Bit]. #100 = #100110; Reads M0 (one bit). #100102 = 1 ; Designates [1 byte]. #101 = #100110; Reads M0 to M7 (8 bits). (If M7 to M0 is 0001 0010, this will be #102 = 18 (0x12).) #100102 = 102 ; Designates [Signed two bytes]. #102 = #100110; Reads M0 to M15 (16 bits). (If M15 to M0 is 1111 1110 1101 1100, this will be #102 = -292 (0xFEDC).) #100102 = 4 ; Designates [4 byte]. #104 = #100110; Reads M0 to M31 (32 bits). (If M31 to M0 is 0001 0010 0011 0100 0101 0110 0111 1000, #104 = 305419896 (0x12345678).) 931 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables (2) To read a word device #100100 = 1 ; Designates [D device]. #100101 = 0 ; Designates [Device No. 0]. #100102 = 0 ; Designates [Bit]. #100103 = 1 ; Designates [Bit 1]. #100 = #100110; Reads the D0 bit 1. (If D0 = 0x0102, #101 =1.) #100102 = 1 ; Designates [1 byte]. #101 = #100110; Reads the low-order byte of D0. (If D0 = 0x0102, #101 =2.) #100102 = 2 ; Designates [2 byte]. #102 = #100110; Reads D0. (If D0 = 0x0102, #102 =258.) #100102 = 104 ; Designates [Signed four bytes]. #104 = #100110; Reads D0 and D1. (If D0 = 0xFFFE and D1 = 0xFFFF, #104 =-2.) Precautions (1) As the PLC data is read asynchronously from the ladder execution, the data is not necessarily the one which was gained when the program was executed. Be careful when reading devices which are changing. (2) If reading of a nonexistent device is attempted by designating the device No. and number of bytes, the 0 value will be read in only for the nonexistent section. (3) When "1" is set to the parameter "#1316 CrossCom", #100100 to #100110 cannot be used as system variables to read PLC data. IB-1501278-D 932 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.29 System Variables (Interfering Object Selection) Detailed description Select 16 interfering objects to use in the interference check III with system variables or R register. Refer to the "PLC Interface Manual" (IB-1501272) for the R register. When selecting an interfering object, specify the specification of the selected interfering object and interfering model coordinate system offset 1. The write command to the system variables (#40000 to #40097) is possible only in the machine tool builder macro programs (O100010000 to O199999998). System variable R register Item Details Setting range (unit) Upper: System variable Lower: R register #40000 R20304 Interfering object enSet enable/disable for each interfer- 0 to 65535 (decimal) able/disable designation ing object. Bit designation (0: enable 1: disable) bit0: Disable 1st interfering object : 0x0000 to 0xFFFF (hexadecimal) bitF: Disable 16th interfering object #40001 R20305 preliminary 0 0 40002 R20306 #40003 R20307 1st interfering object se- Select interfering object definition lection No. to use. 1st interfering object specification 0 to 128 (0: not selected) 0 to 128 (0: not selected) In the configured solid specification 0 to 3 of the interfering object definition, specify alarm area/warning area/ solid setting invalid of the solid in which switching method is selected. 0, 1: Alarm area 0 to 3 2: Warning area 3: Solid setting invalid #40004 R20308 (L) R20309 (H) #40005 R20310 (L) R20311 (H) #40006 R20312 (L) R20313 (H) : 1st interfering model co- Set the interfering model coordinate -99999.999 to 99999.999 ordinate system system offset with a radius value. (I (mm) (radius value) I axis offset 1 axis direction) (*1) 1st interfering model co- Set the interfering model coordinate ordinate system system offset with a radius value. (J -99999999 to 99999999 J axis offset 1 axis direction) (*1) (μm) (radius value) 1st interfering model co- Set the interfering model coordinate ordinate system system offset with a radius value. (K axis direction) (*1) K axis offset 1 : #40077 R20426 16th interfering object selection Same as above Same as above #40078 R20427 16th interfering object specification selection Same as above Same as above #40079 R20428 (L) 16th interfering model coordinate system I axis offset 1 Same as above Same as above 16th interfering model coordinate system J axis offset 1 Same as above Same as above R20429 (H) #40080 R20430 (L) R20431 (H) 933 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables System variable R register Item Details Setting range (unit) Upper: System variable Lower: R register #40081 R20432 (L) 16th interfering model coordinate system K axis offset 1 Same as above #40082 R20434 1st interfering object Interference check III: Specifying disabled interfering object Select an interfering object that you 0 to 65535 (decimal) do not check the interference with 0x0000 to 0xFFFF (hexathe 1st interfering object. decimal) bit0: Disable 1st interfering object (inaction data) bit1: Disable 2nd interfering object : bitF: Disable 16th interfering object #40083 R204325 2nd interfering object Interference check III: Specifying disabled interfering object Select an interfering object that you 0 to 65535 (decimal) do not check the interference with 0x0000 to 0xFFFF (hexathe 2nd interfering object. decimal) bit0: Disable 1st interfering object bit1: Disable 2nd interfering object (inaction data) : bitF: Disable 16th interfering object 16th interfering object Interference check III: Specifying disabled interfering object Select an interfering object that you 0 to 65535 (decimal) do not check the interference with 0x0000 to 0xFFFF (hexathe 16th interfering object. decimal) bit0: Disable 1st interfering object bit1: Disable 2nd interfering object : bitF: Disable 16th interfering object (inaction data) R20433 (H) : Same as above : #40097 R20449 (*1) The interfering model coordinate system offset is the sum of the interfering model coordinate system offsets 1 and 2. Interference check III: designation of disabled interference object (Example) In the case that you do not check the interference between the 1st interfering object and the 2nd interfering object "R20434 (#40082): 0x0002 (disable 2nd interfering object)" or "R20435 (#40083): 0x0001 (disable 1st interfering object)" Since each interfering object is designated to perform the interference check, the setting of the interference check III specifying disabled interference object is repeated, but if either one is on disabled setting, the interference check is not performed. Back side of spindle part (without a workpiece) 1st interfering object (back side of spindle part) Back side of spindle part (with a workpiece) 1st interfering object (back side of spindle part) 2nd interfering object (workpiece part) By specifying the interference III disabled between the back side of spindle part (1st interfering object) and workpiece part (2nd interfering object), these 2 parts are treated as one interfering object. IB-1501278-D 934 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables Precautions (1) When the interfering object selection is input with the system variables, the system variable in which the command range integer is set in R register with the value after the decimal point being ignored. (a) When any value out of the setting range is input in #40000 to #40097, the low-order 16 bits of the input value are set in R register. (b) When "#0" <empty> is input in #40000 to #40097, "0" is set in R register. (2) If you have made a write command to the system variable (#40000 to #40097) in a program except for the machine tool builder macro program, the program error (P241) occurs. 935 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables 22.30 System Variables (ZR Device Access Variables) [C80] Detailed description System variables that can read and write data from and to the ZR device are provided by 2,250 sets (#50000 to #52749). Data can be read and written between the NC machining program and RCPU sequence program by using the ZR device as shown below. How to handle the ZR device in the RCPU sequence program depends on the MTB specifications. Refer to the PLC Interface Manual (IB-1501258) for the DDWR/DDRD command. RCPU C80 Sequence program ZR device NC machining program ZR50000 ZR50001 ZR50002 ZR50003 : ZR51998 ZR51999 D(P).DDWR D(P).DDRD G00 X#50000 Y#50001 ; G01 Z-100. F1000 ; : G31 Z-150. F100 ; #50999 = #5063 ; M30 ; Number of variable sets The table below shows a list of variables specific to C80. A ZR device access variable is based on long-type data, and a ZR device on word-type data. Therefore, when this variable is read or a value is substituted to this variable, it reads and writes two words of the ZR device. The correspondence between the ZR device access variable numbers and ZR device numbers is shown below. Variable No. (2,250 sets) #50000 - #50749 #51000 - #51749 #52000 - #52749 Corresponding ZR device (4,500 units) #50000 ZR50000, ZR50001 #50001 ZR50002, ZR50003 #50002 ZR50004, ZR50005 : : #50000+n ZR50000+2n, ZR50000+2n+1 : : #52749 ZR55498, ZR55499 #51000 ZR52000, ZR52001 : : #51749 ZR53498, ZR53499 #52000 ZR54000, ZR54001 : : #52749 ZR55498, ZR55499 (1) The data range of these variables is -2147483648 to 2147483647. (2) The ZR device is backed up even when the power is turned OFF; therefore, the value is maintained after the power has been turned ON again. (3) Whether this variable is used with the decimal point invalid or valid can be selected for each user backup area according to the MTB specifications (parameter "#6455 bit0 -bit2"). IB-1501278-D 936 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables (4) When "decimal point valid" is selected, the position of the decimal point depends on the MTB specifications (parameters "#1003 iunit" (input setting unit) and "#1041 I_inch" (initial inch)). Therefore, to set a numeric value to a ZR device, consider the position of the decimal point according to these parameters. The table below shows the number of digits that is valid after the decimal point. #1041 I_inch #1003 iunit B C D E Metric 3 digits 4 digits 5 digits 6 digits Inch 4 digits 5 digits 6 digits 7 digits 937 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 22 System Variables IB-1501278-D 938 23 Appx.1: Fixed Cycles 939 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 23 Appx.1: Fixed Cycles 23Appx.1: Fixed Cycles [G81(O100000810) Drill, spot drill] [G84(O100000840) Tap cyclecle] G.1 ; G.1 ; IF[#30] GOTO1 ; IF[#30] GOTO9 ; Z#2 G#6 H#7 ; Z#2 G#6 H#7 ; #2=##5#3003=#8 OR1 ; #2=##5#3003=#8 OR1#3004=#9 OR3 ; G1 Z#3 ; IF[#11] GOTO1 ; IF[#4 EQ#0] GOTO2 ; GOTO2 ; G4 P#4 ; N1 ; N2 ; IF[#14] GOTO5 ; #3003=#8 ; N2 G1 Z#3 ; G0 Z-#3-#2, I#23 ; GOTO7 ; N1 M99 ; N5 ; #29=0#28=#11 ; [G82(O100000820) Drill, counter boring] DO1 ; G.1 ; #29=#29+#11 ; IF[#30] GOTO1 ; IF[ ABS[#29] GE[ ABS[#3]]] GOTO6 ; Z#2 G#6 H#7 ; G1 Z#28 ; #2=##5#3003=#8 OR1 ; M#53 ; G1 Z#3 ; G1 Z-#14 ; G4 P#4 ; M#54 ; #3003=#8 ; #28=#11+#14 ; G0 Z-#3-#2, I#23 ; END1 ; N1 M99 ; N6 G1 Z#3-#29+#28 ; N7 G4 P#4 ; [G83(O100000830) Deep hole drill cycle] M#53 ; G.1 ; #3900=1 ; IF[#30] GOTO2 ; G1 Z-#3 ; #29=#11#28=0 ; #3004=#9 ; Z#2 G#6 H#7 ; G4 P#56 ; #2=##5#3003=#8 OR1 ; M#54 ; DO1 ; #3003=#8 ; #28=#28-#11#26=-#28-#29 ; G0 Z-#2, I#23 ; Z#26 ; N9 M99 ; IF[ ABS[#28] GE[ ABS[#3]]] GOTO1 ; G1 Z#29 ; G0 Z#28 ; #29=#11+#14 ; END1 ; N1 G1 Z#3-#26 ; IF[#4 EQ#0] GOTO3 ; G4 P#4 ; N3 ; #3003=#8 ; G0 Z-#3-#2, I#23 ; N2 M99 ; IB-1501278-D 940 M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 23 Appx.1: Fixed Cycles [G85(O100000850) Boring 1] [G88(O100000880) Boring 3] G.1 ; G.1 ; IF[#30] GOTO1 ; IF[#30] GOTO1 ; Z#2 G#6 H#7 ; Z#2 G#6 H#7 ; #2=##5#3003=#8 OR1 ; #2=##5#3003=#8 OR1 ; G1 Z#3 ; G1 Z#3 ; IF[#4 EQ#0] GOTO2 ; G4 P#4 ; G4 P#4 ; #3003=#8 ; N2 ; M5 ; #3003=#8 ; #3003=#8 OR1 ; Z-#3 ; G0 Z-#3-#2 ; G0 Z-#2, I#23 ; #3003=#8 ; N1 M99 ; M3 ; N1 M99 ; [G86(O100000860) Boring 2] G.1 ; [G89(O100000890) Boring 4] IF[#30] GOTO1 ; G.1 ; Z#2 G#6 H#7 ; IF[#30] GOTO1 ; #2=##5#3003=#8 OR1 ; Z#2 G#6 H#7 ; G1 Z#3 ; #2=##5#3003=#8 OR1 ; G4 P#4 ; G1 Z#3 ; M5 ; G4 P#4 ; G0 Z-#3-#2 ; #3003=#8 ; #3003=#8 ; Z-#3 ; M3 ; G0 Z-#2, I#23 ; N1 M99 ; N1 M99 ; [G87(O100000870) Back boring] G73(O100000831) Step cycle] G.1 ; G.1 ; IF[#30] GOTO1 ; IF[#30] GOTO2 ; #3003=#8 OR1 ; #29=0#28=#11 ; M19 ; Z#2 G#6 H#7 ; X#12 Y#13 ; #2=##5#3003=#8 OR1 ; #3003=#8 ; DO1 ; Z#2 G#6 H#7 ; #29=#29+#11 ; #3003=#8 OR1 ; IF[ ABS[#29] GE[ ABS[#3]]] GOTO1 ; G1 X-#12 Y-#13 ; G1 Z#28 ; #3003=#8 ; G4 P#4 ; M3 ; G0 Z-#14 ; #3003=#8 OR1 ; #28=#11+#14 ; Z#3 ; END1 ; M19 ; N1 G1 Z#3-#29+#28 ; G0 X#12 Y#13 ; G4 P#4 ; Z-#2-#3 ; #3003=#8 ; #3003=#8 ; G0 Z-#3-#2, I#23 ; X-#12 Y-#13 ; N2 M99 ; M3 ; N1 M99 ; 941 IB-1501278-D M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) 23 Appx.1: Fixed Cycles [G74(O100000841) Reverse tap cycle] [G75(O100000851) Circle cutting cycle] G.1 ; G.1 ; IF[#30] GOTO9 ; IF[#30] GOTO1 ; Z#2 G#6 H#7 ; #28=#18 ; #2=##5#3003=#8 OR1#3004=#9 OR3 ; IF[#28 GE0] GOTO2 ; IF[#11] GOTO1 ; #27=3#28=-#28 ; GOTO2 ; GOTO3 ; N1 ; N2#27=2 ; IF[#14] GOTO5 ; N3#26=#4 ; N2 G1 Z#3 ; IF[#26 GE#28] GOTO1 ; GOTO7 ; Z#2 G#6 H#7 ; N5 ; #2=##5#3003=#8 OR1 ; #29=0#28=#11 ; G1 Z#3 ; DO1 ; #28=#28-#26#29=#28/2 ; #29=#29+#11 ; G#27 X-#28 I-#29 ; IF[ ABS[#29] GE[ ABS[#3]]] GOTO6 ; I#28 P1 ; G1 Z#28 ; X#28 I#29 ; M#53 ; #3003=#8 ; G1 Z-#14 ; G0 Z-#3-#2, I#23 ; M#54 ; N1 M99 ; #28=#11+#14 ; END1 ; [G76(O100000861) Fine boring] N6 G1 Z#3-#29+#28 ; G.1 ; N7 G4 P#4 ; IF[#30] GOTO1 ; M#53 ; Z#2 G#6 H#7 ; #3900=1 ; #2=##5#3003=#8 OR1 ; G1 Z-#3 ; G1 Z#3 ; #3004=#9 ; M19 ; G4 P#56 ; X#12 Y#13 ; M#54 ; G0 Z-#3-#2 ; #3003=#8 ; #3003=#8 ; G0 Z-#2, I#23 ; X-#12 Y-#13 ; N9 M99 ; M3 ; N1 M99 ; IB-1501278-D 942 Index Refer to Programming Manual (Machining Center System) (1/2) for Chapter 14 and previous chapters (page 438 and before). Refer to Programming Manual (Machining Center System) (2/2) for Chapter 15 and succeeding chapters (page 439 and later). Symbols Cylindrical Interpolation ................................................... 73 !n (!m ...) L ..................................................................... 522 / ....................................................................................... 16 /n ..................................................................................... 18 D Numerics 2nd Miscellaneous Functions (A8-digits, B8-digits or C8-digits) ....................................................................... 2nd, 3rd, and 4th Reference Position (Zero Point) Return ... 3-dimensional Circular Interpolation .............................. 3-dimensional Coordinate Conversion .......................... 3-dimensional Tool Radius Compensation .................... 3-dimensional Tool Radius Compensation (Tool’s vertical-direction compensation) .................................... 206 831 108 781 296 737 A Acceleration Clamp Speed ............................................ 625 Acceleration/Deceleration Mode Change in Hole Drilling Cycle ............................................................................. 363 Actual Examples of Using User Macros ........................ 425 Arbitrary Axis Exchange ................................................ 538 Arc ................................................................................. 368 ASCII Code Macro ........................................................ 401 Automatic Coordinate System Setting ........................... 753 Automatic Corner Override .................................... 188, 194 Automatic Tool Length Measurement ............................ 846 Axis-based Unidirectional Positioning ............................. 72 Deceleration Check ....................................................... 166 Deceleration Check when Movement in The Opposite Direction Is Reversed .................................................... 174 Decimal point input .......................................................... 34 Deep Hole Drilling Cycle ................................................ 324 Define by Selecting the Registered Machining Surface ..... 708 Detailed Description for Macro Call Instruction .............. 399 Details of Inclined Surface Machining Operation ........... 719 Diameter Designation of Compensation Amount ........... 289 Drilling Cycle High-Speed Retract ................................. 359 Drilling, Counter Boring .................................................. 323 Drilling, Spot Drilling ...................................................... 322 Dwell (Time-based designation) .................................... 200 E Enable Interfering Object Selection Data ....................... 842 Exact Stop Check .......................................................... 161 Exact Stop Check Mode ................................................ 165 Exponential Interpolation ................................................. 89 External Output Commands .......................................... 419 F Back Boring ................................................................... 343 Basic Machine Coordinate System Selection ................ 757 Basic Machine, Workpiece and Local Coordinate Systems .... 751 Bolt Hole Cycle .............................................................. 366 Boring .................................................... 341, 342, 345, 346 F1-Digit Feed ................................................................. 128 Fairing ............................................................................ 615 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/ Synchronous Feed) .................... 130 Feedrate Designation and Effects on Control Axes ....... 138 Figure Rotation .............................................................. 379 File Format ....................................................................... 14 Fine Boring .................................................................... 353 Fixed Cycles .......................................................... 318, 940 C G Changing of Compensation No. during Compensation Mode ... 274 Circular Cutting ........................................................ 80, 351 Circular Interpolation ....................................................... 47 Common Variables ........................................................ 407 Compensation Data Input by Program .......................... 495 Compensation Data Input by Program (Turning Tool) ... 501 Constant Lead Thread Cutting ........................................ 58 Constant Surface Speed Control ................................... 215 Control Commands ....................................................... 416 Coordinate Rotation by Program ................................... 799 Coordinate Rotation Input by Parameter ....................... 806 Coordinate System for Rotary Axis ............................... 754 Coordinate System Setting ............................................ 760 Coordinate Systems and Coordinate Zero Point Symbols .... 3 Coordinate Words and Control Axes ......................... 2, 750 Corner Chamfering Expansion/Corner Rounding Expansion .............................................................. 444, 450 Corner Chamfering I ...................................................... 440 Corner Chamfering I / Corner Rounding I ...................... 440 Corner Chamfering II ..................................................... 447 Corner Chamfering II / Corner Rounding II .................... 447 Corner Rounding I ......................................................... 442 Corner Rounding II ........................................................ 449 Cutting Feed Constant Inclination Acceleration/Deceleration ... 155 Cutting Feedrate ............................................................ 127 Cutting Mode ................................................................. 197 G Code Lists .................................................................... 20 G Cole Macro Call ......................................................... 396 G Command Mirror Image ............................................. 462 G0.5 ............................................................................... 178 G0.5 P1 .......................................................................... 176 G00 .................................................................................. 42 G00 Feedrate Command (,F command) ........................ 123 G01 .................................................................................. 45 G01 A_ ........................................................................... 452 G01 A_ , G02/G03 P_Q_H_ .......................................... 457 G01 A_ , G02/G03 R_H_ ............................................... 460 G01 X_ Y_ ,C ................................................................. 440 G01 X_ Y_ ,R_ ............................................................... 442 G01 X_/Y_ A_/,A_ ......................................................... 451 G01/G02/G03 X_ Y_ ,C_ ............................................... 447 G01/G02/G03 X_ Y_ ,R_ ............................................... 449 G02, G03 ................................................................... 47, 53 G02.1/G03.1(Type1), G02/G03(Type2) ......................... 103 G02.3,G03.3 .................................................................... 89 G02.4,G03.4 .................................................................. 108 G02/G03 P_Q_ /R_ ....................................................... 455 G04 ................................................................................ 200 G05 P1, G05 P2 ............................................................ 558 G05.1 Q1/Q0, G05 P10000/P0, G05 P20000/P0 .......... 599 G05.1 Q2/Q0 ................................................................. 630 G06.2 ............................................................................. 113 B G07 ................................................................................ 119 G07.1 ............................................................................... 73 G09 ................................................................................ 161 G10 I_ J_/K_ ................................................................. 806 G10 L100, G11 .............................................................. 503 G10 L110/L111, G11, G68.2, G69 ................................ 506 G10 L14 ......................................................................... 868 G10 L2/L10/L11/L12/L13/L20, G11 ............................... 495 G10 L2/L12/L13, G11 .................................................... 501 G10 L3, G11 .................................................................. 512 G10 L30, G11 ................................................................ 515 G10 L70/L100, G11 ....................................................... 492 G115 .............................................................................. 525 G116 .............................................................................. 528 G12,G13 .......................................................................... 80 G12.1,G13.1/G112,G113 ................................................ 82 G120.1,G121 ................................................................. 648 G122 .............................................................................. 541 G127 .............................................................................. 486 G140, G141, G142 ........................................................ 538 G16 .................................................................................. 96 G160 .............................................................................. 864 G17, G18, G19 ................................................................ 56 G17, G18, G19 and G02, G03 ........................................ 64 G186 .............................................................................. 842 G20, G21 ......................................................................... 32 G22/G23 ........................................................................ 840 G27 ................................................................................ 837 G28,G29 ........................................................................ 827 G30 ................................................................................ 831 G30.1 - G30.6 ................................................................ 834 G31 ................................................................................ 850 G31 Fn .......................................................................... 860 G31 P ............................................................................ 858 G31.n, G04 .................................................................... 856 G33 ............................................................................ 58, 62 G34 ................................................................................ 366 G35 ................................................................................ 367 G36 ................................................................................ 368 G37 ................................................................................ 846 G37.1 ............................................................................. 369 G38, G39/G40/G41, G42 .............................................. 245 G40.1/G41.1/G42.1(G150/G151/G152) ........................ 466 G40/G41, G42 ............................................................... 296 G40/G41.2,G42.2 .......................................................... 737 G41/G42 Commands and I, J, K Designation ............... 265 G43, G44/G49 ............................................................... 240 G43.1/G49 ..................................................................... 661 G43.4, G43.5/G49 ......................................................... 668 G43.7/G49 ..................................................................... 654 G45 to G48 .................................................................... 308 G50.1,G51.1 .................................................................. 462 G50/G51 ........................................................................ 823 G52 ................................................................................ 762 G53 ................................................................................ 757 G53.1/G53.6 .................................................................. 711 G54 to G59 (G54.1) ....................................................... 766 G60 .................................................................................. 70 G61 ................................................................................ 165 G61.1, G08 .................................................................... 567 G61.2 ............................................................................. 646 G61.4 ............................................................................. 639 G62 ................................................................................ 194 G63 ................................................................................ 196 G64 ................................................................................ 197 G65 ................................................................................ 388 G66 ................................................................................ 392 G66.1 ............................................................................. 394 G68.2, G68.3 ................................................................. 696 G68/G69 ................................................................ 781, 799 G73 ................................................................................ 347 G74 ................................................................................ 349 G75 ................................................................................ 351 G76 ................................................................................ 353 G81 ................................................................................ 322 G82 ................................................................................ 323 G83 ................................................................................ 324 G84 ................................................................................ 329 G85 ................................................................................ 341 G86 ................................................................................ 342 G87 ................................................................................ 343 G88 ................................................................................ 345 G89 ................................................................................ 346 G90,G91 .......................................................................... 30 G92 ........................................................................ 221, 760 G92.1 ............................................................................. 776 G93 ................................................................................ 133 G94,G95 ........................................................................ 130 G96,G97 ........................................................................ 215 G98,G99 ........................................................................ 357 General Precautions for Tool Radius Compensation .... 273 Geometric ...................................................................... 452 Geometric IB .................................................................. 454 Geometric IB (Automatic Calculation of Linear - Arc Intersection) ........................................................... 457, 460 Geometric IB (Automatic Calculation of Two-arc Contact) ... 455 Grid ................................................................................ 369 H Helical Interpolation ......................................................... 64 High-accuracy Control ................................................... 567 High-accuracy Spline Interpolation ................................ 646 High-speed High-accuracy Control ................................ 599 High-speed High-accuracy Control I, II, III ..................... 599 High-speed Machining Mode I, II ................................... 558 High-speed Mode Corner Deceleration ......................... 626 How to Define Feature Coordinate System Using Euler Angles ........................................................ 698 How to Define Feature Coordinate System Using Projection Angles ................................................. 706 How to Define Feature Coordinate System Using Roll-Pitch-Yaw Angles ......................................... 700 How to Define Feature Coordinate System Using Three Points in a Plane ....................................... 702 How to Define Feature Coordinate System Using Tool Axis Direction ............................................... 709 How to Define Feature Coordinate System Using Two Vectors ......................................................... 704 Hypothetical Axis Interpolation ...................................... 119 I Inch Thread Cutting ......................................................... 62 Inch/Metric Conversion .................................................... 32 Inclined Surface Machining ............................................ 696 Inclined Surface Machining and Relationship with Other Functions ....................................................................... 729 Index Table Indexing ..................................................... 207 Indexing Increment ............................................................ 8 Initial High-accuracy Control .......................................... 596 Initial Point and R Point Level Return ............................ 357 Inner Arc Override ......................................................... 195 Input Command Increment Tenfold ................................... 7 Input Setting Unit ............................................................... 6 Inputting The Tool Life Management Data by G10 L3 Command .................................................... 512 Inputting The Tool Life Management Data by G10 L30 Command .................................................. 515 Interference Check ........................................................ 279 Interrupt during Corner Chamfering/Interrupt during Corner Rounding ........................................ 446, 450 Interrupts during Tool Radius Compensation ................ 271 Inverse Time Feed ........................................................ 133 L Line at Angle ................................................................. 367 Linear Angle Command ................................................. 451 Linear Interpolation .......................................................... 45 Local Coordinate System Setting .................................. 762 Local Variables (#1 to #33) ........................................... 408 M M*** ............................................................................... 531 M198 ............................................................................. 378 M96, M97 ...................................................................... 429 M98 I_J_K_ ................................................................... 379 M98,M99 ....................................................................... 372 Machine Zero Point and 2nd, 3rd, 4th Reference Position (Zero Point) ................................................................... 752 Machining Condition Selection I .................................... 648 Macro Call Instructions .................................................. 388 Macro Interruption ......................................................... 429 Manual Arbitrary Reverse Run Prohibition .................... 486 Miscellaneous Command Macro Call (for M, S, T, B Code Macro Call) ................................... 397 Miscellaneous Functions (M8-digits) ............................. 204 Modal Call A (Movement Command Call) ..................... 392 Modal Call B (for each block) ........................................ 394 Modal, Unmodal .............................................................. 20 Multi-part System Simultaneous High-accuracy ............ 597 Multi-step Skip Function 1 ............................................. 856 Multi-step Skip Function 2 ............................................. 858 N Normal Line Control ...................................................... 466 Number of Tool Offset Sets Allocation to Part Systems .... 238 NURBS Interpolation ..................................................... 113 O Operation Commands ................................................... 412 Optional Block Skip ......................................................... 16 Optional Block Skip Addition ........................................... 18 Other Commands and Operations during Tool Radius Compensation ............................................................... 255 P Parameter Input by Program ......................................... 492 Plane Selection ............................................................... 56 Polar Coordinate Command ............................................ 96 Polar Coordinate Interpolation ......................................... 82 POPEN, PCLOS, DPRNT ............................................. 419 Position Command Methods ........................................... 30 Positioning (Rapid Traverse) ........................................... 42 Precautions ................................................................... 423 Precautions Before Starting Machining ........................... 25 Precautions for Inclined Surface Machining .................. 733 Precautions for Inputting The Tool Life Management Data ... 518 Precautions for Using a Fixed Cycle ............................. 355 Precautions on High-speed High-accuracy Control ....... 627 Pre-read Buffer ................................................................ 28 Program format ............................................................... 10 Programmable Current Limitation .................................. 868 R R Specification Circular Interpolation ............................... 53 Rapid Traverse Block Overlap ....................................... 176 Rapid Traverse Block Overlap for G00 .......................... 178 Rapid Traverse Block Overlap for G28 .......................... 186 Rapid Traverse Constant Inclination Acceleration/ Deceleration ................................................................... 142 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration .............................................. 147 Rapid Traverse Rate ...................................................... 122 Reference Position (Zero Point) Return ......................... 827 Reference Position Check ............................................. 837 Reverse Tapping Cycle ................................................. 349 R-Navi Data Input by Program ....................................... 506 Rotary Axis Basic Position Selection ............................. 723 S Scaling ........................................................................... 823 Setting of Workpiece Coordinates in Fixed Cycle Mode .... 358 Simple Macro Calls ........................................................ 388 Skip Function ................................................................. 850 Small Diameter Deep Hole Drilling Cycle ...................... 326 Smooth Fairing .............................................................. 616 Special Fixed Cycle ....................................................... 365 Speed Change Skip ....................................................... 860 Spindle Clamp Speed Setting ........................................ 221 Spindle Functions .......................................................... 214 Spindle Position Control (Spindle/C Axis Control) ......... 223 Spiral/Conical Interpolation ............................................ 103 Spline Interpolation ........................................................ 630 Spline Interpolation 2 ..................................................... 639 SSS Control ................................................................... 585 Start of Tool Radius Compensation and Z Axis Cut in Operation ....................................................................... 277 Stepping Cycle ............................................................... 347 Stroke Check before Travel ........................................... 840 Sub Part System Control I ............................................. 541 Subprogram Call .................................................... 372, 378 System Variable List ...................................................... 870 System Variables ........................................................... 411 System Variables (Alarm) .............................................. 897 System Variables (Coordinate Rotation Parameter) ...... 903 System Variables (Cumulative Time) ............................ 898 System Variables (Extended Workpiece Coordinate Offset) ... 891 System Variables (External Workpiece Coordinate Offset) ..... 892 System Variables (G Command Modal) ........................ 872 System Variables (Interfering Object Selection) ............ 933 System Variables (Machining Information) .................... 901 System Variables (Macro Interface Input (PLC -> NC)) ...... 911 System Variables (Macro Interface Output (NC -> PLC)) .... 917 System Variables (Message Display and Stop) ............. 898 System Variables (Mirror Image) ................................... 902 System Variables (Modal Information at Macro Interruption) .... 874 System Variables (Non-G Command Modal) ................ 873 System Variables (Normal Line Control Parameter) ...... 905 System Variables (Number of Workpiece Machining Times) .... 902 System Variables (Parameter Reading) ........................ 906 System Variables (PLC Data Reading) ......................... 929 System Variables (Position Information) ........................ 893 System Variables (R Device Access Variables) ............ 923 System Variables (Reverse Run Information) ............... 902 System Variables (Rotary Axis Configuration Parameter) ... 904 System Variables (Time Read Variables) ...................... 899 System Variables (Tool Compensation) ........................ 884 System Variables (Tool Information) ............................. 876 System Variables (Tool Life Management) .................... 885 System Variables (Workpiece Coordinate Offset) ......... 890 System Variables (Workpiece Installation Error Compensation Amount) ................................................. 910 System Variables (ZR Device Access Variables) .......... 936 T Tapping Cycle ............................................................... 329 Tapping Mode ............................................................... 196 Thread Cutting ................................................................. 58 Time Synchronization When Timing Synchronization Ignore Is Set .................................................................. 535 Timing Synchronization ................................................. 522 Timing Synchronization Operation (! code) ................... 522 Timing Synchronization Operation Function Using M codes ... 531 Timing Synchronization Operation with Start Point Designated (Type 1) ...................................................... 525 Timing Synchronization Operation with Start Point Designated (Type 2) ...................................................... 528 Tolerance Control .......................................................... 589 Tool Axis Direction Control ............................................ 711 Tool Center Point Control .............................................. 668 Tool Change Position Return ........................................ 834 Tool Compensation ....................................................... 234 Tool Functions (T8-digit BCD) ....................................... 232 Tool Length Compensation / Cancel ............................. 240 Tool Length Compensation Along the Tool Axis ........... 661 Tool Life Management Set Allocation to Part Systems ... 510, 519 Tool Nose Radius Compensation (for Machining Center System) ............................................................. 293 Tool Position Compensation ......................................... 654 Tool Position Offset ....................................................... 308 Tool Radius Compensation ........................................... 245 Tool Radius Compensation Operation .......................... 246 Tool Shape Input by Program ....................................... 503 Torque Limitation Skip ................................................... 864 U Unidirectional Positioning ................................................ 70 User Macro .................................................................... 387 User Macro Commands ................................................. 412 V Variable-acceleration Pre-interpolation Acceleration/ Deceleration .................................................................. 593 Variables Used in User Macros ..................................... 405 W Workpiece Coordinate Changing during Radius Compensation ............................................................... 291 Workpiece Coordinate System Preset ........................... 776 Workpiece Coordinate System Setting and Offset ........ 766 Revision History Date of revision Manual No. Revision details Apr. 2015 IB(NA)1501277-A IB(NA)1501278-A First edition created. Sep. 2015 IB(NA)1501277-B IB(NA)1501278-B The descriptions of M800 Series/M80 Series were revised in response to S/W version A4. The following chapters were added. 7.14.2 Inner Arc Override 15.9.3 Tool Shape Input by Program; G10 L100, G11 15.9.4 R-Navi Data Input by Program; G10 L110, G11 17.2.3 Tolerance Control 17.5 Spline Interpolation 2; G61.4 18.1.6 Define by Selecting the Registered Machining Surface The following chapters were revised. 1.1 Coordinate Words and Control Axes 3.4.2 G Code Lists 5.3 Decimal Point Input 7.3 F1-digit Feed 7.12 Deceleration Check 7.14 Automatic Corner Override 10.2 Constant Surface Speed Control; G96, G97 11.1 Tool Functions (T8-digit BCD) 12.3 Tool Length Compensation in the Tool Axis Direction; G43.1/G49 13.1.4 Tapping Cycle; G84 14.4 Macro Call Instructions 14.5.2 Local Variables (#1 to #33) 15.8 Manual Arbitrary Reverse Run Prohibition; G127 16.2 Sub Part System Control 17.1 High-speed Machining Mode 17.2 High-accuracy Control 17.3 High-speed High-accuracy Control 17.7 Machining Condition Selection I; G120.1, G121 18.1 Inclined Surface Machining; G68.2, G68.3 19.3 Basic Machine Coordinate System Selection; G53 19.6 Workpiece Coordinate System Setting and Offset; G54 to G59 (G54.1) 19.8 3-dimensional Coordinate Conversion; G68/G69 The following chapters were moved. Parameter Input by Program; G10 L70/L100, G11 (15.6 -> 15.9.1) Compensation Data Input by Program; G10 L2/L10/L11, G11 (12.7 -> 15.9.2) Tool Life Management Data Input; G10,G11 (12.7 -> 15.10) Other contents were added/revised/deleted according to specification. Apr. 2016 IB(NA)1501277-C IB(NA)1501278-C The descriptions of M800 Series/M80 Series were revised in response to S/W version B2. The following chapters were added. 12.5 Tool Nose Radius Compensation (for Machining Center System) 12.8 Tool Position Compensation; G43.7 15.9.3 Compensation Data Input by Program (Turning Tool); G10 L12/L13, G11 16.2 Mixed Control 16.2.1 Arbitrary Axis Exchange; G140, G141, G142 22 System Variables (Continue to the next page) Date of revision Manual No. Revision details (Continued from the previous page) The following chapters were revised. Introduction 3.4 G Codes 5.4 Decimal Point Input 6.3 Circular Interpolation; G02/G03 6.4 R Specification Circular Interpolation; G02, G03 6.7 Helical Interpolation; G17, G18, G19, and G02, G03 7.1 Rapid Traverse Rate 7.3 F1-digit Feed 7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration 7.13 Rapid Traverse Block Overlap; G0.5 P1 9.3 Index Table Indexing 10.2 Constant Surface Speed Control; G96, G97 10.4 Spindle Position Control (Spindle/C Axis Control) 12.1 Tool Compensation 13.1.4 Tapping Cycle; G84 14.1 Subprogram Control; M98, M99, M198 14.2 Variable Commands 14.4 Macro Call Instructions 14.6 User Macro Commands 15.7 Normal Line Control; G40.1/G41.1/G42.1 (G150/G151/G152) 15.8 Manual Arbitrary Reverse Run Prohibition; G127 15.9 Data Input by Program 16.3.1 Sub Part System Control I; G122 17.1 High-speed Machining Mode 17.2 High-accuracy Control 17.3 High-speed High-accuracy Control 18.1 Inclined Surface Machining; G68.2, G68.3 19.6 Workpiece Coordinate System Setting and Offset; G54 to G59 (G54.1) 19.10 Coordinate Rotation Input by Parameter ; G10 I_ J_/K_ 21.2 Skip Function; G31 Other mistakes were corrected. Sep. 2016 IB(NA)1501277-D IB(NA)1501278-D The descriptions were revised in response to S/W version C1 of M800 Series/M80 Series. The descriptions were revised in response to S/W version A1 of C80 Series. The following chapters were added. 18.3 Tool Center Point Control; G43.4, G43.5/G49 18.5 3-dimensional Tool Radius Compensation (Tool's vertical-direction compensation); G40/G41.2,G42.2 20.2 Enable Interfering Object Selection Data; G186 22.29 System Variables (Interfering Object Selection) 22.30 System Variables (ZR Device Access Variables) [C80] The following chapters were revised. Introduction Precautions for Safety 3.2 File Format 3.4 G Codes 6.9 Cylindrical Interpolation; G07.1 7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed); G94, G95 12.3 Tool Radius Compensation ; G38,G39/G40/G41,G42 14.1 Subprogram Control; M98, M99, M198 14.6 User Macro Commands 15.9.1 Parameter Input by Program; G10 L70/L100, G11 16.3 Sub Part System Control 17.1 High-speed Machining Mode 17.3 High-speed High-accuracy Control 17.5 Spline Interpolation 2; G61.4 (Continue to the next page) Date of revision Manual No. Revision details (Continued from the previous page) 18.1 Tool Position Compensation; G43.7 18.4 Inclined Surface Machining; G68.2, G68.3 18.5 3-dimensional Tool Radius Compensation (Tool's vertical-direction compensation); G40/G41.2, G42.2 19.7 Workpiece Coordinate System Preset; G92.1 19.10 Coordinate Rotation Input by Parameter ; G10 I_ J_/K_ 21.6 Torque Limitation Skip; G160 22.1 System Variable List 22.5 System Variables (Tool Information) 22.15 System Variables (Time Read Variables) 22.21 System Variables (Rotary Axis Configuration Parameter) 22.27 System Variables (R Device Access Variables) 22.28 System Variables (PLC Data Reading) The following chapters were moved. Tool Length Compensation in the Tool Axis Direction ; G43.1/G49 (12.3 -> 18.2) Tool Position Compensation; G43.7/G49 (12.8 -> 18.1 ) Other mistakes were corrected. M800/M80/C80 Series Manual List These contents are described in the presupposition that all functions of M800/M80/C80 Series are available. Some functions or screens may not be available depending on the machine or specifications set by MTB. (Confirm the specifications before use.) The manuals issued by MTB take precedence over these manuals. Manual M800/M80 Series Instruction Manual IB No. Purpose and Contents - Operation guide for NC IB-1501274 - Explanation for screen operation, etc. C80 Series Instruction Manual IB-1501453 - Operation guide for NC - Explanation for screen operation, etc. M800/M80/C80 Series Programming Manual (Lathe System) (1/2) IB-1501275 - G code programming for lathe system - Basic functions, etc. M800/M80/C80 Series Programming Manual (Lathe System) (2/2) IB-1501276 - G code programming for lathe system - Functions for multi-part system, high-accuracy function, etc. M800/M80/C80 Series Programming Manual (Machining Center System) (1/2) IB-1501277 - G code programming for machining center system - Basic functions, etc. M800/M80/C80 Series Programming Manual (Machining Center System) (2/2) IB-1501278 - G code programming for machining center system - Functions for multi-part system, high-accuracy function, etc. M800/M80/C80 Series Alarm/Parameter Manual IB-1501279 - Alarms - Parameters Manuals for MTBs (NC) Manual M800/M80/C80 Series Specifications Manual IB No. Purpose and Contents - Model selection IB-1501267 - Specifications of hardware unit - Outline of various functions M800W/M80W Series Connection and Setup Manual IB-1501268 - Detailed specifications of hardware unit - Installation, connection, wiring, setup (startup/adjustment) M800S/M80 Series Connection and Setup Manual IB-1501269 - Detailed specifications of hardware unit - Installation, connection, wiring, setup (startup/adjustment) C80 Series Connection and Setup Manual IB-1501452 - Detailed specifications of hardware unit - Installation, connection, wiring, setup (startup/adjustment) M800/M80 Series PLC Development Manual - Electrical design - I/O relation (assignment, setting, connection), field network IB-1501270 - Development environment (PLC on-board, peripheral development environment), etc. M800/M80 Series PLC Programming Manual - Electrical design IB-1501271 - Sequence programming - PLC support functions, etc. M800/M80/C80 Series PLC Interface Manual IB-1501272 - Electrical design - Interface signals between NC and PLC M800/M80 Series Maintenance Manual IB-1501273 - Cleaning and replacement for each unit - Other items related to maintenance C80 Series Maintenance Manual IB-1501454 - Cleaning and replacement for each unit - Other items related to maintenance Manuals for MTBs (drive section) Manual MDS-E/EH Series Specifications Manual IB No. Contents IB-1501226 - Specifications for power supply regeneration type MDS-E/EH Series Instruction Manual IB-1501229 - Instruction for power supply regeneration type MDS-EJ/EJH Series Specifications Manual IB-1501232 - Specifications for regenerative resistor type MDS-EJ/EJH Series Instruction Manual IB-1501235 - Instruction for regenerative resistor type MDS-EM/EMH Series Specifications Manual IB-1501238 - Specifications for multi-hybrid, power supply regeneration type MDS-EM/EMH Series Instruction Manual IB-1501241 - Instruction for multi-hybrid, power supply regeneration type DATA BOOK IB-1501252 - Specifications of servo drive unit, spindle drive unit, motor, etc. Global Service Network AMERICA EUROPE MITSUBISHI ELECTRIC AUTOMATION INC. (AMERICA FA CENTER) MITSUBISHI ELECTRIC EUROPE B.V. Central Region Service Center (Chicago) 500 CORPORATE WOODS PARKWAY, VERNON HILLS, ILLINOIS 60061, U.S.A. TEL: +1-847-478-2500 / FAX: +1-847-478-2650 Minneapolis, MN Service Satellite Detroit, MI Service Satellite Grand Rapids, MI Service Satellite Lima, OH Service Satellite Cleveland, OH Service Satellite Indianapolis, IN Service Satellite St. Louis, MO Service Satellite European Service Headquarter (Dusseldorf, GERMANY) Mitsubishi-Electric-Platz 1 40882 RATINGEN, GERMANY TEL: +49-2102-486-1850 / FAX: +49-2102-486-5910 South/East Region Service Center (Georgia) 1845 SATTELITE BOULEVARD STE. 450, DULUTH, GEORGIA 30097, U.S.A. TEL +1-678-258-4529 / FAX +1-678-258-4519 Charleston, SC Service Satellite Charlotte, NC Service Satellite Raleigh, NC Service Satellite Dallas, TX Service Satellite Houston, TX Service Satellite Hartford, CT Service Satellite Knoxville, TN Service Satellite Nashville, TN Service Satellite Baltimore, MD Service Satellite Pittsburg, PA Service Satellite Allentown, PA Service Satellite Syracuse, NY Service Satellite Tampa, FL Service Satellite Lafayette, LA Service Satellite Western Region Service Center (California) 5900-B KATELLA AVE. - 5900-A KATELLA AVE. CYPRESS, CALIFORNIA 90630, U.S.A. TEL: +1-714-699-2625 / FAX: +1-847-478-2650 San Francisco, CA Service Satellite Seattle, WA Service Satellite Canada Region Service Center (Tronto) 4299 14TH AVENUE MARKHAM, ONTARIO L3R OJ2, CANADA TEL: +1-905-754-3805 / FAX: +1-905-475-7935 Edmonton, AB Service Satellite Montreal, QC Service Satellite Mexico Region Service Center (Queretaro) Parque Tecnológico Innovación Querétaro, Lateral Carretera Estatal 431, Km 2+200, Lote 91 Modulos 1 y 2 Hacienda la Machorra, CP 76246, El Marqués, Querétaro, México TEL: +52-442-153 4250 Monterrey, NL Service Satellite Mexico City, DF Service Satellite BRAZIL MELCO CNC do Brasil Comércio e Serviços Ltda. Brazil Region Service Center AV. GISELE CONSTANTINO,1578， PARQUE BELA VISTA, VOTORANTIM-SP, BRAZIL CEP:18.110-650 TEL: +55-15-3023-9000 JOVIMAQ – Joinville, SC Service Satellite MAQSERVICE – Canoas, RS Service Satellite South Germany Service Center (Stuttgart) KURZE STRASSE. 40, 70794 FILDERSTADT-BONLANDEN, GERMANY TEL: + 49-711-770598-123 / FAX: +49-711-770598-141 France Service Center (Paris) 25, BOULEVARD DES BOUVETS, 92741 NANTERRE CEDEX FRANCE TEL: +33-1-41-02-83-13 / FAX: +33-1-49-01-07-25 France Service Satellite (Lyon) 120, ALLEE JACQUES MONOD 69800 SAINT PRIEST FRANCE TEL: +33-1-41-02-83-13 / FAX: +33-1-49-01-07-25 Italy Service Center (Milan) VIALE COLLEONI, 7 - CENTRO DIREZIONALE COLLEONI PALAZZO SIRIO INGRESSO 1, 20864 AGRATE BRIANZA (MB), ITALY TEL: +39-039-6053-342 / FAX: +39-039-6053-206 Italy Service Satellite (Padova) VIA G. SAVELLI, 24 - 35129 PADOVA, ITALY TEL: +39-039-6053-342 / FAX: +39-039-6053-206 U.K. Service Center TRAVELLERS LANE, HATFIELD, HERTFORDSHIRE, AL10 8XB, U.K. TEL: +49-2102-486-1850 / FAX: +49-2102-486-5910 Spain Service Center CTRA. DE RUBI, 76-80-APDO. 420, 08173 SAINT CUGAT DEL VALLES, BARCELONA SPAIN TEL: +34-935-65-2236 / FAX: +34-935-89-1579 Poland Service Center UL.KRAKOWSKA 50, 32-083 BALICE, POLAND TEL: +48-12-347-6500 / FAX: +48-12-630-4701 Hungary Service Center MADARASZ VIKTOR 47-49 , BUDAPEST XIII; HUNGARY TEL: +48-12-347-6500 / FAX: +48-12-630-4701 Turkey Service Center MITSUBISHI ELECTRIC TURKEY A.Ş SERIFALI MAHALLESI NUTUK SOKAK. NO.5 34775 UMRANIYE, ISTANBUL, TURKEY TEL: +90-216-526-3990 / FAX: +90-216-526-3995 Czech Republic Service Center AutoCont Control Systems s.r.o (Service Partner) KAFKOVA 1853/3, 702 00 OSTRAVA 2, CZECH REPUBLIC TEL: +420-59-5691-185 / FAX: +420-59-5691-199 Russia Service Center NC-TECH (Service Partner) 213, B.NOVODMITROVSKAYA STR., 14/2, 127015 MOSCOW, RUSSIA TEL: +7-495-748-0191 / FAX: +7-495-748-0192 Sweden Service Center HAMMARBACKEN 14, P.O.BOX 750 SE-19127, SOLLENTUNA, SWEDEN TEL: +46-8-6251000 / FAX: +46-8-966877 Bulgaria Service Center AKHNATON Ltd. (Service Partner) 4 ANDREJ LJAPCHEV BLVD. POB 21, BG-1756 SOFIA, BULGARIA TEL: +359-2-8176009 / FAX: +359-2-9744061 Ukraine Service Center (Kharkov) CSC Automation Ltd. (Service Partner) APTEKARSKIY PEREULOK 9-A, OFFICE 3, 61001 KHARKOV, UKRAINE TEL: +380-57-732-7774 / FAX: +380-57-731-8721 Belarus Service Center TECHNIKON Ltd. (Service Partner) NEZAVISIMOSTI PR.177, 220125 MINSK, BELARUS TEL: +375-17-393-1177 / FAX: +375-17-393-0081 South Africa Service Center MOTIONTRONIX (Service Partner) P.O. BOX 9234, EDLEEN, KEMPTON PARK GAUTENG, 1625, SOUTH AFRICA TEL: +27-11-394-8512 / FAX: +27-11-394-8513 ASEAN CHINA MITSUBISHI ELECTRIC ASIA PTE. LTD. (ASEAN FA CENTER) MITSUBISHI ELECTRIC AUTOMATION (CHINA) LTD. (CHINA FA CENTER) Singapore Service Center 307 ALEXANDRA ROAD #05-01/02 MITSUBISHI ELECTRIC BUILDING SINGAPORE 159943 TEL: +65-6473-2308 / FAX: +65-6476-7439 China Shanghai Service Center 1-3,5-10,18-23/F, NO.1386 HONG QIAO ROAD, CHANG NING QU, SHANGHAI 200336, CHINA TEL: +86-21-2322-3030 / FAX: +86-21-2322-3000*8422 China Ningbo Service Partner China Wuxi Service Partner China Jinan Service Partner China Hangzhou Service Partner Philippines Service Center Flexible (Service Partner) UNIT NO.411, ALABAMG CORPORATE CENTER KM 25. WEST SERVICE ROAD SOUTH SUPERHIGHWAY, ALABAMG MUNTINLUPA METRO MANILA, PHILIPPINES 1771 TEL: +63-2-807-2416 / FAX: +63-2-807-2417 VIETNAM MITSUBISHI ELECTRIC VIETNAM CO.,LTD Vietnam Ho Chi Minh Service Center UNIT 01-04, 10TH FLOOR, VINCOM CENTER 72 LE THANH TON STREET, DISTRICT 1, HO CHI MINH CITY, VIETNAM TEL: +84-8-3910 5945 / FAX: +84-8-3910 5946 Vietnam Hanoi Service Center 6TH FLOOR, DETECH TOWER, 8 TON THAT THUYET STREET, MY DINH 2 WARD, NAM TU LIEM DISTRICT, HA NOI CITY, VIETNAM TEL: +84-4-3937-8075 / FAX: +84-4-3937-8076 INDONESIA PT. MITSUBISHI ELECTRIC INDONESIA Indonesia Service Center (Cikarang) JL. KENARI RAYA BLOK G2-07A, DELTA SILICON 5, LIPPO CIKARANG - BEKASI 17550, INDONESIA TEL: +62-21-2961-7797 / FAX: +62-21-2961-7794 MALAYSIA MITSUBISHI ELECTRIC SALES MALAYSIA SDN. BHD. Malaysia Service Center (Kuala Lumpur Service Center) LOT 11, JALAN 219, P.O BOX 1036, 46860 PETALING JAYA, SELANGOR DARUL EHSAN. MALAYSIA TEL: +60-3-7960-2628 / FAX: +60-3-7960-2629 Johor Bahru Service satellite China Beijing Service Center 9/F, OFFICE TOWER 1, HENDERSON CENTER, 18 JIANGUOMENNEI DAJIE, DONGCHENG DISTRICT, BEIJING 100005, CHINA TEL: +86-10-6518-8830 / FAX: +86-10-6518-8030 China Beijing Service Partner China Tianjin Service Center UNIT 2003, TIANJIN CITY TOWER, NO 35 YOUYI ROAD, HEXI DISTRICT, TIANJIN 300061, CHINA TEL: +86-22-2813-1015 / FAX: +86-22-2813-1017 China Chengdu Service Center 1501-1503,15F,GUANG-HUA CENTRE BUILDING-C,NO.98 NORTH GUANG HUA 3th RD, CHENGDU,610000,CHINA TEL: +86-28-8446-8030 / FAX: +86-28-8446-8630 China Shenzhen Service Center ROOM 2512-2516, 25/F., GREAT CHINA INTERNATIONAL EXCHANGE SQUARE, JINTIAN RD.S., FUTIAN DISTRICT, SHENZHEN 518034, CHINA TEL: +86-755-2399-8272 / FAX: +86-755-8229-3686 China Xiamen Service Partner China DongGuang Service Partner China Dalian Service Center DONGBEI 3-5, DALIAN ECONOMIC & TECHNICAL DEVELOPMENTZONE, LIAONING PROVINCE, 116600, CHINA TEL: +86-411-8765-5951 / FAX: +86-411-8765-5952 KOREA MITSUBISHI ELECTRIC AUTOMATION KOREA CO., LTD. (KOREA FA CENTER) THAILAND MITSUBISHI ELECTRIC FACTORY AUTOMATION (THAILAND) CO.,LTD Thailand Service Center 12TH FLOOR, SV.CITY BUILDING, OFFICE TOWER 1, NO. 896/19 AND 20 RAMA 3 ROAD, KWAENG BANGPONGPANG, KHET YANNAWA, BANGKOK 10120,THAILAND TEL: +66-2-682-6522 / FAX: +66-2-682-6020 INDIA MITSUBISHI ELECTRIC INDIA PVT., LTD. CNC Technical Center (Bangalore) PLOT NO. 56, 4TH MAIN ROAD, PEENYA PHASE 3, PEENYA INDUSTRIAL AREA, BANGALORE 560058, KARNATAKA, INDIA TEL : +91-80-4655-2121 FAX : +91-80-4655-2147 Chennai Service Satellite Coimbatore Service Satellite Hyderabad Service Satellite North India Service Center (Gurgaon) 2ND FLOOR, TOWER A&B, DLF CYBER GREENS, DLF CYBER CITY, DLF PHASE-III, GURGAON- 122 002, HARYANA, INDIA TEL : +91-124-4630 300 FAX : +91-124-4630 399 Ludhiana Satellite Panth Nagar Service Satellite Delhi Service Satellite Jamshedpur Service Satellite West India Service Center (Pune) EMERALD HOUSE, EL-3, J BLOCK, M.I.D.C., BHOSARI, PUNE - 411026, MAHARASHTRA, INDIA TEL : +91-20-2710 2000 FAX : +91-20-2710 2100 Kolhapur Service Satellite Aurangabad Service Satellite Mumbai Service Satellite West India Service Center (Ahmedabad) UNIT NO: B/4, 3RD FLOOR, SAFAL PROFITAIRE, PRAHALADNAGAR CORPORATE ROAD, PRAHALADNAGAR SATELLITE, AHMEDABAD – 380015, GUJRAT, INDIA TEL : +91-265-2314699 Rajkot Service Satellite Korea Service Center 8F GANGSEO HANGANG XI-TOWER A, 401 YANGCHEON-RO, GANGSEO-GU, SEOUL 07528 KOREA TEL: +82-2-3660-9609 / FAX: +82-2-3664-8668 Korea Daegu Service Satellite TAIWAN MITSUBISHI ELECTRIC TAIWAN CO., LTD. (TAIWAN FA CENTER) Taiwan Taichung Service Center NO.8-1, INDUSTRIAL 16TH RD., TAICHUNG INDUSTRIAL PARK, SITUN DIST., TAICHUNG CITY 40768, TAIWAN TEL: +886-4-2359-0688 / FAX: +886-4-2359-0689 Taiwan Taipei Service Center 10F, NO.88, SEC.6, CHUNG-SHAN N. RD., SHI LIN DIST., TAIPEI CITY 11155, TAIWAN TEL: +886-2-2833-5430 / FAX: +886-2-2833-5433 Taiwan Tainan Service Center 11F-1., NO.30, ZHONGZHENG S. ROAD, YONGKANG DISTRICT, TAINAN CITY 71067, TAIWAN TEL: +886-6-252-5030 / FAX: +886-6-252-5031 OCEANIA MITSUBISHI ELECTRIC AUSTRALIA PTY. LTD. Oceania Service Center 348 VICTORIA ROAD, RYDALMERE, N.S.W. 2116 AUSTRALIA TEL: +61-2-9684-7269/ FAX: +61-2-9684-7245 Notice Every effort has been made to keep up with software and hardware revisions in the contents described in this manual. However, please understand that in some unavoidable cases simultaneous revision is not possible. Please contact your Mitsubishi Electric dealer with any questions or comments regarding the use of this product. Duplication Prohibited This manual may not be reproduced in any form, in part or in whole, without written permission from Mitsubishi Electric Corporation. COPYRIGHT 2015-2016 MITSUBISHI ELECTRIC CORPORATION ALL RIGHTS RESERVED
advertisement
* Your assessment is very important for improving the workof artificial intelligence, which forms the content of this project
Key Features
- User-friendly interface makes programming easy
- Advanced control algorithms ensure precise and efficient machining
- Robust construction for long-lasting performance
- Wide range of features and capabilities to meet the needs of any application
- Supports a variety of machine tools, including lathes, machining centers, and grinders
- Can be used for a variety of applications, from simple to complex
Related manuals
Frequently Answers and Questions
What are the benefits of using the M800/M80/C80 Series?
The M800/M80/C80 Series offers a number of benefits, including increased productivity, improved accuracy and surface finish, and reduced operating costs.
What are the different models of the M800/M80/C80 Series?
The M800/M80/C80 Series includes three different models: the M800W series, the M800S series, and the M80W series.
What are the key features of the M800/M80/C80 Series?
The key features of the M800/M80/C80 Series include its user-friendly interface, advanced control algorithms, robust construction, and wide range of features and capabilities.
advertisement