Part Programming Manual MACHINEMATE

Transcription

1 MACHINEMATE

2 NOTE Progress is an ongoing commitment at MACHINEMATE INC. We continually strive to offer the most advanced products in the industry. Therefore, information in this document is subject to change without notice. The illustrations and specifications in this document are not binding in detail. MACHINEMATE INC shall not be liable for any technical or editorial omissions occurring in this document nor for any consequential or incidental damages resulting from the use of this document. DO NOT ATTEMPT to use any MACHINEMATE INC product until the use of such product is completely understood. It is the responsibility of the user to make certain proper operation practices are understood. MACHINEMATE INC products should be used only by qualified personnel and for the express purpose for which said products were designed. Should information not covered in this document be required, please contact: MACHINEMATE INC. Fond du Lac, WI Phone: Fax: Document revision: 0712 page 2/352

3 Table of Contents TABLE OF FIGURES AND TABLES BASICS OF NC PROGRAMMING Program Layout Program block Program Word Auxiliary functions (BCDs) Programming functional overview Block suppression Program Repetition Subroutines Comments in NC programs Program number Cycle block layout Reading from External Data Files Program Safety Axis designations for machine tool machines Gantry Axes Resettable Rotational Axis POSITIONING INSTRUCTIONS General positioning instructions Monitoring the axis travel limits G00 linear interpolation in rapid traverse G01 linear interpolation in the feed rate G02, G03 circular interpolation with specified center point G12, G13 circular interpolation with specified radius Helical Interpolation G74 Programmable homing M80 delete remaining path using probe function Positioning instructions G07 Tangential circular interpolation G05, G06 Spline Definition and Spline Interpolation 2D G78, G79 Tangential Setting to the 2D Path INFLUENCING THE PROGRAM M00 program interruption (unconditional stop) M01 program interruption (conditional stop) M02, M30 end of program G10, G11 empty/fill dynamic block buffer G10 Empty dynamic block buffer G11 Fill dynamic block buffer G72, G73 interpolation with precision stop OFF or ON G08, G09 look ahead OFF or ON G186 corner acceleration, contour accuracy Corner Acceleration Contour Accuracy: G75, G76 Curvature...84 page 3/352

4 3.8.1 Curvature Activation Curvature Acceleration Limit G04 dwell time Corner Smoothing G-codes Curvature radius R Corner deviation E Minimum block length Acceleration monitoring Minimum and maximum bend angle The necessity of corner smoothing Programming Problem case: angle too acute Problem case: collision monitor with real-time mill radius correction TECHNOLOGICAL INSTRUCTIONS Influencing the feedrate G94 Inches (Millimeters) per minute IPM/MMPM G95 Inches (Millimeters) per revolution IPR/MMPR F word for feed rate G63, G66 Feed override Programmable acceleration Spindle Control S Word M03, M04 Spindle ON, Clockwise or Counter-Clockwise M05 Spindle OFF M19 Spindle Orientation G63, G66 Spindle Override G92 Spindle speed limitation G96 Constant Surface Speed (Feet/Meter) G97 Revolutions per minute Reversal of rotation at M19, spindle orientation Tool compensation functions Tool radius compensation Tool length compensation values Tool or turret selection Advanced Regulation Technology (ART) Application GEOMETRIC INSTRUCTIONS General geometric instructions G40-G44 Path compensations G53-G59 Part position offsets G70, G71 Programming in metric or inch format G90, G91 Absolute/incremental dimension programming G92 Set axis value G14-G16 Polar coordinate programming Specific geometric instructions page 4/352

5 5.2.1 G17-G20 Plane selection G24-G27 Programmable work field limitation (Safe Zone Programming) G38, G39 Programmable axis motion mirror G51, G52 Part rotation G50 Scaling Dresser, wheel or tool tip radius compensation (DWRC) Entering compensation values in tables Dresser Wheel Radius Compensation DWRC application schemes NC block formats Compensation Entry/Exit Move Types Special Cases GENERAL CYCLE PROGRAMMING Introduction Application of Cycle Blocks Cycle programming Integrating Cycle Blocks in an NC Program Comments Cycle block syntax Basic rules for processing of instructions Numbers and variables Calculation operations and functions Use of P-parameters Use of CNC parameters Conditional instructions and jump instructions Possible errors Instructions Work Cycles General notes Example DRILLING CYCLES Introduction Use of the drilling cycles Allocation of the parameters/definition of terms Selection of the desired drilling cycle Move to the drilling position in X and Y (once or repeatedly) Deselecting of the drilling cycle G80 Cancel the drilling cycle G81 Drilling to final depth G82 Spot facing with dwell time G83 Deep hole drilling G84 Thread cutting with balanced chuck G85 Reaming G86 Bore out G87 Reaming with measuring stop G88 Bore out with spindle halt page 5/352

6 7.12 G89 Bore out with intermediate halt Example: base plate PROGRAM OPTIMIZATION Hints for rational program creation Subroutines Modally effective instructions Value allocation to NC addresses using parameters Hints for Processing Programs Look Ahead Programmable acceleration at Look Ahead Activation of special functions using a subroutine Hints for Avoiding Errors Protection of subroutines against call up as main program Functions not automatically reset at the program end Circular interpolation Avoid dummy blocks at subroutine call up Avoid dummy blocks at subroutine end Avoid dummy blocks at path compensation Collision free movement Contour accuracy (G186) PROGRAMMING VARIOUS CNC FEATURES/CAPABILITIES Angled Wheel Transformation Angled wheel transformation syntax Axes sequence by two step mode Mirroring H and G compensation Automatic Spindle Gear Step (Range) Selection General M40 is Active M41 to M46 is Active Switchover procedure between gear ranges G96 is Active G92 is Active G33/G34 is Active Barrel Cam Transformation General Barrel cam transformation using Cartesian coordinates G Barrel cam transformation with cylinder coordinates G Illegal G-codes during Barrel Cam Real time radius compensation G103, G Barrel cam transformation with centerline deviation of an additional axis and real time radius compensation, G104, G Switching between machine coordinates with barrel cam transformation End of program and change of the operating mode Diameter Programming Programming page 6/352

7 9.4.2 Control reset, end of program Display functions Programming conditions Programming Examples Distance Regulation G265 Axis selection M140 / M141 activation/deactivation of distance regulation Monitoring the axis limits G74 is invalid Fast output signals Output turned on or off by CNC with M-code Position-defined fast M-functions Feed Influencing via Probe Signals General Programming Programming measurement probe logic Masking out input bits via the PLC G92 and setting the remaining distance to zero Measurement probe logic via the interface signal Dwell time Programming with Stop on block pre-processing Feed Interpolation Function and handling Handwheels in Automatic mode General Programming End of program and control reset Cycle-Stop, Cycle-Off Infinitely Rotating Round (or Rotary) Axis General Programming Normal round axis Tool magazine round axis Modulo round axis Multiple Spindles General Spindle programming Thread cutting, G33 and G Spindle speed override rotary switch, G Spindle speed restriction, G Feed rate in mm / rev, or in / rev, G G93, G96 and G Spindle orientation, M Spindle / rotational axis switchover Gear ranges or gear stages Parallel Axes Syntax page 7/352

8 Program examples Positioning Axis Introduction Programming Programmable Oscillation Preparation set Erasing oscillation data Deviation lengths Number of deviations Frequency Dwell times Behavior in case of programming errors Behavior in case of Emergency Stop M20 Start M-code M21 End M-code M00 Programming Program end / home position Error messages Switchover Spindle-Rotary Axis General Programming Spindle running Thread Cutting or Rigid Tapping General Spindle Control Programming thread with uniform pitch, G Programming thread with dynamic pitch, G Definition of the thread block Programming cylindrical thread, G33, G Programming conical thread G33, G Programming lag free thread, G133, G Turning Cycles or Stock Removal Cycles General G271 Stock removal in turning G272 Stock removal in facing Direction of allowance G270 Finishing Cycle G274 Peck finishing cycle G275 Outer diameter/internal diameter turning cycle G276 Multiple pass threading cycle Error messages Part program display PROGRAMMING MACHINEMATE SPECIAL FEATURES Lathe T-code Programming Programming a Rotary-only Motion in G G93 for Programming a Mix of Linear and Rotary Motion Canned Drilling Cycle Letter Programming page 8/352

9 Canned Cycle Programming with Letters not Parameters Canned Cycle Programming: Cross Reference to Section Canned Cycle Programming Examples Two-axes Collinear Tracking Programming Extended Part Offsets Programming Programming the additional Part Offsets Managing the additional part offsets INDEX page 9/352

10 Table of Figures and Tables Figure 1-1: Elements of an NC program Table 1-1: G-Codes Table 1-2: M-Codes Figure 1-2: Nesting depth Table 1-3: ASCII Character Set Figure 1-3: Orientation of the three basic feed axes using the right-hand rule Figure 1-4: Work piece rigid, tool rotates Figure 1-5: Work piece rotates, tool rigid Figure 1-6: Position and direction of feed rate and rotary axes Figure 2-1: G00 when turning Figure 2-2: G00 when milling Figure 2-3: Two successive rapid traverse positioning instructions Figure 2-4: Absolute dimension coordinates (G90) Figure 2-5: Incremental dimension coordinates (G91) Figure 2-6: G01 when turning Figure 2-7: G01 when milling Figure 2-8: G01 Linear interpolation in the feed rate Figure 2-9: Direction of rotation with G02 and G03 (turning) Figure 2-10: Direction of rotation with G02 and G03 (milling) Table 2-1: Interpolation parameters at G02 and G03 (at G17, G18 and G19) Figure 2-11: Example for G Figure 2-12: G12, G13 Circular interpolation in the counter-clockwise direction with specified radius with K > 0 and K < Figure 2-13: G12, G13 circular interpolation with specified radius Figure 2-14: Delete remaining path using probe function (ignoring the probe's radius).. 53 Figure 2-15: Delete remaining path using probe function and measuring probe radius Figure 2-16: CNC reaction to the probe contact Figure 2-17: Straight line/circular arc Figure 2-18: Straight line/circular arc Figure 2-19: Circular arc/circular arc Figure 2-20: M70: Start of spline and end of spline with the curve 0 (natural spline) Figure 2-21: M71: Start of spline with tangential transition and end with curve Figure 2-22: M72: Start of spline with curve 0 and end of spline with tangential transition 61 Figure 2-23: M73: Start of spline and end of spline with tangential transitions Figure 2-24: Path velocity with linear interpolation and spline interpolation Figure 2-25: Tangential setting to the 2D path Figure 2-26: Tangential setting to the 2D path when turning Figure 2-27: Tangential setting to the 2D path when punching/nibbling Figure 2-28: Programming the leading-in at a specific angle Figure 2-29: Programming a changing angle offset using G Figure 2-30: Behavior of the lead-in during a reversal of the motion direction Figure 2-31: Influence of the lead-in at reversal of motion reversal page 10/352

11 Figure 3-1: Contour with contouring error Figure 3-2: Contour processed with precision stop Figure 3-3: Processing of NC blocks with and without "Look Ahead" Table 3-1: Effect of different E word values Figure 3-4: Sharp decrease in speed between motion blocks dependent on the corner acceleration Figure 3-5: Sharp decrease in speed dependent on the angle between successive motion blocks. 82 Figure 3-6: Circle reduction error when pulling out of a circle from standstill Figure 3-7: Corner deviation E Figure 3-8: Curvature radius R Figure 3-9: Curvature radius R with a minimum path shortened Figure 3-10: Curvature bend angle in a corner Figure 3-11: Corner smoothing and corner jumps Figure 3-12: Corner smoothing in G Figure 3-13: Real-time radius correction with corner smoothing Figure 3-14: Corner smoothing with corners rounded outside not inside Figure 4-1: Tool tip radius compensation for rotating tools Figure 4-2: Tool length compensation for rotating tools Figure 4-3: Tool length compensation for fixed tools Figure 5-1: Effect of different tool radii on the work piece contour Figure 5-2: Equidistant left and right of the work piece contour Figure 5-3: Path compensation at the block transition Straight line/straight line Figure 5-4: Path compensation at the block transition Straight line/circular arc Figure 5-5: Path compensation at the block transition circular arc/circular arc Figure 5-6: Move to intersection on a linear path Figure 5-7: Move to intersection on a spiral path Figure 5-8: Comparison of path compensations G41 and G Figure 5-9: Retreat on a linear path Figure 5-10: Retreat on a spiral path Figure 5-11: Generation of intermediate blocks, example Figure 5-12: Generation of intermediate blocks, example Figure 5-13: Generation of intermediate blocks, example Figure 5-14: Angle cut off Figure 5-15: End point radius compensation Figure 5-16: Real-time radius compensation Figure 5-17: Insufficient cutting of internal contours with real-time radius compensation 130 Figure 5-18: Motion with blocks without positioning information in the active plane Figure 5-19: Motion with a change between G41 and G Figure 5-20: Motion with a sign change of the compensation value Figure 5-21: Motion with change of compensation value but no sign change, example Figure 5-22: Motion with change of compensation value but no sign change, example Figure 5-23: Motion with a tool radius that is too large for an inside corner Figure 5-24: Radius smaller than compensation value (R < D) page 11/352

12 Figure 5-25: Motion with a full circle as external contour (with G42) Figure 5-26: Motion with a full circle as external contour (with G44) Figure 5-27: Motion with a full circle as internal contour (with radius compensation). 142 Figure 5-28: Full circle as external contour (with radius compensation) Figure 5-29: Processing with external path compensation at corners, internal contour processing 144 Figure 5-30: Setting work piece zero points Figure 5-31: Programming in metric or imperial format Figure 5-32: Dimension input in absolute dimension programming Figure 5-33: Dimension input in incremental dimension programming Figure 5-34: Set axis value with G Figure 5-35: Definition of a reference point for work piece zero points Figure 5-36: Polar coordinates Table 5-1: Major axis and minor axis Table 5-2: Angle and radius values in the three predefined planes Figure 5-37: Polar coordinate programming without pole point information Figure 5-38: Polar coordinate programming with pole point information Figure 5-39: Circular interpolation plane selection Table 5-3: Circular interpolation planes (G20) Figure 5-40: Work area of a machine tool with the axes X and Y Figure 5-41: Programmable mirror, effect of the programs P1 to P Figure 5-42: Mirror with prior setting of an axis value using G Figure 5-43: Part rotation in the case of active G Figure 5-44: Part rotation in combination with incremental programming (G91) Figure 5-45: Scaling with absolute and relative dimension input Figure 5-46: Grinding wheel offset definitions Figure 5-47: Grinding wheel radius orientation definitions Figure 5-48: Dresser or tool tip radius orientation definitions Figure 5-49: Grinding wheel control point and gauge point definitions Figure 5-50: Inside corner definition Table 5-4: Differences between DWRC entry/exit move types A, B, C Table 5-5: G-codes for DWRC path compensation Table 5-6: Application schemes for DWRC path compensation Figure 5-51: Dress/wheel radius compensation example Figure 5-52: Wheel corner radius compensation example Table 5-7: Activations of DWRC path compensation Figure 5-53: Linear and circular intermediate blocks Figure 5-54: The three compensation entry move types (overview) Figure 5-55: Compensation entry moves type A, linear to linear Figure 5-56: Compensation entry moves type A, linear to circular Figure 5-57: Compensation entry moves type A, circular to linear Figure 5-58: Compensation entry moves type A, circular to circular Figure 5-59: Compensation entry moves type B, linear to linear Figure 5-60: Compensation entry moves type B, circular intermediate blocks Figure 5-61: Compensation entry moves type C, linear to linear Table 6-1: Cycle programming: parameters and instructions Figure 6-1: Transfer of the NC blocks to the interpolator process page 12/352

13 Table 6-2: Calculation operations and functions Table 6-3: Reserved cycle parameters Table 6-4: Summary of CNC data as cycle parameters Table 6-5: IF comparison operators Table 6-6: Summary of cycle block SEL functions Figure 7-1: Reference plane, retract plane and final hole depth Figure 7-2: Drilling cycle G Figure 7-3: Drilling cycle G Figure 7-4: Drilling cycle G Figure 7-5: Drilling cycle G Figure 7-6: Drilling cycle G Figure 7-7: Drilling cycle G Figure 7-8: Drilling cycle G Figure 7-9: Drilling cycle G Figure 7-10: Drilling cycle G Figure 7-11: Example: Base plate Figure 9-1: Relationship between two linear axes with Angled Wheel Transformation 252 Figure 9-2: Example for G222, two step move for Angled Wheel Transformation Table 9-1: Angled Wheel Transformation two-step motion description Figure 9-3: Interpretation of the X and Y values when G102 is active Figure 9-4: Barrel cam transformation Figure 9-5: Meaning of the C and V values when G106 is active Figure 9-6: Osculation plane axis allocations for the cylinder Figure 9-7: Real-time radius compensation Figure 9-8: Barrel cam transformation with centerline deviation Figure 9-9: Diameter Programming Table 9-2: Diameter programming G-codes Figure 9-10: Diameter Programming with negative orientation Figure 9-11: Diameter Programming Point of Contact Table 9-3: Diameter programming conditions Figure 9-12: Position-defined fast M-functions Figure 9-13: Rotations of a normal round axis Table 9-4: Programmable values for a round axis Figure 9-14: Rotations of A axis (normal round) Table 9-5: Programmable values for a tool magazine axis Figure 9-15: Tool magazine round axis Figure 9-16: Modulo round axis Table 9-6: Programmable values for a modulo axis Table 9-7: Definition of a G33/G34 thread block Figure 9-17: Work piece before G33 processing Figure 9-18: Work piece after processing with G Figure 9-19: Work piece with controller running out (G33) Figure 9-20: Work piece with increasing pitch (G34) Figure 9-21: Work piece with decreasing pitch (G34) Figure 9-22: Work piece before processing with G Figure 9-23: Work piece after processing with G page 13/352

14 Figure 9-24: Work piece with controlled running out (G33) Figure 9-25: Stock removal Figure 9-26: Stock removal: direction of allowance Figure 9-27: Stock removal in facing Figure 9-28: Stock removal in facing: direction of removal Figure 9-29: G274 peck finishing cycle Figure 9-30: G275 inner/outer diameter turning cycle Figure 9-31: G276 multiple pass thread turning cycle Figure 9-32: G276 threading cycle and tool tip parameters page 14/352

15 1 Basics of NC Programming 1.1 Program Layout An NC program (part program) is a sequence of processing steps and is divided into program blocks. Each program block contains the information that the machine requires to perform the desired process. N10 G90 Additional conditions N20 G1 X50 Y20 F120 M3 S100 N30 X15 Instruction Sequence of digits Program blocks N40 Y-20 X25 N50 G4 F1000 Address letter Program words Block number Figure 1-1: Elements of an NC program 1.2 Program block Individual lines of an NC program are called program blocks or NC blocks. A program block is the smallest work step that can be taken when processing a work piece. A program block begins with a block number and ends with a block end character. A block number is made up of the address character N with a maximum of four digits. Leading zeros can be omitted. Blocks without block numbers can neither be read nor entered during programming. The block end character used by the CNC is the linefeed character (0AH). Placing a slash / (block slash code) before a block allows the block to be ignored or masked out. (See 1.5 Block Suppression.) The maximum length of a program block is 128 characters (including block end character and optional checksum). To allow editing of an NC program the program blocks are numbered sequentially in blocks of ten with rising block numbers. This provides easy location of program blocks and insertion of additional blocks. Example: N10 G90 N20 G1 X50 Y20 F3000 M3 S1000 N30 X15 page 15/352

16 1.3 Program Word N40 Y-20 X25 N50 G4 F1000 N60 M30 The NC blocks being manually input into the CNC are automatically sorted according to block numbers. The NC block with the lowest block number appears at the beginning of the program and the one with the highest number at the end. The program blocks are processed in the sequence in which they were stored. NC programs entered directly into the CNC are also processed by increasing block numbers. NC programs that have been externally created and then read into the CNC may not be processed by increasing block numbers because the program is not checked for increasing block numbers when loaded. The externally created program will be processed sequentially as ordered in the file, not by increasing block number. The individual information in a program block is called a program word. A program word contains technical, geometrical or technological information related to the program. The sequence of the program words in a block is arbitrary. A program word is made up of an address letter and a sequence of digits with or without a sign. The address letter designates the type of program word. Each address letter must only be programmed once per NC block. If the same address letter is programmed several times in a block during program input, the program block is rejected (error message 5 appears). If the same address letter appears repeatedly in a block from an externally created program that is read into the CNC, the last address letter read becomes effective. The sequence of digits of a word is an integer or a number, consisting of an integer value and a decimal fraction that can be zero. The decimal is separated from the integer by a period. A comma is not admissible. Signs are programmed between address letter and sequence of digits. Positive signs, leading zeros and nonsignificant zeros after the decimal point do not need to be programmed. If the decimal point is not followed by any significant digits, it is automatically set in the display. Example: G1 instead of: M1 instead of: G01 M01 X instead of: X Y12 instead of: Y Z-25.4 instead of: Z There are common uses for many of the letters. These conventions are listed below. Note that these are not all permanent letter assignments. It is possible for axes to get page 16/352

17 any of the letters A, B, C, O, U, V, W, X, Y, Z and for any of these letters to be either a rotary or linear axis. The following axis assignments are typical and are described in more detail later (see 1.15). A B C D F G H I J K L M N P Q R S T X Y Z A-axis command (usually a rotary) B-axis command (usually a rotary) C-axis command (usually a rotary) Tool diameter/radius compensation number Feedrate value CNC function or code Tool length compensation number Circle center distance for X Circle center distance for Y Circle center distance for Z or circle radius (G12/G13) Loop count for subroutine/macro Machine function or code Block sequence number Macro programming variable Subroutine program number to call Rotation or scaling factor Spindle speed (RPM) Tool number or turret position X-axis command (usually a linear) Y-axis command (usually a linear) Z-axis command (usually a linear) The D, F, G, H, I, J, K, M, N, P, Q, R, S letter assignments are permanent, per this list, except where the syntax defined in this manual identifies an alternate meaning (e.g., P and Q are also used in turning cycles, in 9.17) or a feature is not used (e.g., R could be an axis only if G50 to G52 were never used). Note that typically the letters D, G, H, L, M, N, P, Q, S, T never have a decimal point. Program words are considered instructions or additional conditions. An instruction (e.g., G- or M-codes) prepares or triggers a process in the machine tool or the control. An additional condition describes the instructions more exactly (e.g., specifying the destination coordinates for a positioning instruction). Program words can be distinguished as either modal (retentive) or non-modal. Modal program words are active in all following program blocks until they are overridden or overwritten by an instruction or additional condition that cancels them. Non-modal program words are only active in the block in which they are programmed. Modal instructions must therefore only be programmed when they are changing or when additions are necessary. Non-modal instructions have to be programmed in each block in which they are included. Instructions are organized into instruction groups. In any one instruction group all the instructions are summed up but only one instruction can be in effect at a time. Table 1-1 on the following pages contains G-Codes available in the CNC. The tables include notes on group division, effectiveness, whether the respective instruction is page 17/352

18 active at CONTROL RESET and whether positioning instructions are programmable in the same block. G-Codes used to program travel movements within the same block are marked in Table 1-1 by an asterisk (*). Table 1-2 on the following pages contains M-codes, some of which are available only in application specific versions of the CNC. G-Function Meaning Group Effectivity Active after reset? G00 * Linear interpolation with maximum speed 1 Modal G01 * Linear interpolation with programmed speed 1 Modal Yes G02 * Circle or helical interpolation with defined circle 1 Modal G03 * center (clockwise) Circle of helical interpolation (counter clockwise) 1 Modal G04 * Dwell time Blockwise G05 * Definition of spline Blockwise G06 * Activation of spline 1 Modal G07 * Tangential arc interpolation 1 Modal G08 * Look Ahead OFF 7 Modal Yes G09 * Look Ahead ON 7 Modal G10 * Clean dynamic buffer Blockwise G11 * Fill up dynamic buffer Blockwise G12 * Arc interpolation with defined radius (clockwise) 1 Modal G13 * Arc interpolation with radius (counter clockwise) 1 Modal G14 * Polar coordinate programming absolute 3 Modal G15 * Polar coordinate programming incremental 3 Modal G16 * Definition of coordinate system Blockwise G17 * G18 * G19 * G20 * Plane select X/Y Plane select Z/X Plane select Y/Z Plane select programmable Modal Modal Modal Modal G21 * Parallel axis ON 14 Modal G22 * Parallel axis OFF 14 Modal G24 * Work area limit lower boundary Blockwise G25 * Work area limit upper boundary Blockwise G26 * Work area limit OFF 9 Modal G27 Work area limit ON 9 Modal G33 * Thread cutting, constant pitch 1 Modal G34 * Thread cutting, variable pitch 1 Modal G35 * Oscillation Blockwise G38 Programmable mirroring ON 10 Modal G39 * Programmable mirroring OFF 10 Modal G40 * G41 * G42 * G43 * G44 * Tool radius correction OFF Tool radius correction to the left Tool radius correction to the right Tool radius correction to the left with modified activation Tool radius correction to the right with modified activation Modal Modal Modal Modal Modal G45 * Linear intermediate blocks Modal G46 * Circular intermediate blocks Modal G50 * Scaling Modal G51 * Part rotation degrees Modal G52 * Part rotation radians Modal Yes Yes Yes Yes page 18/352

19 G53 * G54 * G55 * G56 * G57 * G58 * G59 * G63 * G66 * G70 * G71 * G72 * G73 * Zero point shifting OFF Zero point shifting 1 ON Zero point shifting 2 ON Zero point shifting 3 ON Zero point shifting 4 ON Zero point shifting 5 ON Zero point shifting 6 ON Feed/spindle override ON Feed/spindle override OFF Programming in inches Programming in metric (mm) Interpolation with exact position OFF Interpolation with exact position ON page 19/ Modal Modal Modal Modal Modal Modal Modal Modal Modal Modal Modal Modal Modal G74 Programmable homing Blockwise G75 G76 Curvature activation Curvature acceleration 7 7 Modal Modal G78 * Tangential direction 2D control ON Modal G79 * Tangential direction 2D control OFF Modal G80 * Canned Drilling Cycles (work cycles) Canned cycle off Modal G81 ^ Drilling to final depth Modal G82 ^ Spot facing with dwell time Modal G83 ^ Deep hole drilling Modal G84 ^ Tapping or thread cutting with balanced chuck Modal G85 ^ Reaming Modal G86 ^ Boring Modal G87 ^ Reaming with measuring stop Modal G88 ^ Boring with spindle stop Modal G89 ^ Boring with intermediate stop Modal G90 * Absolute programming 3 Modal G91 * incremental programming 3 Modal G92 Zero point setting, maximum spindle speed Modal G94 * Feed in millimeters/minute 5 Modal G95 * Feed in millimeters/revolution 5 Modal G96 * Constant cutting speed ON 15 Modal G97 * Constant cutting speed OFF 15 Modal G98 ^ Positioning axis dwell time Blockwise G99 * Axis offset Modal G100 Polar/cylindrical transformation OFF Modal G101 ^ Polar/cylindrical transformation ON Modal G102 ^ Cylindrical transformation ON Modal G103 ^ Barrel CAM transformation, real time radius comp Modal G104 ^ Barrel CAM transformation with centerline deviation Modal G105 ^ G101 with alternative axis addresses Modal G106 ^ G102 with alternative axes addresses Modal G107 ^ G103 with alternative axes addresses Modal G108 ^ G104 with alternative axes addresses Modal G109 * Axis transformation programming of tool depth Modal G110 ^ Axes selection laser power control Blockwise G111 * Definition of voltage 1 (V1), speed (F1), time (T1) Blockwise G112 * Definition of voltage 2 (V2), speed (F2), time (T2) Blockwise G113 * Definition of voltage 3 (V3), speed (F3), time (T3) Blockwise G114 * Definition of time 4 (T4) Blockwise G115 * Definition of time 5 (T5) Blockwise G116 * Definition of time 6 (T6) Blockwise G117 * Definition of time 7 (T7) Blockwise G120 G121 G125 G126 G127 Axis transformation; orientation change of rotary axis Axis transformation; orientation change in a plane Electronic gear box; plain teeth Electronic gear box; helical gearing, axial Electronic gear box; helical gearing, tangential Modal Modal Modal Modal Modal Yes Yes Yes Yes Yes Yes Yes

20 G128 Electronic gear box; helical gearing, diagonal Modal G130 G131 G132 Axis transformation; program orientation change Axis transformation; orientation change Axis transformation; orientation change Modal Modal Modal G133 Lag free threading learning ON Modal G134 G140 G141 G150 G151 G152 G160 G161 ^ G162 ^ G163 ^ G164 ^ G165 G166 G170 G171 Lag free threading learning OFF Axis transformation; orientation designation of work piece fixed coordinates Axis transformation; orientation designation of active coordinates Real-time cutter radius compensation OFF Real-time cutter radius comp ON to the left of path Real-time cutter radius comp ON to right of path ART (Adaptive Regulation Technology) activation ART learning function for velocity factors ART learning function deactivation ART learning function for acceleration factors ART learning function for acceleration changing Modal Modal Modal Modal Modal Modal Modal Modal Modal Modal Modal Modal Command filter OFF Command filter ON Modal Digital measuring signals; block transfer, hard stop Modal Digital measuring signals; block transfer, without hard Modal stop G172 Digital measuring signals; block transfer, soft stop Modal G180 ^ 5-axes transformation OFF Modal G181 ^ 5-axes transformation ON, no rotated coord. sys. Modal G182 ^ 5-axes transformation ON with rotated coord. sys. Modal G183 * 5-axes transformation; define coordinate system Modal G184 * 5-axes transformation; program tool dimensions Modal G186 Acceleration on corners, accuracy of arc interpolation Blockwise G188 * Enable positioning axis motion Blockwise G190 G191 G192 G193 G200 G201 G202 G203 Diameter programming OFF Diameter programming and display ON Diameter display ON Diameter display in actual dimension Corner smoothing OFF Corner smoothing ON with defined radius Corner smoothing ON with defined corner radius Corner smoothing ON with defined radius up to tolerance Modal Modal Modal Modal Modal Modal Modal Modal G210 to Laser power control for 2 nd output channel (like Modal G217 G110-G117) G220 ^ G221 ^ G222 ^ G223 ^ G224 ^ G225 ^ Angled wheel transformation OFF Angled wheel transformation ON - normal Angled wheel transformation ON two-step with angled wheel axis moving first then other axes Angled wheel transformation ON two-step with angled wheel axis moving last after other axes Same as G222 but axes move in machine coord. Same as G223 but axes move in machine coord. Modal Modal Modal Modal Modal Modal G265 Distance regulation axis selection Modal G270 G271 G272 G274 G275 G276 G310 to G317 Turning Cycles Turning finishing cycle Stock removal in turning Stock removal in facing Peck finishing cycle Outer diameter / inner diameter turning cycle Multiple pass threading cycle Laser power control for 3rd output channel (like G110-G117) Modal Modal Modal Modal Modal Modal Modal page 20/352

21 * Axis information is programmable in the same block ^ No axis information is allowed in the same block Table 1-1: G-Codes The currently active G-codes are displayed in the G-codes window of the Information page by entering ALT I: INFO. The above list contains optional G-codes that are only available in application specific versions of the CNC. With typical default settings, then at CONTROL RESET the correspondingly marked G-codes in Table 1-1 are active. For another possible default setting see the G-codes window by entering ALT I: INFO after selection of CONTROL RESET or reference the documentation with control (with any changes to the control defaults). M-Command Meaning M00 * Unconditional Stop M01 (*) M02 (*) Conditional Stop End of Program M03 * M04 * M05 * M19 * Spindle orientation M20 * M21 * M22 * M25 * M30 (*) End of program M40 * M41 * M42 * M43 * M44 * M45 * M46 * M70 * M71 * M72 * M73 * Spindle clockwise Spindle counterclockwise Spindle Stop Oscillation ON, Punching/Nibbling ON Oscillation OFF Nibbling ON Punching with/without dwell time ON Automatic gear selection Spindle gear transmission step 1 Spindle gear transmission step 2 Spindle gear transmission step 3 Spindle gear transmission step 4 Spindle gear transmission step 5 Spindle gear transmission step 6 Spline, beginning and end curve 0 Spline, beginning tangential, end curve 0 Spline, beginning curve 0, end tangential Spline, beginning and end tangential M80 * Delete rest of distance using probe function M81 * Drive on application block (resynchronize axis positions via PLC signal during the block) M M108 M109 M M118 M M128 M140 * M141 * M150 * M151 * to M158 * Reset Bit 1... Reset Bit 8 Reset all (8) bits Set Bit 1... Set Bit 8 Pulsate Bit 1... Pulsate Bit 8 Distance regulation ON (configured by G265) Distance regulation OFF Delete rest of distance using probe function, for a probe input (one of 16, M151-M168) Digital input byte 1 bit 1 (to bit 8) is active probe input (for M150) page 21/352

22 M159 * M160 * M161 * to M168 * M170 * M171 * M200 * M201 * to M208 * M209 * M210 * M211 * M213 * M214 * M215 * M280 * M281 * M290 * M291 * PLC cannot define the bit mask for probe PLC can define the bit mask for probe Digital input byte 2 bit 1 (to bit 8) is active probe input (for M150) Continue look ahead (cancel M171) Stop look ahead in probe program Handwheel in automatic mode ON (activated) Axis select for handwheel in auto (axis 1 to 8) Handwheel parameters Suspend handwheel input (offsets still active) Handwheel in automatic mode OFF Spindle 2 on, clockwise Spindle 2 on, counter clockwise Spindle 2 off or stop Switchable spindle/rotary axis rotary axis on (not spindle), first combination Switchable spindle/rotary axis rotary axis on (not spindle), second combination Switchable spindle/rotary axis spindle on (not rotary axis), first combination Switchable spindle/rotary axis spindle on (not rotary axis), second combination Note: * M-Code will be transmitted as BCD to PLC (*) M-Code will only be transmitted to PLC if the function is actually executed M-Code will not be transmitted as BCD to PLC; these are the fast output signals for the laser power control option, handled internally by the CNC. The above list contains some optional M-Codes that are available only in application specific versions of MACHINEMATE. Many of the M-codes in the table above can be assigned a different value with a machine parameter associated with that feature. Table 1-2: M-Codes page 22/352

23 1.4 Auxiliary functions (BCDs) Auxiliary functions are program words that are used to transfer information from the NC program to the PLC program. Up to four of these auxiliary functions can be preset in the CNC. The address letters M, S, U and T are used for auxiliary functions. The corresponding program words are ignored in the NC program and transferred as BCDs to the PLC Program. The meaning of the BCDs is determined by the machine manufacturer and should be explained in the machine documentation. The M-codes that are listed in Table 1-2 however are predefined but can only be used if the relevant function is also available. Only those M-codes listed in Table 1-2 that are marked by an asterisk (*) are transferred to the PLC. Some M-Codes (e.g., M02, M30) are only transferred to the PLC when the corresponding function is actually executed. For example M02 is only transferred to the PLC when it is at the end of a main program and CONTROL RESET is initiated. M02 is not transferred to the PLC when it is positioned at the end of a subroutine because this would cause a jump back to the main program. page 23/352

24 1.5 Programming functional overview Positioning instructions This is a summary of the programming functions. G00 G01 G02/G03 G12/G13 G74 M80 G07 G05/G06 G78/G79 G08/G09 G101/G105 G102/G106 Program execution instructions M00 M01 M02/M30 G10/G11 G72/G73 G08/G09 G186 G75/G76 G04 Technical instructions: Geometric instructions: G94/G95 F word, S word G63/G66 B word M03/M04/M05 M19 G92 G96/G97 G40-G44 G53-G59 G70/G71 G90/G91 G92 G14-G16 Linear interpolation in rapid traverse Linear interpolation in the feed rate Circular interpolation with specified center point Circular interpolation with specified radius Programmable homing Delete remaining paths using probe function Tangential circular interpolation Spline interpolation 2D Tangential setting to the 2D path Look Ahead over more than two blocks Polar transformation Cylinder pattern development transformation Program stop (unconditional) Program stop (conditional) End of program Empty/Fill block buffer Interpolation with precision stop OFF/ON Look Ahead over more than two blocks Corner acceleration, contour accuracy Curvature Programmable dwell Inches/minute or Inches/revolution Feed rate, spindle speed Feed rate or spindle override ON/OFF Programmable acceleration Spindle ON/OFF (clockwise or counter-clockwise) Spindle Orientation Spindle speed limitation S as constant surface speed or rpm Path compensations Part position offsets Programming in imperial/ metric format (inch/mm) Absolute or incremental programming Axis value settings Polar coordinate programming page 24/352

25 G17-G20 G24-G27 G38/G39 G51/G52 G50 Plane selection Programmable work field limits Programmable axis motion mirror Part rotation in degrees/radians Scaling 1.6 Block suppression Placing a slash (block slash code) before a block marks the block as suppressed. The block is ignored if Alt A: AUTOmatic F3: Execute program 2 F1: (/) Block Read over is selected. When F1:(/) Block Read over is not selected, the blocks are processed like ordinary NC blocks. Cycle blocks cannot be suppressed in this manner. Example: N10 G0 X0 Y0 /N20 G1 X2000 Y300 Is not executed when ignore block read over is selected. N30 G1 X4000 Application: The processing of a family of parts is described in an NC program. All machining operations that are required for part version A, but are not to be executed for part version B, can be preceded by a slash (/). After selection of: Alt A: AUTOmatic F3: Program process 2 F1: (/) Block Read over the blocks marked by a slash are not considered. Note: If Alt A: AUTOmatic F3: Program process 2 F1: (/) Block read over is selected after a suppressed block has already been preprocessed and is waiting in the dynamic block buffer, the suppressed block is not ignored, even if this block has not yet been reached in the actual program execution. 1.7 Program Repetition Program repetitions are programmed with an L-code in the last block along with the instructions M30 or M02: Example: N... L5 M30 The program is repeated 5 times. It is executed 6 times in total. The special case of L0 causes the program to be executed infinitely. Repetition calls in the last block of a subroutine are ignored (see 1.8 Subroutines). At the end of a subroutine, the instructions M02 and M30 cause a jump back to the main program from which the subroutine was called. At the end of a main program, the instructions M02 and M30 initiate CONTROL RESET. page 25/352

26 1.8 Subroutines Subroutine calls are programmed by entering Q followed by the program number of an NC program already available in the CNC. The subroutine call causes the first block of the selected subroutine to be processed as next NC block. A subroutine is also called a subprogram because the syntax in a subroutine is identical to that of a main program (except its very first block cannot be a cycle block). When the main program calls a subroutine, it is really just calling another program to run. Program repetition calls in the last block of a subroutine are ignored and have to be programmed, together with L, in the calling program. They are programmed in the same line in which Q was entered, followed by the number of subroutine runs. Example: N... Q100 L5 The program with the number 100 is called as a subroutine and executed 6 times in total. Further subroutines can be called within subroutines. The nesting depth is limited to 4 times. One main program level and four subroutine levels can be programmed altogether. P100 P200 P300 P400 Figure 1-2: Nesting depth Note: A M30 or M02 code cannot be positioned in a block with a subroutine call, since in such blocks subroutine calls are ignored. Also, subroutines must not start with a cycle block! The example above uses a main program and its subroutines that are in CNC memory. The subroutines must be in the same location as the main program. If the main is in CNC memory then subroutines must be there also. The CNC will search for the subroutine program number first in the CNC memory. This is useful for subroutines common to multiple main programs. If the subroutine is not found there and if the main program is in a disk folder then the subroutine file will be checked in that same folder. When the main program is in CNC memory and the subroutine program number is not found (in CNC memory) then error 152 results. When the main program is in a disk folder and the subroutine program number is not found (in either CNC or the disk folder) then error 761 results. page 26/352

27 When the main program is in a disk folder then the file naming for the subprograms is important. The default format for the letter Q is six digits. Therefore the CNC will look for a file having exactly the correct name to match the subprogram call. For example, a program running from the disk having a block N40Q100 will result in the running of a file named P from the same disk folder as the main program. Other commands in the block with the subroutine call will be executed before the subroutine is called. For example with a block like N300 X10 Q500 the X-axis will move as directed and after its move is done then the subroutine 500 will be called. A subroutine call cannot be made from the X and/or Y block that will run a canned drilling cycle (when one of G81 to G89 is modal). The drilling cycle defines an implied subroutine that runs automatically for the axis move with a modal drilling cycle so another subroutine cannot be run as well from the same block. 1.9 Comments in NC programs NC blocks for the CNC can contain comments. These can be included at any position in the NC block. They have no effect on the processing of the NC block. The comment is enclosed in parentheses. Example:... N20 G1 X0 Y0 Z0 (move to zero point)... This comment is included in the NC block and the block display during processing but is otherwise completely ignored by the CNC. There are two forms of comment that can be used to output notes in the state line:... (MSG, text) (*MSG, text)... In the first case, the text between the comma and the closing parenthesis together with the icon (symbol) for notes is displayed in the status line of the CNC during the processing of the NC block. The text is then cleared again when the next block is processed. In the second case the text remains displayed in the status line until it is either explicitly confirmed or the end of the main program is reached. Note that the MSG often accompanies an M0, an operator stop, so the operator sees the message that is the reason for the stop. If there is no M0, sometimes there will be a short dwell in the block with the MSG (like G4F.5) so that the CNC displays the message and does not skip it as it maintains a high block throughput. In cycle blocks, comments of the form... /Text... can also be used. Here all characters between the slash (/) and the block end are treated as a comment. There are no parentheses in cycle blocks (before a comment). page 27/352