MTC200 Description of NC Cycles. Application Manual SYSTEM200 DOK-MTC200-CYC*DES*V22-AW02-EN-P

Transcription

1 X rapid feed feed first feed * n... appr.. * appr.. * 1... end point Z gradient starting point Z end p. X start. p. X Z MTC200 Description of NC Cycles Application Manual SYSTEM200

2 About this Documentation Description of NC Cycles Title Type of Documentation MTC200 Description of NC Cycles Application Manual Document Typecode Internal File Reference Document Number B397-02/EN Purpose of Documentation This documentation describes the individual cycles like drilling point pattern pocket milling and turning. Record of Revisions Description Release Date Notes B397-02/EN Valid from version 22 Copyright 2002 Rexroth Indramat GmbH Copying this document, giving it to others and the use or communication of the contents thereof without express authority, are forbidden. Offenders are liable for the payment of damages. All rights are reserved in the event of the grant of a patent or the registration of a utility model or design (DIN 34-1). Validity The specified data is for product description purposes only and may not be deemed to be guaranteed unless expressly confirmed in the contract. All rights are reserved with respect to the content of this documentation and the availability of the product. Published by Rexroth Indramat GmbH Bgm.-Dr.-Nebel-Str. 2 D Lohr a. Main Telephone +49 (0)93 52/40-0 Tx Fax +49 (0)93 52/ Dept. BRC/ESM3 (AcKr) Dept. BRC/ESM6 (DiHa) Note This document has been printed on chlorine-free bleached paper.

3 Description of NC Cycles Contents I Contents 1 Introduction Basics Availability of NC Cycles NC Cycle Allocation Table Drilling Overview *G81 - Center Drilling *G82 - Peck Drilling (Brk. Chips) *G83 - Peck Drilling (Rem. Chip) *G84 - Floating Tapping *G85 - Rigid Tapping *G86 - Thread Drilling and Milling *G87 - Reaming *G88 - Boring *G89 - Back Boring Point Pattern Overview *G50 - Cycle Selection *G51 - Linear Pattern *G52 - Pattern Matrix *G53 - Complete Circle Pattern, Main Axis *G54 - Partial Circle Pattern, Main Axis *G531 - Complete Circle Pattern, Main Spindle *G541 - Partial Circle Pattern, Main Spindle *G532 - Complete Circle Pattern, Rotary Axis *G542 - Partial Circle Pattern, Rotary Axis Pocket Milling Overview *G61 - Groove (Rough Machining) *G62 - Groove (Finish Machining) *G63 - Circular Groove (Rough Machining) *G64 - Circular Groove (Finish Machining) *G65 - Circular Pocket (Rough Machining) *G66 - Circular Pocket (Finish Machining) *G67 - Rectangular Pocket (Rough Machining)

4 II Contents Description of NC Cycles 4.9.*G68 - Rectangular Pocket (Finish Machining) Turning Overview *G71 - Long Turning *G72 - Face Turning *G73 - Taper Turning Plunge *G75 Groove Plunge, Quad *G751 - Groove Plunge - Circle Threads *G76 - Thread Cutting *G760 Trapezoid Thread *G761 - Taper Thread *G762 - Thread Sequences Appendix - Rexroth Indramat Function Modules NC_AL_ List of Figures Index Service & Support Helpdesk Service-Hotline Internet Vor der Kontaktaufnahme... - Before contacting us Kundenbetreuungsstellen - Sales & Service Facilities

5 Description of NC Cycles Introduction Introduction 1.1 Basics Cycle handling By means of the carefully directed transmission of data to an NC subroutine with the use of NC variables, it becomes possible to parameterize this subroutine, which is then designated an 'NC cycle'. The user can program 'NC cycles' himself. Programming within NC program No. 99 guarantees general availability within an NC program package. To work with cycles, please see the separately available documentation "NC Cycle Handling", DOK-MTC200-CYC*DES*V22-AW0x-EN-P. Note: When upgrading the control version and its relevant Rexroth Indramat NC cycles, the user must note the allocation of variables and the NC cycle call. The appropriate allocation can be found in the related documentation. All NC programs which call up cycles must be checked and adjusted to the new cycle, if necessary. 1.2 Availability of NC Cycles This manual describes the cycles contained in the cycle library. Note: Since variables are already used in the Rexroth Indramat cycles, these are available for further NC programming purposes only on a limited basis. In addition, branch marks cannot be assigned to NC cycles more than once. Doing so would generate the following message if the NC program package or the parameter block were transmitted to the control unit memory: 'Branch mark defined twice' The first symbol for the branch mark in the cycles supplied by Rexroth Indramat is always ' ' (e.g.,. LABEL). For this reason, a user program should not use the branch mark ' ' as its first symbol. Some of the Rexroth Indramat cycles cannot be processed at all levels. Please note the sample programs and the procedures described.

6 1-2 Introduction Description of NC Cycles CAUTION Program interruption if error message appears In the event of an error message, NC cycles are brought to a halt with the NC command 'HLT' or with the 'Q function'. Please note the messages on the diagnostic display and the text notes concerning the NC cycles. Ÿ A renewed start command using 'ADVANCE' can cause the tool to brake and mechanical damage to the machine. Rexroth Indramat cycles always work in the basic programming unit defined in the process parameters. Ÿ They cannot be switched with G70/G71!

7 Description of NC Cycles Introduction NC Cycle Allocation Table NC cycles Variables Auxiliary functions Input Calculation M function CNC File name Drilling , , 4, 5, 19 C01xxxxx.IND.*G81 - Center drilling , 160 C IND.*G82 - Peck drilling (brk. chips) , C IND.*G83 - Peck drilling (rem. chip) , C IND.*G84 - Floating tapping , , 4, 5 103, 104, 105, 203, 204, , 304, 305.*G85 - Rigid tapping , , 4, 5 103, 104, 105, 203, 204, , 304, 305 C IND C IND.*G86 - Thread drilling and milling , C IND.*G87 - Reaming , 160 C IND.*G88 - Boring , , 4, , 104, 119, 203, 204, , 304, 319.*G89 - Back boring , , 4, , 104, 119, 203, 204, , 304, 319 C IND C IND Point pattern , C02xxxxx.IND.*G50 - Cycle selection C IND.*G51 - Linear pattern , , 190, 191, 193, 194 C IND.*G52 - Pattern matrix , , C IND.*G53 - Complete circle pattern, main axis.*g54 - Part circle pattern, main axis.*g531 - Complete circle pattern, main spindle.*g541 - Part circle pattern, main spindle.*g532 - Complete circle pattern, rotary axis.*g542 - Part circle pattern, rotary axis , , C IND , , C IND , , C IND , , C IND , , C IND , , C IND

8 1-4 Introduction Description of NC Cycles NC cycles Variables Auxiliary functions Input Calculation M function CNC File name Pocket Milling , C03xxxxx.IND.*G61 - Groove (rough machining).*g62 - Groove (finish machining).*g63 - Circular groove (rough machining).*g64 - Circular groove (finish machining).*g65 - Circular pocket (rough machining).*g66 - Circular pocket (finish machining).*g67 - Rectangular pocket (rough machining).*g68 - Rectangular pocket (finish machining) , , C IND , C IND , C IND , C IND , C IND , C IND , C IND , C IND Turning , C04xxxxx.IND.*G71 - Long turning , C IND.*G72 - Face turning , C IND.*G73 - Taper turning , C IND.*G75 - Plunge groove, square , C IND.*G751 - Plunge groove, circle , C IND.*G76 - Thread cutting , C IND.*G760 - Trapezoid thread , C IND.*G761 - Taper thread , C IND.*G762 - Thread sequence , C IND

9 Description of NC Cycles Drilling Drilling 2.1 Overview.*G81.*G82.*G83.*G84.*G85.*G86.*G87.*G88.*G89 NC cycle call The following NC cycles are explained in this section: Center drilling Peck drilling (brk. chips) Peck drilling (rem. chips) Floating tapping Rigid tapping Thread drilling and milling Reaming Boring Back boring Standard drilling cycles can be called indirectly using variable (@189), as described in section 3.1 (.*G50 Cycle Selection). A direct call can be made by entering "BSR.*G##" in the NC program.

10 2-2 Drilling Description of NC Cycles 2.2.*G81 - Center Drilling Input variables Calculation variables NC cycle = Chip depth = Safety distance = Dwell a.) direct BSR. G81 b.) approach position safety distance dwell time depth rapid feed feed Uprg0000.FH7 Fig. 2-1: Center drilling Process Fault message In rapid traverse, the tool is positioned vertically to the selected plane, while maintaining the safety distance (@172) from the approach position. The next step is to drill with feed (@174) to depth (@171). The dwell time (@173) is now processed and then the tool is returned in rapid traverse to the load position. [Cycle works only in G17, G18 or G19 plane]

11 Description of NC Cycles Drilling 2-3 Programming example y A B 0 x cut A B: z 0 x -5 Uprg0001.FH7 Fig. 2-2: Programming example center drilling NC block G90 G0 X10 Y10 Z2 BSR. G81 X40 BSR. G81 Y20 BSR. G81 X10 BSR. G81 Comment Positioning X, Y, Z Allocation of variables Cycle call Positioning X Cycle call Positioning Y Cycle call Positioning X Cycle call

12 2-4 Drilling Description of NC Cycles 2.3.*G82 - Peck Drilling (Brk. Chips) Input variables Calculation variables NC cycle = Chip depth = Chip depth = Safety distance = Lifting = Dwell a.) direct BSR. G82 b.) approach position safety distance chip depth retract chip depth retract depth dwell time rapid feed feed Uprg0004.FH7 Fig. 2-3: Peck drilling (brk. chips) Process Fault message In rapid traverse, the tool is positioned vertically to the selected level, while maintaining safety distance (@ 173) from the approach position. The next step is to drill with feed (@176) to chip depth (@172). A peck drilling motion (@174) is performed in rapid traverse after every feed. The final step is to drill with feed (@176) to depth (@171). The dwell time (@175) is now processed and then the tool is returned in rapid traverse to the load position. [Cycle works only in G17, G18 or G19 plane]

13 Description of NC Cycles Drilling 2-5 Programming example y 30 A 20 0 B x 0 cut A B: z x -25 Uprg0005.FH7 Fig. 2-4: Programming example - peck drilling (brk. chips) NC block G90 G0 X25 Y20 Z2 BSR. G82 X50 Y30 BSR. G82 Comment Positioning X, Y, Z Allocation of variables Cycle call Positioning X,Y Cycle call

14 2-6 Drilling Description of NC Cycles 2.4.*G83 - Peck Drilling (Rem. Chip) Input variables Calculation variables NC cycle = Chip depth = Chip depth = Safety distance = Positioning distance = Dwell a.) direct BSR. G83 b.) approach position safety distance chip depth pre-load distance chip depth pre-load-distance depth dwell time rapid feed feed Uprg0002.FH7 Fig. 2-5: Peck drilling (rem. chips) Process Fault message In rapid traverse, the tool is positioned vertically to the selected level, while maintaining safety distance (@ 173) from the approach position. The next step is to drill with feed (@176) to chip depth (@172). After each feed, there is a chip removal action in rapid traverse to the safety distance, followed by a repositioning reduced by the sum of the 'positioning distance' (@174) prior to another drilling motion to the relevant depth. The final step is to drill with feed (@176) to depth (@171). Dwell time (@175) is processed. The tool is then returned to the approach position in rapid traverse. [Cycle works only in G17, G18 or G19 plane]

15 Description of NC Cycles Drilling 2-7 Programming example y A B 0 x cut A B: z 0 x -25 Uprg0003.FH7 Fig. 2-6: Programming example - peck drilling (rem. chips) NC block G90 G0 X10 Y10 Z2 BSR. G83 X40 BSR. G83 Y20 BSR. G83 X10 BSR. G83 Comment Positioning X, Y, Z Allocation of variables Cycle selection Positioning X Cycle selection Positioning Y Cycle call Positioning X Cycle call

16 2-8 Drilling Description of NC Cycles 2.5.*G84 - Floating Tapping Input variables Calculation variables NC cycle call With cycle.*g84, threads can be bored with the main spindle and with positioning, but not with position interpolation. Because the main spindle can only be used as a leading axis, a following error develops between the main spindle and the infeed axis, which is compensated through a mechanical floating head = Chip depth = Safety distance = = Extension a.) direct BSR. G84 b.) pitch approach position safety distance depth backward whirl of spindle rapid feed feed Uprg0008.FH7 Fig. 2-7: Floating tapping Process In rapid traverse, the tool is positioned vertically to the selected plane, while maintaining safety distance (@172) from the approach position. The next step is to drill with feed to depth (@171), and then to reposition to safety distance (@172) in the feed with the main spindle rotating in the opposite direction, taking into account the extension speed factor (@174). Returning to the approach position in rapid traverse ends the cycle. Note: To achieve a high degree of accuracy, in particular in the break-in range of the thread, the interpolation conditions 'G6' and 'G8' should be set before the cycle is called. Error messages [Spindle not switched on] [Cycle works only in G17, G18 or G19 plane]

17 Description of NC Cycles Drilling 2-9 Programming example y A M10 M10-LH 0 B x 0 cut A B: z x -20 Uprg0009.FH7 Fig. 2-8: Programming example - floating tapping NC block T1 BSR.M6 G54 G90 G0 G6 G8 X25 Y20 Z10 S300 BSR. G84 T2 BSR.M6 G54 G90 G0 G6 G8 X50 Y30 Z10 S300 M3 BSR. G84 Comment Tool change Positioning X, Y, Z Allocation of variables Cycle call Tool change Positioning X, Y, Z Cycle call

18 2-10 Drilling Description of NC Cycles 2.6.*G85 - Rigid Tapping Input variables Calculation variables NC cycle call Contrary to cycle.*g84, this.*g85 cycle has interpolation between the main spindle and the feed axis. This means rigid tapping is possible and no mechanical floating head tap-holder is = Chip depth = Safety distance = = Extension @167 a.) direct BSR. G85 b.) pitch approach position safety distance depth backward whirl of spindle rapid feed feed Uprg0010.FH7 Fig. 2-9: Rigid tapping Process In rapid traverse, the tool is positioned vertically to the selected level, while maintaining safety distance (@ 172) from the approach position. The next step is to drill with feed to depth (@171), and then to reposition to safety distance (@172) in the feed with the main spindle rotating in the opposite direction, taking into account the extension speed factor (@174). Returning to the approach position in rapid traverse ends the cycle. Note: To achieve a high degree of accuracy, in particular in the break-in range of the thread, the interpolation conditions 'G6' and 'G8' should be set before the cycle is called. Error messages [Spindle not switched on] [Cycle works only in G17, G18 or G19 plane]

19 Description of NC Cycles Drilling 2-11 Programming example y M10-LH A M10 0 B x 0 cut A B: z x -20 Uprg0011.FH7 Fig. 2-10: Programming example - rigid tapping NC block T2 BSR.M6 G54 G90 G0 G6 G8 X25 Y20 Z10 S300 BSR. G85 T1 BSR.M6 G54 G90 G0 G6 G8 X50 Y30 Z10 S300 M4 BSR. G85 Comment Tool change Positioning X, Y, Z Allocation of variables Cycle call Tool change Positioning X, Y, Z Cycle call

20 2-12 Drilling Description of NC Cycles 2.7.*G86 - Thread Drilling and Milling Input variables Calculation variables NC cycle = Thread = Thread = Safety distance = Clockwise thread (2) - counterclockwise thread = Milling = Core hole depth = Chip depth = Positioning distance = Dwell = Core hole @169 a.) direct BSR. G86 b.) Drilling Tool radius (R) approach position safety distance Milling Righthand thread Gewindesteigung drill hole depth R safety distance chip depth chip depth approach position pre-load distance pre-load distance approach position safety distance thread pitch thread diameter Lefthand thread drill hole depth dwell time drill hole depth thread diameter R rapid feed feed Uprg0047.FH7 Fig. 2-11: Thread drilling and milling Process In rapid traverse, the tool is positioned vertically to the selected level, while maintaining safety distance (@ 172) from the approach position. From this point, drilling by the amount of chip depth (@176) proceeds to the relevant depth with drill hole feed (@179). After each feed, there is a chip removal motion in rapid traverse to the safety distance, followed by a repositioning reduced by the sum of the

21 Description of NC Cycles Drilling 2-13 'positioning distance' prior to another drilling action to the set depth. The last step is to drill with feed to drill hole depth Dwell time is processed and then the tool is repositioned in rapid traverse to safety distance This is followed by positioning for the milling procedure with distance 2.1 thread pitch before the drill hole depth, in rapid traverse. Then the thread contour, which depends on for a clockwise thread (2) or for a counterclockwise thread (3), taking the radius of the tool into account as well as soft approaches and retractions, is processed on the thread diameter (@170) with the help of a helical curve in milling feed (@174). Returning to the approach position in rapid traverse ends the cycle. Error messages Programming example [Error in variable 173] [Cycle works only in G17, G18 or G19 plane] y M6 A M6-LH 0 B x 0 z cut A B: x -20 Uprg0048.FH7 Fig. 2-12: Programming example thread drilling and milling NC block Comment T1 BSR.M6 G90 G0 X50 Y30 Z10 S3000 M3 Positioning X, Allocation of variables @179=200 BSR. G86 Cycle call X25 Y20 Positioning X, BSR. G86 Cycle call

22 2-14 Drilling Description of NC Cycles 2.8.*G87 - Reaming Input variables Calculation variables NC cycle = Chip depth = Safety distance = Dwell = Plunge = a.) direct BSR. G87 b.) approach position safety distance depth dwell time rapid feed feed Uprg0006.FH7 Fig. 2-13: Reaming Process In rapid traverse, the tool is positioned vertically to the selected level, while maintaining safety distance (@ 172) from the approach position. The next step is plunge feed (@174) to depth (@171). Dwell time (@173) is now processed. The tool is then returned to safety distance (@172) in retract feed (@175). Returning to the approach position in rapid traverse ends the cycle. Fault message [Cycle works only in G17, G18 or G19 plane]

23 Description of NC Cycles Drilling 2-15 Programming example y H7 10H7 0 x z 0 x -20 Uprg0007.FH7 Fig. 2-14: Programming example reaming NC block Comment G90 G0 X25 Y20 Z2 S800 M3 Positioning X, Allocation @175=150 BSR. G87 Cycle call X50 Y30 Positioning X, Y BSR. G87 Cycle call

24 2-16 Drilling Description of NC Cycles 2.9.*G88 - Boring Input variables Calculation variables NC cycle = Chip depth = Safety distance = Lift first main axis = = @163, a.) direct BSR. G88 b.) approach spindle in safety distance disengage first main axis Fig. 2-15: Boring depth oriented spindle stop rapid feed feed Uprg0012.FH7 Process Error messages In rapid traverse, the tool is positioned vertically to the selected level, while maintaining safety distance (@ 172) from the approach position. The next step is to bore to depth (@171) using feed (@174) and processing dwell time (@175). The main spindle is stopped and oriented at 0 degrees. In rapid traverse, the cutter is then retracted by the amount 'lift first main axis' (@173) and then returned to the approach position. The start position in the plane is then approached and the main spindle is switched back on. [Spindle not switched on] [Cycle works only in G17, G18 or G19 plane]

25 Description of NC Cycles Drilling 2-17 Programming example y 48,5H x 0 0 z 50 x -25 Uprg0013.FH7 Fig. 2-16: Programming example boring NC block Comment G90 G0 X50 Y40 Z10 S900 M3 Positioning X, Allocation @175=0.4 BSR. G88 Cycle call

26 2-18 Drilling Description of NC Cycles 2.10.*G89 - Back Boring Input variables Calculation variables NC cycle = Chip depth = Safety distance = Lift first main axis = Lift third main axis = = @167 a.) direct BSR. G89 b.) approach oriented spindle stop spindle in disengage third main axis safety distance Fig. 2-17: Back boring disengage first main axis depth oriented spindle stop spindle in rapid feed feed Uprg0014.FH7 Process Error messages First, the main spindle is stopped, oriented at 0 degrees, at the approach position and then retracted from the center of the bore by the amount equal to 'lift first main axis' (@173). Then, in rapid traverse, it is vertically positioned with respect to the selected plane at safety distance (@172). This is followed by positioning in the center of the bore and starting of the main spindle. The next step is to bore to depth (@171) using feed (@175) and processing dwell time (@176). Again, the main spindle is stopped at 0 degrees. The cutter is then cleared in rapid traverse with an amount equal to 'lift first main axis' (@173) and 'lift third main axis' (@174). This is followed by a return to the approach position in the third main axis. The start position on the plane is assumed and the main spindle is switched back on. [Spindle not switched on] [Cycle works only in G17, G18 or G19 plane]

27 Description of NC Cycles Drilling 2-19 Programming example y A 40 B 0 x 0 cut A B: z 50 Ø30 0 x Ø36 Uprg0015.FH7 Fig. 2-18: Programming example back boring NC block G90 G0 X50 Y40 Z20 BSR. G89 Comment Positioning X, Y, Z Allocation of variables Cycle call

28 2-20 Drilling Description of NC Cycles

29 Description of NC Cycles Point Pattern Point Pattern 3.1 Overview.*G50.*G51.*G52.*G53.*G54.*G531.*G541.*G532.*G542 The following NC cycles are explained in this section: Cycle selection Linear pattern Pattern matrix Complete circle pattern, main axis Partial circle pattern, main axis Complete circle pattern, main spindle Partial circle pattern, main spindle Complete circle pattern, rotary axis Partial circle pattern, rotary axis Then the executed NC cycles are described and the practical use in the MTC200 is presented using a programming example.

30 3-2 Point Pattern Description of NC Cycles 3.2.*G50 - Cycle Selection Input variables Calculation variables NC cycle = NC cycle BSR. Cycle 81 Center drilling 82 Peck drilling (brk. chips) 83 Peck drilling (rem. chips) 84 Floating tapping 85 Rigid tapping 86 Thread drilling and milling 87 Reaming 88 Boring 89 Back boring Process When is entered for NC cycle '. G50', the desired cycle is called indirectly using the value of Cycle '. G50' functions as a branch distributor for point patterns, e.g. pitch circle, pattern matrix, etc. Note: The machine manufacturer must adapt this cycle to the cycle selected for transmission. Fault message [Check variable 189]

31 Description of NC Cycles Point Pattern 3-3 Programming example A B cut A B: 1x Uprg0017.FH7 Fig. 3-1: Cycle selection NC block Comment T1 BSR.M6 Tool change T1 G50 X-345 Y250 Z-16.5 Tool origin G90 G0 X10 Y10 Z1 S2000 M3 Positioning X, @172=1 variables BSR.Pos Cycle call T2 BSR.M6 Tool change T2 G90 G0 X10 Y10 Z1 S4500 M3 Positioning X, @176=450 variables BSR.Pos Cycle call T1 BSR.M6 Tool change T0 RET.Pos X10 Y10 BSR. G50 Drilling position 1 X30 Y-10 BSR. G50 Drilling position 2 X50 Y10 BSR. G50 Drilling position 3 X70 Y-20 BSR. G50 Drilling position 4 X80 Y20 BSR. G50 Drilling position 5 X90 Y0 BSR. G50 Drilling position 6 RTS

32 3-4 Point Pattern Description of NC Cycles 3.3.*G51 - Linear Pattern Input variables Calculation variables NC cycle = NC cycle = Start position of first main axis = Start position of second main axis = Angle = = Number @194 BSR. G51 starting position of second main axis distance distance distance distance angle starting position of first main axis rapid feed Uprg0018.FH7 Fig. 3-2: Linear pattern Process The cycle selected via is first processed at start position The subsequent position is then calculated with the help of variables 'angle' (@182), in terms of the positive direction of the first main axis, and 'distance' (@183). This position is then approached in rapid feed. Once at this position, the selected cycle is called up again. This is repeated the number of times set in Fault message [Cycle works only in G17, G18 or G19 plane]

33 Description of NC Cycles Point Pattern 3-5 Programming example A 0 B cut A B: 0-2,5 Uprg0019.FH7 Fig. 3-3: Programming example linear pattern NC block Comment G90 G0 X50 Y40 Z20 S2500 M3 Approach NC cycle Allocation of variables @181=-30 Allocation of variables BSR. G51 Cycle call

34 3-6 Point Pattern Description of NC Cycles 3.4.*G52 - Pattern Matrix Input variables Calculation variables NC cycle = NC cycle = Start position of first main axis = Start position of second main axis = Distance, horizontal = Distance, vertical = Number of = Number of = Line distance = @193, BSR. G52 line of the angle starting position of second main axis distance line distance line horizontal distance vertical distance starting position of first main axis rapid feed Uprg0020.FH7 Fig. 3-4: Pattern matrix Process The cycle selected via is first processed at start position The subsequent position is then calculated with the use of variables 'distance, horizontal' (@182) and 'distance, vertical' (@183) and then approached in rapid traverse. Once at this position, the selected cycle is called again. This is repeated until all the points of a line (@184) are processed. The further positions of the next line are defined by the variables 'line angle' (@187), in terms of the direction of the second main axis, and 'line distance' (@186). Variable (@185) defines the number of lines that are processed. Fault message [Cycle works only in G17, G18 or G19 plane]

35 Description of NC Cycles Point Pattern 3-7 Programming example A 0 B ,5 0 cut A B: Uprg0021.FH7 Fig. 3-5: Programming example pattern matrix NC block Comment G90 G0 X50 Y40 Z20 S2500 M3 Positioning X, Y, NC cycle Allocation of variables Allocation of variables BSR. G52 Cycle call

36 3-8 Point Pattern Description of NC Cycles 3.5.*G53 - Complete Circle Pattern, Main Axis Input variables Calculation variables NC cycle = NC cycle = Center point of first main axis = Center point of second main axis = = Start = Number BSR. G53 center point of second main starting angle radius center point of first main axis rapid feed Uprg0022.FH7 Fig. 3-6: Complete circle pattern, main axis Process The complete circle pattern defined by variables 'Center point of first main axis ' (@180), 'Center point of second main axis ' (@181) and 'Radius' is divided into equal angular increments by the number of points (@184). The first position is approached in rapid traverse in terms of the 0 degree position of the main spindle while taking the start angle (@183) into account. This is followed by processing by the cycle selected with variable (@189). The main spindle is now staggered in terms of the calculated angular increment and positioned in rapid traverse; the cycle set with variable (@189) is called until the number of points (@184) has been processed. Fault message [Cycle works only in G17, G18 or G19 plane]

37 Description of NC Cycles Point Pattern 3-9 Programming example R50 30 A B 0 60 cut A B: Ø Ø25 Uprg0023.FH7 Fig. 3-7: Programming example, complete circle pattern, main axis NC block Comment G90 G0 X50 Y40 Z20 S500 M3 Positioning X, Y, Drilling cycle Allocation of variables Allocation of variables BSR. G53 Cycle call

38 3-10 Point Pattern Description of NC Cycles 3.6.*G54 - Partial Circle Pattern, Main Axis Input variables Calculation variables NC cycle = NC cycle = Center point of first main axis = Center point of second main axis = = Start = End = Number BSR. G54 end angle center point second main axis radius starting angle center point first main axis rapid feed Uprg0024.FH7 Fig. 3-8: Partial circle pattern, main axis Process The partial circle pattern defined by the variables 'Center point of first main axis' (@180), 'Center point of second main axis' (@181), 'Radius' (@182), 'Start angle' (@183) and 'End angle' (@184), as relates to the positive direction of the first main axis in the selected plane, is divided by the number of points (@185) in equal angular increments. The first position is approached in rapid traverse and then processed in the cycle set in variable (@189). The main spindle is now staggered in terms of the calculated angular increment and positioned in rapid traverse; the cycle set with variable (@189) is called until the number of points (@185) has been processed. Fault message [Cycle works only in G17, G18 or G19 plane]

39 Description of NC Cycles Point Pattern 3-11 Programming example R50 30 A B 0 60 cut A B: Ø Ø25 Uprg0025.FH7 Fig. 3-9: Programming example, partial circle pattern, main axis NC block Comment G90 G0 X50 Y40 Z20 S500 M3 Positioning X, Y, Drilling cycle Allocation of variables Allocation of variables @185=5 BSR. G54 Cycle call

40 3-12 Point Pattern Description of NC Cycles 3.7.*G531 - Complete Circle Pattern, Main Spindle Input variables Calculation variables NC cycle = NC cycle = = Start angle = Number of = BSR. G531 radius R starting angle X rapid feed Uprg0045.FH7 Fig. 3-10: Complete circle pattern, main spindle Process The complete circle pattern defined in terms of the variable 'Radius' (@182) is divided into equal angular increments by the number of points (@184). The first position is approached in rapid traverse in terms of the 0 degree position of the main spindle while taking the start angle (@183) into account. This is followed by processing by the cycle selected with variable (@189). The main spindle is now staggered in terms of the calculated angular increment and positioned in rapid traverse; the cycle set with variable (@189) is called until the number of points (@184) has been processed. Note: Using the spindle is defined in which the workpiece has been loaded. The value for the first spindle can be either 0 or 1, 2 for the second and 3 for the third. Note the PLC user program with respect to the acknowledgement of auxiliary functions for spindle orientation! Fault message [Check variable 185!]

41 Description of NC Cycles Point Pattern 3-13 Programming example ø 150 ø 100 ø 70 ø 50 Fig. 3-11: Programming example, complete circle pattern, main spindle NC block Comment G90 G0 X0 S2 500 M3 Positioning Drilling cycle number 25 Allocation of variables @182=50 Variables for @185=0 BSR. G531 Cycle call Uprg0042.FH7

42 3-14 Point Pattern Description of NC Cycles 3.8.*G541 - Partial Circle Pattern, Main Spindle Input = NC cycle = = Start angle = End angle = Number of = Workpiece spindle NC cycle call BSR. G541 end angle radius R starting angle X Fig. 3-12: Partial circle pattern, main spindle rapid feed Uprg0046.FH7 Process The partial circle pattern defined in terms of the variables 'Radius' (@182), 'Start angle' (@183) and 'End angle' (@184), as they relate to the 0 degree position of the main spindle, is divided by the number of points. The first position is approached in rapid traverse taking the start angle (@183) into account, and then processed in the cycle set in variable (@189). The main spindle is now staggered in terms of the calculated angular increment and positioned in rapid traverse; the cycle set with variable (@189) is called until the number of points (@185) has been processed. Note: Using the spindle is defined in which the workpiece has been loaded. The value for the first spindle can be either 0 or 1, 2 for the second and 3 for the third. Note the PLC user program with respect to the acknowledgement of auxiliary functions for spindle orientation! Fault message [Check variable 186!]

43 Description of NC Cycles Point Pattern 3-15 Programming example ø 150 ø 100 ø 70 ø 50 Uprg0043.FH7 Fig. 3-13: Programming example, partial circle pattern, main spindle NC block Comment G90 G0 X0 S2 500 M3 Positioning Drilling cycle number 25 Allocation of variables Variables for @186=2 BSR. G541 Cycle call

44 3-16 Point Pattern Description of NC Cycles 3.9.*G532 - Complete Circle Pattern, Rotary Axis Input variables Calculation variables NC cycle = NC cycle = = Start angle = Number of = No. of rotary axis (A = 1; B = 2; C @193 BSR. G532 radius R starting angle X rapid feed Uprg0051.FH7 Fig. 3-14: Complete circle pattern, rotary axis Process The complete circle pattern defined in terms of the variable 'Radius' (@182) is divided into equal angular increments by the number of points (@184). The first position is approached in rapid traverse in terms of the 0 degree position, defined by variable (@185), of the rotary axis while taking the start angle (@183) into account. This is followed by processing with the cycle selected with The rotary axis is now staggered in terms of the calculated angular increments and positioned in rapid traverse. The cycle set with is called until the number of points (@184) has been processed. Fault message [@185 No. of rotary axis not 1, 2 or 3]

45 Description of NC Cycles Point Pattern 3-17 Programming example ø 150 ø 100 ø 70 ø 50 Uprg0052.FH7 Fig. 3-15: Programming example, complete circle pattern, rotary axis NC block Comment G90 G0 X200 Z10 S2 500 M3 Positioning Drilling cycle number 25 Allocation of variables @182=50 Variables for @185=3 BSR. G532 Cycle call

46 3-18 Point Pattern Description of NC Cycles 3.10.*G542 - Partial Circle Pattern, Rotary Axis Input variables Calculation variables NC cycle = NC cycle = = Start angle = End angle = Number of = No. of rotary axis (A = 1; B = 2; C BSR. G542 end angle radius R starting angle X rapid feed Uprg0049.FH7 Fig. 3-16: Partial circle pattern, rotary axis Process Fault message The partial circle pattern defined by the variables 'Radius' (@182), 'Start angle' (@183) and 'End angle' (@184), as relates to the 0 degree position, defined by variable (@186) of the rotary axis, is divided by the number of points (@185) into equal angular increments. The first position is approached in rapid traverse taking the start angle (@183) into account, and then processed in the cycle set in variable (@189). This is followed by processing with the cycle selected with The rotary axis is now staggered in terms of the calculated angular increments and positioned in rapid traverse. The cycle set with is called until the number of points (@185) has been processed. [@186 No. of rotary axis not 1, 2 or 3]

47 Description of NC Cycles Point Pattern 3-19 Programming example ø 70 ø 50 ø 100 ø 150 Uprg0050.FH7 Fig. 3-17: Programming example, partial circle pattern, rotary axis NC block Comment G90 G0 X200 Z10 S2 500 M3 Positioning Drilling cycle number 25 Allocation of variables Variables for @186=3 BSR. G542 Cycle call

48 3-20 Point Pattern Description of NC Cycles

49 Description of NC Cycles Pocket Milling Pocket Milling 4.1 Overview.*G61.*G62.*G63.*G64.*G65.*G66.*G67.*G68 The following NC cycles are explained in this section: Groove (rough machining) Groove (finish machining) Circular groove (rough machining) Circular groove (finish machining) Circular pocket (rough machining) Circular pocket (finish machining) Rectangular pocket (rough machining) Rectangular pocket (finish machining)

50 4-2 Pocket Milling Description of NC Cycles 4.2.*G61 - Groove (Rough Machining) Input variables Comment Calculation variables NC cycle = Length = Depth = Chip depth = Safety distance = Angle = Feed of = Feed of feed Width of groove = @163, BSR. G61 approach position safety distance depth of position Z Y depth Z length angle rapid feed X feed Uprg0026.FH7 Fig. 4-1: Groove (rough machining) Process The tool is placed in rapid traverse at the approach position, maintaining safety distance (@174), and vertical to the selected plane. The subsequent feed proceeds with 'Feed of infeed' (@177) to the depth of the cut (@173). The tool then moves linearly with 'Feed of plane' (@176) and length (@171), in terms of the angle (@175), as relates to the positive first main axis. Feed and processing in the plane continue until depth (@172) is reached. The final milling procedure is less than the full chip depth if the distance from the safety distance to the depth is not equal to a multiple integer of the chip depth. Positioning in rapid traverse to the safety distance, followed by movement to the approach position on the plane, then vertically to the plane in the approach position concludes the cycle. Fault message [Cycle works only in G17, G18 or G19 plane]

51 Description of NC Cycles Pocket Milling 4-3 Programming example y A B 0 x 0 25 cut A B: z 0 x -10 Uprg0027.FH7 Fig. 4-2: Programming example - groove (rough machining) NC block G90 G0 X25 Y20 Z10 @175=30 BSR. G61 Comment Start position Allocation of variables for groove (rough) cycle Cycle call

52 4-4 Pocket Milling Description of NC Cycles 4.3.*G62 - Groove (Finish Machining) Input variables Calculation variables NC cycle = Length = Width = Depth = Safety distance = Angle = 2 (CW) or 3 = Feed of = Feed BSR. G62 approach position withdraw position safety distance R R width Z depth Z angle length Y rapid feed X feed Uprg0028.FH7 Fig. 4-3: Groove (finish machining) Process Error messages The tool is placed in rapid traverse at the approach position, maintaining safety distance (@173), and vertical to the selected plane. This is followed by cutting to depth (@172) with 'Feed of infeed/circle' (@177). The contour of the groove is now cut. Depending on variable (@175), it is cut clockwise (2) or counterclockwise (3). It takes into account the radius of the tool, soft approaches and retractions respective the angle (@174). It relates to the positive direction of the first main axis, the length (@170) and the width (@171) with 'Feed of plane' (@176) for straight lines or 'Feed of infeed/circle' (@177) for circles. This is concluded by returning to the approach position in rapid traverse. [Check tool radius!] [Variable Check width of groove!] [Error in variable 175!] [Cycle works only in G17, G18 or G19 plane]

53 Description of NC Cycles Pocket Milling 4-5 Programming example y 10H7 20 A B 0 x 0 25 cut A B: z 0 x Uprg0029.FH7 Fig. 4-4: Programming example - groove (finish machining) NC block G90 G0 X25 Y20 Z10 BSR. G62 Comment Start position Allocation of variables for groove (finish) cycle Cycle call

54 4-6 Pocket Milling Description of NC Cycles 4.4.*G63 - Circular Groove (Rough Machining) Input variables Comment Calculation variables NC cycle = = Start angle = Segment angle = Depth = Chip depth = Safety distance = Feed of = Feed of infeed Width of groove = BSR. G63 approach position safety distance depth of cut Z depth Z radius segment angle start angle Y rapid feed X feed Uprg0030.FH7 Fig. 4-5: Circular groove (rough machining) Process The tool is placed in rapid traverse at the approach position, maintaining safety distance (@175), and vertical to the selected plane. The subsequent feed proceeds with 'Feed of infeed' (@177) to the depth of the cut (@174). With 'Feed of plane' (@176), the tool now moves circularly around the segment angle (@172) with the radius (@170). Both feed and processing in the plane take place until depth (@173) is attained. The final milling procedure is less than the full chip depth if the distance from the safety distance to the depth is not equal to a multiple integer of the chip depth. Positioning in rapid traverse to the safety distance, followed by movement to the approach position in the plane and then vertically to the plane in the approach position, end the cycle. Fault message [Cycle works only in G17, G18 or G19 plane]

55 Description of NC Cycles Pocket Milling 4-7 Programming example y A B x cut A B: z 0-20 x Uprg0031.FH7 Fig. 4-6: Programming example circular groove (rough machining) NC block G90 G0 X50 Y40 Z10 BSR. G63 Comment Start position Allocation of variables for circular groove (rough machining) cycle Cycle call

56 4-8 Pocket Milling Description of NC Cycles 4.5.*G64 - Circular Groove (Finish Machining) Input variables Calculation variables NC cycle = Groove = Width = Start angle = Segment angle = Depth = Safety distance = = 2 (CW) or BSR. G64 approach position safety distance Z width step angle radius depth starting angle Y X rapid feed feed Uprg0032.FH7 Fig. 4-7: Circular groove (finish machining) Process Error messages The tool is placed in rapid traverse at the approach position, maintaining safety distance (@175), and vertical to the selected plane. This is followed by insertion to depth (@174) with half feed (@176/2). The contour of the circular groove is now cut to the width of groove (@171). Depending on it is performed either in a clockwise (2) or counterclockwise direction (3). It takes the radius of the tool into account with soft approaches and retractions. This is concluded by returning to the approach position in rapid traverse. [Check tool radius!] [Variable Check width of groove!] [Variable Check groove radius!] [Variable Check segment angle!] [Error in variable 177!] [Cycle works only in G17, G18 or G19 plane]

57 Description of NC Cycles Pocket Milling 4-9 Programming example y A B x cut A B: z 0 x -20 Uprg0033.FH7 Fig. 4-8: Programming example circular groove (finish machining) NC block G90 G0 X140 Y75 Z10 BSR. G64 Comment Start position Allocation of variables for circular groove (finish machining) cycle Cycle call

58 4-10 Pocket Milling Description of NC Cycles 4.6.*G65 - Circular Pocket (Rough Machining) Input variables Calculation variables NC cycle = = Depth = Chip depth = Safety distance = % of tool = 2 (CW) or 3 = Feed of = Feed BSR. G65 approach position safety distance depth of cut Z depth Z Y X R diameter R rapid feed feed Uprg0034.FH7 Fig. 4-9: Circular pocket (rough machining) Process Error messages The tool is placed in rapid traverse at the approach position, maintaining safety distance (@174), and vertical to the selected plane. The subsequent feed proceeds with 'Feed of infeed' (@177) to the depth of the cut (@173). The contouring of the circular pocket then begins. Depending on contouring is performed either in a clockwise (2) or counterclockwise (3) direction. It takes the tool radius R and its wear (@175) in terms of the circular pocket diameter (@171) into account. Both feed in Z and processing in the plane continue until depth (@172) is achieved. The final milling procedure is less than the full chip depth if the distance from the safety distance to the depth is not equal to a multiple integer of the chip depth. Moving to the approach position in rapid traverse ends the cycle. [Check tool radius <= 0] [Tool radius >= circular pocket radius] [Cycle works only in G17, G18 or G19 plane]

59 Description of NC Cycles Pocket Milling 4-11 Programming example z y ø x Fig. 4-10: Programming example circular pocket (rough machining) NC block Comment G90 G0 X75 Y50 Z10 S3000 M3 @173=15 Allocation of variables circular (rough @178=200 BSR. G65 Cycle call Uprg0035.FH7

60 4-12 Pocket Milling Description of NC Cycles 4.7.*G66 - Circular Pocket (Finish Machining) Input variables Calculation variables NC cycle = Diameter of circular = Depth = Safety distance = 2 (CW) or 3 BSR. G66 approach position safety distance Z depth R R diameter Y rapid feed X feed Uprg0036.FH7 Fig. 4-11: Circular pocket (finish machining) Process Error messages The tool is placed in rapid traverse at the approach position, maintaining safety distance (@173), and vertical to the selected plane. This is followed by insertion to depth (@172) with half feed (@175/2). Then the circular pocket is contoured to its diameter (@171). Depending on this is performed either in a clockwise (2) or counterclockwise (3) direction. It takes the tool radius R into account as well as soft approaches and retractions. Movement to the approach position then occurs. [Tool radius <= 0] [Tool radius >= circular pocket radius] [Check variable 174] [Cycle works only in G17, G18 or G19 plane]