Download to read offline
More Related Content
CNC Programming.pptx
- 1.
- 2.
- 3. Part Programming CNC partprogramming involves a series of alpha-numeric coded instructions that are required to produce a part. The program controls the machine tool movements and controls auxiliary functions auxiliary functions including spindle, coolant, and rotation.
- 4. G - CODE G-Codesare about Geometry control functions controls the movements of a machine, dictating how and where a machine should move to produce a part M - CODE M-Codes are about Machine control functions
- 5. G Codes G00 -Rapid move (not cutting) G01 - Linear move G02 - Clockwise circular motion G03 – Counter clockwise circular motion G20 - inch data specification G21 - metric data specification G28 - return to reference point G98 - feed per minute
- 6. M Codes M00 –Program stop M01 – Optional program stop M03 – Spindle rotation on clockwise M04 – Spindle rotation on counter clockwise M05 – Spindle off M06 – Tool change M08 – Coolant on M09 – Coolant off M30 – Program end, Return to start point
- 7. Start of theProgram [BILLET X80 Z65 - Defines Dimensions of raw material – Diameter 80mm & Length 65 mm G21 G98 - Input dimensions are in mm G28 U0 W0 - Tool Home position M06 T01 - Tool change & Tool number 01 M03 S1500 - Spindle rotates CW & Speed 1500 rpm
- 8. End of theProgram G28 U0 W0 - Tool back to the Home position M05 - Spindle off M30 - Program end rewind
- 9.
- 10. [BILLET X22 Z65 N10G21 G98 N20 G28 U0 W0 N30 M06 T01 - T01 LH Turning tool N40 M03 S1500 N50 G00 X23 Z2 - Initial Position N60 G01 X20 F50 - Depth 2mm N70 G01 Z-45 - Longitudinal Feed 45mm N80 GO1 X23 - Tool Retract N90 G01 Z0 - Back to Initial Point
- 11. N100 G01 X18 N110G01 Z-30 N120 G01 X19 N130 G01 Z0 N140 G01 X16 N150 G01 Z-30 N160 G01 X17 N170 G01 Z0 N180 G01 X15 N190 G01 Z-30 N200 G01 X16 N210 G01 Z0 N220 G01 X13 N230 G01 Z-15 N240 G01 X14 N250 G01 Z0 N260 G01 X11 N270 G01 Z-15 N280 G01 X12 N290 G01 Z0 N300 G01 X10 N310 G01 Z-15 N320 GO1 X11 N330 GO1 Z5 N340 G28 U0 W0 N350 M05 N360 M30
- 12. G90 – TurningCycle G90 X... Z... X – Diameter to be cut. Z – End point in z-axis.
- 13. N60 G90 X21Z-45 F30 N70 X20 N 80 X18 Z-30 N90 X16 N100 X15 N110 X13 Z-15 N120 X11 N130 X10 N140 G28 U0 W0 N150 M05 N160 M30 https://youtu.be/Uom3kaqQ0Lo [BILLET X22 Z65 N10 G21 G98 N20 G28 U0 W0 N30 M06 T01 N40 M03 S1500 N50 G00 X23 Z2 Program 2
- 14. G71 - RoughingCycle G71 U R G71 P Q U W F FIRST LINE U = Depth of cut R = Retract value SECOND LINE P = Sequence number for the start of the program contour Q = Sequence number for the end of the program contour U = Finishing allowance in X W = Finishing allowance in Z F = Feed rate
- 15. G70 - FinishingCycle G70 P Q; •P = start of the contour •Q = end of the contour
- 16.
- 17. [BILLET X22 Z60; N10G21 G98; N20 G28 U0 W0; N30 M06 T01; N40 M03 S1500; N50 G00 X22 Z2; N60 G01 X0 N70 G71 U0.5 R1 N80 G71 P90 Q150 U0.1 W0.1 F50 N90 G01 Z0 N100 G03 X10 Z-5 R5 N110 G01 Z-17 N120 G01 X14 Z-25 N130 G01 Z-30 N140 G02 X19 Z-35 R5 N150 G01 Z-37 N160 G70 P90 Q150 F20 N170 G28 U0 W0 N180 M05 N190 M30
- 18. G75 – GROOVINGCYCLE G75 R(1) G75 X Z P Q F G75 – Groove Cycle R(1) – relief amount X – Groove Diameter Z - Last position in Z-axis P – Incremental depth of cut in X-axis Q – Incremental depth of cut in Z-axis F – feed rate
- 19.
- 20. N50 G00 X82 N55G00 Z-20; N60 G75 R1 N70 G75 X50 Z-31 P2000 Q3000 F50 N80 G00 X82 N90 G28 U0 W0 N100 M05 N110 M30 [BILLET X80 Z65; N10 G21 G98; N20 G28 U0 W0; N30 M06 T01; N40 M03 S1500;
- 21. G76 – THREADCUTTING CYCLE G76 P(1)(2)(3), Q, R G76 X, Z, P, Q, F First line •P(1) = No. of Finishing Passes •P(2) = Chamfer •P(3) = Angle of thread •Q = Minimum cut •R = Finish allowance Second Line X = Minor (core) dia of thread Z = Endpoint of thread P = Depth of thread Q = Depth of first cut F = Pitch of thread
- 22. Major Diameter (D)= 40 mm Pitch = 1.5 mm Thread angle = 60⁰ Thread Height = 0.6134*pitch Minor Diameter (d) = D – (2*Thread Height)
- 23. N70 G75 R1 N80G75 X20 Z-46 P2000 Q3000 F50 N90 G00 X42 N100 G28 U0 W0 N110 M06 T02 N120 G00 X42 N130 G00 Z0 N140 G76 P020060 Q100 R0.1 N150 G76 X38.05 Z-25 P920 Q200 F20 N160 G00 X42 N170 G00 Z5 N180 G280 U0 W0 N190 M05 N200 M30 ⌀40 ⌀20 M40*1.5 25 25 25 [BILLET X40 Z75; N10 G21 G98; N20 G28 U0 W0; N30 M06 T01; N40 M03 S1500; N50 G00 X42 N60 G00 Z-25
- 24. G74 – PECKDRILLING CYCLE G74 R… ; G74 Z… Q… F… ; First Block: R : Return amount (relief clearance for each cut) Second Block: Z : Depth of hole Q : Distance of each pecking F : Cutting feed rate
- 26. [BILLET X60 Z100 N10G21 G98 N20 G28 U0 W0 N30 M06 T01 – Centre punch N40 M03 S1500 N50 GOO X0 Z10 N60 G74 R1 N70 G74 Z-5 Q2000 F10 N80 G01 Z10 N90 G28 U0 W0 N100 M06 T02 - 10mm drill N110 G00 X0 Z5 N120 G74 R1 N120 G74 Z-35 Q2000 F10 N130 G01 Z10 N140 G28 U0 W0 N150 M06 T03 - 20mm drill N160 G00 X0 Z5 N170 G74 R1 N180 G74 Z-35 Q2000 F10 N190 G01 Z10 G28 U0 W0 M05 M30
- 30.
- 31.
- 32. [BILLET X40 Z100; N10G21 G98; N20 G28 U0 W0; N30 M06 T01; N40 M03 S1500; N50 G00 X40 Z2; N60 G90 X40 Z-40 R-1 F30 N70 R-2 N80 R-3 N90 R-4 N100 R-5 N110 G28 U0 W0 N120 M05 N130 M30
- 33. G72 FACING CYCLE G72W(1) R; G72 P Q U W(2) F; G72 - FACING CYCLE W(1) - DEPTH OF CUT R - RETRACT VALUE P - FIRST LINE OF SUBROUTINE Q - LAST LINE OF SUBROUTINE U - AMOUNT LEFT ON FOR FINISHING IN X W(2) - AMOUNT LEFT ON FOR FINISHING IN Z F - FEED RATE
- 34. [BILLET X60 Z100; N10G21 G98; N20 G28 U0 W0; N30 M06 T01; N40 M03 S1500; N50 G00 X62 Z-55; N60 G72 W0.5 R1; N70 G72 P80 Q110 U0.1 W0.1 F50; N80 G01 X50 N90 G01 Z-30 N100 G01 X40 Z-20 N110 Z2 N120 G70 P80 Q110 F30 N130 G28 U0 W0 N140 M05 N150 M30
- 35. G73 - PatternRepeating Cycle G73 U(1) W(1) R; G73 P Q U(2) W(2) F; U(1) = Amount of material to be machined on the X-axis W(1) = Amount of material to be machined on the Z-axis R = Amount of roughing passes P = Sequence number for the beginning of the contour Q = Sequence number for the end of the contour U(2) = Finish allowance on the X-axis W(2)= Finish allowance on Z-axis F = Feed rate
- 36. [BILLET X70 Z160; N10G21 G98; N20 G28 U0 W0; N30 M06 T01; N40 M03 S1500; N50 G00 X72 Z2; N60 G01 X0 Z0 N70 G73 U0.5 W0.5 R0.25 N80 G73 P90 Q130 U0.1 W0.1 F50 N90 G03 X20 Z-20 R10 N100 G01 Z-45 N110 G01 X40 Z-80 N120 G01 Z-105 N130 G02 X70 Z-120 R15 N140 G70 P90 Q130 F20 N150 G28 U0 W0 N160 M05 N170 M30