3 CNC Programming R2CNCCNCCNCCNCCNCCNC.ppsx
- 2. Parts of a CNC program • Just like a written letter to a friend or business contact is comprised of three main parts • salutation, • body, and • closing, a CNC program is essentially broken into three similar main parts: • the salutation “program safe-start,” • the body “material removal,” • and the closing “program ending.”
- 3. CNC Programming • There is no standardized format for writing a CNC program that is compatible with all machine control models. • Each MCU manufacturer has developed its own unique programming format. • Each one has minor differences, but the principles contained in the context of a program are the same among them all. • The programming examples provided in these slides will relate the most closely to Fanuc-type controllers; however, the principles may be applied to any manufacturer’s programming format (see the specific machine’s programming manual).
- 4. CODES • Along with telling the machine what position to go to, the programmer must also provide the machine with instructions telling it what to do at that position.
- 5. CODES G codes M codes Preparatory codes Miscellaneous codes
- 6. CODES G codes M codes Carry out machining operations Establish machine settings Control the machine functions other than tool movements
- 7. CODES G codes Carry out machining operations Establish machine settings
- 8. G Codes - Axial Movements G00 Rapid traverse Moves the tool at a very fast rate to a specified point G01 Linear interpolation Machining in a straight line at a feed rate G02 Clockwise Circular interpolation Machining in a clockwise circular arc at a given feed rate G03 Counter-clockwise Circular interpolation Machining in a counter-clockwise circular arc at a given feed rate G28 Return to machine home position (Rapid traverse) Moves the tool at a very fast rate to the home position
- 9. Coordinate positioning : Radial +X - X +Z - Z We will NOT use Radial system for this course
- 10. Coordinate positioning : Diametral +X - X +Z - Z We will use Diametral system for this course
- 11. G Codes - Axial Movements Tool G00 Rapid traverse Moves the tool at a very fast rate to a specified point G00 X30 Z5 Home Position X30 Z5 40 +X - X +Z - Z
- 12. G Codes - Axial Movements Tool G01 Linear interpolation Machining in a straight line at a feed rate (one or more axes) G01 X30 Z-20 F40 G00 X30 Z5 X30 Z-20 40 +X - X +Z - Z X30 Z5 Feed rate
- 13. G Codes - Axial Movements Ø40 Ø30 35 G00 X30 Z5 G01 X30 Z00 F40 X40 Z-35 1 2 3 (Home 1) (1 2) (2 3) Home Position +X - X +Z - Z
- 14. G Codes - Axial Movements G02 Clockwise Circular interpolation Machining in a clockwise circular arc 1 2 +X - X +Z - Z G02 X40 Z-25 R10 15 25 3 R10 G00 X20 Z5 G01 X20 Z-15 F40 Ø40 Ø20 Clockwise Radius
- 15. G Codes - Axial Movements G03 Counter-clockwise Circular interpolation Machining in a counter-clockwise circular arc 1 2 G03 X40 Z-25 R10 15 3 R10 G00 X20 Z5 G01 X20 Z-15 F40 Ø40 Ø20 25 Ø40 Ø20 +X - X +Z - Z Counter- clockwise Radius
- 16. G Codes – Machine Setup For Milling ONLY G90 Absolute positioning All coordinates are relative to the reference position (i.e. Workpiece Origin) G91 Incremental positioning All coordinates are relative to the current position For Turning ONLY No need to write G code for the following in Turning × Absolute positioning Machine will run on Absolute Mode by default × Incremental positioning U Incremental mode in X axis W Incremental mode in Z axis
- 17. G Codes - Axial Movements G28 Return to machine home position (Rapid traverse) Moves the tool at a very fast rate to the home position G28 U00 W00 Tool will • move 00 in the X direction and 00 in the Z direction (incremental mode) • and then will return to the Home position Incremental mode in X axis Incremental mode in Z axis Important point Tool Home Position 40 +X - X +Z - Z
- 18. G Codes – Machine Setup G20 Imperial input Inch programming units G21 Metric input Millimetre programming units G98 Feed per minute inches/millimetres per minute G99 Feed per revolution inches/millimetres per rev
- 20. CODES M codes Control the machine functions other than tool movements
- 21. M codes : Group 1 M00 Program Stop utility stop for operator actions M01 Optional Program Stop operator selected or ignored M02 Program End needs manual reset to start again from the beginning M30 Program End and Rewind stop and automatic reset
- 22. M codes : Group 2 M03 Spindle ON (Clockwise) M04 Spindle ON (Anti-Clockwise) M05 Spindle OFF M06 Tool Calling M08 Coolant ON M09 Coolant OFF
- 23. Ø50 Ø40 Ø20 10 30 45 50 A B C D E +Z -Z -X +X X40 Z-30 G00 X20 Z5 G01 X20 Z-10 F40 X40 Z-45 G02 X50 Z-50 R5
- 24. +Z -Z -X +X
- 26. +Z -Z -X +X
- 27. +Z -Z -X +X
- 28. +Z -Z -X +X
- 29. +Z -Z -X +X
- 30. +Z -Z -X +X
- 31. +Z -Z -X +X Material to be left for finish pass
- 33. +Z -Z -X +X Roughing depth of Cut Material to be left for finish pass
- 34. Canned Cycles • Many turning operations require tedious and redundant motions, such as the multiple passes performed during a rough turning operation or multiple pecks required for deep hole-drilling operations. • Machine control manufacturers have equipped the controls with features that make these tedious operations easier and faster to program. • These machining routines can be packaged or “canned” into one or two blocks of code and are called canned cycles.
- 35. Stock Removal Turning Cycle : G71 • Function G71 is the stock removal cycle for turning that removes metal along the direction of the Z axis. In a case where there is a lot of material to be removed, this cycle provides an easy method for programming. • There are two program blocks required for function G71. G71 U R G71 P Q U W F Block 1 Block 2
- 36. Stock Removal Turning Cycle : G71 G71 U R G71 P Q U W F Block 1 Block 2 depth of roughing cut (no sign) amount of retract, along the X axis, for each cut block number where the code for the contour begins block number where the code for the contour ends amount of material for finishing to be left on all diameters (X axis) amount of material for finishing to be left on all faces (Z axis) roughing feed rate
- 37. Stock Removal Turning Cycle : G71 Depth of Cut U Retract amount R finish amount to be left on the diameter U finish amount to be left on Z-axis faces W +Z - Z +X -X 10 25 75 50 90 R12.5 Rough Stock diameter 62.5
- 38. Stock Removal Turning Cycle : G71 N30 G71 P40 Q80 U1 W1 F30 N10 G00 X95 Z5 N20 G71 U5 R0.5 N40 G00 X10 Z5 N50 G01 X10 Z-25 N60 X50 Z-62.5 N70 G02 X75 Z-75 N80 G01 X95 Z-75 Block 1 Block 2 Cycle Blocks
- 39. Finishing Cycle : G70 G70 P Q F S block number where the code for the finishing contour begins block number where the code for the finishing contour ends feed rate, effective for blocks P through Q spindle speed, effective for blocks P through Q
- 40. Stock Removal Turning Cycle : G71 and Finishing Cycle G70 N30 G71 P40 Q80 U1 W1 F30 N10 G00 X95 Z5 N20 G71 U5 R0.5 N40 G00 X10 Z5 N50 G01 X10 Z-25 N60 X50 Z-62.5 N70 G02 X75 Z-75 N80 G01 X95 Z-75 Block 1 Block 2 Cycle Blocks G70 P40 Q80 F10 S1500 Finishing Cycle
- 41. Examples of Stock Removal Turning Cycle G71 program •Refer to “CNC Lab Qs” pdf file
- 42. 20 +X - X +Z - Z X12 Z2 Ø10 G21 G98 (Metric unit and feed in mm/min) G28 U0 W0 (Go to home position) M06 T0101 (Tool 1 & Offset 1) M03 S2500 (Clockwise spindle at 2500rpm) G00 X12 Z2 (Go to home position) G94 X0 Z-2 F100 (Facing cycle) Z-4 G28 U0 W0 (Go to home position) M05 (Spindle stop) M30 (Program end and rewind) Facing Cycle : G94 P ( Home → P )
- 43. 20 18 +X - X +Z - Z Z-2 X12 Z2 Ø10 G21 G98 (Metric unit and feed in mm/min) G28 U0 W0 (Go to home position) M06 T0101 (Tool 1 & Offset 1) M03 S2500 (Clockwise spindle at 2500rpm) G00 X12 Z2 (Go to home position) G94 X0 Z-2 F100 (Facing cycle) Z-4 G28 U0 W0 (Go to home position) M05 (Spindle stop) M30 (Program end and rewind) Facing Cycle : G94 P ( Home → P )
- 44. 20 18 +X - X +Z - Z Z-2 X12 Z2 Ø10 G21 G98 (Metric unit and feed in mm/min) G28 U0 W0 (Go to home position) M06 T0101 (Tool 1 & Offset 1) M03 S2500 (Clockwise spindle at 2500rpm) G00 X12 Z2 (Go to home position) G94 X0 Z-2 F100 (Facing cycle) Z-4 G28 U0 W0 (Go to home position) M05 (Spindle stop) M30 (Program end and rewind) Facing Cycle : G94 P ( Home → P )
- 45. 20 18 16 +X - X +Z - Z Z-2 Z-4 X12 Z2 G21 G98 (Metric unit and feed in mm/min) G28 U0 W0 (Go to home position) M06 T0101 (Tool 1 & Offset 1) M03 S2500 (Clockwise spindle at 2500rpm) G00 X12 Z2 (Go to home position) G94 X0 Z-2 F100 (Facing cycle) Z-4 G28 U0 W0 (Go to home position) M05 (Spindle stop) M30 (Program end and rewind) Facing Cycle : G94 P ( Home → P )
- 46. Peck Drilling Canned Cycle G74 G74 R G74 X Z Q F total absolute Z-depth amount of retract peck increment or depth of cut in Z axis Micrometre (µm) Feed rate X-axis hole location (part centerline)
- 47. Clearance Z Q R Clearance G74 R G74 X Z Q F Micrometre (µm) Micrometre (µm)
- 48. Clearance 20 5000 1 Clearance G74 R1 G74 X0 Z-20 Q5000 F50 Micrometre (µm) Micrometre (µm)
- 49. Threading Cycle : G76 G76 P000000 Q R G76 X Z P Q F Block 1 Block 2 number of finishing cuts angle of the thread minor diameter (Major Dia - 2*Thread Height) Final end position of the thread along the Z axis Height of thread in micron (= 0.613*Pitch) First pass depth of cut feed rate (normally equal to the thread pitch). Relief angle (to retract it may be require some angle) minimum cut depth for rough cut depth of the final pass (finishing allowance) Micrometre (µm) in software mm in machine Micrometre (µm) in software mm in machine Micrometre (µm) in software mm in machine
- 50. Threading
- 51. Threading