1 / 56

Numerical Control Programming

Numerical Control Programming. 6.1 NC PART PROGRAMMING. Introduction Coordinate Systems NC Words. 6.1.1 Coordinate System. Z // rotating spindle. Z AXIS workpiece-rotating machine : Z is parallel to the spindle tool-rotating machine : Z is parallel to the tool axis. Z. Z.

helki
Download Presentation

Numerical Control Programming

An Image/Link below is provided (as is) to download presentation Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author. Content is provided to you AS IS for your information and personal use only. Download presentation by click this link. While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server. During download, if you can't get a presentation, the file might be deleted by the publisher.

E N D

Presentation Transcript

  1. Numerical Control Programming

  2. 6.1 NC PART PROGRAMMING • Introduction • Coordinate Systems • NC Words

  3. 6.1.1 Coordinate System Z // rotating spindle Z AXIS • workpiece-rotating machine: Z is parallel to the spindle • tool-rotating machine: Z is parallel to the tool axis Z Z Z

  4. 6.1.1 Coordinate System X // table X AXIS • workpiece-rotating machine: X is the direction of tool movement • horizontal milling machine: X axis is parallel to the table • vertical machine: +X axis points to the right when the programmer is facing the machine. X Z X Z Z X

  5. 6.1.5 NC Words • N, G, X, Y Z, A, B, C, I, J, K, F, S, T, R, M • N: specify the sequence number • G: preparatory word to prepare for control functions (the motion of each axis, coordinate system, coordinate plane, cutter radius compensation, tool length offset……) • M: miscellaneous word to control miscellaneous functions (spindle on/off, start/stop the machine, turn on/off the coolant, change the tool, and rewind the program tape)

  6. 6.1.5 NC Words

  7. 6.1.5 NC Words M CODES

  8. 6.1.5 NC Words • Modal codes and non modal codes/ • modal functions Modal functions stay activeuntil some other command changes it. Modal commands are arranged in sets called “modal groups”, and only one member of a modal group may be in forces at any given time. • non-modal functions Non-modal functions have effect only on the lines on which they occur.

  9. 6.1.5 NC Words modal groups

  10. 6.1.5 NC Words modal groups M CODES

  11. 6.1.5 NC Words N, G, X, Y , Z, A, B, C, I, J, K, F, S, T, R, M • F: feed rate of the tool motion • S: cutting-speed • T: tool number

  12. 6.1.5 NC Words • X, Y, Z, A, B, C: provide the coordinate positions of the tool. X, Y, and Z define the three translational (Cartesian) axes of a machine. A, B and C are used for the three rotational axes about the X, Y, and Z axes. • I, J, K: specify the center for circular motion N, G, X, Y , Z, A, B, C, I, J, K, F, S, T, R, M

  13. 6.1.5 NC Words N, G, X, Y, Z, A, B, C, I, J, K, F, S, T, R, M • R: specify the clearance height in canned-cycle N0010 G81 X1.000 Y2.000 Z0.000 R1.300 Operations in drill cycle G81 : 1. Rapid to location (1,2,2). 2. Rapid down to the R plane:(1,2,1.3) 3. Feed to the Z point, the bottom of the hole:(1,2,0) 4. Operation at the bottom of the hole . 5. Rapid or feed to either the R plane or the initial height.

  14. NC Words

  15. G codes • Unit selection: • G70 (inch), G71(metric) • Coordinates selection: • G90(absolute), G91(incremental) • Working plane selection: • G17(X-Y), G18(Z-X), G19(Y-Z)

  16. Z 23 X 25.2 G92 X25.2 Z23.0 G55 G56 G57 G58 G59 G54 Machine zero Set up working coordinate • Machine zero • is unchangeable and usually is set up with the machine • Working coordinate (is decided by the offset from the machine zero) • G92 • Be defined in program

  17. End Start Rapid traverse: G00 • G00: • to make the machine move at maximum speed. • It is used for positioning motion. G90G00 X20.0 Y10.0 G90: absolute coordinates (20,10) (10,10) (0,0)

  18. Y End 100.0 200.0 X Start Linear interpolation: G01 • G01: • linear interpolation at feed speed. G91 G0l X200.0 Y100.0 F200.0 G91: incremental coordinates

  19. Circular interpolation: G02, G03 • G02, G03: • For circular interpolation, the tool destination and the circle center are programmed in one block • G02 is clockwise interpolation, G03 is counterclockwise interpolation End point Circle center, radius

  20. Y End X Start j Center i Circular interpolation: G02, G03 • Specify Center with I, J, K • I, J, K are the incremental distance from the start of the arc; • Viewing the start of arc as the origin, I, J, K have positive or negative signs.

  21. Y 100 R50 R60 60 40 X O 90 120 140 200 Circular interpolation: G02, G03 N0010 G92 X200.0 Y40.0 Z0； N0020 G90 G03 X140.0 Y100.0 R60.0 F300； N0030 G02 X120.0 Y60.0 R50.0； G92: To define working coordinate G90: absolute coordinates

  22. Circular interpolation: G02, G03 Annotation for Circular Interpolation • I0.0, J0.0, and K0.0 can be omitted. • If X,Y,Z are all omitted in the program, that means start and end of arc are same points. N0020 G02 I20.0 (a full circle) • If I, J, K, and R all appears in circular interpolation instruction, R is valid and I, J, and K are invalid

  23. Machine Zero Specified point A Return to Machine Zero: G28 G28 • The machine passes by the specified point, and then move to the machine zero. G91 G28 X_, Y_, Z_ • X,Y,Z are the coordinate of specified point that is saved in memory of machine. • Usually this instruction is used in the beginning and end of program. G91: incremental coordinates

  24. Machine Zero Specified point in G28 A New specified point in G29 Return to the Specified point : G29 G29 • The machine passes from the machine zero by the point that is specified in G28, and then move to the new specified point. G29 X_, Y_, Z_ • X, Y, Z are the coordinate of new specified point • G28,G29 are usually used to change tool

  25. M code • miscellaneous word • miscellaneous functions: • turn the spindle on/off • start/stop the machine • turn on/off the coolant • change the tool • rewind the program (tape)

  26. M code modal groups

  27. M code: M00, M01 • M00 and M01 both stop the machine in the middle of a program. • M01 is effective only when the optional stop button on the control panel is depressed. The program can be resumed through the control panel.

  28. M code: M03, M04, M05 • M03 turns on the spindle clockwise. • M04 turns the spindle on counterclockwise. (The spindle rpm must be specified in the same line or in a previous line. ) • M05 turns off the spindle.

  29. M code: M07, M08, M09 • M07 and M08 turn on different modes of coolant. • M07: flood coolant on • M08: mist coolant on • M09 turns off the coolant.

  30. M code: M06 • M06 signals the tool-change operation. • On a machine equipped with an automatic tool changer, it stops the spindle, retracts the spindle to the tool-change position, and then changes the tool to the one specified in the T-code.

  31. M code: M02, M30 • M02 marks the end of the program. • M30 marks the end of the tape. It stops the spindle and rewinds the program (tape)

  32. Example • A 2.0-in 2.0-in. square is to be milled using a 1/2-in. end milling cutter (end mill). Write an NC part program to make the square.

  33. Example

  34. G codes with animations http://www.cncezpro.com/gcodes.cfm

  35. Manual Part Programming Example Tool size = 0.25 inch, Feed rate = 6 inch per minute, Cutting speed = 300 rpm, Tool start position: 2.0, 2.0 Programming in inches Motion of tool: p0  p1  p2  p3  p4  p5  p1  p0

  36. 1. Set up the programming parameters Programming in inches Use absolute coordinates Feed in ipm N010 G70 G90 G94 G97 M04 Spindle speed in rpm Spindle CCW

  37. 2. Set up the machining conditions Machine moves in XY-plane Use full-circle interpolation Feed rate Spindle speed N020 G17 G75 F6.0 S300 T1001 M08 Tool no. Flood coolant ON

  38. 3. Move tool from p0 to p1 in straight line Linear interpolation target coordinates N030 G01 X3.875 Y3.698

  39. 4. Cut profile from p1 to p2 Linear interpolation target coordinates N040 G01 X3.875 Y9.125 or N040 G01 Y9.125 X-coordinate does not change  no need to program it

  40. 5. Cut profile from p2 to p3 Linear interpolation target coordinates N050 G01 X5.634 Y9.125

  41. 6. Cut along circle from p3 to p4 circular interpolation, CCW motion target coordinates N060 G03 X7.366 Y9.125 I6.5 J9.0 coordinates of center of circle N060 G03 X7.366 Y9.125 I0.866 J-0.125

  42. 7. Cut from p4 to p5 Linear interpolation target coordinates (Y is unchanged) N070 G01 X9.302

  43. 8. Cut from p5 to p1 Linear interpolation target coordinates (see step 3) N080 G01 X3.875 Y3.698

  44. 9. Return to home position, stop program Linear interpolation target coordinates (see step 3) N090 G01 X2.0 Y2.0 M30 end of data N100 M00 program stop

  45. 10. Complete RS-274 program N010 G70 G90 G94 G97 M04 N020 G17 G75 F6.0 S300 T1001 M08 N030 G01 X3.875 Y3.698 N040 G01 X3.875 Y9.125 N050 G01 X5.634 Y9.125 N060 G03 X7.366 Y9.125 I0.866 J-0.125 N070 G01 X9.302 N080 G01 X3.875 Y3.698 N090 G01 X2.0 Y2.0 M30

  46. Automatic Part Programming Software programs can automatic generation of CNC data Define Tool CNC data Make 3D model Simulate cutting

  47. Automatic part programming and DNC Very complex part shapes  very large NC program NC controller memory may not handle HUGE part program computer feeds few blocks of NC program to controller When almost all blocks executed, controller requests more blocks

  48. Assignment (Learn this software) • CNC Simulator • Download from • http://cnc-simulator.com/download/get.php?f=CncSetup453.exe

  49. Direct Numerical Control (DNC): • A system in which a central computer downloads the NC programs block by block to many NC machine tools simultaneously is called Direct Numerical Control (DNC) system.

  50. DNC • Direct numerical control (DNC) – control of multiple machine tools by a single (mainframe) computer through direct connection and in real time • 1960s technology • Two way communication • Distributed numerical control (DNC) – network consisting of central computer connected to machine tool MCUs, which are CNC • Present technology • Two way communication

More Related