1 / 38

HAAS TRAINING - INTRODUCTION

HAAS TRAINING - INTRODUCTION. HAAS TRAINING - INTRODUCTION. What Is Going To Be Covered? . General Spindle Probe Information Probe Calibration Probe Usage Macro Answer Questions. HAAS TRAINING - INTRODUCTION. HAAS TRAINING - INTRODUCTION. HAAS TRAINING - GENERAL PROBE INFORMATION.

ssykes
Download Presentation

HAAS TRAINING - INTRODUCTION

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. HAAS TRAINING - INTRODUCTION

  2. HAAS TRAINING - INTRODUCTION • What Is Going To Be Covered? • General Spindle Probe Information • Probe Calibration • Probe Usage • Macro • Answer Questions

  3. HAAS TRAINING - INTRODUCTION

  4. HAAS TRAINING - INTRODUCTION

  5. HAAS TRAINING - GENERAL PROBE INFORMATION

  6. HAAS TRAINING - GENERAL PROBE INFORMATION • What Are The Uses of Spindle Probes? • Work Piece Setup • Inspection • Process Control

  7. HAAS TRAINING - GENERAL PROBE INFORMATION G31 SKIP FUNCTION A non-modal operation that causes a linear move to a specified position. It applies only to the block in which G31 is specified. The specified move is started and continues to the end point or until a skip signal is processed (this position is stored in macro variables).

  8. HAAS TRAINING - GENERAL PROBE INFORMATION G31X7.F100. Macro Variable Stores 3.

  9. HAAS TRAINING - GENERAL PROBE INFORMATION G31X6.F100. Macro Variable Stores 6.

  10. HAAS TRAINING - GENERAL PROBE INFORMATION • Major Components Of A Probe System • Probe • Transmission • Interface

  11. HAAS TRAINING - GENERAL PROBE INFORMATION

  12. HAAS TRAINING - GENERAL PROBE INFORMATION

  13. HAAS TRAINING - CALIBRATION

  14. HAAS TRAINING - CALIBRATION (MECHANICAL) Mounting Hardware Assemble Spindle Probe -Attach Probe To Shank

  15. HAAS TRAINING - CALIBRATION (MECHANICAL) Mounting Hardware Assemble Spindle Probe -Attach Stylus To Probe

  16. HAAS TRAINING - CALIBRATION (MECHANICAL) Setup Spindle Probe Dial-In Spindle Probe Stylus To Spindle Center

  17. HAAS TRAINING - CALIBRATION (SOFTWARE) Calibration of Spindle Probes Set the Length of the Probe (Suggest Common Reference Point to Avoid Having to Recalibrate for Every Setup) and Enter Length in Tool Offset Page Fixture a Known Ring Gauge to Table Leaving the I D Free From Interference Find the Center of the Ring Gauge with a Dial Indicator and Enter the X and Y Positions in G59 Find the Face of the Ring Gauge and Enter the Z Position in G59

  18. HAAS TRAINING - CALIBRATION (SOFTWARE) Calibration of Spindle Probes Create New Program and Add G90G80G40G0; G91G28Z0; G90; T20M6; (T?? Tool Number of Probe) G59X0Y1.25; (Position Above Ring Gauge Face) G43H20Z5.; (H?? Tool Offset of Probe) G65P9832; (Turn Probe On) G65P9810Z.25F200. (Protective Position F??? Becomes Modal)

  19. HAAS TRAINING - CALIBRATION (SOFTWARE) G65P9801Z0.T20; (T?? Tool Offset Number) G65P9810X0.Y0.; (Protective Position) G65P9810Z-.4; (Protective Position) G65P9802D2.; (D? is the Diameter Stamped on Ring Gauge) G65P9804D2.; (P9803 if MP700, D? is the Diameter Stamped on Ring Gauge) G65P9810Z5.; (Protective Position) G91G28Z0.; G90; M30;

  20. HAAS TRAINING - CALIBRATION (SOFTWARE) Run Program Slow First Time to Make Sure there were no Programming Errors Run Program Again with the Feed Rate at 100% (Rapid does not need to be 100%) Verify that the Probe Tool Length Offset did not Change Drastically Verify Macro Variables #500 and #501 are Approximately the Stylus Ball Radius (only #501 if MP700, if O9804 was Run #510 through #517 Should also be Approximately the Stylus Ball Radius) Verify Macro Variables #502 and #503 are Less than .002”

  21. HAAS TRAINING - PROGRAMMING

  22. HAAS TRAINING - PROGRAMMING Programming a Spindle Probe When Programming a Spindle Probe a Program Need to be Created, Just is if Programming a Cutting Path

  23. HAAS TRAINING - PROGRAMMING Example Skeleton Program G90G80G40G0; (Preparatory Codes) G91G28Z0; (Send Machine Home in Z) G90; (Return Machine to Absolute) T20M6; (Tool Change Probe In) G54X0Y0; (Call Up Work Offset) G43H20Z5. (Apply Tool Offset) G65P9832; (Turn Probe On) G65P9810Z.25F200.; (Protective Position) (Insert Gauging and Position Cycles); G65P9810Z5.; (Protective Position) G91G28Z0; (Send Machine Home in Z) M30; (End Program)

  24. HAAS TRAINING - PROGRAMMING Inspection Plus + Inspection Plus for MP700 O9810 Protected Positioning O9811 Single Surface Measurement O9812 Web/Pocket Measurement O9814 Bore/Boss Measurement O9815 Finding an Internal Corner O9816 Finding an External Corner O9821 Angle Single Surface Measurement O9821(MP700) XYZ Axis Single Surface O9822 Angle Web/Pocket Measurement O9823 3-Point Bore/Boss Measurement O9817 4th Axis X Measurement O9818 4th Axis Y Measurement

  25. HAAS TRAINING - PROGRAMMING O9819 Bore/Boss on PCD Measurement O9820 Stock Allowance O9830 Storing Multi-Stylus Data O9831 Loading Multi-Stylus Data O9832 Turn Probe On O9833 Turn Probe Off O9834 Feature to Feature X+Y or Z Plane O9835 Updating the SPC Tool Offset O9836 Optimizing a Probing Cycle O9843 Angle Measurement X or Y Plane

  26. HAAS TRAINING - PROGRAMMING (OPTIONAL INPUTS) Bb b= Angle tolerance of the surface Ee e= Experience value. Ff f= Percent feedback when updating a tool offset Hh h= Tolerance value of a feature dimension being measured. Mm m= True position tolerance of a feature.

  27. HAAS TRAINING - PROGRAMMING (OPTIONAL INPUTS) Qq q= Probe overtravel distance for use when the default values are unsuitable. Rr r= An incremental dimension that is used in external features to give a radial clearance from the nominal target surface prior to a Z-axis move. Ss s= Work offset number which will be set. S1-S6 Tt t= Tool offset number to be updated

  28. HAAS TRAINING - PROGRAMMING (OPTIONAL INPUTS) Uu u= Upper tolerance limit. If this value is exceeded there is no tool offset or work offset updated and the cycle is stopped with an alarm. This tolerance is applied to both size and position where applicable. Vv v= Null band. This is the tolerance zone where no tool offset adjustment occurs. Ww w= Print data

  29. HAAS TRAINING - ALARMING METHOD • Inspection Plus can be made to run in two different modes • -Flags and Alarms • -Flags Only • The alarming method is determined in O9724

  30. HAAS TRAINING - ALARMING METHOD

  31. HAAS TRAINING - CYCLE EXAMPLES UPDATING WORKOFFSETS 1) G65P9811Z0S1. Gauge a Z face and update G54 2) G65P9814D1.S3. Gauge a 1” bore and update G56 3) G65P9816X0Y0S6 Gauge an external corner and update G59

  32. HAAS TRAINING - CYCLE EXAMPLES UPDATING TOOL OFFSETS 1) G65P9811Z0T11. Gauge a Z face and update T11 (Length) 2) G65P9814D1.T3. Gauge a 1” bore and update T3 (Diameter) 3) G65P9812X4.T6.F.8 Gauge a 4” pocket and update T6 (Diameter) by 80%

  33. HAAS TRAINING - CYCLE EXAMPLES INSPECTION 1) G65P9811X0.M.005 Gauge a X edge to a Tolerance of .005” 2) G65P9814D1.H.005M.002 Gauge a 1” bore to a Size Tolerance of .005” and Position Tolerance of .002” 3) G65P9812X4.Z-.25W1. Gauge a 4” Web and Print results to RS232 port

  34. HAAS TRAINING - CYCLE EXAMPLES (ADVANCED) PART IDENTIFICATION Protected Positioning Method G65P9810Z0M1. IF[#148EQ0]GOTO100 M98P5000 (Call Up Program for Part A) (Triggered) GOTO500 N100 M98P6000 (Call Up Program for Part B) (Completed) N500 M30

  35. HAAS TRAINING - CYCLE EXAMPLES (ADVANCED) PART IDENTIFICATION Different Size Bores G65P9814D1Q6. IF[#138GT1.4]GOTO100 M98P5000 (RUN PROGRAM A) GOTO5000 N100 IF[#138GT1.9]GOTO200 M98P5001 (RUN PROGRAM B) GOTO5000 N200 IF[#138GT2.4]GOTO300

  36. HAAS TRAINING - CYCLE EXAMPLES (ADVANCED) (CONTINUED) M98P5003 (RUN PROGRAM C) GOTO5000 N300 #3000=10(DIA TOO LARGE) N5000 M30

  37. HAAS TRAINING - CYCLE EXAMPLES (ADVANCED) COORDINATE ROTATION G65P9816X0Y0I2.J2. G65P9810Z5. G17 G68X#135Y#136R#139 MACHINING…….. G69

More Related