Use a Probe to Make Sure a Bore (or Boss) Has the Correct Diameter

Applies to machines built from: 
May, 2009
Known and Unknown WIPS Tasks

The Wireless Intuitive Probing System (WIPS) does many tasks. Some of the tasks are known. For example, WIPS makes these known tasks easier:

  • Set tool offsets.
  • Set work coordinate offsets.

But WIPS does other tasks that you possibly do not know. This document shows you how to make sure a bore (or boss) has the correct diameter.

Example: Make Sure a Bore (or Boss) Has the Correct Diameter.

This example shows you how to make a small program that measures each bore diameter.

This example puts a special small program into a part program. The part program has these cycles:

  • Drill cycle with a 1.0" (25.4 mm) drill (Tool number 1)
  • Contour cycle with a 0.5" (12.7 mm) endmill (Tool number 2)
  • Edge Break cycle with a 0.5" (12.7 mm) chamfer mill (Tool number 3)

 

Do the steps that follow to make the small program. This small program uses the OPM-40-2 probe. The small program measures a bore. If the bore diameter is correct, the program continues. If the bore is not correct, the program stops. The program stops with the probe above the bore that has an incorrect diameter. The operator can push CYCLE START to continue the program. Or the operator can push RESET to operate the program from the start.

This example is applicable only for a mill that has these two components:

  • WIPS
  • Mill software version M16.05 or higher

This example uses a Renishaw’s Bore/Boss Measurement cycle (Macro O9814 ). Refer to English - Renishaw Inspection Plus - Programming Manual - 2008. Read the section "Bore / boss measurement – macro O9814." Know this information from "Example 2:"

 

  1. T01 M06 - Select the probe.
  2. G54 X100.Y50. - Start position.
  3. G43 H1 Z100. - Get offset 1, go to 100 mm (3.94 in).
  4. G65 P9832 - Probe on (includes M19), or M19 for spindle orientation.
  5. G65 P9810 Z-10.F3000. - Protected positioning move.
  6. G65 P9814 X30.S2 - Measure a 30.0 mm (1.181") diameter bore.
  7. G65 P9810 Z100. - Protected positioning move.
  8. G65 P9833 - Probe off (where applicable).
  9. G28 Z100. - Reference return.

    continue

 

The example that follows changes the code from that program (program O9814). The example changes the tool to 20 for the probe. The example measures the bore after the 0.5" (12.7mm) endmill cycle is completed.

 

  1. To use these codes from program O9814, you must add codes that do these tasks:
    • Select the probe (T20 M06)
    • Move to the bore (G00 G90 G54 X0. Y0.)
    • Start the probe (G65 P9832)

    T20 M06 (SELECT PROBE)

    G00 G90 G54 X0. Y0. (MOVE TO BORE)

    G43 H20 Z4. (LENGTH OFFSET)

    G65 P9832 (START THE PROBE)

    G65 P9810 Z-0.2 F100. (PROTECTED POSITIONING MOVE)

  2. Add the code G65 P9814. Include only a D and H value to measure a bore for tolerance:
    • D is the bore diameter.
    • H is the tolerance (permitted error).
    H is a radius value. Thus an H value of .01" gives a .02" diameter tolerance.
    G65 P9814 D1.1 H0.01 (MEASURE A 1.1 INCH DIAMETER BORE)
  3. Add the code to do these tasks:
    • Move the probe away from the part. (G65 P9810 Z4.)
    • Stop the Probe. (G65 P9833)
    • Move the probe to Z zero. (G00 G53 Z0.)

    G65 P9810 Z4. (PROTECTED POSITIONING MOVE)

    G65 P9833 (STOP THE PROBE)

    G00 G53 Z0. (MOVE TO Z0.)

     

  4. Subsequently, the program does these tasks:
    1. The endmill mills the bore.
    2. The T20 M06 code puts the probe into the spindle.
    3. The probe moves to the G54 bore location.
    4. The probe measures the bore.
    5. If the bore error is less than the H (the tolerance), the program continues.
    6. If the bore error is more than H, the program stops.

 

Here is the completed program.

T2 M06 ( TOOL 2, 0.5 INCH DIAMETER FINISH ENDMILL )

G54 G90 G00 X0.1531 Y0.138

(PUT A CIRCLE MILLING PROGRAM HERE)

G90 G53 Z0.

M01

 

T20 M06 (SELECT THE PROBE)

G00 G90 G54 X0. Y0. (MOVE TO BORE)

G43 H20 Z4. (LENGTH OFFSET)

G65 P9832 (START THE PROBE)

G65 P9810 Z-0.2 F100. (PROTECTED POSITIONING MOVE)

 

G65 P9814 D1.1 H0.01 (MEASURE A 1.1 INCH DIAMETER BORE)

 

G65 P9810 Z4. (PROTECTED POSITIONING MOVE)

G65 P9833 (STOP THE PROBE)

G00 G53 Z0. (MOVE TO Z0.)

 

N3

T3 M06 ( 0.5 INCH 45 DEGREE CHAMFER MILL )

( TOOL 3, .5 COUNTERSINK )

G54 G90 G00 X0.2105 Y0.1685

S8000 M03

G43 Z1. H03 M08

(PUT A CHAMFER MILLING PROGRAM HERE)

G0 G53 Z0.

M30

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.

Feedback