[amphib]

I have a Haas mill and a Renishaw 40-2 wireless probe.

I would like to incorporate code into a program to probe the surface of a part and then modify that value to establish the G54 Z offset. Specifically, I want the Z plane to be 0.015 below the probed surface. Can anyone show me how to do this?

Here's the code I use to probe the surface:

T10 M6
G00 G90 G55 X0. Y0. (GETS THE PROBE TO THE CENTER OF THE PART)
G43 H10 Z0.5 (GETS THE PROBE ABOUT 0.5 ABOVE THE PART)
G65 P9359 W54. Z-0.7 (PROBES AND ASSIGNS THE RESULT TO THE G54 Z REGISTER)
G65 P9833 (TURNS OFF THE PROBE)
G53 Z0. (RETRACTS TO THE TOOL CHANGE POSITION)

Thanks!

[generaldisarray]

probes a pocket floor in a forging and sets Z origin in the air above it with stock allowance for facing operation.

There is a user variable line there with the print dimension because I originally thought I had to do all this with my own macro. But a little reading told me that there was a cycle. I left the #500 just as a reference,


( Z ORIGIN PROBING WITH STEP SHIFT)
T20 M06
( Z ORIGIN PROBING WITH STEP SHIFT)
(do not start below zref surf. you will crash)
#500= 0.351 (PRINT DIMENSION FOR STEP)
G00 G54 G90 X-1. Y0.
G43 H20 (PROBE LENGTH OFFSET CALL)
G65 P9832 (PROBE ON)
G65 P9810 Z0.1 F100. (PROTECTED POSITIONING)
Z0. F20.
G65 P9811 Z-0.376 S1 (TOUCH Z SURF AND SET G54 Z)
G65 P9810 Z10. F100. (PROTECTED POSITIONING)
G65 P9833 (PROBE OFF)
G00 G28 G91 Z0.

[sinha_nsit]

I have a Haas mill and a Renishaw 40-2 wireless probe.

I would like to incorporate code into a program to probe the surface of a part and then modify that value to establish the G54 Z offset. Specifically, I want the Z plane to be 0.015 below the probed surface. Can anyone show me how to do this?

Here's the code I use to probe the surface:

T10 M6
G00 G90 G55 X0. Y0. (GETS THE PROBE TO THE CENTER OF THE PART)
G43 H10 Z0.5 (GETS THE PROBE ABOUT 0.5 ABOVE THE PART)
G65 P9359 W54. Z-0.7 (PROBES AND ASSIGNS THE RESULT TO THE G54 Z REGISTER)
G65 P9833 (TURNS OFF THE PROBE)
G53 Z0. (RETRACTS TO THE TOOL CHANGE POSITION)

Thanks!

You are already setting G54 Z0. You wish to modify this. It can be easily done through the associated system variable for G54 Z.
Don't know about Haas, but it is #5223 on i-series Fanucs. Just append this line in the end:
#5223 = #5223 - 0.015
Let us know if it works.