So in HAAS control and Fusion360, you can set wear comp in Fusion, and then when you probe a bore using Fusion routines, you can update the wear value automatically and retry the boring op with the correct comp set.
Is there anything similar to this in PP? Or can I update the tool diameter in Gcode and read the stored probed values? I am new to GCode so pardon my ignorance.
You can update the tool diameter by setting parameter #5410 (be sure to call the tool offset again to apply the change). You can read the results of probing coordinates with parameters #5061-5069. Reference LinuxCNC documentation here on parameters, none of this has changed from our port of LinuxCNC to create Pathpilot.
There is no mechanism to do this automatically in Pathpilot right now, you would need to create a set of macros and modify the post processor to reference those macros.
Great! Thank you.
So my guess is that comp value in Fusion/Post needs to be “In Controller” and not as “Wear” since there is no wear value in PathPilot?
- Probe the bore.
- Read the value
- Read the current value in #5410 (Tool Diam)
- Update the current value in #5410 with : (Expected Bore Diam - Actual Bore Diam [5060-5069])
- Call the tool offsets again.
A good feature request would be to have a page or a section in PathPilots where one can assign buttons to run custom macros.
“there is no wear value in PathPilot?”
Different topic entirely . There is a diameter column in the tool table in Pathpilot and whether you use it as full diameter or wear is up to you (though conversational programs require the full tool diameter). And even if you use the full tool diameter entering .249" for a 1/4" tool is equivalent to applying a .001" wear offset.
“In controller” vs “wear” only changes the offset of the CAM toolpath between expecting a full diameter offset or wear value only. You have the procedure correct.
You can submit a feature request ticket here.
So just to make sure I understand this correct:
If I set in fusion/post a 1/2" tool… And use the setting “Wear” instead of “In Computer”, I can use the Tool Diam field to set tool wear values and expect them to compensate for differences I specify?
Say I probe a hole and read its .02" Smaller than it should, and the operation has a “Wear” option selected. I go to PP offsets and set the Tool Diam to .02 (positive or negative?) and expect it to compensate the diam and make the hole on the next use of the tool .02 larger?
I guess tool diam and setting to “In Controller” is much intuitive, except if you forget to set a diam initially
“If I set in fusion/post a 1/2” tool… And use the setting “Wear” instead of “In Computer”, I can use the Tool Diam field to set tool wear values and expect them to compensate for differences I specify?"
“Say I probe a hole and read its .02” Smaller than it should, and the operation has a “Wear” option selected. I go to PP offsets and set the Tool Diam to .02 (positive or negative?) and expect it to compensate the diam and make the hole on the next use of the tool .02 larger?"
We’re adding separate wear and diameter columns in a future update, fyi.
Awesome and great to hear about the separate column.