Height issue after tool exchange between 3D rough and finish

[Hoosterw]

I am experiencing a height issue after a tools exchange between roughing 3D toolpath and the finish toolpath.
When I do the roughening with an 1mm endmill and I exchange to a 20degrees 0.1V-bit tool I set the height again using the Z probe but when it starts, its off by a tenth or so and runs above the roughening.

I checked and did the toolpathing again, same problem. Used another older file, same. Made the whole first file a new, same problem.

Any idea's where this might occur due to?

Rgds and happy and above all, healthy New Year.

[Adrian]

Are you zeroing to the same place on the material as when you zeroed the roughing tool? Has the roughing pass taken material away from that spot.

Are your tool definitions correct? Especially with the v-bit, if it has a flat on it then you need to define it as an engraving tool rather than a v-bit so Aspire knows about the flat.

[Hoosterw]

Sorry, its a engraving V-bit with a flat spot yes. I checked the tools and they seem ok. and yes I am zeroing height at an untouched part of the piece in both cases in the same place.
As there are more toolpaths then these (also cut outs) I zero of on the same place multpile times.

I even check calibration of the height travel of the machine. Its spot on. I first thought it was hardware related but I think I ruled that out.
So that leaves a software/design issue. I tried leaving more machining tolerance in the toolpath section of the roughening 3D. But that had the same effect.

[Rcnewcomb]

Is it possible that your control software has a tool length offset?

[Hoosterw]

Not likely. It came about when I started a whole new design and file in Aspire.

I ran an imported file from Artcam (my previous design software) and that was ok.
Before using Aspire I ran Artcam files on the machine and these never had the problem.

So it doen't look like the control software.

Thanks anyway.

[Rcnewcomb]

A quick look at the first 50 lines of the G code in the the finish toolpath file should quickly clarify whether or not the issues is with the cut file. Can you post them and tell us what the model thickness should be at the portion being cut?

[Hoosterw]

These are the first. all the same afterwards so less then 50.

T1M6
G17
G0Z20.000
G0X0.000Y0.000S12000M3
G0X124.892Y0.178Z5.000
G1Z-1.250F240.0
G1X127.889Y0.194F720.0
X132.324Y0.258
X120.441Y0.268
X116.959Y0.338
X136.214Y0.348

[Hoosterw]

I am looking at the T1M6 code. That seems a tool change code.
When looking at the processed file it gives an error:20.

[Rcnewcomb]

I believe your control software is GRBL. What post-processor are you using when you save your toolpaths?

[Hoosterw]

Error 20 is unknown command for my controller

[Hoosterw]

G code(mm).tap

Yes in deed GRBL

[Rcnewcomb]

Try the Grbl (mm) (*.gcode) post processor instead.

[Hoosterw]

OK, I will save the toolpath using the new postprocessor and run the files again tomorrow.
I need 2 extra models anyway.

Thanks for helping sofar. rgds Hans.

[Hoosterw]

Dear randall, thank you very much for the help, the issue has been resolved. Running the other post processor was the solutiuon

Rgds Hans

[Rcnewcomb]

Great to hear of your success.

Please show us some photos of your work when you get a chance.