Problem With Threading Post Processing?
Just a quick question to see if anyone else has run into this problem.
I'm having a play with an evaluation version of Dolphin Cam (Partmaster) for lathes, and tries a simple exercise to face, rough, profile, and thread a short shaft. All operations work on Partmaster when simulated. I then used the EMC post processor listed in the program, but there is an issue when the threading G code is used in Linuxcnc. The threading section runs, but instead of cutting parallel to the centreline of the shaft, the thread is cut at an angle of about 20 degrees in the general position it should be. I'm guessing a problem with the post processor, or settings I'm using in Linuxcnc, or something random.
Anyway, it's not a big issue at the moment, but if you have seen this problem before, I would appreciate your advice.
I've had a look at the G code Partmaster generated, (at first it was a bit like reading chicken entrails to find lotto numbers), and that's the problem.
It has a series of G01 moves which position the tool at the correct start point for the thread, (and correctly incrementing the depth on each pass), but the actual thread cutting move is a G00 which goes to a point at the correct Z point, but at an incorrect X point which is outside of he diameter of the proposed thread.
I will try and contact Dolphin, and see what they think.
Skippy1 wrote: It has a series of G01 moves which position the tool at the correct start point for the thread, (and correctly incrementing the depth on each pass), but the actual thread cutting move is a G00 which goes to a point at the correct Z point, but at an incorrect X point which is outside of he diameter of the proposed thread.
Really? It should at the very least be a G33!
Can you edit the postprocessor to use G76?
Skippy1 wrote: I tried the new PP this morning, and it cuts a nice thread parallel to the Z axis. However, there is something screwy going on, as just prior to the start of the threading, it appears as if the sudden change in an offset or something
G76 does that. It isn't Dolphin's fault.
I think it is part of making every pass exactly the same, so it does an X retract, (zero length) Z retract and then X advance at the beginning of the first pass.
This is the G76 cycle:
And each threading pass looks like this:
So each pass ends at the end of the retract at finish-Z and starts with a retract. Which is what you see at the beginning of the cycle, when it is already at the start Z.
I already had Dolphin for lathe and mill, but was only using it for the cnc router. I got it to do the usual turning, profiling, grooving stuff, and with the revised PP, also single-point threading and rigid tapping. (Note that I mainly use CamBam for most 2.5D stuff on the router, as I really like it.) My experience was that the evaluation version of Dolphin worked the same as the licensed version, except for the expiry period, so the issue may be something else?
Attached for your information and use is the latest PP file for Linuxcnc lathe I got from Dolphin. Note that I have changed the file type from .ppr to .txt, so that I could upload it to the forum. You will need to change it back to .ppr to use it.