Problem With Threading Post Processing?

More
01 Dec 2018 09:25 #121675 by Skippy1
Guys,

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.

Cheers, Steve
More
02 Dec 2018 07:43 #121707 by Skippy1
Guys,

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.

Cheers, Steve
More
03 Dec 2018 14:04 #121749 by andypugh

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?
More
04 Dec 2018 02:56 #121797 by Skippy1
I contacted Dolphin support in the UK, and they quickly provided an updated PP file to be used with LinuxCNC. Them new PP produces a G76 move. 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 - it is quite weird. I'm poking through the G code, but I can't work out. what is going on. For those who can read chicken entrails, ;) I will attach the ppr (.txt) file and G code. ;)
Attachments:
More
04 Dec 2018 14:06 #121805 by andypugh

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:
github.com/LinuxCNC/linuxcnc/blob/7fb914...erp_convert.cc#L4700

And each threading pass looks like this:
github.com/LinuxCNC/linuxcnc/blob/7fb914...erp_convert.cc#L4654

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.
More
05 Dec 2018 02:58 #121844 by Skippy1
Thanks Andy,

Re the sudden change in an offset, I think I've messed up my tool offsets. I enabled offset display and the values are all over the place. I think I need to take a deep breath, and read up on a few things before I try anything new.



Cheers, Steve.
Attachments:
Moderators: piasdom
Time to create page: 0.717 seconds
Powered by Kunena Forum