Solidworks CAM CAMWorks Postprocessor

Hi,
i recently changed from Fusion360 to Solidworks 2021 and want to share my Postprocessor that works quite welll for linuxcnc.
My modifications that i missed from this PP :
- i removed the "G28 X0Y0" in the beginning and the end, left the one for "G28 Z0"
- it shows you the size of the stock to work on in the beginning
- it shows you the estimated machining time at the end of the gcode
- the tool-comment section now won't give me an error when opening the gcode in linuxcnc
If you have questions, feel free to ask. If you want to modify it, don't expect much help from me. I'm no expert.

I updated my PP with several smaller bits. The most important is the working compensation part (G41/G42). The old post added a 20 to the pocket number. This didnt work with my tooltable, where T=P number. I removed the addition of 20. To make compensation usable in CAM, make sure to check the following boxes:
 

Hello,
I have a small lathe retrofit with linuxcnc and I don't have the postprocessor, hou don't have this postprocessor
Best regards,
Ciux

I don't know if it works with a lathe, you can at least try it.

Dear Ralfh,

Thank you for sharing the postprocessor in the forum! We figured out to make some changes for our machine and it works well in general. I am still trying to figure out how to properly make use of G41/G42 commands. It works fine with outline and large pockets. But I run into problems when using cutter compensation for small pockets. Somehow, the entry moves don't work. I don't know if this is due to wrong CamWorks options (but already set them according to your post above) or in the PP.

I was wondering if G41 should be in a seperate line like in the examples on the documentation page ?

I was wondering if G41 should be in a seperate line like in the  examples on the documentation page  ?

That should'nt make a difference AFAIK.

I cant troubleshoot a lot because i'm no expert and i abandoned SW again, so just my experience: I often got a error with too small entry moves. I used G41/G42 only on final cuts and sometimes the checkbox "add tool radius to leadin" disengaged even when using my preset. 
Are you aware if the checkbox is enabled, and in addition to your regular leadin move, is small enough to fit in your small pocket? 
You can also play around with leadin-move-styles: parallel, arc, none. Maybe disengage the checkbox and calculate your leadin fully in its tab as small as possible but as big as needed?

Thanks for the reply. When I have some room for bigger leadin moves it works. But I can't figure out how to get it working in small pockets.

I made some screenshots to better explain the situation:

with all the NC settings set according to Ralfh's post above.

The G-Code looks like this:
What I get in LinuxCNC looks like this:


By trying to understand the G-Code I thought the G40 command is too early and should be after the last move with a leadout going back to X0Y0.

Then I get the following:


I tried moving around the G41 command to get better results but it did not work. When reading the code I can't figure out what is not correct? I am very thankful to any hints and help.

By the way Ralfh: We added the G64 command in the START_OF_TAPE section of the PP. The default behaviour of LinuxCNC is to round the corners of Rapid and Cutting moves to achieve the highest possible speed. So this ended up in really large radii which seemed dangerous.

What I would like to get is a different setting for cutting and rapid moves. If possible this could be set globally in LinuxCNC . But from my understanding this is not implemented. So I tried to modify the PP but did not succeed in creating a new modal G64 call with a variable P. P is already taken by other commands and seemed to be defined as an integer.

Ah, i see. Please try to cut the hole with a diameter at least half as big as the diameter of the hole. 

See: linuxcnc.org/docs/2.6/html/gcode/tool_co...:cutter-compensation

Programming Entry Moves -> The minimum length is the cutter radius

When you want to start at X0Y0 and your entry cut is already >3mm and your endmill radius another 3mm you get a hole of at least 12mm? I don't know exactly

If i remember correctly, you can also program the "P" as text in the postprocessor. Linuxcnc doesn't care, it sees a "P" and is happy.