Solidworks CAM post processor

More
03 Mar 2020 20:54 #159107 by jpvonoy
Is there a LinuxCNC post processor for Solidworks CAM? As I understand from a little research, this CAM that is now included with Solidworks is powered by CAMWorks, but without the full features of CAMWorks.

Please Log in or Create an account to join the conversation.

More
06 Mar 2020 07:50 #159298 by key2
Replied by key2 on topic Solidworks CAM post processor
Hi,

which cam do you mean exactly (link?)?
There is hsmworks express for solidworks with linuxcnc-pp included.
Thx

Please Log in or Create an account to join the conversation.

More
07 Jun 2020 00:08 #170429 by Stephanisk
Do you have a link to that one?

Please Log in or Create an account to join the conversation.

More
07 Jun 2020 12:13 #170471 by Aciera

Please Log in or Create an account to join the conversation.

More
07 Jun 2020 15:25 #170495 by bbsr_5a
linuxcnc workes great with the given FANUC11m postprocessor includet in the solidcam database

Please Log in or Create an account to join the conversation.

More
25 Sep 2020 18:28 - 26 Sep 2020 04:20 #183754 by TBoy
Replied by TBoy on topic Solidworks CAM post processor
Most likely the original poster has moved on but yesterday when I was searching for a solution to a couple of issues this was the place that I ended up. This post will also serve as documentation for me and I hope it may help someone else in a similar situation. This is for newbies like myself, experts can feel free to ignore me :)

I have a Chinese OMIOCNC X6-2200 engraving machine. I ripped out the USB controller that came with it for Mach3 and installed a Mesa 7i76e and LinuxCNC. I'm good at the electronics, but not so much on Linux.

I use Solidworks2020 which has an HSMWorks post processor. There is a post processor you can select "LinuxCNC (EMC2)/linuxcnc".
Using this post I had 2 issues:
1- Material was being cut before my spindle motor was up to speed.
2- I was getting rounded corners on inside cuts.

After some googling the solution to 1 is to add "G4 P4" after the motor on command which adds a 4 second delay.
The solution to rounded corners is to add "G64 P.001 Q.001" on the header line. Seems pretty simple, and it is, but nowhere could I find how to do this automatically.

These instructions are for a windows machine.
1- Make a copy of the linuxcnc.cps likely found at c:\Program Files\HSMXpress\posts and put it on your desktop.
2- rename it
3- using Notepad++ or something similar open the file
4- Searched for "spindleSpeed" which takes you to the following line:
sOutput.format(spindleSpeed), mFormat.format(tool.clockwise ? 3 : 4)
5- Added to the end of the line so it looks like:
sOutput.format(spindleSpeed), mFormat.format(tool.clockwise ? 3 : 4), ("G4 P4")
6- Searched for "91.1" which takes you to the following line:
writeBlock(gAbsIncModal.format(90), gFeedModeModal.format(94), gPlaneModal.format(17), gFormat.format(91.1));
7- Added to the end of the line so it looks like:
writeBlock(gAbsIncModal.format(90), gFeedModeModal.format(94), gPlaneModal.format(17), gFormat.format(91.1), ("G64 P.001 Q.001"));
8- save the file
9- double click on the file and HSMWorks will attempt to compile the file. If successful it will offer to Install the Post for HSMWorks.
If you get this message respond "Yes" and you are done. If you get an error message then you have a syntax error in the file and you will need to fix it before the compile is successful.

Now when you "Post Process" a file in Solidworks you select "Setup" "Use Personal Post Library". Select the file name you used in Line 2 above and you are good to go. Check that your .ngc file has the additional G codes and your good to go.
Thanks to all that pointed me in the right direction.
Last edit: 26 Sep 2020 04:20 by TBoy. Reason: fixed a typo
The following user(s) said Thank You: tommylight, Tuxy

Please Log in or Create an account to join the conversation.

More
26 Sep 2020 00:58 #183769 by pippin88
Does your setup have spindle speed feedback into LinuxCNC?

If you have spindle speed into back into LinuxCNC then you can handle that with hal spindle-at-speed. If LinuxCNC does not know what the spindle speed is currently then a pause is a reasonable solution.

Just to point out a typo error: "G64 P.001 G.001" should be "G64 P.001 Q.001". You have it correct in your actual post-processor steps.

Please Log in or Create an account to join the conversation.

Moderators: Skullworks
Time to create page: 0.228 seconds
Powered by Kunena Forum