View Full Version : Camworks mach3 to shopbot

05-19-2014, 03:24 AM
Hey all

A question I think I know the answer to , but in this day age I dunno anymore ;-)

Do I have to regenerate all my mach3 cut files ? Or is there a way that I can convert them so shop bot can use em ?


05-19-2014, 03:50 AM
The ShopBot program can read and run most g-code files (use the file type drop down when opening to select g-code files) which is what the Mach3 files are but I think the only real way to know is to load them up and see what happens in preview.

Some Mach3 files use macros that might not be supported etc.

05-19-2014, 07:39 AM
Your probably going to find it quicker and easier to regenerate. If you used an arc post p, the last time I looked SB would not run I & J commands, tool height offsets (if you use a tool changer) nor any M codes for spindle, vacuum or misting on/off.
the arcs would be the biggest issue to edit

05-19-2014, 09:59 AM
That's the problem ... A few files have worked but the majority don't

I have tried converting to igs/step file and then doing toolpaths in vetric , but the quality is useless ....


05-19-2014, 10:17 AM
What happened to the original source files?

I must admit I never bother keeping cut files I just always regenerate when I want to cut something again. I've been bitten too many times by changes I made to tool settings that I forgot about to run an old cut file.

05-19-2014, 10:59 AM
G2/G3 I and J commands work fine. Spindle control works for both on/off and RPM. The default Post for Mach3 Arc_Inch from Vectric works in SB without problems. There are some commands and formatting that will cause trouble though.

Here's a sample of the output from Vectrics Mach3 Post Processor for comparison to yours.

05-19-2014, 02:46 PM
i have the originals, i just dont know how to write G code for shopbot from camworks ... whats super frustrating is that it 'almost works' .....

this shows typically what happens ...

05-19-2014, 03:51 PM
Doesn't Camworks have a SB post processor? You might contact them about a postp

Scott, thats good news, its been a while since I tried to send g-gode to my SB controller.
I looked for the accepted g-code list on the SB site but couldn't find it.
is the MO3 MO5 the only m codes being converted ? what about pause cycles under the G4?

05-19-2014, 05:29 PM

Take a look at the 'User Guide (http://www.shopbottools.com/ShopBotDocs/files/SBG00142%20User%20Guide%202013%2005%2001.pdf)', page 50 is where it starts. There's a list of supported G/M codes. G04 P is supposed to work, but it doesn't. It seems to just skip over it and not pause. If you wanted to edit a file and put PAUSE or PAUSE 5 (whatever amount of time needed), it would work. Gcode and Sbp code can be mixed in the same file.

05-19-2014, 05:53 PM

It may depend on the version of SB3 you're running too. Some older version may not be able to read some gcode. That first picture that you posted there, was that the preview from SB3? If so, that's an old version, as that previewer hasn't been used for quite some time now.

You could also try the conversion tool under File/conversions and chose to convert gcode. Preview again to see if it is any better.

You might have an option in Camworks to edit the gcode processor or you might have the choice of several different gcode post processors and there might be one that works better. The SB user guide states that a standard FANUC format should be fine.

05-19-2014, 11:20 PM
Thanks for the link Scott, didn't think to look in the manual, very well covered section

05-20-2014, 07:00 AM
aaah, never thought about the version of SB ...

can i send someone a sbd file and see if it has the same problem ?

or is it possible to load it up here and just change to .txt ?

05-20-2014, 07:09 AM
this is the same file as above in the pics ....

05-20-2014, 11:11 AM

It's the G17,18,and 19 (plane assignment) that is causing the problems. If you can change your post proccessor to not use those, or edit the file to not use them, it should work. Also, the very first line is 'O0001' and that gives a unsupported command message that can be ignored, but you could just delete it.

Try this file. I just commented out the offending lines.

05-20-2014, 02:20 PM
wow scott it works !!!

but how do i change the post processor ? and more importantly that i can change it back again

i dont fancy going thru 300000 lines of G code searching out them lines ....

ta !! or shall i just send files to be processed to you ;-) *grin*

05-20-2014, 02:48 PM
ta !! or shall i just send files to be processed to you ;-) *grin*

Nooooo! ;)

I don't know anything about CamWorks, but it looks like you can edit post processors. https://www.youtube.com/watch?v=vXe0s5IbpC4

Do you have a choice of some other posts to regenerate your toolpaths? If you do, try some others that output gcode. Generic gcode, fanuc, mach3, iso, norm_emc etc. and compare the code or see how they run if at all.

05-21-2014, 12:12 PM
Scott !! thanks for the help !!

its working at last , after a few hours on the post processor i can get decent g-code to do the job !

still got a minor problem on 'circle being to small' but i am able to work around it

cheers !!