AnsweredAssumed Answered

SolidWorks CAM Post-Processor for Stepoko/Shapeoko?

Question asked by Steven Erickson on Sep 19, 2018
Latest reply on Feb 5, 2019 by Craig Serkanic

Like • Show 0 Likes0
Comment • 20

My company recently acquired a Stepoko CNC Machine from Sparkfun. We are looking to utilize SolidWorks new CAM feature with the machine for some in-house prototyping. The Stepoko board runs on Grbl v1.1, so I need a post-processor that will output to a format like that. None of the standard machine profiles included with SolidWorks seem to work. I've downloaded and tried to run this post-processor someone developed for just this kind of process, but I still have errors. The G-Code continues to write G41 commands which are not accepted with GRBL for whatever reason. That's not the only issue I have, but it's the main one.

Any suggestions on how to get things up and running?

1 person has this question

Outcomes

20 Replies

Michael Buchli Sep 19, 2018 11:45 AM
Mark Correct
Correct Answer
Steven,

If your machine does not like the Cutter compensation, you can turn it off in the contour mill operations. If you find that it runs after turning off the setting below, I would change the settings and then use "Save Operation Plan" to overwrite the settings in the techdb so you do not have to change it every time. Please post out a short test with this option turned off. It should remove the cutter compensation or G40,G41 commands.

Mike
Like • Show 1 Like1
Actions
- Steven Erickson @ Michael Buchli on Sep 19, 2018 11:58 AM
  Mark Correct
  Correct Answer
  Thanks Mike, that looks like it solved one issue. Now I'm trying to deal with the others. My new G-Code receives errors on the 3 lines marked. "G70", "G72$6", and "G999X2.0456F64.8". I also get an error later on for "Bad Arc Format. R not Supported". Any ideas?
  Like • Show 2 Likes2
  Actions
  - Michael Buchli @ Steven Erickson on Sep 19, 2018 12:08 PM
    Mark Correct
    Correct Answer
    G70 and G72 are traditionally turning cycles. Are you setting this for a lathe or mill? The radius could be a couple things as some controllers need arcs specified in I and J vs. R (radius). HawkRidge also has some posts for generic and specific machines that use different outputs. https://hawkridgesys.com/products/cam/post-processors#free Did the post you receive say it was setup for your machine? I want to understand a little more about what post you are using and if it is for a mill or lathe. John S. has also mentioned a name at Access if you are interested in getting a custom post created.
    
    Mike
    Like • Show 2 Likes2
    Actions
  - James Hurr @ Steven Erickson on Jan 29, 2019 7:58 PM
    Mark Correct
    Correct Answer
    I've also had a lot of trouble with getting CAM to work with GRBL 1.1 (XYZ-Carve = X-Carve machine)
    
    What I've found so far:
    
    You need to tinker with the number of decimal places precision in both Solidworks and the post processor, this may fix your ""Bad Arc Format. R not Supported" error. You can do this within Solidworks and using the Universal Post Generator (UPG) program.
    Otherwise GRBL breaks the radius into multiple straight steps, thinks they don't join up or fit on the arc and spits out an error.
    There's also a setting within GRBL for setting the precision of the error checking, that may affect it also.
    
    The standard post processor takes the machine to machine zero at the start of every program. Using UPG this can be taken out.
    There's some other redundant info in the Gcode also
    
    For some reason all but one of the lead-ins for the contouring stage confuses GRBL, the only one which worked for me is the simplest vertical lead-in.
    Curiously the most complex spiral lead-ins for the roughing stage work perfectly.
    Like • Show 0 Likes0
    Actions
    - Craig Serkanic @ James Hurr on Jan 31, 2019 9:10 PM
      Mark Correct
      Correct Answer
      James, the post on the Hawkridge website works (I do need to get the latest up). I have been working with Robert Futch (in this thread) and we have worked through almost all issues.
      
      -craig
      Like • Show 1 Like1
      Actions
John Stoltzfus Sep 19, 2018 11:47 AM
Mark Correct
Correct Answer
You could contact Access

Scott Gutwein

scottg@accessmfgsys.com
Like • Show 1 Like1
Actions
Josh Guyot Nov 28, 2018 7:35 AM
Mark Correct
Correct Answer
Hi Steven,

I'm also trying to find a workable post processor for a Shapeoko and Solidworks CAM. I'm currently pulling SW files into Fusion 360, setting up the CAM there and then exporting the GCode to SourceRabbit. Did you find a post-processor that works for SW CAM?

Thanks!
Like • Show 1 Like1
Actions
Michael Buchli Nov 28, 2018 12:59 PM
Mark Correct
Correct Answer
HawkRidge Systems is working on a free post for this machine. Today they have several on their website for download. https://hawkridgesys.com/products/cam/post-processors#free Please reach out to Craig @ craigs@hawkridgesys.com I spoke with him this morning to see if they were in process of creating a post for this machine. he said they were working on it but would like to hear from both of you to make the settings to best fit the machine.

Mike
Like • Show 2 Likes2
Actions
- William Finch @ Michael Buchli on Dec 3, 2018 3:25 PM
  Mark Correct
  Correct Answer
  Think I'll ask this here: Is there any plan for a Post Processor for a TinyG board? I think I close to getting the Laguna Router PP to work, but I would feel more warm and fuzzy with a PP for my specific machine.
  
  Thanks!
  Like • Show 2 Likes2
  Actions
  - Michael Buchli @ William Finch on Dec 3, 2018 3:45 PM
    Mark Correct
    Correct Answer
    Hey, William
    
    When I spoke with HawkRidge last week, they are interested in supplying these posts on their website but with the explosion in these types of routers, they are building them as they get requests. Please reach out to the folks at HawkRidge using the emails in the previous string and let them know your thoughts. They would be happy to work with you on these types of machines to make it easy for everyone to use SOLIDWORKS CAM to program.
    
    Mike
    Like • Show 3 Likes3
    Actions
Craig Serkanic Dec 3, 2018 8:24 PM
Mark Correct
Correct Answer
Steven, we are currently working on this and should have something up later this week on our website. https://hawkridgesys.com/products/cam/post-processors
https://hawkridgesys.com/products/cam/post-processors
Like • Show 2 Likes2
Actions
- William Finch @ Craig Serkanic on Dec 4, 2018 12:58 PM
  Mark Correct
  Correct Answer
  Craig,
  
  I think the Laguna Router PP will work pretty well with a TinyG. Perhaps the Stepoko will be exactly the same as the TinyG would be?
  Like • Show 2 Likes2
  Actions
- Steven Erickson @ Craig Serkanic on Dec 4, 2018 1:17 PM
  Mark Correct
  Correct Answer
  Craig,
  
  Thanks for the help! Our Stepoko is kind of on the backburner right now, but next time we use it I'll let you know how the post processor is working for me.
  Like • Show 1 Like1
  Actions
- Robert Futch @ Craig Serkanic on Dec 20, 2018 1:34 PM
  Mark Correct
  Correct Answer
  Hello Craig!
  
  Glad to hear you guys are working on the Carbide 3D GRBL post. I would be happy to provide some test feedback from our device when you guys have something to share.
  
  Thanks!
  Like • Show 2 Likes2
  Actions
Craig Serkanic Dec 4, 2018 1:04 PM
Mark Correct
Correct Answer
ok, we will have a Carbide 3D GRBL post in the router section later this week if you want to try that.
Like • Show 3 Likes3
Actions
- William Finch @ Craig Serkanic on Dec 4, 2018 1:14 PM
  Mark Correct
  Correct Answer
  Fantastic! Thank you!
  Like • Show 1 Like1
  Actions
Robert Futch Jan 15, 2019 6:23 PM
Mark Correct
Correct Answer
It seems Hawk Ridge is still working on their post. In the mean time I have been using the suggested GRBL post and just adding a G20 at the top. I also noticed that the provided GRBL post seems to hide the option to disable Canned Cycles when editing an operation. Not sure if that is the post or SolidWork's fault. GRBL does not do canned cycles so I have to use the M3-tutorial post if I want to do any drilling, then turn off the canned cycles in each drilling operation. That comes with the fixes mentioned elsewhere in this thread and:

- the M3-tutorial post outputs G04 X1 instead of G04 P1.
- the M3-tutorial post outputs O0001 which has to be removed
- the M3-tutorial post allows incremental arcs while GRBL does not

That last one was a weird problem when I was trying to do some slots, then some concentric circles and it just stopped mid operation. I found out the incremental arc operations meant that it was not repeating the circle start location. Shapeoko's software did not throw an error unless you look in the log for the error, error 26 (missing arc axis).

So I had to use the GRBL post to get it to repeat circle start points as needed, then switch to the M3-tutorial post for my drilling operations and fix the G04 problems in a text editor.

If anyone finds the .SRC file for the original GRBL post, share it here! Would be nice to be able to customize it.
Like • Show 0 Likes0
Actions
- Craig Serkanic @ Robert Futch on Jan 16, 2019 1:03 AM
  Mark Correct
  Correct Answer
  Robert, I looked at the GRBL post on our website and I am not seeing the same with our post.
  First the post on our website has an ID# and should read HRS1-00000055A in the parameters on the post processor tab.
  
  GRBL on the Hawk Ridge Website:
  The selection for canned cycle output on or off is present.
  The GRBL also outputs a G20 but it is after the tool comments. Maybe that needs to be before and right after the "%"?
  Our GRBL post was outputting a G04 X1. and I changed that to G04 P1.
  I am unclear on what exactly you are refering to on arc doing incremental. Are you speaking about the centers or the X and Y positions?
  
  M3 - tutorial post.
  I loaded the M3 tutorial post and the selection is not present. Maybe while switching between posts you may not have hit the select button?
  
  I am not sure what GRBL post your are using but the one with the ID# HRS1-00000055A looks to do everything you need except for the dwell. I have changed the dwell let me know about the G20 and clarify the arcs for me and I will correct all of it.
  
  Please let me know
  Like • Show 0 Likes0
  Actions
Craig Serkanic Jan 16, 2019 1:03 AM
Mark Correct
Correct Answer
The Shapeoko is on the Hawk Ridge website.
Like • Show 0 Likes0
Actions
Craig Serkanic Feb 5, 2019 3:00 PM
Mark Correct
Correct Answer
Everyone, please make sure you are using RevB on the Hawk Ridge Website.
Like • Show 0 Likes0
Actions

SolidWorks CAM Post-Processor for Stepoko/Shapeoko?

Outcomes

Related Content

Recommended Content