Welcome to Our Community

Some features disabled for guests. Register Today.

Fusion 360 and xPro v3 Controller

Discussion in 'CNC Mills/Routers' started by Keith Kimura, Aug 10, 2018 at 11:57 PM.

  1. Keith Kimura

    Keith Kimura Journeyman
    Builder

    Joined:
    Jun 26, 2018
    Messages:
    31
    Likes Received:
    4
    Which post processor should be used to generate G-Code from Fusion 360 to the xPro? I'm using the Grbl/grbl configuration selection but sometimes get commands that are invalid as well as some unusual behavior from my Workbee 1010 like unexpected plunges and inconsistent depths.
     
  2. Gary Caruso

    Gary Caruso OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    May 19, 2016
    Messages:
    489
    Likes Received:
    180
  3. Keith Kimura

    Keith Kimura Journeyman
    Builder

    Joined:
    Jun 26, 2018
    Messages:
    31
    Likes Received:
    4
    Hi Gary, thank you for the response. So I'm using the correct one? Grbl/grbl? Which means the errors are occurring either with UGS or at the xPro Controller, correct?
     
  4. Gary Caruso

    Gary Caruso OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    May 19, 2016
    Messages:
    489
    Likes Received:
    180
    Hi Keith, Hard to say without more info, post your grbl $$ settings, and post one of your fusion generated cnc files.
    Cheers
    Gary
     
  5. Keith Kimura

    Keith Kimura Journeyman
    Builder

    Joined:
    Jun 26, 2018
    Messages:
    31
    Likes Received:
    4
    Hi Gary,
    Here are my current grbl $$ settings and one of the fusion generated cnc files. On this particular file the Z-Axis plunged into the workpiece while ramping from 0,0,0 to the first cut location - I stopped the operation but unfortunately it had already cut across the workpiece ruining the entire project board. I appreciate your help.
     

    Attached Files:

  6. Gary Caruso

    Gary Caruso OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    May 19, 2016
    Messages:
    489
    Likes Received:
    180
    Hi Keith, it's your cut file, something is up with your settings, you have all your rapids inside of the work instead of above.. make sure you have your coordinates set correctly, you want Z pointing Up for up positive.
    Maybe your safe retract height is negative instead of positive?
    Also make sure you are zeroing the z at the top of the material.
    This video might help
     
  7. Scotty Orr

    Scotty Orr Master
    Builder

    Joined:
    May 21, 2015
    Messages:
    269
    Likes Received:
    131
    Kieth, I also noticed in your cut file you have an M6 command (which throws an error in grbl). I don't think you are using the post-processor that Gary linked a few posts above. Go back and check that link again. It's the Strooom custom grbl post-processor for F360. (If you look in the images folder, you'll see an example of how to tell F360 where the custom post-processor is.) . Should get rid of the errors.
     
    #7 Scotty Orr, Aug 12, 2018 at 5:05 PM
    Last edited: Aug 12, 2018 at 5:18 PM
  8. Keith Kimura

    Keith Kimura Journeyman
    Builder

    Joined:
    Jun 26, 2018
    Messages:
    31
    Likes Received:
    4
    My apologies, did not recognize that Gary's post was a link and not a statement, sorry. So, I did install the post but when I post process it I get this warning; "Invalid Work Coordinate System. Select WCS 1..6 in CAM software. InFusion 360, set the WCS in CAM workspace | Setup-properties | PostProcess-tab. Selecting default WCS1/G54." I did got to the Post Process tab in Setup but found no selection for default "WCS1/G54" so I changed the "Machine WCS/WCS Offset" to 1 and that eliminated the Warning. If this is correct let me know and can you give me an explanation of the warning and the fix. Thanks. Attached is the G-Code of the test file for you reference.
     

    Attached Files:

  9. Scotty Orr

    Scotty Orr Master
    Builder

    Joined:
    May 21, 2015
    Messages:
    269
    Likes Received:
    131
    Keith, I haven't used the Strooom post-processor yet - I was just pointing out about the link. (I do plan on using it once my machine is back up - just haven't got there yet.) I do think you have to be careful about where your machine is parked when you turn it on. It uses the G53 non-modal command (which the standard F360 grbl post-processor does not use). Your first line is going to plunge 10 units before it moves to WCS1. I'm just saying take care when testing. (And yes, from what I've read 1 is G54, 2 is G55, 3 is G56 and so on.) . Maybe someone who has used strooom can chime in here and explain more.

    There's another discussion of some of these issues here: Need knowledge on Grbl 1.1
     
    #9 Scotty Orr, Aug 13, 2018 at 2:17 PM
    Last edited: Aug 13, 2018 at 3:22 PM
  10. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    916
    Likes Received:
    414
    Strooom is busy updating his post because it does have some issues. It struggles with small lead-in and lead-out arcs which Fusion generates by default.

    Mine has been working for me for some time..... swarfer/GRBL-Post-Processor (which is based on Stroooms)

    The stock GRBL post that comes with Fusion is not in fact usable because it issues tool change commands that GRBL cannot process. It also assumes you have G28 co-ordinates set correctly.

    My post only assumes you have Z home in a safe 'up as far as it will go' position. All you need to do is put the Z up manually and then turn on (or hard reset) the controller.
    My post also allows you to insert manual Gcode commands between operations...
     

Share This Page

  1. This site uses cookies to help personalise content, tailor your experience and to keep you logged in if you register.
    By continuing to use this site, you are consenting to our use of cookies.
    Dismiss Notice