Welcome to Our Community

Some features disabled for guests. Register Today.

Fusion 360 post to Blackbox troubleshooting

Discussion in 'CAM' started by SteamLabs, Jul 6, 2021.

  1. SteamLabs

    SteamLabs New
    Builder

    Joined:
    Mar 29, 2017
    Messages:
    10
    Likes Received:
    3
    I retrofitted an old Intelliteck router with a Blackbox controller. It works fine with Openbuilds CAM, but when I try to use Fusion 360 CAM I run into issues.
    The machine homes to the front left corner, Z homes to the top.
    Limits are:
    X 335
    Y 485
    Z 190

    As soon as I start the program from home, the work axes change to the following:
    X -334
    Y -484
    Z -10
    I get an Alert 2 which doesn't make sense.
    Gcode says G0 X50.xxx Y17.xxx
    If I turn off soft limits the machine will try to go to the rear right corner, so I have to stop it before it crashes.
    I double checked to makes sure everything is in mm.

    I tried starting the program from home and from the top corner of the part, no change.
    Any help is appreciated.
     
  2. Peter Van Der Walt

    Peter Van Der Walt OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Mar 1, 2017
    Messages:
    13,751
    Likes Received:
    4,070
    Homing sets Machine Zero
    Probing/SetZero button sets Work coordinates.

    Are you remembering to Zero the Work Coordinates?
     
  3. SteamLabs

    SteamLabs New
    Builder

    Joined:
    Mar 29, 2017
    Messages:
    10
    Likes Received:
    3
    I've done it both ways.
    I've used the probe to set the work coordinates, and I've done it manually.
    Same issue.
     
  4. Peter Van Der Walt

    Peter Van Der Walt OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Mar 1, 2017
    Messages:
    13,751
    Likes Received:
    4,070
    And you have your Homing Dirs configured correctly? See gnea/grbl
     
  5. SteamLabs

    SteamLabs New
    Builder

    Joined:
    Mar 29, 2017
    Messages:
    10
    Likes Received:
    3
    I thought it was set up correctly, I attached my grbl settings. I can do the check size function and it traces the area where I want to cut. I have successfully used this setup with other CAM. It seems like an issued with Fusion settings.
     

    Attached Files:

  6. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Aug 6, 2013
    Messages:
    3,239
    Likes Received:
    1,815
    Then please post the Fusion file, and your Gcode file.
     
    Peter Van Der Walt likes this.
  7. SteamLabs

    SteamLabs New
    Builder

    Joined:
    Mar 29, 2017
    Messages:
    10
    Likes Received:
    3
    Here are my files.
     

    Attached Files:

  8. Peter Van Der Walt

    Peter Van Der Walt OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Mar 1, 2017
    Messages:
    13,751
    Likes Received:
    4,070
    What kind of spindle are you running on that? And how is the spindle cabling routed?

    Error 2? Ie Numeric value format is not valid or missing an expected value.
    EMI corrupting serial stream? See docs:blackbox:faq-emi [OpenBuilds Documentation] - particularly if the earlier question, results in the answer, a VFD spindle, or a router but with the power cable running adjacent to signal/low voltage cabling
     
    Alex Chambers likes this.
  9. SteamLabs

    SteamLabs New
    Builder

    Joined:
    Mar 29, 2017
    Messages:
    10
    Likes Received:
    3
    I mounted a dewalt 611 router, which is plugged into a relay switch that is controlled by the blackbox.
    Like I said, the machine works with gcode from other CAM systems, just not Fusion 360. I suspect a problem with my settings.

    I meant alarm, not alert as previously mentioned.
    “ALARM:2” : _(“G-code motion target exceeds machine travel. Machine position safely retained. Alarm may be unlocked.”),
     
  10. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Aug 6, 2013
    Messages:
    3,239
    Likes Received:
    1,815
    The gcode is operating in work coordinate system 2, or G55. So you need to setZero for material 0,0,0 with G55 active.

    G54 is the default, so maybe you should use that.
    In Fusion, go to Machining
    right click the 'setup2'
    select edit
    select the rightmost tab, 'post process'
    select WCS 1
    click OK

    upload_2021-7-8_7-59-11.png

    Now when the Gcode generates it will use WCS G54.


    Other things I see that need thinking about:
    Start heights are much higher than needed, wasting time cutting air
    There are no tabs, what is holding the part for the second operation?
    The 2Dcontour lead out collides with the outside stock, turn off the 'leadout' to prevent this.
    You may want to do that contour in 2 operations, a roughing cut with radial stock to leave (what you have now, but with stock to leave), then a finishing pass of full depth with 0 stock to leave at 75% feedrate.
    That object appears to have been scanned and has a lot of points so you may want to mess with Smoothing parameters to reduce the number of points in the Gcode.

    If you have not watched these, then do so now
    https://www.youtube.com/playlist?list=PL9tn9rGywKUW0K4_KIyCTKOFU8ELXzcnV
    the above at a minimum, then watch the rest at
    https://www.youtube.com/playlist?list=PL9tn9rGywKUUGyeBWX5Alt9yzBIp84sD8
     
    Peter Van Der Walt likes this.
  11. SteamLabs

    SteamLabs New
    Builder

    Joined:
    Mar 29, 2017
    Messages:
    10
    Likes Received:
    3
    I appreciate your detailed response.
    I certainly have not optimized the CAM, I wanted to get it working on my machine before spending time optimizing.
    For work holding, I planned on clamping the material, then making 3 holes, screwing those down to the spoil board, then unclamping, eliminating the need for tabs.
    I missed the lead out, thanks for catching that. Also fixed the helix ramp in height.
    I will add finishing passes once I get the basics working.

    This bracket was designed using generative design, turned on smoothing and left it at the default value for now.

    Thanks for your feedback, I will try G54.
     
    David the swarfer likes this.
  12. SteamLabs

    SteamLabs New
    Builder

    Joined:
    Mar 29, 2017
    Messages:
    10
    Likes Received:
    3
    Problem solved. Solution was to make a macro that set G54 to the current position.
    Managed to cut this out of wood as a proof of concept.

    Thanks everyone.
     

    Attached Files:

  13. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Aug 6, 2013
    Messages:
    3,239
    Likes Received:
    1,815
    But that is what the 'setzero' buttons do, and what they are for!
    1. Turn on machine
    2. run home cycle to establish 'hardware knows where home is'
    3. place material in position and fasten it
    4. jog to where 'material 0,0,0' is (what you set as the origin in Fusion) and click setZero for the relevant axes, usually XY and then Z separately for the top of the material. OR jog to where you can probe the corner and probe with the XYZprobe.
    XYZ Touch Probe Plus
     
    Peter Van Der Walt likes this.
  14. SteamLabs

    SteamLabs New
    Builder

    Joined:
    Mar 29, 2017
    Messages:
    10
    Likes Received:
    3
    For some reason my machine doesn't work when I do it that way, as I described in my first post.
    "I tried starting the program from home and from the top corner of the part, no change."
    I also tried "GOTOZERO" and the machine would try to jog past its limits.
     

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