Welcome to Our Community

Some features disabled for guests. Register Today.

f360/ob control

Discussion in 'CAM' started by baum, Jan 16, 2020.

  1. baum

    baum New
    Builder

    Joined:
    Nov 26, 2018
    Messages:
    55
    Likes Received:
    7
    Help..

    I Im just trying to draw the attached pic with a marker on my home brew using openbuilds control and a black box. Im using f360 to program.

    I did what i thought was a basic 2d countour around the outside and each letter. I zero my machine and from my WCS to the first "cut" point it lowers the z by a few MM. Then goes back to zero at that first cut point
     

    Attached Files:

  2. Peter Van Der Walt

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

    Joined:
    Mar 1, 2017
    Messages:
    13,753
    Likes Received:
    4,070
  3. baum

    baum New
    Builder

    Joined:
    Nov 26, 2018
    Messages:
    55
    Likes Received:
    7
    I did use that post. How do I check the g53?
     
  4. Peter Van Der Walt

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

    Joined:
    Mar 1, 2017
    Messages:
    13,753
    Likes Received:
    4,070
    @David the swarfer 's area of expertise :)
     
    Alex Chambers likes this.
  5. Alex Chambers

    Alex Chambers Master
    Moderator Builder

    Joined:
    Nov 1, 2018
    Messages:
    2,681
    Likes Received:
    1,321
    Have a look at your g-code in notepad. Post it here if you want one of us to look at it. As @Peter Van Der Walt said David is an expert on this.
    Alex
     
  6. baum

    baum New
    Builder

    Joined:
    Nov 26, 2018
    Messages:
    55
    Likes Received:
    7
    Here is the txt file
     

    Attached Files:

    • 3.txt
      File size:
      71.9 KB
      Views:
      13
  7. baum

    baum New
    Builder

    Joined:
    Nov 26, 2018
    Messages:
    55
    Likes Received:
    7
    Curre
    Currently i do not have any homing switches. I go to the corner of my "piece" hit the setzero button.
     
  8. baum

    baum New
    Builder

    Joined:
    Nov 26, 2018
    Messages:
    55
    Likes Received:
    7
    So if i use the standard gbrl post in f360 with G28 "yes" It does what i want, however it does ob controller does give an error for the t1 m6 line.

    Also at the end of the program it sends my machine off into space..
     
  9. 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
    firstly can we assume you do not have homing switches?

    in this case you need to 'fake the home' so that the machine conforms to industry standards (for safety! and convenience).
    machine home is where GRBL (the blackbox) turns on or is reset. it will reset when the GUI connects.

    given axis motion like this
    workbee_1510-axis-directions.png
    Home is at the positive ends of axis travel. This is absolutely VITAL in the case of the Z. every bit of Gcode generating software assumes that machine Z=0 is high up away from the work and clamps etc.

    So, how to do a fake home?
    1. Turn it all on
    2. Jog Z high, till it just misses the end of travel.
    3. Jog X and Y to their + ends of travel.
    4. Reset GRBL : disconnect and reconnect the GUI, or press the reset button on the Blackbox.
    From now on, this is machine home, never ever do any work unless this has been set correctly. There are many benefits, one of them being that Fusions Gcode works correctly (and so does all other Gcode).

    But now, how to get this set every time we use the machine?
    Create a macro with this code
    Code:
    G21 G90 G17
    G53 G0 Z0
    G53 G0 X0 Y0
    
    and label it 'goto MCS'
    mcs.png

    Before turning off the machine, click this macro button. The machine will safely raise Z then go to home.
    Now when you power up machine home is already set AND it still remembers the last work co-ordinates you used, BONUS!
    I do many jobs over several days with many power cycles and never lose position and all I have to remember is to click the MCS macro button before I power down..

    So, Fusion settings..... (for the OB post)
    When you are posting there are a bunch of options in the dialog, each one of them has popup help, go read them all now.

    So now with that background , you may want to turn on 'Use machine coordinates at end'. I turn it on for large jobs, but find it easier just to jog out of the way for small jobs.
    You want to adjust the 'end of job' values from -10 to 0, your machine can go right to 0 without hitting a switch.
    f360-b.png
    in the image above you can see the values I have changed highlighted in blue.
     
    #9 David the swarfer, Jan 17, 2020
    Last edited: Jan 17, 2020
  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
    and now for those who desperately want to use the Fusion default GRBL post:
    You still need to create a fake home with a safe Z at HIGH AS POSSIBLE no matter what post or post options you use.

    Set the options highlighted in blue to the values shown:

    f360-c.png

    You can see I have left 'G28 safe retracts' at 'yes'.
    GRBL defaults to having G28 position as 0,0,0
    Therefore the G28 G91 Z0 that this post uses is equivalent to G53 G0 Z0 that the OB post uses and is a SAFE move if you have a good (fake) machine home. (If you change the G28 position and your new position has an unsafe low Z height then please use the other post)

    If you set it to no then YOU have to ALWAYS ensure that Z is retracted before you start a job. ALWAYS!
    You don't know where it is going to move to, so Z has to be at a safe height, every time.
    I garrantee you will break at least one bit before you realize that using the automation is a better choice (-:

    You can of course set the high feedrate to whatever your machines maximum speed is.
    The tolerance can also be changed, the default of 0.001 is so small that it only increases processing time. On my OX I set this to 0.025mm because that is the smallest step for X and Y, no sense having a smaller number if the machine cannot actually do that precision.
     
  11. baum

    baum New
    Builder

    Joined:
    Nov 26, 2018
    Messages:
    55
    Likes Received:
    7
    Thanks for this post! i will give it a shot this afternoon when i get home from work (im in the usa).

    how do i create the macro? is there a tutorial?
     
  12. 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
    here it is:
    open openbuildsCONTROL
    click the 'macro' tab
    click the 'add macro' button
    fill in the fields (only need the name and the macro itself)
    click 'apply'

    now test it with your hand on the emergency stop (-:
     
    Peter Van Der Walt and baum like this.
  13. baum

    baum New
    Builder

    Joined:
    Nov 26, 2018
    Messages:
    55
    Likes Received:
    7
    Your guys are the best! thanks
     

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