Welcome to Our Community

Some features disabled for guests. Register Today.

OpenBuilds CAM Software

Discussion in 'CAM' started by Mark Carew, Oct 8, 2018.

  1. phil from seattle

    phil from seattle Well-Known
    Builder

    Joined:
    Mar 17, 2017
    Messages:
    110
    Likes Received:
    36
    Yeah, I knew the SVG needed reworking to be used to create gcode but my point was that OBCam shouldn't hang on it.
     
  2. Peter Van Der Walt

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

    Joined:
    Mar 1, 2017
    Messages:
    1,916
    Likes Received:
    994
    Calculating toolpath offsets is quite a lor of maths that needs good data to work from. With bad data (ie files that are not toolpath friendly, has missing indexes, odd points etc) it has to work extremely hard to try and figure it out. Internally we use Clipper (just like many other applications like Slic3r, vectric, easel, lw4, jscut and many more does under the bonnet)

    The paid applications uses propriety code to "fix" broken files but you wont be seeing much of that in "Free / entry level applications"
     
  3. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    1,299
    Likes Received:
    655
    and I thought Sketchup was the only one to produce sequences of arcs with reversed endpoints (-:
    The solution in sketchup is to use the BZ tools plugin to 'create polyline' which reorients all the segment directions.
    You only need to do this when the 'phlatten' tool fails to create a clean outline.
     
    Peter Van Der Walt likes this.
  4. Peter Van Der Walt

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

    Joined:
    Mar 1, 2017
    Messages:
    1,916
    Likes Received:
    994
    Oh no, soooo many applications do that! Someday when I get a couple days to work on it, Clipper has some tools to helps with that but any new layer introduced adds complexity that needs a lot of testing :)
     
  5. RaphK

    RaphK New
    Builder

    Joined:
    Sep 10, 2019
    Messages:
    3
    Likes Received:
    1
    Hello

    I'm trying to generate a gcode for cutting with an acro 1515, blackbox controller and 10w endurance laser.

    One point I don't get is that even if I choose "laser operations vector" , the generated gcode does not turn on laser on/off for each path: it turns it on once at the start and off after all paths are processed.
    I need it to turn on before each path and turn off when moving between paths (G0 moving).
    On top of that, how do I get rid of Z Safe Height? setting it to 0 does not work.

    I attached the openbuildscam gcode and an example of what I'd like.
    Could someone please help ?
     

    Attached Files:

  6. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    1,299
    Likes Received:
    655
  7. Peter Van Der Walt

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

    Joined:
    Mar 1, 2017
    Messages:
    1,916
    Likes Received:
    994
    Did you setup Grbl Laser Mode properly : $32=1 most important one to set.
    Read gnea/grbl for full details

    Re the Safe Height, will check and fix soon, for now 0.001 should work
     
  8. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    1,299
    Likes Received:
    655
    what he means is that all Z moves should be replaced by M3/M5 but the file only has a starting M3 and an ending M5, as for a router. I tried it myself and that is what I got, Z moves and M3/M5 as for a router.

    The above is required if $32=0 else you get laser cut lines between objects in the job.

    When $32=1 then G0 moves will turn the laser off which achieves the same thing as a M3/M5 per block.

    I see that the gcode contains extraneous F and S words, which is something that can contribute to streaming errors for short line segments since each line is much longer that it really needs to be and GRBL has to work harder to process each line (same with the trailing zeros which should be trimmed).
    so
    Code:
    ; GCODE Generated by cam.openbuilds.com on 2019-09-10
    G21 ; mm-mode
    G21 G90 G17 F1000 M3
    ; Operation 0: Laser: Vector (no path offset)
    ; Tool Diameter: 20
    
    G0 Z0
    G0 F1000 X0.0000 Y50.0000
    
    G0 Z0
    G1 F600 Z-0.1000
    G1 F800 X100.0000 Y50.0000 Z-0.1000 S760
    G1 F800 X100.0000 Y0.0000 Z-0.1000 S760
    G1 F800 X0.0000 Y0.0000 Z-0.1000 S760
    G1 F800 X0.0000 Y0.0000 Z-0.1000 S760
    G1 F800 X0.0000 Y50.0000 Z-0.1000 S760
    ; retracting back to z-safe
    G0 Z0
    
    M5
    G53 G0 Z0
    G0 X0 0
    M30
    
    should be
    Code:
    ; GCODE Generated by cam.openbuilds.com on 2019-09-10
    G21 ; mm-mode
    G21 G90 G17
    ; Operation 0: Laser: Vector (no path offset)
    ; Tool Diameter: 20
    
    G0 Z0
    G0 X0.0 Y50.0
    M3 S1   ; move this here, where it was it caused a 100% power flash before the job starts
    G1 Z-0.1 S760 F600
    G1 X100.0 Y50.0
    G1 X100.0 Y0.0
    G1 X0.0 Y0.0
    G1 X0.0 Y50.0
    ; retracting back to z-safe
    G0 Z0
    
    M5
    G53 G0 Z0
    G0 X0 0
    M30
    
    is there a howto somewhere for setting a dev environment? maybe I can fix some of this for you.
     
    #98 David the swarfer, Sep 10, 2019
    Last edited: Sep 10, 2019
  9. Peter Van Der Walt

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

    Joined:
    Mar 1, 2017
    Messages:
    1,916
    Likes Received:
    994
    note its for a Laser...
    :) Check the Grbl Wiki gnea/grbl (Laser Mode page): laser Mode in grbl works like this:
    M3 or M4 at the start of the Job enables the laser (you kind want M4 though as it adapts power as a function of acceleration which looks better)
    Then G0 moves are laser-off
    G1/2/3 moves are Laser On
    M5 at the end disables it.
    In particular gnea/grbl - we use the second suggestion (G0 to disable) as its better standard

    As G0 vs G1/2/3 is the ON/OFF you dont want M3/5 between entities, thats long gone Grbl 0.9 way of doing things. Grbl 1.1's been with us since 2016 hehe with this way... People just sometimes forget to set $32=1; Laser Mode (its in our Machine profiles so I assume user forgot to load ours)

    We are up to spec on that man (; - is SketchuCam? :p

    I do agree taking out Z moves for laser, seperate issue, like i said - have to investigate why thats back - took it out a couple months ago but we did go through a heavy rewrite to move the CAM ops to webworkers to speed things up so it mustve jumped back in. Remove Z moves from laser operations · Issue #55 · OpenBuilds/OpenBuilds-CAM
     
    #99 Peter Van Der Walt, Sep 10, 2019
    Last edited: Sep 10, 2019
  10. Peter Van Der Walt

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

    Joined:
    Mar 1, 2017
    Messages:
    1,916
    Likes Received:
    994
    PS @RaphK you should also check, CAM -> Settings -> Select the Acro profile (it sets M4 instead of M3)
    Your file shows S250. Is this a 25% burn (default grbl settings has S1000 = max power)
     
  11. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    1,299
    Likes Received:
    655
    quite, I was editing my post after clicking post a bit too soon...
    not perfectly, but well within usefulness (-: SketchUcam generates an M3/4 and M5 pair for every (what would have been a ) Z move. This does work correctly with GRBL as far as I can tell, guess I need to push 'install laser' to the front of the long list of things to do.
    Here is a sample output from SketchUcam
    Code:
    %
    (Generated by SketchUcam V1.5-58fdf15)
    (Bit diameter: 3.0mm)
    (Feed rate: 2000.0mm/min)
    (Plunge Feed rate: 1000.0mm/min)
    (Material Thickness: 6.0mm)
    (Material length: 790.0mm X width: 550.0mm)
    (Overhead Gantry: true = Conventional Cut)
    (Plunge Diam First)
    (Optimization is ON)
    (LASER for GRBL PWR)
    (Origin offset ~ 9.0mm, ~ 11.1mm)
    (www.PhlatBoyz.com)
    G90 G21 G49 G17 F1000
    G00 X0 Y0
    M05
    G00 X0.000 Y0.000
    M04 S30000
    G01 X100.000 F2000
    G01 Y50.000
    G01 X0.000
    G01 Y0.000
    M05
    G00 X9.387 Y74.671
    M04 S31500
    G01 X42.806 F2000
    G01 Y96.471
    G01 X9.387
    G01 Y74.671
    M05
    G00 X0 Y0 (home)
    M05
    M05
    M30
    %
    
     
  12. Peter Van Der Walt

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

    Joined:
    Mar 1, 2017
    Messages:
    1,916
    Likes Received:
    994
    ahh man, edited posts suck (; as my reply now doesnt address the first wrong reply lol!


    in short form yes... except! M3/5 stops motion. Start/ends of burns will have crisp little spots. Fine for cuts, sucks for engravings. Grbl Laser Mode is awesome and see no reason to recommend hacking around a perfect solution


    Which is your old and still open issue Todo: Optimise G-Code Generator: Don't repeat F/S commands unless changed, also remove modal commands that repeated) · Issue #9 · OpenBuilds/OpenBuilds-CAM :) Priorities! :) (see Build software better, together )
     
    David the swarfer likes this.
  13. RaphK

    RaphK New
    Builder

    Joined:
    Sep 10, 2019
    Messages:
    3
    Likes Received:
    1
    Hi, thanks all for your replies!
    I try to digest all this, I'm just a newbie...

    by the way, I found a gcode optimiser (optimizing the traveling salesman problem for G0) that seems promising, do I open a ticket on github for integrating it on openbuildscam?
    https://xyzbots.com:4000/gcode-optimizer/
     

    Attached Files:

  14. Peter Van Der Walt

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

    Joined:
    Mar 1, 2017
    Messages:
    1,916
    Likes Received:
    994
    Unfortunately in the real world its not so good. It changes order of pocket operations and all other kinds of messes. Played with it a lot, its was coded by a former devpartner of mine (;
    Works well on "certain" files but that eliminates it from integration. It has to be very clever and work on everything. There are better ways of solving it than that... Way better. Post processing gcode, why, when we have the raw data to work with.

    OpenBuildsCAM is low priority though, most code time is spent in CONTROL. Majority of users go for Fusion or Vectric for CAM. OpenBuildsCAM fills that bottom end of free and kinda easy to get you started but we really hope you move on to better as your skills grow

    Too busy making even more awesome stuff, but hey when it slows down, there's still a lot of work to be done on CAM (see git for just some of whats on the todo)
     
    #104 Peter Van Der Walt, Sep 10, 2019
    Last edited: Sep 10, 2019
  15. RaphK

    RaphK New
    Builder

    Joined:
    Sep 10, 2019
    Messages:
    3
    Likes Received:
    1
    Hello

    after some cuts, all is perfectly working as per Peter Van Der Walt and David the swarfer said:
    set $32=1; Laser Mode
    G0 moves are laser-off
    G1/2/3 moves are Laser On
    no need for M3/M5 between entities

    Thanks all for your help!

    By the way, if someone is aware of an illustrator plugin to export gcode to blackbox, please let me know.
    At the moment, I'm trying to modify Diego Monzon's illustrator2gcode panel.
    So far, I modified the G0 instead of G1 setting but there is still a scale issue.
     
    sharmstr likes this.
  16. Cortellini

    Builder

    Joined:
    Jul 11, 2015
    Messages:
    17
    Likes Received:
    23
    Hello Peter,
    I have gotten the machine working and am now addressing GCODE.
    I have looked at several documents that explain gcode and am now
    ready to proceed to the next step.

    Just so you know, when I press the cam.openbuilds.com link at the bottom of
    OpenBuilds CAM page, I receive a 404 Error.
    But when I copy the link and paste in the browser, it takes me to the correct CAM page.

    I am intending to use the Workbee 1510 as a drag-knife. In configuring the Gcode generator,
    drag-knife is does not appear as a tool option. The closest option seems to be the "Plotter Pen" option.
    Will this work?
     
  17. Peter Van Der Walt

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

    Joined:
    Mar 1, 2017
    Messages:
    1,916
    Likes Received:
    994
    Thank you will let the store team know about the link


    In the Setting tab, there is no "tool" for Dragknives as they dont require any interface, no startup commands, etc. Its not a powered tool. They just sit at the end of the z axis and are controller by the z axis

    Everything else happens in the toolpath setup

    drag knife.png
     
    #107 Peter Van Der Walt, Sep 19, 2019
    Last edited: Sep 19, 2019
    sharmstr likes this.
  18. Cortellini

    Builder

    Joined:
    Jul 11, 2015
    Messages:
    17
    Likes Received:
    23
    Thank you for the help.

    I have not as yet discovered how to increase the F (speed) value in the code generator.
    Is the speed limit a function of the machine capability? Is the 1000 value the highest I can expect of the Worbee 1510?
     
  19. Peter Van Der Walt

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

    Joined:
    Mar 1, 2017
    Messages:
    1,916
    Likes Received:
    994
    When you create a toolpath, is when you set feeds. Workbee with belt drive can do over 5000mm/min
     
  20. Cortellini

    Builder

    Joined:
    Jul 11, 2015
    Messages:
    17
    Likes Received:
    23
    Thanks you Peter
     
    Peter Van Der Walt likes this.

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