584,805 active members*
5,350 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > Autodesk CAM > Im stuck please help!!!!
Results 1 to 18 of 18
  1. #1

    Im stuck please help!!!!

    Hi I am an event prop builder.

    Im new to the CNC and I’m building something new with it.

    My issue: my files look good in fusion 360 but in Mach 3 the first line is moving right on top of my stock. In other words. I zero the machine out and press cycle. The tool goes up starts spinning, lowers again and moves accross my material and damages the wood or break the bit. The procedure I want (which I would believe is normal) is that the tool goes up and across a few inches off the material and then lowers or ramps into the wood. Anyone?!?? Help?!?!?

  2. #2

    Re: Im stuck please help!!!!

    raise your feed plane in fusion

  3. #3
    Join Date
    Nov 2014
    Posts
    729

    Re: Im stuck please help!!!!

    Can you just raise the bit above the surface before starting the run? The first couple of months I ran my CNC I added a line in the code to do that automatically and then realized all I have to do is raise it with jog. It moves over to where it's supposed to start and then does what it should.

    I guess it could depend, too, on which post processor you're using...

    David
    David
    Romans 3:23
    Etsy shop opened 12/1/17 - CurlyWoodShop

  4. #4

    Re: Im stuck please help!!!!

    It’s not that... it’s currently 2 inch away from stock top. It’s really only the first movement and the last when returning to home.

  5. #5
    Quote Originally Posted by difalkner View Post
    Can you just raise the bit above the surface before starting the run? The first couple of months I ran my CNC I added a line in the code to do that automatically and then realized all I have to do is raise it with jog. It moves over to where it's supposed to start and then does what it should.

    I guess it could depend, too, on which post processor you're using...

    David
    Im using fusion 360.

  6. #6

    Re: Im stuck please help!!!!

    I called Industrial CNC, Where I bought my machine and they are saying to check my traverse or safe z. Anyone know where that is? or is it that.

  7. #7
    Join Date
    Mar 2003
    Posts
    35538

    Re: Im stuck please help!!!!

    Post a little bit of the g-code.
    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  8. #8

    Re: Im stuck please help!!!!

    (1001)
    (T12 D=0.25 CR=0. - ZMIN=-0.5 - FLAT END MILL)
    G90 G94 G91.1 G40 G49 G17
    G20
    G28 G91 Z0.
    G90

    (2D CONTOUR2)
    M5
    M9
    T12 M6
    S20000 M3
    G54
    M8
    G0 X0. Y-0.125
    G43 Z4. H12
    G1 Z3. F125.
    Z-0.1 F40.
    G2 X-0.125 Y0. I0. J0.125 F125.
    G1 Y4.
    G2 X0. Y4.125 I0.125 J0.
    G1 X4.
    G2 X4.125 Y4. I0. J-0.125
    G1 Y0.
    G2 X4. Y-0.125 I-0.125 J0.
    G1 X0.
    Z-0.2 F40.
    G2 X-0.125 Y0. I0. J0.125 F125.
    G1 Y4.
    G2 X0. Y4.125 I0.125 J0.
    G1 X4.
    G2 X4.125 Y4. I0. J-0.125
    G1 Y0.
    G2 X4. Y-0.125 I-0.125 J0.
    G1 X0.

  9. #9
    Join Date
    May 2005
    Posts
    1662

    Re: Im stuck please help!!!!

    Quote Originally Posted by FantasyDesigners View Post
    It’s not that... it’s currently 2 inch away from stock top. It’s really only the first movement and the last when returning to home.
    That seems to rule out a bad tool length offset
    G28 G91 Z0.
    and this probably repeats at the end of the program.
    That line is telling the machine to return to a Z reference position. Logically that would be Z HOME but that reference may not be HOME.
    This could happen due to a setting in machine parameters or the way the builder configured the machine.

    Try deleting that G28 line. Make sure to start in a safe position and starting in single block mode would not be a bad idea.

    edit/ I've usually seen that line as G91 G28 Z0 but I don't think it should matter
    Anyone who says "It only goes together one way" has no imagination.

  10. #10
    Join Date
    Nov 2014
    Posts
    729

    Re: Im stuck please help!!!!

    Quote Originally Posted by FantasyDesigners View Post
    Im using fusion 360.
    Yes, I know. Fusion 360 is the CAD/CAM program and it includes a post processor. But you have a choice as to which post processor you use. I'm using CNC Router Parts and the file generated doesn't do what yours is doing.

    Attachment 407646

    David
    David
    Romans 3:23
    Etsy shop opened 12/1/17 - CurlyWoodShop

  11. #11
    Join Date
    Jul 2016
    Posts
    660

    Re: Im stuck please help!!!!

    I tried running your code on a simulator, it seems like your Z axis travels too high and reaching the Z UP limit offsetting the Z position then goes back to the wood stock on an offset distance lower than the usual then over feeds the tool bit on the wood stock then it snaps the tool bit or sometimes if the offset is too big it will scrape the table.



    Try adjusting the clearance plane in 360, not too high, you can also loop it back to zero in 360 (but I dont know what setting it is in 360 because I honestly never used the software yet)

  12. #12
    Join Date
    May 2005
    Posts
    1662

    Re: Im stuck please help!!!!

    This thread came to mind while using fusion this evening. When posting code in Fusion there's an area in the window to change some
    of the post processor behaviour. For my post (not Mach3) G28 can be disabled, it's replaced by G53 which is a simpler code. It works
    fine as long as the machine doesn't have something weird like machine zero at the bottom of the Z travel.

    If the machine has an auto tool changer there could be more to consider. It's been years since I was lucky enough to have one.

    Simulators are good but unless it's part of the machine control it could be mistaken about where G28 has been set.
    And it is settable or at least it is on my machine.

    I could be wrong altogether about the problem but G28 is confusing and Fusion is pretty good at spotting collisions.
    That's all. Sorry for rattling on.
    Anyone who says "It only goes together one way" has no imagination.

  13. #13

    Re: Im stuck please help!!!!

    It Started doing it again Today!!!



    (NAME34)
    (T1 D=0.125 CR=0. - ZMIN=-0.25 - FLAT END MILL)
    G90 G94 G91.1 G40 G49 G17
    G20
    G28 G91 Z0.
    G90

    (2D CONTOUR2)
    M5
    M9
    T1 M6
    S18000 M3
    G54
    M8
    G0 X39.8969 Y55.3677
    G43 Z4. H1
    G1 Z2. F125.
    Z1.5 F41.7
    Z-0.2406
    G2 X39.915 Y55.3704 I0.0181 J-0.0598 F125.
    G1 X40.1815
    G2 X40.2383 Y55.334 I0. J-0.0625
    G1 X40.9287 Y53.8337
    Z-0.1506
    X41.0332 Y53.6066
    Z-0.2406 F41.7
    X42.4142 Y50.6058 F125.
    Z-0.1506
    X42.5188 Y50.3787
    Z-0.2406 F41.7
    X43.2091 Y48.8785 F125.
    G2 X43.1524 Y48.7899 I-0.0568 J-0.0261
    G1 X42.0717

  14. #14
    Join Date
    Jan 2007
    Posts
    24

    Re: Im stuck please help!!!!

    You need to run your machine in single block and dry run mode.
    In dry run mode you can control how fast axis will move.

    That way you can troubleshoot and find exact line in your code that is creating problem.

    Only when you verify that everything is working as intended then you can push that green btn and walk away.

    I think that there's an option in Mach3 to use MPG to slowly cycle through program and verify your tool approach and clearance.


    If you type in MDI Mode G28 G91 Z0
    Does your machine moves UP toward home position or down toward a table?

    If it goes down, then your reference point is not set properly.


    Sent from my LG-H872 using Tapatalk

  15. #15
    Join Date
    Jun 2012
    Posts
    108

    Re: Im stuck please help!!!!

    I think I know this. Go to post Process in Fusion 360 CAM , under Program Setting there is a list of stuff, scroll down to G28 and set to no. Every time I do a new part I have to set again.

  16. #16
    Join Date
    May 2005
    Posts
    1662

    Re: Im stuck please help!!!!

    Quote Originally Posted by crocnc View Post
    run your machine in single block and dry run mode.
    Yes or single block and rapid override.
    G90 G94 G91.1 G40 G49 G17
    G20
    this-->G28 G91 Z0. --> press once it does nothing, press again goes to machine Z home?
    G90
    (2D CONTOUR2)
    M5
    M9
    this--> T12 M6 --> does the machine have a tool changer ? If this was answered sorry for missing it.
    S20000 M3
    G54
    M8
    this--> G0 X0. Y-0.125 --> the gouge happens in this move ? If your clear of the part this shouldn't happen.
    G43 Z4. H12
    G1 Z3. F125.
    Z-0.1 F40.
    Anyone who says "It only goes together one way" has no imagination.

  17. #17
    MrSolution Guest

    Re: Im stuck please help!!!!

    Quote Originally Posted by FantasyDesigners View Post
    It Started doing it again Today!!!



    (NAME34)
    (T1 D=0.125 CR=0. - ZMIN=-0.25 - FLAT END MILL)
    G90 G94 G91.1 G40 G49 G17
    G20
    G28 G91 Z0.
    G90

    (2D CONTOUR2)
    M5
    M9
    T1 M6
    S18000 M3
    G54
    M8
    G0 X39.8969 Y55.3677
    G43 Z4. H1
    G1 Z2. F125.
    Z1.5 F41.7
    Z-0.2406
    G2 X39.915 Y55.3704 I0.0181 J-0.0598 F125.
    G1 X40.1815
    G2 X40.2383 Y55.334 I0. J-0.0625
    G1 X40.9287 Y53.8337
    Z-0.1506
    X41.0332 Y53.6066
    Z-0.2406 F41.7
    X42.4142 Y50.6058 F125.
    Z-0.1506
    X42.5188 Y50.3787
    Z-0.2406 F41.7
    X43.2091 Y48.8785 F125.
    G2 X43.1524 Y48.7899 I-0.0568 J-0.0261
    G1 X42.0717
    You are using metric or inch system ?

    Do you setup your tool lenght correctly ?

    Does your machine show G54-G59 work offset and machine offset ?

    When you home your spindle to machine Z0 ( G53 Z0 or G28 G91 Z0 and dont forget G90 in next line!! ) whats the height between top of the table and end of your spindle ? What's the height of your stock which is ready to be machined ? What's the tool lenght along with toolholder (from end of the spindle to the tooltip ?)

    How do you setup your machining Zero in fusion 360 ? Do you set it, in the same position on the machine ? ( on stock )

    Can you share your project for further advice ?

    Cheers

  18. #18
    Join Date
    Jan 2018
    Posts
    1516

    Re: Im stuck please help!!!!

    G28 G91 Z0.
    G28 will send the machine home (up) then Z will come back down to 0.
    If the machine home has gone out a bit for any reason it will crash

    I always delete this line now and replace it with a simple G0 Z0. Never had an issue since.
    Also I always set my Z0 height at 1mm above my stock.

    I find it good practice to G28 at the end of every day before switching off too.

Similar Threads

  1. X value stuck at 0.001
    By OCNC in forum NCPlot G-Code editor / backplotter
    Replies: 3
    Last Post: 02-16-2011, 12:42 AM
  2. stuck ram
    By RP Designs in forum Uncategorised MetalWorking Machines
    Replies: 3
    Last Post: 02-05-2010, 06:44 AM
  3. ATC stuck
    By guydrisc in forum Okuma
    Replies: 2
    Last Post: 11-22-2009, 12:14 AM
  4. Help! am Stuck!
    By ImanCarrot in forum Uncategorised CAM Discussion
    Replies: 6
    Last Post: 11-16-2007, 09:34 AM

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •