Changing G-Code Axis' ?

Results 1 to 12 of 12

Thread: Changing G-Code Axis' ?

  1. #1
    Member
    Join Date
    Jan 2017
    Location
    United States
    Posts
    13
    Downloads
    6
    Uploads
    0

    Lightbulb Changing G-Code Axis' ?

    Fellers, I know I ask a lot of dumb questions. But I learned long ago that if you don't ask the dumb question
    you will make DUMB Mistakes.
    I have G-Code for a project that has the material to be cut laying sideways on the table.
    X= 20 inches
    Y= 16 inches.
    My home made machine won't cut this like that.
    But I can cut Opposite that with X= 16 and Y= 20
    Is there anyway to change the G-Code for the size and direction of my machine?
    I sure appreciate your Expertise.
    Thank You,
    cubs

    Similar Threads:


  2. #2
    Member Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    3364
    Downloads
    0
    Uploads
    0

    Default Re: Changing G-Code Axis' ?

    I would rotate the part 90° in the CAM program, then repost the G-code

    Jim Dawson
    Sandy, Oregon, USA


  3. #3
    Member
    Join Date
    Jan 2017
    Location
    United States
    Posts
    13
    Downloads
    6
    Uploads
    0

    Default Re: Changing G-Code Axis' ?

    Thanks Jim,, Not sure if the Cam information is here. Will look. All I have see thus far is the Tap files.

    cubs



  4. #4
    Member Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    3364
    Downloads
    0
    Uploads
    0

    Default Re: Changing G-Code Axis' ?

    OH, you don't have the original drawing to work with? What CAM program do you normally use?

    Jim Dawson
    Sandy, Oregon, USA


  5. #5
    Member
    Join Date
    Jan 2017
    Location
    United States
    Posts
    13
    Downloads
    6
    Uploads
    0

    Default Re: Changing G-Code Axis' ?

    Jim the Only Cam I have is what came with Mach3 called Lazy Cam.
    But I looked and See CRV Files. I am downloading Corel Graphics to open them.
    They are probably the Cam Files for Vectric Carve.
    What Cam software do you use?

    cubs



  6. #6
    Member Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    3364
    Downloads
    0
    Uploads
    0

    Default Re: Changing G-Code Axis' ?

    I normally use Fusion 360 now, but I used to use CamBam for everything. I still use CamBam for quick jobs, very simple to use. CamBam does have a function that will save a .tap tool path to a dxf file. But that is the tool path rather than the drawing so the tool offsets would already be applied, a bit complicated to derive a rotated tool path from that. If you want to attach your .tap file, I'll see what I can do with it. Change the .tap extension to .txt to attach to a post.

    It would be possible to exchange your X and Y axis using the ports & pins in your Mach3 config screen, but this might require recalibrating the axes.

    Jim Dawson
    Sandy, Oregon, USA


  7. #7
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    33581
    Downloads
    0
    Uploads
    0

    Default Re: Changing G-Code Axis' ?

    You can use G68 to rotate the coordinate system 90°.

    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
    Member Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    3364
    Downloads
    0
    Uploads
    0

    Default Re: Changing G-Code Axis' ?

    Quote Originally Posted by ger21 View Post
    You can use G68 to rotate the coordinate system 90°.
    Thank you Gerry, I learned something new today.

    Jim Dawson
    Sandy, Oregon, USA


  9. #9
    Member
    Join Date
    Jan 2005
    Location
    USA
    Posts
    1860
    Downloads
    2
    Uploads
    0

    Default Re: Changing G-Code Axis' ?

    G68 is dependent on whether your control system supports it. In LinuxCNC the equivelant would be G10 L2 P1 R90 would rotate the G54 (P1) coordinate system by 90 degrees. P0 would be the currently active work coordinate system.

    Other controllers may not support any rotation at all and there are ways around this.

    You could go to your machine settings and change which pins control X and Y temporarily, or even save that config so you can go back and forth easily.

    I wrote a visual basic program once to do this for a particularly long program I didn't have the CAD/CAM for. As I recall, t replaced X with Y, and Y with X but then also had to change the sign on all the "new" y moves or the part was mirrored. That was a long time ago but that's what I remember.



  10. #10
    Member
    Join Date
    Jan 2005
    Location
    USA
    Posts
    9787
    Downloads
    0
    Uploads
    0

    Default Re: Changing G-Code Axis' ?

    Quote Originally Posted by ger21 View Post
    You can use G68 to rotate the coordinate system 90°.
    G68 by itself is not going to do much, you have to tell it what you want it to do, also some controls won't support a G68

    G68 X0 Y0 R90 ( this is the minimum that you will have to use X---- Y---- are your starting point )


    G69G80 (At the end of your program you need to add this line to cancel it )


    G68 is also incremental moves your program will have to match this G91

    Mactec54


  11. #11
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    33581
    Downloads
    0
    Uploads
    0

    Default Re: Changing G-Code Axis' ?

    G68 X0 Y0 R90 ( this is the minimum that you will have to use X---- Y---- are your starting point )
    He's using Mach3, where it's :
    G68 A0 B0 R90

    G69G80 (At the end of your program you need to add this line to cancel it )
    All you need is G69 in Mach3.

    G68 is also incremental moves your program will have to match this G91
    Not according to the Mach3 manual.

    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)


  12. #12
    Member
    Join Date
    Jan 2005
    Location
    USA
    Posts
    9787
    Downloads
    0
    Uploads
    0

    Default Re: Changing G-Code Axis' ?

    Quote Originally Posted by ger21 View Post
    He's using Mach3, where it's :
    G68 A0 B0 R90



    All you need is G69 in Mach3.



    Not according to the Mach3 manual.
    With Mach3 anything is possible

    A0 is normally used for 4th axes rotation

    In Mach4 they have changed it to work the correct way using X and Y

    Mactec54


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
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Changing G-Code Axis' ?

Changing G-Code Axis' ?