584,833 active members*
5,509 visitors online*
Register for free
Login
IndustryArena Forum > CAD Software > Autodesk > G-code telling machine to go to "home" instead of custom zero point (Fusion 360 CAM)
Results 1 to 6 of 6
  1. #1
    Join Date
    Nov 2013
    Posts
    143

    G-code telling machine to go to "home" instead of custom zero point (Fusion 360 CAM)

    Hey guys,

    This might be an easy fix, but I exported G-code yesterday using Fusion 360 CAM, and the G-code works just fine. However, after the cut is finished, the machine is returning to it's "home" position (Ref All Home - Mach3) instead of the zero/zero point that I specified in Mach3.

    Basically, in Mach3 you can have a custom zero/zero point anywhere on the surface. The tool path that I programed yesterday exported the G-code just fine, but why is it telling the machine to return to "home" instead of my custom zero/zero point?

    Is there an easy fix for this?

    By the way, I'm using a CNC router.

  2. #2
    Join Date
    Nov 2013
    Posts
    143

    Re: G-code telling machine to go to "home" instead of custom zero point (Fusion 360 C

    Here's the last few lines of the G-code.

    It's using "G28", which apparently means that it's supposed to return to the machine's reference point. I thought the reference point was zero/zero and not "home", but I could be wrong.

    G1 X4.5 Z-0.2062
    G2 X4.5625 Y-0.5 Z-0.2063 R0.0625
    G1 Y-2.5 Z-0.21
    Y-4.5 F12.
    G2 X4.5 Y-4.5625 R0.0625
    G1 X0.5
    G2 X0.4375 Y-4.5 R0.0625
    G1 Y-0.5
    G2 X0.5 Y-0.4375 R0.0625
    G1 X4.5
    G2 X4.5625 Y-0.5 R0.0625
    G1 Y-2.5
    G0 Z0.6

    M9
    G28 G91 Z0.
    G28 X0. Y0.
    M30

    There are options in the post process where I can tell it not to use "G28", but I believe that would tell it to just stop right where the tool path stops, and that's not what I want. I need it to go back to the custom zero/zero that I set for myself in Mach3.

  3. #3
    Join Date
    Jul 2008
    Posts
    340

    Re: G-code telling machine to go to "home" instead of custom zero point (Fusion 360 C

    In Mach3 there is a configuration page that allows setting the machine coordinate for G28. It's either under the Homing or Safe Z settings. I have mine set to the same position as my tool height touch off plate used during tool changes.

    Sent from my Xoom using Tapatalk
    CRP-4848 CNC Router, CNC G0463 (Sieg X3) Mill, 9"x20" HF CNC Lathe (current project)

  4. #4
    Join Date
    Sep 2012
    Posts
    1195

    Re: G-code telling machine to go to "home" instead of custom zero point (Fusion 360 C

    If your Z axis homes to the top of the Z stroke, I think it's easiest to use G53 at the end of a program. G53 is machine coordinates, so basically the position that you home the machine to is 0,0,0. You can make the end of your code have any final position, but you want to do it using G53 so you aren't in your work coordinates. My end of program code goes:

    G53 G0 Z0
    G53 X0 Y0
    M30

    X0 Y0 in machine coordinates is the back right corner of my machine work area, so this creates the least obstruction for removing parts and adding material. Jog your machine to where you would prefer it stops, then check the machine coordinates in Mach 3 and note them down. Use those in place of X0, Y0 if those aren't where you want to end.

  5. #5
    Join Date
    Nov 2013
    Posts
    143

    Re: G-code telling machine to go to "home" instead of custom zero point (Fusion 360 C

    Quote Originally Posted by mmoe View Post
    If your Z axis homes to the top of the Z stroke, I think it's easiest to use G53 at the end of a program. G53 is machine coordinates, so basically the position that you home the machine to is 0,0,0. You can make the end of your code have any final position, but you want to do it using G53 so you aren't in your work coordinates. My end of program code goes:

    G53 G0 Z0
    G53 X0 Y0
    M30

    X0 Y0 in machine coordinates is the back right corner of my machine work area, so this creates the least obstruction for removing parts and adding material. Jog your machine to where you would prefer it stops, then check the machine coordinates in Mach 3 and note them down. Use those in place of X0, Y0 if those aren't where you want to end.
    EDIT: OK, I see now. G53 is just telling the machine to use the machine coordinates and not your own custom coordinates.

    I'm assuming that I'll have to edit the end of all my code from now on, if I plan to use this software...

  6. #6
    Join Date
    Mar 2003
    Posts
    35538

    Re: G-code telling machine to go to "home" instead of custom zero point (Fusion 360 C

    No, just edit the post. I just took a look at the post editor. If you look at the very end, you can see how it's doing the G28 home code. You should be able to just have it write your G53 commands.
    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)

Similar Threads

  1. X Axis "Goes Off Pattern", "Awry", "Skewed", "Travels"
    By DaDaDaddio in forum Laser Engraving / Cutting Machine General Topics
    Replies: 1
    Last Post: 05-06-2013, 09:59 AM
  2. Adding custom G-Code as a "Feature"
    By murchester2 in forum BobCad-Cam
    Replies: 11
    Last Post: 03-07-2013, 10:41 AM
  3. Replies: 12
    Last Post: 06-27-2012, 12:30 PM
  4. Post adds "A0." code and machine stops
    By lookingforhelp1 in forum Fanuc
    Replies: 10
    Last Post: 08-29-2008, 06:58 PM
  5. Post adds "A0." code and machine stops
    By lookingforhelp1 in forum Post Processors for MC
    Replies: 2
    Last Post: 08-29-2008, 06:14 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
  •