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.

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.

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

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.

Quote:

---

Originally Posted by mmoe

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...

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.