Fusion 360/Mach 3 Gcode program end code help

I'm new to Fusion, but had my mill and Mach 3 for many years. Still don't know 1/10tho LOL But I do not use tool offsets, nor do I use work offsets. All manual tool changes.
But Ive noticed with Fusion when I post my Gcode, if there is tool changes, the end code is different than what I have ever used. G28 sure, But giving it X0 y0 and G91? I always use abs coordinatres. Never Incremental... I've tried editing my machine, Putting in home switch locations etc. But after I run a program, and it ends. It set's me coordinates to something totally messed up...My Home switches are MAX -X and -Y But it seems to overrite them to 0. SO running next program everyhting is all messed. How do I get my NC prog to stop this end code?? Or what do I do to set properly Here is what all my progs end with now...

M9
G28 G91 Z0.
G90
G28 G91 X0. Y0.
G90
M30

Try this, set safe retracts to Clearance Height or G53

https://www.cnczone.com/forums/attac...d=445114&stc=1

If the property settings have a box Use G28 Yes/No change the option to No

But the post processor property settings are probably as Jim has shown, I could be remembering an older pp.

btw: I don't understand the reluctance to use work piece offsets. No real convenience gained in not using them but potential convenience lost imo.

Yes, Setting to safe retract does work. But what perplexes me is with the G28 move, why does it have a G91, then G90 ? That is the part that is messing up my offset I belive. I do like G28, as I have that in Mach 3 set to just before my home switches. I'm not fully understanding wjat it is going with the G90 G91 commands at the end Like I said, totally new to Fusion. I was using a simple 2D CAM up until a few days ago. SheetCAM was the prog

Cyclestart, my mill is a small desktop mill, I only run one part at a time. I use G54 Offset because I zero everything every time. Move things around on the bed to distribute the wear too. Also, cause I don;t really understand fully how to implement them maybe?

Obviously I am completely missing something with the G28

G28 is confusing you because it is a confusing command. The confusing part is it has an intermediate point in it's return to home (or other position defined by parameter). That intermediate point is relative to part xyz zero. If G90 is used with G28 z# you have to take into account the cutters current z position, otherwise the cutter may start moving in a direction not expected. If G91 is used with G28 Z0 the intermediate Z move will be no movement at all, followed by a return to z home. Why is there a G90 between the 2 G28 lines ? I don't know but I believe it does nothing useful or harmful. Clear as mud right ? That's why I avoid G28.
A better written explanation found in a blog:
Link --->https://cncphilosophy.com/g28-g-code-demystified/

re: work piece offsets
It reads like you are using an offset, specifically G54. If I'm guessing your work flow right....after touching off the part there should be offset entries for G54 wherever Mach3 stores that info. How G28 messes this up is a puzzler but I'm not a Mach3 user.

My codes always start:

G90 G94 G91.1 G40 G49 G17
G21
G28 G91 Z0.
G90

and end:

M9
G28 G91 Z0.
G0 X0. Y0.
M30

The G28 moves get on my wick and because I always G28 on morning startup and evening shutdown there is no point to it.
So I change the codes to:
Start:
G90 G94 G91.1 G40 G49 G17
G21
G0 Z30.
G90
(30mm is my safe Z height)

Then end:
M9
G0 Z120.
G0 X0. Y0.
M30

I have never had any problems at all.

If you feel up to it, you can always have a go at modifying your post process to change the code at the start and finish of the file to whatever you like. It's written in Javascript, if you have any capability there.

The post I use (for Centroid) now has the option to use G28 Z0, G28 Z0 Y0 Z0, G30 or nothing, IIRC. I choose to withdraw the spindle fully for safety at the end of any program. But as Jim points out, various options are available in the Mach 3 post pulldown.

Thx for the link. That clears it up a lot. Fusion is doing what I want it to do really. I think the issue I'm having is sometimes Homing the axis is not resetting the machine co-ordinates. It seems I have to home 2 or even 3 times before Mach resets to what I have set for machine Home. I have open loop steppers and been having some issues at times. Sometimes I'll have a issue, and X will be out like 8" or more. Home axis and its hit or miss, on weather it resets machine position. Haven't figured out why it's inconsistient. Working on that one..