Hi all, I am wanting to change the end of path HOME after the tool path is done running. Unfortunately, Fusion doesn't allow this change in the CAM page and wanted to see if anyone on here know where to change this at or the code to change it? I think this is the place line723 in my attachment??

What are you wanting to do at the end of the cutting path?

Hi Graham,

I would like to have the head go to a set machine # for a manual tool change if it is possible. Like y-90 & x-24.
I did omit the line #732 in that pic with // and now the gantry raises then stops. I could live with that if I had to but the tool path actually still shows that it is going back to its home position on the screen and do not feel real comfy with that.
Not sure why Fusion has removed this option in the Post window nor why MACH wouldn't give you this option. This is much easier in Aspire.

I don't think that is the correct bit in the code, that looks like the program end point.

Look/Search for writeBlock(mFormat.format(6) or something similar, this is the tool change code so your move is needed before this line.

The line to add will be something like:-

writeBlock("G50 X-24. Y-90.");

Darn Brother you are so close, but I do not see 6. Define home positions I would think would have this but its not formatted in a way that I understand. This is the code I was looking at and attached. You might not be able to open it but if you can line 1213 defines home? Does this look like I am heading the right direction?
Thank you for your assistance!!

Rufustoad,
Try this post that I made. 
It allows you to use G30 at the end instead of G28 for Safe Retracts.  It's a drop down in the post. 
You will have to set the positions you want inside the #vars.  Change #Var 5181 for X, #5182 for Y, and #5183 for Z.
These are the machine positions that you want the machine to go to when it is finished.  So be sure you populate these variables appropriately. 
For example, I don't want my Z to go all the way back to it's Home Zero Position, so I have variable #5183 set to -5.00 on a machine so it goes 5 inches below the home position.
Same for X and Y.
This post also allows you to use a G30 P2 for the tool change position; it uses this position before each tool change (even the first one).
#5351 X, #5352 Y, #5353 Z.
It is set up the same way; populate the appropriate #Vars with the machine position you want the machine to go to.

https://www.machsupport.com/forum/index.php?topic=46947.0
This is a helpful post as well.

Thank you so much Chad I appreciate it. I am not sure I understand what #Var 5181 for X, #5182 for Y, and #5183 for Z. is?? This does not exist when I open it in Fusion to edit the post?

It is inside Mach4.  Inside the "diagnostics" drop down then "regfile" then variables.  Set the range to include the all #5180 variables you need.
This is a setting for your machine.  Move the machine to the position you want the tool change and home positions to be.
Fill in the appropriate #Vars for the home positions to end the program at.  Then move the machine to the tool change position and fill in the appropriate #vars for the tool change. 

NOTE THESE ARE MACHINE POSITOINS.  These are not work positions... they are machine positions.   

Hey Boss, I want to make 100% sure I am in the right place before I change anything as I have never been here before. Does this look correct?

Yep. That’s it.