Hello John,
In Fusion, if the three processes are all part of the same setup you can combine them in one file by clicking on each one on the Operations page of the NC Program page. They do have to be all using the same cutter in the free version of Fusion however. They do not have to be consecutive to each other.
To combine the three processes if they are not all part of the same setup you can combine them in one file by turning on each setup on the Operations page of the NC Program page and turning on just the processes you wish to make into one file.
You will get a warning message when you do this because it is up to you to make sure you won’t get a crash between the setups - if the stocks are at different heights and the tool is not lifting up enough between them or you are using different origins but you have not setup multiple origins on your machine for instance. But it will output the combined code.
To combine code from Fusion in an editor, open the first file in an editor and scroll to the bottom.
Then delete the last 2 lines. You want to make sure you cutter is ending that file on a lift to a safe clearance height - G53 G0 Z0 in this case. That way it is clear of everything to rapid to the next starting place.
Then open the next file in another instance of your editor:
And delete the first line - the % character.
If your file has a second line that starts with “O” - that is a capital o - then delete that line too.
But note the G54 on line N30. If the first file is G54 also then they will use the same physical origin on your machine table. If you don’t want that you need to make one of them G55 for example but you have to know how to setup multiple origins on your machine.
Now you can copy (CTL-A then CTL-C) and paste it to the end of the first file.
You will need to do the possess all over again at the end of that combined file and the third file to combine them.
From your original post I see you do want multiple origins. That’s a more involved topic. I will try to post something about it latter - maybe not till tomorrow.
But in the mean time here is some bedtime reading for you:
Work offsets (G54-G59)