Cnc Programmer

You will need to modify the GOHOME command in the option file so it outputs a G28 instead of the G00.

I've not ever used the GOHOME command. It seems to be a very poorly documented command in any manuals or other information I've found over the years. I guess a valid question I'd have is why it's needed? Are you bringing the machine to the home position in preparation for a tool change? Are you just moving the tool out of the way prior to a program stop so the operator can check things? Or is this a "move to home" at the end of a program?

There are operations where I need the equivalent of a GOHOME where I have the post processor do the equivalent, but I make the motions part of the particular operation the machine is performing. My general post does such a thing for the following:

(1) At the beginning of the program. This was because we had an old machine that, if you didn't return it to home position before applying a fixture offset, would end up with erroneous positioning.

(2) Immediately before a tool change. This gets the tool changer and its swinging arm away from the part being machined, minimizing the danger of a collision as much as possible.

(3) At the end of the program. To get the tool away from the part and/or to bring the part being machined closest to the front of the machine.

For the machines I usually use, the things I'd need to output for a GOHOME are much more than a simple G28. The typical G-Code is something like:

G00
G49 G28 Z0.0000
G91
G28 X0.0000 Y0.0000
G90

These commands are telling the machine to:

G00 -> Switch to RAPID mode (if not already in that motion mode)

G49 -> Cancel any tool offset currently active

G28 Z0.0000 -> Move to the Z axis home position. We use 3-axis machines, so this will tend to move the tool into a "safe" Z location.

G91 -> Turn on relative motion mode.

G28 X0.0000 Y0.0000 -> Move the X and Y axes to their home position.

G90 -> Turn absolute positioning on.

You've got to know what your machine requires for the specific action you want to perform. For example, on some of our machines the "G49" causes program execution to fail, so it is omitted from code written for them.

As for doing this type of thing with the options generator, I don't see any way to "map" particular NCL commands to G codes and the like. To handle things of this nature I've had to edit the FIL code associated with the post-processor (under "Advanced" in the options generator). I think you'll have to look into doing this kind of thing if you want to handle GOHOME commands issued within your NC sequences/operations. It's not a simple process, but very much worth it if you want to be able generate reliable code without any manual editing.