How can I force a g43 on new operation?

[mxdawg121]

I run several machines - many times I have an M00 programmed mid program to flip parts for other sides. 
ex

setup1

M00

setup2

M00

setup3

M00

ill shift click them all then post. Been doing it like this for a while, however 

None of my post force a g43 on a new operation (doesn’t change tools)

most of machines don’t care they run as they should. One of them is picky and needs a g43 after each m00. 

I’ve tried to modify a post to force a g43 on every initial zmove but can’t figure it out. 

anybody able to help?

[seth.madore]

You can put in an Manual NC of "Force Tool Change", which would send the machine to Z home and reinitialize the tool and height call. Put this in between operations.

 What post processor are you using, and would you have a sample file you can share?

[mxdawg121]

That is a great solution.

 I'd prefer to have it always post a g43 whenever theres a new operation. Our mastercam always post a g43 - im tyring to make everything uniform if possible.

[seth.madore]

What's your post processor and do you have a sample part you could share? (saves me from having to reinvent the wheel).

If you are working with a post processor that you're already fiddling around with, please share that here as well

[mxdawg121]

Yes, of course i'd love to share. I have a few changes to this post, mostly QOL changes. 

[seth.madore]

Easiest thing to do is already in your post, it's called "Safe Start All Operations". This will spit out this:

N1005 (Bore2)
(1/4 Endmill)
N1010 G90
N1015 G53 G0 Z0.
/ N1020 T2 M6 G90
/ N1025 S6500 M3
/ N1030 G54
/ N1035 M8
N1040 G1 X2.3022 Y-0.5452 F650.
N1045 G0 G43 Z0.6 H2

Now, you might want to remove the "/" in front of each line, but that's an easy post edit.

[seth.madore]

 

[mxdawg121]

Im aware of this, when i use this feature - our campro mill goes up to toolchange location, turns the spindle off and back on really quick and it sounds quite unhealthy.

[seth.madore]

Alright, here's what you want to do:

Towards the end of the "onSection", replace this:

   if (xyzFormat.getResultingValue(getCurrentPosition().z) < xyzFormat.getResultingValue(initialPosition.z)) {
      writeBlock(gMotionModal.format(0), zOutput.format(initialPosition.z));
      zIsOutput = true;
    }

With this:

   zOutput.reset();
    writeBlock(
      gMotionModal.format(0),
      conditional(!currentSection.isMultiAxis() || !operationSupportsTCP, gFormat.format(43)),
      conditional(currentSection.isMultiAxis() && operationSupportsTCP, gFormat.format(234)),
      zOutput.format(initialPosition.z),
      hFormat.format(tool.lengthOffset)
    );

I've tested this in your file and it looks like it's doing exactly what you'd like:

N2150 G90 G0 G54 X15.
N2155 G91 G28 Y0
N2160 M00
N2165 (ROTATE)

N2170 (Bore3)
(1/4 Endmill)
N2175 G90
N2180 G0 G43 Z0.6 H2
N2185 G1 X1.865 Y-1.1688 F650.
N2190 G0 Z0.11
N2195 G1 Z0.055 F60.

[mxdawg121]

That does work, i just have concern of the z move before the x and y. Is it possible to add a button to the post preference screen that "Force Tool change all operations" like the safe start - without all the spindle business