I got a reply from a machine company rep who said they don't normally recommend Gcode or programming, but he made a one-time exception and said to try this. It may take me a few days to work it into my schedule, but below is what was recommended. Like him, I'm not responsible for anyone who tries it and I plan to hand trip the toolsetter the first time to test it.
1. Set up your toolsetter on the table
2. Select a work offset coordinate system that you don’t plan on using for your part program, e.g. G58
3. Remove any tool from the spindle and type ‘0’ in the tool dro (this cancels TLO)
4. Remove the collet or tighten the drawbar to the point where the collet no longer protrudes past the spindle face. We will be touching the spindle face off on the toolsetter
5. Use the “Move and set work offset” button on the Z probe screen. This will move the spindle face down until it touches off on the top of the toolsetter, and set the G58 Z position to Zero right at the triggered position of the toolsetter
6. Then, in your g code program, use the following code (I’ll assume you’re in G54 and measuring tool 1 for this example):
a. G49 (Cancel TLO)
b. G58 (Switch to work offset G58)
c. G0 X--- Y--- (move the tool over the toolsetter)
d. G31 Z-10 F15 (probe tool down till it touches the toolsetter)
e. G10 L1 P1 Z#2002 (set the tool length offset value to the G58 Z position where the probe tripped)
f. G0 Z3 (move up to safe distance)
g. G54 (reapply old work offset coordinate system)
h. G43 H1 (apply new TLO for tool 1)