Newb: Older 3+2 Haas setup- COR job setup, Z off -.01 cheat adj Question?

To be honest- the Son and I are newbs in 3+2 Totally self-taught, Youtube, PM forums and Other reading for these first debugging runs
98 Haas OS, Soldiworks w/ HSMWorks CAM. TRT style setup in 3+2 w/ Z tool orientation.
Issue; We come out too deep by -.01 on heights. And he say's it is only in heights on his part when it comes off? length and widths on the actual part seem to come out fine. Something we are just not getting....We're confused why its off on the tops of his part.

The kids measured his COR 2x. re-validated everything. regular 3 axis stuff comes out perfectly. Z is to a few tens. We're stymied where the error is being introduced but I think it's a bit of a few things.

So... I wanted tell the lad to just move the ZG54 .01 (Z-COR) up to compensate for the overcut? He thinks he should just move it in the CAM stl model.
Anywho... not sure if it matters which. He's moving it now for a test.

Ya'know.... I did ask him to make a test part, and try a few different cutters on Z. take a few cuts w/ 2 or 3 tools and see if it's consistent... updated- Several tested. same results...)

But.. since we're so new I wondered if anyone here might have a comment or two? or a suggestion. learning.... How to check precision on a 3_2 setup is something we're trying to learn here.

Enjoy , be safe, Take care.

The best way to set up a 5 axis is to have a single offset that corresponds to the XYZ at the center of rotation, and the A and B axis rotated to match the cad. (Disregarding Dynamic Work Offsets since you have an older machine)

The key is to have everything set-up accordingly in Solidworks. In other words, the XYZ origin is correctly placed in cad and the part is rotated the same as it is going to be in the machine.

Your son is correct that if you change the G54 Z by minus .100" you will mess up your cuts when the A axis (rotation axis parallel with X). Therefore, you will need to move the solid model down by .010" in order to fix the part. I would also take this time to examine why you had the issue. Keep in mind that the trunnion platter on Haas machines is rarely coincident with the center of rotation. For instance on the TRT100, the center of rotation is .8768 above the platter. Therefore, when I am modeling a job, I have a point that is modeled in .8768 above the platter that I can easily use to set my WCS. Generally, I set aside a couple of hours to pull the measurements and set my zero on any new trunnion. I might be stupid, but I always need to think it through.

1] Turn A to zero degrees and sweep in the platter with an indical until it is flat in respect to Z. This is your A zero.

2] Turn the platter to A 90 degrees and align that axis with the x axis. Tighten down the T-Bolts.

3] Turn the Platter to A-90 and confirm alignment. Touch off on platter. Rotate back to A90 and touch off again. The center of rotation is midway between these two points. 1/2 of that dimension is the distance between the platter and the center of rotation. This your Y0 position.

4] Rotate back to A0 and sweep in the center of the platter. [Your Y should be the same as you determined in the previous step... good check]. This location is your X0.

5] I then touch off the gage block that I use for setting tool heights (in my case it is 5 inches above the table). Then I touch off on the platter at A0. This PLUS (if the platter is below the center of rotation) the dimension I determined in step 3 (1/2 the distance between the two Y values with the platter rotated A90/ A-90) is my G54 Z Zero. This step where I really need to step back and sound out all the hard math to make sure that I am correct.

6] Rotate your B axis to whatever you want to suit your fixture.

This dimension needs to be spot on in your cad. In theory, your XYZ and A G54 will never change. Your B will only change if your fixture changes. Everything is controlled by your CAD.

G00 Proto nailed it...

Also I would take an endmill and spin a bore in the center of a block using only the C axis on that old machine. Then indicate the hole... This is XY Zero...

One thing to add - don't assume the Y-centerpoint for both A and B axes is the same. Ideally they should be, but actually might differ slightly. There is a setting on the control to account for this difference. I believe 254.

This difference could also be corrected for in your CAM software. (or post settings)