Probing Z height off of softjaw's surface - getting wrong height

CONTEXT
So as normal, I've performed all of the major operations on the first setup. Facing, drilling, milling, etc. All that I need to do is to flip the part and face off the backside to get it to size. To ensure I get the right height, I place the part in the soft jaws after having probed the top surface of the jaw. Once I place the part into the vice all cutting will occur in Z+. For this example, the facing operation will happen at +15. Z.

For context, the machine is a Haas VF-2 with the full WIPS system, in particular, the probe measuring the z offset is the Renishaw OMP40-2.


THE PROBLEM
The problem I seem to be having is that the part is coming out 0.2mm smaller. So instead of 15.00, it will range from anywhere from 14.75 to 14.94. My gut feeling is that I am placing the part in the vice and it's sitting some way above the jaws. Which doesn't seem to make sense as I do use a dead blow hammer to seat the part into the jaws.

The machine has just been fully calibrated using the ball bar cycle and both probes have been re-calibrated for height, concentricity, etc. The problem I am having as stated above was occurring before the recent calibration (performed by two different engineers) and afterwards so I'm not sure if its a calibration problem but more a mechanical problem. I have had this problem before on other parts however most of the time I've managed to set the offset to account for the difference.

At this stage, I'm not sure what else to try and I'm looking for any ideas/suggestions from someone with more experience/knowledge, I am more than happy to try and have a part waiting for its second op sitting on my desk so can try suggestions immediately.

Setup 1

Setup 2


Probing top of softjaw for second op


and Thank You in advance for any help.

This is a pretty easy fix. Its not your probe, its not your machine. Its your softjaws. The first mistake is that you are touching off with your probe on “top” of the soft jaw, or what should be “Z” zero in your program. You are correct that the 2nd op will be making contact with the z zero surface but when you put a load on your soft jaws to hold the part everything is shifting upward a few thou. In your case .008”. When you mill your soft-jaws you must have a spacer in between the two jaws with a load on the vise. For better accuracy use a torque wrench to tighten the vise with the spacers in between before milling them. After the jaws are to size keep the vise tight with the spacers still inside and then touch off with the probe to set your Z. When you go and actually load the part obviously take the spacers out in between the jaws and use the same torque you used you cut the jaws. You could take a couple of mic checks before you put the part in the machine and run a z measuring cycle to tap the top of the part after you tighten the vise to see if it give you the same reading as you got with your mics outside of the machine.

Another way to set your z is to touch off the top of the part at a known thickness. After the probe stores the G54 Z offset then simply input+ the negative value of the thickness of the part to bring G54 z to the bottom of the part.

Hope this helps!!

I'm guessing SpeedsandFeeds is right on the money. Use a torque wrench, clamp something in the jaws before you touch them off, and use that same torque value on your parts. The fixed jaw of your vise (which appears screwed down) is likely lifting as you clamp.

Another possibility is that the soft jaws were cut with a corner radius end mill, and extra material in the floor/wall transition on them is interfering with the edge of the part.

No way you're getting 0.2mm of lift due to vise tightening.
As mentioned its probably interference between the workpiece edge and the softjaw bottom face/wall transition. Make sure your parts have a nice chamfer or cut relief into the softjaws.

Honestly if I care about the height of a part on the first try I will manually face the top of the stock, set that as the Z home and then subtract my tool height and mic’d part thickness from that offset. That takes all the variables out of the offset as it’s taking the tool, the clamping and jaws/parallels into account.

I'm going to throw this out there as you said it happend on other parts and its a haas vf2.

Take and Indicator put it on the bottom part of your spindle with no tool in it. then push the tool release then let it go do this a few times and see if it moves mine moves .004 (inches not milimeters)
always goes back to zero at close and moves the exact same everytime at open.

only reason I say this is cause ive noticed my z0 on the probe to the tool is off sometimes. that being said I ran a 100 pc order and everything repeated with in .001 ran a 50 pc order next and one part was .003 off. then ran a 150 pcs order and 6 parts varied .003 this was in the last 4-6 months just every once in a while a part would move a few thousands from other parts.
I am sure its the spindle preload as I asked someone to check his machine and its dead nuts when hitting the tool release button as it should be.
it doesnt do it at tool changes with most tools which is odd nor does it do it all the time. heavy cuts or light cuts dont make a bit of difference you wont see any steps.
more than likely its your jaws and how there cut and wether you have a chamfer on the part to miss the corner.
the other thing is if you have a uneven spider when you cut your jaws or your jaws are uneven(canted when closed) and use a perfectly even spinder you will have problems as well.