Inspecting heigh difference in soft jaws using Renishaw - possible?

[Elemental_Garage]

Having a bit of a brain fart today and wanting a bit of help.

I made some soft-jaws for a horn button to engrave, however, I am finding that on the contoured horn top the engraving is hitting on the bottom part of the piece before the top piece. The bottom of the button will engrave at -.006 depth, and the top won't get touched until about -.018, and it's fairly progressive. At first I thought it might be the horn button, as I didn't make it, but I had the same results across two horn buttons so I'm pretty confident it's a "me," problem.

I'm trying to determine if my soft jaws are actually at the same Z height, and wondering if I can use my Renishaw to do that. I'm just not sure how to inspect/measure that using the probe.

Any help is appreciated!

 

[Elemental_Garage]

I think I figured out how to do it, though manually.

I set the Z height on the first soft jaw, then jogged the probe back to zero and recorded the machine absolute position.
Then I did the same on the second soft jaw, recorded that. They are about .0128 difference, which is nearly the exact difference I had to use to get the top to start engraving.

Now to figure out why . . .

These are on Orange vices.

 

[Elemental_Garage]

Cleaned out the higher jaw. Looked like there was one chip stuck in there and re-measured. They are now .0002 height difference.

I'm curious though if there is a way to automate this by just Z probing one surface, Z-probing another, and it giving me the difference in height.

 

[rjwalker1973]

Sure, you could always just probe to two different offsets that are not part of the program and set to z and compare the two offsets.

 

[Elemental_Garage]

Yeah good call. I was just curious if there were any measure macros people are aware of. I know I can input an expected measurement and then probe, and it'll give me the difference, but curious if it could give me the delta between two measurements without knowing the first, if that makes sense.

 

[mhajicek]

This is why I always cut my soft jaws in place, and never save them for reuse. It's about $15 for a set of 4" aluminum jaw blanks, and they can be decked off and reused a few times.

 

[Orange Vise]

Cleaned out the higher jaw. Looked like there was one chip stuck in there and re-measured. They are now .0002 height difference.

I'm curious though if there is a way to automate this by just Z probing one surface, Z-probing another, and it giving me the difference in height.

Yes, probe one surface and save to G58 and probe the second surface and save to G59.

Then use the associated macro variables to compare.

13 - Mill - Macros

www.haascnc.com

	#5301- #5306	G58 work offsets
	#5321- #5326	G59 work offsets

I wish they had a better table, but basically these are the macros for XYZABC.

So G58's Z is #5303 and G59's Z is #5323.

If they were to match perfectly, you'd compare:

IF[#5303 EQ #5323] ...

But since that's unlikely, you're looking for the difference to be within a specified tolerance, so do a subtraction and get the absolute value.

IF[ABS[#5303-#5323] LE .001] GOTO 1234; (Height difference is less than .001)
M30; (Stop)

N1234;
(Do things...)

I don't remember if Haas controls handle ABS. If they don't, just do a double comparison for pos or neg values:

IF[[#5303-#5323 LE .001] OR [#5303-#5323 GE -.001]] GOTO 1234; (Height difference is less than .001)
M30; (Stop)

N1234;
(Do things...)

 

[Chris59]

Sure, you could always just probe to two different offsets that are not part of the program and set to z and compare the two offsets.

Yeah, I've done that many times. I've also just put an indicator in and manualy measured it. I keep an indicator in a holder (not in the machine) so it;s quick.

 

[Elemental_Garage]

Thanks all, really appreciate the tips!

 

[chineshop_guy]

could also have used an indicator in the spindle. i often use the machine with an indicator in conjunction with the operator position screen like height gage

 

[File-Hard]

You can customize the "Timers and Counters" area in the lower right corner of the screen to display a variable, and give it a custom name. I'm not in front of the machine, and it's been years since I did it, so I can't be more specific. I do remember it's dead easy to do, though.

I have mine customized to show me a variable (again, I forget which one) which I have labelled "SIZE", for lack of a better word. This particular variable represents different things, depending on what I've just probed. Sometimes it represents something too obscure to be useful, I think. Anyway, read on...

For example, if I've run the "Single Surface" probing routine, it shows the relative change in the offset value. I use this for situations exactly like yours, and others, where I want an extra "idiot check" before pressing the green button. If I'm already probing stuff, it's faster than jogging around with an indicator.

If I've probed a bore, it shows the diameter. If I've probed a block or pocket, it shows the width. It's very handy. I often find myself measuring a block width with some calipers before probing. A quick glance at my custom variable after probing should agree with my quick caliper measurement. It gives me a warm, fuzzy feeling that the probing routine wasn't fouled by debris, etc.