VF-6 single surface probe setting
Have a brand new Haas VF-6 with probing. Am running castings that I am using the work probe to touch off and set Z axis zero. Problem is that I want to remove .025" from casting and have that be my Z = 0. I can't figure out a way to have touch off with Renishaw work probe NOT be zero but be +.025 Our brute force solution was to just do a quick operation to adjust the preset G54 by summing macro variable for G54 Z value with -.025 to move the G54 work offset down .025". This caused an unanticipated problem with running the mill with "program restart" enabled. Now any time you exit and restart program it does the math operation again and lowers the G54 by .025" NOT a good thing. We can't figure out what variable the probe touch in Z is stored in so we can do the math operation on that variable and not the stored G54. Also does that variable stay fixed until the next probing function? Playing around with the part zero setting options I see nothing that allows for presetting to values other than zero. Any help appreciated!
Re: VF-6 single surface probe setting
Based on a 2007 VF-2ss with Renishaw probing:
G65 P9811 Z.025 S1 should work.
Never put math in a program that you do not want done every cycle!
Probing Z sets #187, but do not use #187 directly. After probing, do #500 = #187 or whatever variable you want. More reliable this way.
Re: VF-6 single surface probe setting
Yeah Matt has it right. Just remember that it's opposite from what you might think. The Z.025 is telling the probe where it is. So it is .025 above zero. Z-.025 would be...well you get it. I use this all the time, usually just .001 or less. We use S54. instead of S1. Haven't tried S1. Does that go to G54?
Re: VF-6 single surface probe setting
I appreciate the feedback. I'll try your recommendations when I can interrupt production. Here is the code we have currently.
G65 P9995 W54.000 A20.000 H-.2000 followed by the Z shift with G10 G91 L2 P1 Z-.025
The P9995 is from the built in Haas probing cycle. We never tried the P9811 and will attempt that. I'll get back on this with results after trying it.
Re: VF-6 single surface probe setting
Crap. I was only looking at the Z. I'm sorry. Our built in codes has :
G65 P9832 (TURN PROBE ON)
G65 P9810 X__ Y__Z__F50 (PROTECTED MOVE TO ABOVE PART)
G65 P9023 A9. S54. Z.025 (PROBE Z SURFACE PUTTING Z.025 BELOW PROBED SURFACE)
Re: VF-6 single surface probe setting
Quote:
Originally Posted by
extanker59
Haven't tried S1. Does that go to G54?
Yessir. S1. is how the Renishaw manual says to do it. I'm glad S54 works for you, less confusing. I'm used to being confused though... "G54" at the machine, "S1." in the macro call and "Work Offset 0" in Mastercam all do the same thing. :rolleyes:
Quote:
Originally Posted by
smithtec
I appreciate the feedback. I'll try your recommendations when I can interrupt production. Here is the code we have currently.
G65 P9995 W54.000 A20.000 H-.2000 followed by the Z shift with G10 G91 L2 P1 Z-.025
The P9995 is from the built in Haas probing cycle. We never tried the P9811 and will attempt that. I'll get back on this with results after trying it.
The built in macros are different than the macros you're supposed to use when programming probe cycles within an actual part program. No idea why, but in my experience it is definitely best to use the macros in the Renishaw manual. Email me at matt (at) rfrcustomfab (dot) com and I'll send you the Renishaw manuals I have. They are from 2004, so programmer beware. You can get them from Renishaw directly as well, I believe.
The trailing zeros in your macro call make me nervous, but are apparently working. Macros can be funny, and very picky some times.
Look in to G52 instead of G10. It is MUCH more straight forward to use. There are posts here and at practical machinist on the subject. G52 Z-.025 would do exactly what you are needing if you want to implement that until you get your probing dialed. Call it at every tool change. It is an absolute number, so calling G52 Z-.025 three times in a row still results in Z-.025. G52 Z0. to cancel.
Re: VF-6 single surface probe setting
I was able to find the Renishaw manual on Haas' website. I also found a dump of the 9000 series macros here in our shop. Looks like the Haas 9995 just uses the 9811 we all are used to in our other older machines. Just kind of buries it in a "one size fits all" 9995 macro. Still waiting on machine time to prove all this out. Big thanks for all the advice!
Re: VF-6 single surface probe setting
The Haas IPS (offsets screen) uses o9995 as the branching program, whereas the Haas VQC use o9023 as the branching program, but yeah they're simply used to call the individual probe subroutines in the background. Just multiple ways to perform the same outcome.
The purpose of the 9995 and 9023 are to string multiple probe cycles together (probe center of rectangular block, etc) but they also include the probe activation codes and also set target probing locations based on the probe's current position which is calculated in absolute coordinates.
Ultimately we're free to write our own specific cycles to call the native Renishaw routines, but there's occasionally some redundancy if you end up activating the probe more than once or whatever. The hardest part is testing for crashes, which is why the o9810 program is invaluable.
Re: VF-6 single surface probe setting
Here's an update. I have been able to get the probe to do all the things necessary using Renishaw macros and have solved my initial problem. Now here's a new related one. When running a probe inspection routine I can't find where the Haas VF-6 writes the probed data. On our Fanuc mills it's typically around Setting #138 or so and we can look at the value from probed diameter (for instance) and follow tool wear, etc. Here's our example of checking a 5.226 +/- .003 inch diameter bore. G65P9814 D5.226 H0.003 does the trick and if the bore is out of range it will stop the machine. We experimented to determine the validity of this but we can't find anywhere in the VF-6 Settings where this data goes to. Forces us to just blindly accept the GO / NO GO test on faith. Anybody figured this out with a Haas mill?
Re: VF-6 single surface probe setting
Re: VF-6 single surface probe setting
I thought I had watched all the pages possible while doing the routine. But you are absolutely right. It is on the 10188 number. Just confirmed it. Thanks for the help!
Re: VF-6 single surface probe setting
Quote:
Originally Posted by
Matt@RFR
The trailing zeros in your macro call make me nervous, but are apparently working. Macros can be funny, and very picky some times.
The trailing zeros in the macro call are a Next Gen. Control "issue" "glitch", whatever you want to call them. I can't tell you right off hand which version update they started with, but I've had them for probably 6 months now. Haas apparently doesn't seem too concerned as they have been there for more than one update.
