What's new
What's new

Probing on Minimill issue

big_i11580

Plastic
Joined
Sep 30, 2015
All

First cnc for me. I bought a new to me 2012 Mini Mill. It has a Renishaw tool presetter and workpiece probe. While running the probe on the corner of my stock, it will travel WAY past the edge and then come in and touch off. I am making softjaws from 2" wide material and it is tripping the over travel sensors in the y axis. Is this maybe a modified parameter in the probing routine? Please be specific where to look, I have a learning curve. Thanks

John

Sent from my Pixel 2 XL using Tapatalk
 
All

First cnc for me. I bought a new to me 2012 Mini Mill. It has a Renishaw tool presetter and workpiece probe. While running the probe on the corner of my stock, it will travel WAY past the edge and then come in and touch off. I am making softjaws from 2" wide material and it is tripping the over travel sensors in the y axis. Is this maybe a modified parameter in the probing routine? Please be specific where to look, I have a learning curve. Thanks

John

Sent from my Pixel 2 XL using Tapatalk

are you using corner probing routine?
what happen if you just use the y routine? or only the x routine

sounds like you might have put some numbers in wrong. can you snap a screen shot of your program it spits out in MDI? use your celphone then post it. t
 
So I finally got back to this. Long story. I made a video so you can see what happens. See below. In the VQC, I selected vise corner and center of part. The block is 8.25" x 2.25" x 1". G54 for work offset and -.6" for z depth. The z works fine but you can see in the video it moves about 3-4" past the part in both directions in x and y. The y move causes an over travel error. My guess is the previous owner changed the distance traveled past the end of the part. Not sure where this is or what to look for. Thanks!

John

YouTube

Sent from my Pixel 2 XL using Tapatalk
 
So I finally got back to this. Long story. I made a video so you can see what happens. See below. In the VQC, I selected vise corner and center of part. The block is 8.25" x 2.25" x 1". G54 for work offset and -.6" for z depth. The z works fine but you can see in the video it moves about 3-4" past the part in both directions in x and y. The y move causes an over travel error. My guess is the previous owner changed the distance traveled past the end of the part. Not sure where this is or what to look for. Thanks!

John

YouTube

Sent from my Pixel 2 XL using Tapatalk


Looks like default over-travel is set really high.

I bet previous owner got too frustrated not starting close enough to the center, and when the cycle runs it hits down on the part. Then they have to make a small adjustment and run again. Rinse, repeat = changing default over-travel.

If previous owner is only finding blocks like in your example, I can see why they did it. Make it easy because you don't have to be close to the center at all (or the size estimate can be way undersized) and the cycle will find the edges just fine. But, if you need to do something else, that can be problematic.



Change setting 23 to off.
Select program 9023
What's yours have for var 27? in the first couple lines of code after the bunch of G04's:

Code:
O09023 (REN EASYSET V3.0) 
(40120737.0C VQC ADDED) 
(HAAS VQC WIRELESS PROBE, English, Inch/MM V3.0) 
(01-06-2012) 
G103 P1 
G04 P1 
G04 P1 
G04 P1 
G04 P1 
G04 P1 
G04 P1 
#3001= 0 
G04 P250 
G04 P1 
G04 P1 
G04 P1 
G04 P1 
G04 P1 
G04 P1 
IF [ #3001 LT 200 ] GOTO999 
#161= 556 (START CALIBRATION VARIABLE) 
IF [ #1 EQ #0 ] GOTO17 
[B]#27= 10 (DEFAULT Q IN MM)[/B] 
(#28=1DEFAULT WORK OFFSET) 
#29= #[ #161 + 4 ] (PROBE OFFSET #560) 
#30= 10 (STAND OFF) 
... etc

Is yours higher than 10? like 70-80? That should be default over-travel in millimeters. Default is 10. I'm not sure if that is also in the renishaw programs in the background, or in the renishaw variables... perhaps, but this is what I found taking a quick look.
 
John, it looks like you're doing everything right. I know there's a variable for approach distance but I'm not finding it in the manual or in my notes. First thing I would do is measure how far over it's going with a tape measure, then cruise through my macro variables and look for a number within 1/2" of that. I believe the approach distance should be set to .400" (10mm) or so, but it can be anything, really.

EDIT: Sidetalker beat me to it, and is more betterer as usual... :toetap:
 
Here is what I have. Looks like it is 10.
607bd35f3f7af7985115531969d277cc.jpg


Sent from my Pixel 2 XL using Tapatalk
 
Well that sucks. Gonna be hard to find where that edit was made. I'm guessing it could be anywhere since the previous owner sounds lazy to me.

Could try reloading those programs. npolanosky just posted these in a thread yesterday. https://www.practicalmachinist.com/...s-vqc-probing-warm-up-etc-362786/#post3342512

Could try that. (I suggest to back up your current ones first!)

Or download all of your current ones and post it here in a zip. I wouldn't mind taking a minute or two to compare to what I've got.
 
So far no difference. I called Productivity. They think it's doubling the values. Waiting to hear back from them

John

Sent from my Pixel 2 XL using Tapatalk
 
Don't use the ones I uploaded- Upon comparing your program to mine, there are some differences between the program for the wired TS27R and the OTS probe. 95% the same, but there's some new/different logic in the OTS program and of course the M-codes to the OTS on aren't there for the wired TS27R

(The wireless spindle probe might be closer, but the O09023 program is just toolsetter stuff)
 

Attachments

  • program.jpg
    program.jpg
    99.9 KB · Views: 97
So far no difference. I called Productivity. They think it's doubling the values. Waiting to hear back from them

John

Sent from my Pixel 2 XL using Tapatalk

Ah, I gave you bad information. I was thinking Q-val would make the cycle overtravel the estimated size... it doesn't - it travels further on the measuring hit.

And if the programs look the same, it must be the calibration?

In 9724 if in metric it sets #179 to 1mm or inch sets to .04
In the measuring cycle it overtravels 5mm (or 5*#179) plus the stylus size in #556/#557... John what do you have for those? They should be approx .117-.118
 
Ah, I gave you bad information. I was thinking Q-val would make the cycle overtravel the estimated size... it doesn't - it travels further on the measuring hit.

And if the programs look the same, it must be the calibration?

In 9724 if in metric it sets #179 to 1mm or inch sets to .04
In the measuring cycle it overtravels 5mm (or 5*#179) plus the stylus size in #556/#557... John what do you have for those? They should be approx .117-.118


#6996= 774
#162= #6998 (STATUS OF PARAMETER 774)
IF [ #4006 EQ 20 ] GOTO400
IF [ #4006 EQ 70 ] GOTO400
#173= 0.05 (INPOS ZONE MM)
#179= 1
#169= 5000 (FAST FEED MM)

IF [ #162 NE 7 ] GOTO140 (SIGMA 5 MOTOR)
IF [ #6507 GT 32000000 ] GOTO150
GOTO145
N140
IF [ #6507 GT 4000000 ] GOTO150
N145
#169= 2500 (FAST FEED FOR SLOW MACHINES- MM)
N150

GOTO500
N400
#173= 0.002 (INPOS ZONE INCH)
#179= 0.04
#169= 200 (FAST FEED INCH)
 
John check variables 556 and 557 under current commands. See here:


snapshot (3).jpg


I just tried this on my VF2-SSYT. Changing these values to say 2.0 I could reproduce your results.

You should do a recalibration to fix this. (or can just put in .118 for now, but it won't be accurate) Who knows what else was modified?


Do you have a ring gage to calibrate with? If not I would suggest to buy one. The stylus can shift over time and it is good to check and recal every so often.
 
Check this out. I'll pick one up. What size and accuracy should I get?
78838d8109d8d335418416854c1bd3f4.jpg


Sent from my Pixel 2 XL using Tapatalk
 
Should I change the value?

Sent from my Pixel 2 XL using Tapatalk

Looks like it was calibrated in metric. Could probably change 556 to .1175 & 557 to .1177 and you'd be working fine for now, although I don't know what else might be affected.

Best to re-calibrate with a ring gage of known size. I use a Ø2" gage

You could probably get away with milling a bore, then calibrating off that, but it will only be as accurate as you can mill and measure that bore. Best to use a proper gage. Suppose it depends what type of tolerances you work to as well.

Calibration cycle in vqc
 
When I got this, everything was in metric. What all do I have to do to switch to English units? It displays in inches but what all do I have to change?
 








 
Back
Top