Probing on Minimill issue
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 23
  1. #1
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6

    Default Probing on Minimill issue

    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

  2. #2
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    400
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    125

    Default

    Quote Originally Posted by big_i11580 View Post
    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

  3. #3
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6

    Default

    I'll run it tomorrow morning and photograph it. Thanks.

    Sent from my Pixel 2 XL using Tapatalk

  4. #4
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6

    Default

    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

  5. #5
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    642
    Post Thanks / Like
    Likes (Given)
    97
    Likes (Received)
    330

    Default

    Quote Originally Posted by big_i11580 View Post
    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 
    #27= 10 (DEFAULT Q IN MM) 
    (#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.

  6. #6
    Join Date
    May 2004
    Country
    UNITED STATES
    State/Province
    California
    Posts
    2,493
    Post Thanks / Like
    Likes (Given)
    885
    Likes (Received)
    1611

    Default

    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...

  7. #7
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6

    Default

    Here is what I have. Looks like it is 10.

    Sent from my Pixel 2 XL using Tapatalk

  8. #8
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    642
    Post Thanks / Like
    Likes (Given)
    97
    Likes (Received)
    330

    Default

    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. Default Programs- VQC, Probing, warm-up, etc

    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.

  9. Likes npolanosky liked this post
  10. #9
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6

    Default

    Here is the O09023

    O09023.zipO09023.zip

  11. #10
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    671
    Post Thanks / Like
    Likes (Given)
    556
    Likes (Received)
    346

    Default

    John,

    Did you compare your probing macros to the ones I gave you yet?

  12. #11
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6

    Default

    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

  13. #12
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    292
    Post Thanks / Like
    Likes (Given)
    234
    Likes (Received)
    93

    Default

    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)
    Attached Thumbnails Attached Thumbnails program.jpg  

  14. #13
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    642
    Post Thanks / Like
    Likes (Given)
    97
    Likes (Received)
    330

    Default

    Quote Originally Posted by big_i11580 View Post
    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

  15. #14
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    671
    Post Thanks / Like
    Likes (Given)
    556
    Likes (Received)
    346

    Default

    Have you run the "settings" program to ensure the macro variables are set correctly?

  16. #15
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6

    Default

    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)

  17. #16
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    642
    Post Thanks / Like
    Likes (Given)
    97
    Likes (Received)
    330

    Default

    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.

  18. #17
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6

    Default

    Check this out. I'll pick one up. What size and accuracy should I get?

    Sent from my Pixel 2 XL using Tapatalk

  19. #18
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6

    Default

    Should I change the value?

    Sent from my Pixel 2 XL using Tapatalk

  20. #19
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    642
    Post Thanks / Like
    Likes (Given)
    97
    Likes (Received)
    330

    Default

    Quote Originally Posted by big_i11580 View Post
    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

  21. Likes YdnaD liked this post
  22. #20
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6

    Default

    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?


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •