Haas - Tool offsetter issue (WIPS) - Tools are off
Close
Login to Your Account
Results 1 to 17 of 17
  1. #1
    Join Date
    Apr 2013
    Location
    Washington, USA
    Posts
    126
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    13

    Default Haas - Tool offsetter issue (WIPS) - Tools are off

    Let me see if I can explain this.

    I have calibrated the tool offsetter using a "master" with a .2552 gauge pin according to the instructions.

    I have used the tool offsetter to get the offset for the Probe itself.

    Probe has been calibrated per the instructions as well.

    I have used the Probe to find the Z offset to the table itself (G55)

    Now....

    I have set a tool using the offsetter. Tool 3 is 1/2" endmill.

    I go to MDI - input G90 G55 - G43 H3 - G0 Z2. (This sends tool 3 to 2" above the table)

    When I go to check it and I put a 123 Block under the tool I have to lower the tool .006 to get it to touch the top of the block.

    Where could this .006" error be coming from? Is is the Probe or the tool offsetter?

  2. #2
    Join Date
    Apr 2019
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    465
    Post Thanks / Like
    Likes (Given)
    98
    Likes (Received)
    200

    Default

    If I had to guess, your tool setter pad isn't level in both axis.

  3. #3
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    2,846
    Post Thanks / Like
    Likes (Given)
    1277
    Likes (Received)
    3679

    Default

    Sounds like you need to shim the table up .006"

    Or maybe, what tool setting routine are you using, the straight down one or the one where it rotates ccw? With a 1/2" cutter, you're right on the edge of the tool setter stylus. Try the rotating one and see if that helps.

  4. #4
    Join Date
    Apr 2013
    Location
    Washington, USA
    Posts
    126
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    13

    Default

    Quote Originally Posted by as9100d View Post
    If I had to guess, your tool setter pad isn't level in both axis.
    This appears to be a problem. I will fix that and see if that solves the issue.

  5. #5
    Join Date
    Apr 2013
    Location
    Washington, USA
    Posts
    126
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    13

    Default

    Ok. Now what's weird is that I leveled that out. And now when I do my offsets I'm getting very large numbers. Before I was getting offsets of say 7.34 for a tool, now that tool is coming in with an offset of 13.7" (?)

  6. #6
    Join Date
    Apr 2019
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    465
    Post Thanks / Like
    Likes (Given)
    98
    Likes (Received)
    200

    Default

    If you leveled I'm x and y, you need to go through the entire probe calibration process.

  7. #7
    Join Date
    Oct 2012
    Location
    Orange county, CA
    Posts
    100
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    22

    Default

    you calibrated the master for a diameter with a pin, but you didn't appear to calibrate the length. There's a complete probe calibration option in VPS that needs a calibrated tool with known gage length and diameter.

  8. Likes Prototypical, ARB liked this post
  9. #8
    Join Date
    Apr 2013
    Location
    Washington, USA
    Posts
    126
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    13

    Default

    Quote Originally Posted by coyoinu View Post
    you calibrated the master for a diameter with a pin, but you didn't appear to calibrate the length. There's a complete probe calibration option in VPS that needs a calibrated tool with known gage length and diameter.
    This was the problem. I got it within .0005 or better now. I had to play around with the gauge length numbers to get it.

  10. #9
    Join Date
    Apr 2019
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    465
    Post Thanks / Like
    Likes (Given)
    98
    Likes (Received)
    200

    Default

    Need to use a dial test indicator to measure the gage length. Zero on the face of the spindle then zero in the control under position. Wheel the Axis up and zero the dti on the bottom face of the calibrated tool

    That number on the position page is your gage length you will use for probe calibration

  11. Likes Prototypical, Booze Daily liked this post
  12. #10
    Join Date
    Apr 2013
    Location
    Washington, USA
    Posts
    126
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    13

    Default

    Quote Originally Posted by as9100d View Post
    Need to use a dial test indicator to measure the gage length. Zero on the face of the spindle then zero in the control under position. Wheel the Axis up and zero the dti on the bottom face of the calibrated tool

    That number on the position page is your gage length you will use for probe calibration

    aahhh...ok. I will do this. I remember being told a long time ago that the gauge length started at some imaginary plane close to the face of the spindle. I will do this tomorrow and see what I get. thanks!!

  13. #11
    Join Date
    Apr 2019
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    465
    Post Thanks / Like
    Likes (Given)
    98
    Likes (Received)
    200

    Default

    If you need photos or a better explanation, I can send photos.

  14. #12
    Join Date
    Apr 2013
    Location
    Washington, USA
    Posts
    126
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    13

    Default

    Quote Originally Posted by as9100d View Post
    If you need photos or a better explanation, I can send photos.
    Thank you but I think I understand. I'll get a better idea in the morning.

    thanks a bunch!

  15. #13
    Join Date
    Apr 2013
    Location
    Washington, USA
    Posts
    126
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    13

    Default

    Quote Originally Posted by as9100d View Post
    Need to use a dial test indicator to measure the gage length. Zero on the face of the spindle then zero in the control under position. Wheel the Axis up and zero the dti on the bottom face of the calibrated tool

    That number on the position page is your gage length you will use for probe calibration

    This actually didn't get me a correct number. It gave me a larger number than what I was previously using. But perhaps if I started with that number it might have been a different story.

    So what I did was started off with 4.9" (scale measure) gauge length. Went through the entire process. Set a tool using the new parameters (1/4" endmill). Used the probe to touch off the table for a Z=zero (G59) Sent the 1/4" tool to 2" above the table using G59. Checked it with my 123 block. The tool was .0052" above the 123 block. So I subtracted .0052 from my 4.9" gauge length - 4.8948" now. Went back to calibration page and used 4.8948 as the new number, went through entire process again. Now tools are coming out within .0002 when I check with a 123 block.

  16. #14
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,450
    Post Thanks / Like
    Likes (Given)
    545
    Likes (Received)
    779

    Default

    If you are not shifting the tool over half the diameter you will get about that much error. The tool setter is 10MM and since endmill bottoms taper inwards towards the center its actually straddling the probe with the recess of the taper.

  17. #15
    Join Date
    Apr 2013
    Location
    Washington, USA
    Posts
    126
    Post Thanks / Like
    Likes (Given)
    40
    Likes (Received)
    13

    Default

    Quote Originally Posted by g-coder05 View Post
    If you are not shifting the tool over half the diameter you will get about that much error. The tool setter is 10MM and since endmill bottoms taper inwards towards the center its actually straddling the probe with the recess of the taper.
    I would do it while rotating. The tool was moving half the diameter over, spinning then touching off. The issue I found was that my master gauge length was not correct. Now my tools are coming in within .0002.

  18. Likes Mike1974, g-coder05 liked this post
  19. #16
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,723
    Post Thanks / Like
    Likes (Given)
    1536
    Likes (Received)
    1762

    Default

    I know there are work arounds, but save yourself the headaches and get one of these -

    CAT40 Tool Probe Calibrator - Made in USA MariTool

    It's soooo nice to have an actual tool to use in each machine. I noticed when I started at this job that on each machine the work probe had differing H values, by as much as .25", even though using a scale they checked the same. When our tool probe went down I "made" them (asked nicely I mean LoL) buy a master calibration tool like this ^ one (we have a little different one than the Maritool). After setting up the tool probe in the machine that needed a replacement, I re-did the calibration in the next machine and lo and behold now the work probes are within .001" of each other.

  20. Likes Prototypical, ARB liked this post
  21. #17
    Join Date
    Dec 2002
    Location
    Granville,NY,USA
    Posts
    3,932
    Post Thanks / Like
    Likes (Given)
    326
    Likes (Received)
    425

    Default

    Quote Originally Posted by Mike1974 View Post
    I know there are work arounds, but save yourself the headaches and get one of these -

    CAT40 Tool Probe Calibrator - Made in USA MariTool

    It's soooo nice to have an actual tool to use in each machine. I noticed when I started at this job that on each machine the work probe had differing H values, by as much as .25", even though using a scale they checked the same. When our tool probe went down I "made" them (asked nicely I mean LoL) buy a master calibration tool like this ^ one (we have a little different one than the Maritool). After setting up the tool probe in the machine that needed a replacement, I re-did the calibration in the next machine and lo and behold now the work probes are within .001" of each other.
    The MariTool master makes life easy and quick. No worries

  22. Likes Mike1974 liked this post

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
  •