Problem with 5 axis matsuura - Page 2
Close
Login to Your Account
Page 2 of 2 FirstFirst 12
Results 21 to 29 of 29
  1. #21
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    3,642
    Post Thanks / Like
    Likes (Given)
    2067
    Likes (Received)
    1345

    Default

    It's definitely a positional is it?
    ie when indexing, the part IS flat after axis lock, and the chamfer tool just takes off too much the one face from the "top" (which is the face that's furthest from centre of table/part?)
    Are you sure that when the table indexes it locks at C0 being flat and zero, and not locks at 1.5degrees or something random although repeatable?

    I've had this on a 4th doing peripheral work and it was a parameter... for 3x identical machines...OEM never set 1x parameter...

  2. #22
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    801
    Post Thanks / Like
    Likes (Given)
    129
    Likes (Received)
    438

    Default

    Theoretically, someone could have gotten in there and really screwed up the calibration using the EZ-5 or whatever it is called. Matsuura told me to never futz with it, that the machines don't move and one can do more harm than good LOL.

    boosted does G54.4 need to be called or is it turned on by parameter? I'm still stuck on the fact that I only see a G54.1 P call and no other 5-axis specific WCS or operating mode seems to be active.

    It does seem like we agree that either:
    1) the work piece is at COR on the C Axis, OR
    2) you require some kind of compensation function to be active

    Since the work piece is demonstrably not at COR (or it would cut right in the same plane as it was probed, A0.0 and C0.0) and since this code was spliced in (and doesn't have any visible compensation calls) we need to figure out what calls they are using in the rest of the program.

    I suggest the OP go into the program and search for G68.2, G54.2, and G54.4 and see what the other toolpaths are using.

  3. Likes empwoer liked this post
  4. #23
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    402
    Post Thanks / Like
    Likes (Given)
    558
    Likes (Received)
    172

    Default

    Quote Originally Posted by boosted View Post
    Hopefully somebody with more Matsuura specific expertise can chime in. I do know a few things for certain though.

    - They can definitely program from COR and probe to compensate for error. That is what WSEC is for. The probed values would go into the "shift" instead of the standard work offset page.

    - G68.2, tilted workplanes is totally separate from dynamic work offsets. They can be combined or used separately. Dare I say most (at least most IME) 5 axis fanucs are being programmed using COR and tilted planes.

    - Dynamic Work Offsets are the shit, and it is shocking that so few people are utilizing them.

    - WSEC or DWO are dependent on your COR being calibrated correctly (and recorded in parameters) to function correctly. This is probably not your issue here though.
    yes, but you have to put in the work shift values into the table...

    we run our LX160 using straight up DWO and its programmed that way, havent had any issues with it yet.

  5. #24
    Join Date
    Oct 2006
    Location
    New Hampshire
    Posts
    188
    Post Thanks / Like
    Likes (Given)
    79
    Likes (Received)
    46

    Default

    I see G68.2 in that program which but I see no dynamic Work offset. Nothing in the probing sub says that the updated info is going into WSEC.

  6. #25
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    321
    Post Thanks / Like
    Likes (Given)
    52
    Likes (Received)
    168

    Default

    Fanuc gives access to the WSEC table as macro variables. Lot's of folks are writing probing routines to automatically handle small corrections with WSEC. Without seeing all of the code, it's really hard to speculate what's going on in that regard.

    As Rick said, my understanding is that there still must be a G54.4 called after the G54.1. I was speculating that perhaps Matsuura was doing something unexpected there.


    To the OP; it's time to start familiarizing yourself with 5 axis methodology, and that Fanuc programming manual. There are so many things that could potentially go wrong here, that it's going to be really difficult to diagnose over the internet. I think you are either seeing a programming error, or a combination of physical and programming errors.

    Personally, I'm a huge fan of starting from zero. Check that the COR is correct, and that your work offsets are in the correct spot after probing.

  7. #26
    Join Date
    Jan 2010
    Location
    Gilroy CA
    Posts
    4,387
    Post Thanks / Like
    Likes (Given)
    3169
    Likes (Received)
    2450

    Default

    Looks like the problem is the post. It is not outputting G68.2 for A0C0 Positions

    aka (TOP) does not call g68.2 so if your part is 1.00 off in X and 1.00 off in Y you will have a problem at A0C0 but your side operations will be correct.

    Have your post guy make sure to force G68.2 during all operations even if its 0 angle change it will still affect XYZ shifts from workoffsets

  8. Likes JMC liked this post
  9. #27
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    801
    Post Thanks / Like
    Likes (Given)
    129
    Likes (Received)
    438

    Default

    OP did you get this sorted?

  10. #28
    Join Date
    Jan 2020
    Country
    CANADA
    State/Province
    Alberta
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    0

    Default

    Yes, sorry, i got it figured then forgot to come back with an update. Unfortunately as far as i know we dont have CAMplete. And if it had a licence fee they almost certainly never used it here. We have gibs but i dont really use it, so far its been simple enough work to just write the code. I beleive the problem was not having a g68.2 for the top of the part as a few people mentioned already. I think what happened was the guy who used to work here before me was probing these parts at 90 degrees and didnt leave any notes in his programs about his setups, so like a sane person i probed all the tables at 0 degrees. I didnt realize without the g68.2 the machine wouldnt know where the part is at 90 degrees. I thaught before that it was only for tilting the table on its c axis and not the b.

  11. #29
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    321
    Post Thanks / Like
    Likes (Given)
    52
    Likes (Received)
    168

    Default

    Quote Originally Posted by IconoclastAl View Post
    Yes, sorry, i got it figured then forgot to come back with an update. Unfortunately as far as i know we dont have CAMplete. And if it had a licence fee they almost certainly never used it here. We have gibs but i dont really use it, so far its been simple enough work to just write the code. I beleive the problem was not having a g68.2 for the top of the part as a few people mentioned already. I think what happened was the guy who used to work here before me was probing these parts at 90 degrees and didnt leave any notes in his programs about his setups, so like a sane person i probed all the tables at 0 degrees. I didnt realize without the g68.2 the machine wouldnt know where the part is at 90 degrees. I thaught before that it was only for tilting the table on its c axis and not the b.
    Just want to clarify that this is the issue. The top plane still doesn't need a G68.2, and adding a blank G68.2 shouldn't fix anything.


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
  •