535,290 active members*
2,957 visitors online*
Register for free
Login
IndustryArena Forum > Machine Controllers Software and Solutions > G-Code Programing > Help needed with Yasnac work coordinate system
Results 1 to 7 of 7
  1. #1
    Registered
    Join Date
    Jan 2010
    Posts
    99

    Help needed with Yasnac work coordinate system

    Hey all,
    I've become familiar with Fanuc controls and am now trying to set up two new machines with Yasnac controls (one i80, one J300), and one major difference between these and Fanucs (0m, 18m, 0im, 18im, 31i) is tripping me up...

    We're using G54-G59 work offsets, and everything is working great except in this one instance:

    program is reset or finished on its own at M30
    Handwheel is moved (to clear chips) and then program is started...

    At this point we are losing our position... I'm trying to understand what I'm doing wrong to ensure a program started from the beginning (at any point and after any manual moves) will run in the correct position... There appear to be differences between how Fanuc and Yasnac handle G52 local coordinate system, but I prefer (and in practice we don't) to not use G92 G52 at all...


    If i watch the "Run|Command" screen after resetting a program, moving the handwheel, and restarting the program i can see the position data on that screen stay fixed until reset is pressed again, and the problem never appears when reset is pressed before cycle start (after moving)...

    I need to find a way to clear this programmatically, in my tool change macro ideally... here are some code snippets of what works fine in fanucs:

    Code:
    O9020(M6   TOOL CHANGE)
    T#20
    G0G80G91M9
    #148=-1
    G28Z0M6T#20
    #148=#20
    M58
    G49G40
    G90
    M99
    and here is my Yasnac Tool change, adding the G52 didn't help

    Code:
    %
    O9020(M6   TOOL CHANGE)
    T#20
    G00 G80 G49 G90 Z0 M9
    (G00 G80 G49 G52 G90 Z0 M9)
    #148=-1
    G91G28Z0M6
    #148=#20
    G90G49G40
    M99
    both are called with simple programs like:
    Code:
    M6T2
    M1(TOOL2 3. FACE MILL)
    M3S3500
    G54X0.2876Y-3.1461
    G43Z1.H2
    /M9
    T6
    G0Z0
    (MAKING CHIPS)
    G0Z1.0
    M6T2
    M1(TOOL2 3. FACE MILL)
    M3S3500
    G54X0.2876Y-3.1461
    G43Z1.H2
    /M8
    T3
    G0Z0
    (MAKING CHIPS)
    M6T3
    M1(TOOL3 .500 EM)
    M3S14000
    G54X0.2876Y-3.1461
    G43Z1.H3
    /M8
    T2
    G0Z0
    (MAKING CHIPS)
    G0Z1.0
    M6T2
    M30
    any help greatly appreciated
    - gwarble

  2. #2
    Gold Member
    Join Date
    May 2004
    Posts
    4519
    Are you calling G90 when program is restarted?

  3. #3
    Registered
    Join Date
    Jan 2010
    Posts
    99
    Quote Originally Posted by txcncman View Post
    Are you calling G90 when program is restarted?
    Programs always start with a call to that M6 macro, which internally controls G90/G91 and always finishes with G90 left on (as can be seen in macros above, and works fine on Fanucs)

    Thanks

    edit: flipping around G90/G91 in my macro doesn't make any difference (as expected)... All code pretty much is run in G90 (absolute) mode except G28/G30 (reference return) which run in G91 for obvious reasons
    I'm leaning towards not understanding how Yasnac handles G52 differently than Fanuc, but i guess it could also be something related to "handwheel interrupt" parameters or differences, but in that respect it appears to work just like fanucs

  4. #4
    Registered
    Join Date
    Jan 2010
    Posts
    99
    the only working solution i've found is G52 X0 Y0 Z0 in my tool change macro, which i don't want (homes all axis)

    i took a video of:
    Running a program, cutting air
    moving handwheel in X
    auto mode, running same program you can see its in the wrong X location!
    then running a third time with no handwheel movement is in the correct position

    [ame=http://www.youtube.com/watch?v=l_Svaf43078]Yasnac Work offset problem - YouTube[/ame]

  5. #5
    Registered
    Join Date
    Jan 2010
    Posts
    99
    a couple parameters that sound related but do NOT fix my problem:

    pm0007.3: Addition of work shift correct (this applies or ignores the "update" work shift to work offsets g54-g59)

    pm2002.0-4: Validity of automatic mode handle offset (1st-5th axis)

    pm2003.1: Valid operation of automatic mode handle offset
    0: Other than rapid traverse
    1: Only in interpolation mode

    pm4001.4: Presetting of workpiece coordinate system shift distance at the completion of zero return (g54-g59; pm4143)

    pm4006.0-4: Automatic coordinate system setting (1st - 5th axis)
    (these were on, but turning off made no change)

    Also removing all look-ahead/high speed machining code (HON GON GOF HOF) made no difference...


    This is a MyCenter-1Xi with Yasnac i80 and a Matsuura RA-2G with Yasnac J300... both acting the same, and both different than the dozen fanucs we have... Any help GREATLY appreciated

    Thanks
    - Joel

  6. #6
    Registered
    Join Date
    Jan 2010
    Posts
    99
    of course its always the simplest thing... i've always just ignored the "Manual Absolute" software switch on the Fanucs after learning to set them ON years ago for the way we run the machines, not fully understanding how the Fanucs act when its set to OFF...

    Found and turned on "Manual Absolute" in the settings page and voila, works like i want...

    Hope this helps someone else

    Matsuura doesn't have a soft switch for this, but pm0000.4 is the equivalent parameter, and pm4011.2,3,7 are related

  7. #7
    Registered
    Join Date
    Jan 2011
    Posts
    7

    Re: Help needed with Yasnac work coordinate system

    Thank you

Similar Threads

  1. Replies: 14
    Last Post: 12-13-2013, 12:56 AM
  2. Replies: 13
    Last Post: 01-08-2013, 03:38 PM
  3. Work Offset Coordinate System G59 Pxxx
    By SpruTormaCam in forum SprutCAM
    Replies: 1
    Last Post: 10-29-2011, 02:12 AM
  4. coordinate system
    By kiethnt in forum G-Code Programing
    Replies: 6
    Last Post: 04-26-2007, 01:46 PM

Tags for this Thread

Posting Permissions

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