Old Yasnac controller G54 issue
Close
Login to Your Account
Results 1 to 14 of 14
  1. #1
    Join Date
    Mar 2018
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    29
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    2

    Default Old Yasnac controller G54 issue

    Likely just something I don't know as I bought this machine and brought it into my little hobby shop to learn some CNC stuff.

    I've been able to zero the machine, then setup a G54 offset and make it active, but with in MDI or MEM i get a "020: Prog Error (G)" any time it's called and I have to hit reset. In MDI G54 is now my active offset and everything I run is based on it, if I'm running an actual program then I have to edit it and remove the G54, although it's still the primary coord system.

    Changing to any others seems to do the same thing. I set up a simple G55 that is 3" off of machine zero in X/Y and I can go to MDI, run G55, get the Prog Error, reset then go to X0 Y0 and be 3" off X/Y, run G54, get Prog Error, go to X0 Y0 and be where expected for G54.

    Is there more to setting the current coordinate system than just calling it? Why might I be getting this error?

    The manual suggests:
    020 PROG ERROR (G)
    Unusable G code or G code not included in options programmed
    ???
    seems odd that it works other than interrupting what ever I'm doing and having to reset the alarm

    20200219_140742.jpg

  2. #2
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    816
    Post Thanks / Like
    Likes (Given)
    76
    Likes (Received)
    281

    Default

    Quote Originally Posted by TD-4242 View Post
    Likely just something I don't know as I bought this machine and brought it into my little hobby shop to learn some CNC stuff.

    I've been able to zero the machine, then setup a G54 offset and make it active, but with in MDI or MEM i get a "020: Prog Error (G)" any time it's called and I have to hit reset. In MDI G54 is now my active offset and everything I run is based on it, if I'm running an actual program then I have to edit it and remove the G54, although it's still the primary coord system.

    Changing to any others seems to do the same thing. I set up a simple G55 that is 3" off of machine zero in X/Y and I can go to MDI, run G55, get the Prog Error, reset then go to X0 Y0 and be 3" off X/Y, run G54, get Prog Error, go to X0 Y0 and be where expected for G54.

    Is there more to setting the current coordinate system than just calling it? Why might I be getting this error?

    The manual suggests:
    020 PROG ERROR (G)
    Unusable G code or G code not included in options programmed
    ???
    seems odd that it works other than interrupting what ever I'm doing and having to reset the alarm

    20200219_140742.jpg
    I had a crap load of those acrolocs through the years but its been a while.
    post your code. I am thinking you dont have a g90 in there on the line or before before on your g54 code.
    g54 works just fine on that control and on those machines.
    example
    G00G90G54X1.0Y1.0

  3. #3
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,844
    Post Thanks / Like
    Likes (Given)
    871
    Likes (Received)
    2611

    Default

    The error code means that the control is not optioned to use G54-G59. The functionality is in the firmware but it is easy for the firmware to drive an error code when the G code is called and the correct option parameter value is not set.

  4. Likes avto762 liked this post
  5. #4
    Join Date
    Mar 2018
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    29
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    2

    Default

    Quote Originally Posted by Delw View Post
    I had a crap load of those acrolocs through the years but its been a while.
    post your code. I am thinking you dont have a g90 in there on the line or before before on your g54 code.
    g54 works just fine on that control and on those machines.
    example
    G00G90G54X1.0Y1.0
    Just testing with a very simple hand written gcode, not actually making a part:

    O0099
    N10 G10 Q2 P1 X3. Y-3. Z-1.;
    N20 G90;
    N30 G00 G54 X0. Y0. Z0.;
    M30;


    N10 is used to set the G54 offset, this works and is reflected in the settings as per the manual

    #6516 30000
    #6517 - 30000
    #6518 - 10000


    (these parameters assume 4 digits for decimal so are actual 3.0000 -3.0000 -1.0000)

    N20 should of course set Absolute Programming

    N30 should then rapid to the G54 offset, but always gives me the error

    020: PROG ERROR (G)

    I've tried several variations of N20/N30 with having different things on different lines etc.

    The Oddest part is that once G54 errors, it is still set as the active work offset correctly and can be removed from the program and everything works. I just wouldn't be able to setup two parts and change from G54-G55 or I'll get the error and the program would stop.

  6. #5
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,844
    Post Thanks / Like
    Likes (Given)
    871
    Likes (Received)
    2611

    Default

    Quote Originally Posted by TD-4242 View Post
    .......N30 should then rapid to the G54 offset, but always gives me the error......
    See post 3 above. Your machine does not have the option for using G54-G59 codes activated. If need be, I can post a picture of the manual page that shows that codes G54-G59 are optional.

  7. #6
    Join Date
    Mar 2018
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    29
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    2

    Default

    So why does G54 work offset work then? I can set G54 either with G10 call or manually in the parameters screen #6517-6519 to be 3 inches off machine zero in X/Y, call G54 and get the error, reset the error and go to X0 Y0 and be 3 inches off machine zero.

    Other than the error stopping the program and needing a reset it sets the work offset just fine.

    Here's the manual:
    Yasnac MX1 Operator Manual pdf - CNC Manual

  8. #7
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    816
    Post Thanks / Like
    Likes (Given)
    76
    Likes (Received)
    281

    Default

    Quote Originally Posted by TD-4242 View Post
    So why does G54 work offset work then? I can set G54 either with G10 call or manually in the parameters screen #6517-6519 to be 3 inches off machine zero in X/Y, call G54 and get the error, reset the error and go to X0 Y0 and be 3 inches off machine zero.

    Other than the error stopping the program and needing a reset it sets the work offset just fine.

    Here's the manual:
    Yasnac MX1 Operator Manual pdf - CNC Manual
    Vance is correct if you dont have the option turned on its not going to work. all my acrolocs had the same control and the option on I assumed they all did.

    Call Larry at D&L service in peoria AZ he has tons of parts and knows these machines like the back of his hand. He worked for acrolock for like 15 years before he started a repair place in the 90's

    Does yours have the 2 pages of G53 G59 offsets I believe there is 4 per page ie G53 G54 G55 G56 next page G57 G58 G59

  9. #8
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,844
    Post Thanks / Like
    Likes (Given)
    871
    Likes (Received)
    2611

    Default

    Quote Originally Posted by TD-4242 View Post
    So why does G54 work offset work then? I can set G54 either with G10 call or manually in the parameters screen #6517-6519 to be 3 inches off machine zero in X/Y, call G54 and get the error, reset the error and go to X0 Y0 and be 3 inches off machine zero......
    But it really does not work. Every new fixture offset you call in the program causes an alarm that you have to reset and then do a program restart which on the MX series controls has its own kind of funky operation with often unpredictable behavior.

    The MX1 control was the first Yasnac to have fixture offsets available as an option. Most good builders included the function in their standard spec, but some made it an option. Most of the functionality was there so that a simple change of one bit of one of the option configuration parameters gave full functionality. Of course back in the day of the MX1 controls if your builder did not include fixture offsets in their standard spec, one only had to cough up ~$1200 to Yaskawa for one of their techs to come in, flip the rotary switch to 4 (maybe 7, been so long since I messed with an old Yasnac I have forgotten), change the bit, turn the switch back to 0, cycle the power, and job done. Usually about a 5 minute process.

    Since Yaskawa has been out of the CNC biz for ~15 years I wonder if a sympathetic tech back there might just whisper the parameter and bit if asked nicely.

    I looked through my tiny collection of option info for the MX controls and while I have a few, fixture offsets are not included. In the era of the MX1, I worked for Yamazen which at that time was the Mori Seiki importer. Mori included fixture offsets as standard on their machines so I never had need back then to activate the option.

  10. #9
    Join Date
    Mar 2018
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    29
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    2

    Default

    Very interesting and disappointing. Living in the current shared tech and open source world has warped my mind and made me forget how secretive everything was back then. I'd hope that since they are out of the business they would have released their internal maintenance/tech/repair manuals but I can't seem to find anything of the like. Only the operator level manuals.

  11. #10
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,844
    Post Thanks / Like
    Likes (Given)
    871
    Likes (Received)
    2611

    Default

    Quote Originally Posted by TD-4242 View Post
    ..... made me forget how secretive everything was back then.......
    I don't think it was about being secretive, it's about business and making money. The control builders offer a bare bones product to the machine builders. The machine builders get to spec the control features to suit their business model. Some builders, in order to keep the base machine price low, do not improve the base control spec and hope to sell control options at big markups. Other builders sell their machine at a higher base price, include many options, and sell on features, not cost.

    While Yaskawa no longer produces CNC controls, they still support their legacy products. I've not had contact with them for several years, but would be surprised that if one contacted them about adding a option they declined the order. Maybe someone at McKenna would share the info. Worth a call maybe?

  12. #11
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    432
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    72

    Default

    did you for grins and giggles. try your g90 on the same line as your g54?

  13. Likes dbramley liked this post
  14. #12
    Join Date
    Mar 2018
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    29
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    2

    Default

    yea, same issue. Any line with G54 sets the WCS but then throws an alarm that has to be reset to continue.

  15. #13
    Join Date
    Mar 2018
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    29
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    2

    Default

    For now, since I'm just learning G-code and the machine and not doing multiple parts, I'm sticking with G92 as the offset. Hopefully I can find a solution to the G54-59 issue by the time I needed it.

  16. #14
    Join Date
    May 2011
    Location
    Mesa, AZ
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    My old machine uses MX3 controller, I use fusion to post and had to alter the post processes to move G54 to a different line of code. Shoot me an email and I will send you my post. Also fixed the issues I was having with tapping.

    My email is my tag line with yahoo.com at end. I also bought an old Matsuura Mv-600c to “cut my teeth” in CNC.

    Dan


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
  •