Fanuc O-TC and G54
Close
Login to Your Account
Results 1 to 19 of 19
  1. #1
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    3,306
    Post Thanks / Like
    Likes (Given)
    1173
    Likes (Received)
    1235

    Default Fanuc O-TC and G54

    The O-TC does not support additional work offsets (not even as an option AFAIK), instead relies on work shift.

    G54-G58 do not exist and alarm out when you try and enter them.

    However, it is somehow aware of G54 as it's clearly set as a default at startup, it's right there in the list of active modals.

    Is there any way to prevent this control from alarming out when it encounters a G54? It's the only real hurdle in being able to use a single unified post for my O-TC and our Oi-TC.

  2. #2
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,557
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1396

    Default

    Quote Originally Posted by gregormarwick View Post
    The O-TC does not support additional work offsets (not even as an option AFAIK), instead relies on work shift.

    G54-G58 do not exist and alarm out when you try and enter them.

    However, it is somehow aware of G54 as it's clearly set as a default at startup, it's right there in the list of active modals.

    Is there any way to prevent this control from alarming out when it encounters a G54? It's the only real hurdle in being able to use a single unified post for my O-TC and our Oi-TC.
    Hello gregor,
    I suspect that the alarm being raised is p/s010. That being so there is no parameter solution I'm aware of, but there is a fudge you could use. Register the number 54 in whatever parameter that is available between 6050 and 6059 to create a Custom G Code, G54. Lets say 54 is registered in parameter 6050, create a program under the number O9010 that contains nothing other than M99 to return control to the calling program. When G54 is encountered in your program, program O9010 should be called and immediately return control to the Block following where the G54 in the calling program was encountered.

    Regards,

    Bill

  3. #3
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    3,306
    Post Thanks / Like
    Likes (Given)
    1173
    Likes (Received)
    1235

    Default

    Quote Originally Posted by angelw View Post
    Hello gregor,
    I suspect that the alarm being raised is p/s010. That being so there is no parameter solution I'm aware of, but there is a fudge you could use. Register the number 54 in whatever parameter that is available between 6050 and 6059 to create a Custom G Code, G54. Lets say 54 is registered in parameter 6050, create a program under the number O9010 that contains nothing other than M99 to return control to the calling program. When G54 is encountered in your program, program O9010 should be called and immediately return control to the Block following where the G54 in the calling program was encountered.

    Regards,

    Bill
    Very clever Bill!

    When the machine is finished it's current job I'll give that a go and let you know how I get on.

    Alternatively, that solution might be somewhat confusing to the operator, so I might have to live with two posts. We'll see!

    Cheers.

  4. #4
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,557
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1396

    Default

    Quote Originally Posted by gregormarwick View Post
    Very clever Bill!

    When the machine is finished it's current job I'll give that a go and let you know how I get on.

    Alternatively, that solution might be somewhat confusing to the operator, so I might have to live with two posts. We'll see!

    Cheers.
    Hello gregormarwick,
    It should be no more confusing than the program encountering a G54 and not raising an alarm. If the O9000 Series Programs are protected and hidden via parameter, as they should be, the operator will not be aware of the Macro Program being called by G54. It will seem that the program reads G54 and advances to the next Block.

    Regards,

    Bill

  5. #5
    Join Date
    Jun 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    793
    Post Thanks / Like
    Likes (Given)
    460
    Likes (Received)
    301

    Default

    Have you checked with Fanuc? I believe it is an option for turning but rare. Fanuc options must be purchased and loaded like Okuma does. Gone are the days of merely flipping a parameter.

  6. #6
    Join Date
    Feb 2006
    Location
    Republic of Texas
    Posts
    2,425
    Post Thanks / Like

    Default

    916.2 ymmv

  7. #7
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,046
    Post Thanks / Like
    Likes (Given)
    760
    Likes (Received)
    2135

    Default

    G54-G59 is available on a 0TC with firmware versions other than 660 and 662.

  8. #8
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,100
    Post Thanks / Like
    Likes (Given)
    4542
    Likes (Received)
    1582

    Default

    A while back I posted these pictures of our Johnsford lathe with the 0-T control. One on the far right has has the G54 G55 G56 fixture offsets on it. Weather it's a 0-T"C" I don't know?

    Brent

    Geometry Offset on the Lathe Yang ML25A Fanuc O-T

  9. #9
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,046
    Post Thanks / Like
    Likes (Given)
    760
    Likes (Received)
    2135

    Default

    Quote Originally Posted by yardbird View Post
    .....Weather it's a 0-T"C" I don't know?
    Hey Brent,

    If you want to know, post up the firmware version and I'll look in my info and see if it shows up.

    Kevin

  10. #10
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,100
    Post Thanks / Like
    Likes (Given)
    4542
    Likes (Received)
    1582

    Default

    Quote Originally Posted by Vancbiker View Post
    Hey Brent,

    If you want to know, post up the firmware version and I'll look in my info and see if it shows up.

    Kevin
    Hey Kevin,

    I wouldn't even have any idea where or what to look at to tell you what version it is? Not the first clue? Lol...

    How do you tell what version of firmware it is?

    Brent

  11. #11
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,046
    Post Thanks / Like
    Likes (Given)
    760
    Likes (Received)
    2135

    Default

    On the 0 series the firmware number shows on the screen for a moment when you boot the control. Sometimes if the CRT is a bit slow to warm up you won't have a chance to see the number before it is gone. If that happens just turn the control back off, count to 3 and turn it back on. Usually that will let you catch the number.

  12. #12
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,100
    Post Thanks / Like
    Likes (Given)
    4542
    Likes (Received)
    1582

    Default

    Not exactly sure what it is so this is what I saw. It ain't up there long that's for sure. Lol...

    Freaking sideways picture wtf?

    Brent

    20190419_003724.jpg

  13. #13
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,100
    Post Thanks / Like
    Likes (Given)
    4542
    Likes (Received)
    1582

    Default

    Quote Originally Posted by alphonso View Post
    916.2 ymmv
    For what it's worth my 916.2 = 1

    Brent

  14. #14
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,046
    Post Thanks / Like
    Likes (Given)
    760
    Likes (Received)
    2135

    Default

    0667 means it is an 0TC-F. The F indicates FAPT which was Fanuc's conversational lathe programming software. Does your machine have conversational?

  15. #15
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,100
    Post Thanks / Like
    Likes (Given)
    4542
    Likes (Received)
    1582

    Default

    No not that I'm aware of. It's a "C" axis lathe but none of the tooling came in with it so we've never used it. I'm almost positive it doesn't but maybe I need to look it over better. Can't imagine where I'd find it I've been all through it.

    Brent

  16. #16
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,100
    Post Thanks / Like
    Likes (Given)
    4542
    Likes (Received)
    1582

    Default

    Can you shut it off by parameter? What I mean is not to load the conversational programming when it boots up at startup? Hell maybe its shut off? The danm thing comes on almost instantly.

    Brent

  17. #17
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    3,306
    Post Thanks / Like
    Likes (Given)
    1173
    Likes (Received)
    1235

    Default

    Mine is a 669. I set 916.2 and lo and behold I now have work offsets. They look exactly like Brent's - hidden behind a toggling softkey. So thanks all for that!

    Next question is, how do they work? There is no Measure soft key like on the Oi, and MZ doesn't work like when setting the work shift. There must be an easier way than calculating the offset and entering it directly?

  18. #18
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,100
    Post Thanks / Like
    Likes (Given)
    4542
    Likes (Received)
    1582

    Default

    On this particular machine that's exactly what I do. I've never got this figured myself. The guy in post 6 has a detailed description on how to use the measure function but I was unsuccessful when tried it on my machine. Maybe I wasn't doing something exactly right? Maybe he'll show back up here?

    Have a look below. Talk about finding a needle in a haystack! Lol

    Brent

    Problem getting my head around work offsets on lathe

  19. #19
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,557
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1396

    Default

    Quote Originally Posted by gregormarwick View Post
    Next question is, how do they work? There is no Measure soft key like on the Oi, and MZ doesn't work like when setting the work shift. There must be an easier way than calculating the offset and entering it directly?
    Hello gregor,
    If your control has User Macro and you let me know how you're setting Tool Geometry, I can give you a Macro Program for setting the Work-shift Offset value of the Offset of choice.

    Regards,

    Bill


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
  •