Results 1 to 11 of 11
  1. #1
    barbter is offline Stainless
    Join Date
    Oct 2007
    Location
    UK
    Posts
    1,347

    Default Fanuc OT special Gcodes

    Hi all,
    We have a warner swasey fanuc 0ta cnc lathe.
    Apparently it has 'special' gcodes.....

    Is G33 (what the machine has) an exact equivalent to G32 (long hand threading)
    Is G78 (what the machine has) as exact equivalent to G92 (box threading)

    And why the non standardisation?

    Cheers

  2. #2
    metlhed is offline Stainless
    Join Date
    Jan 2007
    Location
    Ohio
    Posts
    1,153

    Default

    Fanuc has different groups of codes...but not sure if this is the reason. I know that Group C includes the G32 for the multi-X lines and G92 is tapping without live tool. I have the diffs somewhere for the 18i-T. Some aren't even close if I remember correctly. It is just a param change 'tween Group A and Group C.

  3. #3
    metlhed is offline Stainless
    Join Date
    Jan 2007
    Location
    Ohio
    Posts
    1,153

    Default

    You have probably opened a can of worms with this one...Machine builders have tons of options offered with Fanuc. It is a general control and NOT machine specific (Haas/Okuma/Mazak...etc.) so Fanuc will configure control to what the builder wants. Just wait for the anti-Fanuc crowd to chime in...wait for it...wait for it...they'll be here soon.

  4. #4
    Boris is offline Titanium
    Join Date
    Oct 2005
    Location
    England
    Posts
    3,017

    Default

    You wait until the heidehain mob turn up

    You used to be able to get a TNC control that had everything turned up by default, if you wanted a simple control you bought a 150 or 155, you wanted something better you got a 370
    Now on the 530 there are 3 levels of options and you gotta pay for each one exactly like Fanuc and their freaking 900 parameters.

    Boris

    Oh well least Heidehain give you a usable control at the bottom range of the options

  5. #5
    Heinz R. Putz is offline Hot Rolled
    Join Date
    Mar 2006
    Location
    Columbus, Ohio
    Posts
    918

    Default Fanuc codes.

    Warner Swasey used the European version of the G Codes for the European market, that makes sense, does it not?
    There is a group A, a group B and a group C. You have B if the G92 is called G78..
    You would also have a G92 instead of the G50 we use here.
    Your G78 should be the equivalent of our G76 if you have the C group.
    However, if you have the B group, then the G92 is equivalent to the G78....
    Feed in inches per minute is G94 for both B and C.
    Back to feed per rev is G95 for both B and C.
    I bet you have B.
    Totally confused? Do not blame Fanuc, its the fault of the machine builder.
    Even today some builders still do it.
    I visited the showroom of Emco Maier recently here in Columbus and they are actually selling their training machines with the European version of the G-Codes as standard for teaching in this country where 99.9% of all shops use the A group..
    The regular codes like G0, G1. etc., are the same, so is G41, G42, G40, G97, G96.
    If you need, I can list all the differences.
    Heinz.
    http://home.columbus.rr.com/hputz

  6. #6
    metlhed is offline Stainless
    Join Date
    Jan 2007
    Location
    Ohio
    Posts
    1,153

    Default

    Heinz, Group C in USA, G76 is auto thread...not the same in Euro code Group C?

  7. #7
    Heinz R. Putz is offline Hot Rolled
    Join Date
    Mar 2006
    Location
    Columbus, Ohio
    Posts
    918

    Default Fanuc G-Codes.

    G76 in group C is our G74 (Peck Grooving or Peck Drilling in Z), I actually had to look it up in my only Fanuc manal that lists all 3 G-Code sets.
    Heinz.

  8. #8
    barbter is offline Stainless
    Join Date
    Oct 2007
    Location
    UK
    Posts
    1,347

    Default

    Heinz,

    It looks like we have Group B then. I've never been 'special' before!
    Our multi line threading is G33
    Our box threading is G78 (I like the look of this although haven't used it yet. Nice and simple to understand because you can see the code).
    We have G76 threading (I've got some questions on this - that'll be another thread then)
    We set our max RPM with G92

    Thanks,
    Standardisation is a wonderfull thing, if only people would do it!

  9. #9
    g-coder05's Avatar
    g-coder05 is offline Stainless
    Join Date
    Mar 2006
    Location
    Zhongshan China
    Posts
    1,807

    Default

    In g33 does adding a (K) value always make the cycle progressive lead. ive been using this on a Mazak to machine some Nuclear threads but was wondering if i jump to funuc is it gonna change. the matirial is 3.0 dia and 42" long and the thread progression is .0014 per inch.

  10. #10
    metlhed is offline Stainless
    Join Date
    Jan 2007
    Location
    Ohio
    Posts
    1,153

    Default

    Quote Originally Posted by Heinz R. Putz View Post
    G76 in group C is our G74 (Peck Grooving or Peck Drilling in Z), I actually had to look it up in my only Fanuc manal that lists all 3 G-Code sets.
    Heinz.
    Heinz,

    I know that you are a well respected and even revered Fanuc Guru, but the 18T Hardinge T42-SP I was with for 8-1/2 years used C Group and G76 was auto thread-just required an extra 0 in the undecimaled codes. The 21i-T on the EmcoMaier upgraded to .00001 I was with for 5 years was the same...G76=auto thread.

  11. #11
    gcodeguy is offline Cast Iron
    Join Date
    Jun 2007
    Location
    Easton, PA
    Posts
    482

    Default

    barbter, G78 may be easy to understand, but it is a zero degree lead-in toolpath. Personally I like to have a lead-in. If you are using a CAD/CAM system, then use the G33. You can still see each pass, but will be able to make the lead-in any angle you want. You can manually program the lead-in (did it for a few years on CHNCs), but obviously this will require more work on your part as the programmer.

    Since getting controls with the G76 threading canned cycle, I've never looked back. Occasionally may have to program each pass, but prefer not to whenever possible.

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
  •