1997ish Fanuc 21t g84 tapping cycle
Close
Login to Your Account
Results 1 to 7 of 7
  1. #1
    Join Date
    Dec 2016
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    83
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    15

    Default 1997ish Fanuc 21t g84 tapping cycle

    The Fanuc controller for my hardinge cobra cnc lathe uses a m29 for a internal chucking mode. Therefore, I can not use it for rigid tapping. Do I just replace it with a M3?

    Will that controller take a G84 taping cycle? It will not take a g81 drill and rapid retract. Which drill/tap canned cycles will it take.

  2. #2
    Join Date
    Oct 2014
    Country
    CANADA
    State/Province
    Ontario
    Posts
    129
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    47

    Default

    I've got a lathe with the same control, albeit about 6 years newer. It requires M29 when rigid tapping but that's because it has live tooling as well. If you haven't put M3 into the program though, does the machine know which direction to turn the spindle?

    As for G81, a simple drill and retract, use G01 instead. It should accomplish the same thing, as least it does on mine. It would alarm out if G81 was programmed. G83 works fine for peck drilling, you'll probably need to program the peck distance like Q1000 instead of Q0.1 as it may not like decimals for the Q value.
    Last edited by Rapid_Tech; 04-04-2018 at 09:08 AM.

  3. #3
    Join Date
    May 2008
    Country
    SOUTH AFRICA
    Posts
    1,587
    Post Thanks / Like
    Likes (Given)
    1169
    Likes (Received)
    658

    Default

    From my knowledge for fanuc turning G81 does not exist... it is a mill cycle. G83 is the only face drilling cycle. I think Rapid_Tech just made a typo when he wrote "G83 works fine for peck tapping" and probably meant peck drilling.

    There are parameters that change whether it full retracts or not after each peck from memory but I could be wrong on that point. I remember messing around with those quite a while ago so that if I G83 it full retracts after each peck and not only after the full depth. You could just make your peck amount, Q as Rapid mentioned, LARGER than the depth of your hole and it should go to full depth and then rapid out.

    Not all G84 tapping cycles need a M29, it just depends how the tapping cycle is setup. Mine varies from machine to machine. Even if it is needed I switch the spindle on before my M29 line anyway as a habit I guess. So the spindle turns,you approach the part then M29 S200 without M3 in that line because as far as I know G84 is right hand tapping and because you have turned the spindle on before that you don't need it.

    Try it out without a part in the machine. Also have you tried M29 S100 yet? It might be setup that if it reads M29 and S in the same line that it knows what it is doing.

  4. #4
    Join Date
    Mar 2003
    Location
    Upstate New York USA
    Posts
    281
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    43

    Default

    Rigid tapping was not available on the Cobra machines, the PLC would need to be re-written to allow M29 to be used for rigid tapping and not internal chucking. The G80 canned cycles would have been an option on that control as rigid tapping was not offered they were not included in the control package

    Tom

  5. #5
    Join Date
    Dec 2016
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    83
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    15

    Default

    Im trying to get a post to work that will output something that will work from hsm. I think that just eliminating the cycle and getting it to output G0 and G1 insead of canned cycle will work fro drilling and this for tapping with a floating holder...


    O0001(RIGID TAPPING)

    G20G40 (HARDINGE)

    G97 S50 M13

    M98 P1

    T909 (TAP HOLE 5/8-18)

    X0. Z0.5

    G32 Z-0.5 F0.049 - Feed is in thread pitch - .001

    G4 X0.5

    M14

    G4 X0.4

    G32 Z.05 F0.05 - Feed is in thread pitch

    M98 P1

    M30

  6. #6
    Join Date
    Oct 2014
    Country
    CANADA
    State/Province
    Ontario
    Posts
    129
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    47

    Default

    [QUOTE=NAST555;3153362]From my knowledge for fanuc turning G81 does not exist... it is a mill cycle. G83 is the only face drilling cycle. I think Rapid_Tech just made a typo when he wrote "G83 works fine for peck tapping" and probably meant peck drilling.

    Yeah, mixed them up by accident.

  7. #7
    Join Date
    Mar 2003
    Location
    Upstate New York USA
    Posts
    281
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    43

    Default

    The code you have for the tap should work with a floating tap holder however do not dwell after the M14 command

    Tom

  8. Likes Ox liked this post

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
  •