Running just a finish pass using G76 threading cycle
Close
Login to Your Account
Likes Likes:  0
Results 1 to 15 of 15
  1. #1
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    678
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    327

    Default Running just a finish pass using G76 threading cycle

    When threading on a cnc lathe with G76 threading cycle is there a way to run just a finish pass sort of like a g70 does to a g71 cycle. A Mazak has a way to do this. Its really handy when trying to get your offset set correctly on your threading tool. You can just keep changing your offset a little at a time and rerunning the thread finish until your gauge fits without rerunning the whole cycle.

  2. #2
    Join Date
    Dec 2003
    Location
    poulsbo, wa, usa
    Posts
    910
    Post Thanks / Like
    Likes (Given)
    67
    Likes (Received)
    393

    Default

    I know haas and mori has a single pass code,, you well need to start the code at the same RPM , spot in Z and I think spot you stopped at in X ,, but you still might be off in that most of the time when you program a G76 code you program it to cut at a 29* infeed angle ,, that well change were your would be on the finish pass in Z ...

  3. #3
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    678
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    327

    Default

    So by the looks of it, the answer is no. LOL

  4. #4
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,875
    Post Thanks / Like
    Likes (Given)
    331
    Likes (Received)
    1905

    Default

    Quote Originally Posted by cuttergrinder View Post
    So by the looks of it, the answer is no. LOL
    Actually, the answer is absolutely a YES!
    Finish OD + Thread + Chase OD + Chase Thread.

    In the Chase Thread operation use everything from the Thread cycle, but on the second line of the G76 make the Q value to be the same as the P value.
    If you want 2 spring passes ( I do ) then make Q to be .0001 or so smaller than P.

    On a Haas it is even easier and better, but that is not what you've asked for.

  5. #5
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    820
    Post Thanks / Like
    Likes (Given)
    77
    Likes (Received)
    281

    Default

    Quote Originally Posted by SeymourDumore View Post
    Actually, the answer is absolutely a YES!
    Finish OD + Thread + Chase OD + Chase Thread.

    In the Chase Thread operation use everything from the Thread cycle, but on the second line of the G76 make the Q value to be the same as the P value.
    If you want 2 spring passes ( I do ) then make Q to be .0001 or so smaller than P.

    On a Haas it is even easier and better, but that is not what you've asked for.
    what he said ^^
    dont forget if your using a 2 line code the number of finsh pass's need to be changed or added as well.

    I set my main thread set to run 2 finish passes(spring pass) the chamfer and od chase then in my last thread set I put only 1 in.

  6. #6
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    678
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    327

    Default

    Quote Originally Posted by SeymourDumore View Post
    Actually, the answer is absolutely a YES!
    Finish OD + Thread + Chase OD + Chase Thread.

    In the Chase Thread operation use everything from the Thread cycle, but on the second line of the G76 make the Q value to be the same as the P value.
    If you want 2 spring passes ( I do ) then make Q to be .0001 or so smaller than P.

    On a Haas it is even easier and better, but that is not what you've asked for.
    So I assume doing this will still allow the machine to line up with the original thread? Also for normal 60 threads, do you use 60 for the thread angle or do you use 30 like you would on a manual lathe(actually I usually use 29 1/2 on a manual). Or do you have program it at 0 degrees if you want to run a finish later? Sorry for the questions but I have to have this this all figured out before I pop a 12' shaft in this lathe that needs threads. Something small if I messed it up wouldn't be a big deal, but scrapping a 12" dia. x 12' long shaft is quite another.

  7. #7
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    3,835
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1728

    Default

    Quote Originally Posted by D.D.Machine View Post
    ... most of the time when you program a G76 code you program it to cut at a 29* infeed angle ...
    I used to do that, coming from an engine lathe and all, then one day my Sandvik guy said, "Don't do that !"

    Using full form threading inserts, he said they work better and last longer if you come straight in. So I tried it and he was right.

  8. #8
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,777
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1481

    Default

    Quote Originally Posted by cuttergrinder View Post
    So I assume doing this will still allow the machine to line up with the original thread? Also for normal 60 threads, do you use 60 for the thread angle or do you use 30 like you would on a manual lathe(actually I usually use 29 1/2 on a manual). Or do you have program it at 0 degrees if you want to run a finish later? Sorry for the questions but I have to have this this all figured out before I pop a 12' shaft in this lathe that needs threads. Something small if I messed it up wouldn't be a big deal, but scrapping a 12" dia. x 12' long shaft is quite another.
    Hello cuttergrinder,
    Its as Seymour suggests with regards to taking an additional pass (passes) at full depth, the Q value is specified with the P value of the 2nd G76 Block.

    The angle specified if you want only the Leading Edge of the insert to cut is the Included Angle of the Thread Form (the included angle of the Threading Insert), not the Angle/2. Specifying any angle less than the Included Angle of the Thread Form will have the Insert cutting on both the Leading and Trailing Edge, but more on the Leading Edge until a Zero value is specified. At Zero, the same amount is cut by the Leading and Trailing edge of the insert.

    In addition to ensuring that the same Z Start Point and Spindle Revs be used when repeating a G76 Threading Cycle, when programming to take an additional pass at full depth with another G76 Cycle, its important that the same Angle and Thread Height that was specified in the "Threading from Scratch" G76 Cycle be specified in the full depth repeat G76 cycle. The control uses the following algorithm to calculate a forward shift of the tool at the Start to accommodate a Thread Form Angle specified in the G76 Block

    ZShift = TAN(A/2) x (d x sqr(n))

    Where:
    A = Include Thread Angle specified
    d = First Pass DOC (Q Value of 2nd G76 Block)
    n = nth number of Threading Pass (1st, 2nd, 3rd and so on)

    It progresses this way until d x sqr(n) - d x sqr(n-1) is less than the Minimum DOC that is specified (set). Ultimately, the DOC will equal the Thread Height, therefore, if the same Thread Form Angle and Thread Height is used in both G76 Cycles, then the Threading Tool will track the same path.

    Regards,

    Bill
    Last edited by angelw; 02-11-2020 at 02:22 PM.

  9. #9
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    678
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    327

    Default

    Thanks everyone. As always much very useful information.

  10. #10
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    678
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    327

    Default

    Years ago we made some figure 8 grease grooves in some bushings by using g code inside of a Mazatrol program on a Mazak lathe. If I was to do this on a Fanuc, Im thinking I can use G32. Am I correct. When we programmed the Mazak we made the spindle turn 1/2 revolution while it was moving minus in z and then another 1/2 rev. while moving in +Z. Then there we would increase the depth of the tool a small amount and just keep repeating this until it was to depth. It worked well but we had to write all the code by hard. Im assuming you could use a macro to increase the tool depth after one cycle. I remember we had to make the lead exact so that the spindle would turn exactly 1/2 turn while moving -in Z. If not it would make multiple figure 8 grooves in the bushing.

  11. #11
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,257
    Post Thanks / Like
    Likes (Given)
    4790
    Likes (Received)
    1647

    Default

    Quote Originally Posted by SeymourDumore View Post
    Actually, the answer is absolutely a YES!
    Finish OD + Thread + Chase OD + Chase Thread.

    In the Chase Thread operation use everything from the Thread cycle, but on the second line of the G76 make the Q value to be the same as the P value.
    If you want 2 spring passes ( I do ) then make Q to be .0001 or so smaller than P.

    On a Haas it is even easier and better, but that is not what you've asked for.
    I wasn't able to get this to work. Least I could get was two passes. Curious you have actually stood there and watched your 0i-TC run the two line G76 cycle in 1 single pass?

    Brent

  12. #12
    Join Date
    Mar 2003
    Location
    Upstate New York USA
    Posts
    287
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    44

    Default

    it will always generate 2 passes, 1 at full depth and then 1 spring pass. It is how the FANUC works

  13. #13
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,875
    Post Thanks / Like
    Likes (Given)
    331
    Likes (Received)
    1905

    Default

    Quote Originally Posted by yardbird View Post
    I wasn't able to get this to work. Least I could get was two passes. Curious you have actually stood there and watched your 0i-TC run the two line G76 cycle in 1 single pass?

    Brent
    Brent, no, I couldn't make the damn thing do one pass only, minimum is two.
    And yet, the very very same code on the Mits MSX 850 will make a single pass chase.
    There's gotta be some parameter sticking in the Oi to force an additional pass on the same X.

  14. #14
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,257
    Post Thanks / Like
    Likes (Given)
    4790
    Likes (Received)
    1647

    Default

    Quote Originally Posted by SeymourDumore View Post
    Brent, no, I couldn't make the damn thing do one pass only, minimum is two.
    And yet, the very very same code on the Mits MSX 850 will make a single pass chase.
    There's gotta be some parameter sticking in the Oi to force an additional pass on the same X.
    Yeah me neither! Thanks for testing this on your machine, beginning to think people thinking I'm crazy. It very well could be a parameter but I've never run across anything listed that would make you think so.


    My guess is that the G76 cycle is in the "functions to simplify programming" section of operator's manual listed as a "multiple repetitive cycle". By definition multiple would suggest more than one. Only thing I can figure is if you wanted to run one thread pass Fanuc intended the user to use one of the other threading codes? Like I say that's just horseshit I dreamed up. Unless someone finds a parameter or something, that's all I got. Lol

    Brent

  15. #15
    Join Date
    Mar 2003
    Location
    Upstate New York USA
    Posts
    287
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    44

    Default

    been running FANUC controls for over 30 years for a machine tool builder and have never been able to make only one pass with a G76 cycle, there are no known parameters that I am aware of I believe it is something internal to the FANUC cycle and they way that this war written internally
    Tom


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
  •