G76 Tapered Thread Cycle
Close
Login to Your Account
Results 1 to 16 of 16
  1. #1
    Join Date
    Jul 2011
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    324
    Post Thanks / Like
    Likes (Given)
    69
    Likes (Received)
    38

    Default G76 Tapered Thread Cycle

    So in my shop I cut pretty much 99.9% straight thread. But I have a customer who wants 150 1/2"NPT male threads single pointed. But all the thread cycles ive tried are being a pain in the butt and I get 6 parts and the insert chips. Does anyone have a 2 line g76 I could use as a guide to set it up. Ive tried using the G32 for the taper and its pretty much worthless as it doesnt seems to wanna read on my machine. Thanx in Advance.

    P.S. I thread a lot and never have issues. This thread is just giving me a fit.

  2. #2
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,424
    Post Thanks / Like
    Likes (Given)
    5026
    Likes (Received)
    1759

    Default

    You do like all the straight threads but you add a R to the second line. It's the distance in radius value of the total Z move. If nobody shows up with one and if I remember can post an example when I get in tonight.

    Brent

  3. Likes nissan300ztt liked this post
  4. #3
    Join Date
    Jul 2011
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    324
    Post Thanks / Like
    Likes (Given)
    69
    Likes (Received)
    38

    Default

    thanx the machine I usually use only accepts g92 thread cycles. Our newer machine doesnt get much threading work. And like anything else you dont use your programming skills you forget sometimes.

  5. #4
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    216
    Post Thanks / Like
    Likes (Given)
    532
    Likes (Received)
    57

    Default

    What is the material? Maybe the first pass is too heavy and is killing inserts prematurely. Are you turning the taper before you thread?
    I always use G92 cycle with NPT threads.

  6. #5
    Join Date
    Jul 2011
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    324
    Post Thanks / Like
    Likes (Given)
    69
    Likes (Received)
    38

    Default

    Quote Originally Posted by Fancuku View Post
    What is the material? Maybe the first pass is too heavy and is killing inserts prematurely. Are you turning the taper before you thread?
    I always use G92 cycle with NPT threads.
    Nope. Customer specifically gave us print yo not turn the angle. .840" diameter. And first cut is only .003". Material is 304ss. And I didnt know you could use a g92 to do a tapered thread.

    Sent from my LM-V600 using Tapatalk

  7. #6
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,424
    Post Thanks / Like
    Likes (Given)
    5026
    Likes (Received)
    1759

    Default

    My day shit counterpart makes a bunch of these. I myself don't make them. They are for inhouse use. Butter them up with pipe dope and wrencher down. He is cutting the taper before chasing the threads. You never say but this is run on a i series Fanuc control.

    Brent

    N50(1/2-14 NPT)

    G0G99G40G54X12.Z7.T0
    T0707
    G97S300M3
    G0X6.Z.1
    G0X1.05Z.1M8
    G76P030060Q0070R0
    G76X.755Z-.80R-0360P0570Q0070F.07142
    G0X7.M9
    G0G40X12.Z7.T0
    M1

    20210509_235945.jpg
    20210510_000623.jpg

  8. #7
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,117
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1740

    Default

    Quote Originally Posted by nissan300ztt View Post
    Nope. Customer specifically gave us print yo not turn the angle. .840" diameter. And first cut is only .003". Material is 304ss. And I didnt know you could use a g92 to do a tapered thread.

    Sent from my LM-V600 using Tapatalk
    Hello nissan300ztt,
    Some people just don't have a clue. By not permitting the taper to be turned is simply making the part considerably harder to make and you would have to use a full form threading insert, or stuff around cutting the crest of the thread by cutting the taper again after the thread was cut.

    You could cut the taper before screw cutting, leaving the diameter of the taper up on size and it would be impossible to tell if the thread was cut with the taper pre-cut or not.

    Taper cutting with G92 uses the same type of "R" argument as G76, representing the amount of radial difference in the taper from where the tool starts in fresh air in Z at the start of the thread, to the Z finish point of the thread. Following is the syntax for cutting a taper thread with G92.

    G92X__ Z__ R__ F__

    Where:
    X = X coordinate for thread pass at the large diameter of the taper (male thread).
    Z = Z Finish Point of thread.
    R = Radial amount of taper between Z start and Z finish point and will be in a minus direction when cutting a male thread.

    Not cutting the Taper will make using the G76 cycle difficult. The X specified in the G76 cycle is the Minor Diameter of the Thread at the large diameter of the taper. The first pass of the threading cycle takes a specified first DOC amount. This amount would be applied at the large diameter of the taper, and at the small end of the taper, if it had been cut, by the "R" argument specified in the cycle. If the taper is not cut, the tool will start with a DOC at the start of the thread equal to the first DOC amount, plus the amount of radial taper. In Brent's example in Post #6, that DOC for the first pass would start at 0.043" at the start of the thread and wash out to 0.007" at the Z Finish point, large diameter of the thread. I would not be surprised to see the insert break on the first pass.

    The same difficulty would apply with the G92, with either a lot of air cutting, or a more difficult programming project than it needs to be, by programing specific X and Z values for the first part of the taper until down to a diameter where the last part of the thread can start to be cut.


    Regards,

    Bill

  9. Likes nissan300ztt, TeachMePlease liked this post
  10. #8
    Join Date
    Jul 2011
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    324
    Post Thanks / Like
    Likes (Given)
    69
    Likes (Received)
    38

    Default

    So I was put back on this job today and ended up email the engineer in charge of this job and explained the situation and they said cutting the taper was fine. LOL. I need to get out my programming books again its been a long time since I used some of these thread canned cycles. Thanx for all the input.

  11. #9
    Join Date
    Jul 2011
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    324
    Post Thanks / Like
    Likes (Given)
    69
    Likes (Received)
    38

    Default

    Quote Originally Posted by yardbird View Post
    My day shit counterpart makes a bunch of these. I myself don't make them. They are for inhouse use. Butter them up with pipe dope and wrencher down. He is cutting the taper before chasing the threads. You never say but this is run on a i series Fanuc control.

    Brent

    N50(1/2-14 NPT)

    G0G99G40G54X12.Z7.T0
    T0707
    G97S300M3
    G0X6.Z.1
    G0X1.05Z.1M8
    G76P030060Q0070R0
    G76X.755Z-.80R-0360P0570Q0070F.07142
    G0X7.M9
    G0G40X12.Z7.T0
    M1

    20210509_235945.jpg
    20210510_000623.jpg
    That program worked great. Thanks for the information. Engineer was very happy with the outcome.

  12. #10
    Join Date
    Jul 2019
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    4,081
    Post Thanks / Like
    Likes (Given)
    3969
    Likes (Received)
    796

    Default

    Quote Originally Posted by nissan300ztt View Post
    So in my shop I cut pretty much 99.9% straight thread. But I have a customer who wants 150 1/2"NPT male threads single pointed. But all the thread cycles ive tried are being a pain in the butt and I get 6 parts and the insert chips. Does anyone have a 2 line g76 I could use as a guide to set it up. Ive tried using the G32 for the taper and its pretty much worthless as it doesnt seems to wanna read on my machine. Thanx in Advance.

    P.S. I thread a lot and never have issues. This thread is just giving me a fit.
    Understand the frustration. Tapered threads they only need to be done right either on lathe or mill with threaders which is my preferred method on them.


    Dang insert? You could use more passes most likely. Material and quality of insert are known variables too the simple variety. Also you might rough thread it then finish thread it with a another threader. That way the chipped insert can actually keep being used. I think it is best to salve that problem completely.

    At the least pace your threading inserts and check for the chipped insert before removing the part. That way you can back off and clean up the threads likely where the chipped tooth left material.

    Don’t do things dirty allow some good machining practices. At least you can determine the rate at which that insert stops giving you good threads and change it before it chips at least.

  13. #11
    Join Date
    Jun 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,524
    Post Thanks / Like
    Likes (Given)
    812
    Likes (Received)
    665

    Default

    G76 can cut tapered - insert an "R" value in the line with the taper amount. "R-" will taper upwards towards the rear, "R+" will taper downwards.

  14. Likes nissan300ztt liked this post
  15. #12
    Join Date
    Jul 2011
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    324
    Post Thanks / Like
    Likes (Given)
    69
    Likes (Received)
    38

    Default

    Quote Originally Posted by DouglasJRizzo View Post
    G76 can cut tapered - insert an "R" value in the line with the taper amount. "R-" will taper upwards towards the rear, "R+" will taper downwards.
    Yeah I know just wasnt sure the actual values for the 1/2" NPT. I got it sorted.

  16. #13
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,117
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1740

    Default

    Quote Originally Posted by nissan300ztt View Post
    Yeah I know just wasnt sure the actual values for the 1/2" NPT. I got it sorted.
    Hello nissan300ztt,
    The easiest algorithm to use in calculating the R value to use in the G76 Cycle is:

    R = Z x 0.03125

    Where:
    Z = Total Z move of the tool
    0.03125 = Radial Constant for diameter taper of 1:16

    Regards,

    Bill

  17. Likes nissan300ztt liked this post
  18. #14
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    245
    Post Thanks / Like
    Likes (Given)
    146
    Likes (Received)
    48

    Default

    refer to this thread I posted a couple weeks ago. This may help you out. We do threading on Mitsubishi Meldas 500 controller so the format may be different from yours but it is very similar to fanuc.

    Help with writing 1/8 NPT G76 threading cycle.

  19. #15
    Join Date
    Jun 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,524
    Post Thanks / Like
    Likes (Given)
    812
    Likes (Received)
    665

    Default

    Quote Originally Posted by nissan300ztt View Post
    Yeah I know just wasnt sure the actual values for the 1/2" NPT. I got it sorted.
    Cool! Glad to hear it. It works pretty well. Yeah, G32 and G92 can give more "control" but with a zillion lines of code. I use G76 whenever possible.

  20. #16
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,372
    Post Thanks / Like
    Likes (Given)
    75
    Likes (Received)
    262

    Default

    Quote Originally Posted by angelw View Post
    Hello nissan300ztt,
    The easiest algorithm to use in calculating the R value to use in the G76 Cycle is:

    R = Z x 0.03125

    Where:
    Z = Total Z move of the tool
    0.03125 = Radial Constant for diameter taper of 1:16

    Regards,

    Bill
    I use Z/32 which is easier to remember.

  21. Likes nissan300ztt 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
  •