Need Help! 1/2-14 NPT Programming


Results 1 to 5 of 5

Thread: 1/2-14 NPT Programming

  1. #1
    Registered
    Join Date
    Apr 2010
    Location
    USA
    Posts
    14
    Downloads
    0
    Uploads
    0

    Default 1/2-14 NPT Programming

    Could anyone copy and paste an good example of code for the profile and threading for an external 1/2-14 NPT using the single line G76 cycle? Its for a Haas TL2, .031R turning tool, 60 DEG non-topping threading insert. I don't think the infeed angle (plunge/flank-cut) matters for the numbers I'm after but I could be wrong about that. Sorry if I look like a big dummy but I'm not confident of the numbers I come up with from the dimensions given in the machinist's handbook. Thanks Guys.

    Similar Threads:


  2. #2
    Registered
    Join Date
    May 2007
    Location
    USA
    Posts
    941
    Downloads
    0
    Uploads
    0

    Default

    This is for a Fanuc


    X.88Z.3
    G76X.7479Z-.8285K.0571D150I-.0347F.071429A50.

    HTH

    EDIT: Oops. Just noticed you also want the profile. This is an old sucker. Hope it is right. Okay, laid it out in MC to double check it.


    N200M91 (ROUGH TURN THREAD 1/32R TOOL)
    T0202S3000M3
    X.9Z.005
    G1X.2F.01
    Z.02
    G0X.85
    G1Z-.1
    U.02
    Z.02F.015
    X.6191
    X.8289Z-.0849F.01
    X.85Z-.4234
    Z-.87
    X.87
    M92
    M1

    N400M91 (FINISH TURN THREAD 1/64R TOOL)
    T0404S3000M3
    X.7Z.02
    G1Z0F.01
    X.25F.003
    Z.02F.015
    G0X.63
    G1X.6451Z.005
    Z0F.002
    G3X.6748Z-.0062R.021
    G1X.8194Z-.0785F.003
    X.84Z-.4088F.006
    Z-.875F.003
    X.86
    M92
    M1

    Last edited by g-codeguy; 08-31-2011 at 01:55 PM.


  3. #3
    Registered hutch07's Avatar
    Join Date
    Sep 2007
    Location
    usa
    Posts
    105
    Downloads
    0
    Uploads
    0

    Default Re: 1/2-14 NPT Programming

    ½ - 14 NPT Male thread Inch Programming

    Thread Pitch 0.07142 Thread Taper 1:16 on Diameter
    Thread Height 0.05714” Root Diameter at start 0.6977
    Root at finish 0.7485”


    T0909 (THREAD)
    G90 G00 X1.25 Z0.2
    G01 X0.88 Z0.15
    G76 P010060
    G76 X0.7485 Z-0.812. P0571 R-0.0301 Q0200 F0.07142



  4. #4
    Gold Member
    Join Date
    Feb 2006
    Location
    india
    Posts
    1531
    Downloads
    0
    Uploads
    0

    Default Re: 1/2-14 NPT Programming

    Q and R words in the first block specify min DOC and finishing allowances, respectively.



  5. #5
    Registered
    Join Date
    May 2007
    Location
    USA
    Posts
    941
    Downloads
    0
    Uploads
    0

    Default Re: 1/2-14 NPT Programming

    Quote Originally Posted by hutch07 View Post
    ½ - 14 NPT Male thread Inch Programming

    Thread Pitch 0.07142 Thread Taper 1:16 on Diameter
    Thread Height 0.05714” Root Diameter at start 0.6977
    Root at finish 0.7485”

    T0909 (THREAD)
    G90 G00 X1.25 Z0.2
    G01 X0.88 Z0.15
    G76 P010060
    G76 X0.7485 Z-0.812. P0571 R-0.0301 Q0200 F0.07142
    Wow. Old thread. The example I gave was for a Fanuc control. No Haas in the shop. .15 is a 2 revolution lead. Enough I suppose, but I prefer at least .3. Doubt you will see a difference in cycle time. Using Fanuc G76 for examples, the .02 is a hefty first cut depending on material. If there is no under-cut behind the thread, you might want to consider making this change...P010160 The second 01 will have the insert pulling out at the end of the cut as fast as the machine will allow. A P000029 or P010060 will keep the insert down in the cut for one revolution at the final end point...ringing the thread.. I only use a compound infeed of 60 when having a chatter problem. Normally I use...P000129. I seldom use a spring pass because we almost always deburr the thread and re-thread so I don't need an extra spring pass on the original thread cycle.

    If the Haas G76 is the same as a Fanuc G76, you might want to also consider something like this...P000129Q30R.001. As Sinha posted the Q30 clamps DOC at .003 per side once the control's math figures a cut less than .003 DOC. The R.001 makes the final cut at .001 DOC.

    For anyone considering programming using Macro B, I can highly recommend Sinha's book.



Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

1/2-14 NPT Programming
1/2-14 NPT Programming