Results 1 to 3 of 3

Thread: taper thread cutting programme

  1. #1
    Join Date
    Jun 2009
    Posts
    7
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Question taper thread cutting programme

    Sir,
    i need taper thread cutting programme in cnc turning center for any npt pipe threads.

  2. #2
    Join Date
    Apr 2009
    Location
    Kansas
    Posts
    82
    Thanks
    0
    Thanked 6 Times in 6 Posts

    Default Re: taper thread cutting programme

    Hope this helps
    This was made from 3/4 bar stock
    O1234(1/8-27 NPT)
    N10G54T0202
    G50S2000
    G96S600M4
    G0X.85Z0M8
    G1X-.062F.003
    G0X.65Z.05
    G1Z-1.5F.006
    X.7
    G0Z.05
    X.55
    G1Z-1.5
    X.6
    G0Z.05
    X.45
    G1Z-.95
    X.5
    G0.05
    X.25
    G1Z0
    X.373Z-.03F.0015(CHANFER)
    X.397Z-.35F.006(THREAD TAPER)
    Z-.95
    X.48
    X.54Z-1.015
    Z-1.5
    G0X6.Z6.
    M1
    N20T0303
    G97S1000M3
    G0X.525Z.5M8
    G76P010055Q0010R0005
    G76X.36Z-.35P0150Q0050R-0200F.0357
    G0X8.Z8.
    M30
    %

    G76- Canned threading cycle

    G76 P010060 Q.002 R.0005 (first G76 sets parameters for threading)
    G76 X Z P Q F R (cuts the thread)

    The first G76 isn't needed but is recommended.
    - G76 P Q R

    P010060 sets 3 things
    - first 2 digits is the amount of finish passes - 01

    - second 2 digits is % of the lead or pullout exiting the thread- 00
    00 = almost no angle at pullout and 99 = 9.9 leads away start out

    - third 2 digits are the angle of infeed - 60
    0,29,30,55,60,80 are usable (0-90 is ok)

    Q.005 sets the minimum cut amount during threading

    R.0005 sets the cut amount of the last pass

    The second G76 cuts the thread.
    -G76 X.1876 Z.3 P.0302 Q.01 F.05 (R-.002) FOR 1/4-20

    X.1876 =Minor Dia. of thread

    Z.3 or (W) =The ending Z of the thread

    P.0302 =Height of thread in radius (Maj-Min)/2

    Q.01 =Amount of the first cut. All the rest of the cuts are calculated.

    F.05 =Feed-rate 20 TPI 1/20=.05

    R = R is optional for tapered threading. R is the amount of
    difference in X from start to finish in Z. When cutting threads
    moving Z and X in a positive direction R is a negative value.
    Last edited by chucker; 06-16-09 at 08:35 AM. Reason: added info

  3. #3
    Join Date
    Aug 2012
    Posts
    2
    Thanks
    1
    Thanked 0 Times in 0 Posts

    Default Re: taper thread cutting programme

    I need to program a 1/4-18 pipe thread in my Haas Lathe.

Similar Threads

  1. Transfert de programme
    By SMARA in forum Automation & Interfacing / Installation / Ladder logic
    Replies: 2
    Last Post: 07-06-10, 01:37 PM
  2. Re: taper thread cutting programme
    By joeybetsy in forum Programming / Applications
    Replies: 1
    Last Post: 06-16-09, 07:38 AM
  3. tool mark when cutting taper
    By thelonegunmen in forum Mori Seiki Lathes & Mills
    Replies: 4
    Last Post: 02-11-09, 07:26 AM
  4. thread mill programme
    By niallmeg in forum Programming / Applications
    Replies: 1
    Last Post: 04-01-08, 07:19 AM
  5. can you identify a problem with this programme please.
    By martin in forum General CNC & Manufacturing Discussion
    Replies: 2
    Last Post: 11-08-07, 05:11 PM

Posting Permissions

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