Page 1 of 2 12 LastLast
Results 1 to 20 of 34
  1. #1
    laminar-flow is offline Stainless
    Join Date
    Jan 2003
    Location
    Pacific Northwest
    Posts
    1,019

    Default Any tips on single point NPT ID and OD threads

    I have the gauges, well at least a L-1 OD and L-1 and L-3 ID.

    Small stuff, 1/8 and 1/4.

    Any been there done thats would be appreciated.

  2. #2
    SeymourDumore is offline Diamond
    Join Date
    Aug 2005
    Location
    CT
    Posts
    6,304

    Default

    Whuh! That's a little broad question.
    You're interested in gaging or setting up and making the threads?

    For starters maybe, the taper amount is measured from the end of the thread to the beginning of the thread. This means an OD NPT will have a negative taper, while the ID NPT will have a positive taper amount.

    That was my WTF dilemma the first time.

    But as I've said, may want to narrow your question a little.

  3. #3
    laminar-flow is offline Stainless
    Join Date
    Jan 2003
    Location
    Pacific Northwest
    Posts
    1,019

    Default

    I'm need to cut some ID and OD NPT threads occasionally in Aluminum and Plastic.

    Just wanted to check it there were any thing to watch out for.

  4. #4
    SeymourDumore is offline Diamond
    Join Date
    Aug 2005
    Location
    CT
    Posts
    6,304

    Default

    Maybe not as straight forward as standard threads, but it's still just a thread.
    I always turn/bore the taper to 3/4"/foot, never just use a drill.
    Then I draw the start and end points of the minor in CAD, get the radial difference for the taper amount to plunk in the G76 cycle.
    REMEMBER! The start and end points if your TOOL that's important.
    IOW if you start threading .1 from the face and thread .2 beyond the L3 length, you HAFTA! use those X values in the cycle!!!

  5. #5
    sinha is offline Cast Iron
    Join Date
    Sep 2010
    Location
    india
    Posts
    278

    Default

    For more information on G76, which you actually need to use, look at the other thread on G76:
    Thread using g76

  6. #6
    Gary E is offline Diamond
    Join Date
    Jan 2006
    Location
    Houston, TX
    Posts
    5,860

    Default

    Quote Originally Posted by laminar-flow View Post
    I'm need to cut some ID and OD NPT threads occasionally in Aluminum and Plastic.

    Just wanted to check it there were any thing to watch out for.

    Small stuff, 1/8 and 1/4.

    Any been there done thats would be appreciated.

    THAT's why TAPS and Dies are made

  7. #7
    laminar-flow is offline Stainless
    Join Date
    Jan 2003
    Location
    Pacific Northwest
    Posts
    1,019

    Default

    Seymour,

    "Then I draw the start and end points of the minor in CAD, get the radial difference for the taper amount to plunk in the G76 cycle."

    Should that not always be the same, the taper amount?

    "REMEMBER! The start and end points if your TOOL that's important."

    I assume you meant "of" your tool.

    "IOW if you start threading .1 from the face and thread .2 beyond the L3 length, you HAFTA! use those X values in the cycle!!!"

    Doesn't the G76 start away from the start point with a bit of dwell anyway?

  8. #8
    <jbc>'s Avatar
    <jbc> is offline Titanium
    Join Date
    Jun 2011
    Location
    Oberaargau Switzerland
    Posts
    2,268

    Default

    Generally speaking, the finished male part should be softer than the female, if you expect to screw the female more than a few times.

  9. #9
    SeymourDumore is offline Diamond
    Join Date
    Aug 2005
    Location
    CT
    Posts
    6,304

    Default

    Quote Originally Posted by laminar-flow View Post
    Seymour,

    A:
    Should that not always be the same, the taper amount?

    B:
    I assume you meant "of" your tool.


    C:
    Doesn't the G76 start away from the start point with a bit of dwell anyway?

    A: Nope!!! The taper amount is dependent on where you start from and where you end. The actual taper is the radial difference between those, the ACTUAL start X and the ACTUAL finish X points.

    B: Yup, thick finger syndrome and dyslexia is a common occurrence here.

    C: Nope, the G76 cycle starts from where you positioned the tool JUST BEFORE the cycle is invoked.

  10. #10
    SeymourDumore is offline Diamond
    Join Date
    Aug 2005
    Location
    CT
    Posts
    6,304

    Default

    Quote Originally Posted by Gary E View Post
    THAT's why TAPS and Dies are made

    Gary, care to see some drawings where the notes explicitly require SINGLE POINT THREADING for the ports?
    Threadmill is allowed, tap and dies are not.
    Similarly, you just ain't gonna make an acceptable NPT thread for aircraft standards with a die. Tap, maybe, but certainly not a die.

  11. #11
    gorrilla is offline Stainless
    Join Date
    May 2007
    Location
    Central Texas, West and North of Austin
    Posts
    1,191

    Default

    Quote Originally Posted by laminar-flow View Post
    I have the gauges, well at least a L-1 OD and L-1 and L-3 ID.

    Small stuff, 1/8 and 1/4.

    Any been there done thats would be appreciated.
    You doing this on a lathe, since your talking about single pointing. There is a process for doing it in a mill, with the tool following the lead and the taper. Never done it,looks like a tremendous PIA, only practical on ginormous threads, IMO.
    So that leaves us with the subject at hand. I was going to suggest thread milling, but your in a lathe obviously, and not one with live tooling?
    What Seymour is trying to communicate is for you to be sure you account for the full Z travel, including your amount that you start from in front of the thread, plus the amount you run past the thread. Programming for only the taper amount(3/4/inch), then moving say .2 longer than the part, in order to start and finish in the clear, would give you an incorrect taper. Bad part is, depending on how much you missed it, you might not notice it with your gauging. Can you say "scrap"?
    I like to start my G76 about .1 in front of the part, in order for the machine to have plenty of room to get the lead worked out. Old habit really, from doing this on a manual with a taper attachment. CNC with it's ball screws and encoder can start much closer. How far you run out the ack of the thread is up to you and whether there's a shoulder back there. But with the sizes your talking about, tool length is gonna have a lot to do with it also.
    I agree with the idea of tapering the raw hole before you thread it. Sidesteps a lot of problems, again with that tiny tool, you need all the help you can get.
    In your G76 cycle, assuming you use the two line version ,the taper is in the R dimension, in the second line. Expressed in a radius. This is where you program the taper in your threads. Just remember to trig out how much taper you need for the full amount of Z travel your tool will encounter, whether it's actually making chips the whole way or not. As you can probably tell, I program this stuff in longhand, with no CAM. We use what we have.

  12. #12
    litlerob's Avatar
    litlerob is offline Hot Rolled
    Join Date
    Jun 2009
    Location
    PDX, OR
    Posts
    547

    Default

    You don't need to "trig" anything out. The taper amount is .75 per foot or .0625 per inch, so if you are traveling 2" along the Z axis than your taper amount is going to be .125 radially. If you are travelling .1" plus 2 " because you are starting .1 in front of the part than the taper amount would be .1313

    Robert

  13. #13
    sinha is offline Cast Iron
    Join Date
    Sep 2010
    Location
    india
    Posts
    278

    Default

    Quote Originally Posted by litlerob View Post
    ..if you are traveling 2" along the Z axis than your taper amount is going to be .125 radially...
    .125 is diff in radius or dia?

  14. #14
    Kyle Smith's Avatar
    Kyle Smith is online now Hot Rolled
    Join Date
    Apr 2008
    Location
    Helmer, Indiana, USA
    Posts
    940

    Default

    Quote Originally Posted by <jbc> View Post
    Generally speaking, the finished male part should be softer than the female, if you expect to screw the female more than a few times.
    Its been my experience the male part should be harder than the female if you expect to screw it more than a few times.

  15. #15
    laminar-flow is offline Stainless
    Join Date
    Jan 2003
    Location
    Pacific Northwest
    Posts
    1,019

    Default

    Hi,

    Here is what we ended up with. Thanks for the help and please comment.

    (1/8-27 NPT FITTING)

    (RUN TOOL 1 TO SET STOCK)
    T101
    G54
    G00 X0.2
    G00 Z0.04
    M00

    M08

    (END FACE)
    T101
    G54
    G50 S2000
    G96 S250 M03
    G00 Z0.2
    G00 X0.6
    G00 Z0.04
    G72 P401 Q402 U0 W0 D0.01 F0.002
    N401 G00 Z0.
    G01 X0.6
    N402 G01 X-0.01
    Z0.05
    G00 X0.6
    M01

    (OD TURN)
    T101
    G54
    G50 S2500
    G96 S250 M03
    G00 X0.6
    G00 Z0.
    G71 P201 Q202 U0.001 W0.001 D0.01 F0.003
    N201 G01 X0. F0.002
    G01 Z0.
    G01 X0.329
    G01 X0.39 Z-0.03
    G01 X0.408 Z-0.32
    G01 X0.408 Z-0.405
    G01 X0.55
    G40
    G01 X0.6
    N202

    G42 (TNC RIGHT ON)
    G70 P201 Q202 (FINISH PASS)
    G00 Z1.

    (OD THREAD)
    T202
    G54
    G97 S500 M03
    G00 X0.475
    Z0.
    G04 P1.
    M08
    M23
    G76 X0.3314 Z-0.32 K0.03 I-0.01 D0.002 F0.037
    G00 X0.475 Z0.1
    G00 X0.6
    G00 Z1.
    M01

    (OD CLEANUP)
    T101
    G54
    G50 S2500
    G96 S250 M03
    G00 X0.6
    G00 Z0.
    G42 (TNC RIGHT ON)
    G70 P201 Q202 (FINISH PASS)

    G00 Z1.
    (OD THREAD CLEAN)
    T202
    G54
    G97 S500 M03
    G00 X0.475
    Z0.
    G04 P1.
    M08
    M23
    G76 X0.3314 Z-0.32 K0.002 I-0.01 D0.0005 F0.037
    G00 X0.475 Z0.4
    G00 X0.6
    G00 Z1.
    M01

    M09
    G00 X0.6
    G00 Z3.
    M30

  16. #16
    SeymourDumore is offline Diamond
    Join Date
    Aug 2005
    Location
    CT
    Posts
    6,304

    Default

    Quote Originally Posted by laminar-flow View Post

    (OD THREAD)
    T202
    G54
    G97 S500 M03
    G00 X0.475
    Z0.
    G04 P1.
    M08
    M23
    G76 X0.3314 Z-0.32 K0.03 I-0.01 D0.002 F0.037
    G00 X0.475 Z0.1
    G00 X0.6
    G00 Z1.
    M01

    You're being a little ambitious with starting at Z0 me thinks.

  17. #17
    litlerob's Avatar
    litlerob is offline Hot Rolled
    Join Date
    Jun 2009
    Location
    PDX, OR
    Posts
    547

    Default

    Quote Originally Posted by sinha View Post
    .125 is diff in radius or dia?
    Right!! one is a bone in your arm, and one is a Defense Intelligence Agency.

  18. #18
    laminar-flow is offline Stainless
    Join Date
    Jan 2003
    Location
    Pacific Northwest
    Posts
    1,019

    Default

    Seymour, Yes I was thinking the same, but with the chamfer it seemed to be just fine.

    Is that not a good idea and for what reason?

    To do it with a lead in, it will require just some more CAD work.

  19. #19
    TURNMASTER1 is offline Plastic
    Join Date
    Dec 2010
    Location
    Eastern Washington, USA
    Posts
    29

    Default

    Quote Originally Posted by laminar-flow View Post
    Seymour, Yes I was thinking the same, but with the chamfer it seemed to be just fine.

    Is that not a good idea and for what reason?

    To do it with a lead in, it will require just some more CAD work.
    No, It will take no more CAD work, just move the Z start to Z.2 in both Thread cycles.

    If you use the cad for this you are making it to hard.

    The reason is to give the machine time to become in sync with itself, the importance increases as the rpm and coarseness of the thread increase. Relates to the machines ability to follow the same path each time and it removes thread lead error.

    Jeff

  20. #20
    SeymourDumore is offline Diamond
    Join Date
    Aug 2005
    Location
    CT
    Posts
    6,304

    Default

    Quote Originally Posted by TURNMASTER1 View Post
    No, It will take no more CAD work just move the Z start to Z.2 in both Thread cycles.

    If you use the cad for this you are making it to hard.

    Jeff

    DEAD WRONG!!!!

    Moving the Z in the + direction WILL IN FACT change the taper amount!!!
    Remember, the taper amount is the actual radial distance from the end X dimension. If you start .2 away from the part while keeping the same taper ( I ) amount, you will have a shallower ( less than 3/4/foot) taper.

    Laminar

    It really depends on your control. Looks like you're using a single line G76, which may mean a Haas machine. In my early days not knowing any better, I did start at Z0 and have never actually blown a thread.
    On the Mori with a '08 vintage Oi-Tc control however, the manual explicitly says to start at a sufficient distance away from the part to allow the spindle speed settling and the feedrate too synchronize with it. It states to start no less than 1 pitch distance away.

Page 1 of 2 12 LastLast

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
  •