Page 1 of 2 12 LastLast
Results 1 to 20 of 21
  1. #1
    deadend is offline Hot Rolled
    Join Date
    Aug 2007
    Location
    Nashport. Oh
    Posts
    653

    Default Acme thread tap drill formula

    Does anybody have a formula for Acme tap drills. Making a nut for a cross slide lead screw off a monarch lathe. The thread is 1.25"-4, which a 5 is standard.Nut is trashes so can't get the I.D. measurement. I figured around .970. Just would like some 2nd opinions. Thanks

  2. #2
    Clive603 is offline Titanium
    Join Date
    Aug 2008
    Location
    Sussex, England
    Posts
    2,292

    Default

    Basic minor diameter for Acme is OD - pitch. In the real world there needs to be an allowance under the basic diameter for clearance. According to Machinery's Handbook 20 thou per inch of diameter is right for general purpose threads of 10 TPI and coarser which comes out at 0.975 so you are close enuf for government work.

    However if you plan to tap the thread there should be info with, or on, the tap set as to what starter size drilled hole should be used. There are small variations, especially when you start taking into account the class of thread required. ACME taps are ill behaved beasts at the best of times. Takes a far braver man than I to start from a drilled hole, especially in phosphor bronze. Given the choice I'd screw-cut the whole thing to the best possible fit on the feed-screw, or at least get the basic shape in and use the tap to finish off.

    Clive

  3. #3
    Forrest Addy is offline Diamond
    Join Date
    Dec 2000
    Location
    Bremerton WA USA
    Posts
    9,340

    Default

    Clive is right. Acme taps start crooked every time in the scale of accuracy needed from machine tool lead screws. Bore the minor diameter, then rough the thread with a tool.

    The secret is to use a boring bar about 1/2 addendum smaller than the minor diameter. Bump the tool out every few cuts and pick up the thread again. I bored the thread and dial back enough to clear the tool just enough so it wouldn't rub the thread flank a you revers back with te extended tool in the clearance. If you want to open the half nut and crank back the carriage you wind up using such a skinny boring bar it flexes too much. Reversing back is intimidating, yes but necessary.

    A lot of people have been bit with the idea that all you need is an Acme tap and you can make a new lead screw nut for a worn lead screw. Maybe so if he lead crew is in good shape and you have a series of three graduated Acme taps with minor dia pilots on them. A GP tap intended for general manufacturing won't do the job required for making lead screw nuts for machine tools where PD accuracy and axis alignment are primary concerns.

    Bore the thread of your Acme nut with a narrow tool then widen when you get to depth. This way you can fit the new nut to a re-cut lead screw having a contant pitch diameter. If you're kick and there's very little wear on the lead screw AND the tap cut threads very close the what the lead screw requires, you're lucky. Tap away once you get the thread roughed out.

    RE-CUT A LEAD SCREW? What's this? If you're gonna replace a worn out nut you will find the lead screw will be worn in the center and still new at the ends where it seldom runs. Make a new nut to snugly fit the end and it will rattle in the middle like a BB in a boxcar. Set the lead screw up with a follow rest and re-cut the flanks to barely clean up the center of the wear. The thread will be narrow and the space wide but it's necessary if you want to restore the machine's B/L to 0.003" from 0.060" or more. A standard Acme tap will do you no good here. It's all custom machine work and non-standard fitting but you avoid making a whole new lead screw.

    The result is a thread with a cylindrical pitch dia, no bell mouth, and a constant backlash that properly fits the nut. Some lead screws are 4 x as long as the nut's minor diameter. Heroic methods are therefore indicated.

    If it was easy anyone could be a machinist.
    Last edited by Forrest Addy; 07-20-2010 at 12:18 AM.

  4. #4
    DWolfhope is offline Plastic
    Join Date
    May 2010
    Location
    usa
    Posts
    38

    Default

    (1) 1 divided by TPI
    (2) Subtract this amount from the OD. for pitches 10 and greater always add .005 for drill size. For pitches less than 10 TPI take the amount from
    step 1 and multiply x.05 (5%) and add this to the drill size. This is for 95% to 100% of threads

    example

    1.25 x 4 acme
    1/4 = .25
    1.25 - .25 = 1
    .25 x.05 = .0125
    1. plus .0125 = 1.0125 drill sze

  5. #5
    Join Date
    May 2010
    Location
    Kolding Denmark
    Posts
    10,983

    Default

    Quote Originally Posted by deadend View Post
    Does anybody have a formula for Acme tap drills. Making a nut for a cross slide lead screw off a monarch lathe. The thread is 1.25"-4, which a 5 is standard.Nut is trashes so can't get the I.D. measurement. I figured around .970. Just would like some 2nd opinions. Thanks
    You're right, 5 TPI is standard for ACME 1.25.

    I'm sitting here with ASME/ANSI B1.5 ACME SCREW THREADS.

    For ACME 1.25 - 5 TPI the minor (bore) diameter is 1.05 to 1.06"

    For ACME 1.375 - 4 TPI the minor (bore) diameter is 1.125 to 1.1375"

    N.B. This is for tolerance classes 2, 3 and 4G.

    So, if you subtract 1.125 and 1.1375 from 1.375 you get 0.25 and 0.2375.
    1.25 - 0.25 is 1.00 and 1.375 - 0.2375 is 1.1375.
    Subtract 0.25 and 0.2375 from 1.25 and you have your min. and max. bore diameter.
    i.e. 1.25 - 0.25 = 1.00 and 1.25 - 0.2375 = 1.0125

    I could add more detailed info on to what I have for ACME threads in another thread. Screw threads - uses, tolerances and general info.

    For what I have on ACME (and it doesn't really answer your question) then see http://www.f-m-s.dk/ACME%20threads.pdf

    Anyone want me to add on more about ACME or any other screw thread? If so - what?
    Last edited by Gordon B. Clarke; 07-20-2010 at 06:55 AM. Reason: mistake

  6. #6
    mrainey's Avatar
    mrainey is offline Stainless
    Join Date
    Jul 2004
    Location
    Spartanburg, South Carolina
    Posts
    1,503

    Default

    For ACME 1.25 - 4 TPI the minor (bore) diameter is 1.125 to 1.1375"

    Are you sure?

  7. #7
    Join Date
    May 2010
    Location
    Kolding Denmark
    Posts
    10,983

    Default

    I agree with mrainey

    Those are the sizes for ACME 1.375 - 4 TPI - NOT 1.25

  8. #8
    Join Date
    May 2010
    Location
    Kolding Denmark
    Posts
    10,983

    Default

    Just to go on record. Any tolerances mrainey gives I'd be inclined to go along with

    Even if they weren't the same as mine LOL

    Hows that for a compliment?

  9. #9
    DWolfhope is offline Plastic
    Join Date
    May 2010
    Location
    usa
    Posts
    38

    Default

    Here is a thread report for the 1.25 - 4 Acme
    Attached Files Attached Files

  10. #10
    Join Date
    May 2010
    Location
    Kolding Denmark
    Posts
    10,983

    Default

    Fantastic - I got it right

  11. #11
    Join Date
    May 2010
    Location
    Kolding Denmark
    Posts
    10,983

    Default

    Quote Originally Posted by DWolfhope View Post
    Here is a thread report for the 1.25 - 4 Acme
    Nice printout by the way

  12. #12
    deadend is offline Hot Rolled
    Join Date
    Aug 2007
    Location
    Nashport. Oh
    Posts
    653

    Default Job done!

    Bored it 1.00" no tap unless the boss wanted to pay $700.00 the new nut from Monarch was $1040.00 So we single pointed it, had to float the tool a little bit .005" on a side . Good fit, Thanks guys
    I guess the 4 TPI was for the .500" revolution of the cross slide movement

  13. #13
    Join Date
    May 2010
    Location
    Kolding Denmark
    Posts
    10,983

    Default

    Quote Originally Posted by deadend View Post
    Bored it 1.00" no tap unless the boss wanted to pay $700.00 the new nut from Monarch was $1040.00 So we single pointed it, had to float the tool a little bit .005" on a side . Good fit, Thanks guys
    I guess the 4 TPI was for the .500" revolution of the cross slide movement
    Thanks for keeping us up to date and knowing there's now one less problem in the world

  14. #14
    Join Date
    May 2010
    Location
    Kolding Denmark
    Posts
    10,983

    Default

    Quote Originally Posted by mrainey View Post
    Are you sure?
    This is one for you or anyone else that can answer.

    At what depth should pitch diameter be measured for API NC50 4-" IF external and internal thread? What then are the pitch diameter tolerances?

    Thanks in advance - he wrote optimistically

  15. #15
    4GSR's Avatar
    4GSR is offline Titanium
    Join Date
    Jan 2005
    Location
    Victoria, Texas, USA
    Posts
    3,067

    Default

    Quote Originally Posted by Gordon B. Clarke View Post
    This is one for you or anyone else that can answer.

    At what depth should pitch diameter be measured for API NC50 4-" IF external and internal thread? What then are the pitch diameter tolerances?

    Thanks in advance - he wrote optimistically
    According to the Drilco RHC Handbook, "The Bible of the oil tool industry",
    picth diameter is 5.042" at .625" from face of pin. The depth at pitch line is .0518". Without going into fine details, the pin thread controls the pitch diameter of the box thread, which in "tenths" is about the same as the pin thread. API Spec 7 details this in "gaging practice."

    Ken Stokley

  16. #16
    4GSR's Avatar
    4GSR is offline Titanium
    Join Date
    Jan 2005
    Location
    Victoria, Texas, USA
    Posts
    3,067

    Default

    Quote Originally Posted by DWolfhope View Post
    Here is a thread report for the 1.25 - 4 Acme

    BTW- "Gagemaker" rules!!!!

    Of course, their information for the thread itself comes from ANSI Standards. I've used it for over twenty years now.

    Ken

  17. #17
    Join Date
    May 2010
    Location
    Kolding Denmark
    Posts
    10,983

    Default

    Quote Originally Posted by 4GSR View Post
    According to the Drilco RHC Handbook, "The Bible of the oil tool industry",
    picth diameter is 5.042" at .625" from face of pin. The depth at pitch line is .0518". Without going into fine details, the pin thread controls the pitch diameter of the box thread, which in "tenths" is about the same as the pin thread. API Spec 7 details this in "gaging practice."

    Ken Stokley
    Ken, thanks. Two more pieces of info and I'll bow each time you pass

    What is the tolerance of 5.042" and the total angle of the thread?

    As I only intend making something to measure one specific API thread then buying a book and/or a standard seems a bit much and I doubt if the customer would pay. I already have most of the necessary standards for the more common threads.

    If you're interested then this is how I intend doing it:

    http://www.f-m-s.dk/Tapered%20pipe%20threads.pdf

    At least in principle, as the thread inserts will be made for the thread in question.

    I've got several ANSI standards if anyone needs information from me. Living in Europe means that getting the necessary American standards isn't always as easy as it might seem plus a great deal more expensive

    Gordon

  18. #18
    Masheen4140 is offline Plastic
    Join Date
    Aug 2010
    Location
    Saskatoon, Canada
    Posts
    32

    Default

    I use this site for all my acme and stub acme needs


    iCrank ACME Thread Designer

  19. #19
    jdj
    jdj is offline Diamond
    Join Date
    Oct 2007
    Location
    detroit,mich.
    Posts
    4,670

    Smile

    Quote Originally Posted by deadend View Post
    .Nut is trashes so can't get the I.D. measurement.


    I had to look up at your location. This sounds like a european way of saying THE NUT IS TRASHED.

  20. #20
    4GSR's Avatar
    4GSR is offline Titanium
    Join Date
    Jan 2005
    Location
    Victoria, Texas, USA
    Posts
    3,067

    Default

    Quote Originally Posted by Gordon B. Clarke View Post

    What is the tolerance of 5.042" and the total angle of the thread?

    Gordon

    Gorton,

    Send me your email address by PM and I'll get you a more detailed information on the 4-1/2 IF connection.

    The tolerance on the PD is "Hold it as close as you can", the angle is very loose, I don't have that information handy, it's like a +/-1/2 degree.

    Some of us take the mating connection and use it for a gage. A person has to be very good at what he does when doing this. Of course, the mating part has to be to "Gage" too! Mating part can get you trouble if your'e not carful, too. I know over here, there are shops that will rent out their gage for a minimum fee, or free of charge, or for a favor. Might find some one over there do the same, and let you borrow their gage. Just a thought.

    Ken

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
  •