Results 1 to 20 of 21
Thread: Acme thread tap drill formula
07-19-2010, 01:08 PM #1
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
07-19-2010, 02:00 PM #2
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.
07-19-2010, 06:06 PM #3
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.
07-20-2010, 05:58 AM #4
(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
1.25 x 4 acme
1/4 = .25
1.25 - .25 = 1
.25 x.05 = .0125
1. plus .0125 = 1.0125 drill sze
07-20-2010, 06:31 AM #5
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
07-20-2010, 06:52 AM #6For ACME 1.25 - 4 TPI the minor (bore) diameter is 1.125 to 1.1375"
Are you sure?
07-20-2010, 07:00 AM #7
I agree with mrainey
Those are the sizes for ACME 1.375 - 4 TPI - NOT 1.25
07-20-2010, 07:03 AM #8
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?
07-20-2010, 01:12 PM #9
Here is a thread report for the 1.25 - 4 Acme
07-20-2010, 02:19 PM #10
Fantastic - I got it right
07-20-2010, 02:20 PM #11
07-20-2010, 02:59 PM #12
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
07-21-2010, 02:10 AM #13
10-23-2010, 03:39 AM #14
10-23-2010, 08:06 AM #15
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."
10-23-2010, 08:09 AM #16
10-23-2010, 08:47 AM #17
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:
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
10-23-2010, 09:18 AM #18
10-23-2010, 09:40 PM #19
10-24-2010, 09:52 AM #20
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.