What's new
What's new

Acme thread tap drill formula

deadend

Hot Rolled
Joined
Aug 18, 2007
Location
Nashport. Oh
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
 
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
 
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:
(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
 
Here is a thread report for the 1.25 - 4 Acme
 

Attachments

  • Thread Disk Report.pdf
    7.4 KB · Views: 1,208
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
 
This is one for you or anyone else that can answer.

At what depth should pitch diameter be measured for API NC50 4-½" 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
 
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
 








 
Back
Top