thread depth

[freddycougar]

hi all is there a formula for determining the depth of the thread baised on the pitch..

i want to thread internal and external 3 inch.. 40 tpi
thanks
freddy

 

[randyc]

Freddy, there are approximations that work well for coarse threads.

For the situation that you describe (40 tpi) you should consult "Machinery's Handbook" and obtain the dimensions from tables based on the class of thread that you require.

If you don't happen to have access to the reference, say so and someone will give you the dimensions.

 

[toolmakerjim]

40 TPI on a 3" dia.? heres what i would do.
make a master gage using thread wires or thread triangles for the class of fit you want. save this plug gage and make a ring gage to fit the plug then make your parts using the approiate gage to fit you threads...jim

 

[freddycougar]

thanks for the reply.. i do not have the book yet

 

[toolmakerjim]

how many are you doing and whats the application?...jim

 

[freddycougar]

i am making two of each .. bearing holder and retaining nut? IM NOT SURE TO CALL THIS A NUT AS IT HAS EXTERNAL THREADs

 

[randyc]

Andrew, I'm going to make a couple of copies from "Machinery's Handbook" and send them to your e-mail address.

Follow Toolmakerjim's advice about making and measuring the master plug gage and the mating ring gage.

If you don't know how to make the three wire measurement, post and someone will help you.

Tables will be on the way shortly ...

 

[freddycougar]

THANK YOU randyc abd thak you tmJim

 

[John Garner]

freddycougar --

Is it reasonable to presume that you want to cut a Unified threadform? (The Unified threadform had been in widespread use in the US since 1949, when it replaced the previous-generation threadform that was commonly referred to as the National Standard.)

The most basic profile of Unified threadform has 60 degree flank-to-flank angles with a 1/8-Pitch flat at the Major Diameter and a 1/4-Pitch flat at the Minor Diameter. The general Unified standard allows -- but does not require -- a radius instead of the flat at the Minor Diameter of a male thread. There are also variants of the Unified standard that require a radius instead of a flat, but they are not particularly common.

If you want to cut the basic Unified threadform, the formula for the theoretical Single Depth of Thread is 5/8 x Pitch x Cosine 30 degree. As a step-by-step numerical example, for a 40 Thread Per Inch Unified screwthread the Single Depth would be 5/8 x (1/40 inch) x Cosine 30 degree = 0.625 x 0.025 inch x Cosine 30 degree, which to 4 decimal places is 0.625 x 0.025 inch x 0.8660 = 0.0135 inch.

Theoretically, the "tap drill size" would be the Major Diameter reduced by twice the Single Depth of Thread, but this would provide for a full thread, which is only trivially stronger than a 75% thread but is much more difficult to tap. An effective Rule of Thumb to calculate the tap drill size for a Unified thread is Major Diameter - Pitch.

I'll add a word of warning: If someone is paying you to make these threads, you are morally and legally obligated to work to the standards defined by your customer . . . and that means the published standards, not to something you found on an Internet Bulletin Board.

John

 

[randyc]

OK Freddy, the excerpts from "Machinery's Handbook" are on the way. I've included the forulae, pictorial and the dimensions for some common pitches (e.g. 40 tpi).

edited:

"formulae" not "forulae", fingers are getting stiff

 

[toolmakerjim]

if your just making two of these heres the quick and dirty way of doing it.
turn your part to 3" setup your threading tool and with the cross slide set to "0" at touch off and the compound set the same advance the compound .018" to .019" if you have the proper flat on your tool point (1/8 X pitch)fot this case this factor is insignificant.
after cutting both pieces to the same numbers set up for the ID threads bore to 2.975" then thread to fit the other OD pieces...jim

 

[freddycougar]

again thanks lots.. i have all the info i need..

 

[tattoomike68]

3" 40 TPI will be a nightmare if it gets a spec of dirt or gets cross threaded then you have junk.

I used to make hydraulic cylender heads that were 6-3/16" 16 tpi and it was too fine, they would gaul from a tiny ding and ruin a $5,000 cylender, we went to 12 and had no more problems.

good luck, but 40 tpi is asking for trouble.

 

[spope14]

here are some formulas I use, they are referenced by machinery's handbook, and a great textbook for machining called "machine Tool Practices" by Kibble, Neeley, and White.

Based on Unified national form class 2 common: External first

Pitch of thread - distance between two equal points on a thread = 1/n of 1 divided by the number of threads per inch. A 40 thread will give .025 as the answer.

Thread depth = .613/n or .613 divided by the number of threads per inch. Also .613 x pitch of thread. Your answer will be 0.0153 both ways.

If you are using a compound rest at 60 and 1/2 degrees off centerline (or 29 1/2 degrees off perpendicular of centerline), a way to cut threads to depth is to use the compound rest handwheel for your depth. There is a formula for the depth using the compound rest, and it is:
.708/n or .708 divided by the number of threads per inch. Your answer will be .0177 for the compound rest dial to be noved in, a few thou at a time. use .018. There is a inal "finish pass" required, move the crossfeed in .001 (.0005 for a 2:1 dial) after the compound rest infeed is completed and you will have a cleaned up cut that hits both sides of the tool, and leaves a real smooth fit.

Internal threading:

Bore size determination - based on the 75% to 80% model of tap drilling
Single depth of thread = P x .541 P= Pitch, .541 is a "constant".

Bore diameter for the thread: d = D - (p x .541 x 2) or bore diameter = Major diameter - (pitch x .541 x 2) Do the parentheses part first. Your answer works up as follows: (.025 x .541 x 2) = .0270 Major diameter is 3.000 so 3.000 - .0270 = 2.973 for your bore.

Using the compound rest set at 60 and 1/2 degrees parallel to the centerline handle facing TO the chuck (29 1/2 degrees perpendicular), and a threading boring bar, the formula for outfeed of the compound rest dial is:
P x .625 or pitch of thread x .625. For your thread, this is .025 x .625 or .0156.

I am sure this was all mentioned above in some form, I just was in a groove. I do love threading unified national threads, and these formulas have been beat into me since I was a wee apprentice, an onfirmed through the textbooks I mentioned. Hope this helps, if not, I can send something called the "math reference sheet" I have worked up over the years.

 

[freddycougar]

i got it done.. 40 is way to fine, i switched to 20 tpi and it looks way better..
Thanks GENTS..
freddy
btw spope i will try using the compound on the next one...

 

[atomicbear]

More accuracy for depth of thread formula

spope14 said:

"here are some formulas I use, they are referenced by machinery's handbook, and a great textbook for machining called "machine Tool Practices" by Kibble, Neeley, and White.
Thread depth = .613/n or .613 divided by the number of threads per inch. Also .613 x pitch of thread. Your answer will be 0.0153 both ways."

You are correct. However...
For a bit more accuracy - the number to use for single thread depth is .61343 divided by TPI. .613 will work in a pinch, but you should use the full 5 places for accuracy.

--atomicbear

 

[billmac]

10 years later?

 

[TheCook]

10 years later?

Maybe atomicbear thought that it wasn't urgent