Why Can't I find the major diameter of a male NPT Thread?

[Dave K]

I"m looking in my machinists handbook, and looking online, everyone is giving the same chart. And these charts are only showing pitch diameters at certain points of the thread. So how do I know what diameter to turn it to? Trying to make a male 2 inch NPT

 

[Gordon B. Clarke]

I"m looking in my machinists handbook, and looking online, everyone is giving the same chart. And these charts are only showing pitch diameters at certain points of the thread. So how do I know what diameter to turn it to? Trying to make a male 2 inch NPT

Pipe diameter 2.375"

Diameter at thread face: 2.335"

Taper 1:16

I've also sent a PM

 

[sfriedberg]

Gordon has probably straightened you out, so allow me to play Captain Obvious for the day. The T in NPT stands for "tapered". You don't turn or cut threads on a cylinder of constant diameter for tapered threads. That is why all the documentation is giving you diameters at specific points on the thread.

 

[Dave K]

Gordon has probably straightened you out, so allow me to play Captain Obvious for the day. The T in NPT stands for "tapered". You don't turn or cut threads on a cylinder of constant diameter for tapered threads. That is why all the documentation is giving you diameters at specific points on the thread.

I am aware of the the N, the P, and the T stand for. I know it's tapered, but you have to start at the nose of the part, at some diameter. Where is this info given? Every chart is showing what the thread pitch diameter is at certain points, but telling where the major is.

 

[Dave K]

Pipe diameter 2.375"

Diameter at thread face: 2.335"

Taper 1:16

I've also sent a PM

Thanks Gordon, but where did you get the turn diameter at the nose of the part from? I knew the pipe diameter and the taper angle, just couldn't find the diameter at the nose.

 

[SeymourDumore]

Dave

I believe our ancestors couldn't have been more cryptic if they tried when describing certain features of a tapered thread. ( all of it actually )
Basically, they do give major diameter at "Pipe Face" and at "Gage Notch"
Pipe face might be obvious ( yupp, that is the nose of the part ), but the Gage notch ....
Where the heck is that? Well the gage notch is the length of hand engagement ( L1). Got it?

Now try this with an internal NPT shall we?
The minor dia is still called at Pipe face... But which pipe face? Is it the mating Male pipe? Or is it the pipe you're about to thread?
The answer is: It is the pipe you're about to thread.
But then the other minor definition is at Pipe end... But which pipe? The pipe you're about to thread? Or is it the mating Male pipe?
Well, it is the mating male pipe. And where is it in depth? Well, of course it's at L1 ( curiously not called gage notch anymore )

Grrrr.....

And yes, Gordon's numbers are correct.
The major @ the front of your thread is 2.3351, and it is 2.3624 @ Z-.4360 (L1) away from the face.
And while we're at it, might as well give you the Minor @ Pipe Face : 2.2029

 

[Dave K]

Dave

I believe our ancestors couldn't have been more cryptic if they tried when describing certain features of a tapered thread. ( all of it actually )
Basically, they do give major diameter at "Pipe Face" and at "Gage Notch"
Pipe face might be obvious ( yupp, that is the nose of the part ), but the Gage notch ....
Where the heck is that? Well the gage notch is the length of hand engagement ( L1). Got it?

Now try this with an internal NPT shall we?
The minor dia is still called at Pipe face... But which pipe face? Is it the mating Male pipe? Or is it the pipe you're about to thread?
The answer is: It is the pipe you're about to thread.
But then the other minor definition is at Pipe end... But which pipe? The pipe you're about to thread? Or is it the mating Male pipe?
Well, it is the mating male pipe. And where is it in depth? Well, of course it's at L1 ( curiously not called gage notch anymore )

Grrrr.....

And yes, Gordon's numbers are correct.
The major @ the front of your thread is 2.3351, and it is 2.3624 @ Z-.4360 (L1) away from the face.
And while we're at it, might as well give you the Minor @ Pipe Face : 2.2029

Thanks Seymour, I'm looking at the drawing in machinist handbook, and understanding a bunch of it, but still not seeing how that major at the front of the thread got determined. Can you explain that?

 

[bigjon61]

Pitch diameter + thread height will get you within a couple of thousandths. I believe they got the answer by trigonometry using the major diameter at OAL of thread. Too late for me to calculate it myself.

 

[SeymourDumore]

Thanks Seymour, I'm looking at the drawing in machinist handbook, and understanding a bunch of it, but still not seeing how that major at the front of the thread got determined. Can you explain that?

Dave, sorry, but no! Not anymore!

I once spent about 3 hours drawing up a true 3/4NPT thread in CAD.
I've used the Pitch diameters at various lengths ( which are given ), then drew in the 60deg thread angles at the given pitch diameters, then added the basic
flats and the theoretical thread heights to come up with a very exact number.
And that was for a single external thread!
I would have had to go through the very same routine to draw the internal equivalent.

NO FINE WAY!!! Not Again!!!

Literally the day after I've contacted MRainey and purchased ThreadPal.

Frankly, that was one of three best decisions I have ever made when it comes to software! ( NcPlot is the second, I will not dare mention the third )

On a serious note though, damm shame on the publishers of Machinery Handbook ( and any and all other publications ) that makes you go through
a fucking set of calculations ( rivaling that of a moon-launch ) just to come up with a diameter that you need to hold for an NPT thread.

They give a shit ton of calculations to figure out the pitch here, there and everywhere, when at the end of the day there is no fine way to realistically and accurately
measure pitch on an NPT thread without a top-notch CMM ( and perhaps a profilometer added )
How'bout an accurate MAJOR diameter at the beginning of the thread ( perhaps with tolerances ) and the angle of the thread ( and do us all a favor and forget deg/minute angles will'ya )
After that we can now either CAD it or trig-it the rest of the way!

Gordon:

I am not in any way bashing you, but perhaps you can chime in and let us know how one could use the information available from the idiotic Machinery Handbook
and apply a formula to get the exact values for Major and Minor diameters ( since no CNC control that I know of has any setting where a Pitch is to be defined in it's cycle )

Otherwise, I recommend to all to just go out and buy ThreadPal!

 

[litlerob1]

I never got what the big deal is. Not trying to make myself feel better or anything, but it's pretty straight forward. Below is from G-Images, but I believe that is the specification page from M.H.

In M.H. (otherwise known as Decoration or Coffee cup Coaster), it gives you the Largest Turned diameter "D" in this case 2.375, and it tells you what the taper amount is 3/4" per Foot. I Turn it, Indicate it (maybe), then I Thread it.

IMO NPT, API all that is over Engineered, not saying that it doesn't need to meet Print, but...........

Sfriedberg, I think that the "T" actually stands for Thread.

R

 

[Gordon B. Clarke]

Otherwise, I recommend to all to just go out and buy ThreadPal!

I have a pretty impressive "library" of thread standards and information. However to give the numbers I gave to Dave I did in fact use ThreadPal. Have had it for several years, use it frequently and love it.

What I sent to Dave by PM is this and some will now probably accuse me of spamming but it could solve many problems for some of you. One pair of inserts can measure all pitches in the link.

http://f-m-s.dk/3.06.1.pdf

Among the standards I have are ANSI/ASME B1.20.1 and 20.3. However sending and taking copies is
technically illegal. I know though it happens all the time.

I could often help by sending links from my website but to some this is a "No no". I certainly agree it would be spamming if I just did it for no reason other than to sell.

To go from mm to inches just divide by 25.4.

 

[SeymourDumore]

I have a pretty impressive "library" of thread standards and information. However to give the numbers I gave to Dave I did in fact use ThreadPal. Have had it for several years, use it frequently and love it.

Gordon, ( PM sent ), Thank You!!!

 

[RC99]

So how do I know what diameter to turn it to?

Just the nominal pipe OD size. or 2 3/8"

 

[Gordon B. Clarke]

I"m looking in my machinists handbook, and looking online, everyone is giving the same chart. And these charts are only showing pitch diameters at certain points of the thread. So how do I know what diameter to turn it to? Trying to make a male 2 inch NPT

The more I think about it the stranger I find your question/problem.

The thread diameter is the pipe OD. If the pipe OD is larger than it should be the thread will be longer and vice versa with a smaller OD.

Your thread length should give you a good idea as to where you are. Assuming you get the taper right

 

[Dave K]

I never got what the big deal is. Not trying to make myself feel better or anything, but it's pretty straight forward. Below is from G-Images, but I believe that is the specification page from M.H.

In M.H. (otherwise known as Decoration or Coffee cup Coaster), it gives you the Largest Turned diameter "D" in this case 2.375, and it tells you what the taper amount is 3/4" per Foot. I Turn it, Indicate it (maybe), then I Thread it.

IMO NPT, API all that is over Engineered, not saying that it doesn't need to meet Print, but...........

Sfriedberg, I think that the "T" actually stands for Thread.

R

If you are correct, then yes, that's easy. But the 2.375 (D) is showing the diameter of the male pipe, but doesn't really specify if that's right where L4 ends with the top of the thread. That's why I was questioning it.

 

[Dave K]

The more I think about it the stranger I find your question/problem.

The thread diameter is the pipe OD. If the pipe OD is larger than it should be the thread will be longer and vice versa with a smaller OD.

Your thread length should give you a good idea as to where you are. Assuming you get the taper right

There's nothing in the machinists handbook stating that the pipe O.D. is equal to the thread major at L4. I can certainly trig out the tangent of the angle from 2.375 diameter X the length of L4 to get the front nose diameter, but my question is, is that truly the major of the thread.

 

[litlerob1]

There's nothing in the machinists handbook stating that the pipe O.D. is equal to the thread major at L4. I can certainly trig out the tangent of the angle from 2.375 diameter X the length of L4 to get the front nose diameter, but my question is, is that truly the major of the thread.

L4 is where the Minor Diameter of the Thread should end, (or the End Point on the Z axis in the program) on an External NPT or API. So to answer your question; YES! It is the Major Diameter of the Thread (which is irrelevant BTW) Think of it like using a Pipe Tap, the Minor diameter only matters so much.

Part of the reason it isn't specified, is because it doesn't matter. What matters Ultimately is how the Thread Gages.

The key is don't overthink it.

R

 

[SIM]

There's nothing in the machinists handbook stating that the pipe O.D. is equal to the thread major at L4. I can certainly trig out the tangent of the angle from 2.375 diameter X the length of L4 to get the front nose diameter, but my question is, is that truly the major of the thread.

Yup...your right. Kinda sorta.
The Pipe OD is the Major, use L4 for your taper length, trig the starting diameter, verify with thread gauge.


Pipes and lumber have the dumbest specifications ever.


Pipe- a 2" pipe measures 2-3/8" on the OD with 2-1/16"" ID IF its sch40, if it's sch80 the ID becomes 1.9" with 2-3/8 OD Ahhh wah???

Lumber- a 2x4 actually measures 1-1/2" x 3-1/2"...really??? Does that make sense to anyone? Who gives a sh$t what size it started out as...when your done measure the F'n thing and call it that.

 

[litlerob1]

Lumber- a 2x4 actually measures 1-1/2" x 3-1/2"...really??? Does that make sense to anyone? Who gives a sh$t what size it started out as...when your done measure the F'n thing and call it that.

I heard there is a guy Suing Lowes for selling him 2x4s that were NOT 2" X 4". Funny thing is he may win.

R

 

[Dave K]

Just the nominal pipe OD size. or 2 3/8"

You would turn it straight for a tapered thread? Wouldn't you want to turn it at the same angle that the thread is going to be?