Results 1 to 20 of 23
Thread: NPT thread bore dimensions
10-28-2009, 02:03 PM #1
NPT thread bore dimensions
Guys, kinda stupid question here, but do need some help.
I'm getting ready to make some NPT threads in Inco 625 on a lathe, and I need to get them to specification not only in pitch dia and depth, but the min diameter bore dims as well.
Spent the last hour looking through the Machinist handbook and trying to decipher even the fine print stuff, but am yet to figure out how to calculate the bore diameter for a 3/4-14 Internal NPT thread.
I have the pitch diameters at the beginning of the thread, the pitch dia at the nominal length of the part, the taper angle ( 1 over 16 ), the nominal length, minimum OAL length ( wrench makeup ) and even the truncation allowances.
What I can't friggin' find is the minor diameter at any point of the thread!!!
I do have one number, which is .9105 dia, and is defined as: Basic Minor Diameter at small end of pipe.
Now, just what the hell does that mean? Is it the minor dia on the pipe's external thread, or the minor diameter on the internal thread?
A 3/4" pipe's nominal OD is 1.05", but without knowing the OAL length of the thread I can't figure out what this number mean.
Can someone kick me in the ass and point in the right direction please!
10-28-2009, 02:07 PM #2
Sorry but I'm
On this one.
I always find this to be a major pain.
Why does it have to be so criptic?
10-28-2009, 02:52 PM #3
1* 47' just so the 6 step guage fits. (Internal or external)
THAT'S what I know...
I just went'n looked, but I don't have an internal 3/4 pipe 6 step. (3 step?) Otherwise I could measure one for you.
Think Snow Eh!
10-28-2009, 03:14 PM #4
Can you work from the pitch diameter? For 14 tpi the thread height is .061" so for the various PD measurements given in the handbook, just add .061 to the PD for the external thread at that location, and subtract it from the PD for the internal thread. Will that work?
Note: the PD is measured at half the height of the thread, but working across a diameter means that you double the 'half height' value. That ignores the 'flat' on the thread or the necessary minimum clearance, so you might also allow for the amounts shown in the truncation table.
10-28-2009, 03:46 PM #5
I always have problems with this too. It would be nice to have a sketch of the profile or bore for ID NPT threads.
10-28-2009, 04:08 PM #6
Ox, I'd like the tapered bore dimensions. Got the gage with the "hand-tight" flat on it, but really want to have the bore dim.
Is the pitch at 1/2 distance?
Using your idea, I was trying to calculate them out on standard threads by using ( Major bas - Minor bas ) / 2 + Minor bas . the result is always larger than the Pitch high limit.
I'd guess it's close, but there outta be a formula somewhere for the NPT-s!
I guess I'll draw up something based on the known values and see what the actual drawing shows.
Looks like that .9105 from the book isn't the minor on the pipe, as it would be way out long.
Curious about why pipe threads so secretive???
I know there are a whole bunch of different pipe thread standards, but that's even more reason to have a nominal spec or formula for each of them.
Unless It's one of those Freemason or Iluminati things.
10-28-2009, 04:41 PM #7
I have a chart for "RC" or "PT" pipe threads, it uses what it calls a "gage line" to dimension a diameter at a certain depth in the bore. Some simple math and you got what you need for the bore size. I am pretty sure I dont have one for NPT threads, but I will check tomorrow.
10-28-2009, 04:49 PM #8
Ok so maybe I'm just not following at all here and if so I'll just claim to be drunk...
I kinda thought that was just your TDS? say from a TDS chart? so I had to look too...
Page 1848 of the 26th Edition of the MH. Table 3, Internal Threads in Pipe couplings, NPSC for pressure tight joints with lubricant or sealer. ANSI/ASME B1.20.1-1983(R1992)
3/4" says Minor dia Minimum .925". Oddly enough the TDS is 59/64th or .9219" (close enough?)
I smell burnt toast
10-28-2009, 06:47 PM #9
Say there, while your drinking - I am gunna go ahead and look green and ask what TDS is.
If you hurry and answer - I can delete this post before it times out and not look so dorky. You having a conversation with yourself tho - well ....
Well - outta curiosity I dug out Edition 23 and found your chart on page 1615 and finally got enough info to figger out what you are talking about.
Tap Drill Size.
I think Mr. Dumore is lookin' to bore the taper...
Dumore, Here's what I'd doo if I was so wrapped up in this. (I take it you have some brown bottles of some import that I never heard if going as well?
Just bore the taper out to a bit larger than you think it should be and then run your threading cycle. Adjust to where your thread guage fits and cut off. Eyeball how big the flats are on your crests and tweek.
(Just guessing that your gunna runa test sample first enyhow eh?)
Think Snow Eh!
10-28-2009, 06:58 PM #10
Its been a few years since I got to single point internal pipe threads that had to be all pretty and such, funny enough most of them were 3/4" too.
I do remember just using regular TDS and then boring the taper before threading. I think I only bored/tapered to the length of engagement. You can also buy tapered reamers made for sizing the holes before tapping/threading. Then again I think a shaped insert made for that size pipe thread should pretty well take care of it?
10-28-2009, 07:34 PM #11
10-28-2009, 08:52 PM #12
Here is what flowed out of the green bottle and ACAD.
Applies to the internal thread tapered BORE only!!!
Start diameter: .9397
End diameter @ min depth: .9051 @ .5533
For the THREAD:
Starting Major diameter: 1.0475
End major @ min thd depth: 1.0129 @ .5533
Taper amt @ min depth: .0173 @ .5533
Thread height ( between truncated crests) : .0539
I mean COME ON!!! This is so freakin' retarded!!!
Why the hell does NPT have to be calculated when it's all so goddam common!!!
10-29-2009, 03:16 AM #13
Here's a screenshot from ME ThreadPal - took a couple of mouse clicks to get there. Extensive data for forty types of threads.
I got tired of banging my head against the wall too.
10-29-2009, 07:40 AM #14
Ok, now I feel like a bafoon.
Mike, thanks for the link and look forward to a quick purchase.
Looks like the only difference there is between your sw. and my calculation is the minor at the start. Seems to be the deviation is exactly the basic crest truncation.
Crest: .0024-.0056 [.004]/side, .008 diameter
ThreadPal start dia: .9317
My Calculated start dia: .9397
10-30-2009, 04:54 PM #15
Have any luck yet?
Try this with a 1/64 tnr bore.
I.D. THREAD FANUC 2LINE METHOD
G76 P010060 Q20 R10
G76 U.09 Z-.76 R-314 P571 Q40 F.0714
SINGLE LINE YASNAC
G76 U.09 Z-.76 I-314 K571 D60 A60 F.0714 P1
If you need to make thread larger or smaller change the u.09 to size the gage
10-31-2009, 05:26 AM #16
I do tons of internal pipe threads and the easiest cure for the problem is to buy NPT thread forming inserts in the TPI size you need and when the thread gage fits then the minor bore size is also correct providing you didn't bore it to big to start with, it takes a little trial and error, you can also buy the check gages for the minor bore and L1 and L2 depths to check for proper taper. Before we got the forming inserts I would have to start small and adjust the boring tool and threading tool until I achieved the proper truncation on the minor dia. of about .003 flat and then raise both tools equally until the gage fit, then go make the program correct so no major offset was required the next time.
10-31-2009, 08:07 AM #17
10-31-2009, 08:33 AM #18
Guys, thanks for the replies, job came out tits.
I used my numbers for the bore and left it as it was.
The only thing I had to play with was the threading tool, and adjusted it by +.009, and I'm just guessing that was because of the sharp tip on the AG60 insert.
04-22-2014, 08:24 AM #19
Can someone run the numbers in that software for 1/2-14 npt internal thread
04-22-2014, 09:24 AM #20
I've run a lot of 3/4x14 NPT. We drill it .875", which of course is going to come out a bit bigger. Start point is X.9,Z.1, and final X is .995, with a Z-.800. R line in the Fanuc 21iT is the taper, and its at .0887. Feed is .07143. This is in the Fanuc two line G76 coding. Hope this helps. Let me know if the program would help, I'll post it if I need to.