NPT internal thread crest truncation limits?

[Finegrain]

Hi guys,

I'm doing some 1/8" and 3/4" internal NPT threads. Single-form threadmill. I got to thinking that, unless you make a perfectly tapered bore, the upper threads are going to have sharp crests.

I checked MHB and it has a table of allowed thread truncation. The range for 27 TPI is .0012" - .0036", while the range for 14 TPI is .0024" - .0056" (page 18643 in my 28th edition).

There is also some verbiage about these tolerances only applying to high-pressure applications.

So, am I supposed to use a multi-form threadmill in lieu of making a very precise tapered bore?

Thanks, and regards.

Mike

 

[Finegrain]

I may have found the answer ... correct me if I'm wrong.

According to Threadcheck.com:

NPTF ("dryseal") requires crest truncation measurement.

NPT does not require crest truncation.

NPT PIPE THREADS

• NPT Threads- Are considered "General Purpose" Pipe Threads.
• NPT Threads- Are intend to be sealed at the Crest & Root with Teflon Tape, Pipe Dope, or Other Types of Sealant.
• NPT Threads- Do not require "Crest Check," L-3, or L -2 gages.
• NPT Gages- Made to ANSI/ASME B1.20.1.

 

[HuFlungDung]

I'd bore the taper, then thread mill it. You can interpolate the taper with a taper end mill, or a bull nose endmill, or ream it with a taper pipe reamer.

A multi-tooth NPTthread mill would probably be a better choice as it can 'top' the threads for you.

 

[Bobw]

Taper reamers are fairly cheap...

If the customer doesn't care, I generally don't care..

Dry seal... NPTF??? been a while.. Its got to be right if the customer actually cares

Sometimes in nasty material.. A taper reamer makes your life easier weather you need it to meet the
spec or not.

 

[Finegrain]

OK, how then do you know the tapered bore is the right size within a thousandth or two, in-process, so you can match the bore to the threadmill? IME threadmills have to be offset-adjusted during runtime.

I do already taper the bore to ease the load on the threadmill but leave it undersize so as to not have over-truncated threads.

Regards.

Mike

 

[HuFlungDung]

Well, you could just measure the mouth of the hole in a sample thread with a caliper. That will get you close.

The taper dimensions can be ascertained from the tables in Machinery's handbook. I believe the pitch diameter at the start of the thread is a table value that I work from. Add or subtract the single full thread height from the PD to get the OD or ID of the taper (depending on if you are working ID or OD threads).

But typically, I'd just take a trial cut or two, gage it with a plug, modify the interpolation diameter according to the rise/run of taper threads (1:16), This is all done quickly with my cadcam software.

 

[Booze Daily]

OK, how then do you know the tapered bore is the right size within a thousandth or two, in-process, so you can match the bore to the threadmill? IME threadmills have to be offset-adjusted during runtime.

I do already taper the bore to ease the load on the threadmill but leave it undersize so as to not have over-truncated threads.

Regards.

Mike

There is a 6 step plain taper gage for gaging truncation.

 

[cosmos_275]

you can also pick up the big ID and the angle from these reamers: mcm pipe reamers. I've done that before before running a pipe tap through: bore the cone with a ball end mill.