Results 1 to 20 of 22
Thread: NPT tapping
02-21-2012, 08:04 AM #1
I'm going to use a couple of npt taps the first time (1/4,3/8,1/2).
How deep do you need to tap to get the correct length ?
02-21-2012, 08:16 AM #2
To do it right, you need to use a tapered reamer on the holes before you tap them to get a full thread.
John Welden liked this post
02-21-2012, 08:25 AM #3
That's a tough one. You really need a plug gauge to be accurate. You can get fairly close by going to a depth of about 2/3rd's of the thread length of the tap. If you can find a true gauge, use that, but if not you should at least get a mating thread from a known quality source. With something such as a hex socket pipe plug, try to get between 3 and 3-1/2 turns of engagement.
I've made a lot of pipe threads in those sizes over the years and never used a reamer before the tap. Since none were ever rejected by customers (some of them ISO-certified), I assume they were standards-compliant threads.
02-21-2012, 08:49 AM #4
Stingray, I've done this several times. This type of tapping requires more focus. I'd go with Pixman's advice: "you should at least get a mating thread from a known quality source". Good luck.
02-21-2012, 09:13 AM #5
Generally its right around 6 threads from the top of the tap, 6 threads left sticking out of the hole that is.
02-21-2012, 09:52 AM #6
It seems most if not all are from China these days. Even a professorial plumbing supply had Chinese fittings.
I learned about Chinese pipe fittings a couple years ago working on the rentals, it's near impossible to make a water tight connection with them. Unable to seal the joint with teflon tape and pipe sealant I gave up and ran a die over the male fittings and a tap into the female threads, problem solved.
I did notice the threads on China-sourced brass fittings do seal as they should.
02-21-2012, 09:57 AM #7
I usually use a quality fitting to check depth , 3-4 turns before it gets finger tight . I have also had better luck getting nice threads using a tapered reamer .
02-21-2012, 10:06 AM #8
02-21-2012, 10:58 AM #9
The way I gauge the threads when I don't have a proper traceable calibrated gauge is to screw in the male-threaded part by hand until it stops, then count how many full turns I get before the parts separate.
I believe that is more accurate than counting the turns in because it can be rather ambiguous as to when the engagement truly starts when screwing it in.
jdj liked this post
02-21-2012, 11:29 AM #10
As others have stated, you can tap without taper reaming. Morse Cutting Tools recommends:
1/4 NPT - drill with a 7/16 bit to a minimum depth of 0.78125 & tap to a depth of 0.72525
3/8 NPT - drill with a 37/64 bit to a minimum depth of 0.8125 & tap to a depth of 0.7565
1/2 NPT - drill with a 45/64 bit to a minimum depth of 1.03125 & tap to a depth of 0.96025
Following these recommendations will only give you a full thread for the first 2 to 3 threads.
02-21-2012, 09:46 PM #11
I always use a taper reamer for the pipe size being tapped and then leave 7 threads showing at the top of the tap when I back it out and call it good. Has always worked for me.
oldbrock liked this post
02-21-2012, 10:11 PM #12
Stingray, If the pipe threads you are tapping require any precision at all then you really need to use a NPT Plug gage to be sure of proper length of engagement. Otherwise, most of the methods already listed should suffice. Also, if you are going to use a pipe reamer, then you should also check the reamed depth with an NPT Crest gage, as reaming too deep may create a thread that will not seal.
02-22-2012, 01:24 AM #13
Ok, I will try the above methods on a couple of scrap pieces and see what works.
Thanks for all the input.
As for the Chinese stuff mentioned : I've noticed the same thing with the BSPT threads usually employed here for pipe sealing. I could get them to seal with strings and grease though. However I've noticed that some sections of the pipes were virtually impossible to get a thread started. Seems like the metal is a lot harder in that section.
Well, Chinese quality.
I think we in the west still have a future if we keep producing quality.
02-22-2012, 03:49 AM #14
Not sure of the manufacturer but my 1/8 - 27 NPT tap has a notch about 2/3 of way up leaving 6-7 threads above it. I like it cause it is easy to see where to stop. I also have never used tapered ream before tapping but it sounds like a good idea, sure would make getting the tap started easier I think. I'll try it next time.
02-22-2012, 01:57 PM #15
Ok, i'm a hobbiest and got an 18 mm drill they suggested to do the 1/2 npt.
First both with my boring stand and hand drill it went difficult to get a smooth hole. I could only smoothen it out using a 13 mm to predrill it.
I did this in alu so as not to go into to hard material.
When I went to 6 threads from the end, one of my AN fittings with an 1/2 npt on the other side would only go in a couple of threads by hand. It was better when i drove the tap in to about 2 threads from the end. This was a alu plate of ca 15 mm thick.
Also in one of the holes some of the threads were broken.
I went looking for one of those reamers but boy are those expensive.
Hm, harder than I thought.
02-22-2012, 11:09 PM #16
I was always taught to gage NPTs not by the engagement, but by the standoff (# of threads projecting above the hole) if no proper gage was available. Start at the "pullout" or vanishing point of the thread on the fitting or whatever you're using, and count roots (not crests) down to the face of the part. There should be between 2 and three showing when hand tight.
02-22-2012, 11:29 PM #17
Stingray, if you give me your email I'll send a copy of the 2 relevant pages in ANSI/ASME B1.20.1 (Pipe Threads, General Purpose) so you can see the exact sizes you are looking for as well as just about everything else.
Before anyone asks then I can't post them in PM as that would be violating copyright.
02-22-2012, 11:43 PM #18
I usually shoot for 5 threads sticking out if the material thickness allows. This always seems to give me a good 4 turns with a gage. For something 3/8 thick I would probably leave 6-7 threads out.
01-19-2017, 08:39 AM #19
A Delrin Acetate potting fixture requires a 1/4-NPT thread. The pipe fitting will be changed out with each use. I have tried 3 tapped holes in scrap at 1/2, 5/8, 3/4 deep with letter R drill. Each will work, but if the user overdrives the pipe fitting it deforms the Delrin. A CAD drawing is supplied with the part and must be representative of the actual build. What is an acceptable depth for the tap drill when using a 4 flute hand tap?
01-19-2017, 10:16 AM #20
I'm a former DuPont employee and worked at the plant that made Delrin(TM). As amazing as Delrin properties are, it seems to me that there is potential disaster in using a plastic fitting and a metal (I assume) pipe in a user-made fitting. Mongo the super-mechanic ("Gee, if 50 lb-ft is good, 500lb-ft is better! Where's my cheater bar?") can be very ingenious in defeating supposedly fool-proof assembly instructions. I suppose brass or steel are out of the question, eh?
A minor quibble: Delrin's an acetal, not acetate.
digger doug liked this post