NPT female thread

[newtoid1986]

Hi guys,
I've got 120 stainless parts to turn with a 1/8"-27 NPT female thread. I've been given a tap specifically for stainless.
I want to be nice to the tap so I'd like to vote an internal taper before tapping.
Online data tells me to drill first 8.4mm.
My question is what taper angle do I machine and how deep?
The 8.4 hole can be through the 20mm long part.
Thanks in advance

 

[Booze Daily]

Taper angle is in the Machinist's Handbook. Bore until it washes out to your thru hole.
You'll want a smooth taper gage (L2?) for 1/8 NPT to know when your minor is correct.

 

[Jhn3:16]

NPT Taper Angle is 1°47'
Not sure how deep to bore as typically wouldn't cut taper when using a tap, just drill the hole. Although I do understand taking good care of a tap in stainless!
What do you have for a gauge?

Brandon

 

[deadlykitten]

aint it possible to use a knife ? ... i will check to see if i have data for that thread


if it is tapered, than there will be a lot of pressure on the tap, while a knife will take it easy

 

[deadlykitten]

here, if the tap fails :

ISCAR Cutting Tools - Metal Working Tools - IR/L-NPT
ISCAR Cutting Tools - Metal Working Tools - IR/L-NPTF

about dimensions and stuff, i have not looked yet ... maybe you/someone will figure it out

if not, just ring a bell

 

[litlerob1]

If you are dead set on boring the taper it is .75" per 12". But I'll say this, I have tapped a bunch of NPT holes, a bunch meaning more than I care to even guess at. I never bore a taper, unless it's in Inco, Hastelloy, Hardox or some other bullshit from Neptune or Saturn or wherever they get that garbage. I just drill it and tap it, the tap will create the taper for you. So if your doing it to save the tap, meh, it isn't that hard on the taps. But if your doing it for the needed application, some wanker is going to be in there with a taper gage or something then there you go.

 

[Limy Sami]

Or use a reamer to taper the hole, like these Taper Pipe Reamers - MSCDirect.com

 

[BALNH]

Saw your turning

We drill them, dust the hole with an endmill to pilot size, then threadmill with a full form threadmill. We do this in 316 and 304. The thread quality is far superior to a tap. When you program make sure to program the correct taper angle in the helix.

Oops just saw that your turning. Never mind.

 

[doug925]

If I am (on a lathe) drilling the Q drill for an 1/8"NPT, I don't bother with tapering the hole, beyond the entry chamfer.
Once we go beyond 1/2" NPT we drill and bore the part (entry chamfer, and taper) prior to single point threading.

As pointed out above, the taper is 0.75" per foot, included. That is 0.0625" / inch, included, or 1/32"/inch on a side.

Doug.

 

[Ox]

If it's 303, I would think that you should not need the taper reamer on 1/8".
I don't get into that usually until about 3/4" ???


If it's NOT 303, then you should be thinking about not using a tap in the first place.





edit:

As noted above by '925, while it is listed as "R" being the tap drill for 1/8" NPT, you will need to use a Q if you are planning on checking with a profile guage for NPTF.




-----------------------

Think Snow Eh!
Ox

 

[Gerrythewelshman]

tapered threads

I hope i have att. my info