Some pipe tapping questions

[Sbarner]

So currently we are tapping NPT threads on our VMC. It seems to work well for threads from 1/16 NPT to about 3/8. I've got to do a couple 3/4 NPT threads and I want to threadmill them. Threadmilling NPTs is kind of a new area for me, so I have a couple questions:

 

First off, what is the preferred practice regarding the taper of the hole before threadmilling? Taper or no? If yes, then what is the diameter that is at the top of the hole? Is the tapdrill size the big part of the taper or the small end?

 

Secondly, I've got a chart that says for a 3/4 NPT tap, one would go 15/16" deep. Would I want to threadmill that deep, or more specifically, what is the depth that one would go using a threadmill? The handtight engagement?

 

Thanks in advance.

[jeff]

First off, what is the preferred practice regarding the taper of the hole before threadmilling? Taper or no?

 

Personally I don't taper my holes when threadmilling NPT's

 

The tap drill size is for the small end of the taper.

As for depth, I go as deep as my threadmill will allow me to go, then adjust my diameter to fit the gage.

[horsepowered]

I do as Jeff does as far as the depth. I go as far as the threadmill will allow and adjust. I pre taper the holes with a 2 degee endmill. This eliminates burrs at the top. But then I use a single flute thread mill for pipe threads and do it in one pass.

[Mic6]

Drill, Chamfer, mill thread, comp out to gauge fit

[Sbarner]

Thanks all. Extremely helpful. WHat diameter are you initially threadmilling to before comping the tool? The handtight diameter?

[andate caga]

Treadmill to the basic diameter. They will usually cut small, comp from there.

 

I lie the SCT staggered tooth NPT threadmills.

[jeff]

Thanks all. Extremely helpful. WHat diameter are you initially threadmilling to before comping the tool? The handtight diameter?

 

Do you have an NPT gage with a ground flat on it?

I measure the diameter where that flat is and program that as my base dia.

It's typically +/- 1 turn from that flat

[reidmachine]

So currently we are tapping NPT threads on our VMC. It seems to work well for threads from 1/16 NPT to about 3/8. I've got to do a couple 3/4 NPT threads and I want to threadmill them. Threadmilling NPTs is kind of a new area for me, so I have a couple questions:

 

First off, what is the preferred practice regarding the taper of the hole before threadmilling? Taper or no? If yes, then what is the diameter that is at the top of the hole? Is the tapdrill size the big part of the taper or the small end?

 

Secondly, I've got a chart that says for a 3/4 NPT tap, one would go 15/16" deep. Would I want to threadmill that deep, or more specifically, what is the depth that one would go using a threadmill? The handtight engagement?

 

Thanks in advance.

 

Here's a link to the folks who know threadmilling to a T

 

http://www.vargus.com/vardex/

 

Good luck, hope this helps.

[High Performance]

I threadmill lots of NPT holes. Vardex threadmills are garbage in my experience. I recommend Seco Thread mills. Dont waste your time with tapering the hole. thats old school. Some drawings call for drill. 687 and ream taper. Ignore that. Drill .718 and threadmill to size from a straight hole with a seco thread mill. it will be much faster. The exact tool I used was a .718 KSEM drill, and a 2 insert regular length NPT seco thread mill. very quick.

[High Performance]

I threadmill lots of NPT holes. Vardex threadmills are garbage in my experience. I recommend Seco Thread mills. Dont waste your time with tapering the hole. thats old school. Some drawings call for drill. 687 and ream taper. Ignore that. Drill .718 and threadmill to size from a straight hole with a seco thread mill. it will be much faster. The exact tool I used was a .718 KSEM drill, and a 2 insert regular length NPT seco thread mill. very quick.

[High Performance]

I threadmill lots of NPT holes. Vardex threadmills are garbage in my experience. I recommend Seco Thread mills. Dont waste your time with tapering the hole. thats old school. Some drawings call for drill. 687 and ream taper. Ignore that. Drill .718 and threadmill to size from a straight hole with a seco thread mill. it will be much faster. The exact tool I used was a .718 KSEM drill, and a 2 insert regular length NPT seco thread mill. very quick.