What's new
What's new

#### M Code

##### Aluminum
Hello,

I am using NPT Thread Calculator to calculate the NPT thread dimensions.
But I am confused
Drill size is 7/16” but how long is deep?
Thread Size is ¼ with 18 TPI but what is the total depth of the thread?

My understanding for example ¼ NPT will include

= 0.2278 + 0.1667 = 0.3945
If total depth = 0.3945
Drill 7/16” depth can be 0.6945” for clearance only (flexible)

Is this the way to calculate NPT machining dimension?
The value 0.2278 will be inspected using the plug gauge?

Thanks,

#### werkzeug

##### Plastic
I tap a standard 1/4-18 Pipe Tap 0.95 in. deep to get to plug depth

#### M Code

##### Aluminum
I tap a standard 1/4-18 Pipe Tap 0.95 in. deep to get to plug depth

My problem is how to specify drill depth and thread depth

#### gregormarwick

##### Diamond

My problem is how to specify drill depth and thread depth

You don't specify the depth. NPT is a gauged depth taper thread.

#### M Code

##### Aluminum
You don't specify the depth. NPT is a gauged depth taper thread.

I mean by the depth how long is the traveled point in Z -Direction (starting point) when performing NPT thread mill operation?

Thanks

#### M Code

##### Aluminum

Thank you so much, in this for 1/4 - 18 thread starting point generated as Z-0.3945.

However, before thread what is the depth of drilling operation?

What about the chamfer or thread relief is it going to be counted from the threads turn or no? in other word during inspection the flush from the chamfer or after the chamfer?

What is the depth and angle of the chamfer?

Thanks sir

#### Booze Daily

##### Titanium
Well, you're going to need to drill deeper than .3945.
Flat on the gage should be flush to face +/- 1/2 turn.
Caliper across the gage at the dia of the flat. Your chamfer needs to be bigger than that. 45 deg typically.

#### GENERALDISARRAY

##### Hot Rolled
Measure the cutting length on the threadmill you are using. That is my cut depth for the threadmill. The drill depth obviously needs to be greater than that.

As per the asme b1.20.1-2013 the gaging point is the point of last thread scratch on the chamfer. Where the chamfer exceeds the major of the thread. Try to keep your chamfer theo as close as possible to the major as you can. Since most people expect the gage flat to be flush with the end of the part. Regardless of chamfer. The chamfer angle is not covered in the spec that I see. I use a 90 deg included spot tool.
Dont forget

#### M Code

##### Aluminum
Measure the cutting length on the threadmill you are using. That is my cut depth for the threadmill. The drill depth obviously needs to be greater than that.

As per the asme b1.20.1-2013 the gaging point is the point of last thread scratch on the chamfer. Where the chamfer exceeds the major of the thread. Try to keep your chamfer theo as close as possible to the major as you can. Since most people expect the gage flat to be flush with the end of the part. Regardless of chamfer. The chamfer angle is not covered in the spec that I see. I use a 90 deg included spot tool.
Dont forget

Thank you sir.

So I understand:
1- not all the chamfer length is included in gauging, only after the first thread appear on the chamfer, gauging point will start
2- chamfer 45 Deg. can be 0.04" per side (thread height) in case of 1/4 - 18

the cutting length of the tool is 0.598" but in the case of 1/4-18 what if machining 0.3945" deep as per tables (L1+L3)... does the tool need to fit for all the cutting length to perform the (Hand-tight Length)??

#### M Code

##### Aluminum
Well, you're going to need to drill deeper than .3945.
Flat on the gage should be flush to face +/- 1/2 turn.
Caliper across the gage at the dia of the flat. Your chamfer needs to be bigger than that. 45 deg typically.

Chamfer Deg. is 45
Length of the chamfer can be the thread height?

#### Booze Daily

##### Titanium
Chamfer Deg. is 45
Length of the chamfer can be the thread height?

Yes.
Tool only needs to go .394 deep. You can use comp to get the gage to fit.
The extra length is because that thread mill can also cut 3/8 NPT which has a longer length of engagement.

You are probably overthinking this. Just make the gage fit and make it look pretty.

#### M Code

##### Aluminum
Yes.
Tool only needs to go .394 deep. You can use comp to get the gage to fit.
The extra length is because that thread mill can also cut 3/8 NPT which has a longer length of engagement.

You are probably overthinking this. Just make the gage fit and make it look pretty.

What if the tool go deep more than .394 like 0.53

is that going to be ok for 1/4 NPT? since the gauge is fit with hand-tight lenght

#### LKeithR

##### Stainless
...You are probably overthinking this. Just make the gage fit and make it look pretty...

I would think that it would be easy to make a couple test pieces and adjust from there. I'm strictly
manual so I don't thread mill but when I tap pipe threads the drill goes in all the way or right through
the part. No consideration given to the drill depth. Would it be different if you're thread milling?

#### mjk

##### Titanium
re drill depth
if its an NPT or any pipe thread, pretty good chance its drilled to cavity depth of the area where the (liquid or gas) is contained
Rarely will you see a blind pipe thread unless its a special application for a future access connection

Replies
18
Views
2K
Replies
2
Views
1K
Replies
6
Views
1K
Replies
19
Views
4K
Replies
25
Views
3K