NPT Tapping 5

[markb2]

Hello,
I am wondering about tapping a 1/4" NPT threads. The drawing from my customer shows the hole 18mm deep and tapped this depth. I see from the handbook the tapping size is 7/16". when i drill my hole then go to tap it, the tap won't go down this depth, maybe only 10mm. Should the hole be tapered ?
Also he has given me a dwg. of a 10mm thick plate with a hole drilled & tapped 1/8" NPT. I assume/guess i just tap from one side as far as the tap will go??
There must be some standard that these thread depths should be. any help appreciated.

 

[gbednar]

MarkB2,
I have a Screw Data Selector that shows the tap drill diameter and depth of effective thread per size for NPT.

For 1/8"-27 it states a tap drill diameter of 0.339"(R) and an effective thread length of 0.264" (7mm approx)

For 1/4-18 it states a tap drill diameter of 0.437" and an effective thread length of 0.402" (Less than 11mm)

As for the drawing "SHOWING" full depth threads; I would contact the customer and ask if the illistration is incorrect.

If you try and tap to what the drawing shows, you had better purchase several taps!! They break rather easily.

Hope this helps.

 

[markb2]

gbednar,
Thank you very much, this makes sense.where would i get a screw data selector like yours?

 

[gbednar]

MarkB2
This is not the exact scale I have but this is a link to site that contains the information

http://www.engineersedge.com/pipe_internal_thrd.htm

If you go to

http://www.engineersedge.com

there is information on all types threads ect...

The exact scale is made by Alvin & Co in Dallas Texas. I really don't remember where I got it. You may be able to puchase one at your local CAD supply store.

 

[EdDanzer]

Short projection pipe taps are made for shorter length pipe threads, only a few companies make them. They will require a different tap drill and may have to be reamed with a special reamer before tapping harder material.
J&L Industrial,

http://www.jlindustrial.com,

and

http://www.mscdirect.com

have them in their catalogs.

 

[mrainey]

You can get detailed dimensional data about NPT threads from this free program.

http://bellsouthpwp.net/r/s/rsnmar/METhreads.zip

 

[mrainey]

By the way, note that length of effective thread is not the same as required tap depth. My data shows that your blueprint callout of 18mm tap depth is within the normal tolerance range for 1/4 NPT (standard tolerance is +- one thread).

 

[markb2]

Thanks guys,
I think mrainey's last point is a key issue. "length of effecive thread is not the same as required tap depth." looking at your link

http://bellsouthpwp.net/r/s/rsnmar/METhreads.zip

as you have allready pointed out
it seems that the tap depth of 18mm shown on my drawing is correct. the chart says 17.445mm.
So basically i'm back to my original problem.
so with your help, we've estblished:
1)Tapping Drill 7/16"
2)Tapping Depth 17.5mm approx.
3)effective thread length of 0.402" or 10.2mm
the only way i can see of achieving the tapping depth is to increase the tapping size! or some way make a tapered hole! when the tap gets down approx.10mm then the top of the hole is smaller than the root of the tap.
Thanks guys.

 

[gbent]

To make certain NPT threads are the correct depth, a thread plug gage is needed. Some gages are marked only for "basic" depth, and some have min and max limits also. Without a gage, I would tap the holes until 6 full threads are remaining on the top of the tap. This will produce an in tolerance hole for almost all taps.

 

[markb2]

thanks gbent,
if i had a gauge then it would tell me that i needed to tap the hole deeper. but the tap wont go down any deeper.

 

[mrainey]

You say the hole depth is called out as 18mm. Are you allowing for the drill point? If not, the tap may be bottoming out on the drill point. You might need to drill deep enough to get the full diameter x 18mm deep (if allowed), or drill 18mm deep with the drill then use an end mill or flat-bottom drill to remove the drill point.

Just a thought.

 

[mrainey]

One last thought.

A pipe tap machines a tapered thread from a cylindrical hole, thus the top of the tap WILL be cutting the minor diameter.

Look at the value for "Minor Diameter at Face of Part" for an internal thread. It equals .4471, which is larger than your 7/16 drill.

Pipe tapping requires a good bit of torque, and can be a bit brutal in some materials. What sort of machine are you using. How does it stack up in terms of power and rigidity?

If your setup is marginal, you might want to consider Ed's idea of prepping the hole with a tapered pipe reamer after drilling.

 

[markb2]

no, the hole is full diameter for 18mm deep. the tap is only going down 10.5mm approx.
thanks, mrainey.

 

[markb2]

thanks for your help guys. i just got a mail from another guy with this link

http://www.sct-usa.com/pt12.asp

.

 

[mrainey]

Also some good technical discussion on this topic at:

http://groups.google.com/groups?dq=...ups?hl=en&lr=&ie=UTF-8&group=alt.machines.cnc

 

[diamondjim]

Markb2,
You might ask the customer what his mating part looks
like. Normally the depth of a tapered pipe tap is not
shown. His requirement does not make any sense unless he
is using some non-standard male thread. The answer might
be to provide a counterbore at the surface if he is
certain about the depth. Ask if that is an option.

 

[grinderguy]

I have been thru this many times. What your customer says will determine what you do. Here are two things to know. Use a tapered pipe reamer after the tap drill. This reduces the chip load. Nearly Every tool catalog will have them. The normal or standard pipe thread gauges are not "plus or minus" the ground reference line. Read the explanation that comes with the gauge, Do-all has the one I use.

Robert Setree

http://www.advanced-grinding.com

 

[CARDIACKID]

FROM MY EXPERIENCE, THIS IS KNOWN AS A "SHORT PROJECTION" TAP. YOU WILL NEED TO GRIND YOUR TAP TO THE CORRECT LENGTH
IE. REMOVE THE LEAD-IN THREADS, TO ACHIEVE YOUR 18MM(.708&quot
NO, THE HOLE IS NOT TAPERED. THE TAP IS TAPERED. THATS'
HOW YOU ACHIEVE A SEAL BETWEEN YOUR FEMALE/MALE THREADS.
WHERE DOES THE CUSTOMER WANT TO SEAL, AT TOP OR BOTTOM OF HOLE? STANDARDS SAY 1/4-18 NPT IS 7/16"DIA. HOLE X 7/16" DEEP. ROUGH CALCULATIONS YOU NEED TO GRIND OFF .074" OFF
THE END OF YOUR TAP TO ACHIEVE GAGE AT 18MM.

 

[Mechineer]

Are you doing this on a CNC machine or a manual machine? If your doing it on a CNC machine thread mill it.