What's new
What's new

NPT thread dims? How do you program for CNC?

Armedsask

Aluminum
Joined
Aug 25, 2009
Location
Saskatchewan, Canada
NPT thread dims? Edit: Chart Added

I recently had to do a quick one off job cutting some external 1 1/4" NPT threads in some plastic. Rather than getting our programmer to do it offline, I figured I can just hand write a simple program at the machine.

Since it was plastic, I figured a quick turning path to produce the taper, and then thread it. I then spent an hour scratching my head and trying to calculate what diameters to turn the material to and what coordinates to program the threading too. The Machinery's Handbook gave me pitch diameters and I faked it from there until it fit since it wasn't a critical part.

It got me thinking, there must be an easier way to figure this out. How do you guys do it? It's there a chart our there or formula I can use to figure out my programing points? I hate spending an hour doing calculations just to cut some simple pipe threads. All our pipe thread is usually programmed offline so I've never really had to do with it before.

Any help is greatly appreciated.
 
Last edited:
I downloaded the trial verison of Threadpal. Great little program but I'm not paying $100 for a program I'll only use once or twice.

I drew up a little diagram in Solidworks and I'm just punching in the numbers and making up a chart. So far my numbers match up with the Threadpal, so I'll just do it that way.

I'll post the chart when I have it done so others can use it.
 
I downloaded the trial verison of Threadpal. Great little program but I'm not paying $100 for a program I'll only use once or twice.


Suit yourself.
But when the inspector comes calling with a thread dim being out a few tenths that you didn't even know about, I bet Threadpal becomes wicked cheap in comparison.
 
Like I said in my initial post, this is for jobs that are quick and dirty one offs, like some guy just wanting pipe threads cut for some project. Tolerance is checked with the corresponding fitting, not a gauge.

There is no inspector for what I'll be using this for.

The following chart was created using the data from the Machinery's Handbook. The only numbers I came up with were the Major Diameter at Face (D2), Minor Diameter at Face (D3), and Length of Taper (L2). These were done by drawing the pipe in Solidworks and plugging in the different numbers.

I make no guarantees as to the accuracy of the following chart. Use at your own risk.

Basic-External-NPT-Thread-D.jpg
 
Last edited:
If you're going through the troubles of drawing it up in Solidworks, why not just program it offline? It should be just as fast.
 
here is I think a nice description of what you have to face when cutting a NPT tapered thread

12b.jpg


Using


Notation
H = 0.866025p = height of 60deg. sharp V thread
h = 0.800000p = height of thread on product
p = 1/n = pitch (measured parallel to axis)
n = number of threads per inch
a = 30deg. = thread flank angle
ß = 1deg. 47 min. = thread taper angle for 1/16 taper
fc = depth of truncation at crest
fr = depth of truncation at root
Fc = width of flat at crest
Fr = width of flat at root

Technical Specifications for NPT Taper Plug and Ring Gauges
 
You can figure everything you need out from the Machinery's Handbook, although it seemed it was about as clear as mud. But you can get there.

For your situation my best suggestion would be to make a program for each size you are going to do, and just keep those in your machine memory. I did kind of the same thing, but with Mastercam programs since I have access to that.
 
If you're going through the troubles of drawing it up in Solidworks, why not just program it offline? It should be just as fast.

Interesting suggestion: do you have to understand how to manually turn this tricky thread on let's say a conventional lathé or would SolidWorks solve the headache for you?

The other interesting question would be: why would you need Tread(Pay)Pal besides an expensive SolidWorks licence? You would expect that SolidWorks would support NPT thread anyway?
 
I don't know what CAM software you might use, we use SolidCAM. When I model the part, I draw the taper into it and it will guide the tool on that taper. I think the angle is 1.783 degrees from centerline.

The length is determined from whatever specs are given either by the print or online information, and of course the upper diameter is the O.D. of the pipe.

CAM software makes it easy, automatically putting out the correct I value for thread taper. You would have to trig out the dimensions if you were coding it at the controller, allowing for extra Z and accounting for that in your I value. I believe the I value is negative for an O.D. right hand tapered thread.
 
Interesting suggestion: do you have to understand how to manually turn this tricky thread on let's say a conventional lathé or would SolidWorks solve the headache for you?

The other interesting question would be: why would you need Tread(Pay)Pal besides an expensive SolidWorks licence? You would expect that SolidWorks would support NPT thread anyway?

I don't speak Aland Islandian, so can someone please interpret this for me?

The fact that Solidworks ( or whatever CAD ) supports NPT threads is pretty fucking meaningless when you program and then measure the finished product.

ThreadPal tells you what to measure to what tolerance and even gives you a good starting point as to how.
 
ThreadPal tells you what to measure to what tolerance and even gives you a good starting point as to how.

I put off buying threadpal for years.. It was on my "to do" list, but I just never got around to
it.. Then one day I had a bunch of oddball threads to do... 11/16-20 UNJ type of threads...

It paid for itself with in a week.. I never had to calculate anything, I didn't have to find the
formula for thread wires, I didn't have to find a machinery's handbook, I didn't have to figure
out where I left my copy of the J thread spec, I didn't have to go googling looking for a chart for
form taps....

Just open threadpal, type in your thread and *BAM*!!!! Everything you could possibly need to
know about that thread is right in front of your face.. 30 seconds tops. It even prints
all the goodies out in a nice report form for you that you can put in the pile of paperwork
to send off to your customer.

I'd say its one of the best investments I've made, its paid for itself in saved time many times
over and its fricken CHEAP, I think $80 or so when I bought it, its $100?? now.. Worth every
penny.
 
I don't know what CAM software you might use, we use SolidCAM. When I model the part, I draw the taper into it and it will guide the tool on that taper. I think the angle is 1.783 degrees from centerline.

The length is determined from whatever specs are given either by the print or online information, and of course the upper diameter is the O.D. of the pipe.

CAM software makes it easy, automatically putting out the correct I value for thread taper. You would have to trig out the dimensions if you were coding it at the controller, allowing for extra Z and accounting for that in your I value. I believe the I value is negative for an O.D. right hand tapered thread.

That's all fine, but doesn't help you measure the part on the machine. You need to measure the pitch diameter of the first couple of threads and need to know what figure you're trying to hit.

I made a few of the larger pipe threads as gages many years ago. I used MH data to figure out the PD, which I measured using the 'two wire' method.

Even having gages doesn't always get you what you want: I have a customer who wants his pipe threads left oversize to accommodate his china made fittings which are (unsurprisingly) tapped too deep on the gage.
 
That's all fine, but doesn't help you measure the part on the machine. You need to measure the pitch diameter of the first couple of threads and need to know what figure you're trying to hit.

I made a few of the larger pipe threads as gages many years ago. I used MH data to figure out the PD, which I measured using the 'two wire' method.

Even having gages doesn't always get you what you want: I have a customer who wants his pipe threads left oversize to accommodate his china made fittings which are (unsurprisingly) tapped too deep on the gage.

It kind of does, but only in the sense that companies are using rapid 3D scanning to check parts. However it only uses the CAD model to do this and not the CAD software....
 
Programing the OD and thread info for the CNC is difficult using Machinery's Handbook info if you do it only occasionally. Did it again to clean up the program and it took a lot less time. Then I reversed it to see how easily I could do a thread from scratch using dinosaur CAD.
Today I could do it less than an hour on a new thread, next year probably longer. For threading you need your minor diameter .2 from the end of the part if that is where your threading will begin, will Thread Pal work that dimension out? How about chamfers at various places on the thread? I attached a photo and my CAD result from this part I did last year. The "A" (taper for the thread run) dimension was easy as I multiplied the length of the thread run (.7) by -.03125 to get the figure.

When I use my CAD to draw a .03125 taper per inch I get 1 degree 47 minutes and 23. something seconds instead of the 1 47 the hand book says. Is may CAD broken or is the M Handbook rounding it off?
3-8PIPER.jpg

Pipethreads.jpg
 
For threading you need your minor diameter .2 from the end of the part if that is where your threading will begin, will Thread Pal work that dimension out?

Why???

Doesn't your lathe have an acceleration distance that it uses?

And the chamfer.. Mazatrol. Start diameter (threadpal gives you that for internal and external
pipe threads, no screwing around with the handbook), angle, finish Z, and chamfer..

Turning Done.

Follow that up with the same profile for the thread, and Thread Pal
gives you the thread depth.. And your done. Quick and easy.

Usually you have to do a little tweak since the point of your threading
tool is usually set a little behind the Zzero point of the tool.. And
different threading tool nose radiuses can mess with your numbers a bit.

And the other fun thing.. There are only so many pipe threads.. Do it once
for each pitch, and then scale for diameter.. And WRITE IT DOWN!!! and
you'll never have to do it again.
 








 
Back
Top