thread mill 3/8 NPT internal???

[Bill H]

I need to mill some internal 3/8 NPT threads using a single point tool.  It seems that in order to do this I need to know the depth of the thread plus its major diameter at either the big end or the small end.  I've looked at so many charts my head is spinning and I'm just not getting it.  Can some please just give me the friggin' numbers?  Thanks!

[crazy^millman]

You got a machinist hand book? You also need the correct plug gage to check the depth. They of course are tapered and can be handled many different way. Look in the machinist hand book or even do a goggle search.

 

Engineers Edge has it look it up over there.

 

HTH

[Bill H]

I've looked at so many charts my head is spinning and I'm just not getting it.  Can some please just give me the friggin' numbers?  Thanks!

 

Ron - Please see my original post. 

[CADCAM3D5AXIS]

Hi Bill

Try these Numbers

http://www.engineersedge.com/hardware/taper-pipe-threads.htm

Hope that helps it looks like it is what you need  plus you do need a gauge or a mating part so you do not over cut .

[Bill H]

I guess I wasn't clear.  I've got the Machinist's Handbook and have seen a million other online charts similar to what's on the Engineer's Edge site.  I don't understand them.  The Engineer's Edge chart, for example, shows five different lengths (L1 through L5).  None of these seems to be the depth that I need to program to if I'm trying to mill a 3/8 internal NPT thread with a single point cutter.  Is the programmed depth a combination of some of these lengths and, if so, which ones?  Likewise, all of the diameters shown are to the thread's pitch diameter.  I need the major diameter at either the top or the bottom of the thread.  How do I get this dimension?

 

Sorry if I sound snotty, I'm just really tired and frustrated.

[Dont]

I guess I wasn't clear.  I've got the Machinist's Handbook and have seen a million other online charts similar to what's on the Engineer's Edge site.  I don't understand them.  The Engineer's Edge chart, for example, shows five different lengths (L1 through L5).  None of these seems to be the depth that I need to program to if I'm trying to mill a 3/8 internal NPT thread with a single point cutter.  Is the programmed depth a combination of some of these lengths and, if so, which ones?  Likewise, all of the diameters shown are to the thread's pitch diameter.  I need the major diameter at either the top or the bottom of the thread.  How do I get this dimension?

 

Sorry if I sound snotty, I'm just really tired and frustrated.

If you have a gage go .625 deep put 1.7899 in angle and use .612 Dia for major to start comp tool till gage is good.

[Dont]

If you have mastercam lathe do a thread in there has a thread chart in thread op. I wish mill had the chart.

[Dont]

Monday I could post up some numbers I use that are safe I always have to comp tool to dial in with gage.

[jlw™]

Monday I could post up some numbers I

 

use that are safe I always have to comp tool to dial in with gage.

Always have to sneak up on threadmills, especially tapered threads.

 

I do believe your overthinking it.

 

What material is it? Unless it's just a wicked material i prefer tapping for pipe threads.

[Dont]

Monday I could post up some numbers I

use that are safe I always have to comp tool to dial in with gage.

 

Always have to sneak up on threadmills, especially tapered threads.

I do believe your overthinking it.

What material is it? Unless it's just a wicked material i prefer tapping for pipe threads.

I'm not the one that needs the help.

[Dont]

Monday I could post up some numbers I

use that are safe I always have to comp tool to dial in with gage.

 

Always have to sneak up on threadmills, especially tapered threads.

I do believe your overthinking it.

What material is it? Unless it's just a wicked material i prefer tapping for pipe threads.

I only machine plastic where I work taps leave mean burrs shrink and thread milling leaves a much nicer thread and you can comp as tool wears.

[crazy^millman]

I guess I wasn't clear.  I've got the Machinist's Handbook and have seen a million other online charts similar to what's on the Engineer's Edge site.  I don't understand them.  The Engineer's Edge chart, for example, shows five different lengths (L1 through L5).  None of these seems to be the depth that I need to program to if I'm trying to mill a 3/8 internal NPT thread with a single point cutter.  Is the programmed depth a combination of some of these lengths and, if so, which ones?  Likewise, all of the diameters shown are to the thread's pitch diameter.  I need the major diameter at either the top or the bottom of the thread.  How do I get this dimension?

 

Sorry if I sound snotty, I'm just really tired and frustrated.

 

Well you do sound snotty and I have done my share of 30 hour straight shifts when no internet to help me. I had to look all of this up in my machinist handbook and figure it out almost 2 decades ago.  The taper is 1° 47'′ 24"″ (1.7899°) and like I said you get the correct gauge supplied to you by the company you are working for. You program it nominal and then adjust your size till the gauge fits correctly. I can throw many different numbers at you, but the gauge is you best way to machine the correct size on NPT. I had a customer 20 years ago reject $50k of parts all made to the standard, because they didn't stack correctly like their previous supplier. I took our gauges onsite and showed them all they were correct to the standard and they had to buy the parts. Come to find out the parts they were trying to mate them to were never made correct before. It was always just a make a thread and call it good enough. Once I showed them how we were machining the parts they gave us more work because we were making everything to the approved standard. Once they were using all of our parts they never had another problem again.

 

Make with a gauge you are good try to make it to some numbers and you risk making bad parts.

[Matthew Hajicek - Singularity]

This is for steel, so multiple passes and with a full profile tool.  Working backward, I do two passes at nominal, one 20% of the material away, and another an additional 30% of the material away.  The material is figured as the radial distance from the pilot hole to the major diameter of the thread.  Also, the larger the pilot hole is the better; I tend to use 50% thread in steels unless otherwise specified.

 

 

 

 

[Bill H]

You program it nominal and then adjust your size till the gauge fits correctly. I can throw many different numbers at you, but the gauge is you best way to machine the correct size on NPT.

Ron Branch -

 

I really appreciate you taking the time to respond and I am in complete agreement that a gage is necessary to make sure the parts are machined properly.  However, I still need nominal values to create the program in the first place.  I tried to explain that I don't understand which dimensions to use from the Machinist's Handbook and various other tables.  Can you enlighten me?  For example, when Mastercam prompts me for the Thread Depth on the linking parameters page, what dimension from the Handbook table do I use here?

[Bill H]

Matthew Hajicek -

 

Thank you!!!!  This is the information I've been looking for.

[jlw™]

I only machine plastic where I work taps leave mean burrs shrink and thread milling leaves a much nicer thread and you can comp as tool wears.

Easy there big fella, only quoted you to ditto sneaking up on threadmilling.

 

Threadmilling usually is the way to go in plastics.

[Brian B 74]

I have this pinned up in my cubicle.  This is what I use for my threadmilling of NPT threads.

 

https://sizes.com/materials/pipeThrd.htm

 

 

[Tinyfxds]

This is the chart we always use for thread milling.  http://www.trentonpipe.com/ti_threadformdatachart.html 

 

The first 4 rows have all the information about the size of the thread and the pipe that the thread is on.

 

The 9th row from the left gives us our thread depth and the 2nd to last row gives us our tap drill size.

 

I also wrote on the paper copy of this sheet that the taper is 1.783333 degrees.

 

If you want to add a nice chamfer to these holes just add  .030" to the diameters in column 2

 

I've been using this chart for 15 years without a problem.