programming NPT taps so no one has to "tweak"

[jlw™]

Gentlemen,

 

For myself and guys I trust I always program NPT taps so that they start and go to a safe depth.  Then the guy running it gages it and goes in the program to adjust the G84 Z so that it goes to depth and then go on about business.

I'm at a point where I have a few I don't want doing that yet.  Is there a formula that any one is using to get NPT taps to go to depth with out adjustment?  We run so many flavors (basically what ever is cheapest) on NPT taps that I can't just measure one and go with it.

 

It's never been a concern before but we have some young guys who are learning.  I need to play it safe as possible.  You guys  who ship your program cross country, how do you handle NPT taps?

[Sticky]

If you want a set value that will gage the same every time, you HAVE to standardize your actual tap MFG and PN.

 

Another option is threadmilling, but even with that you usually need to fudge the cutter comp or your geometry in mc to get it to gage right.

 

That said, once you have a process with either method, and dedicated tooling, you can pretty much gaurantee it will come out right as you transfer it to other jobs. Time well spent IMO.

 

Once you start threadmilling npt you probably won't want to go back to tapping.

[The Cathedral]

 

 

Once you start threadmilling npt you probably won't want to go back to tapping.

 

^^^^^^

 

Once you have a standard set of tooling, it's easy to do. Program it once, tweak it until it's good, and save those parameters for future use. Save your tools to a specific library for each material type, and then it's pretty much drag and drop for future programs.

 

There are too many variables when you are using multiple manuf. tap brands, especially if it's not you picking out the tap for the setup.

[crazy^millman]

If you want a set value that will gage the same every time, you HAVE to standardize your actual tap MFG and PN.

 

Another option is threadmilling, but even with that you usually need to fudge the cutter comp or your geometry in mc to get it to gage right.

 

That said, once you have a process with either method, and dedicated tooling, you can pretty much gaurantee it will come out right as you transfer it to other jobs. Time well spent IMO.

 

Once you start threadmilling npt you probably won't want to go back to tapping.

 

I agree been threadmilling NPT for well over 20 years and I shake my head every time I see someone tapping NPT. Better quality thread and better finished and never the worry about hitting the correct depth You have it all figured out and make the toolpath and done. I had a Mill guy mad as all get up I was thread milling the NPT using a Standard Threadmill not to long ago. He was telling me there was not way to make a NPT with a standard Threadmill of the same pitch. I just laughed and said watch. Once it was all said and done and the NPT threads were perfect and looked like new money he had nothing else to say about that.

 

To me it is like asking a lathe guy to go get a Thread die to cut OD threads on a CNC Lathe. Anyone with any kind of experience you ask to do it. Same thing for me tapping a NPT hole. Forget the tap and Threadmill it and have a nice day.

[Newbeeee™]

I've only ever made NPT threads for tooling so it doesn't really matter ie not a production (real) job.

I've always tapped and could never stop the vertical line that runs up the tread.

So I would say threadmill for this very reason

[civiceg]

Skipped tooth NPT taps and pecking help to make a pretty thread. 

[Mike@Lustre]

Skipped tooth NPT taps and pecking help to make a pretty thread. 

 

 

yeah stagger tooth NPT taps can work really well , used them a lot on 316SS and Aluminum Bronze parts , way less cutting pressure to produce a quality thread .

 

and I have to agree , to do it right using taps you have to use one source for taps and stick with that source , each NPT tap brand I have used have all had shuttle differences in design .

[Oppiz]

I've never got a handle on thread milling.    I bought a couple thread mills to try and busted them and never went back.  Maybe I'll take another stab at it. Any help?

[Rstewart]

Maybe you could post up a file that you created with Your threadmill tool and Path.   Myself or one of the other very knowledgeable peeps could have a look at it.

[crazy^millman]

I've never got a handle on thread milling.    I bought a couple thread mills to try and busted them and never went back.  Maybe I'll take another stab at it. Any help?

 

Anytime. Shoot me and email and if I am too busy I will ask someone in the group to take a look. I think this is a must in today's manufacturing.

[jlw™]

I'll help you too.  Threadmilling is the way to go.

 

Send me a file or two and I'll put a few paths and some tool in it.

[Mike@Lustre]

how small of a thread do you thread mill ?? my co-worker has done tons of thread milling in his day and stated the used it for threads over 1" .

[Guest]

how small of a thread do you thread mill ?? my co-worker has done tons of thread milling in his day and stated the used it for threads over 1" .

 

I've gone down to 4-40

[Sticky]

how small of a thread do you thread mill ?? my co-worker has done tons of thread milling in his day and stated the used it for threads over 1" .

 

We thread mill down to 1/8npt, I would do 1/16" if I had the need and much smaller.

 

The most common problem issue I see with peoples threadmill problems are that they don't properly calculate the feedrate for having such a large tool in a small diameter.

[djstedman]

We do thread milling as small as 2-56 and have gone up to over 12 inches in diameter. 

 

On one particular part we have done thousands of 2-56 holes.. in 15-5PH Stainless - For a lot of materials thread milling is the way to go if you ask me.. done right its as fast or faster than tapping and a more reliable process.

[Newbeeee™]

M3.

That said, we've just gone over to DC taps for stainless and no threadmilly!

[Oppiz]

I mainly thread holes from 4-40 up to 3/8-16.  I might have time today to mess with threadmilling. Thanks for all the help offers and I will be taking you up on them. BTW the machines I'll be trying this on  are a Okuma Genos 560 and a Cinci with a fanuc 18I

[Sticky]

done right its as fast or faster than tapping and a more reliable process.

 

 

I can't agree with that. Any modern tap is going to tap a gage worthy hole 3-10x faster than thread milling. But all that speed isn't worth anything if you have to babysit the operation.

 

[djstedman]

I started that comment with "For a lot of materials thread milling is the way to go if you ask me"  .. in that context I stand by what I said..

 

I didn't mean to imply thread milling would always be faster than tapping.

[Sticky]

I only responded to the speed part of your statement. I also like thread milling, but it is WAY slower than tapping.

[jlw™]

I only responded to the speed part of your statement. I also like thread milling, but it is WAY slower than tapping.

I agree. I tap with OSG Exo taps all the time. Especially through holes where I know I can go deep enough so they don't have to chase them. Ended up running the Vtech some today after the A team went home for the day. Ran an OSG M24 tap 2.5in deep, 16x. Took just under 4 minutes. I love me some thread milling but in applications that just need threads... let that tap eat.

[crazy^millman]

I agree. I tap with OSG Exo taps all the time. Especially through holes where I know I can go deep enough so they don't have to chase them. Ended up running the Vtech some today after the A team went home for the day. Ran an OSG M24 tap 2.5in deep, 16x. Took just under 4 minutes. I love me some thread milling but in applications that just need threads... let that tap eat.

 

I agree, but the topic was NPT so my answer was directly to that instance and that instance only not meant as a blanket statement that all threading with milling must be threadmilling.

[jlw™]

I agree, but the topic was NPT so my answer was directly to that instance and that instance only not meant as a blanket statement that all threading with milling must be threadmilling.

I greatly appreciate your input too! I was just chasing the conversation.

 

I guess it's a case by case preference for me.

[BenzB]

For a standard projection NPT tap 12 turns deep will get you pretty darn close to the gage depth. Typically within 1/2 turn of the flat on the gage. Doesn't matter who makes the tap. Short projection taps are another matter. I haven't dealt with them but there should be an industry standard that they are made to.

Having said that, I have to agree with the threadmilling advocates. Write the program once, dial it in and save it. Treat it as a subroutine. Use the same threadmill everytime and it becomes a no brainer. It is also a lot easier to adjust the thread with cutter comp than with a tap wrench. If you've ever tried to drive taps over 3/4" manually you'd appreciate threadmilling no matter how long it takes.