Sign in to follow this  
Followers 0
Shawn Wentzel- Wenteq Inc

NPT carbide threadmill

9 posts in this topic

I am trying to do a 3/8 NPT thread with a carbide threadmill that has 12 teeth. The tool has the taper built in so do I not need a taper angle in the threadmill parameters?

Share this post


Link to post
Share on other sites

I haven't machined a NPT thread in a while, but when I did, we had a set depth value we would go to, mill a plain circle(with proper in/out of course), then comp the tool out until the gauge fit right. In this case, you shouldn't need to put in an angle value, just do 1 revolution or add a finish pass, but if it was a single point cutter you would use the angle value on a prepped hole.

Share this post


Link to post
Share on other sites

quote:

You need the angle for the threadmill to follow.


+10000

 

It will not work without it!!!

Share this post


Link to post
Share on other sites

It WILL work but it is not correct. When I first started with npt we didn't use the angle and never had a problem with the npt sealing. But I have started to use it. Mastercam makes it easy. The angle is 1 degree 47 minutes. I think I use 1.78 degrees.

Share this post


Link to post
Share on other sites

you need the program to follow an angle?

even if the cutter has the angle on it?

headscratch.gif

I'll have to try that next time, I've always just done 1 revolution with skim passes and it's turned out just fine for me.

Share this post


Link to post
Share on other sites

Jeff, if you do more than one rev, it will be pulling up away from the angled profile if you don't use the angle value. Actually, even less than a full rev will pull it away, you just won't notice unless it were a pretty coarse thread.

Share this post


Link to post
Share on other sites

The thousands of internal pipe threads I have machined, I have never added a value in the taper angle box and never had a problem with the threads. Hmm, maybe I outta try it with the taper angle next time and see what happens. Using the threadmill toolpath and a 3/8-18 NPT, I have used the following parameters (conservative to me, but have worked very well) using an Accupro thread mill (.360" dia, MSC item #02154854). .675" Major Diameter, .5625" Drill Diameter, 11 active teeth, 2100 rpm @ 5 IPM, .611" depth, .055556 pitch, 5 multipasses at .015" with a spring pass.

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!


Register a new account

Sign in

Already have an account? Sign in here.


Sign In Now
Sign in to follow this  
Followers 0

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us