Jump to content

Welcome to eMastercam.com
Register now to gain access to all of our features. Once registered and logged in, you will be able to create topics, post replies to existing threads, give reputation to your fellow members, get your own private messenger, post status updates, manage your profile and so much more. This message will be removed once you have signed in.
Login to Account Create an Account
Photo

NPT carbide threadmill

- - - - -

  • Please log in to reply
8 replies to this topic

#1
Shawn Wentzel- Wenteq Inc

Shawn Wentzel- Wenteq Inc

    Member

  • Members
  • PipPip
  • 183 posts
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?

#2
Guest_CNC Apps Guy 1_*

Guest_CNC Apps Guy 1_*
  • Guests
You need the angle for the threadmill to follow.

#3
Mic6

Mic6

    Advanced Member

  • Members
  • PipPipPip
  • 3,248 posts
  • Location:Sunnyvale, Ca
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.

#4
CNCGUY

CNCGUY

    Advanced Member

  • Members
  • PipPipPip
  • 515 posts

quote:


You need the angle for the threadmill to follow.

+10000

It will not work without it!!!

#5
doyleg

doyleg

    Advanced Member

  • Members
  • PipPipPip
  • 857 posts
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.

#6
jeff

jeff

    Advanced Member

  • Members
  • PipPipPip
  • 6,605 posts
you need the program to follow an angle?
even if the cutter has the angle on it?
graemlins/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.

#7
Zoober

Zoober

    Anigilohi

  • Members
  • PipPipPip
  • 5,707 posts
  • Location:Valencia, Ca.
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.

#8
peon

peon

    Advanced Member

  • Members
  • PipPipPip
  • 1,031 posts
n/m

#9
peon

peon

    Advanced Member

  • Members
  • PipPipPip
  • 1,031 posts
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.