Jump to content


- - - - -

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

Posted 03 September 2010 - 08:56 AM

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

Posted 03 September 2010 - 10:50 AM

You need the angle for the threadmill to follow.

#3 Mic6

Mic6

    Advanced Member

  • Members
  • PipPipPip
  • 3,235 posts
  • Location:Sunnyvale, Ca

Posted 07 September 2010 - 03:26 AM

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

Posted 07 September 2010 - 04:22 AM

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

Posted 07 September 2010 - 09:33 AM

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
  • 6,569 posts

Posted 07 September 2010 - 09:47 AM

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
  • 5,691 posts
  • Location:Valencia, Ca.

Posted 07 September 2010 - 10:26 AM

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
  • 1,029 posts

Posted 08 September 2010 - 04:57 AM

n/m

#9 peon

peon

    Advanced Member

  • Members
  • PipPipPip
  • 1,029 posts

Posted 08 September 2010 - 05:04 AM

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.