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?
0
NPT carbide threadmill
Started by
Shawn Wentzel- Wenteq Inc
, Sep 03 2010 08:56 AM
8 replies to this topic
#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
-
- Members
-
- 3,179 posts
Advanced Member
- 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
-
- Members
-
- 515 posts
Advanced Member
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
-
- Members
-
- 857 posts
Advanced Member
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
-
- Members
-
- 6,402 posts
Advanced Member
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.
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
-
- Members
-
- 5,681 posts
Anigilohi
- 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.
#9
peon
-
- Members
-
- 977 posts
Advanced Member
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.
