NPT thread milling question

[R&C]

I bought a Accupro carbide 1/4-18 npt thread mill - the tool came from MSC page 392 order # 02154854

its a Helical design.Its a 4 flute ( end Mill type)

Now for my question. I asked the supplyer how to use the cutter as i have never used one.

They told me to go down to depth and circle mill around inside the pre drilled hole and it cuts the thread.

 

This does not work. it looks like it just cut groves. Has anyone one here used them ?

Do i need to Helex one thread pitch ?

I have asked everyone i can i search on the fourm but did not come up with anything.

Thanks

[Hardmill]

I bought a Accupro carbide 1/4-18 npt thread mill - the tool came from MSC page 392 order # 02154854

its a Helical design.Its a 4 flute ( end Mill type)

Now for my question. I asked the supplyer how to use the cutter as i have never used one.

They told me to go down to depth and circle mill around inside the pre drilled hole and it cuts the thread.

 

This does not work. it looks like it just cut groves. Has anyone one here used them ?

Do i need to Helex one thread pitch ?

I have asked everyone i can i search on the fourm but did not come up with anything.

Thanks

 

 

Yeah youll need to helix just like any other threadmill.

 

 

 

 

 

 

 

 

 

 

 

 

PEACE

[R&C]

On utube they show clips of the tool just going around the hole.

do i need to helix all the way up or just one thread pitch?

[R&C]

[Hardmill]

I would guess one pitch.

See if someone else chimes in whos done it before

 

 

 

 

 

 

 

 

 

 

 

PEACE

[Jeremy Herron@DBS Solutions™]

I do threadmill with taper angle of 1.76 or whatever it is. If you want to verify, I always open lathe and do a threading toolpath and tell it draw thread and check the geometry it creates.

[Jeremy Herron@DBS Solutions™]

And as long as it has enough teeth for the depth of thread one pitch is plenty.

[RobertELee]

I've always done 1 1/4 thread pitches just to make sure everything is clean and smooth, but with the tapered nature of a pipe thread it will hardly cut anything after that one revolution.

[R&C]

Thank you all for your help. i should have came here first.

[gcode]

you need to use the Thread mill.

It a sub menu of the Circle toolpaths

You need to set the correct pitch which is 1/18

and define the proper circle diameter.

I'm not sure what that is, but will post in the morning when I can look it up at work..

 

ps moving this to the main fourm as well

[Manuel0822]

I know it's a little too late now but if you take a look at that video you posted at 0:24, you will see how the animation has a red arrow pointing up for right hand thread and pointing down for left hand thread a little later.

 

As just described above you need to go 1 pitch helix for multi teeth cutters and the full helix to depth for single teeth cutters. +1 to Gcode on using thread mill tpath for it.

 

HTH

[gcode]

The Stellram threading app gives the following for a 1/4-28 NPT

You should define the hole the threadmill cuts at Ø.536

Your depth should be .4, though I usually go about .050 deeper

Pitch will be 1/18 or .0556

You should set your number of teeth bug enough that the toolpath only makes one pass.

If the LOC is .75 is would be (.75/.0556) = 13.48 so set it at 13