Tapered Threads

[Chris Rizzo]

Ok, I'm running (trying) some tapered threads here...m30 x 1.0 with a 1 degree taper (.5 degree per side). Should I set my threadmill taper angle parameter be set to 1 degree or .5 degree?

 

I've got it set to .5 now, and am at about .0065 overcut and still no-go.

[Jimmy Wakeford from Barefoot CNC]

The .5 sounds right. The problem maybe that the major dia is set incorrect. I think the major dia is set from where you start (bot or top). If starting at bot and setting the maj dia there it would get to big on top.

 

The way to overcome this is to use wear comp and adjust at machine.

[Chris Rizzo]

Yeah, I've been scratching my head on this one a bit.

 

-I've got an arc drawn the minor dia set at the bottom my hole, which I select as my driving geometry for the bore. Drive that with a .5 degree emdmill.

 

-Then I drew an arc, also at the bottom, with the major diameter of thread. Select that as my driving geo for thread mill.

 

-Set taper to .5 degrees.

 

Make sense? I've got her to fit at .008 overcut. Does'nt seem quite right...

 

thx for the help Jimmy.

[Harryman]

On a UN series thread, the flat at the top and bottom of the thread is .125 x pitch, right?

 

I'm not sure but I think it's pretty similar for metrics. If your thread mill has a pointy tooth form, that could easily account for why you needed to bump the diameter out a bit more than you expected.

[Code_Breaker]

What type of thread are they? NPT?

 

Code_Breaker

[Chris Rizzo]

I wish they were NPT or something quantifiable. Reverse engineering an OEM motorcycle part. Havn't been able to find this particular metric taper thread pitch in any handbook, so I've been going off of what I can get from my comparator.

 

They are m30 x 1.5 (I mistakenly said 1.0 in my first post), with a .5 degree taper per side...

 

I'm cutting an internal thread with a single point style tool, yes with a sharp point.

 

Since I can't find any legitimate thread table data, I certainly am flying by the seat of my pants here, and not suprised that I'm having "issues"...I just want to make sure that I'm entering data properly (taper angle, driving geo for minor bore, & driving geo for major thread dia.), and not going wrong there....I did get it to fit with .008 overcut (and it is liquid tite so-far), which is "probably" within tolerance. I just hate saying: "maybe probably within tolerance"...but then again threading is go / no-go..and I've got a go!

[Chris Rizzo]

Actually, it is a tapered thread, so I've got both go AND no-go....which eludes the question of whether it is correct or not!

 

Man, straight threads are easy!

[Jimmy Wakeford from Barefoot CNC]

There you go cmr.. just cut'em straight. Man that was easy.

[gallavant]

Are you using "threadmill"? If so - the "Major" diameter is what your major becomes AFTER adding taper, and if you overcut another .05" (or whatever) beyond the hole to get a clean leadout you have to add THAT to the major as well. The angle for the taper is per side. Just figured this out after making 2 bad caps with buttress threads from aluminum that are almost 4" in diameter. This is an ongoing issue with the program I guess and they have some complaints into support to fix it.

[Chris Rizzo]

I am using threadmill.

 

quote:

---

"Major" diameter is what your major becomes AFTER adding taper,

---

So are you selecting the major dia. for your driving geo at the "small end" or the "large end" of the taper? And I think that the overcut parameter is adding to the major dia....

 

thx and good luck!

[Roger Peterson]

Major diameter is at the large end of the taper. And there have been enhancement requests to add functionality to threadmill.

 

 

HTH