1 inch 56 thread mill

[mike561h]

Hi guys,

 

Never did this before. Can anyone lay me out on threading a 1 inch 56 into brass. The boss does not wantt o do in the cnc lathes. What tool should I order ?

Thanks

[88Matt]

how deep it the tap hole?

If this isn't a thread u make often i would use a single point thread mill. Cycle time will be alittle longer than if u use a 56 pitch multitooth cutter, but it will cut pretty fast in brass.

[Tim Simmermon]

You would have to go with a single point thread mill such as the one linked below. It would be the most economical way as I believe you would otherwise have to make a special.

 

http://www1.mscdirect.com/CGI/NNSRIT?PMPXN...&PMT4NO=9474376

[?Mark]

quote:

---

The boss does not wantt o do in the cnc lathes

---

Why the hell not?

If it's possible to do it on a lathe, it'll almost always be the easiest way to go...

[mike561h]

the cnc lathes are backed up and he wants to do the threading on the other side when we face to size. it will be going .5 deep thread.

 

thanks,

[Storkman]

so 28 threads, single point sould run pretty fast.

[mike561h]

tim ,

 

i am confused on identifying the tool pitch 56 diam. 1. ?????

thanks

[88Matt]

56 threads per inch

1" / 56 = 0.0179" pitch

 

This what u r asking?

[Tim Simmermon]

Mike,

 

Have you threadmilled before?

[mike561h]

no threadmilling experience. ;o(

[PGW Steve]

Hmmmmm if a guy had a 28 tpi insert and ran the program twice with a second start point one pitch higher........

[Tim Simmermon]

Mike,

 

Check out this thread (active today). They have some great info there.

 

http://www.emastercam.com/ubb/ultimatebb.p...ic;f=1;t=021674

 

With a single point tool, the tool will engage to your major OD and then helix with a Z level change that equals your pitch (.0179"). So everytime that your tool goes around in a full circle it will move .0179" in the Z. You can either start at the bottom and work your way up, or start at the top and work your way down. The advantages of both are discussed in the other thread.

[Psychomill]

Vardex makes a 56 pitch threadmill insert in several sizes and lengths. That's what I use to mill a 1"-56 thread in brass, SS, aluminum etc....

 

Check here....

 

[Rick Henrickson The Boeing Co.]

I dont think the 28 pitch would work it would be a 2 start thread wouldn't it?

[PGW Steve]

Stupid me LOL

[Storkman]

Actually I don't do alot of threadmilling. But could you not use a 14tpi? The first tooth would cut the 1st thread and the second would cut the 4th thread. Just run the pitch for 56tpi and run around it 3 times. Am I wrong again?

[88Matt]

for ease and quality, i'd use the single thread mill. u r not really gaining much on your cycle time with anythingelse. IMHO

 

Matt

[Rick Henrickson The Boeing Co.]

14 tpi would give you a 4 start thread no worky

 

88matt I think getting the multi pitch threadmills are much faster than single pointing

[Guest]

Multiple tooth is the way to go if you can find one. In many cases you can complete your thread in 1 rotation.

 

Single points work well when needed but you must machine the entire length of the thread

[Storkman]

quote:

---

14 tpi would give you a 4 start thread no worky

---

 

To my thinking. the first tooth after 4 revolutions would blend to the second tooth. I see no 4 start thread in there.

[Guest]

That's the problem Terry, you're thinking again.

 

[Rick Henrickson The Boeing Co.]

I am not positive was just thinking

[Charlie Pierson]

Methinks the lead of the th'd would be ok but

the geo at the major dia's crest would have much too large a radius.

Might work if the th'd mills teeth came to a point.

Then again, if the 14p th'd mill id used like that for a 56p thread, there might be clearance problems in the th'd form due to helix angle differences.

 

my .02

 

cp

[crazy^millman]

Ok so some things have been thrown out here. Do not use the 14 TPI insert for this reason alone that no one is thinking about. The raduis on a 14 is alot different than a 56 so you will lose the effect thread you have by doing this the same applies to the 28 insert again they are made for full profile and you are not doing full profile threads for a 56 if you use them.

 

The full profile insert is desined to make a full thread top and bottom when used with the correct Minor Dia. It put the correct radius in Creast or Major dia of the thread and then puts the correct radius on the root of the thread which is the minor.

 

If you can not get him to spend the money on a 56 insert then look to the single point tool but make sure it is has been made to the correct thread a 14-28 thread tool most times dose not have a sharp point on the end of it and again you loose some effect thread on the interal milling of it. I like a .002 radius max on tools when doing this small of a thread size when having to do milling or turning.

 

HTH

[Storkman]

Thanks for the info Ron, I knew we kept you around for somefin.