Advice On 4-40 External Thread

[recordist]

I'm looking for a bit of advice on cutting a thread:

Material is 6061 Alum. We have a 3" X 4" X 1/2" deep pocket machined out, leaving several posts/islands about .135 dia X .38 long. These posts are to be O.D. threaded 4-40 X .3 deep.

Is a thread mill the best way to go about this? I worry about the posts breaking off as soon as the tool touches them...

I was thinking of possibly leaving the post oversize, cut the top 1/3, thread mill that 1/3, then continue with the 2nd 1/3, then the final 1/3 (shorter sections of posts should be more stable and sturdy, yes?).

Or is there another type of tool, like a die, that could spin the threads on the posts? Like rigid tapping, but with an O.D. tool? This would give constant overall pressure and the posts would be less likely to break...

If the 6061 is much more sturdy than I'm thinking in my head, and a thread mill is probably the best way to go, might it be best to step it in? Run the cut with an extra .005, then again with an extra .002, then to final size?

THANKS for any advice!

[recordist]

Maybe a single-point thread mill to reduce tool pressure, rather than a full-contact insert with 5 or 6 teeth?

Anybody making small diameter O.D. threads have a few tips to share?

Thanks in advance!

[Gary55Ford]

What are the posts used for? And how long do you think they will last being aluminum.
Could you posibly drill&tap the pocket and use 4-40 studs?

[ctate2000]

If you have a good machine and take multiple passes it should be possible. Machine drift and tool runout will be the two factors which will give you the most problems. I like the drill, tap and stud idea if possible. This will allow you to replace stripped threads. Finding al studs that size may prove dufficult.

[Andre' B]

You could do it in stages.
Leave the posts say 1/4" diameter.

    _
   | |  Mill and thread this part.
  /   
  |   |
__|___|__

    _
   | |
   | |  Mill and thread this part.
  /   
__|___|__

    _
   | |
   | |
   | |  Mill and thread this part.
__/_____

Edit: You will just have to pretend there is a backslash on the right side, bloody BBS keep removing them.

It is a common practice when thin wall milling, should work fine for threading small posts.

[recordist]

From my original post:
"I was thinking of possibly leaving the post oversize, cut the top 1/3, thread mill that 1/3, then continue with the 2nd 1/3, then the final 1/3 (shorter sections of posts should be more stable and sturdy, yes?)." - Andre B used a bit of graphics to illustrate what I meant, I probably didn't state it as clearly - but that does seem a pretty good way to go...

Others have suggested 4-40 studs - that would be a nice solution, but the customer needs this out of a single piece of aluminum...nothing is ever easy, is it?

I still haven't found any tools like I was thinking of (like a high-speed precision die, to spin the threads on the post)...is there any such thing? Something similar that might work without too much modification?

Thanks!

[scadvice]

...on a test piece first. Unless I read what you wrote to fast...you did not say you had tried it yet. I think you can do it.
I've cut them to that depth in the same material, but I think they may have been 6-32's. I cut 50 or 60 post without a loss. I'll check in the morning to be sure on the size. If they are 4-40 thread, I'll post a picture. I used a 3/16 diameter carbide single point type with three cutting points like a "T" slot cutter. You can find them in the MSC catalog.
One other suggestion... use a endmill with a small radius on the corner when you mill the post so they will not break off so easy at the base when you thread mill or screw a part on them.
If they do break, then your stepping idea may be the way to go, but I would thread mill right over the steps (thread mill top down) and then clean up after with a very small endmill to min. side forces. Then lightly use a very soft ss wire brush on a dremel to clean up if needed.
Steve

[scadvice]

: ...and they are 4-40!! However they are .210 long, not .300. I wouldn't think you will have any problem doing them that long and there is a cutter available.
You can get the tool from MSC and it is just under .100 in diameter and made by Scientific Cutting Tools Inc. PN SPTM098L and the MSC catalog # is 40232837.
I'm getting a picture of a part and the single point thread mill for you and will send it later today.
Steve

[scadvice]

Hope it helps..
Steve

[beege]

What about acorn dies? or perhaps this link will help?

http://www.nationaldistribution.com/geometric.htm

[recordist]

A couple of very helpful suggestions - THANKS!

Especially nice getting a photo of a part and tool, Steve!

At least now I don't feel like this is so crazy. Still not the easiest thing, but not crazy.

I really appreciate the help, will try to reciprocate on this board - knowledge is nothing unless it is shared.