Turning very small parts -tips?

[SRT Mike]

I have a gigantic lathe - an Okuma LC40 that can turn something like 24" parts. It has a max spindle speed of 3000rpm... that's all I have to work with. Bearing that in mind....

I have some very small parts to make... they are button caps for a switch. It looks basically like a tiny nail with a shaft and a larger diameter head where the head is flat. The thing is that the head is 5mm diameter and the shaft is 3mm, and the total length is 3.5mm. I am open on the material - probably 6061 aluminum but I could also use something like 303 stainless, it's my call there (AL is better because some may get anodized).

I can turn the parts OK, thats not a problem. The three things I am concerned about is

1) I only have 3000rpm's to work with - is that going to be a problem?

2) What would be the best way to hold the stock prior to cutting? I have a hydraulic 3-jaw chuck. I've seen adapters that go in the 3-jaw and allow the use of 5C collets. I figured that would be the best way to hold the part of this size for turning

3) I only need to machine from one side, but the front end of the shaft (the small end) will have a chamfer on the front and the back (the head of the nail, so to speak) must be nice and flat since this is what actuates the switch below it and it must be to tolerance. But whenever I part off I always get a little "teat" on the piece that falls off. I've heard of people using parting tools with an angle on them so that it cuts through at the part before it cuts through at the stock. Are they custom ground tools? My parting tool is 0.120" wide - thats actually quite a lot of material to take off for such a small part... are there special narrow parting tools out there with the slant angle? Or is there another/better way to get a nice finish on the part besides what I just described?

[Verfur]

turning the shaft, look into hollow mills maybe even customize it for the head as well
one plunge in Z and part off with a oh say .06 inch wide L or R insert and even then it will most likly leave a pip just back way off on the feed as it gets real close. on the jaws a 5c collet would be nice but even a set of master jaws (pad system for 3jaw chucks)
hope you dont have to make tons of them.

This is a perfect second op lathe part

[little bubba]

Easy, even with a giant lathe, providing you can get the chuck pressure down low enough.

You can hold the tiniest stock in the biggest 3 jaw CNC chucks. Its not difficult, the smallest I have held was .093"(2.4mm??) stock in an 8" chuck.

Set the jaws for internal clamping, get them as close as you can, then run an endmill as a boring bar to cut the jaws, it only needs to be mildly bigger or on size of what your stock size, since it will cut on all flutes. Step over if you need it larger, just make sure that the flutes of the endmill are set in line with the X axis.

Flip over to external clamping, and now you have a GIANT chuck that can hold tiny little parts, even on a bar feed.

For your particular part, which really isn't that small, I would flip it, since the top side of the head needs to be flat, and is the critical part. Face it, then use a groove tool to get the shank size and part off, done.

[Verfur]

Like bubba said bored jaws will work. I asume you are worried about the stock falling out between the chuck jaws at least thats bin may dismay with the small stock VRS. Big three jaw chuck. The only way is if you can limit the travel distance on the chuck for open or orientate the spindle with one jaw strait down for the stock to sit on and I hope you are using a bar puller and not a bar feeder.

And do I need to say watch the rest of the tools for clearance on the chuck and Jaws.

If you are going from the head end check Micro 100 for a ID groove tool to turn and part off the whole part.

P.S. bring a deck of cards for somthing to do while in cycle

[HapSmo19]

You dont need to buy or make any adapters(with a simple exception) to run a 5C set up with soft jaws.

Screw the collet block nut tight onto the collet and measure the Z distance from the largest diameter on the tapered end of the collet to the front face(the side facing the tapered end of the collet) of the nut.

If the depth of your jaws is less than this distance, you'll need to turn a ring-spacer(simple exception) to go between the nut and the taper to make up this difference. Aluminum will work and a diameter larger than the nut is a good idea.

If the depth of your jaws is greater, you'll need to mill down the backside of the jaws to the same Z measurement with a theoretical diameter large enough to allow clearance for the collet nut.

Boring the jaws:

I make a large, thin aluminum disk that fits behind the jaws and allows minimal actuation of the chuck when clamped. This is imortant if your picky and want to keep the collet from flopping around when it's unclamped.

Set chucking pressure to 6psi and bore the collet profile. Cut the area between the taper and the nut oversize. I believe the dimension is 1.250 but it should be bored through between 1.260 and 1.270. The idea here is, when clamped on the collet, you locate on the collet taper and the front face of the collet nut. Not the middle(shank) area. This way, closing the jaws PULLS the collet closed.

Anyway, mark your jaws and remove one to get the collet and nut/spacer in there. Run chucking pressure at 6-8psi and the slits in the collet between the jaws. Don't clamp with nothing in the collet. You just saved youself at least $400.00.

I've never had any problem repeating to within .0002 with this set-up.

Good luck.