I have a part to make where the O.D. runs out from the I.D. by .056. In other words, the I.d. will be machined first, and then I need to fixture it so the I.D. is running out by .056, and then I can turn the O.d. Part is going to have a .500 - .503 I.D., and will be 1.9 inches in length. Really not a hard part at all, just need some good ideas.

Mount in 4-jaw, machine the ID.
Get some dial indicators and move the part .056" off center in the chuck, then turn OD.

Or drill the hole, then mount it on an expanding collet in the mill and mill circles around the outside.

Ok, dopey me left out an important piece of information. This part I have to make will be a 500 piece order. Sorry. Needs to be fast loading and unloading.

I'll take my dope slap to go please.

Mount expanding collet in collet block, and mill the offset on the collet, or, put in 4-jaw, and turn the offset.

RAS

I do some larger parts by turning an ATS expanding mandrel off-center, but due to your small id size and long length this might not work, is there any way you can turn the od first then holding off-center in the collet/pads?

Ras,

I don't have a 4 jaw for my cnc lathe, and it would be expensive to buy one for this job, as I'm not sure this job will repeat. It could be one time only.

dcrace,
I guess I should describe a little more of the part. There is an O.d. and an I.D that run true to each other, and then there will be 2 flanges on the ends that need to run out from the rest of the part. So, there really is nothing left to chuck on with the O.D.
I already thought of using an expanding collet from Mitee-bite. I will machine it down for the .5015 grip, and then mount it off center by .056, and then I can turn the O.D.

I'm still open to other ideas though, just in case there's something I haven't thought of yet.

Appreciate the help so far.

Dave:

Is the runout the radial offset or is it TIR? Needs to be defined. What accuracies are required.

Turn the concentric stuff, then circular mill the offset items.

Run on a lathe that can do eccentric turning.

If the part is steel use a cam grinder to create the eccentric elements.

.

I've posted these parts a few times. Everthing here is offset including the axis of the ball on the threaded stud.

Does not have to cost much. Bore a 5c extended reach collet, and make inserts to fit the bore. (the collet bore is on center, the inserts are bored in a mill to whatever offset is needed).

I usually bore the inserts by mounting the collet set up in a hardinge dividing head, because everthing fits just like on the lathe. Close the collet, bore the insert, then remove it and saw the compression slots on a band saw.

But any method that keeps the bore axial (parallel to the long axis) will work. This one is 1-3/4" bore due to the fact that I had a bar of that size aluminum to chop off whenever a new insert is needed. If you are going to run 500 parts, it would be worth starting with steel. Aluminum does wear and ther edges round a bit over time.



smt

smt

The runout is radial offset. Accuracies are only plus or minus .005.

If I run the eccentric on a mill, I will need to do both sides individually since they are on opposite ends of the part. That would mean two times of chucking. On a lathe, I can chuck only one time and turn both ends. I don't have a lathe that does eccentric turning. Needs to be fast. There are 500 pcs to do.

Stephen,

Sounds interesting, but I can't see the pics. Is it just me or did something go wrong?


EDIT: Nevermind, it just opened up.

I'm still a little vague on this part. Are you going to finish the id complete, then do the od to the offset finished id?

You can mount them on a mandrel with offset centers. Put a dog on the mandrel and run them between centers. For faster cycle times, make two mandrels.

I will do the O.D. and I.D. together. Then I want to I.D. chuck offcenter, and turn the two ends.

What would drive the part? If the dog drives the mandrel, what's stopping the part from spinning on the mandrel?

Heres a shaft i turned



bolted the 4 jaw to the mill...dialed it in and zeroed the axises over center..cranked X over 1.500 (1 thou tol on offset and runout), tossed the 3 jaw on and kept adjusting the 4 jaw till the 3jaw was zeroed....clamped, bolted, bolted on counter weight...mounted on lathe, dialed rough part in (machined it in 3 peices, then pressed the shafts into the plate and welded)

part came out perfect (3 0.0005 dia on one side and a 0.001 tol dia on the other)

Dave - due to the qty i would either make an offset mandrel with a drill tapped end and use a bolt to nip the part in place or

make an offset split bush to locate on the centre dia. - hold this in bored jaws on cnc turn end 1 turn comp. around turn end 2

Smudge

This part can be made on a cnc lathe with driven tooling in one hit.Probably make more profit and certainly less hassle subbing it out.Even easier on a swiss if you can find someone who can be bothered setting up for 500 pieces.

Smudger,

Yeah, that's kinda the ideas I had in mind, but I posted this in hopes that someone would have some magical idea for it.

Mark,

I don't have a lathe with driven tooling. Subbing it out would defeat the purpose of taking the job in the first place.

If you are holding on the OD, use an Emergency 5C collet and machine the bore .056 off center.
If you are holding on the ID, do the same thing with an expanding mandrel
I do this all the time. Then I can run them in my turning center just like any other part.

I'm going to use the expanding mandrel offcenter. That way the only thing I need to cut while off center, is the 2 ends. I think it's the best I'm going to get.

Thanks to everyone for the ideas. Still open for that magic wand type idea.