Turning a thin walled part- ID or OD first?

Question Boy · Feb 19, 2006

I have to turn an aluminum part (6061 or 7075)with a 1.41" OD, and 1.29" ID (.060 wall). The depth of the bore is 1.48". I'll be starting with 1.5" dia. stock.

Should I do the boring first, or the outside turning first? Does it matter?

I think I should save the machining that requires (creates?) the smallest cutting forces for last, but I'd like an experts advice.

Thanks,

Patrick

morsetaper2 · Feb 19, 2006

Which diameter is the most critical fit? The OD or the ID? Which has the tighter tolerance? Those are some things to consider.

Motomoron · Feb 19, 2006

Every time I've made a tube from a piece of bar stock I've wondered after the fact why I didn't just start with tube.

That said, I usually cut the OD fairly close, hog out the inside, finish the bore, and make the final pass for the OD last, just in case any internal stress in the bar relieved by the boring resulted in the OD changing, however minimally.

I'd probably cut the more critical dimension last in any event.

Motomoron · Feb 19, 2006

Hahaha.

2 guys 15 miles apart answering the same question at the same time.

Question Boy · Feb 19, 2006

The ID is more critical, but it's an easy ±.003.

I would start with a tube, but the part has a flat bottom- like a small paint can.

FranH · Feb 19, 2006

Finish the ID first. Make a plug with .0005 clearance and threaded so a screw can pull it out after. The plug will keep the OD from crushing. OR bore the ID to max..turn the OD and check for the amount the ID was crushed. The next piece bore to finish plus the amount crushed...turn the OD at same speed and feed as the first time.

The latter worked for me when special threading a 32 pitch ID and OD on the same end of the part...aluminum and .032 diameter difference from ID major dia and OD minor dia ... both class 3 threads.

matt_isserstedt · Feb 19, 2006

Interesting question. If you can set this up so both surfaces are accessible just with a tool change from OD turning tool to a boring bar, you can get close from both ends.

As you say, I'd stick with light cuts there at the end. I'd also go with HSS to cut down on the tool point pressure.

I made a .050" D-bit reamer recently...not the same job, but a thin flexy piece...about 1/4" long, it turned out quite well, just took lots of light cuts as I got down there.

-Matt

jim rozen · Feb 19, 2006

That's still a pretty thick wall, you won't have
trouble with the OD crushing. The problem
will be that the thing will ring like a bell
when you turn the last surface.

The plug will help for that, or use some clay
or sheet lead to deaden it.

Another approach would be to turn both the
OD and ID in the same setup, that's how they'd
do it with a turret lathe.

Jim

Gary E · Feb 19, 2006

Can you bore and turn the ID and the OD then cut it off?

I did that on a very thin walled heat treated alloy steel part that also had class 3 threads inside. I then made a threaded plug to hold the part to finish the cut off end.

gbent · Feb 19, 2006

For multiple parts, or if things don't work any other way, make pie (full contact) soft jaws. Finish the outside first, then chuck with full contact jaws.

wesg · Feb 19, 2006

One setup. Bore the ID. Wad up a paper towel and stuff it inside to cut the chatter. Turn the OD. If it still wants to sing, don't sneak up on it, make the final pass 20 or 30 deep with a relatively sharp pointed tool. That gives you a more rigid part to cut.

I've done .040 wall 1" OD pieces 3" long like this. No problem at all.

TheMetalDoctor · Feb 20, 2006

Pat,

You got me. If you start with a tube before machining how can it have a flat bottom? I can see where you might have a step in the bottom, but not a flat bottom as there is no bottom in a tube.

Either way, finish the o.d. last. If you are chucking up on a tube, put in a close fitting plug to chuck on so you don't distort the wall. Finish the i.d., then o.d. I don't think you will have any problem with dimensions that you have given. If it starts singing, slow it down and take lighter cuts. Any mass added inside the bore when you go to finish will help, but with .06 wall I don't think you will have any problem.

TMD

jim rozen · Feb 20, 2006

Hmm. Another take on it: Bore the ID first
and use a mandrel to hold it for the OD turn.

You will have to rig the mandrel to be expanding
somehow, you could slit it and use a pusher
screw near the chuck to expand it out.

Jim

winchman · Feb 20, 2006

"Make a plug with .0005 clearance and threaded so a screw can pull it out after."

A good idea, but be sure to make it from something other than aluminum if you want to get it out. You should also put oil or grease on the plug, but you'll need a path for air to get out/in as the plug is installed/removed.

Roger

HuFlungDung · Feb 20, 2006

There is such a thing as expanding 5C mandrels that will work within a blind hole. They use a taper head screw to expand the body, said screw is pulled back by the threaded end of the collet. The threaded end of the collet is actually a seperate piece from the rest of the collet. So as the drawtube is actuated, this pulls the taper head back into the mandrel, expanding it. Works quite well.

You can get these in sets of 4 from Shars Tool for about 50 bucks.

spope14 · Feb 20, 2006

Hu got it right. I use these things all the time. Go with it.

jim rozen · Feb 20, 2006

Internal expanding 5C collets work great,
I use them all the time. They are a bit
limited on length though, so if used for this
deep hole application they will have to be
turned very carefully and the part seated
on likewise.

Jim

SND · Feb 20, 2006

Here's how I went about doing a little job last week. It was a 316 stainless sleeve.

ID was 4.110" OD was 4.150. ( .020"wall). 6.25"long.

I roughed the inside of the pipe to 4.05" then roughed the outside to 4.300( started with a 4.5" od, 3.8" ID)

Next step I took some tick rubber strips and wraped them fairly tight on the OD of the piece with some tape. I finished the inside with a solid carbide bar.

Then I took the rubber strips off and carefully stuffed them inside the sleeve and put the pipe center in. ( Wet rags work pretty good too )

Pretty simple really, just takes a bit of time.

In your case you don't need to put a pipe center.

One thing to check is your tolerances. It often dictates what gets cut first and last.

If you have a very tight ID tolerance. Rough ID, Finish OD, Finish ID.
IF you have a very tight OD tolerance. Rough and finish ID, then finish OD since you have very little material to take off the OD anyway.

Question Boy · Feb 21, 2006

Thanks guys, I appreciate the suggestions. The boring bar arrived today, and I'll program the machine tonight. Probably give it a whirl tomorrow.

Patrick

Ox · Feb 21, 2006

Just put it on your twin turret machine and cut both at the same time.

Actually - I think you have enough wall that it shouldn't be much of an issue. ???

Think Snow Eh!
Ox

Turning a thin walled part- ID or OD first?

Stainless

Diamond

Stainless

Stainless

Stainless

Hot Rolled

Diamond

Diamond

Diamond

Diamond

Titanium

Titanium

Diamond

Stainless

Diamond

Stainless

Diamond

Diamond

Stainless

Diamond

Similar threads