length to chuck on lathe part

I need to run some parts that are bigger and heavier than the usual size in our shop and need some advice. Parts will be made from Ø9" by 10.5" long 6061 aluminum. Parts will be grooved in the middle to Ø5" leaving the ends a bigger diameter and will be bored to about Ø3.0". While doing any turning i will probably use a tailstock for support. But for facing, drilling and boring im worried about part coming out of chuck. These will be run on hitachi seiki cnc lathe with a Ø10" chuck. What kind of jaw length do i need to feel safe? Should i buy long aluminum jaws i can bore out to at least 2" or maybe 3" deep for chucking? My hardened jaws only have about 1/2" gripping length on them. Our normal work size is like Ø5" x 5" long parts. We do bigger diameter stuff sometimes like Ø9" but always under 5" long. Any advice would be appreciated. Thanks.

Getsideways said:

I need to run some parts that are bigger and heavier than the usual size in our shop and need some advice. Parts will be made from Ø9" by 10.5" long 6061 aluminum. Parts will be grooved in the middle to Ø5" leaving the ends a bigger diameter and will be bored to about Ø3.0". While doing any turning i will probably use a tailstock for support. But for facing, drilling and boring im worried about part coming out of chuck. These will be run on hitachi seiki cnc lathe with a Ø10" chuck. What kind of jaw length do i need to feel safe? Should i buy long aluminum jaws i can bore out to at least 2" or maybe 3" deep for chucking? My hardened jaws only have about 1/2" gripping length on them. Our normal work size is like Ø5" x 5" long parts. We do bigger diameter stuff sometimes like Ø9" but always under 5" long. Any advice would be appreciated. Thanks.

Click to expand...

CNC brings limitations as well as advantages, so this might not be useful, but..

An "all manual lathe" guy might "batch process" as follows:

First op: Put a clearance bore 10.5" through on a(ny) decent drillpress,

Second op: IF, and ONLY IF, your Drillpress can't deliver with a decent reamer, Lay the now "tube" on a raised & shimmed vee-block PAIR atop the lathe carriage (presuming no hor-bore), and ream or line bore it to finished ID.

Drillpress OR lathe, the work don't motate. Boring bar or bespoke "D" reamer does. "D" reamers are cheap and cheerful. Accurate, too.

Third op: Using that finished bore, mount it on an internal (tapered sleeve) expanding mandrel 'tween centers, so as to face both ends and turn the OD & reduced center in one final setup, and with "rather good" concentricity to the bore. "Automagically" good, even. Not a lot of set-up time to it if your mandrels are decent goods.

Or you MAKE a good 'un.

Nuisance work, three-stepping it, but near-zero risk of it getting away and ruining a part.

Or ruining your whole day.

Steady rests exist, too. For all-manual lathes, anyway. You might not have one?
Mandrels can he had faster and cheaper than steady OR tall jaws, work better, can be DIY'ed faster and cheaper if need be, too.

CNC is at its best with custom workholding engineered to the specific work at hand ....and even "live" tooling.

Odds and sods that do not fit your on-hand workholding and tooling can be a Royal Pain in the Computerized Numerical Control arse.

You knew that already, yah?

Trying to EXTEND sub-optimal workholding with nought but taller jaws?
Fraught with risk. You knew that also.

It CAN work.

Mandrels will work. Least-risk.

Not new.

2CW

And of COURSE I have the mandrels.

Breakheart Tool single-enders as well.

Preparation is 90% of any job.

Preparation to do each job CHEAPLY, too!

Might consider machining a circular dovetail on the end of the part, and bore a set of soft jaws to match. If necessary, buy the stock with enough extra length to do this if you have to sacrifice the end of the bar for the sake of chucking it. I'd cut the angled surface on the stock by means of the manual lathe, but you can probably do it with great care on the cnc as well.

Some guys might use carbide grippers (with the diamond knurl pattern) mounted in a set of soft jaws. With a power chuck, you can set those in pretty good into the stock.

Crazy good manual guy at work had a similar issue. If I remember correctly he center drilled with the part bearly in the chuck, put tail stock in and faced as far as he could, then drilled and bored it, put a plug in and back in with tail stock. I walked up to it as he was boring and said holy shit aren’t you afraid it’s going to come out and he said most of the cutting force is into the chuck. Good point, but scary none the less.
I wouldn’t cut the od or face without support

Do the hard jaws have teeth or are they smooth? If they have good teeth on them you should be just fine with 1/2" in the chuck as long as the bottom (face) of the part is seated square against every jaw and you are chucked tight enough. If necessary, start the job by facing, then turning a 3/4" length diameter to grip on, then turn the job around. I do this all the time when I only have a little to grab on. That way you'll be gripping on a nice round diameter with the face squarely seated against the jaws when you start doing the heavier cutting. If your machine isn't rigid enough and you get chatter you'll need to devise a method to use a center for some extra support. Either a bell center or a plug as mentioned earlier would be good.

When cutting at the larger diameter I'd take it easy on the feed just to be safe. Stick to maybe 1/8" DOC max and maybe .010" feed and adjust from there if it does good. You could also make a flat disc that's larger than your bore with a center in it and just push it against the face with the tailstock center when you're doing the OD work if you're nervous about it. I keep a couple different sizes of these near the lathes just for such use, they can be handy.

G50 is your friend. Buy some soft jaws and not worry.

Dave