Expected roundness after parting off?

Having trouble with a "ring" shaped part, should have been really simple but is driving me up the wall. Material is a stainless of some sort, harder than I remember 303 being built not terrible to machine on tools, AMS spec of some flavor or another. Seems to be running at normal SFM's for stainless. Problem that I am having is maintaining any kind of roundness after parting off the ring. 2 1/4 OD, 1.590 ID, 1/2" long running on a barfed subspindle machine. Material is solid barstock. Process is rough turn the OD, drill the ID, finish bore the ID, part off/ subspindle transfer holding on the ID and finish turn the OD. I have +/- .0005 on the OD, and cannot hold the roundness within the upper and lower limits of the diameter tolerance. I can get anywhere from .0007-.0015 out of round on the OD. I believe that the part is round right up until I part it off the bar, confirmed by running an indicator on the turned diameters and getting less than a tenth indication. I don't think it is the subspindle turning op, same indicating and checking for the runout yields negligible indicator movement. Low chucking pressure, and the out of round condition on the diameter is measuring at 180 degrees, three jaw chuck I would expect it to be at 120? Seems like the material has some stresses in it that don't come out until the part is relieved from the bar. Tried different order of ops, like parting close to off and finish turning hoping for some stress relief. Less aggressive feedrates to no effect. Current theory (yet untested) is trying to drill the core with a smaller drill, thinking that the 1 1/2 drill may be putting more force close to the diameter that I am parting off at. I'd rather not add a third turning op, fairly high volume part. Anybody have a situation similar before that they would be willing to share their fix?

I had that happen ONCE.. It was 13-8... And it wasn't so much out of round (at least that I remember),
The ID shrank, and not consistently (could have been out of round)...

Either way, just had to part 'em off and skim the ID's as a last op. And it was
a shit load of 'em.

I also don't recall what we tried to get them to-size before part off, but it didn't work.

Not sure if I understand everything. Do you have a 3 jaw on each end, main and sub? If so what kind of jaws are you using? When working with rings just out of the fixed headstock chuck as I don't have a sub spindle I always used pie jaws on all operations, that combined with as low clamping pressure as possible seemed to help a lot toward making round parts. The more contact area you have with the surface the better.

Running 3 jaw chucks on both the main and sub. Main chuck is a 10" Kiti, standard issue soft jaws bored to the OD of the part. Working probably 1 1/2 from the end of the jaws, subspindle is a 6" Kiti using soft jaws of the pointed style, clamping on the ID. There is a small separation between the jaws when clamped, probably somewhere around 1/8" gap. I think they are what you could refer to as ID pie jaws. Low clamping pressure on the sub, as low as it can go. Another thing I had thought about trying was to reduce the contact on the ID of the sub, i.e. cut the jaws down to 3 smaller points of contact, seems like the clamping pressure on the subspindle side actually straightens the ring out to the out of round condition of the first op.

Dualkit said:

Not sure if I understand everything. Do you have a 3 jaw on each end, main and sub? If so what kind of jaws are you using? When working with rings just out of the fixed headstock chuck as I don't have a sub spindle I always used pie jaws on all operations, that combined with as low clamping pressure as possible seemed to help a lot toward making round parts. The more contact area you have with the surface the better.

Click to expand...

I had a job running thin wall(.093) bushings and found that if I cut off to within about a 1/16 wall before finish turn and bore it would help with the roundness.

Any chance you can post some pics? I have made parts a lot thinner with fine I.D. & O.D. threads out of 6061 aluminum that started with 3" O.D. tube with .250 thick walls. After lots of experimentation I got them to come out round. How many parts do you have to make? That will determine the best course of action. Can you post a rough sketch of one? Sounds like your sub spindle has been turned into an expanding mandrel. Pretty sure that will distort the parts unless the walls are pretty thick.

We've had lots of reports of variability of commodity-grade stainless steels for a while, the mills aren't paying as much effort to producing consistent bar anymore. If there's money in the project, getting a premium SS from Carpenter or the like could help you.

The other thing you can try is extending the "rough tube" prior to finish cuts, and make sure your parting tool is as free cutting as possible. For example, instead of rough turning only a little more than the 1/2" plus cut off width, rough and drill ~1.5" deep. Start your part operation, cut to ~.025" wall, then finish the OD, ID, and final part. The free-cutting parting tool puts less stress into the material before cut off, but may require more frequent changeout to keep the process stable.

Obviously, each fresh bar will require the deeper roughing and drilling, but from there it's just the incremental additional depth needed to get the final part lenght. You will start getting eccentric drilled holes if you don't maintain good concentricity of the tooling or if the machine and chuck are not in good shape. For the OD, a slower plunge in to the previously roughed diameter will take care of runout before the next incremental cut.

Thanks for the conversation on this, I'm pretty well stuck. I have tried parting off and leaving a thin wall before the finish turn, didn't help. Describing the subspindle jaws as an expanding mandrel would be pretty accurate. It was turned on size to the ID of the part. I'll make some sketches tomorrow, the wall is pretty thin. There are actually 2 diameters on the part, the major diameter is 2.100 and the smaller is 1.740, with the 1.590 thru that does get pretty thin. I did try relieving the jaws under the smaller diameter, didn't help either. I also tried drilling deeper than the part, I drilled 2 3/4 deep each time to no avail. The free cutting parting tool may have something, I am using a fairly aggressive parting tool. I tried reducing the feedrate on the parting tool, that didn't make a difference either.

Any reason you can finish turn the OD prior to your cutoff? It's amazing sometimes how easy it is to distort a part even in a well bored set of jaws and low chuck pressure. Any bar whip in your main spindle will kill you on OD roundness, but you probably know that already.

i go through this a lot since 95% of what we cut is SS and i have found that the 15 degree iscar partoff insert works great for it but there are some tradeoffs of course like it doesn't last as long as the 8 degree.
also like has already been posted, the SS isn't as good as it used to be unless you pay for it. you might try stress relieving a bar and see if that helps.

Material stress is a very common and normal thing and the biggest PITA with tight tolerance work. I have parts that go .002+ out of round, seen over .004". Some 625 material I use has insane stress and requires the right approach. I have a few ways to minimize it, roughing/drilling a long ways in(or right through) helps. Also have some straightening fixtures to bump certain parts back into roundness. Some stuff flat out needs stress relieving in an oven.

Other issues can be parts that expand/grow all around, and the rare one that shrinks.
Managing material stresses is one of the real fun voodoo things of metal working.

I'd swap my process around if you can, I'd try finishing the OD on the main, roughing the bore and do the finish bore on the sub where you can use pie jaws to put compressive rather than expanding stresses on the ring.

Tonytn36 said:

I'd swap my process around if you can, I'd try finishing the OD on the main, roughing the bore and do the finish bore on the sub where you can use pie jaws to put compressive rather than expanding stresses on the ring.

Click to expand...

Tony, it seems the OD is the critical one, and I'd expect he'd be worse off finishing the bore after final turning the OD.

why not parting off and than put in on a kaliber, try to sandwich the part so there is no clamping force radial but axial.

No idea what the print calls out for Roundness or Concentricity. But if it's just a diameter that you need to keep in tolerance, I would do exactly what you are doing and just leave more material on the OD. You say in the OP that you can verify that part-off operation is causing it to spring, but everything else is fine. If the ID is not super critical for Roundness or Concentricity to the OD, and the part springs at part-off, leave more stock on the OD for the second Op.

R

R

Reading this again, I'm suspecting the second op holding method as not being optimal, and it's contributing to the OOR of the OD. Lspotts38, can you post some pictures of the subspindle chuck and jaws, as well as one with the part on it pre-finish op? And are you sure there's no burrs or other aspects of the piece that could influence how the part is seating on the sub jaws?

Have you confirmed pressure and uniform jaw movement on the sub chuck? Master jaws or mating grooves aren't damaged, or have been crashed?

One thing to do also to help troubleshoot, mark the sub chuck. Before you unchuck the next part, mark it corresponding to the mark on the chuck. Run 3-5 parts and see if the ovality is staying clocked to the mark. This could indicate a clamping issue. You could have one master jaw worn slightly and you are actually clamping it oval under clamping load.

Second, Stop the process after the hand-off and chucking of the ring on the sub. Put an indicator on the part OD and see if the ovality is present before machining.

If the ovality is consistently clocked, Disclamp the bar from the main, roll it 30 degrees or therebouts, and re-run the cycle checking for the clocking of the oval. If it is in the bar, it should roll with the bar. If it is in the fixturing or process, it won't make any difference in where the ovality is clocked.

Good stuff here guys. Re Tony turning the part around, that was my initial setup and turning the OD's to finish size then finishing the ID, that was when I initially found the out of round. I have not tried that with the deep drilling idea yet, might be worth a shot. I would describe the out of round as an oval. No roundness specified, I just need to make the part between the upper and lower diameter limits. Re litlerob, I have confirmed that the diameters are round pre-partoff, but it seems that the subspindle clamping actually takes the ovality out of the part, like it straightens the part back to round, which doesn't do anything for me when the chuck is released and the part returns to its oval shape. Both of the chucks are in good shape, I am 95% confident that it hasn't been crashed, just put the machine in the summer of '16, and it hasn't been used much. I also like the checking the clocking of the out of round, that is not something that I have been tracking. I'll give that a look as well. The straightening idea is interesting too. Thanks everybody for the responses, I'll keep you updated.

If your sub jaws are cut to match the diameter of the bore, when they open to size the could be "re-rounding" the OOR bore, and so warping the OD. This might be a case where having three narrow contact jaws at just enough pressure to prevent slipping will do better for you. Light cuts to make sure you don't displace the part.

lspotts38 said:

Good stuff here guys. Re Tony turning the part around, that was my initial setup and turning the OD's to finish size then finishing the ID, that was when I initially found the out of round. I have not tried that with the deep drilling idea yet, might be worth a shot. I would describe the out of round as an oval. No roundness specified, I just need to make the part between the upper and lower diameter limits. Re litlerob, I have confirmed that the diameters are round pre-partoff, but it seems that the subspindle clamping actually takes the ovality out of the part, like it straightens the part back to round, which doesn't do anything for me when the chuck is released and the part returns to its oval shape.

Click to expand...

This is good information. It would be easy enough to verify, with an Indicator if the part is being forced back into round with the second chucking. Then my advise doesn't get you very far, huh? I think Tony's advice of verifying that the jaws are NOT/ARE causing issues is important. A picture would be worth Thousand words. Marking the parts and the Chuck's alignment is good to start to figure out how much out of round, where out of round, and shape of Roundness. Indicate everything and compare to after chucking, possible solution would be use of a Bung, or Slug for the ID.

Another thing is, 304 is a potato chip post Machining, where other SS's are much more stable. Because you haven't specified the grade of SS, I'm guessing the print doesn't specify, maybe just says "Stainless Steel", giving you some wiggle room.

OTOH I have built parts in the past that were specified 304L with 3.5" OD and .0625 wall----we just set up a flat plate and an Indicator on a Height gauge, and used a soft face Hammer to get them Round-ish. Sucked but it worked. Obviously different parts than yours, but.....?

One more thing, have you tried Milling the part off the bar, instead of Parting it off, to reduce cutting force?

R