Because of the large size, I’m using a three-jaw chuck to hold the raw material (round aluminum bar).
I’m currently trying to turn it in two operations: the first one turns down the smaller diameter and parts it off. Then I take the chuck off and hold the small end in a collet. Then I profile the rest of it, and bore the center (at least, that’s what I’m going to try to do tomorrow).
The problem is that to hold the raw material in the chuck for the first op, a lot of it goes to waste inside the chuck jaws. I have to make a few of these, so leave the bar as long as possible, which means a fair bit of unsupported stickout.
The facing and profiling go pretty well, but the parting seems to have a lot of issues. Chatter, and manages to move the stock in the chuck. I’m still trying to understand how the part I made above ended up pulling the stock in +Z by a couple of mm (as evidenced by the gap between it and the chuck face), even though the it parted reasonably accurately, and both parting faces are flat (although the chatter shows up).
I’m using a nice Sandvik parting tool and insert, and going in about 0.4 mm/rev at 200 m/min (up to the RPM limit, anyway).
And all this with undersize stock (50 mm round)! The full-size stock is even bigger.
So, does anyone have any advice for holding stock that’s too big for the 5C collets? The chuck is the only way, right?
And what can I do to improve my parting behavior? Lower feed? Is the tool too high or too low (it’s pretty much on the center)?
Lastly, can anyone recommend good feeds & speeds for these operations, including the boring and reaming, for 6061? I’ve been struggling to find good advice online.
I don’t have a ton of lathe experience so perhaps someone more seasoned will have a better idea but when using a chuck, you’re going to have waste. If you don’t want to cut up your bar into smaller lengths, your best option will be a steady rest on the table to counter the tool pressure, or a live/dead center on a tailstock to support the far end.
I think it is also worth investigating a thinner parting tool to help get better parting results.
FWIW. I have an 8L and usually work in brass and AL but have used this recipe for 303 SS as well. For parting I like to run the machine at 100SMF and 0.002" in/rev.
I’d never heard of step collets before. I’m struggling to find an example of their use, but I’ve gathered that you machine out a bore in them appropriate for the size of stock you want to hold. That would work well, I think, if I had to make more than half a dozen of these. Although I guess I could use it for anything I make out of that raw stock size.
Yeah, I have a couple of Tormach parting tools. Perhaps I should go back to using one of those.
It occurs to me that I can probably start with a much smaller piece of raw stock, cut on the chop saw, and clamp it near the front of the chuck. Then machine the small diameter portion and front wall, and instead of parting it off, just do op two on the whole thing. That would let me skip the entire parting operation.
I’m not having any luck finding a video showing how one actually uses a step collet. I think that would be an excellent video for Tormach to make
I found some very inexpensive step collets from Shars, but they don’t appear to have the pins in the gaps to help with the initial setup prior to machining. Do you have advice on how one might use these? Clamp it down closed and machine a smaller-than-nominal bore? Put shims in the slots?
So the small end is going back in the chuck?
Or in a collet?
At any rate, I would cut my stock with 0.030 to .060" extra at each end. You only need to hold on to about 5/8". Measure stick out and repeat. Touch off on the face, Z zero, move Z-.060 and RE zero. Machine a finished diam with another perpendicular face. OP 1 done.
Rinse and repeat.
OP2
Flip and clean up the other face. Measure and set the distance for the next zero using the chuck jaws or the part in the collet. Turn remaining material.
Check alignment before turning if critical.
Remember you have excess material all around so OP1 stock doesn’t have to be perfectly aligned. OP2 alignment is much more important.
I part at 600rpm and .0012 to .0015" per rev on a 15L. The PP settings are too aggressive for me.
Full disclosure: I haven’t used a step collet before. I talk to machinists on a regular basis that use them, however. All versions I have seen have pins in them and are treated much the same as an Emergency collet (turn out the geometry you want then knock the pins out)
The pins are only there to keep the collet from collapsing during the initial machining. If they’re not included, you can use drill rod, shims, or whatever else you have kicking around to stand in for them.
I wouldn’t clamp the collet down on nothing and machine it because you’ll end up with a bit of an outward taper on the bore walls when the collet is released. Might not amount to anything but it could reduce your grip on the part depending on how big the slots in the collet are.
This does often happen to me, if you can do this, calculate what you need to make two parts and a bit more so you can hold the second part in the chuck
Step collets require a cage to have any real clamping power. The cage screws onto the nose of the collet closer. You can see both in the eBay listing attached. You would have to make a custom threaded insert for your spindle or purchase a collet chuck that is threaded.
