What's new
What's new

Machining Thin Wall

jephw

Aluminum
Joined
Jul 23, 2020
Good day everyone.
I need some advice on this particular job - see picture attached. The material is SS 316L. The part has a taper at the very end, resulting in a thin wall when finishing the OD. Best practice ensure concentricity after the OD and ID are complete?

The customer mentioned that the company that ran this job in the past had to use a plug when machining the OD because of the thin wall. Is this necessary or can this be avoided with proper feeds/speeds and using inserts that are sharp/positive and shallow DOC. What are your thoughts on this?
Screenshot (4).png
 
Hi jephw:
I doubt you can make this work to those tolerances without the plug...316 is pretty ductile and will fold in a bit when you turn the OD, even with a positive rake dead sharp tool with a truly tiny tip radius.
With a custom ground positive rake tool that has a 0.002" or so tip rad you might get away with it, but I am pretty sure you'll be disappointed with any typical insert tooling.
Also if you do try this, I'd turn the ID finished and then turn the OD in short steps to stabilize the developing shape as much as possible with the un-turned stock until you've turned a fair ways down the length.
Another way you can try is to turn a taper on the OD too, and then just keep reducing the OD taper with successive cuts until your final pass is cylindrical.

Does your lathe have a tailstock you can run a plug in with and hold it in position?
Can you dial down the tailstock pressure and still run the machine?
How many do you have to make?

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Last edited:
Hi jephw:
I doubt you can make this work to those tolerances without the plug...316 is pretty ductile and will fold in a bit when you turn the OD, even with a positive rake dead sharp tool with a truly tiny tip radius.
With a custom ground positive rake tool that has a 0.002" or so tip rad you might get away with it, but I am pretty sure you'll be disappointed with any typical insert tooling.
Also if you do try this, I'd turn the ID finished and then turn the OD in short steps to stabilize the developing shape as much as possible with the un-turned stock until you've turned a fair ways down the length.
Another way you can try is to turn a taper on the OD too, and then just keep reducing the OD taper with successive cuts until your final pass is cylindrical.

Does your lathe have a tailstock you can run a plug in with and hold it in position?
Can you dial down the tailstock pressure and still run the machine?
How many do you have to make?

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
I have a programmable tailstock and I will try and use it to insert the plug.
I have a few hundred of them to make.
Would you reccomend making the plug out of a plastic like UHMW? I will try some of your ideas if I can't make it work a plug will be the next option, thanks for your help.
 
Actually, another option - totally opposite of "sneaking up on it", is to take the OD all in one go.
Just feed less - make razor wire.
The wall thickness ahead of the cut will help to stabilize.


------------------

Think Snow Eh!
Ox
 
Hi again jephw:
I'd say if you're going to go to the trouble of making and using the plug, you will have better success with it if it's metal...at least aluminum and for preference, steel.
Remember, you want to keep the stainless tube from collapsing under the force of turning, and if you use a soft material I'm not certain it will prevent that deflection.

The problem with the tailstock is that on some makes and models of turning center, you need a minimum tailstock pressure to allow the program to run...I'd find that out before investing in making the plug.
If it turns out you can't use the tailstock, you have to use a piece of threaded rod through the tube with some kind of cap at the headstock end and your plug snugged up with a hex nut at the tailstock end.
If you have to do that for several hundred parts you will grow to hate the job because you'll be tied to it, forever screwing around with that stupid plug.

If it was me, I'd first try the custom ground turning tool.
If you can find a triangular or rhomboid insert with a super small nose radius and if you have a grinder with a 150 grit or finer diamond wheel, you can put some top rake on the insert and make it dead sharp at the same time.
Next step is to bore the cone with your normal boring bar.

Last step is to turn an OD taper say 10 degrees or so and get the tip of it dead nuts on size.
Then take another pass making an 8 degree taper, then on down until your OD is cylindrical.
You don't take anything further off the tip after the first pass.
With a 4 degree internal cone, the part wall is still awfully skinny, but with a really sharp tool you just might get away with it if you baby the cuts.

You can also try to take it all in one big pass after your first OD taper cut, using a super slow feed (like 0.0005" per rev) and not trying to break the chip.
You want the chip to come off like unrolling toilet paper...violating every rule you ever learned about speeds and feeds.
If the tip radius is small enough and if the tool has positive rake and is fed slowly enough you can take an enormous cut with it before it starts to chatter, and with a tiny tip radius the forces going radially into the part stay minimal so with luck the tube doesn't collapse.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Last edited:








 
Back
Top