lathe / swiss screw tool radius? Stainless 316

Hi all!
I am designing a small shaft that needs a little flange. there's a lot happening in a small place, so i want to model the tool radius instead of a sharp corner.

shaft is ~.1" diam, stainless 316.
this will be a production part (100/year). I suspect made on a screw machine.

What is a reasonable (minimal) corner radius? I am hoping you will say .003"...

cheers!
ssr

subsearobot said:

Hi all!
I am designing a small shaft that needs a little flange. there's a lot happening in a small place, so i want to model the tool radius instead of a sharp corner.

shaft is ~.1 diam, stainless 316.
this will be a production part (100/year). I suspect made on a screw machine.

What is a reasonable (minimal) corner radius? I am hoping you will say .003"...

cheers!
ssr

Click to expand...

so, you say swiss screw, so is that diameter .1 mm or inch?
I assume inch since your radius is in inch, but it's not clear..

next you don't define what is going on, the amount of stress... you add a radius to kill off the stress riser, and also to handle any other torque that needs to be relieved.

I won't have the answer since my engineering background is from the 70s and I didn't finish it and never put it to use.

shaft is ~.1 inch diam.
also worth noting- I am not looking for design advice, but for DFM advice.

Speaking as a Dumb F'ing Machinist: sure, do whatever you want.

Speaking as a mechanical designer (but not an engineer): RPM, shaft and flange lengths, mechanical supports and stress on those, attachment methods, torsional stress, balance and resonant frequency issues, blah blah would be good to know.

But yeah. A .003" radius is good. Perfect, in fact. Better than whatever Brunel would have come up with, that's for sure...

For the record your typical insert tool corner radius is .008 and up on front turn, back turn and groove inserts. Try to design the part around that. Of course smaller radiused tools are available but in a smaller selection.

Dualkit said:

For the record your typical insert tool corner radius is .008 and up on front turn, back turn and groove inserts. Try to design the part around that. Of course smaller radiused tools are available but in a smaller selection.

Click to expand...

awesome. typical insert tool corner radius is really the question that i was trying to ask. I'll start there, and soon learn that i need a custom tool...

subsearobot said:

awesome. typical insert tool corner radius is really the question that i was trying to ask. I'll start there, and soon learn that i need a custom tool...

Click to expand...

For the record, typically the smaller the radius, the less tool life, and 316 is typically hard on tools, and the smaller the diameter the more of a PITA it is to work with materials that aren't friendly. At that .1 diameter I believe as you mentioned it is a Swiss screw machine job.

.004” isn’t too hard to find either, but again huge trade off with insert life. Is cutting a shallow and narrow groove below the shoulder an option?

Nerdlinger said:

.004” isn’t too hard to find either, but again huge trade off with insert life. Is cutting a shallow and narrow groove below the shoulder an option?

Click to expand...

I have used front turning inserts with a .001 corner radius for a medical device company that wants sharp fillets, even on 303 they don't seem to last very long, even crawling on SFM.

Dualkit said:

I have used front turning inserts with a .001 corner radius for a medical device company that wants sharp fillets, even on 303 they don't seem to last very long, even crawling on SFM.

Click to expand...

They think physics don't be like it is, but it do.

I can get inserts down to .001" radius. I don't like using them. .003" and .004" are fairly common, but they're going to add to manufacturing cost because they'll still have poor tool life. .008" is the absolute minimum I like to program with, and even better if it can be .010" or .015" so I can program a radius move to generate the radius, instead of just ramming the insert into a corner...

Anything below a .006 true radius on carbide is a problem and cost to make should go way up.
Rads down in the thou or three are often put on by hand and if checked under 350x mag don't really look like a radius and the clearance will not be right so tool life is all over the place.
Seen so much lying in this, but the customer has 30X so won't know or worse yet the maker is at 32x. User just thinks it wore out fast. Like Doritos, eat em up, we will make more.
An upsharp carbide tool corner lathe or mill will be cutting a .001/.002 corner very quickly in use in metals.

How do you intend to check this finished part radius?
Can this corner be undercut slightly to prevent interference with mating part and allow a bigger rad or tool corner breakdown?
This is how toolholder pockets are often made so as not touch the sharp and unused side of a double sided insert that is sitting down if no shim seat.

For sure it can be done and the micro-maching guys live in this world all day long but try hard not to design around such radius.
It seems so easy in the CAD where the world is perfect. If only it worked so nicely when making parts to be shipped.
Bob

subsearobot said:

Hi all!
I am designing a small shaft that needs a little flange. there's a lot happening in a small place, so i want to model the tool radius instead of a sharp corner.

shaft is ~.1" diam, stainless 316.
this will be a production part (100/year). I suspect made on a screw machine.

What is a reasonable (minimal) corner radius? I am hoping you will say .003"...

cheers!
ssr

Click to expand...

100 per year is a production part?

.008” almost never get complaints, less in 316 is going to be no end of issues with finish, speed or edge breakdown.


Sent from my iPhone using Tapatalk