What's new
What's new

HELP! Turning small diameter stainless steel 316


Jul 13, 2022
Good morning fellow machinists.

I was wondering if anyone could help me. I am struggling with feeds and speeds on smaller diameters.

WHEN MACHINING THE JOB CHATTERS LIKE CRAZY. Length of job is 56mm and a 20mm stock diameter.

I am turning stainless steel 316 down to 8mm Diameter using Iscars f3m range in a maple tech CNC lathe max RPM 4000.

What feeds, speeds and depth of cut should i be using? I am currently running at 110m/min DOC 1.4 F0.18 - 0.22.
When reaching diameters of 12mm and below, the machining process starts squealing terribly. My guess is this happens due to loss of cutting speed.

What should i do !!!?
Any help would be greatly appreciated!


May 21, 2020
As much as it may seem low SFM is to blame due to your RPM being maxed out it's more likely that it just isn't rigid enough at that diameter for the speed you are going. First step whenever encountering chatter should always be try going slower. sometimes very slow. I seem to remember from my lathe days sometimes need to to get as low as 100 SFM with a very slow feed and a lot of taper to get some stainless parts to come out. Not sure your quantity but it can get you through the job.
Keep in mind these are SFM numbers. MM would be about 1/3..??

Some tricks you may try to get the cycle time down once you figure out how slow you need to finish it at,

Maybe rough it extra big while it chatters then take two slow finish passes (assuming this doesn't wreck tool life)
Another option that can work on some tougher jobs is rough (and finish if tolerance isn't tight) in steps. : stick the part out 15mm, machine that, then 30, machine that...
Maybe you can even finish it little by little if you have some transitions in the part geometry to hide it in.
I also really hope you already ruled out the tailstock, Seems like the obvious answer but ya know, those work good.

Sorry to ramble but with minimal info on your scenario I could bother you with 20 questions like people like to do before they answer or I could just give you 20 answers

Good luck. hopefully something here helps.


Jun 28, 2012
Mt Clemens, Michigan 48035
So you are getting really NICE results from 20 mm down to just before 12 mm? Or just "less bad" results?

If "nice", are you, or are you NOT raising the RPM as diameter decreases so as to hold that sweet-spot @ (wotever) surface (units) per minute has been working for you?

Tool center-height is less forgiving of error as diameter decreases. Is it set optimally?

Coolant? No coolant? Is your workpiece temp shooting-up markedly by the time you approach the smaller diameter?

How much of that 56 mm is unsupported in the cut? Smaller diameters are less stiff than larger ones.

You may have to change the way you approach it, but there ARE ways.

Here's one in a 303 Stainless Alloy that is far the more extreme as to reduction in diameter, but has similar run-length - in two clampings, yet - and is as "unsupported" as it gets.

If Joe can do THAT?..... 30 thou is UNDER ONE mm, yah?

Your tasking should be easy enough. Even in 316.

Capt'n Obvious
Jo Pie mentioned bringing in tha tail for support, I was thinking that that if running such a part often one could have a tool holder with having a couple threded holes on the away side and an added bar with a hole so it might/would act like a steady on the part being turned..

Booze Daily

Sep 18, 2015
Rough and finish the 8mm dia first before machining anything else on the bar. That will allow the stock to give you the most support.
Also use the smallest nose radius you can. I've even finish turned with a groove insert since they have smaller corner radii than most typical turning inserts.


May 8, 2020
try using the stock to support your cut. you would slow down your feed accordingly. only going to be relevant on the last pass as your stock is large in relation to your finished diameter and the size of your cutting tool face...