Lathe Turning Stainless Steel
Hi All,
I have a nice little lathe called called a Southbend Magnaturn. It's got a 2000 rpm spindle on it and it's previous owner used to cut just about anything with it.
I have done plastic, copper, brass and aluminum on it without a problem. However, I need to do some stainless steel parts and I have no idea where to start with for feeds and speeds.
My part is 1.375" diameter, and I'm cutting part of it down to 1" and putting 8 tpi threads into it.
If someone could give me some safe starting points, I'd really appreciate it.
I'd like to know:
- Suggested RPM
- Suggested starting cut per rev (ie. .050, .040, etc...)
- Suggested DOC per pass
I'm only using three tools, a rougher, a finishing tool and a threading tool.
I also need to do some boring on the other side of the part.
Thanks much,
Wade
PS. If anyone has a good resource for a lathe feed and speed calculator, I'd really appreciate it.
Similar Threads:
Most of the time you can use the cutter's recommended feeds and speeds to start...but that is normally just your starting point. As far as the three tools you've mentioned...that doesn't give us anything to go off. Are they HSS, Carbide, coated, not coated, TNR?...you see....many variables...so just check with the tool manufacturer.
Looking over your post you don't even mention what stainless you are cutting. They vary widely in regards to speed and feed.
Tim
Whoops. You are right, I did miss some stuff. Sorry about that. I thought of starting mfg feeds and speeds, but I admittedly got some import cutters and didn't get any feeds and speeds with them that I can recall.
I'm going to be using 303 stainless.
All cutters including the threading tool are Carbide TIN coated.
Wade
Almost every cutter MFR has a website with speeds and feeds now. 303 is the easiest stainless to machine.
Do you have a machinist handbook? (or google?...LOL)
https://www.google.com/search?q=303%...ient=firefox-a
Tim
I haven't found any for this mfg.
Machinist Handbook > NO
Google > Yes but have found to big of a range of suggestions that I don't know if they are accurate.
The reason I'm asking here is to hopefully get a conservative starting point from someone who has actually done turning on stainless so I don't immediately trash my tools. I figure that someone who has turned stainless before can give me a safe RPM, DOC and Feedrate to get started with.
I'm hoping that isn't too much to ask for. People give suggestions for milling all the time as far as rpm, feeds and speeds go, but I rarely see suggestions for feeds and speeds for turning?
Wade
Coated carbide you can run 500ss easy. Chip load is whatever you want - use your aluminum loads and you will be fine.
For the actual threading, maybe go 200SS
Tim
Thanks for the info. That slow huh? Is it because stainless is a gummier material?
In my CAM software I think I currently have the DOC at something like 0.030" deep. Will that be OK or should I go with more or less DOC?
Also, I'm assuming coolant is going to be as must, right?
Wade
I would suggest you get a Machinist Handbook and start reading it. Stainless is not gummier than aluminum. It is harder (to keep it simple), which creates more heat when you cut it, which can in turn harden the material even more as it is being cut. Which is why the SS is slower, to avoid the work hardening effect. You can run faster than that given the correct insert grade and coating.
What SS do you run aluminum and brass at? With a max rpm of 2k, you will be at about 1500, so you can't run much more SS anyway.
Tim
I ran over 1000 pcs of 2" diameter aluminum at 1000 RPM with I think a .045 DOC and about .005 feed rate.
Honestly, like I said, it's been so long since I did lathe work I forgot a lot of stuff. When I commented on the slowness I was thinking RPMs, not Surface Speed.
This is also why I asked the question on here. Needed to get my head back into the turning thought processes.
Thanks again for the help.
You are right, I should buy Machinist Handbook, but I'm worried I'll fall asleep trying to read it. LOL
Take care,
Wade
No need to read the whole thing front to back! It's a reference.
Supported and feeds are usually posted on the manufacturers website(for the carbide).
I run 303 at anywhere from 500-900 depending on the insert and its geometry, depth of cuts anywhere from .03" to .1."
I don't have specifics for you but that has already been covered. I do have a few comments though.
You keep the surface speed down to prevent work hardening which takes place as a side effect of machining stainless. Work hardening can sneak up on you real fast when machining stainless thus the default is to go slow with a generous feed. If your tool rubs on or try's to cut the hard surface you will destroy a tool real fast.Originally Posted by wwendorf
The goal with the slow surface speeds is to reduce the work hardening. The goal of the stiffer feeds is to make sure you are cutting well under the surface that was previously cut to hopefully avoid having the cutter engage the hard surface.
Depth of cut depends more on horse power and rigidity than anything. However if it was me I'd prefer stiffer feeds over deep depth of cuts.In my CAM software I think I currently have the DOC at something like 0.030" deep. Will that be OK or should I go with more or less DOC?
Coolant or cutting lube should be used almost all of the time. It really doesn't matter what you are machining as it improves surface finish and extends tool life. Well as long as you aren't using tools shocked by coolant.Also, I'm assuming coolant is going to be as must, right?
Wade
In any event you really need to get with Google and the web. Just about every cutter manufacture out there has some sort of web site with information on the tooling they sell. They know the specifics of their tooling and are the best source for starting information to apply those cutters.
Got it all figured out. Hardest part was drilling a .325 hole, and I wound up doing that at 300 rpm with a .001 Inch per Rev. It was slow, but I don't care about speed with these parts, just care about making them accurately.
Outside of a 1.375 diameter was cut at 900 rpm, 0.006 IPR with a .030 DOC.
Boring was done at .020 DOC, 600 rpm, 0.003 IPR.
I'm sure I could tweak the settings a lot, but for my first time in 303 SS, my first part was dead on exactly what I needed. I used a fogbuster with KoolMist as well.
Can't complain.
Thanks again everyone who responded,
Wade
Do not apply what you have learned machining 303 stainless to the machining of any other grade of stainless unless you want some surprises, and burnt out tools. 303 is a free machining stainless steel alloy that is almost as easy to machine as leaded steel it is not at all like any other stainless alloys.
An open mind is a virtue...so long as all the common sense has not leaked out.
I'm well aware of how different materials are to machine. I choose 303 BECAUSE it was easy to machine.
That being said, thanks for the reminder. I do prefer aluminum.
Wade
Reply with Quote
