Machining 303 Stainless Steel

[richardandtracy]

I have just bought myself a 3m long bar of 14mm dia stainless (type BS970: 303S31, EN 10088: No. 1.4305, name X8CrNiS19-9, aka 303L for US users). The cost was a painful £10.56 + VAT, but it should do me for a few years.

 

I plan on eventually using it for a pen, once I've learnt how to use the material and a prototype in aluminium is shown to work. The bar is 'free machining' by stainless standards, but from my first efforts it seems to be very tough.

 

Now, I'm wanting to drill, turn and knurl this material.

1) Do I need high cobalt drills? I currently use HSS jobber drills.

2) Can I knurl it?

3) I have normal steel cutting indexible carbide tips, do I need special tips with a different angle?

 

I have done all my turning to date without coolant. On my first effort with this the material got rather hot (I'm fairly sure the carbide tip was red, can't be completely sure about that but I do know that the swarf came off brown not silver) - is it necessary to use coolant? If so, I need to pop out and get a small 12v fish pond pump...

 

Finally, can any machinists give me any advice about depth of cut, feed/speed etc? I think 0.25mm depth of cut is as much as my lathe can cope with - it was working very hard to manage that deep a cut. Basically - if you can give me the benefit of any lessons you've learnt, I'd appreciate it!

 

Thanks in advance,

 

Richard.

Edited February 24, 2009 by richardandtracy

[Wwillco]

Richard-

I in no way can answer all the questions that you have on it; can only give what little experience I have with turning 303. On my last boat we had to turn some valve stems out it on our archaic metal lathe- we were in a bind, and out of inconel, so 303 had to do. Its been several years, so I can’t remember the settings or technical specs we used; most of that info was placed in confidential quality assurance documents for later reference anyway.

 

1. Can it be gnurled: yes.

2. We used high cobalt on ours; I’m not sure if less will work though.

3. We did use coolant for ours, but we were also worried about screwing up the temper of the metal. If you’re making pens out of it, not high pressure valve components, I doubt that will be much of a worry.

 

Hopefully someone else can give you better specs on speed/depth of cut, but maybe this info will be some help. I would recommend getting that fish pump though.

 

Luck-

Will

 

 

[Clydesdave]

As stainless steel goes, 303 is about the easiest to machine. Fact is, stainless is tough and it's tough to machine. The rule of thumb is it takes six times longer to do the same job in stainless than it takes in aluminum. So, here's some information:

 

Feeds and Speeds: I can calculate this out better for you once I get to work, but it is slower, much slower.

 

Rigidity: You need more power and rigidity than some lathes (assumption) can offer.

 

Cutting Fluids: You will want a heavier oil. Light oils like WD-40 work well on aluminum and do nothing for stainless. They make cutting oils that are specificaly formulated for stainless and I've found they work pretty well. Water soluable coolants are better than nothing, but not much better.

 

Drills: Cobalt at least (rather than High Speed Steel). You're going to make them dull, you might as well use something that you can sharpen.

 

Carbide inserts are great because they last longer and the geometry is consistantly perfect. You cannot run a negative rake, chip angle needs to be shallower than an aluminum insert. Chip breaker is a necessity. Titanium Nitride or some other coating like it works wonders.

 

Tip of the day for cutting stainless: Stainless work hardens immediatly. When you get a chip running, keep it running. Once the chip stops and the cutter runs against the part without removing metal, that area work hardens. After that it requires much higher pressures at the cutting surface to start again.

 

Stainless is tough. It is tough to machine, tough ON machines and wears cutters. Be ready for that. It's tough on machinist too.

 

I'm kind of getting the impression that you are turning pretty fast in order to turn your cutter that hot, and if you're having trouble taking a .25 mm cut (that's only .010") you either have a large radius on the cutter, or your machine is just too small. Slow the machine down first; 100 - 150 rpm. Use lot's of good cutting oil.

 

Let's hear how that works out.

 

 

[richardandtracy]

As stainless steel goes, 303 is about the easiest to machine. Fact is, stainless is tough and it's tough to machine. The rule of thumb is it takes six times longer to do the same job in stainless than it takes in aluminum. So, here's some information:

 

Feeds and Speeds: I can calculate this out better for you once I get to work, but it is slower, much slower.

 

Rigidity: You need more power and rigidity than some lathes (assumption) can offer.

 

Cutting Fluids: You will want a heavier oil. Light oils like WD-40 work well on aluminum and do nothing for stainless. They make cutting oils that are specificaly formulated for stainless and I've found they work pretty well. Water soluable coolants are better than nothing, but not much better.

 

Drills: Cobalt at least (rather than High Speed Steel). You're going to make them dull, you might as well use something that you can sharpen.

 

Carbide inserts are great because they last longer and the geometry is consistantly perfect. You cannot run a negative rake, chip angle needs to be shallower than an aluminum insert. Chip breaker is a necessity. Titanium Nitride or some other coating like it works wonders.

 

Tip of the day for cutting stainless: Stainless work hardens immediatly. When you get a chip running, keep it running. Once the chip stops and the cutter runs against the part without removing metal, that area work hardens. After that it requires much higher pressures at the cutting surface to start again.

 

Stainless is tough. It is tough to machine, tough ON machines and wears cutters. Be ready for that. It's tough on machinist too.

 

I'm kind of getting the impression that you are turning pretty fast in order to turn your cutter that hot, and if you're having trouble taking a .25 mm cut (that's only .010") you either have a large radius on the cutter, or your machine is just too small. Slow the machine down first; 100 - 150 rpm. Use lot's of good cutting oil.

 

Let's hear how that works out.

Perfect, thanks very much.

I was running at 1600 rpm, I'll knock it back to the slowest speed I can (approx 160 rpm). The tool tip I have is approx 0.25mm rad at the end. The surface on all my tool tips is TiN coated - they last much better that way, as a result I've only worn out 3 tooltips since I got the lathe in 2001 (yep, it also shows I don't use it that much). The chipbreakers are intact too. The lathe can be a bit flexible for some jobs - particularly milling with the built in milling head - but I'd be surprised if it can't cope in the end with 303SS once I get the rest sorted out.

 

I shall try to get some heavy cutting oil. Thus far I've tended to drip waterbased fluid on the work from a washing up liquid bottle when I've felt the need for it (not often).

 

I'll see about cobalt drills. I've found an industrial supplier locally that sells them for about 5x the HSS jobber drill price, so I'll have to work out what I need rather than get a set.

 

Regards,

 

Richard.

 

[Clydesdave]

Okay. That 14mm bar is going to be able to be turned at better than 160 rpm..... Here we go (in English units)

 

Austenitic 303 series stainless steel, Coated Carbide cutter

 

Optimum feed rate is .028" / revolution Average is .013" / rev

Surface feet / minute is Optimum 625 feet / min Average is 815 feet / min

 

14 mm = .5502 inches N = spindle speed (rpm) V = cutting speed in feet / min pi = 3.1416

 

N= 12 * V / pi * dia

 

N= 12 * 815 / pi * .5052

 

N= 9780 / 1.5871

 

N= 6162 Feed = .013" / rev

 

Good luck with that!!!! Holy Mackeral, they must have had one heck of a machine to do that!!!!!!!!

 

Even with the power and rigidity of my machines (which are substantial), practicality dictates running at 12.5% of that or: 770 rpm and .0015" / rev feed. That sounds more resonable to me.

 

The calculations are from The Machinery's Handbook 28th edition; Erik Oberg; Industrial Press Inc. The calculations do not take into account the horsepower of, or the rigidity of your machine.

 

That's how it's done.

[btboone]

Just keep it cool. If it's allowed to get hot and harden, it's over. It will break your drills and cause all sorts of havoc. There's no real down side to slower other than the part taking longer. Titanium is the same way. Using the calculated values, I would get a pretty short tool life. If I slowed things way down, I would get around 10 times the tool life.

[someonesdad]

The big rule for things like stainless, monel, etc. (the tough to machine stuff) is slow down. If you were turning 14 mm diameter stuff at 1600 rpm, that sounds way too fast and you're going to generate a lot of heat. I know folks like to use carbide, but I'm still a fan of HSS for turning. I have three main turning bits that have developed over the years and they work well for steel, aluminum, and brass, which are what I use the most (actually, about 90% of my turning except threading is done with one bit). They also work fine on "free machining" stainless. I know the books give different tool angles for these different materials, but that's empirical information for good tool life and good production. If you guys like, I'll post a picture and drawing of this "universal" cutting bit that works well for me.

 

I like HSS because I can pop the tool off the lathe and take it to the grinder for a touch-up or bump it with a hone to sharpen it up in the lathe. I've got carbide bits and tool holders, but use them very rarely -- one reason I don't like them much is that they're not good for interrupted cuts. However, I do like them to get under the crud on a casting or some badly rusted steel.

 

Anyway, when turning stainless, I usually just slow down and turn it like regular steel. I dribble mineral oil on it for lubrication (mainly for drilling), but I usually just turn dry. But stainless work can just get too hot from friction, so I'll just shut the lathe off and go do something else for a while to let it cool off. I'm usually not in a hurry. It's been a while since I turned some stainless, so I just went into the shop and chucked up a 1/2" chunk of bar stock of 303. I dropped the lathe into back gear and turned it at 60 rpm and could easily turn the whole bar into chips (i.e., take a 1/4" deep cut) with a normal feed of 0.0046" per revolution. I remember once playing around and finding out that this lathe would take 1" off the diameter of a 2" diameter steel bar in one cut and it didn't strain all that much. The key is just going slowly to keep the heat down.

 

Clydesdave sounds like a professional machinist, so I'll bow to his knowledge. Still, I've been hobby machining for 40+ years and have found things that work for me. The only thing about stainless that still worries me is drilling and tapping small holes (say, 2-56 and under). Oh, and some of the stainless alloys that don't contain S or Se can work harden mercilessly, as Clydesdave points out.

[richardandtracy]

Thank you all.

 

It sounds as if I need to take it slow & cool, but not take too little off. And use coolant/cutting fluid.

Somehow I don't think I'll be taking it up to 6000 rpm...

 

someonesdad, if you could post a drawing of your cutter, it would be appreciated.

 

Right. I think it's now time for me to make some mistakes so I can ask what I've done wrong!

 

Regards,

 

Richard.

 

[someonesdad]

Here's a picture of the toolbit. It's made from a chunk of Armstrong 7/16" cobalt HSS:

 

http://www.gdssw.com/fpn/toolbit.jpg

 

 

Here's a sketch of the angles. There's very little back rake; maybe even a degree or so of negative rake (the intent was that it be zero rake, as it was first a roughing cutter). It works well on steel (stainless and carbon steel) and free machining brass. I also use it sometimes with aluminum, but usually switch to the other toolbit which has more back rake. But this tool bit shown here is quite versatile (most of my cutting is towards the headstock). I can rough as deep a cut as I want, then grab the diamond hone and give the thing a few licks to smooth things out and that radiused nose will produce a nice finish. I've got hundreds of toolbits laying around, but this does most of my cutting.

 

http://www.gdssw.com/fpn/toolbit1.jpg

 

BTW, that's Herbin Perle Noire on canary paper. Do you know how many canaries they have to kill to make that much paper?

[richardandtracy]

Thanks for that. I'll print it off & have a bash myself. So far all my sticks of HSS are 5/16" square - as that's also the size of my carbide insert tool holders, and I can use pretty much the same starting point with shims to get them on the lathe centreline.

 

I shall have to have a go & see if it'll work better than my carbide tools.

 

Regards,

 

Richard.