|Andrew Johnston||14/02/2011 22:02:25|
1509 forum posts
I've recently had the need to make some parts on my CNC mill from 316 stainless steel. This has been rather a steep learning curve, so I thought I'd write a few notes on what I have learnt; the hard way of course.
The parts concerned are from 1.5mm 316 stainless steel sheet, and have complex outlines and internal cutouts. I had three off, of two parts, to make, and didn't fancy doing it on a manual mill. The S/S used is 316 because, after machining and bending, the parts need welding.
I have turned a fair amount of 303 and 316 stainless steel with few problems and have always got an excellent finish using carbide insert tooling. I have done very little milling of stainless steel and no CNC milling of it, until now.
I used two cutters; a 6mm three flute centre cutting uncoated endmill, and a 2mm four flute centre cutting TiALN coated endmill, both from Garr Tool.
Looking up Machinery's Handbook gave a surface speed of 200fpm for carbide in 316. Being cautious, so I thought, I downgraded that to 120fpm, corresponding to 2000rpm for the 6mm cutter. Choosing a chipload per tooth of 0.05mm gave a feedrate of 300mm/min. After a couple of broken cutters and another one worn out, I did what I should have done in the first place; put the kettle on and then look up the Garr Tool machining data. For 316 they give 20-35m/min and a feedrate of 0.01-0.025mm/tooth for a 6mm cutter. I chose 22.6m/min (1200rpm) and a chipload 0.025mm/tooth for a feedrate of 90mm/min. What a difference! The cutter ploughed through the cuts slowly but smoothly; yippee!
Figures for the 2mm cutter were 3500rpm and 70mm/min feedrate. That seems a very high rpm, but the diameter is three times smaller, so for the same surface speed the rpm needs to be three times higher. The feedrate equates to a chipload 0.005mm/tooth, at the lower end of the manufacturers recommendations.
I have added a few pictures in an album showing the parts and few snapshots of the machining in progress.
A few other random snippets. I used flood coolant at all times, mainly to flush away the swarf. The depth of cut with the 6mm cutter was 1.7mm, to ensure complete break through. With the 2mm cutter the same total depth was achieved in four passes, each of 0.45mm. Typically, despite breaking several 6mm cutters, I didn't break a single 2mm one. The aluminium subplate is sacrificial. Better to cut into it than the table! Once it gets too badly mangled I'll either recycle it or give it a facing cut. It's scrap anyway; it was cut from a larger sheet that, due to a brain fart on my part, was ordered to the wrong size for a previous project. In retrospect I am amazed that the 6mm cutter actually worked with the original speeds and feeds; it just wasn't sustainable for even one part. The local professional tool shop sold me some 6mm cutters with a small radius (0.3mm) on the tips as specially for stainless steel. I haven't tried them, but can see that it makes sense, as the cutters wear initially on the sharp tips; if you don't break them first of course!
One other thing, I also mangled a HSS drill on the manual mill too, by hesitating, and then getting it red hot trying to finish the hole. It was a vivid way to relearn the lesson of never, ever let the tool dwell when machining stainless steel. It'll work harden before you know it. Then only carbide will touch it, if you're lucky.
I hope this is of use to somebody, if only to prevent wallet damage. Mind is still sulking.
PS: Sorry about the mixed units, that's just the way it goes, and I'm comfortable speaking both imperial and metric so it doesn't bother me.
Edited By Andrew Johnston on 14/02/2011 22:04:37
|49 forum posts|
Are your coated toolbits HSS or solid carbide?
Whenever I have tried to machine at recommended feeds and speeds, the toolbits end up broken, so I'm not the only one to suffer.
Take care of the wallet.
|John Stevenson||15/02/2011 01:31:20|
2527 forum posts
I am working with a company at the moment that is developing a hand held machinists calculator and believe me the speeds and feeds saga is exactly that.
Plenty of tables out there but no one mentions a variable that takes into account the machine.
Many of the commercial cutter manufacturers assume every one has the all singing, all dancing latest Mori Seki with 5 axis as a 30,000 rpm refrigerated spindle and quotes insane speeds and feeds.
|615 forum posts|
Did you ever try low speed high torque?
You get none of the heat issues, tooling has to be tip top and the machine needs good stiffness to compensate.
I've used this approach on both alu and stainless, but only as a hobbyist dood, high speed can be too nerve racking and prone to error issues.
|David Colwill||15/02/2011 09:48:16|
|145 forum posts|
I have some of Cutwels alpha mills and never had satisfactory results with them. I had a job to do on my cnc and decided to work out the speeds and feeds properly. I used the kennametal calculators:-
All of a sudden my previously useless cutters performed brilliantly.
The moral of this particular thread must be:-
If in doubt sacrifice a goat before you start!
|86 forum posts|
What mill did you use? Is it for hobby use or the to bring the bead on the table?
"I used two cutters; a 6mm three flute centre cutting uncoated endmill, and a 2mm four flute centre cutting TiALN coated endmill, both from Garr Tool.
Looking up Machinery's Handbook gave a surface speed of 200fpm for carbide in 316."
Solid carbide end mill needs to be run the hell of it:
I'm not very familiar with these, but I have impression that HSS and solid carbide is of completely different animal. Carbide probably would do better with a rigid setup, machine and if the spindle can run it to the table. HSS probably wins on all other situations.
Probably not for SS, but I have heard that solid carbide cutters are used often without liquid, but blasted with copius amount of air.
|Andrew Johnston||15/02/2011 21:45:21|
1509 forum posts
Thanks for the replies, I'll try and answer, or comment, roughly in the same order.
Both cutters were solid carbide. The small amount of manual milling I've done with stainless steel was with HSS cutters, and that was very slow. I reckon about 80% of my CNC milling is with carbide cutters.
I'm beginning to see that feeds and speeds are bigger than a saga, more of a Wagnerian opera. There seem to be wildly differing figures, and opinions, published for similar cutters in a given material. I have used the G-Wizard software from the cnccookbook website, but to be honest I didn't find it that easy to use, and sometimes got some rather odd numbers out. When it went to subscription I decided not to use it any more. I can do the basic sums in my head, or with a calculator, more quickly; none of it is that critical.
As I understand it the best way to utilise a smallish CNC mill as opposed to a manual mill is to take small cuts at fast speeds and feeds, rather than 'hogging' out slowly with a larger cutter. I regard 1200rpm as fairly slow. I haven't worked out the power required for the achieved metal removal rate, but I expect it to be well below the capability of the mill. I suspect I'm limited by the cutter, not the power available. All the internal radii were 3mm, so I needed to use a 6mm or smaller tool.
It's certainly difficult to know where to set speeds and feeds. Some of the published data seems over-optimistic, but on the other hand some of 'hobby' magazines seem to be unduly pessimistic. In the end I suppose one has to experiment and build up one's own knowledge base of what works with the equipment one has available.
The mill is a Tormach, so high end hobby. However, for this job I got paid, as part of a much bigger project. The downside is that I designed the parts, so I can't complain about iggerant designers if there's a problem making them! I also understand that industry often uses airblast to remove swarf. I have read that you can get a better price for scrap if it isn't contaminated with coolant. I don't have an air supply in the workshop so I used a coolant flow to remove the chips. That was the primary purpose of the coolant, to remove the chips, not to cool the tool. I normally turn S/S dry without any problems. Apart from hopping about and muttering naughty words if you get a hot chip on the back of the hand that is!
I can't remember if I mentioned it, but all the milling was set to be climb milling.
|Ian S C||16/02/2011 10:38:07|
3247 forum posts
Andrew, you know that the main reason for cutting oil is to make the chips stick to the back of your hand. Ian S C
|Andrew Johnston||16/02/2011 11:27:12|
1509 forum posts
Well, I never knew that! I always thought it was for washing the workshop floor and walls, since that's where most of mine seems to end up. It's one reason I've given up using coolant when turning with carbide inserts. At any sensible speed the coolant only has to get onto the chuck and it's half way up the wall and across the floor. I use coolant on the lathe when using HSS tooling, for drilling and for parting off, except in brass and cast iron.
Coolant gets used on the mills mainly for chip clearance, and for cooling on the horizontal mill, as all the cutters I use on it are HSS. At some point I expect I'll get around to replacing the coolant pump on the Bridgeport. I've had two pukka Bridgeport coolant pumps go down with partial shorts in one phase. In the end I bought a brand new three phase pump. I just haven't missed it enough yet to get round to fitting it.
Please login to post a reply.