[Janos]

Hey all, I have a question for you. We have a piece of 316 stainless that has to go on a BIG diet, Sooo we have decided to put the shell mill on the job. But...... I would like to get a good starting point with the speeds and feeds. We typically run a TON of aluminum so this stuff is a bit new to me.

Thanks Janos

[cutting edge]

A little more info would help. What diameter face mill? How many inserts? What size machine?

[Janos]

Ooops, sorry!! Had a very long day and I wanted to end it.

3" Valenite sheer mill ( I will have to get back with you on the inserts. )
6 inserts
Haas VF-4 w/ 20 Hp

Right now it has a castrol lube in it fo alum but when we just faced the part the cuttung edges got wiped out.

Thanks janos

[cutting edge]

I run 316L alot. I run a 3 inch face mill(6 inserts) at 250 rpm and 5 ipm on a VF3SS. I'm cutting .213 off a part that is 2.5 inches wide. I take it in two steps of .106 I can cut about 40 parts like that. Obviously you can go a little faster but your tool life will suffer.

I am using RTW inserts. The part number is SEHW43A6. Hope that helps.

[Janos]

Thanks, I appreciate you help!:cheers:

Janos

[jackson]

This is what my software put out it is pretty accurate you may change a bit as was said for tool life

[djr76]

Might want to run that dry as well. I face mill 304 structural at work and run it dry with good results. The coolant might be shocking it to much, and make sure your using a tough ss grade like vp5135.

[DONNYBRASS]

This is what my software put out it is pretty accurate you may change a bit as was said for tool life

what type of software is it and whats it called. and were can you get it.

[jackson]

what type of software is it and whats it called. and were can you get it.

http://www.mrainey.freeservers.com/ Here is the site i recommend getting the ME Consultant Pro & ME thread Pal as you will see from the site they are worth the money

[Janos]

I run 316L alot. I run a 3 inch face mill(6 inserts) at 250 rpm and 5 ipm on a VF3SS. I'm cutting .213 off a part that is 2.5 inches wide. I take it in two steps of .106 I can cut about 40 parts like that. Obviously you can go a little faster but your tool life will suffer.

I am using RTW inserts. The part number is SEHW43A6. Hope that helps.

The guys I am asking the info for got a .750 valenite indexable shoulder mill and went by what the salesman suggested which was 900 rpm and 15. ipm at .03 deep and quickly dispached a set of inserts. I took your info and adjusted them to the new tool and it seemed to work quite nicely. It was still buzzing along when I left it.:wee:

What kind of coolant do you use for it? They bought a Castrol product that is clear. The kind we use at my day job is Basocut Swisslube (I think my spelling is correct) It works great on pretty much everything.

Thanks Janos

[PBMW]

I have a recurring job in 316. Nasty stuff. I have a 2 1/2" face mill with round incerts. SECO REHR 1605M0T m14 T25m. I turn these at 382 rpm and feed it at 6 to 8 ipm. Takes .100 a pass full width. I can buzz along for quote a while before I have to turn the buttons.

[cutting edge]

The guys I am asking the info for got a .750 valenite indexable shoulder mill and went by what the salesman suggested which was 900 rpm and 15. ipm at .03 deep and quickly dispached a set of inserts. I took your info and adjusted them to the new tool and it seemed to work quite nicely. It was still buzzing along when I left it.:wee:

What kind of coolant do you use for it? They bought a Castrol product that is clear. The kind we use at my day job is Basocut Swisslube (I think my spelling is correct) It works great on pretty much everything.

Thanks Janos

I use Blaser BC40 NF. I am currently running the stainless job that I told you about. I tried something a little different. I was just running a clean up pass on the part and ran the 3 inch face mill at 509 rpm and 18 ipm with a depth of cut about .020. Part is 2.5 wide and 6.25 long. I ran about 60 parts like this before the inserts let go. I haven't tried taking the larger cut yet. Will report back later.

Glad to hear that worked for your friend!

[JMFabrications]

Im glad this thread came up because I was getting ready to ask a similar question. Im face milling 304 SS for the first time today using a Miltec 4" freedom cutter with 6 carbide Octagon TiCN inserts. Thier data suggests using 800 sfm and .008 chipload which came out to be about 764 rpm and 37ipm according to CIMCO calculator. The cut was rough and it chipped the inserts a bit, it just seems way to fast.

http://www.miltecusa.com/FreedomCutt...dsandFeeds.htm

I was using Blaser Swisslube 2000, and I have yet to try it dry. My DOC is .025". Ill take some of the suggestions from this thread and see how they work out tomorrow, but if anyone has any other pointers Id greatly appreciate it. This is on a HAAS VF2 20HP machine.

Thanks,
Jim

[Geof]

I think 800 fpm is very fast, even very, very, very fast. I am not a great one for following manufacturers suggestions and would probably aim for something like 200 or 300 fpm max. I would also bump up the feed to 0.01 or maybe even a bit higher and would take the doc up to at least 0.05 and might even try 0.10.

With a high speed and shallow depth of cut I think all you are doing is creating a wonderfully work hardened surface which is really rough on the cutter.

[jackson]

Im glad this thread came up because I was getting ready to ask a similar question. Im face milling 304 SS for the first time today using a Miltec 4" freedom cutter with 6 carbide Octagon TiCN inserts. Thier data suggests using 800 sfm and .008 chipload which came out to be about 764 rpm and 37ipm according to CIMCO calculator. The cut was rough and it chipped the inserts a bit, it just seems way to fast.

http://www.miltecusa.com/FreedomCutt...dsandFeeds.htm

I was using Blaser Swisslube 2000, and I have yet to try it dry. My DOC is .025". Ill take some of the suggestions from this thread and see how they work out tomorrow, but if anyone has any other pointers Id greatly appreciate it. This is on a HAAS VF2 20HP machine.

Thanks,
Jim

I dont cut a lot of 304 on my mills but i do on lathes and i run it dry might try it

[jackson]

And for the coolnt question i use Qualichem Q-cut 250 i went with it over the blaser for one i dont like the guy that sales it here and i tested the Q-cut and it improved my tool life in my lathes by 40% and my mills by 50% and i run brass, alum, 12L14, 303ss, 316ss, ext and i run them all at refract of 5 mills and lathes both, i have 8 cnc machines and a drum last me well this one has lasted 7 months time for a new one i try to change out tanks every 6 months or so this stuff really dos not seem to get as used as some of the other coolnts i have used.

[JMFabrications]

I think 800 fpm is very fast, even very, very, very fast. I am not a great one for following manufacturers suggestions and would probably aim for something like 200 or 300 fpm max. I would also bump up the feed to 0.01 or maybe even a bit higher and would take the doc up to at least 0.05 and might even try 0.10.

With a high speed and shallow depth of cut I think all you are doing is creating a wonderfully work hardened surface which is really rough on the cutter.

Thanks for the tips, ill def take your advice. Im warming up the machine now so ill check back later today and let you know the results. The reason im taking such a shallow cut is that the stock is 1/2" thick and I want to keep it as close to that as possible. I just want to level out the stock and take that nasty mill coating off the top and bottom. Im making turbocharger flanges that will get welded so the thicker they are the less chance of warpage. The most I could probably go is .035" DOC which might help a bit.

Thanks,
Jim

[Geof]

.... I just want to level out the stock and take that nasty mill coating off the top and bottom...

At .025 you are barely getting under the work hardened surface from the mill. I work mostly in aluminum and think stainless is a real pain and plate material a double or triple pain. But I guess aluminum is not really up to turbocharger flanges .

[JMFabrications]

So I just got done cutting some flanges. Attached are a few pics for you guys to look at. I took Geof's advice and went with a .01 chip and 300 SFM with a .04" DOC full width of the cutter, RPM was 286 and IPM was 17. I was using climb cutting and running the cutter DRY. The inserts did not chip and appear to be in great shape, just some wear on the coating. However im not sure if the finish is as smooth as it should be, a looks a little "FISH SCALED".

1st pic is right after face milling, 2nd is the chips, 3rd is the final part. Will a little more SFM get me a smoother finish?

Jim

[Geof]

That looks very nice. Your fishscales do come from the high feed rate at a low rpm and you can raise the rpm or lower the feed. I would go with 0.03 DOC keeping rpm and feed the same to get the skin off then go down the extra .01 and cut the feed down to .005 per tooth or less if you want a smoother finish. However, if you look at flange faces on exhaust manifolds sometimes they do have this fishscale finish and I know on high pressure pipe flanges the surface is deliberately machined with a high feed rate to get a textured surface which stops the gasket extruding.