Cutting stainless - paging Harold V!

Well, I'm not harold. I can't even play him on the internet!

But I can suggest you use a horizontal mill for this and a plain milling cutter if you possibly can.

Otherwise I would suggest you will be taking about 0.050 deep at a pass. You will most likely want to use a two flute end mill for this.

Jim

================================================== please reply to: JRR(zero) at yktvmv (dot) vnet (dot) ibm (dot) com ==================================================

Owch... I don't know that I envy you that job :-)

A 1/8th endmill capable of milling a 3/8" deep slot will be quiet bendy and that'll likely limit your depth of cut and speed of movement.

From my experience doing similar things, you may find that even a carbide endmill that size won't last anywhere near 275 inches of slotting in stainless.

I've actually found that stainless (even 303) is a real PITA to machine with small endmills. The difference between takign a big enough chip to avoid work-hardening and breaking the cutter can be quiet small.

Could you use a slotting saw to take out most of the meat then finish up the ends with the endmill? The less material you have to remove with that tiny endmill the better (for your wallet and your patience)

I'd suggest chain-drilling the slot first but then again, those tiny endmills can have a tendency to catch on the work-hardened edge of the holes as you take out the remaining web of material and snap in the blink of an eye.

But don't take my word as gospel, I'm not a professional machinist and odds are that *I've* been doing similar things all wrong anyway :-)

-- you can contact me via

I definitely agree with this. Use a plain milling cutter for this job. I've not had to cut 1/8" slots in stainless rounds like this but I have cut more 1/4" slots than I care to ever try again. This job screams milling cutter. I know that the best I ever managed was about

Wayne Cook Shamrock, TX

Bruce,

I could use a slotting saw in the horizontal mill. The slots are closed on each end, so I suppose I could plunge cut the slotting saw if I find one in a small enough diameter.

Thanks,

George

Hmm.. . looking through my trusty catalogs. Maybe a keyseat cutter might work.

We sometimes make butterfly shafts for exhaust systems, not 303 but usually 316, do them on a Bridgeport with a fixture made to be 2 V blocks with clamps. Use a slotting saw, cut through as far as possible from one side, then lift the quill and move the table to finish from the other. 3/32" wide, and half inch shafting, keep the speeds low and it works well, just have a good supply of sharp cutters. Feeds will be heavier than you would expect, and keep the cutter wet with your coolant/lube of choice. Arbor for slotting saws aren't hard to make and they're a lot cheaper than woodruff cutters.

We sometimes make butterfly shafts for exhaust systems, not 303 but usually 316, do them on a Bridgeport with a fixture made to be 2 V blocks with clamps. Use a slotting saw, cut through as far as possible from one side, then lift the quill and move the table to finish from the other. 3/32" wide, and half inch shafting, keep the speeds low and it works well, just have a good supply of sharp cutters. Feeds will be heavier than you would expect, and keep the cutter wet with your coolant/lube of choice. Arbor for slotting saws aren't hard to make and they're a lot cheaper than woodruff cutters.

Ah haa.... you've discovered the secret trick.

Woodruff key cutters are like little tiny plain milling cutters, already mounted on an arbor.

Don't use a carbide end mill for this job.

If you go with a woodruff key cutter, do a good job of calculating the sfpm number - it's a lot slower than you think, especially for stainless. Also figure what the feed rate should be, probably higher than you think to keep it from work-hardening.

Use a good cutting fluid. Some folks swear by water-based like soluble oil, as the water does a good job of carrying away the heat. That's the real bug in doing stainless, the material has very low thermal conductivity so it's easy to overheat tools.

I myself stick with my standard lard oil/kerosene mix. Another excellent choice would be dark sulfurized thread cutting oil from HD.

Good luck.

Jim

================================================== please reply to: JRR(zero) at yktvmv (dot) vnet (dot) ibm (dot) com ==================================================

Try to find one with staggered teeth, more $$$$$. The typical straight tooth key seat cutter isn't exactly a free cutting tool.

Something I've done, only not on that many slots, is to drill through the material using a .120 drill and spacing the holes about .135-.150 apart then endmilling to size. Takes a long time but it's cheap for the drills. Maybe drill through just the end area of the slots then use the keyseat cutter. A 5c indexer would be pretty handy doing it that way, you could drill the ends of the slot then rotate 90deg, cut with keyseat cutter then rotate 180deg and keyseat again etc.

JohnF

Hey George,

Sorry to not have been of service, but you've been handed some pretty good advice as far as I'm concerned. I strongly endorse the method suggested by Lennie, especially if you can support the opposite end of the part while holding it in an indexing head. You might be able to cut the slot before cutting the parts to length, thus providing holding lengths, assuming you wouldn't otherwise have some available. If, by chance, you need a radius at the ends of the slot, it wouldn't be all that hard to go back and clean out the corners with a carbide end mill, a four flute, and progressively plunge instead of feed longitudinally. Stainless isn't fun to machine with small end mills, where they like to break like glass. By using an index head as has already been suggested, you can use a combination of woodruff cutters and end mills to do the job. May take a little time, but it will work with reasonable results. The comments about straight tooth Woodruff cutters is right on the money, but don't be too concerned if you're locked in to a straight tooth. It will be somewhat more lumpy when cutting, but it will do the job. I'd caution you to make sure that the cutter is pushing away from the outer end of the part if it's not supported, not climb milling. Otherwise it will most likely pull into the cutter and you'll have a horrible crash, that's assuming you end up holding the parts in an index head and the end isn't supported. .

If you choose to do the job in a vise, I'd suggest you use a slightly undersized drill on each end location, then open the holes on each end with a 1/8" carbide 4 flute end mill. Using multiple flutes will help prevent chipping, sort of on the same order of having enough teeth in contact with work when sawing. Start on one end and plunge through, then move the mill table about .020" or so for each plunge cut and repeat.until you've moved from one end to the other. You can then take a light cut on each side to clean it up. With your generous tolerance, you can end up with a very nice looking slot and not be much over .125", so long as you stick with a carbide end mill. HSS will likely deflect a little more, although it will work. Cutting the entire depth of each side of the slot will work fine this way. The advantage of this method is that the material is totally supported by the jaws so you don't get any deflection. Given the information you've provided, I think I'd run the job this way if it was up to me. You can support the shafts on an aluminum parallel, or remove your hardened one once you have the piece located in the vise.

One more thing. If you have any options on material, try to buy 303 Se, not

Hope this helps, George. Let us hear how it goes.

Harold

Since you have 100 of these to do, why not check out what a water jet shop would charge you to cut these slots. If you try this with end mills you are going to spend lots of time and eat lots of end mills.

Thanks everyone! Some great advice and ideas that are much appreciated. Lennie's idea to cut from both sides didn't even occur to me. . . duh!

Thanks again,

George