Aluminum Without Coolant

[DeusExMachina]

I just have a small desktop mill (taig) and I mostly cut AL. Recently though I had a nice 3-flute 1/4" HSS (uncoated) Roughing End Mill decide to melt a large pile of aluminum to its surface. I had been running the end mil at 6700 rpm, 0.05" doc, at about 15 IPM.

I think that perhaps my chip load was too low and I dulled the cutter end down to the point where it was just rubbing at the aluminum instead of cutting it -- I'm not sure to be honest. The End mill had about 120 hours on it before it decided to melt my part. The cutter can probably be saved, just need to knock the wad of aluminum off the end but I decided to get a few carbide end mills.

I now have a couple 1/4" 3 Flute (uncoated) finishing carbide end mills and I'm wondering what sort of speed/feed I can run these things at -- Dry. I've heard in most cases you should run carbide as fast as possible (in my case 10k rpm).

Assuming 400 SFM, 10k Rpm, and a 0.00125" chip load/tooth I've come up with a feed of 37.5 IPM (DOC To be determined after playing with the cutter a bit). This seems a little high to me to run without coolant.

I've never used carbide before so some general tips would be greatly appreciated. Carbide is a much more brittle material then HSS and doesn't like interrupted cutting much, is it better to climb or traditional mill with carbide and is step over an issue?

Since its more brittle, I'd assume a larger step over (so that more of the end mill is engaged at a time with the material) would be better?

I know carbide can withstand much higher temperatures and is in general much harder then HSS. But aluminum is rather sticky, how fast can carbide be run in aluminum before it starts to gall up?

Thanks in advanced.

[kingfisher]

Can't you run a mister or some kind of a lube setup off a airline? It would make a big difference. I work for a major cutting tool company and all of my stuff is in the car right now. I would be happy to figure out the speeds and feeds for you and let you know where you should be.

You will want your tools to hang out as short as possible with a very good rigid holder.

your not saying if you side cutting or slotting? What kind of aluminum?

Max your speed......if you are running normal aluminum with coolant you could run around 36,000 RPM's but of course you can only go max of 10,000 rpms. Tools and holder need to be a good solid set up.

Your feed rate should be around 45 IPM. I actually came up with 60 IPM but this is all just a guess without looking at your setup and no coolant.

[Geof]

What alloy are you cutting? Some aluminum alloys will gall up the cutter no matter what; the best easily available alloys for machining are 6061 and 7075.

You can easily run your uncoated carbides at 10,000 rpm and it really makes little difference what speed you run them at without some form of coolant/lubricant you are likely to get aluminum adhering to the cutter.

You do not need to swamp the cutter in coolant but you do need something to act as a lubricant and let the chip flow over the cutting edge nicely. In a pinch automatic transmission fluid will work very well just painted on along the cut line or squirted from a sprayer.

[mc-motorsports]

Why 3 flute? Not on a 1/4" EM anyway. Someone is going to argue with me, no doubt, but you'll be better off with a 2 flute.

The first rule to aluminum cutting is GET THE CHIPS OUT! A good high pressure flood coolant is best, if you use a mister, you'll need more air than coolant, put a valve on the coolant line so you can crank the air pressure without fogging your shop. Otherwise, just use a blast of air, but coolant helps A LOT with cutting aluminum. Welding chips is going to be your limiting factor, most of the time anyway.

I'm guessing your slotting? Slotting is the most difficult thing because the chips don't have anywhere to go. If your pocketing, your better off with a deeper cut and a smaller step over. That will both increase your material removal rate, if you set your parameters right, and extend the tool life by using more of the flute and not just the corner. Plus it will be easier for the endmill to eject the chips and your not cutting so much with the corner of the endmill and rubbing the face, this is where you will generate the most heat and be more prone to welding chips.

Always try to use the biggest endmill you can because you will have more flute clearance, and usually spindle power isn't a problem. I won't use a 3 flute on anything smaller than 1/2". High helix endmills tend to work better if your just using a flood coolant, kinda just dumping coolant on the part. With a mister or just air, they don't eject the chips well enough. If your using a mister, just use a standard helix. And if your slotting, use a standard helix. You have the right feeds and speeds, DOC and step over when the chips eject out the top of the endmill with ease.

[DeusExMachina]

The material is 6061 T6. Yes I'm slot milling, the slot is 0.375" deep (the part is a lead mold -- after doing the roughing its finished using a tapered ball end mill). The slot isn't terribly wide, so 1/4" is the biggest that I can use. It is a 45 degree helix bit -- though I haven't tested the difference this makes yet.

My last bit was a standard helix and about 30% of the chips we're thrown out of the hole while milling. The program takes awhile to run so usually about every 10 minutes or so I'd blow the chips out that piled up in the part. Though so far, the general consensus here is get some sort of cooling airblast/flood/mist whatever heh.

[metlcutr55]

clearing chips is key. i dont have flood coolant, but i run a mister. and when i push more, i up the mist more. another thing ive found is walmart sells a store brand aerosol called tech lube. supposed to be a wd40 or crc generic, its pretty poor for lubing things, but at $1.19 a can it works well to keep aluminum from sticking to end mills and enhances surface finish. stinks tho.