Better luck machining aluminum

Iggy, it *aluminum*, aluminum is routinely machined dry. Coolant isn't your problem, but it's getting you wrapped around the axle and not focused on where your problem actually is. I machine quite a bit of aluminum and pretty much never use any sort of coolant, or even sprays of WD-40. The only time I use fluids on aluminum is when hand tapping.

I can't see your G-code, but forget the coolant and try something like

1200 RPM, 0.100" depth of cut and 10 IPM. If you have a two flute end mill this is only like 0.005" chip load, very conservative. Watch how it cuts at that feed rate and try the feed rate override to bump the feed up if it looks happy. You have a 2-3 HP machine, you should not be taking cuts that are a fraction of what my 1 HP machine happily takes.

Take a look at:

Pretty much all of that aluminum was machined dry on my wee little 1J Bridgeport (except of course for the parts turned dry on my lathe). The only place coolant was used was on the engraving with a tiny carbide engraving bit.

"Pete C." fired this volley in news:4c522b8e$0$10427 $ snipped-for-privacy@unlimited.usenetmonster.com:

Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete on the last issue.

I do a great deal of work in 6061 with no coolant and no problems moving significant amounts of metal -- even with my old BP "M" head, which is fractional HP.

LLoyd

agree with the above - with the last piece of aluminum I machined on my Abene mill, I needed a 1/2 inch by 3/4 inch deep rabbet around the edges of a slab - I put in a 1 inch end mill at whatever my table of RPM said for aluminum and milled it in a single pass, I think I had the feed set to 4 inches per minute, but it's been a while - worked perfectly. of course this is a manual mill, not CNC, but that shouldn't matter

7

I also agree wit no coolant necessary. I do lots of milling on 1/4 tooling plates of 6061. I began with mist coolant, but the mister leaked, so I stored it in an old plastic waste basket. One day the janitor spotted it and threw it out. It was in a waste basket, right? Since then I mill dry with two-flute end mills.

Almost all my work is completely through the plate, so chips are not usually a problem. In your case, they will be. Can you rig up a shop vacuum to suck out the chips? That and a 1" chip brush will get the job done.

Paul

I had pretty good luck machining aluminum with an end mill made for aluminum and a mist coolant setup. I think the mist coolant system mainly helped by blowing chips away from the cutter. My end mill was a 3 flute for aluminum that I bought from McMaster Carr IIRC. The 3 flutes gave more strength than

2 flute and more chip clearance than a 4 flute, or at least the ad said something to that effect. It's time to put Quincy to work!

RogerN

Actually I have decided to make a pump from the mill to work. It is inside the mill's base. It is not that hard to get to, through the side door.

I will make the coolant pump controlled by EMC instead of just the panel switch. That way I will be able to turn on coolant with M8 command.

The weird thing is that there is liquid in the sump now, but it seems to be straight oil. Once I get it to work, hopefully tonight, I will pump it all out and look. It may be all the lubricating oil from the ways that accumulated.

i

OK, that's good. I guess I was just spinning the cutter too fast.

i

Yes, I have a vac nearby, I suck chips with it routinely

I'm not sure coolant really helps pick up the feedrate. From the other thread it seems you are using a 3/8" endmill? I'd probably use 1800 RPM there, and for a

4-flute cutter I'd feed at about 10 IPM. And, much better to take lighter cuts and keep the cutter moving rather than taking a deep cut and crawling. At least, that's MY method.

That oil in your sump is probably an oil-based coolant. Might be even messier than water-based, but it probably works fine, too.

Jon

Roger, just how far do the chips fly?

i

No, it's difficult to spin it too fast really, but the feed rate needs to be appropriate for the cutter RPM. Again it comes down to the chip load, i.e. the amount of material removed by each flute of the end mill each time it rotates around, which is a function of the RPM, feed rate and number of flutes.

Chances are you were feeding far too slow on that first attempt, which resulted in very thin chips which stayed in the cut area and got mashed together gumming everything up. I lost track of where that post was, but you can certainly calculate what your chip load was for it and I bet it was 0.001" or less which is far too low.

Additionally, note that there are a lot of folks out there cutting aluminum dry, with a CNC router spinning a bit at 20,000 RPM and moving at quite high feed rates on home built CNC routers. You can find a bunch of these online.

Pete, I will try some more. The problem is, one mistake and the endmill snaps off. I think that I should practice with square end endmills instead of the ball ends. I have much more of those.

i

I think that part of my problem is that I use a ball endmill. I will mess more with it on the weekend.

No, it is just a mess of way oil that accumulated.

i

I saw a video of that, very impressive.

i

Practice with HSS end mills, not brittle carbide ones.

On Fri, 30 Jul 2010 06:51:20 -0500, "Pete C." wrote the following:

I haven't yet started machining metal (my jobs are usually minor fab and in sheet metal), but I think I just tasted a key element in my education here, Pete. Thanks for sharing that.

-- To see what is right, and not to do it, is want of courage or of principle. -- Confucius

It can be difficult to get adequate surface speed near the center of a ball-nose cutter. It's tricky to program them for complex cuts, and plowing through solid metal with one is problematic.

You usually use them to get the radius you need when you're cutting only on one side, and even then, you have to program speeds and feeds carefully so you aren't pushing the center of the ball at a rate faster than it will actually cut chips. Profiling is especially tricky.

As for speeds, you can't run an ordinary mill at surface speeds in aluminum that are too fast for a carbide cutter. With a 3/8" endmill, you can't turn it too fast for HSS. And that's even running dry.