You can get router bits for cutting aluminum dry from www.onsrud.com. They won't be cheap, though.

I'll second this. These bits can run at 'ludicrous speed' and the geometry won't try to pick up the sheet like a typical spiral end mill will. I'm pretty sure they come in down cut as well, which would help keep the sheet from singing you a tune.

I have had some success using a stick form of 'grinders paste' and a new one that I like is made by Boeing (yes, the jet company). In practice often I will trace out the path with a pen in the mill first, then go back and smear the stick lube on the cut line sort of like it was a crayon. Your compressed air stream will keep the tool cooled down (very important) but won't pick up the waxy stick lube. The lube does a very good job keeping the cutter surface 'slick' so it won't collect aluminum, and does not saturate everything around it like liquid coolant.

Hi Simpson36
That lube sounds like real good stuff, do you have a proper name for it or a link to were you buy it from. Just out of interest sake what size cutters are you using and how much depth per cut are you takeing per pass?
I tried to cut some alloy a while ago with a 2 flute 6mm bit apparently made for alloy cutting, I run the router at 7krpm 1500mm/min add with a  cut depth of 1mm/pass on 10mm plate, The first and second pass were fine until the cutter pulled itself out of collect and cut 10mm in one pass, funny thing the motor didn't loose a rev the cnc started loosing steps in X and Y , Probably from the tool load but didn't stall in movement or break the cutter. So I decided back then that cut down cutters are the only way to go!
From those with experience how noisy is it? or how noisy is it meant to be? When I tried it back then it was a like high pitch squealing and screeching. I don't think that's right.
Cheers
Katoh

In my experience it is quite noisy because the aluminum sheet vibrates close to the bit. Anyway you can get an acceptable finish in one pass, or if you want to make it better you can leave 0.2mm for a finish pass

I don't really need a great finish because all the cuts are going to be welded up against another part or hidden.
To cut a 6mm plate in one pass, I thought would be to excessive for the cutter and machine. On timber I use the rule of thumb 1/2 x cutter dia = max cut depth. I thought alloy would be even less.
Katoh

This tools are supposed to cut one diameter whithout problems but with aluminum i wouldnt try, specially if is not good quality.
Onsrud has some nice chipload tables online and at the back of their catalog. If i remember well, they give the values for 1xD and then they say that for 2xD decrease 25% feed and 3xD decrease 50%, but it is not clear for me wether thay reffer to full slotting.
Always try to keep the recommended chipload and SFM. If you dont feel confortable feeding too fast, lower feed but also lower rpm to mantain chip load and SFM. Otherwise you will generate too much heat.

Thanks for that, that's basically what I was thinking, I was thinking to use a 6mm cutter and do it 3 pass on 6mm plate, or I don't know if I'm pushing my luck too much now, is to use a 1/8" cutter in do it in 4 passes that's about 1.5mm per pass, I really need to sit down with some scrap and try a few different things.

From those with experience how noisy is it? or how noisy is it meant to be? When I tried it back then it was a like high pitch squealing and screeching.

A larger tool will probably be quieter. When cutting hardwood , a 1/4" bit will literally scream, where a 3/8" bit will be nearly silent.

On timber I use the rule of thumb 1/2 x cutter dia = max cut depth

If you're machine is up to it, you should be able to cut 1-1.5x dia. Yesterday I was cutting walnut 3/4" deep with a 3/8" cutter, at 400ipm. With harder wood, like maple, I decreased the depth to 3/8".


I found a post on another forum from someone who cuts 1/8" 6061-t6 aluminum all the time. Uses an Onsrud 63-622. Cutting dry. .03125"/pass (.8mm), 85ipm and 19000rpm.

You are always going to be better off cutting all the way thru the material in one pass if you can, even if you need to use a slightly larger cutter. Likely marine grades of aluminum are called for here and those cut fairly clean. If I remeber correctly, the machine in question has enough power to make the 6mm cut.

The biggest issue in cutting aluminum in multiple dry passes is keeping the slot clear of chips, and heat generated at the bottom of the slot. Re-cutting chips also makes heat and lots of vibration, and the cutter rubbing on the sides of the slot make a lot of heat that cannot be carried away in the chip. A thru cut automatically clears the chips, runs cooler and smoother. In my experience, the clogging of multi flute cutters always starts at the bottom of a slot where the heat is highest. That's one reason a single point 'router' type bit is best to use as it only has a single contact point with the bottom of the slot. You can modify a normal cutter to resemble this profile by grinding the end to a concave shape, but better to spend the bucks and buy the excellent cutters produced specifically for this type of operation.

I'll just throw in a Simpson tip-of-the-week here for those who have 'tried everything' and still cannot get a multi pass cut to work for them. If you are having a bad time with a particular material, you can try offsetting each successive pass by say .003" to the climb milling side of the cut. The result is faily dramatic. There is a rather complicated explanation for this that I won't go into here, but I toss it out there as an option for those who are inclined to experiment. 

Gentlemen
 I'm starting to get a bit confused now. I cant see my cnc cutting a 6mm sheet of marine Alloy 5086 with a 6mm cutter in pass, I can only see a lot of stress on the machine, a huge tool load, and a good possibility of loosing steps. and or damage to the cutter, spindle or even the CNC mechanics. My very good friend with his Huge Bridgeport CNC mill will only take passes to 1/2 the dia of the cutter, and he does this for a living.
Gerry even you wrote about the other thread the guy who cuts 1/8 sheet in nearly 1mm passes, and Yes I can see the advantage of offsetting each pass, but It just sounds like a lot of material to be removed in one pass.
I don't really know, or maybe I'm just a bit of a SOOK when it comes to my machinery but I don't like when I here them struggling, and when it happens you can hear them, I'm sure no good can come from it.
I know my Machine and with a 3/8" cutter at 120"/min  with 5mm passes its very happy in melamine and most timbers, I once had the problem were my final finishing pass ended up before my cutting passes and it cut 3/4"  MDF in one pass, the result was not pretty, it did not loose steps but hold downs failed due to the tool load and 2 ton of cnc bolted to a concrete slab started to shake and vibrated, pretty scary stuff.
The day when the cutter pulled out and it was cutting 10mm thick plate with a 6mm cutter in one pass, was definitely bad enough, now that's only 1.7 times cutter dia. I cant see this as being a good thing.
Katoh

With a 5HP spindle, you definitely have enough spindle power to make those cuts in a single pass. Sounds like the issue you have is machine rigidity, and possibly lack of stepper power.

I've been running $100K+ routers for the last 10 years, so I have a little experience. Sometimes cutting deeper and faster will make much less noise than shallower and slower. Also, how well the part is held down has a large influence on noise generated. I used to use a router with vacuum pods. When cutting near the pods, the sound volume could be as much as 5 times lower than when cutting in unsupported areas. At my new job, with a 5x12 vacuum table with two 40HP pumps, cut's are much quieter. I can cut 3/4" MDF in a single pass, with a 3/8" bit, at 700ipm. If the bit is sharp, it won't make hardly any noise at all.

Get a good 3/8" compression cutter and you should have no trouble cutting 3/4" melamine in a single pass at 500ipm, if your machine is up to it. Your spindle certainly should be.