Dry Aluminium Cutting Problem

[JAZZCNC]

Jazz,
what was the DOC and rpm for the G spot??????

Wouldn't know It's a Fooooking myth doesn't exist. .

Roughing endmills are only really useful when used with flood coolant, since the general idea is they make very small chips which are more easily washed away.

Not exactly true has I use 3 flute 8mm and 10mm carbide Rippers dry cutting 5 to 6mm DOC with no problem and can actually cut 100% diameter if required and the specs say upto 1.5x Diam full slot but my machine doesn't like handling that DOC so I keep it safe.
These rippers must have a finish pass has they leave a rippled/ridged surface, great for if you need a grippy surface like spindle mount holes.!!

Hmm, I tired cutting thinner passes each time I had a problem as I thought it would create less heat. Perhaps I need to cut deeper. Chip extraction is obviously key too, but how do you do it well without coolant? I have a reasonable vaccum but a lot of the alu chips are too heavy to extract well that way. It works great for wood :)

What depth do you tend to do got the first pass, Jazz, and what tool do you like to use for general contouring? Do you use a ripper/rougher or a smooth flute?

P.S. Thanks for all your advice chaps!

Yes try cutting deeper but you must clear the chips.!

Blown air is the secret, Oh and having the machine vertical helps greatly. ..!!
Vacuum has to be very strong but still doesn't clear enough, esp when slot cutting deep. Blown air is the only thing other than high pressure flood coolant that will clear the chips fully but again it's messy and you need a good or large compressor.
Either way your into mess and decent blown air setup with correct chip load gives just has good result has low pressure coolant because your not re-cutting chips which you still are with low pressure coolant. The best for tool life and finish is high pressure high flow coolant but for that you need a full enclosure or a Wet suit.!!
I prefer blown air has it's dry and don't have machine enclosed, the mess of dry chips I can deal with.!

Depending on Job I use ripper for hogging away material then finish with either HSS or carbide twin flute. I actually prefer HSS has it gives a better finish it's just wear out quicker but because I'm only often doing finish pass they last ok.
Some times I'll use Carbide on longer jobs for the full job if I'm being lazy and don't want to change tools.

I tend to cut between 2 to 2.5mm DOC for 6mm twin flute HSS often around 800mm/min 10-11,000rpm full slot. (Cutwell code E5521060)
6mm 2 flute Carbide between 2-3mm 900/1100mm/min 12-14,000rpm.
6mm 1 flute carbide 1-2mm 600/800mm/min 11-13,000rpm.
With the 8mm carbide ripper around 800-900mm/min 5-6mm DOC 8-10,000rpm (Cut well code E5711080)

I'm often adjusting the RPM and feeds on the fly depending on how the material is cutting and the load on spindle. I Don't really watch RPM and just monitor the Load on VFD and if it's getting too high then I know I'm being greedy. I never push the Load so high there's no overhead just in case hit any sticky spots or for when tool starts to wear.
After a while your ear will be your best tell to how well it's cutting but the VFD load is a good tool to watch.!

To give you some idea I never gum up cutters above 4mm and below that then I'm nervous has hell for both gumming and snapping so go OTT on the air and coolant.!! . . .But still rarely gum them up.!!