You have bought the cutters so you cannot change that, however, do not get small diameter four flute again if you want to use them on aluminum.
Two flute, uncoated and if you can get it micrograin carbide; these cutters will have a shinier appearance than most uncoated carbide cutters.
Speed (rpm): With carbide you can easily go up to 3000 feet per minute and a simple calculation shows that to get this at the periphery of a 1/8" diameter cutter you would need to spin it at aroung 91,000 rpm. I think I am safe in making the assumption this is faster than you have available. Go as fast as you can; no matter what size cutter you are using go at top speed with your machine.
Feed (ipm): With two flute carbide cutters 1/4" and above it is probably possible to feed at 1% of the cutter diameter per tooth, i.e., 0.005" per rev or 20 ipm at 4000 rpm. But, you should only be taking a depth of cut of about 50% of the tool diameter with an engagement of up to 60%, i.e. 0.125" deep and 0.15" wide.
But you have 1/8" four flute and you are cutting full width so you have to be very conservative, stay down in the 2 - 4 ipm region for now until you have completed some successful cuts and then maybe start going faster.
Plunging? As Leeway suggests, NO, not a good idea. The flutes load up with chips very quickly; milling cutters are really meant to cut sideways not down. Ramping in is acceptable but make it a gentle wrap for a small cutter; maybe one cutter diameter down for each inch of forward travel.
Lubricant/coolant. Absolutely essential. You can probably get away with brushing it along the intended cut line or use a little spray can. I have never found WD40 to be very good on any material; the ATF works very well on aluminum but, of course, the best thing is a proper cutting fluid.
An open mind is a virtue...so long as all the common sense has not leaked out.