I would not say I have the best practice but mostly good enough for company workshop. I am an engineer, not a certified technician. The best practice would be get the settings from your machine and tool manufacturer. And if there is any contradiction you should follow their guideline instead of random guy on the internet.
You gave no background on you or your machine so I am trusting that you already have the machine setup, calibrate and done machining on wood/plastic before.
First step would be get a physical machining handbook, it should contain 90% recommended info for difference materials and bits.
Any bit that does not have Aluminium in the coating will work on aluminium. High-end coatings work better for “strong” alloys and last longer. Nevertheless, uncoated high-speed steel is fine to get started. There is no need to get solid carbide bits when you just started, they have more narrow working range and cost much much more so you need to dial it right from the start. High-speed steel and cobalt runs slower and shorter lifetime but can be re-sharpened. 2-5$ bits from China is too cheap, spending ~5-10$/bit get the job done before it breaks.
If you have fixed bed (router) machine then go for 2-3 flutes bits. If the bed does move then you can go full 4-6 flutes as spindle is more rigid.
For drilling, the flutes length should be 2x diameter longer than intended drill length. Drill point angle: 118° is enough for aluminium. Helix angle: 30° is good enough, 10° angle might be needed for harder aluminium alloy.
Once you are comfortable, go for black oxide coated drill bits and ZrN coated or solid tungsten carbide mill bit for rough cut would be my recommendation. Diamond coated or solid tungsten carbide for finishing.
First number to look up is cutting speed: Vc (m/min) for material group. Non-ferrous materials are group N in ISO. Roughly 100-250m/min is usual for aluminium with >8% Si and 220-600m/min for <8% Si. While this does not change much, you should still get the correct number from catalogue or lookup similar tools.
Spindle speed is now: n = Vc x 1000 / (pi x D)
D being your tool diameter.
Table feed (mm/min): Vf = Fz x Z x n
Fz being feed per tooth from catalogue. Usually 0.1-0.3 mm for aluminium.
Z is number of tooth.
n we just calculated.
Step-down (Ap) and step-over (Ae) change depending on tool geometry so it totally depend on what you buy. Though aluminium is soft so sub 0.05mm step-over cut is difficult, there should be 0.05-0.1mm left for finishing cut.
Drilling, pretty much the same as other materials.
Table feed (mm/min): Vf = Fn x n
Fn is feed per revolution from catalogue.
If you want to drill deep holes then you need to pay attention to pecking and pilot hole. Through holes need to slow down ~50% for the last diameter length.