Find out what the sfm recommended for the material is.
Steel is 60-200 sfm (depending on hardness). Aluminum is 150-300 sfm. These numbers are for HSS, about 3x that for carbide.
rpm = sfm * 4 / dia
so for 80 sfm steel with a 0.5" endmill : rpm = 80 * 4 / 0.5 = 720 rpm
Now that is for cutting with coolant, so drop by about 1/3 to keep temperatures good if cutting dry (and then adjust to get straw colored chips).
When starting out, feed rate tends to be the hardest thing to judge (hence the beauty of a DRO that tells you how fast you are feeding), and a lot of novices just wing it, which is not the secret to getting a good surface finish. Adequate chip load is important as the metal the endmill removes helps keep it cool. Too slow a feed rate results in excessive heating of the end mill, to fast a feed rate results in a poor finish.
ipm = rpm * chip load * flutes = 720 * 0.002 * 4 = 5.8 ipm
For endmills, generally use a 4 flute for steel and ALWAYS use a 2 (or 3) flute for aluminum.
Chip load depends on material, and diameter of endmill (YMMV)
Steel: 0.o01"/flute for 0.25", 0.002"/flute for 0.5".
Aluminum: 0.004"/flute for 0.25:, 0.006"/flute for 0.5"
DOC choice is generally based upon spindle power. There is a calculation for it, but I generally don't bother and cut based on sound. A little bit of experience gets you comfortable with how deep to make your starting cuts.
Another way to this is to use a free online calculator (like the link below) or the more advanced offline GWizard of HSMAdvisor (all of which give you spindle power calculations):
http://zero-divide.net/?page=fswizard