RPM is determined by tool diameter, and material, by calculating SFPM - Surface Feet Per Minute as follows:
SFPM = (PI * ToolDiameter * RPM) / 12 or,
RPM = (SFPM * 12) / (PI * ToolDiameter)
This is usually rounded to:
RPM = SFPM * 4 / ToolDiameter
SFPM is a function of the tool material and the work material. For mild steel being cut with HSS cutters, SFPM should be around 80. For aluminum, 400 SFPM is a good average. If using carbide, double or triple those numbers. So, if you're cutting mild steel with a 1/2" HSS endmill:
RPM = (80 * 4) / 0.5 = 320 / 0.5 = 640 RPM
Feed rate is a function of RPM, the number of flutes on the tool, and the "chip load", which is the nominal thickness of the chip each tooth carves out:
FEED(in IPM) = RPM * #Flutes * ChipLoad
Chipload is a function cutter diameter, and for roughing cuts ranges from perhaps 0.0004" for very small endmills (1/16") to perhaps 0.008" for large ones (1"), and varies linearly for sizes in between. So, for a 1/2" 4-flute endmill, assume a 0.004" chipload, and you get:
FEED = 640 * 4 * 0.004 = 10.2 IPM
Depth of cut should be as much as you can get away with, which will be limited by spindle power, machine rigidity, and coolant used.
Now, you're not likely to reach this numbers on a small mill, due to the limited spindle power, limited rigidity, and inadequate cooling. So, start by setting the calculated RPM, pick what you feel is reasonably modest depth of cut, and start by feeding at perhaps half the calculated rate. Increase feed rate until finish quality starts to degrade. When you reach that point, back off on the feed rate perhaps 10%. Now increase depth of cut until the machine starts shaking, or the spindle motor starts laboring, then back off a bit.
There are no canned numbers, as every job is different, and you have to learn how to "read" the machine. Some rules of thumb:
Keep chip load as high as possible. If you find you have to reduce feed rate well below the calculated value, then reduce the RPM to keep the calculated and actual feed rates reasonably close. Running high RPM with low chip load will cook tools faster than anything.
USE COOLANT!! You will never come anywhere even close to the calculated numbers without coolant. A mist system will work wonders, with very little mess.
Here are some typical numbers I use on my knee mill, running mist coolant:
1/2" 4-flute HSS endmill cutting 1018 steel: 700 RPM, 5 IPM, 1/2" DOC
1/2" 2-flute HSS endmill cutting 6061 aluminum: 3100 RPM, 12 IPM, 1/2" DOC