Before we get into calculating the best feeds and speeds for your goals, there are a few more concepts we need to understand.
Chipload: Chip Thickness per Tooth
While feedrates are specified in length units per minute, the more important measurement is something called "Chipload". Thing of a chip as looking something like a comma in cross section, or perhaps an apostrophe. One starts big and gets smaller at the end. The other starts small and gets bigger at the end. We'll ignore that difference for a moment, though it is important as we shall see later.
Chipload is a measurement that is independent of spindle rpm, feedrate, or number of flutes that tells how hard the tool is working. That's a very useful thing, as you could imagine. Hence, manufacturers and machinists typically like to talk about chipload for a particular tool.
You can see that a tool with more flutes (cutting edges) has to be fed faster to maintain a particular chipload. Since each tooth is going to take a cut every rotation, a tooth has only a fraction of a rotation in which to cut a chip that reaches the chipload thickness. During the time it takes to rotate the next tooth to start cutting, the tool has to have moved far enough to shave off a chip that is thick enough. Hence, tools with more flutes can be fed faster. A 4 flute endmill can be feed twice as fast as a 2 flute, all other things being equal.
Why do Tools Break from Too Much Chipload?
You can imagine that forces simply become too great if a tool tries to take too much "bite" by having too much workload. This can chip or break the cutter.
But there is a second issue that comes from too much chipload--the chips get bigger and eventually can't get out of the cutter's way. Beginning machinists probably break more tools because they don't get the chips out of the way fast enough than because the force of the feed is breaking the tool. If the cutter is down in a deep slot, the chips have a particularly hard time getting out of the way. We use air blasts, mists, and flood coolant to try to clear the chips out of the way, but if they're way down a hole or slot, it makes it that much harder, and we have to reduce speed.
More exotic tools are available with 5, 6, 10 or more flutes. Experienced hands will tell you that if you're profiling (where there's lots of chip clearance) steel and aren't using 5 or 6 flutes, you're leaving money on the table. Let's run the numbers in G-Wizard. Suppose we're profiling some mild steel--1020 or some such. We're going to profile the outside of a part, so there's plenty of clearance. Cut depth will be 1/2", cut width 0.100", and we'll use a 1/2" TiAlN Endmill. Here are the numbers:
4 Flute: 3158 rpm, 29.8 IPM. MRR is 1.492 cubic inches/minute. A little over 1 HP.
5 Flute: Same rpms, now 37.3 IPM. MRR = 1.865. 1.3 HP. That's 30% faster cutting.
6 Flute: Now 44.8 IPM. MRR = 2.238. 1.6 HP. 60% faster than the 4 flute case.