How to cut stuff. If you're of a metric mind, you'll have to do your own conversions. Here's a web page that will help understand this explanation: http://www.whitney-tool.com/html/calculatorSpeedFeed.html
RPM: The first and most important parameter you need to keep in mind is RPM. RPM is arrived at via the formula: RPM = (4 x CS) / Dia. where CS is cutting speed. Cutting speeds are associated with materials. Each material has it's own cutting speed for each type of cutter. There are a number of good charts available that list cutting speeds. (See above.)
Keep in mind: The formula is a simplification derived from pi. It's easy to get away with this because the cutting speeds are approximations subject to a number of variables. The charts and the formula just provide a good starting condition. However, once you arrive at a good rpm for your particular machine, using your favorite coolant and your typical cutter, it's easy to back figure your actual cutting speed which will then give better results the next time you machine that material.
FEED: Feed is arrived at via chip load. Chip load is simply the thickness of the chip. Chip thickness varies with RPM and feed so if you change your RPM you are changing your chip load unless you also change your feed. Obviously, the inverse is also true.
VARIABLES: The big variables are rigidity, coolant and cutting tool.
The more rigid your machine and setup, the faster you can go. It's as simple as that. The cutting speed charts and chip load charts are for middle of the road average machines and machining operations. If your machine and setup is exceptionally rigid, you can adjust everything upward. If your machine and/or setup is lightweight, adjust downward.
Coolant is a real mixed bag. Naturally, the best coolants are messy, bad for your health and bad for your machine. (Must be some corollary to Murphy?s Law) Coolant should be avoided if possible or at least minimized. Micro drop application systems work well but are expensive. Spray mist is affordable but will put a lot of mist into the air that eventually settles on everything. Use only with coolants made for misters. No matter how good your ventilation is, you'll be breathing some of it. Flood coolant is the cheapest and messiest. Best used on machines built for it. So, on the one hand, we try to avoid coolant but, on the other, coolant will improve finish and tool life tremendously. Pick your poison.
Cutting Tools: In general, the softer the material, the sharper your tool needs to be. CBN inserts for hard turning actually have a bit of negative rake. Look at a roughing insert for steel and you'll see that the edge has a small radius. At the other end of the spectrum, plastic needs a very sharp cutter.
DOC: Depth of Cut. DOC is almost impossible to define. DOC is the one parameter that is most affected by the variables. The only thing that can pinpoint DOC is experience with your machine and your setups. Use common sense, start conservatively and work your way up. DOC is also affected by your chosen speed and feed.
Materials: Material science is essential to machining. I'm often asked 'how do I machine aluminum (or steel or plastic etc.)'? This is a bit like asking how fast a car can go. Which car? Which engine? Street or Bonneville Salt Flats? There are a LOT of different types of steel and aluminum and plastic. They all have different properties and they all machine different. It's often cost effective to buy a material that's a bit more expensive just because it will machine so much better. A lot of forethought to your material will save a lot of work down the way. Go to a site that sells these materials and they will often list the machining properties, physical properties and the cost. My personal favorite is McMaster Carr. Once you have a specific material in mind, it's much easier to address questions.
Tips: 6061 is a good, all around choice for aluminum and is quite affordable. If you experiment and get the feed and speed just so, it can be machined dry. The trick is the get the chip to part company with the cutter. Aluminum likes to stick to the cutter, then comes back around and sticks to the next chip then in an incredibly short period, totally gum up the cut. If you can get the chip out of there, this won't happen. If the speed and feed are working together the chip sails right out of there. In general, when conventional milling you will need a small step-over (~10%) and a high feed rate. When climb milling back you need a large step-over (~60%) and low feed rate. To machine dry, you will need to keep the rpm lower to keep from heating things up too much. If you do need a lubricant, WD40 is excellent. A very small amount is needed. I buy it by the gallon.
Steel requires the least amount of explanation. If your machine is heavy enough to cut it just follow the speed & feed guidelines. Coolant is recommended.
Polymers. I already mentioned that plastic wants a keen edge. Particularly the softer plastics. What I didn't mention is some polymers can be surprisingly abrasive. If your cut starts out good then shortly develops a burr, you've lost your edge. It will look and feel sharp but it's not. Switch plastics or switch cutters. Go to carbide. Keep your rpm low enough not to melt the material. Coolant can sometimes benefit.
Hope this helps,