The Tool Diameter is specified by the tool manufacturer, also known as the Cutting Diameter.

Through cutting and profiling - a good rule of thumb is to keep the diameter equal to or larger than 1/6 of the material thickness, as this allows you to use full passes without having problems due to the end mill deflecting under cutting loads. For example, if you are cutting 3/4" thick material, the smallest end mill used for cutting or profiling would be 1/8".

Pocketing - to mill a pocket, you can save a lot of time by first "clearing" the majority of the material with a larger end mill and then running a second program to finish cutting the pocket edges that couldn't be reached by the larger cutter. To clear the pocket, you typically want to use the largest diameter tool that you have, which works with the material that you're cutting and fits inside the pocket. Then, use the largest diameter tool that works with the outline of the pocket for finishing, taking note of the minimum radius of the outline path that results.

Flutes are the spiraled part of the end mill which allow for cutting on the edge. The number of flutes can be counted by looking at the tip of the end mill and counting each cutting surface. For example, the photo shows a end mill with four flutes.

For CNC Routers you typically want fewer flutes as the spindles run much faster than conventional milling machines. For example our Velox router's max speed is 18,000 RPM whereas the bridgeport mills max speed is 5,000 RPM.

Surface Speed is the linear speed that each tool edge will travel at, through your material while cutting.

The maximum surface speed is determined by a combination of the nature of the material that you are cutting, and the nature of the material that your end mill is made of. Since end mills are typically quite expensive, you probably don't want to determine this experimentally. Most end mill manufacturers have done this work and publish lists of optimal surface speeds for various materials, using their end mills. For most end mill materials and surface coating combinations with the same description (eg. "titanium nitride (TiN) coated carbide"), maximum surface speeds are similar across manufacturers. Usually, the surface speeds listed by end mill manufacturers are maximum speeds, and it works well to cut at or below this speed (a few materials actually have a minimum surface speed for proper cutting, but this is relatively rare). You should start any new job at 50% (or less) of this maximum, in order to be able to observe any problems and pause the machine before a hazardous situation occurs - while surface speed is independent of feed rate in principle, using typical chip loads results in a tendency for feed rate to scale with surface speed.

Chip load per tooth is the appropriate amount of material that one cutting edge of the tool should remove in a single revolution.

Chip load is usually between 0.001" and 0.010", with exact maximum chipload determined by end mill manufacturers based on the end mill and stock material characteristics, like surface speed.

Most prototyping work on any material can be done well with a chipload of 0.005" for roughing passes and 0.002" for finishing passes. Even the sharpest blades have some roundness to the blade edge and just rub against the stock material before the pressure is high enough for it to start cutting. With the smallest chiploads (like 0.001" or even 0.002"), it is possible for the blade to just mash the material underneath and never create a chip, especially if the end mill is dull. If this happens, you must use a larger chipload to prevent overheating (including fire!), because a significant amount of the heat generated during the cutting process is ejected with the chips!