Runout is a measurement of how concentric the tool is with the spindle center of rotation. It can be measured (in microns) with a dial indicator.
Runout is especially dangerous when cutting small chip thicknesses because it changes the amount of material each flute removes. This can overload one cutting edge and cause wear or breakage.
Rubbing happens when the cutting tries to cut a chip thickness so small that it rubs against the material instead of cutting. Rubbing can be fixed by increasing the feedrate. There is more information on rubbing and chip thickness in the advanced feeds and speeds.
Cutting mainly on the tool tip (traditional milling) causes more deflection than cutting deeper and spreading the load along the whole side of the endmill (high efficiency milling).
As an endmill rotates the flutes contact the material and while they are in contact the endmill experiences a sideways cutting force. Because the flutes are not always in contact with the material the cutting force will vary through each revolution, causing vibration.
If the cutting force is low and your setup is rigid vibration from bad cut stability is not usually a problem. However if you want nicer surface finish or are experiencing vibration issues it is good to check your cut stability.
Low depth of cut, large width of cut, single flute endmill: the one flute contacts material 50% of the cut and there is no contact 50% of the cut. The endmill is experiencing periodic force which can cause vibration and possibly resonance.
High depth of cut, small width of cut, three flute endmill. This creates a consistent force on the tool because as one flute comes out of contact with the material the next flute comes into contact. Specific depths and widths of cut can create perfect cut stability (calculator).
Vibration is the most important factor for improving surface finish and is discussed in its own section above.
In metal climb creates a better surface finish because it starts cutting at the thickest part of the chip, which avoids rubbing.
Conventional cutting start the cut at the thinnest part of the chip, which means the flute will rub against the material until it reaches a chip thickness where it can start cutting.
However for very soft materials like foam, climb will give a worse surface finishes because can rip extra material out with the chip.
The next most important factor is stepover when doing surface finishing using ball or bull nose endmills. Due to the rounded profile small cusps are left between passes creating surface roughness. Use a cusp height calculator to determine how high these cusps will be.
The best way to reduce the cusp height is to use the largest radius tool possible. You can also reduce the stepover but this will increase the machining time.
The feed per tooth for all tools affects the theoretical surface roughness on vertical walls in exactly the same way as cusp height with ball mills. Between each circular cut there is a uncut cusp of metal. Higher feed per tooth increases the height of the cusp and therefore increases surface roughness.
You can use the same calculator to determine feed per tooth cusp height, just enter the feed per tooth where it asks for stepover. However, the theoretical surface roughness from this factor is very small (0.001-0.3 Ra), much smaller than realistic milling surface finishes. This is because bad surface finishes are mostly caused by vibration, not feed per tooth.
In soft materials (aluminium, brass, plastic...) sharper tools will create a better surface finish.
In hard materials (ferrous, titanium...) sharp edges are too fragile and break or dull quickly, which leaves a worse surface finish. In hard materials it is better to use a coated tool that is less fragile. The coating adds a radius to the cutting edge, so coated tools will always be duller than uncoated tools.
Finding the best surface speed is complex because there are several factors connecting surface speed to surface finish.
Higher surface speed means higher RPM, which can increase the vibration. Reducing the RPM and keeping the same or slightly lower feed per tooth is a great first step to improve surface finish by reducing vibration.
However higher surface speed can make the cut cleaner because the material shears faster and reduces material adhesion to the cutter (built up edge).
Like many things in machining there is an optimal range: too fast increases vibration and heat, and too slow can cause material adhesion to the cutter.
No tool cuts what was programmed perfectly: tools bend due to cutting pressure and tool diameter wears over time. In order to hit a desired tolerance you have to measure and account for the errors of your tool.
Example: I want to make a bore between 49.995 and 50.005mm. I will use a 0.5mm finishing stepover. The finishing stepover can't be too small otherwise the difference between the test cut stepover and the final cut stepover can be a large percentage.
It is also good practice to measure the bore at multiple depths to check if it tapers. Multiple finishing passes can reduce tapering.
https://knowledgebase.tormach.com/1100m/spindle-tram-adjustment
