When looking at carbide endmills, you will see a specification for shank diameters called H6. This from the ISO-286-2 tolerances for shafts. For our 1/2" example, the standard says within the shaft diameter range of 10-18mm the tolerance is +0/-11 microns which converts to +0.0000/-0.000433".
Most carbide endmill manufacturers purchase pre-ground carbide rod already cut to length with a chamfer on one end that will be the shank end. Below is a sampling of ten 1/2" rod blanks measured at three points. Blue is the chamfer/shank end, red is the middle and green is the cutter end.
To meet the H6 tolerance, the rod cannot be under 0.499567". Blank #1 exceeds the tolerance only on the shank end and should be rejected. Blank #8 does not exceed the tolerance on the blank end, but is up against it on the cutter end and middle.
Some manufacturers have tighter shank tolerances of H5 (+0/-0.000315) and H4 (+0/-0.000197). Again these were for a 1/2" shank.
Making it work I am going to punt on part of this to John Bradford of Makino below.
I would add to his great recommendations that you test the runout in the spindle at operating temp. Use a good 50 Millionths test indicator and a mag base or gage stand with fine adjust shafts. We will part from our normal advice and say that pre-balanced holders will work here (the endmill has so little mass) and that the holder’s projection or diameter will not make a difference one way or another. Runout and balance are key, but the tool is still very flexible and dynamics are in play. While we can't tap test miniature endmills there is some science that can be applied. The Harmonizer by MLI can record the sound of the cut and determine resonate speeds where the flexing is at its worst and need to be avoided. This will work with spindle speeders and air spindles if you can adjust the output speed. https://goo.gl/WLeUy4
On standard spindles and toolholders, RCSA can be used to model the miniature endmill and predict stable speeds. Once you get a process dialed in you will want repeatability of the tool stick-out. The rings used on PCB drills might be a good solution if the shanks are 1/8" or 3mm.
Stiffer means higher frequencies and higher speeds. Shorter should mean stiffer, but too short can be detrimental for other reasons. If you let any of the flute or washout (where the wheel grind continues past the flute length) to recede into the holder or collet you are creating a stress concentration on a smaller profile than the full round shank. It will take a lot less force to break the tool.
As Professor Scott Smith from UNC Charlotte likes to say, "Random processes produce random results". If you have been following our posts you will have learned that a milling tool is a flexible beam and that changing the length of that beam, even a small amount, will change its frequency and can impact the tool's performance. You will also have learned that rotating a spiral fluted endmill in a toolholder can change the balance of the assembly significantly. If you have something running really good, you want to keep it that way.
Most toolholders other than side-locks use friction to hold the endmill shanks. So you need help to get repeatable tool changes. We found these wrench-free aluminum shaft collars from Ruland Manufacturing. The aluminum won't damage the cutting edges and holds up to the heat of shrinkfits. You can also use steel set screw collars or drill stops.
Set the tool projection from the tool tip, not the back end. Overall length is not a tightly controlled spec in ISO or ANSI, so measuring from the back or using backup screws will not give you a repeatable tool stick-out. You can use a caliper depth rod or depth micrometer to set the projection, just subtract the collar thickness.
Also, use the slot in the collar to orient the tip of one tooth, like a gunsight. This will retain balance. Look through the slot and rotate the tool until the tip lines up with the slot. If you are using variable pitch endmills, identify tooth #1 and set to that each time. Put a witness mark on the end of the toolholder and use that as your target when orienting the new tool with the collar's slot. Balance the tool assembly first, place the collar on the tool while still in the holder and line up the slot to a tooth. Mark the toolholder at the slot with a center punch or drill point. For a collet chuck, torque the nut to the proper value, then mark the nut just as above.
Sharing information about high performance milling technologies, the result of 30 years of research.