Hi Jason,

Buy what you need as you need it!

2 - 1/8" drill mill - meh
2 - 1/4" drill mill - and meh. I did recently purchase a 3/16" mill drill for a particular project and it is cool for bridge pin holes because you can drill and chamfer without a tool change. However, you can't use vacuum obvious reasons.

another alternative is to get coated hss tools. TiN, AlN, or TiCn. here's why:

-cheaper then solid carbide.

-a bit more shock resistant then carbide in the larger sizes. .125 >

-sharper then carbide. yes sharper. hss is a wrought material and as such can obtain and hold a higher degree of edge sharpness, while carbide tools are made from sintered powder. under a microscope you'll see inclusions at the cutting edge. in your hands you can feel the difference.

-the coatings are very wear resistant and wood is abrasive. run dry and tested to destruction on horrible to machine metals like inconel, stainless, titanium, molybdenum, hastelloy, invar, etc.. they are more then a match for simple wood. hss in either t15 or m42 grade can handle a good deal of heat and abrasion and when combined with a coating that is usually rc 72 and higher, makes for an economical combination. in modern cnc programming, using today's high speed milling strategies on aluminum, we'll often rough out the majority of the material with cheap, disposable, offshore coated tools that can take a serious beating then come back in with high end carbide tools to finish with.

-the coatings can help prevent chips from sticking to the tools and provide lubricity at the cutting edge.

when you get down to the smaller sizes under .125 though, then go with carbide for the higher core strength. in either case investigate a coated tool.

your tooling list seems to gravitate towards 2 flute tools. in the smaller sizes, 3 or 4 flute tools have a larger core diameter that can help with tool breakage, but the trade off is decreased chip capacity. also 2 flute tools generate unpleasant harmonics and vibrations in the higher rpm ranges whereas odd numbered flutes cancel each other's vibrations out and can generate a smoother finish on side walls. these harmonics can sometimes be dialed out by dampening the fixturing or by finding the harmonic frequency range of the machine and staying away from that rpm area. a quick and dirty test is to place a indicator point on the rotating spindle and the base to the machine and run through the rpm ranges. look for the rpm the shows the most movement on the dial. write that speed down and avoid that range when programming.

fwiw, true aluminum specific tools generally have a high helix, 35 deg and up. this is the amount of spiraling that the flute has ground on the tool. they are designed this way for fast chip evacuation, high feed rates, and a high rate of shear in side milling applications with non-ferrous metals. the down side is that they have significant "pull". meaning that if your part isn't fixtured down firmly you run the risk of lifting it off the table and throwing it, or pulling the tool out of the collet, or on a less then sturdy diy machine pulling the head downward. this would be something to consider when pocketing pick ups, tremolo pockets, neck pockets, or full depth cuts on the outside body contours in a solid body electric for example. but not a big issue in shallow depth of cut or open surfacing projects like bridges, the backs of necks, fingerboard surfaces, etc...

for inlay pocketing i'd look for reverse spiral tools. yes you can drive chips down to the floor of the pocket and get some re-cutting going on, but the advantage of a clean pocket lip is worth it imo.

btw, what kind of machine do you have?

sorry for the wall of text but as an mfg engineer i get fired up about cutting tools and machining!

I also use a large diameter bottom cleaning bit from grizzly for spoilboards and truing up surfaces of vacuum fixtures.

What you left out was tiny tools for fret slotting and inlay.