Do you have a budget? It's hard to give recommendations in a vacuum.
I would recommend against buying anything over 1/2" in carbide until you are familiar with the machine. You'll just be throwing away money and $86 is not a small mistake. I'd probably start with 1/8" 3/16" 1/4" and 1/2". You could throw 3/8" in if you like, but it's not super necessary. There's really never any reason to have end mills above 1/4" in increments of less than 1/8 though, and usually 1/4 is a better interval.
Depending on what tool holders you get (not a good idea to use in a collet chuck, as the flutes on the second end will get clamped against the collet), Lakeshore's double end mills are a good investment and can save you about 33% on sizes 1/2" and under.
Extended length isn't necessary at the start. You'll figure out what you need it for and then you can buy it as needed (probably only will need 1/4" and 1/2").
Corner radius is always preferred if you don't need a square shoulder. The number one reason end mills go bad is the corners of the flutes chip and then the cutting edge gets destroyed. Corner radii help prevent this.
Carbide reamers are a waste of money for FRC purposes (Maritool doesn't even sell anything above .500 in carbide). Stick with HSS.
We don't bother reaming anything we CNC unless we want a precise slip fit. Press fit bores are just as easily achieved via circular interpolation. It's generally a good idea to have a healthy stock of reamers though.
This is pretty much the best face mill you can buy for aluminum (we have one). The problem is the inserts are extremely pricey, only give you 2 cutting edges, and cannot be used to cut anything but aluminum or plastic. That kit is a fantastic deal as you would pay $700 for the inserts and body normally.
I'd probably recommend
this guy as it's dirt cheap, has a unbeatable warranty (destroy it, even while being an idiot, and the replacement is free), uses cheap inserts that can be indexed 4 times, and can take inserts for ferrous and non-ferrous materials (he only sells ferrous inserts but I'm certain he could find you non-ferrous ones). Your machine can't take a decent cut with anything over 2". 45 vs 90 only matters if you intend to cut to a shoulder with the face mill. 45 cuts better.
Maritool sells nothing but high quality stuff, but you want bright finish drills and the only standard drill bits he sells are black oxide. Aluminum has an affinity for black oxide and will stick to it. The parabolic drills are unnecessary. They won't work well in anything but aluminum and a standard 118* or 135* drill works just fine in Al. No need for anything but HSS either.
There's nothing wrong with the 82* countersink, but you'll need either a spot drill or a mill/drill to spot drill holes and chamfer any features that are not holes. Close vs free doesn't have much to do with the accuracy of the machine as compared to what it is you're assembling and how much slop you can afford (or how much you need to actually be able to put it together). We use free because #7 becomes a dual purpose drill.
Form taps are great but they're a fantastic way to get yourself in trouble if you don't fully understand how they work and the relationship between percent of thread profile, class of thread, and H-limits. Essentially you have to drill a larger hole than a cut tap uses, but that hole is not always the same size depending on what the H limit of the tap you buy is.It can also become problematic when you have a part that for one reason or another you can't or don't want to tap on the machine and you drill it for a form tap and then someone else hand taps them with a cut tap without realizing the difference. They're also only good for ductile materials (aluminum, low carbon steels, some stainless)
More important than the cutting tools you get, you need to get workholding and toolholding. These are a significant investment relative to the cost of cutting tools.