Ahhh... well you should be aware that all carbide is certainly not created equally :) ... we've tried all kinds of different endmills and Hanita just trumps everything. The cool thing is if you don't do stupid things with your machine and just mill aluminum or softer materials, you'll never need to buy but one endmill per diameter.
http://www.ebay.com/itm/HANITA-TR-4C43-1-2-3-Flute-Carbide-TiAlN-0-03-Corner-Radius-End-Mill-H20/121232809304?_trksid=p2054897.c100204.m3164&_trkparms=aid%3D222007%26algo%3DSIC.MBE%26ao%3D1%26asc%3D20140407115239%26meid%3Df19ea6613e2e4dca883202a3d2b9fafc%26pid%3D100204%26prg%3D20140407115239%26rk%3D7%26rkt%3D30%26sd%3D281502190095
That's a good example of what I use for Aluminum... we use a longer length of cut (LOC) because they serve as multi-purpose end mills and don't chatter too bad at 2.5x diameter (for example, a 1/2" would have 1.25" LOC), but that's a very good price for it and I doubt you'd need much more than that for that mill... if you're finishing, and the endmill is on size (hasn't been reground), you can step down the finish passes by the LOC and still get a clean finish... I don't know the sizes of stuff you generally machine, but 2 or 3-flute carbide is great for non-ferrous metals... I prefer a SHARP 2-flute HSS endmill for plastics...
I realize the prices of software are absolutely stupid, and I haven't tried any Linux versions of CAD/CAM, but we generally design in Solidworks and export a parasolid to Mastercam. The parasolid comes in Mastercam with the geometry traced and a solid model. I like to separate the geometry and solid into two layers and use a third for toolpath lines. from there, you just trace your toolpath lines from the geometry and create toolpaths (which keeps you from bastardizing the model).
For surfacing, you can rough/finish in 3D with the 3D toolpaths, It will ask for a drive and check surface. The drive surface is what you want to machine, and the check surface is used when you don't want a cutter to hit a wall or something in the way. If the toolpath insists on going out of your boundary, you can trace a containment line around your drive surfaces. For most applications you can use 3D parallel for flat surfaces (which steps over gradually and traces your surface in YZ axis) and 3D contour for steep surfaces (which steps up or down gradually and traces the surface on XY axis)... note that turning on create curves in all axis in your tolerance menu will greatly shorten the G-code, as otherwise it plots it in tiny XYZ increments.
For surface machining, you have to remember that the bigger the tool, the bigger the step you can take and create the same scallop height (the distance between the crests of the ballnose). So while a 1/2" ballnose can take .014 steps and still leave an easily sanded finish, a 1/8" ballnose would require a .0035 for the same finish... but you were likely well aware of this...
A couple programs that are nice to have handy that automatically calculate speeds/feeds:
http://www.cimco.com/download_registration.php3?area=1&id=20&prodname=CIMCO_Feed_and_Speed_-_Freeware
http://www.emastercam.com/board/files/file/777-chip-thinning-calculator-for-windows/
The chip thinning calculator is for high-speed toolpaths or very light depths of cut... since your endmill isn't engaged much in the part, your speeds and feeds can increase sometimes astronomically... otherwise you're basically just burning up the edge on the cutter or producing alot of unnecessary heat on the part...
Of course, you'll always be limited by your 2000 RPM, but those give you a more mathematical option to calculating speeds and feeds other than "I'm gonna go turtle" :P
If you're using teeny cutters you'll just plug in 2000 RPM automatically and figure out a chip load that works...
Off the top of my head, in standard 1018 (cold rolled steel)... 1/8" should handle a .0008 chipload, 1/4" - .0012, 1/2" - .0018, 3/4" - .0024... those are conservative enough for overnight production runs. your Surface Footage a Minute (SFM) for Aluminum on that mill SHOULD be around 600 (keep in mind you can run it up to 5000 SFM with the right setup/cutter/machine), but small cutters will want more RPM... calculate off the average diameter in contact with the dremel bits... you can certainly ramp up your chipload from a conservative 1018 standard on plastics and aluminum, but it's all depending on what tool you're using and the rigidity of your setup.
But yea, most plastic runs better with air cooling unless you're running some obscene SFM which can melt the plastic while it's cutting... Aluminum, however, tends to gawd up a cutter without coolant. if you ever get ahold of brass, it machines like butter, but beware of the chips... they're the herpes of machining... it's like fucking glitter man :)
Typical SFM for Carbide/HSS in our shop
1018: 400/80
Aluminum: 1000/200
Delrin: 2000/400
Nylon: 1250/250 (namely cause it's spongy and you can't hold on to it without it flexing in)
UHMW: 1250/250 (see Nylon for why so slow)
360 Brass: 600/120
...use the HSS SFM for drills and if you're working with weird impregnated plastics, just look up the machinability in comparison with one of the aforementioned materials and calculate by percentage...
Seeing as it's just a hobby and you're not mass producing PCB circuits, I don't know if any of that was even helpful... but it is what it is... happy machining! :)