Go with the TTS - Tormach Tooling System. If you use their holders, its way easier to run through tool changes. Sure its a bit pricier, but its really nice to be able to run a program with 5 tools and not have to stop and Z0 the tool each time. You could probably get some used holders off ebay or something. 2 drill chucks, a bunch of endmill holders, a 2.5" or so facemill.
You can get away with most of your machining with a .250" endmill. HSS is good for aluminum, its a lot less rigid (i.e. breakable) than carbide. You'll need some larger some smaller cutters, but in general, go with either .250", .5" if it needs to be bigger, or any smaller size as needed. .250" is a good workhorse for FRC sized stuff.
I can't say much about coolant, but I could probably ask some guys on Monday about what we use at work.
An edge finder would be good, but if you really don't want to spend the money, stick a nicely ground .500" pin in a collet or drill chuck, push your piece up against the pin, and call that zero. A DTI is pretty essential for relocating parts around anything ciruclar (holes or bosses), so I would go for one. McMaster should be ok, just don't expect it to put up with abuse or last a long time. But its a good place to start until you really understand what you need.
For Z0ing, that's exactly what a lot of people do - try to slide something between the tool and the workpiece until it no longer fits. Your trusty .500" ground pin is good for this, as is a 1-2-3 block or anything else that you know is a very precise size.
As far as CAM software goes, I've had great experiences with HSMXpress. It's free for solidworks, and Autodesk owns it so I can only imagine you can get it for Inventor. MasterCAM is great, but might be overkill if you can't get it super cheap.
I would stay away form the 4th axis for now until you get to know your tools and machine. It's rare that you'll need it. If you want to do cool stuff with making hex, there's always these (
http://www.mcmaster.com/#collet-blocks/=t442a5) used with a vice.
A PCNC 1100 isn't super powerful or rigid, so I would stick to shallower cuts, on the order of maybe .040" to .050". I've always been conservative with my cutting since I usually don't make more than half a dozen or so of any given part. 2 or 3 shallow cuts is way better than 1 deep cut at 1/3 of the feed. I've never been able to get G-wizard to give me good numbers on a Tormach, it just doesn't have the coolant flow or rigidity needed to get those numbers. Stick to .050" deep, and adjust your cutting feed as necessary to not break tools/give a good finish.
Other things: Get a 90 degree spot drill bit. I use them all the time for spot drilling, chamfering, and occasionally countersinking. If you can spot drill and pre-chamfer a hole at the same time and then break all your edges with the machine at the end of the program, your parts are way nicer and come out faster.
Build a small tool library of stuff that always stays in the holder. Set the heights once, never worry about them again. I mean, how many tools do you really need? A spot drill, a few end mills, a face mill, and a few drill bits (these change often though).
My workflow on the PCNC 1100 was usually take oversize stock. face mill a bit off the top, machine the part almost complete with .125" or so stock on the bottom, clamped in the vice, flip the part over and clamp the finished edges in the vice, and run the facemill to cut off that .125" extra. It works for most parts, it keeps all or most of your features done in the same setup, and you don't leave any stock surfaces.