Here's my 2 cents on insert tooling on home shop sized machines-
Don't waste money on inserts and holders using the common TPG type inserts. Since those were designed long ago some newer designs have come out that work better and if you shop around the prices aren't much more for the better ones.
I'm assuming you have home shop sized machines and this means you want tools that use positive rake, meaning they cut the metal more like an HSS tool rather than "rubbing it off" using a negative rake insert, which requires much more horsepower and rigidity.
On a lathe I would recommend tools that use the CCMT type insert. This is a positive insert with built in chip breaker that cuts really well on small machines (much better than a typical TPG insert) and since its an 80 degree insert the same tool holder can be used for both turning and facing in the same mounting, so you only have to buy a single holder to get started. I like the Hertel holders, they're made by and just as good as the Kennametal ones and all the parts are exchangable. J&L Industrial often has the Hertel tools on sale, but you'll find these from many other manufacturers like Micro 100 also.
The industry standard listing for a CCMT holder that allows both facing and turning is SCLCR. They're available in a variety of shank sizes and generally 2 insert sizes are used. In the larger ones like the 5/8" shank I have (full model # SCLCR103) the CCMT3251LF insert is used, in smaller shank sizes they go down to the CCMT2151LF size, both work well.
As mentioned earlier you can get good deals on this standard insert on Ebay.
www.carbidedepot.com also has good prices on these inserts.
If you have a small shop, rather than stocking insert types for both steel and aluminum you can get away just buying an insert designed for steel and using it on aluminum also. It won't last quite as long on aluminum but will work very well. The CCMT3251LF and CCMT2151LF inserts I mentioned above are good all around inserts for both light roughing and finishing, and have a small radius to provide good surface finish. For more aggressive roughing you can buy some MF inserts also. Make sure to buy the inserts in a carbide grade rated for mild steel, in the Hertel series that would be grade HC210.
You can also buy boring tools and endmills that use this same CCMT insert. I haven't used the endmills but I would expect they probably work pretty well.
For my endmills (on the wise recommendation of tmngcarbide from this forum) I went with tools that use the APKT style inserts. This is a highly positive insert that was designed for efficient cutting on smaller machines, ie BP sized machines. After switching to these type end mills I got the best surface finish on 6061 parts that I had ever seen on my BP clone CNC machine. The endmills come in style that accept either the 1003 or 1604 size insert, for smaller machines the 1003 size is the way to go and they're a little cheaper.
Endmills using APKT type inserts are available from a variety of vendors and also on Ebay. Keep in mind that the smallest endmill size that uses at least 2 inserts is 5/8", if you go below that you go down to one insert which slows down the feed rate.
For both turning and milling you have to change your approach when using carbide, cranking up both your feeds and your speeds. As a rough rule of thumb increase your SFM (and RPM) by 3 compared to your HSS SFM's. For feed you need to keep in mind that carbide doesn't like small feed rates and the insert will often chip if you use too low a feed rate. On the lathe tools mentioned above they typically spec a minimum feed rate of 0.003" IPT (inches per turn), with a max typically around 0.008" IPT. With an endmill you need a feedrate that yields a Chip Load per tooth of at least 0.003".
As I mentioned earlier, if you try to cut with feed rates that yields less IPT and chip load than describe above, the inserts will wear out quickly and your surface finish will be poor. On a CNC machine this is easy to implement, on a manual machine it takes more care.
Also remember that when setting up a cut with carbide tooling its much better to use a high RPM and feed rate and lower depth of cut than to use a lower feed rate and high depth of cut as your IPT and chip loads will end up too low with the latter approach. I always start with RPM's and feed rates pushed high with a small depth of cut and then carefully increase the depth of cut until the finish quality suffers or the machine starts to complain.
Insert tooling can be troublesome on interrupted cuts as the inserts are prone to chip. They make special tougher inserts in the CCMT size for this application.
The CCMT holders can also use CCGT inserts when you need light cuts, these are sharper, have even more positive rake and are designed to take lighter cuts. I find that with these positive inserts the sharp ones like CCGT will allow you make cuts very similar to what you could do with a sharp HSS tool (lowering the feed rate to get a better finish for example), and I never use HSS tooling in my shop at all anymore.
That's another good thing about the CCMT type inserts compared to a TPG and some of the other older types, the CCMT are available for a much wider variety of applications. But to be honest for the work we do (prototype, very small production run) 90% of the time I'll use the standard CCMT3151LF insert, its pretty flexible and gets the job done.
One thing I should have mentioned about carbide endmills is that you need to be careful to avoid chip recutting, this will wear the inserts quickly. This can be an issue when cutting pockets, to avoid it I used compressed air nozzles to clear the chips from the pocket or of course a coolant system will work. I don't use a full coolant system on my open BP clone machine so as to avoid the mess, we have a Trico Micro-Drop unit that both applies compressed air and a lubricant that's applied in small "micro-drop" quantities so you don't get a big mess. So far that system has been working well for us.
Good luck-
Paul T.