in any CNC cutting operation, most of which you haven't told us about yet. There's the tool, for instance. You mention a 1mm carbide tool, but not how many flutes it has, the length, the helix slope, or the cutting angle. More flutes make a tool stronger, but the shallower flutes of a 4-flute cutter will clog easier, and clogged tools tend to break. A longer tool, obviously, is also more prone to breakage than a shorter one of the same diameter. A higher helix will eject chips faster, but also can tend to grab the material more. Brass wants a fairly flat cutting angle, but most endmills are designed for aluminum, which wants a more acute one. See if you can find some recommended specifically for brass. Carbide is a very hard material, and it wears out slowly, but that doesn't seem to be your immediate issue. Carbide doesn't hold as sharp an edge as High Speed Steel, and it's a lot more brittle. It might be that using HSS tooling instead of carbide will solve your problem.
Then there's the speeds and feeds. You say you're going "slow", but not what you mean by that. Metals are cut much more slowly than wood. If you're breaking bits, try .5ipm and work your way up from there. Your 8k rpm spindle might be fine for wood, but it's quite fast for brass. If you can slow it down further without losing torque, that might help. And while .2mm (is that depth or width of cut?) doesn't sound like much, you could reduce it by half - remember, this is CNC; you don't have to crank the mill, just let it run; it'll finish in its own good time if nothing breaks.
Another thing to consider is the cutting strategy. Are you engaging the tool on both sides, or just cutting one side away? It's much more stressful to do the former than the latter, so if you must do that, reduce feedrates accordingly. And if you're plunging straight into the material, that can break tools as well; endmills don't drill particularly well. Make sure you've got center-cutting endmills (some aren't capable of plunge-cutting at all) and try to design your toolpaths with ramping entries rather than plunges.
Metal-cutting operations are dependant on rigidity above all. If the spindle runs out a little, big wood-cutting tools won't be affected much, but small metal-cutting ones will break. Likewise any untoward movement in the stock, or in the machine itself, will break tools. There may be a better way of holding onto your brass stock that will keep it from flexing at a certain point, and messing up the machining operation. It may be that your router just isn't rigid enough to deal with machining metal; that type of machine was primarily designed to cut wood, after all. While some metal-cutting operations might be possible for it, others may not. But try some of the suggestions above before you give up...