As someone who's been doing some micro-engraving, a potato-quality proof-pic and then a few thoughts:
First, specific tips regarding not breaking tiny tools:
You need to cut with the correct chip-load on the cutter for the sake of longevity, rather than maximum material removal rates, within the limitations of the Nomad/Shapeoko, so you have to set your feeds & speeds based on the diameter of the tool, and the number of flutes.
The guidelines for this are:
Start with feed-per-tooth values of tool diameter x 0.005, so on a 1/64th tool that's ~0.00008in, rounding up. That means at 10krpm your feedrate is: 0.00008 x 10,000 (spindle speed) x 2 (flute count) = 1.6 IPM
Yes, I know that seems silly slow. So only use the teeny weeny tool where you absolutely need to.
If you're feeling ballsy, you could increase your multiplier to 0.8% instead of 0.5% of tool diameter, and in ideal milling conditions I've seen recommendations going as high as 2% for aluminum, so test at your own discretion.
Depth of cut on tiny tools should be no more than 100% of the diameter of the tool when adaptive cutting, and 50% when slotting at the given above calculated feed-rate.
If you want to cut things faster, you're going to need a higher-speed spindle. If wishes were spindles, I'd have an NSK 3060 series with quick-change tool-holders that can run at 60krpm....
Now general suggestions:
1) Use Fusion360 & the integrated cam and use adaptive clearing path strategies as much as possible. You really want to be careful not to put too much lateral force on the tool (because snap). If you do this and have lateral engagement of 30-40% of tool diameter you'll be prolonging tool-life. Pay attention to chip-thinning though—if you use a lesser step-over, you can increase your feed per tooth to keep chip size consistent. Harvey Tool has a good blog post about chip thinning worth a read.
2) Machine in C360 brass if your application allows it—it's a leaded alloy, which sometimes does and sometimes doesn't matter. It's often called "free machining" brass, because it cuts well.
3) A little coolant helps a lot to preserve tool life. For brass you can use soy-based oils.
4) I'd recommend using 3-flute cutters as you're spindle-speed limited and at that size of cutter and 2 flutes will take 50% longer, meaning you've got to run the machine at that size that much longer. I wouldn't recommend higher flute-counts due to evacuation and chip-thinning issues in tight pockets.
5) I assume you're only using the 1/64th tool for finishing passes, and doing the bulk of the work with other tools, right? this piece I was working on went through 4 tools in the end on my Shapeoko3: 1/8th 2-flute, 1/16th 3-flute, 1/32 2-flute, and then a 90° v-engrave taking a few passes to get down to proper engraving depth.