I usually compensate with varying router speed as the cut deepens.
In my experience V bits are extremely durable but I also use good bands, Kyocera and Destiny. The flat on the end on mine are around 0.010 and they have cut pretty much everything without chipping out or any issues. On feedrate, really depends on the material but the end of the cuts with v carving will usually be around full engagement and it can have a tendency to chatter if you don’t keep an eye (metals). Lubrication is important in metals, especially the first few passes, helps with the tip sfm issues. Keep in mind you can also use v bits for adaptive cutting, I like a 0.009 opt for two flutes (has to be less that tip flat diameter)
Ballnose -
https://www.iscar.com/ita/Calculators.aspx?units=M#
Lots of good calcs there, thinning based on type of cut and surface quality. Imo ballnose cut quality is mostly on how you leave your finishing stock. Its still a good idea to cam out based on chipload but keep in mind you can push much harder because you aren’t removing that much.
One tip is for finishing it to run square approaches as it can have a certain visual effect. Stepover equal to chipload, minimum 0.001/0.001 and I usually max around 0.005/0.005 depending on desired surface or time limit.
Also when using fusion it can be a good habit of duplicating your adaptive roughing and running it with a ball and rest machining to the previous op. This will get 3d surfaces much closer to final shape and minimize load spikes of going directly from square rough to ball finish.
edit deleted stuff about sfm. Doesn’t really matter here.