Hi Dave,

Taking each point in turn:

#1 Only ever used a 3mm carbide, nothing smaller. I think it would snap on my machine at those rates but possibly depends on how rigid your machine is.

#2 DOC for 3mm carbide has been about 0.3mm for me. It's quite possible I'm shortening it's life doing this but it works well but I only use it occasionally and it's still going strong.

#3 I'd use 4 holding tabs. Now in Vectric Cut2D the thickness is relative to the bottom of the cut. For that cut I would ask for 6mm total depth to make sure it went right through. Therefore 0.5mm tab would not actually hold the part and I'd need to input a tab depth of 1.5mm to get 0.5mm. I think I'd go for at least 2mm tab to make sure it did not vibrate on the last finish pass.

#4 If the part is complex (long run time, chance of an e-stop or other problem) then I'd do a roughing cut leaving 0.1mm for the outside as a finish cut.

#5 I would not attempt all that with 2mm cutter! Use 6mm or 8mm if possible to cut most of it out, then finish pass with the same bit, then go in again with the 2mm for the detail.

#6 Don't leave the oval hole as a free cut. When the cutter gets to the end the oval part will jam against the bit and mark the work, then fly across the workshop. AMHIK.
You can use tabs, but it is a pain to clean up by hand inside there, so better still is "pocket" it out (turn it all to swarf).

As a strategy I think I would:
Spot all the holes (leave finishing for the drill press)
Pocket out all the internal holes and slots (i.e. not an internal profile)
Rough profile the exterior with 6 or 8mm carbide, leaving 0.1mm
Finish profile the exterior with 6 or 8mm carbide in one full depth pass (but still use same tabs as when roughing)
Switch to 2mm cutter and profile the outside again to get the detail then profile the inside of the pockets
Cut away the tabs and tidy up the edges by hand