Thermal pads under IC, how to place vias without soldermask / Decoupling question
TI recommends using solder-mask-defined thermal pads without solder mask around the thermal vias. Solder going though the holes and causing voids (not shorts) is said to not be a problem if the via hole diameter is kept to 0.3mm or less. Spacing of 1mm is suggested, and of course the vias should not have thermal reliefs. 



Putting vias just in the corners would degrade the thermal performance. 

If cost is no object, some fabs can plug the thermal via holes with copper. 

If the pad is actually used to carry significant current then the usual  considerations apply, you can split the plane or do other things to control current flow, but it is not usually necessary, especially on a mostly digital board. You really can consider all the thermal vias a single connection to the ground plane for most practical purposes- an exception might be if you had some insanely sensitive amplifier very close to the thermal pad so that it caused voltage gradients in the ground plane- but that would be bad layout practice to have such things too close to each other and without some kind of isolation moat etc.