Using polygon pours for small signals in PCB design
I use Altium for layout and I try to avoid the polygons wherever I can. First, they are cumbersome to create, second you have to take care of the pour order and third, they obscure view of the other layers. I don't know if other layout tools have the same problems though. I use internal planes for boards with 4+ layer count that I want to have GND and/or power planes, which are much easier to create and give you a transparent view. Also as the others pointed out, mismatch of thermal drain between the pads of chip resistors and capacitors can lead to tombstoning in reflow processes. 

Also, for routing high speed signals there are many guidelines which you can find on the web. These guidelines depend on the type of the signal and frequency. I would assume satisfying those requirements (minimal crosstalk, impedance and/or length matching, etc) with using polygons all the time would be very difficult if not impossible. My preference is using polygons only when necessary, which as you have pointed out if there is a need for maximizing copper area for an SMPS circuit power line, etc. 

Regarding the GND pour creeping between the pads, I would also avoid that. The reason is that those copper areas will probably not be covered with soldermask for 0402 case, so the solder from the pads could creep to the bare copper and create shorts. For bigger components this may not be a problem. However, you should always take clearance and creepage rules into account based on the voltage differential between different nets, in addition to soldermask expansion and manufacturing processes. Solder creeping is also an issue with vias that are placed to close to the pads. If there is no soldermask between a via and a pad that are placed very close, the solder can fill the via during soldering process and then you will have a bad solder connection for that pad.

Also I noticed a couple of acute angles in your design. These also should be avoided for the long term reliability of the design. The reason is that the acute angles can trap the solution used to etch the traces, and that can lead to disconnection in the long term.