Q:

Should vias be used for every GND connection?

When making a two layer board with the bottom layer being a GND plane, should every GND pad for ICs and passives be directly connected to the GND plane using a via, or should I route all of the GND pins of components close to one another together and then use a single via to connect to the GND plane?
EDIT: Having a GND plane on the top would dramatically reduce the number of vias needed. However, this answer to a related question says:

You are right, there is really very little reason to use both the top
  and bottom of a two layer board for ground.
What I usually do for two layer boards is to put as much of the
  interconnects as possible on the top layer. This is where the pins of
  the parts are already anyway, so is the logical layer to use to
  connect them. Unfortunately you usually can't route everything on a
  single layer. Paying attention and thinking carefully about part
  placement will help with this, but in the general case it is not
  possible to route everything in one plane. I then use the bottom plane
  for short "jumpers" only when needed to make the routing work. The
  bottom plane is otherwise ground.

A:

It's more complex than this in a lot of occasions because sensitive analogue ground connections may benefit significantly from a local star-pointing regime in isolation to the ground plane with just one solid via-area to the bottom main ground plane.
This is done to avoid inevitable digital currents in the ground plain creating small unwanted digital noise signals between points on the localized analogue "star point system".
Also routing power directly to the most hungry components is also a good idea then, tee-off for the ground plane. Plenty of times I've seen examples of audio amps oscillating because the power tracks have gone to the chip via input connections despite a decent ground plane being used.
On the other hand, with switching regulators, different tactics are used and the main aim would be to group the components that produce a lot of ground current to one area of copper "land" - here I'm thinking of a buck converter where the input capacitor to the chip, the power ground on the chip, the flyback diode ground and the output capacitor ground are star pointed back to the chip's power ground.
This usually prevents upsetting the feedback point from rattling around and you get the expected result of a low noise and well-regulated output.
I'm sure there are other great examples.

