Electronic – Combining ground traces and ground planes using the same connection

2) I highly recommend AGAINST cutting ground anywhere near high-speed signals. Stray capacitance really doesn't have too much of an effect on digital electronics. Usually stray capacitance kills you when it acts to create a parasitic filter at the input of an op amp.

In fact, it is highly recommended to run your high-speed signals directly overtop of an unbroken ground plane; this is called a "microstrip". The reason is that high frequency current follows the path of least inductance. With a ground plane, this path will be a mirror image of the signal trace. This minimizes the size of the loop, which in turn minimizes radiated EMI.

A very striking example of this can be seen on Dr. Howard Johnson's web site. See figures 8 and 9 for an example of high-frequency current taking the path of least inductance. (in case you didn't know, Dr. Johnson is an authority on signal integrity, author of the much lauded "High-Speed Digital Design: A Handbook of Black Magic")

It's important to note that any cuts in the ground plane underneath one of these high-speed digital signals will increase the size of the loop because the return current must take a detour around your cutout, which leads to increased emissions as well. You want a totally unbroken plane underneath all your digital signals. It's also important to note that the power plane is also a reference plane just like the ground plane, and from a high-frequency perspective these two planes are connected via bypass capacitors, so you can consider a high-frequency return current to "jump" planes near the caps.

3) If you have a good ground plane, there's pretty much no reason to use a guard trace. The exception would be the op amp I mentioned earlier, because you may have cut the ground plane underneath it. But you still need to worry about the parasitic capacitance of a guard trace. Once again, Dr. Johnson is here to help with pretty pictures.

4.1) I believe that multiple small vias will have better inductance properties since they are in parallel, versus one large via taking up approximately the same amount of space. Unfortunately I cannot remember what I read that led me to believe this. I think it's because inductance of a via is linearly inversely proportional to radius, but the area of the via is quadratically directly proportional to the radius. (source: Dr. Johnson again) Make the via radius 2x bigger, and it has half the inductance but takes up 4x as much area.

The layout you showed looks like what's called copper-backed coplanar waveguide (CBCPW). That means the ground return for the waveguide is not just in the coplanar grounds (the ground fills on the same layer as the signal traces) but also in the plane layer immediately "below" the signal layer. This structure is fairly esoteric, in the sense that I've only seen it used in digital systems when data rates exceed 20 Gb/s.

I found what looks like a reasonable discussion on the differences between CBCPW and microstrip in a Microwave Journal article by Rogers Corp engineers.

This article shows that the CBCPW has lower loss than microstrip at frequencies where radiation loss becomes important in the microstrip, roughly from 25 GHz and up, which explains why CBCPW is not widely used at lower frequencies.

Addressing your question, the article points out some special requirements for grounding vias in CBCPW structures:

For proper grounding, CBCPW circuits employ vias to connect the top-layer coplanar ground planes and the bottom-layer ground plane. The placement of these vias can be critical for achieving the desired impedance and loss characteristics, as well as for suppressing parasitic wave modes.

This basically means that without frequent stitching vias between the coplanar ground and the backing ground, power could be transferred to undesired propagation modes, which would cause either excess insertion loss or strong dispersion in the transmission line characteristics.