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.
There isn't one.
That said, there are some thing I've gathered over time. What you do with the ground planes depends heavily on what you're trying to do. You could be trying to provide low impedance paths, or you could be trying to isolate one area from another, or you could be trying to deal with EMI.
There certainly is a performance penalty for doing it wrong, but you may not really care unless you're dealing either with high frequency circuits or precision analog work. The number of fluctuating bits of the ADC reading with inputs grounded, or the spectral purity of an RF signal as measured by a spectrum analyzer will tell you how wrong you are with any design. It's generally impossible to get it 100% right (datasheet spec) unless you've a system as simple as their test circuits.
The most complicated ground connection problems have to do with RF frequencies, and with signals that are either weak or are passing through traces which are susceptible to EMI coupling in that frequency. At microwave frequencies, a centimeter is enough to make a very effective antenna and mess with things. I remember a professor of mine once told me that when he was working in the industry, they'd leave plenty of points where two grounds could be shorted together, and then an engineer would test each of them one by one to see which gave the best performance. They were working with high frequency (microwave) circuits.
Typically, there's three kinds of 'ground plane' like elements you'd be wanting to short.
Real ground planes. For some reason or the other you've got many of them, and you want to connect them together. This is probably the most common occurrence of the problem in the run of the mill circuits.
Ground / guard traces that are running along with signal lines which may be providing a return path, guarding a high frequency signal or one bound to/from a high impedance source or sink. This could either be to prevent signal leakage or to prevent EMI coupling.
Multiple ground planes which are actually the same ground.
To begin with, you should understand that there isn't really a universal ground, and also that different grounds in the same circuit arent necessarily the same ground. A typical example you'd come across is a datasheet for an ADC that talks about analog and digital grounds. This is to make sure that the oh so noisy digital circuitry doesn't mess with the high resolution ADC you've paid extra for. Different kinds of circuits have different characteristics when it comes to their interaction with the ground. Since digital circuits are characterized by a sudden spike in current at each clock, they tend to be particularly noisy at the clock frequency, and subsequently at harmonics and sub harmonics. Bypassing capacitors are supposed to deal with this, but they rarely do a thorough enough job to get milli or microvolt resolution possible from the ADC using a relatively quieter analog ground with much less switching going on.
Similarly, power grounds tend to be noisy because loads like motors and solenoids tend to be noisy, either because of effects of commutation or things like PWM. The high currents involved and the finite ground resistance (even a chunk of copper has some resistance) means that the transients showing up on the power ground tend to be higher. Sometimes high enough to completely screw up your encoder measurements while controlling a motor for instance.
The goal, then, is to isolate these grounds best you can. That means that they dont overlap, at all. You don't put analog ground on the top and digital ground at the bottom. Everything to do with analog goes with the analog ground, and everything to do with the digital goes with the digital ground in separate areas of the pcb. When the goal is isolation, you connect the planes together at a single point. More than one point can be disasterous since it leads to current loops and hence EMI problems and unintended antennae. The point where the grounds are all shorted is usually referred to as the star ground point of the circuit and is as close as you're going to get to a circuit wide ground. Generally, these should be shorted as close and centrally as possible to a place where the two circuits interact, usually an ADC or DAC. In truely haphazard designs, you'd short them near the supply and pray for the best. This is type 1.
In type 2, you have some sort of a guard trace. If the trace is at ground, then you're probably worried about EMI and not leakage. In the case of leakage, you'd want to drive the guard at close to the signal level. In both these cases, you want the guard to be as low impedance to the source as possible. This means multiple vias dropping down to the ground plane at regular intervals, if the trace is to be grounded.
The third and somewhat less exotic variety, and really is sort of just stating the obvious. This has to do with the vias taking decoupling caps to ground or the random vias shorting top and bottom ground planes. Once you've created a star ground and isolated the different areas, you want each ground to be as uniform as possible. For example, you don't want there to be a measurable potential difference between two corners of analog ground plane. You do this by providing a low impedance path to the star ground - each pin or pad that needs to be grounded goes to the plane which provides it a straight shot to the star ground point. Having the plane has the added advantage of providing a return path under each signal trace, which avoids current loops forming which may act as antennae. In cases where the ground plane must be broken, but you need to have a return path, you would provide an alternate route through another layer. If you have multiple planes with ground in the same area (note:these must be the same ground), periodic vias can help reduce impedance slightly.
Best Answer
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:
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.