This is a very complex issue, since it deals with EMI/RFI, ESD, and safety stuff. As you've noticed, there are many ways do handle chassis and digital grounds-- everybody has an opinion and everybody thinks that the other people are wrong. Just so you know, they are all wrong and I'm right. Honest! :)
I've done it several ways, but the way that seems to work best for me is the same way that PC motherboards do it. Every mounting hole on the PCB connects signal gnd (a.k.a. digital ground) directly to the metal chassis through a screw and metal stand-off.
For connectors with a shield, that shield is connected to the metal chassis through as short of a connection as possible. Ideally the connector shield would be touching the chassis, otherwise there would be a mounting screw on the PCB as close to the connector as possible. The idea here is that any noise or static discharge would stay on the shield/chassis and never make it inside the box or onto the PCB. Sometimes that's not possible, so if it does make it to the PCB you want to get it off of the PCB as quickly as possible.
Let me make this clear: For a PCB with connectors, signal GND is connected to the metal case using mounting holes. Chassis GND is connected to the metal case using mounting holes. Chassis GND and Signal GND are NOT connected together on the PCB, but instead use the metal case for that connection.
The metal chassis is then eventually connected to the GND pin on the 3-prong AC power connector, NOT the neutral pin. There are more safety issues when we're talking about 2-prong AC power connectors-- and you'll have to look those up as I'm not as well versed in those regulations/laws.
Tie them together at a single point with a 0 Ohm resistor near the power supply
Don't do that. Doing this would assure that any noise on the cable has to travel THROUGH your circuit to get to GND. This could disrupt your circuit. The reason for the 0-Ohm resistor is because this doesn't always work and having the resistor there gives you an easy way to remove the connection or replace the resistor with a cap.
Tie them together with a single 0.01uF/2kV capacitor at near the power supply
Don't do that. This is a variation of the 0-ohm resistor thing. Same idea, but the thought is that the cap will allow AC signals to pass but not DC. Seems silly to me, as you want DC (or at least 60 Hz) signals to pass so that the circuit breaker will pop if there was a bad failure.
Tie them together with a 1M resistor and a 0.1uF capacitor in parallel
Don't do that. The problem with the previous "solution" is that the chassis is now floating, relative to GND, and could collect a charge enough to cause minor issues. The 1M ohm resistor is supposed to prevent that. Otherwise this is identical to the previous solution.
Short them together with a 0 Ohm resistor and a 0.1uF capacitor in parallel
Don't do that. If there is a 0 Ohm resistor, why bother with the cap? This is just a variation on the others, but with more things on the PCB to allow you to change things up until it works.
Tie them together with multiple 0.01uF capacitors in parallel near the I/O
Closer. Near the I/O is better than near the power connector, as noise wouldn't travel through the circuit. Multiple caps are used to reduce the impedance and to connect things where it counts. But this is not as good as what I do.
Short them together directly via the mounting holes on the PCB
As mentioned, I like this approach. Very low impedance, everywhere.
Tie them together with capacitors between digital GND and the mounting holes
Not as good as just shorting them together, since the impedance is higher and you're blocking DC.
Tie them together via multiple low inductance connections near the I/O connectors
Variations on the same thing. Might as well call the "multiple low inductance connections" things like "ground planes" and "mounting holes"
Leave them totally isolated (not connected together anywhere)
This is basically what is done when you don't have a metal chassis (like, an all plastic enclosure). This gets tricky and requires careful circuit design and PCB layout to do right, and still pass all EMI regulatory testing. It can be done, but as I said, it's tricky.
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.
Best Answer
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.