How to think about ground planes

[yungman]

yungman, I think the element in need of discussion here is your perception of 'a propagating wave'. Within the planes of a PCB, they may act as a waveguide, but most certainly not a propagating wave. Any source of disturbance will cause an EM wave to propagate out in a guided structure.
EM energy within a waveguide may propagate in several possible modes, maybe even several such modes together. This is a combination of currents and magnetic fields, the magnetic fields, obviously, within the space between planes but the currents are real, physical surface currents on the conductors, and are the current under discussion when it comes to talking about what RF currents are present on planes. (Currents, which I may add, do not simply disappear at the plane edge but are variously reflects and/or are carried over onto the other side of the plane - which might then be a radiating surface if it is the last one in the stack.) First you need to clarify where you are talking about Vcc plane or Vcc trace. I believe:

1) Either way, the di/dt is going to propagate out as TEM wave as the dielectric thickness is most likely much much smaller than the wave length of the highest frequency component. And it propagates.
2) The current on the surface is formed as the consequence of boundary condition of the tangential H wave. It is every bit real current as you can measure it. But it is not what the conventional current that the electrons flow from one end of the wire to the other end. Real electrons move too slow for that. Yes when an EM wave got reflected back, boundary condition again, will create surface current density as if the current reflected back. But again, it is the consequence of the boundary condition even though it is every bit a real current.
3) In the Vcc plane case with no bypass cap or any other low impedance return point, I don't disagree about when current reach the edge of the board, it reflect back as the impedance hit the air boundary which is 377Ω. Part of the EM wave radiate into the air from the edge of the board, but this is not in the scope of the discussion. Most EM wave reflected back and cause the reflection. But with any bypass cap in the board, it provide a low impedance path and the wave patent get complicated.
4)
Your latter point is all-important. A system in which such guided waves do not damp quickly may result in evident interference. A single solitary pulse that damps/dumps its energy straight to ground might [if that is possible], in theory, have an interfering effect but I think it is unlikely in the most part (for what we'd regard as 'consumer' level electronics).
Mirror currents between planes, or a plane and a track, therefore need to dissipate promptly. The interference comes when those mirror currents are inhibited by impedances back to its source (they are currents on the circuit associated with that part). If they do not, then that energy may bounce around for a while, generating interference at any resonant frequencies associated with it bouncing around, which would be a function of the geometry/termination impedances.

I don't think reflection has been in the discussion. It is well know that reflection exist. But I believe there is a big difference between a system with Vcc plane vs Vcc trace. In Vcc trace case all reflection are confined between the Vcc trace and the ground plane right underneath as microstrip lines. EM wave follow the microstrip structure. In the case of Vcc plane that get complicated. Are you trying to say even in the case of Vcc trace, the ripple of the di/dt still ripple out like a stone in the pond? That I cannot agree, but of cause I don't claim I am the expert and know everything, I can just say this within the scope of my knowledge. If you have reference otherwise, I love to read it.Therefore, these surface currents may, harmlessly, appear on either the analogue or digital planes [and also to note - either on +ve or -ve planes] providing those planes have low impedance to source. IF surface currents appear on a plane or a track that is not connected to source by a low impedance - particularly for example a signal track (analogue or digital) that terminates in some form of detector circuit - then that energy in that impromptu waveguide is likely to bounce around for a while with nowhere to sink to.
I agree it will bounce back and fore within the guided structure which is the trace in the Vcc trace case. Most will not bounce out of the guide structure.
A big problem with all this is that at very high frequencies, of the order of board-dimension wavelengths, a 'simple' direct DC low resistance to source may not be enough to prevent resonances. The reason decoupling capacitance might then help might, alternatively [rather than simply regarded as 'high-pass coupling'], be seen to be tuning the frequencies such that the resonances of the board do not match up with frequency content of any likely induced surface currents.

It should not be a surprise, then, that PCB EMC can easily enter the world of the 'dark arts' if the basics have not been got right in the first place, because a failing board might be made to work again with a little nibble of a plane here, a little thicker track there, or a new component value, and although computer simulations have come a long way such subtleties are usually not well-simulated.

I never even talk about reflection and standing wave pattern, I assume it exist. I am more talking about the pattern of the disturbance on the ground plane and nothing more. As this is very important for any trace that run over the disturbance. As long as the traces are not on the path of those disturbance, they can bounce back and fore for all I care.

I believe EM wave radiate out at the edge of the board in the Vcc plane case if it has not been stopped. But I don't think that would be a big problem as the impedance of the two planes guided structure is so much lower than 377Ω that most reflect right back into the board. EM radiation also exist in Vcc trace just like microstrip still radiates into the air as it is not a perfect wave guide and other modes of propagation can exist if the given frequency is high enough.

But as I said, if you have article about this topics, I love to read it. My knowledge is mainly from EM books and RF books. EMC books give practical example where they more worry about interference in signal traces, not about bounce in two copper planes.

In real life case, this bouncing problem in Vcc plane case can mostly be avoided by:

1) Having 0.01uF in parallel with 100pF surface mount cap between the two planes close to the Vcc pin of the IC.
2) Design the stack up so the Vcc and GND plane are right next to each other, separated only by 5mils so they form a distributed cap to make an almost perfect bypass cap to frequency of wave length equal to 10 times the separation which is 50mils!
3) For very fast IC, I even put a copper pour on the side of the IC connect to the Vcc pin on top of the ground plane to create a cap of about 20 to 50pF cap.

I don't believe that this is black magic. It's all about whether you are interested in it and willingness to pursue it. From my experience, a lot of engineers don't like to deal with EMC. To them, it is boring and they rather get on with the circuit design. I am one of the odd balls that fascinated by EMC and I love pcb layout. I remember one of the company I worked for actually hired an EMC expert called Chris Kendell...I am not joking, he actually looked like Santa! He hosted a two day class for us. I can see all the other people were kind of spaced out through out the session, I was about the only one that kept asking question and interacted with him. In another company, when I told the other engineers that I am very into EMC design, all they could say is "Thankyou thankyou!" To me, designing EMC is even more interesting than all the op-amp etc. Even in RF, my interest is mostly on designing filters, matching network using distributed elements so the board looks like a maze of copper line pattern rather than with lump components. I always insisted in laying out my own boards and it is not like those engineers sitting behind the pcb designer and use a stick to point at the screen. I layout out even an eight layer board with mixed signals, that contain processor, switching power supplies circuits, RF transmitter and various op-amps with USB and Firewire. This was done on 4 individual 1.5"X1.5" rigid FR4 with Dupont flex circuit in between them to form one long unit. You don't get more critical than this in EMC and crosstalk point of view. Never once I use cut ground plane. I proof this with real life successful circuit design and layout time after time. I am particularly interested in very dense mixed signal pcb design. And I am talking about laying out pcb from schematic to gerber files ready to sent to board house. This kind of pcb design make op-amp, ADC, DAC circuit design like cake walk.

There is always something new to learn. If you have articles on ripple in two plane setup, I would love to read it. I would like to get it right one day.