on the subject of copper pours : those can be actually very ineffective and cause of trouble... as frequency increases the return path is flowing right beneath the coupled source trace. ( for low frequencies the electrons kinda flow wherever they like in the ground plane , for high frequencies they follow the shape of the trace above...)
here is a potential problem on a multilayer board :
top layer trace in horizontal direction
inner one is a ground plane
inner two is anotehr signal plane where there is again a trace in horizontal direction..
due to the tight coupling there now is intermodulation betwene the two signals... it happens because of the ground plane !
so , for signals contaiting high frequencies : DO NOT run them on top of each other shielde by a groundplane. you still need to cross at 90 degree angles. simply because the return current will cause intermodulation in the ground ( ground bounce )
i have sene designs where a bus transceive was routed with half the traces above the ground plane , half below the ground plane... and all the return currents nicely intermodulated in the plane itself.. causing havoc.
you always need to analyze your current loops. currents should never share a common pathway ( sometimes you cannot avoid , and sometimes you can ). that is the principle between having 'analog and 'digital' grounds. you keep the noise in the digital ground. digital circuits have really good noise margin ( don't overdo it though
)
the analog ground is anothe rmatter then. and you can only use a piece of copper as a shield if there is NO current flowing in it.
other fun tidbits : planes canradiate tremendously. example : 4 layer board : inner two layers are a power and a ground.
parts are concentrated in the center. with large 'open area's' towards the edge of the board.. this is effectively a dipole.... two pieces of copper sticking out with noewhere for the current to return... radiation galore !
so , if you have large open spaces on a board : create a return path : slap a few capacitors close to the edge so any ac current (dc current does not radiate) is shunted through the caps and the dipole is effetively shorted.
we had this problem in a Co rack. one of the boards was a diagnostic card. since all boards are the same size this board was mainly empty apart from a littel lump of parts( some cpu and assorted parts ) close to the back end card connector ( these boards slide in large 24 inch telecoms racks. i was working on ADSL central office boards at the time )
only a few signals travel from the far end to the front. some led's and an rs232 connector.
this board was radiating as hell... we thought its the rs232 , its the leds... tried everything. ferrite beads , whatever.
until we simply placed a few 10nF caps at the front of the board. that solved the problem. the planes were simply long antennas radiating .
So her : remove the plane under the void area's or shunt it with a cap.