Should I do a ground copper pour on a 4-layer PCB in order to shorten return current paths?

Question

I'm designing a 4-layer PCB with the SIGNAL/GND/POWER/SIGNAL stackup.

Since I have a dedicated ground plane layer, I've decided not to pour ground connected copper on the top and bottom signal layers, as I've read in other topics on the exchange that pouring ground on these external signal layers while already having a dedicated ground plane layer will bring little to no benefit, and might create EMI problems.

But, here's the thing : I have I2S traces running at roughly 12 Mhz, as well as some SD card interface traces which run at 50 MHz. I believe the rise times for these are gonna be pretty short, so the signals on these are (if I'm not wrong) going to want to follow the trace path for their return current, not the shortest path.

And some of these signals go through vias between the 2 signal layers. When changing layer, the return current is gonna seek for the nearest path to the reference plane, which would be, for example, the nearest capacitor ground via or MCU ground pin via. Again, my knowledge of grounding is limited but I believe that this would create a ground loop. My board is audio oriented and I wouldn't want to hear the induced "hum" sound in the audio output...

Pouring copper connected to the ground plane and "sprinkling" some ground vias in this copper pour area would allow for short paths to ground pretty much everywhere on the top/bottom layers, reducing the size of ground loops, but again as I said in the first paragraph some say that it can bring EMI problems (such as the pour acting as an antenna).

Should I pour ground on the top and bottom layers or not ? Answers on similar questions had a vague conclusion, some saying yes, some saying it is not necesary but can be done, some saying no, don't do it...

Answer 1

It is unlikely that pouring ground on top and bottom will create EMI problems as long as you make sure there are no large, via-less islands of GND copper on the top and bottom. You have to use vias to connect your GND pour to GND plane. If there are large sections of pour that cannot be stitched to the GND plane with vias, it is better to delete those sections.

On boards with a lot of unused space on top and bottom, copper pours can be a pretty good idea with very little, if any downside. Probably the only downside is that once you put in the copper pours, it may be difficult to continue modifying the PCB design. You may have to delete all the pours if you do any re-routing, because otherwise they are in the way. Typically, adding copper pours is done after all other aspects of the design are complete.

Changing layers

Do you also have a VCC plane? High speed signals should be routed so that they are close to a plane layer. The closest plane layer to a signal is called the "reference plane" for that signal. Generally it is OK to use VCC as a reference plane. When you run a signal from top to bottom on a four layer board, that is called a change of reference plane. It is a good idea to put some small ceramic capacitors near any place where you have a high speed signal change reference planes. The capacitor is connected to the two reference planes and guarantees a low impedance path for AC current between the planes.

Changes of reference are often done and should not create a problem for you. Some higher speed busses (such as the various DDR's) may require that certain signals be routed adjacent to certain reference planes with no vias to other layers. But you should not have that problem.

Coupling of copper traces to surrounding GND copper on the same plane is relatively weak compared to the coupling to a plane layer above or below the trace. So putting copper pour on top and bottom will only have modest impact on signal integrity. But that impact is generally favorable from the perspective of minimizing radiated emissions, in my experience.