Can return currents travelling through ground plane be coupled to signal lanes

Question

In a PCB with proper stack up like sig-gnd-sig-gnd etc. I was wondering if return currents going back to source (let's say battery) through proper ground planes can be coupled to signal lines above and below? This seems not possible because ground plane has the smallest resistance and the return currents may not find a better way to the source, reactance between ground plane and signal lines may be too high for currents to choose or if they jump to signal lines, they may not find a way to ground as well. I am quite confused about grounding, shielding and return currents. Can you give me some direction on how I can master and understand these concepts?

Answer 1

You mention a stackup of Sig/Ret/Sig/Ret.

So let's consider a signal trace on L1. A high frequency current will generate a return current in conductors that are immediately nearby. As the trace is laid out over a plane, most of this current will be in the plane underneath the trace. No current will be induced in lower layers, because L2 plane shields these. However return currents can be induced in other L1 conductors that are close by. Therefore, you can find various rules as how tightly to space signal traces on L1. E.g. there is a (handwaving) "3-H" rule, which says the gap between signal traces should be at least 3 times the dielectric thickness between L1 and L2. More sensitive signals (like precision analog stuff) may require more lateral spacing.

Now for the case of a low frequency current in a L1 trace, the return current will spread across the entire return node. If that node is the "ground" node and both planes are ground, then return current will spread across both planes. Luckily DC current do not induce parasitic voltages into other traces, but there is a range of frequencies (around the audio range typically) where return current already does spread and the frequency is high enough for it to already affect other traces.

So if you need to pass around low frequency AC signal, e.g. in audio, and you do care about integrity and precision, it is mandatory to use dedicated return traces for these signals, to keep them in specific places. Note, that these dedicates traces do turn the signal into a differential signal. This goes to show that "single-ended precision signals" do not exist.

Answer 2

Can you give me some direction on how I can master and understand these concepts?

The whole point about a GND plane is that a particular signal's return current (flowing in the GND plane) must interact with the signal's forward current passing down a track on the signal layer.

That interaction ensures that the physical path taken by the forward current is "copied" by the return current in the GND plane. This is a natural phenomena and is sometimes called proximity effect. It boils down to the fact that a GND plane signal return current will tend to travel down the shortest electrical route and, that's not just the shortest ohmic route but the shortest inductive route. That route is directly below the signal trace.

In other words, the return current attempts to shorten the inductive path and, as a by-product, it emits less interference and is less susceptible to contamination from other signals.

So, despite having the whole of the GND plane available, a signal return current having AC characteristics will tend to follow the same path as the forward current. Loop inductance is minimized.

This implies that both forward and return current take a route that both minimizes EMI generated and, reduces the potential for EMI received. Therefore, signal return currents are less likely to interfere with other signal lines than you might think. I'm not saying there is no interference (because there can be) but, I am saying it's not as big-a-deal as I suspect you think it is. This is what a GND plane brings to the party.