Does it make sense to place ground plane "island" within power plane layer for return paths of traces on adjacent layers?

Question

I have the following layer stack up: Layer 1: Components and traces Layer 2: Dedicated ground plane Layer 3: Power plane Layer 4: Additional traces as needed

I have read (I'm a beginner at circuit design) that it is best that traces have a ground plane either on the layer immediately below or above said traces for return path. However, given I have some traces on layer 4, the layer immediately above these traces would be my power plane, not my ground plane. Would it then make sense to place a relatively small ground plane island within the greater power plane (layer 3) that corresponds to the location of the traces on layer 4 such that there is a ground plane directly above these traces? And then stitch this ground plane island to my dedicated ground plane (layer 2) using vias? Within the attached image, you will find that I have attempted to create such a small island directly beneath the feedback traces for my buck converter (stitching vias not yet added). Would this be beneficial? Is it not required for these short traces (app. 15mm in length)? I've already included a ground plane for signal trace return paths within the power plane layer (seen in the second image), however this seems more straightforward as my power plane doesn't need to be in the top portion of my PCB in the first place. Thank you.

Answer 1

This is going to be a "it depends" situation. Specifically, what the circuit is actually doing: the currents involved, the frequencies, analog and digital coupling.

First rule of thumb:

Don't break the power plane unless you can objectively justify why you are doing that

Without knowing much about your circuit, what I'm seeing, is that you are going to create a parasitic antennae. This is bad for two reasons: one it will radiate interference. This will be fun during compliance testing. And two, it will also be susceptible to external interference.

Fortunately, fixing one of these problems fixes both at the same time. The whole philosophies and theories behind ground planes is rooted in high frequency current return paths - AC current takes the path of least impendence NOT necessarily the path of least resistance. This is the whole idea of having a ground path (the ground plane) under the trace - it minimizes the loop the current takes thus its inductance. Lower inductance is therefore lower impedance at AC. And Impendence is basically the resistance to (high-frequency) AC.

Having said all that, just be mindful of the AC return paths and you should be good. With the little info I know about your circuit, and my experience, can get this done with a solid plane. Which is generally ideal.

Reasons for breaking the plane: You need high voltage isolation (creepage/clearance). Or, you need to isolate sensitive circuits from ground bounce. Both cases require you know what you are doing, but the latter really needs thought put into before you make things worse. Like way worse.

Answer 2

This is in reference to your previous question? What should I do when clearance boundaries overlap with SMD pins?

Feedback traces don't need any special treatment. Definitely don't cut up a plane (a far worse sin, not something to be done lightly and unknowingly) when signal bandwidth is low -- these will be MHz if that; even loose wires will suffice.

Likely more important is avoiding direct coupling from the switching node to these traces. This is easily avoided by putting them (DW and FBs) in different locations, or on opposite sides. As-is, you have both, and I gather, a reference plane of VOUT, which is likely quiet enough not to be a problem.