PCB Layout - Ground Plane Return Path

Question

I am designing a 4 layer PCB with power planes and a ground plane, with mixed voltage signals and high currents. I have two possible isolated ground plane configurations, and I am wondering which would be better in terms of reducing EMI and noise. The logic circuit includes a microcontroller with ADCs, so I don't want the high current ground to interfere with the analog signals. The power section drives a motor, so the ground there will be very noisy. Here are my power planes.

One of my ground plane configurations forces the logic level ground return path to follow the same path as the supply path to the regulator. For this configuration, I am assuming that it is better for the logic ground currents to return to the regulator's ground pin. The advantages I can see are that the current will return in the same path as the supply, so there is no inductance created by current loops. The isolation from the high current ground also seems to be better (not sure if this is true).

The other ground plane configuration allows for a more direct current path from the logic ground to the supply ground for minimal resistance (instead of the regulator's ground), but it creates a larger current loop. It also seems to be less isolated from the high current ground (again not sure about this).

Which ground plane configuration would be better for EMI and signal integrity, and why? In general, if I have a regulator, should the ground return path be optimized to return to the ground of the regulator (and then back to the supply ground), or straight back to the supply ground?

Answer 1

This sounds odd -- but try not partitioning your ground plane. Instead, make sure that the components and traces for a given subsystem (logic, analog, digital) all stay in their respective areas instead of "spilling over" with high-speed digital traces running through analog circuits for instance. Ground plane currents will take the lowest impedance path back to the source, which at high frequencies follows the trace they are the return for.

Answer 2

If your goal is reducing EMI and noise you probably don't need a split ground plane. The split plane is typically done when you have sensitive analog devices (e.g. ADCs) and you want them to have a clean ground reference. It's better to avoid partitioning the ground plane.

High frequency return currents will follow a reference plane – they might use a power plane for return, especially for traces on whatever side of the board is closer to the power plane (often the bottom layer in 4-layer boards). For this reason it's important to make sure high frequency digital traces follow a continuous reference plane. If you partition ground, you must ensure no trace ever crosses the gap, making the routing harder as the board gets more constrained.

If a trace cross a partition in the ground plane, the return current will go the long way around. If a trace crosses a gap between power planes and is using the power plane to return, it may go on a long tour of your board to find a high frequency route between two disconnected power planes. See my answer here on high frequency routing.

As usual Henry Ott has good advice as well.