I’m designing a 2-layer PCB where the top layer is densely packed with through-hole and surface-mount components, while the bottom layer has minimal routing. From an EMI/EMC perspective, which ground plane strategy would be theoretically optimal:
Ground plane (copper pour) on the top layer only
Ground plane (copper pour) on the bottom layer only
Ground planes on both layers with stitching vias
I believe option 2 might be superior since it provides low-impedance return paths and minimizes current loop areas, though option 3 could be beneficial depending on the specific layout. If there’s a better approach I haven’t considered, I’d appreciate your suggestions.
For best results, you want as solid a ground plane as possible. That means dedicating the bottom layer to ground and avoiding routing on it whenever you can.
To maintain copper balance, it’s also a good idea to add copper pours on the top layer to fill unused areas. If those pours don’t serve another purpose, you can connect them to the bottom ground plane using stitching vias, it won’t make a huge difference in EMI/EMC performance, but it’s still good practice for mechanical and thermal balance.
Between your listed options, #3 (ground planes on both layers with stitching vias) is technically the best overall. However, in terms of pure EMC performance, #2 (ground on the bottom only) is almost just as effective.
And as a side note: unless you’re working in very high volumes or under tight cost constraints, it’s worth considering a 4-layer board. They’re much more affordable nowadays and significantly simplify achieving good EMC performance and layout quality.
A copper pour surrounded by component pads and traces is not the same as a true ground plane. The purpose of a ground plane is to give return currents the shortest, lowest-inductance path possible, something that’s impossible when the copper area is heavily interrupted by footprints and routing.
In a dense top layer, the “ground pour” there is mostly just leftover copper connected to ground. Its main benefits are copper balance (to prevent board warping) and reducing etchant usage, not providing a low-impedance return path. Connecting it to the real ground plane helps ensure it doesn’t float and radiate noise, but it won’t act as a functional plane. With that in mind:
Option 1: Not a ground plane at all — just a decorative pour with limited electrical benefit.
Option 2: A true ground plane, provided the bottom layer is kept as continuous as possible.
Option 3: Functionally the same as Option 2 for EMI/EMC purposes; the top pour adds little beyond copper balance and thermal reasons.
So, from an EMI/EMC standpoint, Option 2 is optimal. If you have open areas on the top layer, you can pour copper there and tie it to ground with vias, it won’t hurt, but don’t expect it to improve EMC significantly.
Basically I agree with Will. If you add copper pour on layer 1, be careful because if, for any reason, a copper island is created, not connected to layer 2, then you will get more issues than benefits. If layer 1 is quite crowded I think option 2 is the best option.
There already are a collection of good replies to this thread. Two layer PCBs can be very hard to get right to the point where they pass the EMC standards. Of the options listed 2 is the easy one to go for, though 3 could be fractionally better if done well.
But if the best application of approach 2 or 3 is not quite good enough to meet the EMC standards, you may find that reducing the PCB thickness could get a good enough improvement to get a pass. This is because the thickness of 1.6mm has become seen as the standard thickness to use, but a 1mm or even 0.5mm thick board will improve the coupling between layers and if it is just a few dB that you need, this could be the simple answer. In the old days there used to be things called PCMCIA cards and their standard thickness was 0.5mm, in which both 2-layer and 4-layer boards were often made.