# In a 2 layer PCB with a top layer densely populated, from an EMI & EMC point of view should the ground plane be on top, bottom or both and why?

Suppose I have a 2 layer PCB with the following characteristics:

• Top layer is relatively densely populated by both THT ad SMD components
• Bottom layer has very few traces

Among the following, what is the best option from a theoretical EMI & EMC point of view and why?

1. Top ground plane (copper pour)
2. Bottom ground plane (copper pour)
3. Both top and bottom ground planes with connecting vias

If you think another option not listed might be better please do propose it and explain why.

This is a theoretical question so I don't have a concrete example to show. Feel free to report some practical examples.

My guess is that option 2 would be the best since it allows for the current to choose the path of least resistance and avoid large loops, although maybe depending on the layout option 3 might also be reasonable.

• What makes you think that 1 or 2 is better than 3? Looking at return paths, option 3 is good at least as 1 and 2, since it is both of them... Commented Aug 11, 2019 at 18:09
• If you turn the board upside down top becomes bottom.... what’s your question? Commented Aug 11, 2019 at 18:18
• @Andyaka the point is that one layer is densely populated by components and traces.. (i.e. the top one in this case, but it may be the bottom one as far as the problem is concerned). Commented Aug 11, 2019 at 18:45
• Commented Aug 12, 2019 at 3:27
• Why are you putting your SMDs on top in a mixed tech board? Generally mixed technology assemblies have the SMDs on the bottom (copper) side along with most of the traces; this was originally done to allow for single-pass wave soldering of all the things, but also allows the top (component) side to serve as the ground plane in a two-layer board. Commented Aug 12, 2019 at 4:11

You want as solid ground plane as possible, so you should have the ground on bottom and preferably have no other traces there.

For better copper balance you should also have the copper pours on the top layer to fill the empty spaces. If there isn't any better use for it, connecting the pours to the bottom ground plane with vias is a good choice. Though this has little to no effect on EMC performance.

So from your options the number 3 is the best, but if you are considering only EMC performance the option 2 is practically equally good.

Though, with these questions about 2 layer boards, I always like to remind that nowadays 4 layer boards are cheap, and using 2 layers is recommended only if you have to save every last penny, i.e. you have huge volumes. Otherwise the higher design cost of two layers will outnumber the higher production cost of 4 layers

• +1 for pointing to the 4 layer board possibility. Commented Aug 12, 2019 at 10:07

A copper pour amongst a bunch of component traces is NOT the same as a ground plane. This is because the whole point of a ground plane is to provide currents the shortest, lowest inductance (smallest loop) possible path. This does not happen in a copper pour riddled with component pads and traces since the ground/return currents must take the long route around all the interruptions.

It's just a copper pour so less etchant is required and enure more symmetrical copper balance on both sides of the board (to prevent warping) that has been connected to a fixed potential so that it doesn't float and cause EMI issues.

With this in mind:

Option 1 is not a ground plane at all.

Option 2 is a ground plane.

Option 3 is not two ground plane connected by vias. It's one copper pour on top which has been connected to a ground plane on the bottom via copper pour.

• So are you answering the OP with option 2? Your answer doesn't say... Commented Aug 11, 2019 at 19:08
• @TonyM My point was to tell the OP the facts and have him draw his own conclusion. From an EMI/EMC point of view the difference should not matter between 2 and 3. But that doesn't mean 2 and 3 are the same in all other matters. Commented Aug 11, 2019 at 19:57