I am working an ATmega32u4 based custom board. I think I am done with majority of the routing. Now I need to work on the proper shielding of EMF. So I began putting ground pour on the top plane.
Now the question is, I have a couple ground traces (in blue) on the bottom layer, and was wondering if I should also have a ground pour on the bottom layer too?
Ground pour on the top layer is not really doing much. Having a ground pour on the top would make make sense if you didnt have a ground plane on the bottom. So definitely add a ground plane on the bottom and try and keep all routing on the top.
What I would do is have a power pour on the top, and a solid ground plane on the bottom. Now all your return currents have somewhere to go won't fringe across gaps or over other traces.
The ground pour on the top layer (under the microcontroller) does nothing. It has no harm, but it really doesn't have a benefit either (assuming you have a ground plane).
Where there is mostly or entirely a single supply rail, I think it's a bit better to pour ground on one side and Vdd on the other (I usually specify GND on the bottom).
There's not much downside to doing copper pours tied to the rails, provided your rules allow a larger than minimum gap (so manufacturability is not impacted).
I would suggest you go a different route with your pour layout. Put a large ground pour on the bottom with vias from the ground pins down on to it. Then put a VCC pour on the top side that ties all the VCC pins together (remember to choke the AVCC pins if you want to do low noise ADC measurements). Put the decouplers as close as possible to the chip.
The reason for doing this is that it ensures that all the VCC pins have an equal and low impedance path to the power supply and prevents circulating currents in the supply rails/pins. Good supply rail design is as important as managing your ground return path from the perspective of EMC so this can help a lot. As long as the VCC plane is properly decoupled it will also serve as an effective shield for the chip's internal die and leads so you don't lose anything over it not being a ground plane.
Using Different Voltages for Planes in a 2-Layer Board is not suggested. because of it's capacitor behavior.
For Reducing Ground Resistance and better Current flow to Ground, It is Better to use GND pour on BOTH sides and it is recommended to use VIA under ICs to eliminate current circles under smd IC planes and improve circuit stability from the aspect of EMC.
