Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It only takes a minute to sign up.
Sign up to join this community
In a multilayer board with a GND plane directly under the top layer, does adding a copper pour to the top layer give extra value in terms of reducing crosstalk and EMI? If all signal traces already have an adjacent GND plane, can a copper pour provide additional benefit?
(Assuming that stitching vias are used appropriately, and there are no unconnected copper islands to act as antennas).
Adding copper between signals to reduce crosstalk only works if the copper is effectively grounded at the frequency of interest. For audio, it can potentially help. But for high speed clocks, it will likely make the crosstalk worse since the fill copper has high impedance to GND (relatively speaking).
To reduce crosstalk, focus on leaving lots of space around the potential aggressor signals such as clocks. The worst thing you can do is route them along side each other or directly over/under without a ground plane between.
Think of it this way. Two traces next to each other act as terminals of a capacitor. The gap between them is the dielectric. A wider gap means less capacitance, and therefore less crosstalk. Adding copper to the gap has the same effect as using a thinner gap (more crosstalk), unless that copper is grounded well. And at high frequencies, it is just not possible to ground that copper well.
So there may be good reasons to flood the outer layers with GND copper. It is often done. But adding copper between aggressor and victim signals will probably not reduce crosstalk. Use a large gap instead.
In a multilayer board with a GND plane directly under the top layer, does adding a copper pour to the top layer give extra value in terms of reducing crosstalk and EMI? If all signal traces already have an adjacent GND plane, can a copper pour provide additional benefit?
Can a Faraday cage work just as effectively with one wall open?
The picture shows that devices are protected from an external field in all directions i.e. the more sides of the "cage" you have, the more complete the protection.
It works both ways and not just against high voltages (incoming). Local emissions (outgoing) of EMI are significantly reduced when using a "full cage" and this is what happens when you fill the "gaps" up on a PCB.
Consider also the "patch" antenna: -
It uses a ground plane and the top copper emits EM waves. It relies on the dimensions to the bottom ground plane and the width of the top copper to obtain resonance at just the right frequency. If that top-copper is surrounded by grounding copper then its effect is disrupted greatly.
Thin copper (35 micron is the standard, or 1.4 mils) will be fully penetrated, thus offer NO SHIELDING to either displacement currents of E-fields or to the eddy currents of H-fields, for edgerates (rise times) of 1uS.
Having an extra layer should provide another 6dB attenuation, because the I*R drop in the foil will be cut in half.
Depending on board stackup the top copper pour could potentially provide the smallest loop area for signals existing only on that layer. For example, if you had a thick 4 layer board and the inner layers were spaced close to each other but far from the outer layers.
