Bad EMC Advice Recently Spotted on the Internet

Reasons often cited for using a ground pour include:

• Ability to achieve a lower characteristic impedance with a thinner trace. But no space is saved, because maintaining a uniform ground pour on both sides of a trace requires even more space than a wide trace.
• Reduced crosstalk to nearby traces. But copper pours are not a particularly effective or reliable way to reduce crosstalk when the return plane is 0.25 mm or less below the signal traces. Proper lateral spacing of the signal traces achieves the same isolation with no danger of introducing unwanted resonances or coupling signal power to nearby structures through the plane structure.       

Even if the spacing between power and ground pins of the active device happens to match the length of the decoupling capacitor (as often depicted in drawings accompanying this advice), sharing a via connection to the ground plane unnecessarily increases the inductance of ground connection for one or both components. A good rule of thumb for any component operating at high frequencies is that every connection to the ground plane should be done at the component pin (i.e., no ground traces). This minimizes ground bounce in active devices and minimizes the connection inductance of decoupling capacitors.   

In most cases, the spacing between active device power and ground pins is not a good match for the decoupling capacitor length. In those situations, trying to share power and ground via connections forces the designer to use traces to make one or both connections. This adds inductance and potentially interferes with the routing of other signal traces.

Of course, most devices in SOIC, QFP or TSOP packages don't have really low target impedances. For these devices, the capacitor mounting indicated in the drawing is probably fine. However, it is never optimum and certainly not convenient. If high-frequency decoupling is important, then don't rely on guidelines like this. Take the time to get it right for your particular application.   

Faraday cages only work if no conductors penetrate the boundary. Stitching the edges of the ground planes in a circuit board doesn't prevent power from coupling into and out from the traces and vias between the planes. In some situations, stitching around the perimeter of a resonant cavity can actually enhance this coupling.   

Of course, one could argue that radiation from the edges of the cavity formed by the planes is reduced. But the most effective way to reduce edge radiation from a cavity is to stitch the planes together at many points randomly throughout the cavity. This prevents the cavity from resonating and eliminates any significant edge radiation. It is not necessary or desirable to make the majority of these connections around the board's perimeter. 

Another important point is that a ground trace around the board's perimeter on the outer layers does not prevent or reduce radiated emissions from the board. Yes, it can change the field patterns near the edge and, sometimes, this is desirable. On average though, it doesn't reduce the field strength. It just changes the location. Ground traces around the board perimeter should never be the default. They should only be used in specific situations to meet a well-defined goal.     

Since planes and traces labeled "ground" are often the reference voltage for signals leaving the circuit board, it is often necessary to bond them at high frequencies even if they are isolated at low frequencies. This adds cost and takes up space, so current-returns should only be isolated when it is absolutely necessary. The test to determine when isolation is necessary is easy to perform. Multiply the worst-case DC resistance of the shared return path by the maximum low-frequency current in the source circuit. If the resulting voltage would disrupt the operation of the victim circuit, and filtering won't help, then isolation is required.

Note that there are often legitimate safety-related reasons for isolating high-voltage current-returns from system ground. For more information see our tutorial on Grounding.  

The local vs. global decoupling capacitor distinction is important, but a capacitor that provides local decoupling on one board might be used to provide global decoupling on another board. There are no specific properties of the capacitor itself that determine whether it is local or global. 

The term "bulk capacitor" is often used to describe capacitors with a relatively large nominal value that are designed to provide global low-frequency decoupling. High-frequency decoupling is generally provided by ceramic capacitors in small packages. These can be local or global depending on the powerbus geometry and the decoupling strategy employed. For more information, see our article titled Circuit Board Decoupling.