Issue link: https://iconnect007.uberflip.com/i/1295812
OCTOBER 2020 I DESIGN007 MAGAZINE 21 why all return planes should be GND layers so that stitching vias between GND planes can be placed adjacent to each signal via transition to minimize the possibility of exciting the cavity resonance. Cavity resonances are (at first) a signal integrity issue, but the amplification of cav- ity resonance excited by fast rise time sig- nals at high frequencies can also contribute to electromagnetic emissions. The frequency components of the voltage noise are related to the peak impedance of the cavity and the frequency components of the return currents. In any complex system, with typical intercon- nect density, avoiding signal layer transitions is not practicable and is an issue that design- ers must live with. However, one can learn to avoid injecting excessive noise into the cavity or at least minimize the impact. Figure 4 gives an example of a signal trace on the top microstrip layer routed outside the reference plane area. I see this all the time when I analyze PCBs. The signal path is very close to the edge of the PCB, and the refer- ence planes are not located directly under the trace to provide full field coverage. The electric fields (blue) tend to couple to the plane edges, whereas the magnetic fields (red) radiate out- ward omnidirectionally. The fringing effect creates a very "hot" area and will radiate and possibly create coupling issues to nearby cir- cuits, cables, and slots in enclosures. Figure 5 illustrates the cross-section on a microstrip trace, and its associated plane return current distribution (red). Where the electric fields (blue) are more tightly coupled to the plane directly below the trace, the return cur- rent also exhibits tighter coupling. But where the field spreads out from the trace, the larger loop area between the signal and the return current path increases the inductance. Return current tends to couple to the sig- nal conductor, falling off in intensity, with the square of increased distance. A stripline (inner layer) return current distribution is narrower with the fields more intense above and below the trace. The electric field spreads out to approximately three times the width of the trace (on both sides), so it is important to ensure there is enough plane coverage to pre- vent radiation. To reduce emissions and increase immunity, when routing a PCB, try to avoid positioning critical signals close to the edge of the board. This creates a more robust system for electro- magnetic compatibility. There are various approaches pertaining to reducing radiation edge effects from the PCB. In many cases, energy can be reflected, pos- sibly creating additional internal cavity reso- nance effects and coupling to internal vias, also resulting in increased radiation. When plane pairs resonate, their emissions come from the fringing fields at the board edges. With ground/power plane pairs, edge-fired emis- sions can be reduced by reducing the plane separation and lowering the AC impedance. Alternatively, make the power planes slightly smaller (~200 mils) than the GND plane. This modifies the pattern of the fringing fields, pull- ing them back from the edge, and may help reduce emissions to some extent. Figure 4: Trace routed outside the reference plane area (simulated in HyperLynx). Figure 5: Microstrip plane return current distribution.