Issue link: https://iconnect007.uberflip.com/i/873992
September 2017 • The PCB Design Magazine 49 Figure 3: Amplitude at the far end of planes as input frequency is swept (Source: Eric Bogatin). frequency components, above the bandwidth of the signals. So, how should engineers and PCB designers go about reducing cavity resonance and emis- sions? • A thin dielectric, in the plane cavity, is the most effective way of reducing the peak amplitude of the modal resonance. It reduces spreading inductance and the impedance, of the cavity, and also reduces the resonance peaks by damping the high-frequency components. Thinner plane separation implies less area of equivalent magnetic current at the plane pair edge, or equivalently less local fringing field volume, and therefore lower emissions for a given field strength. • A dielectric material with a high dielectric constant (Dk) should be selected to add more planar capacitance. This is contrary to the typ- ical choice of high-speed materials that require a low Dk. Remember; we are talking about the dielectric embedded between the planes, which has little impact of the signal properties. • The parallel resonant frequencies, of the cavity, can be pushed up above the maximum bandwidth of the signals, by reducing the plane size and by adding stitching vias between (sim- ilar) planes of a cavity. • Where the length of a rectangular plane is a simple multiple of its width, such as 1, 1.5 or 2, the resonant frequencies of the length and width directions will coincide at some frequencies, causing higher-Q peaks—more intense resonances—than usual. So it is best to avoid square planes and simple L:W ratios by choosing ir- rational numbers. • When plane pairs resonate, their emissions come from the fringing fields at the board edg- es. With ground/power plane pairs, edge-fired emissions can be reduced by reducing the plane separation, as described earlier, but this technique can- not generally be used for multi- ple planes. Alternatively, make the power planes slightly smaller (~200 mil) than the GND plane. This modifies the pattern of the fringing fields, pulling them back from the edge, and may help reduce emis- sions to some extent. Optimization of the PDN is a trial and error process. A combination of modifications to di- electric constant and thickness, of the material, together with an adjustment of plane size can usually establish the minimum resonance for a given configuration. Employing AC PDN analy- sis software (Figure 4) allows one to integrate the layer stack and dielectric materials with the PDN and enables visualization of these critical adjustments. If you can't see it, you can't fix it! Points to Remember • Plane pairs, in multilayer PCBs, are essen- tially unterminated transmission lines. • If a transmission line is mismatched or un- terminated, there will be standing waves–ringing. • When return current flows through the impedance of a cavity, between two planes, it generates voltage which can excite the cavity resonances. • Other signal vias, also passing through this cavity, can pick-up this transient voltage as crosstalk. • This cavity noise propagates as standing waves spreading across the entire plane pair. • The slightest amount of coupling, from signal paths, can drive resonances and give rise to long range noise voltages within the cavity. PLANE CAVITY RESONANCE