Reader Steve Purcell writes:
I've been using power and ground copper pours on every board I've done since taking a signal-integrity course years ago from another individual. I wonder whether they are helping me. I have a PMC card design that is failing, and I'm beginning to suspect the PCI trace impedance, because I can't find any other problems. Could the power and ground pours have changed the impedance to the point where the circuit is no longer functional? Do I really need these pours if I already have solid power and ground planes?
The "poured-ground" (more commonly called a "ground-fill") technique is useful on two-layer boards that lack solid reference planes. It reduces crosstalk due to electric-field (capacitive) coupling. Ground fill works particularly well in high-impedance analog designs that lack solid planes. For example, your VCR undoubtedly uses the ground-fill and guard-trace concepts to reduce coupling between the digital and analog sections.
To see how ground fill works, imagine the electric-field lines spewing forth from an active trace:
- Wherever these lines terminate, they induce currents. (This concept is the "displacement-current" idea that Maxwell's equations so elegantly describe.)
- Electric-field lines generally terminate on the nearest metallic object.
- If the nearest metallic object is another trace, the electric-field lines induce currents (crosstalk) on that trace (Figure 1a).
- Hanging a lot of grounded metal in the region between the aggressor and the victim provides many opportunities for the electric-field lines to terminate on the grounded metal, instead of on your victim circuit—thus reducing crosstalk (Figure 1b).
On a multilayer board with solid power and ground planes, the ground fill serves no function. You already filled the entire region between aggressor and victim with continuous, solid planes of metal stretching everywhere. The ground fill simply raises that same, grounded metal up one layer to the surface of the board, instead of leaving it down on layer 2 or 3—an almost meaningless change in geometry.
In the multilayer digital environment, ground fill does not significantly reduce crosstalk. Additionally, as Purcell points out, ground fill has the distinct disadvantage of modulating the impedance of any traces that run adjacent to a filled area. For those reasons, I do not use ground fill on multilayer digital boards.
Let me also point out that high-speed digital circuits are classified as low-impedance circuits, meaning that they have circuit impedances of much less than 377Ω, the impedance of free space. Most noise problems in low-impedance circuits are caused by magnetic-field coupling (that is, inductive coupling), as opposed to electric-field (or capacitive) coupling. Reducing magnetic-field coupling requires continuous return-current conductors running parallel to the signal traces everywhere, keeping the returning signal current close to the outbound signal current. Solid reference planes provide this function. Isolated, discontinuous regions of ground fill do not help reduce magnetic-field coupling between traces or radiation from the board.