Controlling for densely packed interconnects.

When high frequencies are involved, energy is traveling everywhere. Whether it be to or from an RF device, or purposefully directed by an antenna, or the unwanted emissions from electronics devices that require you to turn them off during takeoff and landing, high-frequency noise really gets around. On a printed circuit board level, such noise coupling is usually referred to as crosstalk. But crosstalk isn’t limited to one line coupling onto another line. Energy can be transferred from one via to another, even if those vias are on opposite ends of the board. It can also be coupled through the power system. These other methods of energy transfer aren’t what are generally referred to as “crosstalk,” but they yield the same result: unwanted energy coupled from one place to the next.

In a PCB design, it is usually complicated enough to design interconnects that meet requirements for impedance, loss and timing. Trying to squeeze all those interconnects into a small space adds the complication of having to control crosstalk as well.

1. Space things out. The most obvious solution to any noise coupling situation is to add distance between the aggressor and victim. For coupled traces, this means spacing traces farther apart. Noise coupling tends to decrease proportional to the distances of the traces to the reference plane, so designing a stackup with small dielectric heights is a good starting point. You can sweep through various spacing values for a specific board design in a simulation tool (Figure 1). This allows you to determine a minimal required spacing between traces. If you can’t meet spacing requirements on your board, you can adjust parameters like line lengths to find acceptable maximum line lengths for a given spacing.

2. Add enough grounds. Even if all the traces are spaced very far apart, a design can have a great deal of crosstalk if it lacks enough grounds in connector and cables. Crosstalk occurs in traces due to mutual coupling; a similar phenomenon can occur when signals in a connector have a shared return path. Since ground pins act as return paths in connectors, it is important to provide enough ground pins to permit signals to have separate return paths. A 1:1 ratio of signal to grounds is usually a good starting point.

3. Add stitching components. Similar to the case of enough ground pins in a connector, you also need ample stitching vias going through the board where you have signal transitions. This becomes incredibly important for fast, single-ended memory interfaces like DDR3, where you can have multiple signals transitioning layers in the same area. It is usually best to put any layer transitions close to the ICs where decoupling capacitors and stitching vias already exist, but for other layer transitions, it is important to put a stitching via or capacitor for every signal transition. If you don’t have any stitching vias, or only a few, you will end up with shared return paths between signals, and a great deal of coupled noise. Vias can couple noise over very long distances through the plane cavity. This, too, can be
simulated (Figure 2).

In this example, the vias are placed 6" apart, and the noise coupled from one via to the next is simulated. With no transition via, shown in blue, the noise induced into the plane cavity is quite large and results in a great deal of coupling onto the victim signal. With a stitching via added, shown in yellow, that noise is greatly reduced.

4. Build a solid power distribution network. Another common type of noise coupling is simultaneous switching noise, or SSN. In lab measurements, SSN is very difficult to distinguish from crosstalk, because it exhibits a similar waveform shape and lines up with the signal edges. However, SSN is a symptom of an inadequate power distribution network (or PDN). If the PDN impedance is too high at the power pins of an IC, when all the I/Os switch at once, their switching current will induce a voltage that can be seen on the signals themselves. This type of coupling can be eliminated by designing a PDN that exhibits a low impedance across a wide frequency range. This typically requires placing a large number of decoupling caps on a design close to the IC power pins, having a closely-coupled power-ground plane pair in the stackup, and connecting them all together using short, low-inductance connections.

With an awareness of the common causes of noise coupling in a PCB design, and armed with the tools to evaluate solutions to these problems, you can certainly keep the energy in your PCB confined to exactly where you want it to be.

Pat Carrier is a technical marketing engineer at Mentor Graphics (mentor.com); This e-mail address is being protected from spambots. You need JavaScript enabled to view it .