We’ve examined a couple mechanisms for crosstalk, so what options do we have to reduce this undesirable effect? Well, utilizing guard traces is commonly considered a “best practice” by many PCB designers for reducing crosstalk. Guard traces are grounded copper lines running parallel to sensitive traces on a PCB. The figure below shows a guard trace inserted between two signal traces on a PCB.
Now that you know what they are, should you start sprinkling these into your designs? Unfortunately, most designers just throw them in without considering if the benefits outweigh the additional costs and complexity they can add to a given design. Let’s take a moment to examine when the use of guard traces is appropriate.
Are Guard Traces Right for My Design?
Under certain conditions, guard traces can reduce crosstalk between adjacent traces by an order of magnitude. However, achieving this degree improvement is typically only possible on designs without solid ground planes. If you’re using a classical stackup, then you already have a ground plane in your design, which, in a homogenous digital system, provides nearly all the benefits of guard traces. If your design contains analog circuitry (particularly high power circuits) or if you’re mixing logic families (like TTL and ECL) guard traces may still be beneficial.
As an example, on a PCB with adjacent traces separated by 40 mils (centerline distance) and a dielectric thickness of 5 mils separating the traces above the ground plane, the crosstalk will measure less than 2%. In a design utilizing a common logic family (all TTL or all ECL for example) this level of crosstalk will not affect performance and guard traces buy you pretty much nothing. If you’re mixing logic families though, this level of crosstalk may be problematic. Simply examine the noise margin of your design to determine whether or not 2% crosstalk is enough to upset your lower voltage swing logic components.
Much of PCB design is trial and error, so what if you have a fabricated design that is exhibiting unacceptable levels of crosstalk between adjacent traces? It is always best to go back to first principles and try to understand the coupling mechanism. With that said, inserting a guard trace may help. The rule of thumb is that inserting a guard trace grounded at regular intervals (such as the one shown in the figure above) between signal traces will reduce crosstalk to approximately 25% of it’s current level (a substantial change to be sure!).
Guard traces are just one tool in a PCB designer’s toolbox to reduce crosstalk. As with any tool, you must know how and when it is appropriate to use it. When a design exhibits substantial noise problems, it is always best to try to understand the underlying noise source. Under certain conditions though, guard traces can be very effective in reducing crosstalk.