The idea behind this principle is to reduce the coupling between circuits by basic physical separation. The actual amount of separation is difficult to specify for all applications and, of course, depends on the wavelengths of the signals in each section (one-quarter-wavelength gaps being a minimum). As a basic guide, a 5-mm gap between circuits all around is usually adequate.

Segmentation of circuits is usually performed by using a moated (empty) area around each circuit or functional block. Hence, some patterning is required of any ground and power planes. Patterning the ground and supply rails prevents a power surge or noise voltage on one circuit block (which may be able to handle the event) from being returned via the ground on another circuit block (which cannot tolerate such an event). Although the ground connections and supply rails may meet at the power input to the PCB, by separating, the loops for supply and ground return are controlled for each circuit.

Figure 1. Segmentation: separation of circuits by function or operating speed.

Function and operation speed should segment circuits. High-speed digital circuits tend to have high instantaneous current demands at clock edges, and therefore these circuits should be placed closer to the power supply unit (PSU) inlet than slower circuits such as analog functions and interface circuits (see Figure 1). It is important to note that it is not the absolute power demand that causes EMC problems within a system, but rather transients in the power demand.

Circuits that will interface with the outside world or with other PCBs within the end system must be near the PCB edge; there should be no trailing wires across a PCB within a system. Some circuits on a PCB are known to be noisy or are intended to handle dirty signals from off-board systems. Filtering might be required at these circuit inputs, so a secondary segmentation within the circuit block might be required to handle the off-board signal filters at the PCB interface. A separate moated ground plane for interface circuits would be another good EMC measure, especially if the system has a safety ground (or an EMC ground) that could be referenced for electrostatic discharge (ESD) and transient suppression circuits directly at the interface socket.

The main objective of a grounding pattern is to minimize the ground impedance and the size of any potential ground loops from a circuit back to the power supply. Note that this is not simply minimizing the resistance at the frequencies of interest for EMC; it is inductive reactance of the tracking that usually dominates the impedance characteristic.

Guard Ring. This is a ground-connected track that does not carry a return current for the circuit under normal operation. Its purpose is mainly to serve as a return source for radio-frequency current radiating out of, or incident to, the PCB (see Figure 2). It is usually tracked around the outer edge of a PCB and around connectors and input-output circuits. If a separate safety ground is being used, the guard ring can be connected to this rather than system ground, and safety or ESD devices could sink their current via this track. The guard ring can act as a field-fringing sink and can be placed around the edge of a power plane, as well as around the tracking layers.

Figure 2. Guard ring. The grounded track normally carries no current.

Single-Sided Ground Tracking. A grounding strategy can still be implemented on a single-sided PCB. The first consideration is to plan for a wide ground track covering as much of the PCB as possible. Do not attempt a ground plane and then etch out the plane for tracking. Doing so can actually cause more problems than it solves because it could leave unconnected metallized areas within the PCB that reflect signals through the board or act as receivers and inject capacitively into nearby tracks. It is preferable to attempt a star arrangement of connecting ground and power, but this can be difficult with only single-layer tracking.

Using inductor-capacitor filters at the input to each circuit segment from a daisy-chained power rail could compensate for the limited available tracking because the inductors from the supply rail can be used as bridging components. A guardrail can be placed around the edge of a PCB, connecting to the ground at the input to the PCB only. Even on a single-sided board, this approach helps reduce field fringing at the board edge. If a shield proves necessary, leaving the guard ring as a solder-masked track provides a suitable place to attach the shield.

Ground Grid (Ground Matrix). A ground grid forms a series of box sections on the PCB. A ground area beneath each integrated circuit (IC) on the component side also helps (even if a full grid cannot be implemented); decoupling capacitors can be tied directly to the IC supply line using this area. To maintain low impedance, a thick track for the ground grid is preferred, but with high-pin-count surface-mount components, a thick track is not always possible. A thin track completing the grid is better than no track at all. Even though a thin track is not a particularly low-impedance solution, it still minimizes loop areas for both ground currents and signal-return paths.

Mirror Supply Lines. For ground grids to be truly effective at minimizing signal loops, a similar pattern for the supply should be attempted, mirroring the ground paths wherever possible (see Figure 3). However, it is not necessary for the supply path to completely grid the same way the ground does. Comb or star supply arrangements can be very effective when coupled with a complete ground grid (comb patterning should not be used on grounding schemes).

Figure 3. Mirror supply and ground paths. A thinner power track reduces field fringing.

Having the supply track slightly narrower than the ground helps reduce supply field fringing and reduces crosstalk from the supply rail to nearby signal tracks.

Safety or ESD/EMC Ground. A separate safety ground designed as either a plane or a guard track is particularly useful where signals enter and exit the system. Often the safety ground cannot be used over a complete PCB plane because the leakage current specifications are exceeded by capacitive coupling effects. A low-value decoupling capacitor between the signal and safety ground, and close to any off-board signal connectors, provides a high-frequency current link between system and safety references. Capacitive coupling between analog and digital grounds close to any signal interface should also be planned to capacitively bridge any moat region at the signal interface.

On a multilayer PCB, the ground and power planes should be planned first. If one of the supply planes has to be sacrificed for tracking, it should always be a power plane. The ground plane should be maintained intact wherever possible.

Increasing the PCB stack and including one or more ground planes can solve many EMC problems encountered with both single- and double-sided PCB designs. A preferred stack would have ground and power planes separated by a prepreg layer (foil build) or thin laminate, with a thick laminate between power and tracking and between ground and tracking. Using a thin layer between the power and ground planes minimizes the distance between them, thereby maximizing the effective capacitance. A PCB capacitor constructed in this manner has a very high frequency response (high self-resonant frequency) and low series inductance.

Multilayer PCB Ground Possibilities. Several of these grounding strategies, including placing a surface ground grid on digital sections with buried or even multiple ground planes, can be implemented on a PCB structure with many layers and a ground plane. Wherever there are several ground circuits, the circuits must be interconnected to maintain a low impedance and short return loops.

Copper fill, a common technique for use with some analog circuits, introduces areas of copper on the portions of the PCB surface that carry no signals and therefore should be grounded. Although this can potentially reduce field fringing and improve decoupling, the copper areas can be inadvertently left disconnected, which can induce electromagnetic interference (EMI) problems. This technique is not suitable for digital circuits because it can create differences in signal skew as well as propagation delay between tracks that could lead to functional failures. Consequently, copper fill is not particularly popular for many modern designs and should be used with care on analog circuits. Ground stitching, which refers to placing multiple vias between ground areas on different layers, can be used with guard rings and large grounded surface areas that result from copper fill. If the system's chassis is grounded, using plated through holes for the stitching points and further connecting these to the chassis can produce very quiet PCB designs.

Grounding strategies can be the key to successfully reducing EMI during the design of a PCB. Addressing EMC problems at this very early stage can eliminate the need for additional components and can minimize the need for redesign of the PCB later, when the cost is much higher.