Grounding Strategies for Printed Circuit Boards
Segmentation and grounding patterns can be used to control EMC
Design and layout of a printed circuit board (PCB) for electromagnetic
compatibility (EMC) is probably the most cost-effective measure possible
in the quest for EMC compliance. It is cost-effective because it requires
no additional components. It requires just the knowledge of EMC layout
methods and experience in applying them. Some critical errors in layout
that can cause an EMC problem cannot be resolved simply through the
application of additional filters; relaying the PCB may be the only
solution, and getting it right the first time therefore offers the lowest-cost
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
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
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
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.
Martin O'Hara is senior design consultant for Telematica Systems
Ltd. (Northampton, UK) and author of EMC at Component and PCB Level
(Newnes; Woburn, MA). He can be reached at MOHara@
Back to March/April
Table of Contents