When it comes to switching power supplies, the importance of a
good printed circuit board (PCB) layout can't be overstated.
Developing the schematic and debugging the breadboard is a good
start, but the final, critical challenge for the designer is laying
out the PCB. Fortunately, understanding the phenomena behind the
operation of the typical switching power supply makes this effort
Designers are involved with every aspect of the design of the
switching power supply, including the PCB layout, because it is the
designer who best understands the functional requirements of the
The designer should never allow a PCB designer to use
auto-routing. The autorouter only connects nodes that carry the
same signal name as stated in the netlist, disregarding the length
of the traces needed to accomplish these connections. The
autorouter also considers all grounds to be the same signal and
connects them together without consideration for the actual types
of signals running through certain traces. For the power supply
designer and the PCB designer to execute a good PCB layout, knowing
the signals that flow between components is very important.
Appreciating the subtle "black magic" aspects of the PCB layout
is essential. Layout factors can affect the performance of the
switching power supply and the market success of the product.
The aspects of the product's operation that affect the printed
circuit board design include:
- Radiated EMI (electromagnetic interference)
- Conducted EMI
- Power supply stability
- Operational longevity.
Regulatory approval bodies such as UL, IEC, and numerous others
throughout the world test the two forms of EMI. A product must pass
stringent EMI tests before it can be sold into its respective
Power supply stability and operational longevity affect the
product's basic operation and customer satisfaction.
Switching power supplies have large current pulses with very
sharp edges flowing within the power supply circuit. These large
current pulses have the greatest effect on the creation of EMI, and
should be the primary focus of the PCB designer. Currents flow in
definable loops, so the circuits carrying these currents should be
laid out first. The low-level control circuitry is subsequently
coupled into specific spots in the layout.
Figure 1 displays loops for the three major basic
topologies of switching power supplies. All of the other topologies
are variations of these three.
Listed in order of greatest to least effect on noise generation
and operational performance, the loops shown in figure 1 are as
- The power switch high current loop
- The rectifier high current loop
- The input source loop
- The output load loop.
The input source and output load current loops are filtered by
input and output EMI filters (not shown). The currents are largely
composed of DC current. The AC components of these currents are
created by the power supply and should be kept to a minimum. AC
components are the elements that make up conducted EMI. Any AC
energy that is allowed to pass over a long enough length of a
conductor is radiated into the product's environment.
The input and output loops are of secondary concern because the
large AC pulses seen inside the supply are filtered by the input
filter and output filter capacitors. Filtering sets their potential
for creating high-frequency noise problems at less than the two
high-current AC loops.
It is worthwhile to follow-up with an analysis of the input and
output loops because they are directly measured by the regulatory
agencies. The power switch and rectifier current loops are entirely
AC, or more appropriately, pulsating DC. They have trapezoidal
current waveforms with high peak currents and very sharp edges
PWM switching power supplies operate in one of two modes:
- Discontinuous mode (seen below in Figure 2A)
- Continuous mode (Figure 2B).
Figure 2: The modes of operation of switching power
supplies are shown here. In discontinuous mode, the output
rectifier(s) is allowed to completely empty the magnetic element of
its magnetic energy before the power switch once again turns on. In
continuous mode, some residual energy is allowed to remain in the
magnetic element when the power switch begins to turn on for the
next cycle. The current flowing at the end of each period is
rapidly interrupted by high speed switches which results in very
high di/dt transitions.
High rates of dV/dt occur simultaneously on these signals,
creating high periodic power impulses rich in high-frequency
components. The power switch and rectifier loops, as a result, are
very noisy and deserve extraordinary attention. The input power
switch loop flows between the input filter capacitor
(CIN), through the primary winding of the transformer
(or inductor), to the power switch and back through the ground to
the input capacitor.
The rectifier loop flows between the secondary winding of the
transformer (or output of the inductor), through the rectifier to
the output filter capacitor (COUT), and returns through
the ground to the transformer or inductor. There is always a filter
capacitor composing part of both loops because the capacitors are
the only local source or sink of the high-frequency current needed
by the switching power supply. The input source and output load
current loops can be viewed as low frequency currents that charge
or discharge the input and output filter capacitors respectively,
at a virtual DC rate.
The power switch loop and the output rectifier loop(s) should be
laid out so that the loop has a very small circumference and is
composed of traces with considerable width and length.
First, the circumference of the loop controls the amount of RF
energy that can be radiated at lower frequencies where a
significant amount of conducted RF energy exists. By making the
loop circumference as short as possible, the loop does not provide
an efficient antenna for these lower noise frequencies.
A typical power supply conducts noise frequency components that
remain very high until about 100 times the switching frequency and
then fall at a rate of between -20 to -40dB per decade. The lower
the frequency a loop is allowed to radiate, the more energy that is
allowed to escape into the environment.
Secondly, the width of the traces used within the high current
loops directly dictates the amount of voltage drop that appears
around the loop. This voltage drop, when created by high current,
also creates RF radiation. The inductance and resistance exhibited
by a trace is inversely proportional to its width. Inductance
lowers the frequency response of a loop and is therefore a more
efficient antenna at lower frequencies, so loop traces should be as
wide as possible. Wide traces also provide better heatsinking for
the power switch and rectifier(s).
Figure 3 shows an example of a layout for the power
switch and rectifier loops in a buck converter. Notice the very
short distances between all members of the two main AC loops.
Figure 4 shows an example layout for the rectifier loop
within a flyback converter. The output rectifier loop in
transformer-isolated topologies has the same layout requirements as
the input power switch loop.
Parallel capacitors are commonly used to lower the overall
equivalent series resistance (ESR) and equivalent series inductance
(ESL) of a filter capacitor. Lowering the ESR and ESL allows the
resulting filter capacitor to source or sink higher levels of
ripple current with much less internal heating.
Here, the PC board layout has a direct affect on how much
sharing occurs in the current and heating of the paralleled
capacitors. The physical characteristics of the PCB layout between
the other components in the loop and each capacitor must be as
similar as possible.
If the layout and each capacitor are not identical, the
capacitor with the lower series trace impedance will see higher
peak currents and become hotter (i2R). To promote this
sharing, the form of the leads to both capacitors should be
Traces between the components within the loop should be as short
and wide as possible. Any parasitic impedance that is introduced by
the layout effectively isolates the capacitor from the loop,
causing the high frequency current pulses to seek other sources or
sinks outside the loop. This creates more conducted EMI when the
high current pulses are allowed to escape from the loop and enter
the external circuitry.
Figure 5: The physical characteristics of the PCB layout
between the other components in the loop and each capacitor must be
as similar as possible. In 5a, the loops are different lengths. In
5b, the ideal arrangement for the board components has both loops
closer in length and similar impedance.
It is better to consider the grounds within a switching power
supply separately, even though they make up one leg of the high
current loops previously discussed. Grounds represent the lowest
potential return path for the currents and the potential from which
all other signals are measured. They carry both DC and AC signals
being conducted between various points in the physical ground
system. Sections of the ground system should be considered
separately from one another. If these grounds are interconnected
improperly, the power supply can become unstable.
There are three grounds within a switching power supply:
- Input high-current ground
- Output high-current ground
- Low-level control ground.
Figure 6 shows the grounds for the three major switching
power supply topologies. The connection of the low-level control
ground to the overall grounding system is very specific.
The main purpose of the power supply controller is to precisely
regulate the output voltage. To do this, the controller's high-gain
error amplifier should be directly connected to the bottom of the
output filter capacitor. In this way, noise voltages from the high
current loops are not summed into the low-level sense signals. The
controller usually needs to sense a small signal across a current
sensing resistor as well as drive the gate or base of a power
If there are separate analog and power ground pins on the
controller IC, they should be routed separately to the ground side
of the current sensing resistor. If the IC does not have separate
ground pins, then the trace between the IC and the ground end of
the current sense resistor should be short and wide.
Another good way to reduce radiated EMI is to place large areas
of ground plane on the opposite side of the PCB and around these
high current traces. The ground planes act as electrostatic shields
for some of the RF energy already radiated. These large conductor
areas trap radiated EMI and dissipate it within eddy currents
created by the RF energy.
One last and very important factor in designing PCB layouts for
switching power supplies is the capacitive coupling of the AC node
voltages into their heatsinks or into nearby ground planes. The
coupling is severe in through-hole designs, but can also be a
serious problem in surface-mount applications.
The coupling is created by high AC voltages that appear on
specific nodes within the switching power supply. Examples of these
- Drain connection of the power switch
- AC node connected to an output rectifier
- Any snubber or clamp networks connected to these nodes.
In through-hole applications, the power switch is typically a
power package with a tab bolted to a heatsink and a 5mil
(0.005-inch, 0.13mm) insulator between them. The drain tab of the
power switch has AC peak-to-peak voltages of either one or two
times the input voltage. In many supplies, the heatsink is earth
grounded which provides a path for the capacitively coupled noise
energy to exit the enclosure. Insulator makers have pads with
embedded foil in them that cuts the capacitance in half.
The problem of minimizing capacitance is less significant in
surface-mount applications because capacitance formed by 0.062-inch
(1.6mm) thick F4 PCB material is much smaller. Additionally, it is
rare that earth ground is brought onto the PCB, but the noise could
couple into other sensitive signals. The goal is to reduce this
parasitic capacitance by creating PCB structures that exhibit low
capacitance, such as locating susceptable signals one the same side
instead of underneath the noisy node or cross-hatching any ground
planes beneath the noisy node.
The EMI Filter Layout
An EMI filter is needed any time a power lead or leads are
allowed to exit the product's enclosure, which should also provide
some RF shielding. Filters are intended to reduce, but cannot
completely eliminate, the high frequency currents conducted within
the DC input or output wiring. Regulatory bodies test conducted EMI
by placing a special current transformer (a line impedance
stabilization network or LISN) in series with the input and/or
output power lines. The tester then plots the spectrum of the
emerging current waveform from DC to over 1GHz. The product under
test must emit a current spectrum lower than the specified limits
at all frequencies.
The filters are designed to not pass the high frequency noise
created by the PWM switching power supply. If the parasitic factors
of the filter components themselves are not well known and the
components are not laid out properly, some switching energy can
couple around the filter components to traces on the other side of
the filter. This allows some of the high frequency energy to escape
into the environment or into the rest of the system. Once in the
external wiring, this conducted RF energy will then radiate into
the surrounding environment as radiated EMI.
A good guideline is to place the EMI filter as close as possible
to the point where its signal exits the enclosure. The layout of
the actual EMI circuitry should also be as close to "in-line" as
possible. "Zig-zaging" the layout can cause input and output traces
to be in close proximity to each other, thus promoting inductive
Example: Printed Circuit Board Designs
The design examples that follow (Figures 7 through 12)
illustrate layouts that are part of a larger PCB not bounded by
edges of a PCB. The power supplies are generally powered from an
external AC/DC power supply.
The examples have not been built and debugged. Sub-circuits such
as snubbers and clamperes may need to be added to make the designs
The Buck (Step-Down) Converter
The buck converter illustrated below provides an output voltage
of 3.3VDC and can deliver up to 3A to a load. It is powered by a
12V battery pack or from a wall transformer. The input voltage may
go as high as 30VDC, which makes the converter useful in many
portable applications such as notebook computers.
|Buck Converter Specifications
||+5V to +30VDC
|Maximum Output Current
Figure 7: Schematic of the buck (step-down) converter.
The circuit may be easily scaled to operate at different input
voltages or to deliver a different output voltage or maximum
current. The semiconductors, filter capacitors, inductor, and the
PCB layout would have to be modified to operate optimally for any
Figure 8: PCB layout for the buck converter
The Boost Converter
The boost converter design shown here derives its input power
from a +5V logic supply and could provide power to any associated
analog functions or interface circuits. Once again, the design can
|Boost Converter Specifications
||+5V - 7VDC
|Maximum Output Current
Figure 9: Boost (step-up) converter derives input power
from a +5V logic supply.
Figure 10: PCB layout for the boost converter
The Flyback Converter
The flyback converter (Figure 11) can be used as a step-up,
step-down or an inverting power supply.
|Flyback Converter Specifications
||+5V - +24VDC
||+5V +/-2% at 0.75A (max)
+12V +/-5% at 0.25A (max)
-12V +/-8% at 0.25A (max)
Figure 11: The flyback converter's transformer is more
complicated to design, but its added cost can be recovered
considering the flyback converter can replace two or more buck or
boost supplies within a system.
Figure 12: PCB Layout for a flyback converter