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 much easier.

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 power supply.

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 market.

Power supply stability and operational longevity affect the product's basic operation and customer satisfaction.

Current Loops

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 follows:

1. The power switch high current loop
2. The rectifier high current loop
3. The input source loop
4. 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 (di/dt).

Representative Waveforms

PWM switching power supplies operate in one of two modes:

• Discontinuous mode (seen below in Figure 2A)
• Continuous mode (Figure 2B).

(2A)

(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 (C_IN), 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 (C_OUT), 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.

Paralleled Capacitors

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 symmetrical.

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.

Grounds

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:

1. Input high-current ground
2. Output high-current ground
3. 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 switch.

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 nodes are:

• 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 coupling.

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 workable.

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.

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 new requirements.

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 be scaled.

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.

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