When a prototype power board is powered up for the first time, the best possible outcome is that it not only works but also runs quietly and stays cool. That outcome is far less common than designers would like. A frequent problem with switching power supplies is an "unstable" switching waveform: in some cases the jitter falls in the audio band, and the magnetic components then emit audible noise. When the root cause lies in the PCB layout, tracking it down can be genuinely difficult. That is why a correct PCB layout at the very beginning of a switching power supply design is so critical.
A good layout optimizes power supply efficiency and relieves thermal stress. More importantly, it minimizes noise and the interaction between traces and components. To achieve these goals, the designer must understand the current conduction paths and the signal flow inside the switching power supply. The power supply designer must also understand both the technical details and the functional requirements of the end product, and should work closely with the PCB layout designer on the critical power layout from the moment the board design project starts. The design elements summarized in the sections below should be kept firmly in mind when laying out a non-isolated switching power supply.
Highlights:
- Layer stack planning decides noise coupling: a ground or DC voltage layer placed between the high-current power stage layer and the sensitive small-signal layer shields analog routing from switching noise, and it should not be split unless absolutely unavoidable.
- The pulsed (switching) current loop, or hot loop, must be given the smallest possible circumference with short, wide traces; parasitic inductance in this loop both radiates magnetic fields and produces voltage ringing and spikes on the traces and MOSFETs.
- The high dV/dt switching node is a strong EMI source, so its copper area is a deliberate trade-off between minimizing coupling capacitance and providing enough heat-spreading area for the power MOSFETs.
Layout Planning
For a DC/DC power supply embedded on a large circuit board, obtaining the best voltage regulation, load transient response, and system efficiency requires placing the power supply output close to the load device, so that interconnect impedance and conduction voltage drop along the PCB traces are minimized. The supply must also be given good airflow to limit thermal stress; if forced-air cooling is available, place the supply near the fan.
In addition, large passive components such as inductors and electrolytic capacitors must not block the airflow passing over low-profile surface-mount semiconductors such as power MOSFETs or PWM controllers. To prevent switching noise from interfering with analog signals in the system, sensitive signal traces should be kept out from under the power supply wherever possible. If that cannot be avoided, an internal ground layer must be placed between the power layer and the small-signal layer to serve as a shield.
The key is to plan the location of the power supply and its board space requirements early, during system design and planning. Designers sometimes disregard this advice and concentrate their attention on the circuits that appear more "important" or more interesting on a large system board. Power management is then treated as an afterthought, with the supply dropped into whatever spare space is left on the board. That approach is highly detrimental to an efficient and reliable power supply design, because the power stage is precisely the part of the board where current density, heat, and noise are concentrated.
For multilayer boards, a good approach is to place a DC ground layer or a DC input/output voltage layer between the high-current power component layer and the layer carrying sensitive small-signal traces. The ground layer or DC voltage layer provides an AC ground that shields the small-signal traces from the noisy power traces and power components.
As a general rule, the ground layer or DC voltage layer of a multilayer PCB should not be split. If a split is unavoidable, minimize both the number and the length of the traces on those layers, and route them in the same direction as the high currents so that the impact is minimized.
A poor six-layer stackup and a poor four-layer stack-up for a switching power supply are both characterized by the same mistake: the small-signal layer is sandwiched between a high-current power layer and a ground layer. This arrangement increases the capacitive noise coupling between the high-current/high-voltage power layer and the analog small-signal layer. In the corresponding good six-layer and four-layer designs, the ground layer is used to shield the small-signal layer, which helps to minimize inter-layer coupling noise. The essential points are these: always place a ground layer adjacent to the outer power stage layer, and use thick copper for the outer high-current power layer to minimize PCB conduction loss and thermal resistance.

Poor structures of six-layer (a) and four-layer (c) switching power supply PCB boards, with the small-signal layer sandwiched between the high-current layer and the ground layer; in the better six-layer (b) and four-layer (d) des
Power Stage Layout
A switching power supply circuit can be divided into two parts: the power circuit and the small-signal control circuit. The power stage contains the components that carry large currents. As a rule, these components should be placed first, and the small-signal control circuit should then be placed at the specific points defined by the power stage layout.
High-current traces should be short and wide, so that PCB inductance, resistance, and voltage drop are minimized. This is especially important for traces that carry pulsed currents with a high di/dt.
A synchronous buck converter contains both continuous current paths and pulsed current paths. The continuous current paths are the ones that carry current throughout the switching cycle, while the pulsed (switching) current paths carry current only during part of the cycle. The pulsed current paths include the traces connected to the following components: the input decoupling ceramic capacitor CHF, the upper control FET QT, the lower synchronous FET QB, and the optional parallel Schottky diode.
These high di/dt current paths contain PCB parasitic inductance. Because of this parasitic inductance, the pulsed current path not only radiates magnetic fields but also generates large voltage ringing and voltage spikes on the PCB traces and on the MOSFETs. To minimize PCB inductance, the pulsed current loop, often called the hot loop, must be laid out with the smallest possible circumference, and its traces must be short and wide. Every additional millimeter of loop perimeter adds inductance, and that inductance converts fast current transitions into voltage overshoot and radiated energy.
The high-frequency decoupling capacitor CHF should be a ceramic capacitor of 0.1μF to 10μF with an X5R or X7R dielectric, which offers very low ESL (equivalent series inductance) and ESR (equivalent series resistance). Larger-dielectric materials such as Y5V can lose a substantial part of their capacitance at different voltages and temperatures, so they are not the best material choice for CHF.
A layout example for the critical pulsed current loop in a buck converter places all power components on the same side of the board and routes all power traces on the same layer, so as to limit resistive voltage drop and the number of vias. When a power trace must be routed to another layer, choose a trace that belongs to the continuous current path rather than to the pulsed path. When vias are used to connect PCB layers within a high-current loop, use multiple vias to minimize impedance.
A boost converter has a different loop topology. Here the high-frequency ceramic capacitor CHF should be placed close to the output of the MOSFET QB and the boost diode D. In the corresponding boost pulsed current loop layout, the key objective is to minimize the loop formed by the switch QB, the rectifier diode D, and the high-frequency output capacitor CHF. The difference from the buck case is important: the pulsed loop is defined by which components conduct the switched current, not by the physical position of the input connector, so the loop must be identified before components are placed.
A synchronous buck design example illustrates the importance of these decoupling capacitors. The board is a dual-phase 12V-input synchronous buck supply with a 30A maximum output, built around an LTC3729 dual-phase single-VOUT controller IC. At no load, the waveforms at the switching nodes SW1 and SW2, as well as the output inductor currents, are stable. But if the load current exceeds 13A, the waveform at the SW1 node begins to lose cycles. At higher load currents the problem becomes more severe.
Adding two 1μF high-frequency ceramic capacitors at the input of each channel solved the problem. The capacitors isolate the hot loop area of each channel and minimize it. Even at the maximum load current of 30A, the switching waveforms remained stable.
The High dV/dt Switching Region
In both the buck and the boost topology, the SW voltage swing between VIN (or VOUT) and ground has a high dv/dt rate. This node contains a rich content of high-frequency noise components and is a powerful EMI noise source. To minimize the coupling capacitance between the switching node and other noise-sensitive traces, the SW copper area might be made as small as possible.
However, the SW node must also conduct the large inductor current and must provide a heat-spreading area for the power MOSFET, so the PCB area devoted to the SW node cannot be too small. As a general recommendation, a ground copper area should be placed underneath the switching node to provide additional shielding.
If the design has no heat sink for the surface-mount power MOSFETs and the inductor, the copper area must have sufficient thermal dissipation area. For DC voltage nodes such as the input voltage, the output voltage, and the power ground, the sensible approach is the opposite: make the copper area as large as possible.
Multiple vias help to further reduce thermal stress. Determining the appropriate copper area for a high dV/dt switching node is therefore a design balance between minimizing dv/dt-related noise on one side and providing good MOSFET heat dissipation on the other.
Power Pad Geometry
Pay attention to the pad geometry of power components such as low-ESR capacitors, MOSFETs, diodes, and inductors. Poor and good power component pad patterns differ in ways that directly affect noise, thermal resistance, and efficiency.
For decoupling capacitors, the positive and negative vias should be placed as close to each other as possible to reduce the PCB ESL. This is particularly effective for low-ESL capacitors. Small-value, low-ESR capacitors are usually relatively expensive, and incorrect pad geometry together with poor routing will degrade their performance and therefore increase the overall cost. Under normal circumstances, correct pad geometry reduces PCB noise, lowers thermal resistance, and minimizes trace impedance as well as the voltage drop across high-current components.
A common error when laying out high-current power components is the inappropriate use of a thermal relief. Using thermal reliefs where they are not necessary increases the interconnect impedance between power components, which causes higher power loss and degrades the decoupling effectiveness of low-ESR capacitors. If vias are used in the layout to carry large currents, make sure there are enough of them to reduce impedance. In addition, do not use thermal reliefs on these vias.
An application with several on-board power supplies that share the same input voltage rail requires one more consideration. When these supplies are not synchronized with each other, the input current traces need to be isolated from one another to avoid common-impedance noise coupling between the different supplies. In that situation, whether each supply has its own local input decoupling capacitor is actually not very critical.
For a polyphase single-output converter, giving each phase a symmetrical layout helps to balance thermal stress across the phases.
Switching Power Supply PCB Layout: Control Circuit Isolation, Loop Area, and Inductor Placement
Layout Design Example
It is a 3.5V to 14V input, maximum output 1.2V at 40A dual-phase synchronous buck converter using the LTC3855 Polyphase current-mode step-down controller. Before starting the PCB layout, a good habit is to mark the high-current traces, the high-noise high-dv/dt traces, and the sensitive small-signal traces in different colors on the logical schematic. Such a drawing helps the PCB designer distinguish the different routing classes.
QA is the high-side control MOSFET and QB is the low-side synchronous FET. The ground area of QB can optionally be increased to obtain more output current. Under the power component layer, place a solid power ground plane.
Control Circuit Layout
Keep the control circuit away from the high-noise switching copper areas. For a buck converter, a good approach is to place the control circuit near the VOUT+ terminal; for a boost converter, place the control circuit near the VIN+ terminal, so that the power traces carry continuous current. The intent is to keep the high-current power paths continuous and to avoid making them carry switched current over unnecessary lengths of copper.
If space permits, there should be a small distance (0.5 in to 1 in) between the control IC and the power MOSFETs and inductor, which are high-noise and high-heat components. If space is tight and the controller is forced to sit close to the power MOSFETs and inductor, pay special attention to isolating the control circuit from the power components with a ground plane or ground traces.
The IC has an exposed GND pad, which should be soldered to the PCB to minimize electrical impedance and thermal resistance. Several key decoupling capacitors should be placed right next to the IC pins.
The control circuit should have an independent signal (analog) ground that is different from the power-stage ground. If the controller IC has separate SGND (signal ground) and PGND (power ground) pins, they should be routed separately. For a control IC with integrated MOSFET drivers, the small-signal portion of the IC pins should use SGND.
Only one connection point is needed between signal ground and power ground. A reasonable method is to return the signal ground to a clean point on the power ground plane. Connecting the two ground traces only under the controller IC achieves the two-ground arrangement. In this example, the IC has an exposed ground pad. This pad should be soldered to the PCB to minimize electrical and thermal resistance. Multiple vias should be placed in the ground pad area.
Decoupling capacitors for the control IC should be close to their respective pins. To minimize connection impedance, a good method is to connect the decoupling capacitors directly to the pins without going through vias. The LTC3855 pins that should have nearby decoupling capacitors are the current-sense pins Sense+/Sense-, the compensation pin ITH, signal ground SGND, the feedback divider pin FB, the INTVCC voltage pin, and the power ground pin PGND.
Loop Area and Crosstalk
Two or more adjacent conductors can produce capacitive coupling. A high dv/dt on one conductor couples current into another conductor through parasitic capacitance. To reduce noise coupling from the power stage to the control circuit, keep high-noise switching traces away from sensitive small-signal traces. If possible, place high-noise traces and sensitive traces on different layers and use an internal ground plane as a noise shield.
If space permits, the control IC should be a small distance (0.5 in to 1 in) from the power MOSFETs and inductor, which are both noisy and hot.
The FET driver pins TG, BG, SW, and BOOST on the LTC3855 controller all have high dv/dt switching voltages. The LTC3855 pins connected to the most sensitive small-signal nodes are Sense+/Sense-, FB, ITH, and SGND. If the layout places sensitive signal traces near high dv/dt nodes, a ground trace or ground plane must be inserted between the signal trace and the high dv/dt trace to shield the noise.
When routing gate-drive signals, short and wide traces help minimize impedance in the gate-drive path. The routed high-side FET driver traces TG and SW should have minimum loop area to minimize inductance and high dv/dt noise. Likewise, the low-side FET driver trace BG should be close to a PGND trace.
If a PGND plane is routed under the BG trace, the AC ground return current of the low-side FET will automatically couple into a path close to the BG trace. AC current flows along the smallest loop and the lowest impedance it can find. In this case, the low-side gate driver does not need a separate PGND return trace. The best approach is to minimize the number of layers through which the gate-drive traces pass; this prevents gate noise from propagating to other layers.
Of all small-signal traces, current-sense traces are the most sensitive to noise. The current-sense signal amplitude is usually less than 100mV, which is comparable to the noise amplitude. Taking the LTC3855 as an example, the Sense+/Sense- traces should be routed in parallel with minimum spacing (Kelvin sensing) to minimize the chance of picking up di/dt-related noise.
In addition, the filter resistor and capacitor for the current-sense traces should be as close as possible to the IC pins. This filter arrangement works best when noise is injected into long sense lines. If inductor DCR current sensing with an RC network is used, the DCR sense resistor R should be close to the inductor, and the DCR sense capacitor C should be close to the IC.
If a via is used on the return path to Sense-, the via should not contact other internal VOUT+ layers. Otherwise, the via may conduct a large VOUT+ current, and the resulting voltage drop may corrupt the current-sense signal. Avoid placing current-sense traces near high-noise switching nodes (TG, BG, SW, and BOOST traces). If possible, place a ground plane between the layer containing the current-sense traces and the power-stage trace layer.
If the controller IC has differential remote voltage-sense pins, use independent traces for the positive and negative remote-sense lines, and also use Kelvin connections.
Trace Width Selection
For a given controller pin, the current level and noise sensitivity are unique, so the trace width must be selected for each signal. Small-signal nets can generally be narrower, using traces 10mil to 15mil wide. High-current nets (gate drive, VCC, and PGND) should use short, wide traces. These nets should be at least 20mil wide.
Chapter 6: Guidelines for Inductor Placement on Switching Power Supply PCBs
Question
Where should the coil be placed?

Answer
Switching regulators used for voltage conversion employ inductors to temporarily store energy. These inductors are usually quite large and must be allocated space in the printed circuit board (PCB) layout of the switching regulator. This task is not difficult, because the current through the inductor may change, but it cannot change instantaneously. The change can only be continuous and is usually relatively slow.
A switching regulator switches current back and forth between two different paths. This switching is very fast; the specific switching speed depends on the duration of the switching edges. The traces through which the switching current flows are called hot loops or AC current paths. They conduct current in one switching state and do not conduct current in the other switching state. In a PCB layout, the hot-loop area should be small and the path should be short so that parasitic inductance in these traces is minimized. Parasitic trace inductance produces unwanted voltage offset and causes electromagnetic interference (EMI).

Switching regulator for step-down conversion (with the critical thermal loop indicated by the dashed line).
The pic a buck regulator in which the critical hot loop is indicated by a dashed line. As can be seen, coil L1 is not part of the hot loop. Therefore, it can be assumed that the placement of this inductor is not critical. Keeping the inductor outside the hot loop is correct, so in the first instance its placement is secondary. However, several rules should be followed.
Do not route sensitive control traces under the inductor (neither on the PCB surface nor below it), in inner layers, or on the back side of the PCB. Because of the current flow, the coil produces a magnetic field, and this field affects weak signals in signal paths. In a switching regulator, one key signal path is the feedback path, which connects the output voltage to the switching regulator IC or to a resistor divider.

Example circuit of the ADP2360 buck converter with coil placement locations.
The figure above shows an example circuit for the ADP2360 buck converter with an inductor placement.
It should also be noted that a real coil has both capacitive and inductive effects. The first winding of the coil is connected directly to the switch node of the buck switching regulator, as shown in Figure 1. As a result, the voltage change across the coil is as strong and as fast as the voltage at the switch node. Because the switching time in the circuit is very short and the input voltage is high, considerable coupling effects can be produced on other paths on the PCB. Therefore, sensitive traces should be kept away from the coil.
The figure shows an example layout for the ADP2360. As can be seen, the yellow feedback path is at some distance from coil L1. It is located on an inner layer of the PCB.
Some circuit designers do not want any copper layer under the coil in the PCB. For example, they provide cutouts under the inductor, even in the ground plane layer. The goal is to prevent the ground plane under the coil from forming eddy currents due to the coil's magnetic field. This method is not wrong, but there is also an argument that the ground plane should remain continuous and should not be interrupted:
- A ground plane used for shielding works best when it is uninterrupted.
- The more copper on the PCB, the better the heat dissipation.
- Even if eddy currents are generated, these currents flow only locally, cause only small losses, and hardly affect the function of the ground plane.
Therefore, the ground plane layer, even under the coil, should remain complete.
In summary, although the coil of a switching regulator is not part of the critical hot loop, it is wise not to route sensitive control traces under or near the coil. The various planes on the PCB, such as the ground plane or the VDD plane (supply voltage), can be constructed continuously without cutouts.
Related Reading:
Printed Circuit History and PCB Classification Guide
Grounding Principles, Star Ground, and Ground Planes in PCB Design
Mixed-Signal IC Grounding and Decoupling: AGND, DGND, and Clock Jitter