Buck Regulator PCB Layout and Grounding
"Noise problem" is a phrase every circuit board designer eventually hears. Solving it can consume hours of lab testing, only to reveal that the root cause is a poorly laid out switching power supply. The fix may require a new layout, which can delay the product schedule and increase development cost.
This article provides practical guidance for printed circuit board (PCB) layout and routing so designers can avoid these noise problems. The example layout uses the ADP1850 dual-channel synchronous switching controller. The first step is to identify the regulator's current paths. Those paths then determine where the devices should be placed in a low-noise layout.
Highlights:
- Identify the AC and DC current paths before placing components. Small high-current loops reduce ringing, overshoot, and ground bounce.
- Keep power devices and bypass capacitors close together, use separate AGND and PGND planes, and join them at the negative terminal of the output capacitor.
- Treat switch-node, gate-drive, current-sense, FB, and ILIM traces as high-δI/δt or noise-sensitive paths. Use short direct routing, Kelvin sensing, and optional snubbers or gate resistors where needed.
PCB Layout and Routing Guidelines
In a switching converter, high-current paths and low-current paths are physically close to one another. AC paths carry spikes and noise, high DC paths produce considerable voltage drop, and low-current paths are often sensitive to noise. Good PCB layout starts with identifying the critical paths, then arranging the components and providing enough copper area so that high currents do not corrupt low-current signals. A poor layout typically shows up as ground bounce and noise injection into the IC and the rest of the system.
Step 1: Determine the Current Paths
These power devices must be placed carefully to avoid undesirable parasitic capacitance and inductance, which can cause excessive noise, overshoot, ringing, and ground bounce.
Switching current paths such as DH, DL, BST, and SW leave the controller and must be arranged to avoid excessive parasitic inductance. These traces carry high δI/δt AC switching pulse current that may reach or exceed 3 A for several nanoseconds. The high-current loop must be small to minimize output ringing and avoid picking up additional noise.
Low-value, low-amplitude signal paths, such as compensation and feedback components, are sensitive to noise. Keep these paths away from the switch node and power devices so that interference is not injected into them.
Step 2: Physical Floor Planning
PCB floor planning is important. The current-loop area must be minimized, and the power devices must be arranged so that current flows smoothly without sharp corners or narrow paths. This helps reduce parasitic capacitance and inductance and eliminates ground bounce.
Figure 1 shows the PCB layout of a dual-output buck converter using the ADP1850 switching controller. Note that the power-device placement minimizes both the current-loop area and parasitic inductance. The dashed lines indicate high-current paths. This floor-planning technique can be used with both synchronous and asynchronous controllers. In an asynchronous controller design, a Schottky diode replaces the low-side switch.

Figure 1 | PCB layout of a dual-output buck converter using the ADP1850 controller
Step 3: Power Devices: MOSFETs and Capacitors (Input, Bypass, and Output)
The current waveform at the top and bottom power switches is a pulse with very high δI/δt. The paths connecting the switches should therefore be as short as possible to minimize noise picked up by the controller and noise transmitted by the inductive loop. When using a pair of DPAK or SO-8 packaged FETs on one side of the PCB, it is best to rotate the two FETs in opposite directions so that the switch node is on one side of the pair. Use a suitable ceramic bypass capacitor to bypass the high-side drain current to the low-side source. Place the bypass capacitor as close as possible to the MOSFETs (see Figure 1) to minimize the inductance around the loop formed by the FETs and the capacitor.
The placement of the input bypass capacitor and the bulk input capacitor is critical for controlling ground bounce. The negative terminal of the output filter capacitor should connect as close as possible to the source of the low-side MOSFET. This helps reduce the loop inductance that causes ground bounce. Cb1 and Cb2 in Figure 2 are ceramic bypass capacitors; the recommended range for these capacitors is 1 μF to 22 μF. For high-current applications, add a larger filter capacitor in parallel, as shown by CIN in Figure 1.
Thermal Considerations and Ground Planes
Under heavy-load conditions, the power MOSFETs, inductor, and large capacitors generate substantial heat through their equivalent series resistance (ESR). For effective heat dissipation, the example in Figure 1 places large copper areas beneath these power devices.
A multilayer PCB dissipates heat better than a 2-layer PCB. To improve both thermal and conductive performance, use 2 oz copper on standard 1 oz copper layers. Multiple PGND layers connected together with vias also help. Figure 2 shows a 4-layer PCB design with PGND planes on the top, third, and fourth layers.

Figure 2 | Cross-sectional view: connecting the PGND layer to improve heat dissipation
This multi-ground-plane approach isolates noise-sensitive signals. As shown in Figure 3, the negative terminals of the compensation components, soft-start capacitor, bias input bypass capacitor, and output feedback divider resistors all connect to the AGND plane. Do not connect any high-current or high δI/δt path directly to the isolated AGND plane. AGND is a quiet ground plane in which no large current flows.
The negative terminals of all power devices, such as the low-side switch, bypass capacitors, input capacitor, and output capacitor, connect to the PGND plane. This plane carries the high current.
Voltage drop within the GND plane can be large enough to affect output accuracy. A wide trace connects the AGND plane to the negative terminal of the output capacitor, which can significantly improve output accuracy and load regulation.

Figure 3 | Connection from the AGND layer to the PGND layer
The AGND plane extends all the way to the output capacitor, and the AGND and PGND planes connect to vias at the negative terminal of the output capacitor.
Figure 3 shows another technique for connecting the AGND and PGND planes: the AGND plane connects to the PGND plane through vias near the negative terminal of the output bulk capacitor.
Current-Sense Paths
To prevent interference noise from degrading accuracy, the current-sense path of a current-mode switching regulator must be laid out properly. Dual-channel applications require particular attention so that any crosstalk between channels is eliminated.
The ADP1850 dual-channel buck controller uses the on-resistance of the low-side MOSFET, RDS(ON), as part of its control-loop architecture. This architecture senses the current flowing through the low-side MOSFET between the SWx and PGNDx pins. Ground-current noise in one channel can couple into the adjacent channel. Therefore, make the SWx and PGNDx traces as short as possible and place them close to the MOSFET for accurate current sensing. Connections to the SWx and PGNDx nodes must use Kelvin sensing, as shown in Figure 2 and Figure 4. Note that the corresponding PGNDx trace connects to the source of the low-side MOSFET. Do not arbitrarily connect the PGND plane to the PGNDx pin.

Figure 4 | Grounding techniques for two channels
By contrast, for dual-channel voltage-mode controllers such as the ADP1829, the PGND1 and PGND2 pins connect directly to the PGND plane through vias.
Feedback and Current-Limit Sense Paths
The feedback (FB) and current-limit (ILIM) pins are low-signal-level inputs, so they are sensitive to capacitive and inductive noise interference. FB and ILIM traces should avoid high δI/δt traces. Do not let traces form loops, which increase unwanted inductance. Adding a small MLCC decoupling capacitor, such as 22 pF, between ILIM and PGND helps filter noise further.
Switch Node
In a switching regulator circuit, the switch (SW) node is the noisiest point because it carries large AC and DC voltage and current. The SW node needs a large copper area to minimize resistive drop. Placing the MOSFETs and inductor close together on the copper layer minimizes series resistance and inductance.
Applications that are more sensitive to electromagnetic interference, switch-node noise, and ringing can use a small snubber. The snubber consists of a resistor and capacitor in series (RSNUB and CSNUB in Figure 5) placed between the SW node and the PGND plane. It reduces ringing and electromagnetic interference on the SW node. Note that adding a snubber may reduce overall efficiency slightly by 0.2% to 0.4%.

Figure 5 | Snubber and gate resistors
Gate-Driver Paths
The gate-drive traces (DH and DL) also handle high δI/δt and often produce ringing and overshoot. These traces should be as short as possible. Direct routing is preferred, and feed-through vias should be avoided. If vias are required, use two vias per trace to reduce peak current density and parasitic inductance.
A small series resistor on the DH or DL pin, approximately 2 Ω to 4 Ω, can slow the gate drive and reduce ringing. During layout, reserve space for a 0 Ω gate resistor to preserve flexibility for later evaluation. The added gate resistance extends the gate-charge rise and fall times, which increases the MOSFET switching power loss.
Summary
Understanding the current paths, their sensitivity, and proper device placement is the key to eliminating noise problems in PCB layout. The layout principles described above are used on power-device evaluation boards to achieve best performance. Evaluation board documentation UG-204 and UG-205 describes the ADP1850 layout in detail.
All switching power supplies have the same types of components and similar current-path sensitivities. Therefore, the guidelines illustrated with the ADP1850 current-mode buck regulator also apply to voltage-mode and/or boost switching-regulator layouts.
Conclusion
There is no simple answer to the question of how to handle AGND and PGND grounding. Therefore, the discussion continues. Earlier we noted that many switching regulator users adopt the board layout and grounding connection type from the example circuits provided by IC manufacturers. This is useful because you can usually assume that the manufacturer also tested each IC with that configuration. Moreover, as can be seen in the examples provided in Figure 1 and Figure 2, the respective IC pinouts are suitable for local ground connections next to PGND and AGND, or for separate grounding. In practice, the manufacturer's layout should be treated as a proven starting point, not as a universal rule for every board.
Related Reading:
Eight Layout Considerations for Differential Filters on PCBs
Improving PCB Immunity to Power Supply Variations in Converter Systems
PCB Layout for Accurate Temperature Measurement: PCB vs Ambient
Best Grounding Practices for Data Converters: Return Paths and Error Voltage
High-Temperature IC Packaging: Die Attach, Wire Bond, Solder and PCB
isoPower Radiated Emissions: Dense PCB Layout Guide
PCB Thermal Design: Junction Temperature and Power Dissipation
LFCSP Package Rework: Safe Removal and Replacement on PCBs
PBGA Rework Procedure: Removal, Pad Cleaning, Paste and Placement