The PCB layout of any DC-DC converter is critical to the optimal performance of the design. Bad PCB layout can disrupt the operation of an otherwise good schematic design. Even if the converter regulates correctly, bad PCB layout can mean the difference between a robust design and one that cannot be mass produced. Furthermore, the EMI performance of the converter is dependent on the PCB layout, to a great extent. In a buck converter, the most critical PCB feature is the loop formed by the input capacitor or capacitors and power ground, as shown in Figure 11-1. This loop carries large transient currents that can cause large transient voltages when reacting with the trace inductance. These unwanted transient voltages disrupt the proper operation of the converter. Because of this, the traces in this loop must be wide and short, and the loop area as small as possible to reduce the parasitic inductance.

• Place the input capacitor or capacitors as close as possible input pin pairs: VIN1 to PGND1 and VIN2 to PGND2. Each pair of pins are adjacent, simplifying the input capacitor placement. With the VQFN-HR package, there are two VIN/PGND pairs on either side of the package. This provides for a symmetrical layout and helps minimize switching noise and EMI generation. Use a wide VIN plane on a lower layer to connect both of the VIN pairs together to the input supply.
• Place bypass capacitor for VCC close to the VCC pin and AGND pins: This capacitor must routed with short, wide traces to the VCC and AGND pins.
• Use wide traces for the CBOOT capacitor: Place the CBOOT capacitor as close to the device with short, wide traces to the CBOOT and SW pins. It is important to route the SW connection under the device through the gap between VIN2 and RBOOT pins, reducing exposed SW node area. If an RBOOT resistor is used, place as close as possible to CBOOT and RBOOT pins. If high efficiency is desired, RBOOT and CBOOT pins can be shorted. This short must be placed as close as possible to RBOOT and CBOOT pins as possible.
• Place the feedback divider as close as possible to the FB pin of the device: Place R_FBB, R_FBT, and C_FF, if used, physically close to the device. The connections to FB and AGND through R_FBB must be short and close to those pins on the device. The connection to V_OUT can be somewhat longer. However, this latter trace must not be routed near any noise source (such as the SW node) that can capacitively couple into the feedback path of the converter.
• Layer 2 of the PCB must be a ground plane: This plane acts as a noise shield and a heat dissipation path. Using layer 2 reduces the inclosed area in the input circulating current in the input loop, reducing inductance.
• Provide wide paths for V_IN, V_OUT, and GND: These paths must be wide and direct as possible to reduce any voltage drops on the input or output paths of the converter and maximizes efficiency.
• Provide enough PCB area for proper heat sinking: Enough copper area must be used to ensure a low R_θJA, commensurate with the maximum load current and ambient temperature. Make the top and bottom PCB layers with two-ounce copper and no less than one ounce. If the PCB design uses multiple copper layers (recommended), thermal vias can also be connected to the inner layer heat-spreading ground planes. Note that the package of this device dissipates heat through all pins. Wide traces must be used for all pins except where noise considerations dictate minimization of area.
• Keep switch area small: Keep the copper area connecting the SW pin to the inductor as short and wide as possible. At the same time, the total area of this node must be minimized to help reduce radiated EMI.

Figure 11-1 Input Current Loop