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 regulator 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 input capacitors, and power ground, as shown in Figure 10-1. This loop carries large transient currents that can cause large transient voltages when reacting with the trace inductance. These unwanted transient voltages will 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. Figure 10-2 shows a recommended layout for the critical components of the LMR33630-Q1.

1. Place the input capacitor or capacitors as close as possible to the VIN and GND terminals. VIN and GND pins are adjacent, simplifying the input capacitor placement. With the VQFN 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. A wide VIN plane must be used on a lower layer to connect both of the VIN pairs together to the input supply; see the layout example.
2. Place bypass capacitor for VCC close to the VCC pin. This capacitor must be placed close to the device and routed with short, wide traces to the VCC and GND pins.
3. Use wide traces for the C_BOOT capacitor. Place C_BOOT close to the device with short/wide traces to the BOOT and SW pins. It is important to route the SW connection under the device to the NC pin, and use this path to connect the BOOT capacitor to SW.
4. 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 GND 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 regulator.
5. Use at least one ground plane in one of the middle layers. This plane acts as a noise shield and also act as a heat dissipation path.
6. Provide wide paths for VIN, VOUT, and GND. Making these paths as wide and direct as possible reduces any voltage drops on the input or output paths of the converter and maximizes efficiency.
7. Provide enough PCB area for proper heat sinking. As stated in Section 8.2.2.11, 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.
8. 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 should be minimized to help reduce radiated EMI.

See the following PCB layout resources for additional important guidelines:

• Layout Guidelines for Switching Power Supplies
• Simple Switcher PCB Layout Guidelines
• Construction Your Power Supply- Layout Considerations
• Low Radiated EMI Layout Made Simple with LM4360x and LM4600x

Figure 10-1 Current Loops with Fast Edges