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 capacitors and power ground, as shown in Figure 8-19. 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 disruption, the traces in this loop must be wide and short, and the loop area as small as possible to reduce the parasitic inductance. Figure 8-20 shows a recommended layouts for the critical components of the LM63635-Q1.

1. Place the input capacitors as close as possible to the VIN and PGND terminals. VIN and PGND pins are adjacent, simplifying the input capacitor placement. TI does not recommend thermal reliefs in this area.
2. Place a bypass capacitor for VCC close to the VCC pin. Place this capacitor close to the device and routed with short, wide traces to the VCC and PGND pins. TI does not recommend thermal reliefs in this area.
3. Use wide traces for the C_BOOT capacitor. Place C_BOOT close to the device with short and wide traces to the BOOT and SW pins. TI does not recommend thermal reliefs in this area.
4. Place the feedback divider as close as possible to the FB pin of the device. If an external feedback divider is used with the ADJ option, place R_FBB, R_FBT, and C_FF close to the device. The connections to FB and AGND 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. Connect the thermal pad to the ground plane. The thermal pad (DAP) connection must be soldered down to the PCB ground plane. This pad acts as a heat-sink connection and an electrical ground connection for the regulator. The integrity of this solder connection has a direct bearing on the total effective R_θJA of the application. TI does not recommend thermal reliefs in this area.
7. Provide wide paths for VIN, VOUT, SW, and PGND. 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. TI does not recommend thermal reliefs in this area.
8. Provide enough PCB area for proper heat-sinking. As stated in Section 8.2.2.8, enough copper area must be used to make sure of a low R_θJA, commensurate with the maximum load current and ambient temperature. The top and bottom PCB layers must be made with 2oz copper and no less than one ounce. Use an array of heat-sinking vias to connect the thermal pad (DAP) to the ground plane on the bottom PCB layer. If the PCB design uses multiple copper layers (recommended), these thermal vias can also be connected to the inner layer heat-spreading ground planes.
9. 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.

See the following PCB layout resources for additional important guidelines:

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

Figure 8-19 Current Loops With Fast Edges