The switching node rise and fall times should be minimized for minimum switching loss. Proper layout of the components to minimize the high frequency current path loop (see Figure 12-1) is important to prevent electrical and magnetic field radiation and high-frequency resonant problems. The following is a PCB layout priority list for proper layout. Layout of the PCB according to this specific order is essential.

1. Place the input capacitor as close as possible to the PVCC supply and ground connections and use the shortest copper trace connection. These parts should be placed on the same layer of the PCB instead of on different layers and using vias to make this connection.
2. Place the inductor input terminal as close as possible to the SW terminal. Minimize the copper area of this trace to lower electrical and magnetic field radiation but make the trace wide enough to carry the charging current. Do not use multiple layers in parallel for this connection. Minimize parasitic capacitance from this area to any other trace or plane.
3. The charging current sensing resistor should be placed right next to the inductor output. Route the sense leads connected across the sensing resistor back to the IC in the same layer, close to each other (minimize loop area) and do not route the sense leads through a high-current path (see Figure 12-2 for Kelvin connection for best current accuracy). Place decoupling capacitor on these traces next to the IC.
4. Place the output capacitor next to the sensing resistor output and ground.
5. Output capacitor ground connections must be tied to the same copper that connects to the input capacitor ground before connecting to system ground.
6. Route analog ground separately from power ground and use a single ground connection to tie charger power ground to charger analog ground. Just beneath the IC use analog ground copper pour but avoid power pins to reduce inductive and capacitive noise coupling. Use the thermal pad as a single ground connection point to connect analog ground and power ground together, or use a 0-Ω resistor to tie analog ground to power ground. A star-connection under the thermal pad is highly recommended.
7. It is critical to solder the exposed thermal pad on the backside of the IC package to the PCB ground. Ensure that there are sufficient thermal vias directly under the IC, connecting to the ground plane on the other layers.
8. Decoupling capacitors must be placed next to the IC pins and make trace connection as short as possible.
9. The number and physical size of the vias must be enough for a given current path.