11.1.1 Feedback Traces

Run the feedback trace as far from the inductor and noisy power traces as possible. The feedback trace should be as direct as possible and somewhat thick, which sometimes involves a trade-off, but keeping the feedback trace away from inductor EMI and other noise sources is more critical. Run the feedback trace on the side of the PCB opposite of the inductor with a ground plane separating the two.

11.1.2 Input/Output Capacitors

When using a low-value ceramic input filter capacitor, it must be located as close as possible to the VIN pin of the IC. This will eliminate as much trace inductance effects as possible and give the internal IC rail a cleaner voltage supply. Some designs require the use of a feed-forward capacitor connected from the output to the feedback pin as well, usually for stability reasons. In this case, it must also be positioned as close as possible to the IC. Using surface-mount capacitors also reduces lead length and lessens the chance of noise coupling into the effective antenna created by through-hole components.

11.1.3 Compensation Components

External compensation components for stability must also be placed close to the IC. Surface mount components are recommended here as well for the same reasons discussed for the filter capacitors. Locate the surface-mount components away from the inductor.

11.1.4 Traces and Ground Planes

Make all of the power (high current) traces as short, direct, and thick as possible. It is good practice on a standard PCB board to make the traces an absolute minimum of 15 mils (0.381 mm) per Ampere. The inductor, output capacitors, and output diode must be as close as possible to each other. This helps reduce the EMI radiated by the power traces due to the high switching currents through them. This will also reduce lead inductance and resistance as well, which in turn reduces noise spikes, ringing, and resistive losses that produce voltage errors. The grounds of the IC, input capacitors, output capacitors, and output diode (if applicable) must be connected close together directly to a ground plane. It would also be a good idea to have a ground plane on both sides of the PCB. This will reduce noise as well by reducing ground loop errors as well as by absorbing more of the EMI radiated by the inductor. For multilayer boards with more than two layers, a ground plane can be used to separate the power plane (where the power traces and components are) and the signal plane (where the feedback and compensation and components are) for improved performance. On multilayer boards, the use of vias will be required to connect traces and different planes. It is good practice to use one standard via per
200 mA of current if the trace must conduct a significant amount of current from one plane to the other. Arrange the components so that the switching current loops curl in the same direction. Due to the way switching regulators operate, there are two power states. One state when the switch is on and one when the switch is off. During each state there will be a current loop made by the power components that are currently conducting. Place the power components so that during each of the two states the current loop is conducting in the same direction. This prevents magnetic field reversal caused by the traces between the two half-cycles and reduces radiated EMI.

11.1.5 Ground Planes

Each output driver of these devices is capable of 2-A peak currents. Careful layout is essential for correct operation of the chip. A ground plane must be employed. A unique section of the ground plane must be designated for high di/dt currents associated with the output stages. This point is the power ground to which the PGND pin is connected. Power ground can be separated from the rest of the ground plane and connected at a single point, although this is not necessary if the high di/dt paths are well understood and accounted for. VCC must be bypassed directly to power ground with a good high frequency capacitor. The sources of the power MOSFET must connect to power ground as must the return connection for input power to the system and the bulk input capacitor. The output must be clamped with a high current Schottky diode to both VCC and PGND. Nothing else should be connected to power ground.

VREF must be bypassed directly to the signal portion of the ground plane with a good high frequency capacitor. TI recommends low ESR/ESL ceramic 1-mF capacitors for both VCC and VREF. All analog circuitry must likewise be bypassed to the signal ground plane. See Figure 25.