[The first article in this series explains the purpose of the low-pass filter components in Class-D amplifiers and how to calculate their values.]
PCB design can limit the performance or reduce the reliability of a class-D amplifier if some basic layout guidelines are not followed. The following describes some good PC board layout practices for class-D amplifiers. The STA517B (175 watts per channel) digital power amplifier with two BTL outputs is used as an example, but the basic concepts are the same for all class-D amplifiers.
Figure 1 - Schematic for a stereo BTL class-D power amplifier
A good ground plane is the key to a good class-D amplifier layout. The bottom side of the circuit board should be used exclusively as a ground plane if possible; a full ground plane will provide the best performing and most reliable design. If you must place signal or power traces on the bottom side of the board, keep them as short as possible. If necessary, bring the trace back to the top side of the board for a short distance to break up long traces on the bottom side.
Vias are used to connect components on the top side of the board to the ground plane on the bottom side of the board. However, vias also block current flow on the ground plane so they should be used judiciously.
The area directly beneath the amplifier should be filled with copper. If the amplifier has an exposed pad or slug on the bottom of the package, then the IC should be soldered to the ground under the amplifier so that it can act as a heat sink. In this case, the ground should extend out from underneath the IC on both sides so that it is exposed to free air. The ground under the amplifier should have many vias to conduct heat to the bottom of the board so it can be used as a heat sink as well.
Running signals underneath the amplifier is not advised. Several vias should be stitched into the ground plane to ensure that the ground points of all components have a direct, low-impedance path to each other. This is particularly important for the output filters. All of the filter grounds should have a direct path back to the ground plane underneath the amplifier.
Power Supply Bypass Capacitors
Power supply bypass capacitors are extremely important for insuring reliability and preventing noise and crosstalk. The amplifier output stages draw large amounts of current and switch on and off very quickly. The parasitic inductance between the bypass capacitors and the amplifier power supply inputs can generate large spikes when the output switches, therefore the parasitic inductance must be kept as small as possible. A 100nf capacitor should be used in parallel with a 1µf capacitor on each of the supply inputs for the amplifier power stage to minimize the impact of resonance between the stray inductance and the bypass capacitors.
The 100nf capacitors should be located as close as possible to the IC (no more than 2 mm away). They should also be on the same layer as the IC to minimize the total path length (and stray inductance) as shown in figure 1. The 1µf capacitors should be placed next, as close as possible to the 100nf capacitors.
Figure 2 - Using the bottom side of the board for the 100nf capacitor ground connection can lengthen the total trace length considerably and have a negative effect on circuit performance.
Large bulk storage capacitors should also be used to decouple the amplifier from the power supply. The value of the bulk storage capacitors will depend on the amount of current required by the amplifier. The bulk storage capacitors should have star connections to the amplifier and the power supply and they should be located as close to the amplifier as possible (ideally less than 30mm).
Figure 3 - The 100nf bypass caps should be placed closest to the IC.
Figure 4 - The 1uf caps should be placed after the 100nf caps. Vias connect the 1uf caps to the ground plane on the bottom of the board.