The PCB layout of any DC/DC converter is critical
to the excellent 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 EMI-critical PCB
feature is the loop formed by the input capacitor or capacitors and power ground.
This loop is shown in Figure 8-70. This loop carries large transient currents that can cause large transient
voltages when reacting with the trace inductance. Excessive transient voltages can
disrupt the proper operation of the converter. Because of this, the traces in this
loop must be wide and short while keeping the loop area as small as possible to
reduce the parasitic inductance. Figure 8-71 shows a recommended layout for the critical components of the LM644A2-Q1 circuit.
- Place the input capacitor or capacitors as close as
possible to the input pin pairs: VIN1 to PGND1 and VIN2 to PGND2.
Place the small capacitors closest. Each pair of pins are adjacent,
simplifying the input capacitor placement. With the QFN package, there are
two VIN/PGND pairs on either side of the package. This provides a
symmetrical layout and helps minimize switching noise and EMI generation.
Use a wide VIN plane on a mid-layer to connect both of the VIN pairs
together to the input supply. Route symmetrically from the supply to each
VIN pin to best use the benefits of the symmetric pinout.
- Place the bypass capacitor for VCC close to the VCC pin
and AGND pin: This capacitor must be routed with short, wide traces
to the VCC and AGND pins.
- Place the CBOOT capacitors as close as possible to the
device with short, wide traces to the CBOOT and SW pins: Make sure
to route the SW connection with a short wide trace to handle the current,
but not longer than necessary to avoid generating common mode noise.
- Place the feedback divider as close as possible to the
FB pin of the device: Place RFBB, RFBT,
CFF if used, and RFF if used, physically close to
the device. The connections to FB and AGND through RFBB must be
short and close to those pins on the device. The connection to
VOUT 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.
- Make layer 2 of the PCB a ground plane: This plane
acts as a noise shield and as a heat dissipation path. Using layer 2 reduces
the enclosed area in the input circulating current in the input loop,
reducing inductance.
- Provide wide paths for VIN, VOUT,
and GND: These paths must be as wide and direct as possible to
reduce any voltage drops on the input or output paths of the converter to
maximize efficiency.
- Provide enough PCB area for proper heat sinking:
Enough copper area must be used to make sure a low RθJA,
considering 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. Note that the
package of this device dissipates heat through all pins. Wide traces can be
used for all pins except where noise considerations dictate minimization of
area.
- Keep the 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.