Data Sheet
ADAU1463/ADAU1467
APPLICATIONS INFORMATION
BULK BYPASS CAPACITORS
AVDD PVDD IOVDD DVDD
PCB DESIGN CONSIDERATIONS
3.3V
A solid ground plane is necessary for maintaining signal
integrity and minimizing EMI radiation. If the PCB has two
ground planes, they can be stitched together using vias that are
spread evenly throughout the PCB.
+
+
+
+
10µF
10µF
10µF
10µF
Figure 85. Bulk Bypass Capacitor Schematic
Power Supply Bypass Capacitors
Component Placement
Bypass each power supply pin to its nearest appropriate ground
pin with a single 100 nF capacitor and, optionally, with an
additional 10 nF capacitor in parallel. Make the connections to
each side of the capacitor as short as possible, and keep the trace
on a single layer with no vias. For maximum effectiveness, place
the capacitor either equidistant from the power and ground pins
or, when equidistant placement is not possible, slightly nearer to
the power pin (see Figure 83). Establish the thermal connections
to the planes on the far side of the capacitor.
Place all 100 nF bypass capacitors, which are recommended
for every analog, digital, and PLL power ground pair, as near as
possible to theADAU1463/ADAU1467. Bypass each of the AVDD,
DVDD, PVDD, and IOVDD supply signals on the PCB with an
additional single bulk capacitor (10 µF to 47 µF).
Keep all traces in the crystal resonator circuit (see Figure 14) as
short as possible to minimize stray capacitance. Do not connect
any long PCB traces to the crystal oscillator circuit components
because such traces may affect crystal startup and operation.
POWER GROUND
Grounding
Use a single ground plane in the application layout. Place all
components in an analog signal path away from digital signals.
CAPACITOR
TO POWER
Exposed Pad PCB Design
The device package includes an exposed pad for improved heat
dissipation. When designing a PCB for such a package, consider
the following:
•
Place a copper layer, equal in size to the exposed pad, on all
layers of the PCB, from top to bottom. Connect the copper
layers to a dedicated copper PCB layer (see Figure 86).
TO GROUND
Figure 83. Recommended Power Supply Bypass Capacitor Layout
Typically, a single 100 nF capacitor for each power ground pin
pair is sufficient. However, if there is excessive high frequency
noise in the system, use an additional 10 nF capacitor in parallel
(see Figure 84). Place the 10 nF capacitor between the devices
and the 100 nF capacitor, and establish the thermal connections
on the far side of the 100 nF capacitor.
TOP
GROUND
POWER
BOTTOM
VIAS
COPPER SQUARES
Figure 86. Exposed Pad Layout Example—Side View
VIA TO
VIA TO
GROUND PLANE
•
Place vias such that all layers of copper are connected,
allowing for efficient heat and energy conductivity. For an
example, see Figure 87, which shows 49 vias arranged in
a 7 × 7 grid in the pad area.
POWER PLANE
100nF
10nF
Figure 84. Layout for Multiple Power Supply Bypass Capacitors
To provide a current reservoir in case of sudden current spikes,
use a 10 µF capacitor for each named supply (DVDD, AVDD,
PVDD, and IOVDD) as shown in Figure 85.
Figure 87. Exposed Pad Layout Example—Top View
For detailed information, see the AN-772 Application Note,
A Design and Manufacturing Guide for the Lead Frame Chip
Scale Package (LFCSP).
Rev. A | Page 203 of 207