Discrete capacitors can be used to effectively filter power supply noise up to 250 MHz. For discrete capacitors,
the footprint and physical size have a significant effect on the frequencies in which the capacitors provide effective
de-coupling. To minimize series inductance, use smaller-packaged ceramic capacitors (
such as
0402 or 0201).
Use a mixed selection of capacitor values,
such as
1.0 uF to 0.001 µF, to lower the impedance across a wide
frequency range. It is best to decouple each power ball with an 0201 size capacitor placed on the solder side of
the board, under the BGA footprint. The largest value possible (typically 1000 pF) should be used for these
capacitors. Larger value caps (1.0 to 0.01 uF) can be used around the periphery of the device to decouple the
lower frequency noise. The smaller values should be placed closest to the device. Multi-layer ceramic chip
capacitors (
such as
10 to 22 µF) can be used for bulk de-coupling of lower-frequency components. The proximity
of these capacitors is not critical; therefore, they can be placed well outside the BGA matrix if necessary.
Capacitor footprint layout is important in determining the frequencies at which they are effective. Avoid adding
trace segments from the capacitor pads to the vias. These segments add more series inductance, thereby
lowering the discrete capacitor LC resonant frequency. Place the vias tangentially to the capacitor pads, and if
possible, add multiple vias per pad. (Refer to
Right the First Time: A Practical Handbook on High Speed PCB and
System Design,
by Lee Ritchie). If a plane capacitor is not possible (this is typically the case for 4- and 6-layer
boards), add power or ground fill areas on the signal layers, as follows:
If a signal layer is referencing a DC ground plane, fill with power
If a signal layer is referencing a DC power plane, fill with ground
These copper fill areas tie to the main power and ground planes, through the component balls.
illustrates examples of how various footprints for 0603-size capacitors can change series inductance.
Figure 16. Capacitor Footprint Effects on Series Inductance
It is strongly recommended to measure the attenuation-versus-frequency profile of each power rail on a
completed board that is loaded only with bypass capacitors (a VNA can be used for this). This serves to confirm
that there are no attenuation holes in the power-de-coupling design. If holes do exist, capacitor values of some of
the capacitors can be adjusted to fill them.
PEX 8618 Quick Start Hardware Design Guide – Version 1.2
Copyright © 2009 by PLX Technology, Inc. All rights reserved.
20
