Login
Register

ENGLISH简体中文
(Chinese)日本語
(Japanese)РУССКИЙ
(Russian)

Products

Solutions

Design

Buy

Support

About Us

My Maxim

Maxim > Design
support > App notes
> Audio
Circuits > APP 4079

Sep 04, 2007

Keywords: layout, pcb, rf immunity, tdma noise,
rf susceptibility, emc

Download,
PDF format (71kB)

[?]

APPLICATION NOTE 4079

Minimize Noise in Audio Channels with Smart PCB
Layout

Abstract: This
application note discusses several factors that affect audio
functionality in a cell-phone PCB design. The article shows
examples of a problematic and a well-designed PCB for a cell
phone. The differences between the two layouts are discussed,
with emphasis given to design considerations that improve
audio function.

Attend
this brief webcast by Maxim on
TechOnline

Introduction
For PCB
layout engineers, cell phones provide the ultimate challenge.
Each subsystem has conflicting requirements, and modern cell
phones include nearly every subsystem found in a portable
device. A well-designed PCB must both maximize the performance
of each device connected to it and prevent the various
subsystems from interfering with each other. Inevitably, the
conflicting requirements of each subsystem result in some
compromise. Finally, although audio functionality in cell
phones is increasing, the audio circuitry is often given the
least consideration during PCB design.

Component Placement
The first step of any PCB design
is choosing where to place the components. This task is called
"floor planning." Careful component placement can ease signal
routing and ground partitioning. It minimizes noise pickup and
the board area required.

Cell phones contain a mixture
of digital and analog
circuitry that must be separated to prevent noise from the
digital portion from interfering with the sensitive analog
circuits. Partitioning the PCB into a digital and an analog
region simplifies the separation task.

The RF section
of a cell phone is typically considered analog. Yet there is a
common problem in many cell-phone designs where noise coupled
from the RF section into the audio circuitry is demodulated
into audible noise. To prevent this, the RF and audio sections
should be separated as much as possible.

Once the PCB
has been partitioned into analog, digital, and RF sections,
the component placement within the analog section must be
selected. Components should be placed to minimize the distance
that audio signals travel. Locate the audio amplifier
as close to the headphone jack and loudspeaker as possible.
This positioning will minimize EMI
radiation from Class
D speaker amplifiers, and minimize the noise
susceptibility of low-amplitude headphone signals. Place the
devices supplying the analog audio as close to the amplifier
as possible to minimize noise pickup on the amplifier inputs.
All input signal traces will act as antennas to RF signals,
but shortening the traces helps reduce the antenna efficiency
for frequencies typically of concern.

Example Component Placement
Figure 1 shows an
example of poor audio component placement. The most serious
problem is that the audio amplifier is placed quite far from
the audio sources. This distance increases the chances of
noise coupling because the traces are more prone to pass near
noisy digital circuitry. The long traces can also be efficient
RF antennas. In cell phones using GSM
technology, these antennas can pick up the GSM transmission
and feed the signal into the audio amplifier. Nearly all
amplifiers will demodulate the 217Hz envelope to some degree
and generate unwanted noise on the output. In the worst case,
this process causes noise on the output that completely
overwhelms the desired audio signal. Minimizing input trace
lengths thus prevents the signal from ever reaching the
amplifier.

There is another problem with the component
placement in Figure 1: the amplifier is not placed near the
speaker and the headphone jack. If the speaker amplifier is
Class D, then the long speaker traces increase the EMI
radiation from the amplifier. This radiation could potentially
prevent the device from passing government-mandated testing.
The long headphone and speaker output traces both increase the
trace resistance,
thus decreasing the power delivered to the
load.

Finally, since the components are so spread
apart, the traces connecting the components will be routed
near other subsystems in the phone. Not only does this
distance increase the difficulty of routing the traces, but it
also increases the difficulty of laying out other parts of the
phone.

Figure
1. Example of poor component placement in a cell
phone.

Figure 2 shows the same components as
Figure 1, but rearranged to use the space more effectively and
to minimize trace lengths. Notice how all the audio circuitry
has been partitioned to be near the headphone jack and the
speaker. The audio input and output traces are much shorter
and the nonaudio circuitry has been moved to a different part
of the PCB. This design will have lower overall system noise,
be less susceptible to RF interference, and be easier to
layout.

Figure
2. Example of good component placement in a cell
phone.

Signal Routing
When considering noise and distortion
on the audio output, signal routing typically has limited
impact. There are, nonetheless, some steps to ensure that
performance is not compromised.

Loudspeaker amplifiers
typically are powered directly from the main system voltage
and require relatively high current.
Resistance in the trace will result in voltage drops that
reduce the supply voltage of the amplifier and waste power in
the system. The trace resistance also causes the normal
fluctuations in supply current to convert to fluctuations in
voltage. To maximize performance, use short wide traces for
all amplifier power supplies.

Differential
signaling is an advantage that should be exploited
whenever possible. Differential inputs provide noise immunity
by rejecting any signal that is common to the positive and
negative signal lines. There are several considerations to
ensure that the differential amplifier is effective.
Specifically, it is important that the differential signal
pairs have the same length and the same impedance.
The signal pairs should be routed as close to each other as
possible to ensure that they pick up the same noise.
Differential inputs on amplifiers are particularly effective
in reducing noise from the digital circuits in the
system.

Grounding
Grounding plays the single, most significant
role in determining whether the device's potential is achieved
by the system. A poorly grounded system will likely have high
distortion, noise, crosstalk,
and RF susceptibility. Although one can question how much time
should be devoted to system grounding, a carefully designed
grounding scheme prevents a large number of problems from ever
occurring.

The ground in any system must serve two
purposes. First, it is the return path for all currents
flowing to a device. Second, it is the reference voltage for
both digital and analog circuits. Grounding would be a simple
exercise if the voltage at all points of the ground could be
the same. In reality, this is not possible. All wires and
traces have a finite resistance. This means that whenever
there is current flowing through the ground, there will be a
corresponding voltage drop. Any loop of wire also forms an
inductor. This means that whenever current flows from the
battery to a load, and back to the battery, the current path
has some inductance. The inductance increases the ground
impedance at high frequencies.

While designing the best
ground system for a particular application is no simple task,
some general guidelines do apply to all systems.

Establish a Continuous Ground Plane for Digital
Circuits
Digital current in the ground plane tends to
follow the same route that the original signal took. This
path creates the smallest loop area for the current, thus
minimizing antenna effects and inductance. The best way to
ensure that all digital signal traces have a corresponding
ground path is to establish a continuous ground plane on the
layer immediately adjacent to the signal layer. This layer
should cover the same area as the digital signal trace and
have as few interruptions in its continuity as possible. All
interruptions in the ground plane, including vias, cause the
ground current to flow in a larger loop than is ideal,
thereby increasing radiation and noise.

Keep Ground Currents Separate
The ground currents
for digital and analog circuits must be separated to prevent
digital currents from adding noise to the analog circuits.
The best way to accomplish this is through correct component
placement. If all the analog and digital circuits are placed
on separate parts of the PCB , the ground currents will
naturally be isolated. For this to work well, the analog
section must contain only analog circuits on all layers of
the PCB.

Use the Star Grounding Technique for Analog
Circuits
Star grounding uses a single point on the
PCB as the official ground point. This point, and only this
point, can be considered to be at ground potential. In a
cell phone the battery ground terminal is a logical choice
for the star
point. Do not think of currents as flowing into the
ground plane and disappearing; rather consider all ground
currents as flowing back to this ground point.

Audio
power amplifiers tend to draw relatively large currents that
can adversely affect both their own and other ground
references in the system. To prevent this problem, provide
dedicated return paths for bridged-amplifier power grounds
and headphone-jack ground returns. Isolation allows these
currents to flow back to the battery without affecting the
voltage of other parts of the ground plane. Remember that
these dedicated return paths should not be routed under
digital signal traces because they could block the digital
return currents.

Maximize the Effectiveness of Bypass
Capacitors
Nearly all devices require bypass
capacitors to provide instantaneous current. To minimize the
inductance between the capacitor and the device supply pin,
locate these capacitors as close as possible to the supply
pin which they are bypassing. Any inductance reduces the
effectiveness of the bypass capacitor. Similarly, the
capacitor must be provided a low-impedance connection to
ground to minimize the capacitor's high-frequency impedance.
Directly connect the ground side of the capacitor to the
ground plane, rather than routing it through a trace.

Flood All Unused PCB Area with Ground
Whenever
two pieces of copper run near each other, a small capacitive
coupling is formed between them. By running ground flood
near signal traces, unwanted high-frequency energy in the
signal lines can be shunted to ground through the capacitive
coupling.

Example Grounding
Figure 3 shows an example of
a well-grounded system. Note, first, that the PCB is
partitioned into a digital section at the bottom and an analog
section at the top. The only signals crossing the partition
boundary are I²C control signals, and these have a direct
return path following the signal trace. This layout ensures
that digital signals will remain in the digital section of the
board and that no digital ground currents will be blocked by
the splits in the ground plane. Also note that most of the
ground plane is uninterrupted. Even in the digital section
where there are interruptions, they are far enough apart to
allow currents to flow freely.

For this example the
star point is in the upper left corner of the PCB. The breaks
in the analog portion of the ground plane allow the Class D
and charge-pump currents to return to the star point without
interfering with the general analog ground plane. Also note
that the headphone jack has a dedicated trace returning the
headphone ground current to the star point.

Figure
3. Example of a silkscreen and ground layer of a well-grounded
design.

Conclusion
Although creating a well-designed PCB can
be time-consuming and challenging, the investment is well
worth the time spent. The end result is a system with less
noise, higher immunity to RF signals, and less distortion. The
PCB will also have better EMI performance and may require less
shielding.

Ultimately, if the PCB is not carefully
designed, preventable problems will be discovered when the
product is in test. These problems are much more difficult to
fix once the layout is complete, and often demand significant
time to correct. All too often the fixes require additional
components that add to the total system cost and
complexity.

An abbreviated version of this application
note appeared in the July 16, 2007 issue of EE Times, a
CMP publication.

Automatic updates
Would you like to be
automatically notified when new application notes are
published in your areas of interest? Sign
up for EE-Mail™.

Download,
PDF format (71kB)
APP 4079: Sep 04, 2007

AN4079, AN 4079, APP4079,
Appnote4079, Appnote 4079

|

|

|     Privacy Policy
|     Legal Notices

Copyright © 2011 by Maxim Integrated
Products