Analysis of a speaker using
Abaqus-Dymola
co-simulation
This example illustrates the use of the co-simulation technique to
couple system-level logical models and functional-level models in
Dymola
with a physical model in
Abaqus/Explicit.
Mobile devices like tablets and smart phones are increasingly becoming an
important part of our lifestyle. One of the critical features that determines
the overall quality of such a device is the audio quality of the speaker. The
most commonly used speaker in mobile devices is based on the principle of
moving coil transduction, as described by Jackman et al. (2009). An
electromagnetic field applied on the voice coil generates a mechanical driving
force (known as the Lorentz force) that generates the sound by imparting motion
to the diaphragm. There are several key design challenges in the selection of
the transducer and its placement. Some of the important issues to be addressed
in the audio system design are discussed below.
Audio system design
The mobility and lightness of the device are major considerations, and space
is at a premium. Providing many features in a mobile device requires numerous
components, and packaging plays a critical role as these components compete for
the limited available space. The smaller the audio speaker, the poorer its bass
response. The enclosure behind the diaphragm in the speaker (referred to as the
“back volume”) has a major influence on the speaker performance; it affects the
audio quality by introducing cavity resonances at high frequencies and by
reducing the compliance at low frequencies. In other words, the smaller the
back volume, the lower the quality of the low frequency (bass) sound output.
The designer must take measures to maximize the back volume, conforming to the
packaging needs of the device in addition to providing an excellent bass audio
quality.
The audio quality is reduced due to the inherent nonlinearities such as the
total harmonic distortion. Even for microspeakers with very low diaphragm
motions or excursions, the nonlinearities due to the mechanical resistance at
the restraints (in addition to acoustic losses in ports) tend to be dominant.
The nonlinearities are guided not so much by the displacement but by the
velocity of the diaphragm excursion (Klippel and Knobloch, 2013). Hence, there
is a need to model the nonlinearities that can be appropriately modeled in the
time domain to reproduce the physically accurate solution. Simulating the audio
response as a harmonic analysis in the frequency domain may provide inaccurate
results, especially at higher levels of nonlinearity.
For transducer design it is important to have a flat frequency response
while making sure that the sound output is as large as possible without
distortions. The first resonant mode (along with the damping) sets the maximum
for the sound output. The flat frequency response (at least in the
mid-frequency range; e.g., 1000–6000 Hz) is ensured by shifting the second
resonance peak as far away as possible from the first resonance peak.
Interaction through the co-simulation technique
This example discusses a methodology that simulates the diaphragm excursion
(and the subsequent acoustic response) due to electromagnetic excitation as a
transient problem. The electromagnetic circuit of the speaker is assumed to
have no direct contribution to the structural response of the system and,
hence, is modeled independently as a reduced-order logical system in
Dymola.
The structural-acoustic response of the diaphragm in the speaker assembly is
modeled with its full three-dimensional finite element representation in
Abaqus/Explicit.
The
Abaqus
model and the
Dymola
model interact with each other through the co-simulation technique in the time
domain.
Abaqus
model
The
Abaqus
model of the speaker is shown in
Figure 1.
Features such as very short edges or small faces, although important for
machining and packaging of a component, have almost no bearing on the mechanics
of the problem. Including such features in the numerical analysis could result
in a very fine mesh density, leading to increased computation time. Such minor
geometric details are excluded by combining the feature with an adjacent larger
feature. Nodes and elements are created to conform to the original geometry.
The diaphragm occupies the region in between the front volume and the speaker’s
back volumes, as shown in
Figure 1.
Symmetric notches and the racetrack-like separation between the center and the
annulus region in the diaphragm (shown in
Figure 2)
are designed to achieve the flat frequency response and the first resonant
peak, respectively. The other speaker components that hold the diaphragm in
place are considered rigid and are not modeled. The radius of the hemispherical
acoustic domain corresponds to one-third of the largest acoustic wavelength.
Additional details on the modeling of the speaker are described in Jackman et
al. (2009).
Dymola
model
The electromagnetic component of the speaker, which functions primarily in
the low frequency range, can be idealized with a lumped-parameter model in
Dymola,
as shown in
Figure 3.
The advantage of using a lumped-parameter model is twofold; it simplifies the
modeling and improves the performance dramatically. The electromagnetic part of
the model is assumed to have a linear response to the electromagnetic
excitation; hence, it is modeled with a resistor and an inductor. The current
sensor output from
Dymola
is used as an actuator in
Abaqus,
and the velocity output of the sensor from
Abaqus
is used as an actuator in calculating the back electromotive force
(EMF) in the system-level functional model.
Abaqus modeling approaches and simulation techniques
Two cases are studied. The first case analyzes loading with a white noise
signal to check the drop in the signal amplitude over the audible frequency
range. The second case analyzes loading with a fixed frequency signal to check
the fidelity of the response of the speaker.
Summary of analysis cases
Case 1
White noise analysis.
Case 2
Response fidelity analysis.
The sections that follow discuss the analysis considerations that are
applicable for both cases.
Analysis Techniques
Abaqus-Dymola
co-simulation provides a convenient way to couple system-level logical and
functional-level models in
Dymola
with a physical model in
Abaqus.
The
Abaqus
user subroutines
UAMP and
VUAMP can be used to design such system-level models interacting
with physical models, but the user is required to manually code the user
subroutine.
Dymola
provides a host of libraries that have components belonging to different
engineering domains (such as fluid, thermal, and electromagnetic) as well as
mathematical operators (such as controllers and Boolean operators) that can be
easily dragged and dropped as icons into a user interface to build the
system-level model. Co-simulation with
Abaqus
involves passing the state of the physical system in
Abaqus
as sensor data to Real Input interfaces in
Dymola
while reading the Real Output interfaces from
Dymola
into
Abaqus
as actuators. For more details about co-simulation, refer to
System-Level Modeling between Logical and Physical Interactions.
Mesh design
The diaphragm is modeled with reduced-integration conventional shell
elements (S3R and S4R), and its rim is meshed with first-order reduced-integration
hexahedral continuum elements (C3D8R). Modeling the diaphragm with solid elements instead of shell
elements allows the acoustic domain to be cut away more easily. The acoustic
domain, both in the back volume and the volume exterior to the diaphragm, is
modeled with three-dimensional continuum acoustic linear tetrahedral elements (AC3D4). The mesh of the acoustic domain is nonuniform, with the largest
element size being less than one-eighth of the shortest acoustic wavelength.
Materials
The units used in the
Abaqus
model are mm-tonnes-sec, and SI units are used
in
Dymola.
The diaphragm material in
Abaqus
is polyimide (Young's modulus=3677; density=1.4 × 10−9; structural
damping=1.5); the voice coil is made of steel (Young's modulus=110,000;
Poisson's ratio=0.3; density=3.3 × 10−9); while the air is modeled
as the acoustic medium (bulk modulus= 0.142; density=1.2 × 10−12).
The electromagnetic circuit in
Dymola
has a resistor of 5 ohms, an inductor of 5 × 10−5 H, and a coupling
factor of 3.14159 N/A.
Boundary conditions
Boundary conditions are not applied to the acoustic regions that are in
contact with the surfaces of the speaker components to enforce the rigid
assumption that an
Abaqus
acoustic domain without any boundary condition is assumed to be a rigid
termination. The surface impedance for the nonreflecting spherical boundary of
the acoustic medium is defined as 550.
Constraints
The structural and acoustic media are coupled through tie constraints. The
diaphragm's rim is rendered rigid with its reference point at the center of the
rim.
Output requests
The component of the translational velocity of the reference node of the
rigid rim of the diaphragm along the direction perpendicular to the
hemispherical flat surface of the acoustic medium is declared as a sensor. This
sensor output from the diaphragm is passed into
Dymola
as an input signal. The pressure at a certain location in the front volume
acoustic medium is also stored as history output.
Run procedure
The
Abaqus
model can be run on any supported platform (Windows/Linux), whereas the
Dymola
portion of the co-simulation can be run only on Windows 64-bit platforms. For
more details on how to submit an
Abaqus-Dymola
co-simulation job, please refer toSystem-Level Modeling between Logical and Physical Interactions.
You can use the abaqus fetch utility to obtain the
Dymola FMU files for the examples using the following
commands:
abaqus fetch job=EMsystem_cosim_white_noise.fmu
abaqus fetch job=EMsystem_cosim_frequency.fmu
Case 1: White noise analysis
This case analyzes loading with a white noise signal to check the drop in the signal amplitude
over the audible frequency range.
Analysis Techniques
A concentrated force with amplitude as white noise is applied on a rigidly
fixed dummy node, and a sensor of this concentrated force at this node is
passed from
Abaqus
into
Dymola
as an input value.
Loads
A white noise signal voltage of unit magnitude is applied through a sensor
on a dummy node in
Abaqus,
as mentioned above.
Solution controls
This analysis is run for a duration of 0.03 s, thereby setting a threshold
frequency of 33 Hz as the lower limit for the frequency range of the audio
signal to obtain an accurate response from the speaker. The models's stable
time increment of ~10−8 determines the Nyquist frequency of 1 ×
106 Hz as the higher limit for the frequency range of the audio
signal to obtain an accurate response.
Output requests
An additional sensor for a concentrated force on a dummy node along the
direction of loading is defined for transferring the white noise to
Dymola
from
Abaqus,
as mentioned above.
Case 2: Response fidelity analysis
This case analyzes loading with a fixed frequency signal to check the
fidelity of the response of the speaker.
Loads
A signal voltage of 2 mV with a frequency of 2000 Hz is applied. In
Abaqus
the reference node of the rigid rim of the diaphragm is actuated by the Lorentz
force that was computed in
Dymola.
Solution controls
This analysis with a signal frequency of 2000 Hz must be run for at least
0.005 s to obtain a steady response of the speaker for a few wavelengths of the
signal.
Discussion of results and comparison of cases
For the response fidelity analysis, the acoustic signal is reciprocated in
the diaphragm and in the air at almost 2000Hz, as shown in the velocity and
pressure plots in
Figure 4
and
Figure 5,
respectively.
Jackman, C., M.
Zampino, D. Cadge, R.
Dravida, V. Katiyar, and
J. Lewis,
“Estimating Acoustic
Performance of a Cell Phone Speaker Using Abaqus,”SIMULIA
Customer Conference, 2009.
Klippel, W., and D.
Knobloch, “Nonlinear Losses in Electro-Acoustical
Transducers,” The Association of Loudspeaker Manufacturers
& Acoustics International (ALMA), Winter
Symposium, 2013.
Radcliffe, C., and S.
Gogate, “Velocity Feedback Compensation of
Electromechanical Speakers for Acoustic Applications,”
International Federation of Automatic Control, Triennial World Congress, 1996.
Figures
Figure 1. Abaqus
model of the speaker. Figure 2. Diaphragm of the speaker in the
Abaqus
model. The highlighted red region is rendered rigid with its reference node at
the center highlighted in red. Figure 3. Dymola
model showing the electromagnetic circuit of the speaker. Figure 4. Response fidelity analysis: velocity of the reference node of the
rigid part of the diaphragm. Figure 5. Response fidelity analysis: pressure at a point in air in front of the
diaphragm.
