Acoustic, Shock, and Coupled Acoustic-Structural Analysis
Analyses performed using acoustic elements, an acoustic medium,
and a dynamic procedure can simulate a variety of engineering phenomena
including low-amplitude wave phenomena involving fluids such as air and water
and “shock” analysis involving higher amplitude waves in fluids interacting
with structures.
An acoustic analysis:
is used to model sound propagation, emission, and radiation problems;
can include incident wave loading to model effects such as underwater
explosion (UNDEX) on structures interacting
with fluids, airborne blast loading on structures, or sound waves impinging on
a structure;
in
Abaqus/Explicit can
include fluid undergoing cavitation when the absolute pressure drops to a limit
value;
can be used to model an acoustic medium alone, as in the study of the
natural frequencies of vibration of a cavity containing an acoustic fluid;
can be used to model a coupled acoustic-structural system, as in the
study of the noise level in a vehicle;
can be used to model the sound transmitted through a coupled
acoustic-structural system;
requires the use of acoustic elements and, for coupled
acoustic-structural analysis, a surface-based interaction using a tie
constraint or, in
Abaqus/Standard,
acoustic interface elements;
can be used to obtain the scattered wave solution directly under
incident wave loading when the mechanical behavior of the fluid is linear;
can be used to obtain a total wave solution (sum of the incident and
the scattered waves) by selecting the total wave formulation, particularly when
nonlinear fluid behavior such as cavitation is present in the acoustic medium;
can be used to model problems where the acoustic medium interacts with
a structure subjected to large static deformation;
in
Abaqus/Standard can
include a coupled structural-acoustic substructure that was previously defined
(Generating Substructures);
can be used to model both interior problems, where a structure
surrounds one or more acoustic cavities, and exterior problems, where a
structure is located in a fluid medium extending to infinity; and
is applicable to any vibration or dynamic problem in a medium where
the effects of shear stress are negligible.
A shock analysis:
is used to model blast effects on structures;
often requires double precision to avoid roundoff error when
Abaqus/Explicit
is used;
may include acoustic elements to model the effects of fluid inertia
and compressibility;
may include virtual mass effects to model the effect of an
incompressible fluid interacting with a pipe structure;
can be used to model both interior problems, where a structure
surrounds one or more fluid cavities, and exterior problems, where a structure
is located in a fluid medium extending to infinity; and
in
Abaqus/Explicit
can include air blast loading on structures using the
CONWEP model.
Acoustic elements model the propagation of acoustic waves and are active
only in dynamic analysis procedures. They are most commonly used in the
following procedures:
In general, analysis with acoustic elements should be thought of as
small-displacement linear perturbation analysis, in which the strain in the
acoustic elements is strictly (or overwhelmingly) volumetric and small. In many
applications the base state for the linear perturbation is simply ignored: for
solid structures interacting with air or water, the initial stress (if any) in
the air or water has negligible physical effect on the acoustic waves. Most
engineering acoustic analyses, transient or steady state, are of this type.
An important exception is when the acoustic perturbation occurs in a gas or
liquid with high-speed underlying flow. If the magnitude of the flow velocity
is significant compared to the speed of sound in the fluid (i.e., the Mach
number is much greater than zero), the propagation of waves is facilitated in
the direction of flow and impeded in the direction against the flow. This
phenomenon is the source of the well-known “Doppler effect.” In
Abaqus/Standard
underlying flow effects are prescribed for nodes making up acoustic elements by
specifying an acoustic flow velocity.
Acoustic elements can be used in a static analysis, but all acoustic effects
will be ignored. A typical example is the air cavity in a tire/wheel assembly.
In such a simulation the tire is subjected to inflation, rim mounting, and
footprint loads prior to the coupled acoustic-structural analysis in which the
acoustic response of the air cavity is determined. See
Defining ALE Adaptive Mesh Domains in Abaqus/Standard
and
ALE Adaptive Meshing and Remapping in Abaqus/Standard
for more information.
Acoustic elements also can be used in a substructure generation procedure to
generate coupled structural-acoustic substructures. Only structural degrees of
freedom can be retained. The retained eigenmodes must be selected when an
acoustic-structural substructure is generated. In a static analysis involving a
substructure containing acoustic elements, the results will differ from the
results obtained in an equivalent static analysis without substructures. The
reason is that the acoustic-structural coupling is taken into account in the
substructure (leading to hydrostatic contributions of the acoustic fluid),
while the coupling is ignored in a static analysis without substructures. More
details on coupled structural-acoustic substructures can be found in
Generating Substructures.
A volumetric drag coefficient, ,
can be defined to simulate fluid velocity-dependent pressure amplitude losses.
These occur, for example, when the acoustic medium flows through a porous
matrix that causes some resistance (see
Acoustic Medium),
such as a sound-deadening material like fiberglass insulation. For direct time
integration dynamic analysis we assume there are no significant spatial
discontinuities in the quantity ,
where
is the density of the fluid (acoustic medium), and that the volumetric drag is
small at acoustic-structural boundaries. These assumptions, which can limit the
applicability of the analysis, are discussed further in
Coupled acoustic-structural medium analysis.
The direct-solution steady-state dynamic harmonic response procedure is
advantageous for acoustic-structural sound propagation problems, because the
gradient of
need not be small and because acoustic-structural coupling and damping are not
restricted in this formulation. If there is no damping or if damping can be
neglected, factoring a real-only matrix can reduce computational time
significantly; see
Direct-Solution Steady-State Dynamic Analysis
for details.
Some fluid-solid interaction analyses involve long-duration dynamic effects
that more closely resemble structural dynamic analysis than wave propagation;
that is, the important dynamics of the structure occur at a time scale that is
long compared to the compressional wave speed of the solid medium and the
acoustic wave speed of the fluid. Equivalently, in such cases, disturbances of
interest in the structure propagate very slowly in comparison to waves in the
fluid and compressional waves in the structure. In such instances, modeling of
the structure using beams is common. When these structural elements interact
with a surrounding fluid, the important fluid effect is due to motions
associated with incompressible flow (see
Loading due to an incident dilatational wave field).
These motions result in a perceived inertia added to the structural beam;
therefore, this case is usually referred to as the “virtual mass
approximation.” For this case
Abaqus
allows you to modify the inertia properties of beam and pipe elements, as
described below. Loads on the structure associated with incident waves in the
fluid can be accommodated under this approximation as well.
Natural Frequency Extraction
Abaqus
can compute both real and complex eigensolutions for purely acoustic or
structural-acoustic systems, with or without damping. Exterior acoustic
problems may also be solved.
Selecting an Eigensolver
In a coupled acoustic-structural model, real-valued coupled modes are
extracted by default using the Lanczos eigenfrequency extraction procedure.
Coupling may be suppressed in the frequency extraction step; in this case the
structural elements behave as though the interface with the acoustic elements
were free (as though this surface were “in vacuo”), and the acoustic elements
behave as though the boundary with the structural elements were rigid.
Extracting the coupled acoustic-structural modes is also available for the
AMS eigensolver.
Structural-acoustic coupling is ignored if the subspace iteration
eigensolver is used.
When applying the AMS eigensolver to a
coupled structural-acoustic model,
Abaqus
by default projects and stores the acoustic coupling matrix during the natural
frequency extraction, for later use in coupled forced response analyses. The
structural and acoustic regions are not actually coupled during the
eigenanalysis;
Abaqus
solves the two regions separately but computes and stores the projected
coupling operator for use in subsequent steady-state dynamic steps. Only
structural-acoustic coupling defined using tied contact is supported. You can
suppress this coupling if desired. Damping due to acoustic volumetric drag is
also projected by default during an eigenanalysis and is restored by default in
subsequent steady-state dynamic steps. Projecting and storing the acoustic
coupling matrix during the natural frequency extraction is also available for
the Lanczos eigensolver based on the SIM
architecture.
Damping and Inertia Effects in an Acoustic Natural Frequency Extraction
Since damping is not taken into account in real-valued modal extraction,
the volumetric drag effect is not considered, except for its small contribution
to any nonreflecting boundaries (see
Coupled acoustic-structural medium analysis).
The damping contributions due to any impedance boundary conditions
(element-based or surface-based) or acoustic infinite elements are not included
in an eigenfrequency extraction step, but the contributions to the acoustic
element mass and stiffness matrices are included. Similarly, the (symmetrized)
stiffness and mass contributions of acoustic infinite elements are included in
an eigenfrequency extraction step, but the damping effects are neglected.
Modal analysis of damped and radiating acoustic systems can be performed
in
Abaqus
as well. Using the complex eigenvalue extraction procedure, the damping
contributions of acoustic infinite elements, nonreflecting impedance
conditions, and general impedance layers are restored to the element operators.
If an underlying flow field is defined for the acoustic region by
specifying an acoustic flow velocity, the natural frequencies and modes are
affected. However, in real-valued frequency extraction only the acoustic
element mass and stiffness matrices contribute to the solution. Since the
formulation for acoustics in the presence of a flow field requires a complex
part in the element operator (damping matrix), the real-valued procedure can
include the effects of flow only to a limited degree. The complex frequency
procedure in
Abaqus/Standard
includes the damping matrix contribution and is, therefore, required when modes
of a system with moving fluid are sought. The complex frequency procedure can
be used only following the Lanczos real-valued frequency procedure.
Virtual mass effects defined for beams by adding inertia (Additional Inertia due to Immersion in Fluid)
are included in modal analysis: their effect is simply to add inertia to a beam
element.
Interpreting the Extracted Modes in a Coupled Structural-Acoustic Natural Frequency Analysis
While all the modes extracted in a coupled Lanczos structural-acoustic
natural frequency analysis include the effects of fluid-solid interaction, some
of them may have predominantly structural contributions while others may have
predominantly acoustic contributions. Coupled structural-acoustic eigenmodes
can be categorized as follows:
Most generally, an individual mode may exhibit participation in both
the fluid and the solid media; this is referred to as a “coupled mode.”
Second, there are the “structural resonance” modes. These are modes
corresponding to the eigenmodes of the structure without the presence of the
acoustic fluid. The presence of the acoustic fluid has a relatively small
effect on these eigenfrequencies and the mode shapes.
Third, there are the “acoustic cavity resonance” modes. These are
nonzero eigenfrequency coupled modes that have a significant contribution in
the resulting dynamics of the acoustic pressure in mode-based dynamic
procedures.
Fourth, if insufficient boundary conditions are specified on the
structural part of a model, the frequency extraction procedure will extract
rigid body modes. These modes have zero eigenfrequencies (sometimes they appear
as either small positive or even negative eigenvalues). However, if sufficient
structural degrees of freedom are constrained, these rigid body modes
disappear.
Finally, there are the singular acoustic modes, which have zero
eigenfrequencies and constant acoustic pressure; they are mathematically
analogous to structural rigid body modes. The structural part of the singular
acoustic modes corresponds to the quasi-static structural response to constant
pressure in unconstrained acoustic regions. These eigenmodes are predominantly
acoustic and are important in representing the (low-frequency) acoustic
response in mode-based analysis in the presence of acoustic loads, in the same
way that rigid body modes are important in the representation of structural
motion. As is true for the structural rigid body modes, if a sufficient number
of constrained acoustic degrees of freedom is specified (one degree of freedom
8 per acoustic region is enough), the singular acoustic modes will disappear.
In models with only one unconstrained acoustic region (the most common case)
only one singular acoustic mode will be computed. In general there are as many
singular acoustic modes as there are independent unconstrained acoustic
regions. If these modes are present, they are always reported first by the
Lanczos eigensolver; and a note at the bottom of the eigenfrequency table in
the data file provides information about the number of singular acoustic modes.
The generalized masses and effective masses can help distinguish between
the various types of modes and can be used to assess which modes are important
for subsequent mode-based analyses. In addition, the acoustic contribution to
the generalized masses is reported as a fraction for each eigenmode. The closer
the value of this fraction is to unity, the more pronounced is the acoustic
component of this eigenmode. An acoustic effective mass is also computed for
each eigenmode. This scalar quantity is scaled such that when all eigenmodes in
a model are extracted, the sum of all acoustic effective masses is equal to 1.0
(minus the contributions from nodes with restrained acoustic degrees of
freedom). The acoustic effective mass can be compared between different modes:
the higher the acoustic effective mass, the more important (typically) the mode
is for accurate representation of the acoustic pressure. For example, the fluid
cavity acoustic resonance modes will have larger acoustic effective masses
compared to the other modes.
Modal Superposition Procedures
In
Abaqus
acoustic domains are handled quite similarly to solid and structural domains.
Real-valued eigenmodes, resulting from a previous real-valued eigenfrequency
extraction procedure with or without coupling effects included, are used as a
basis for modal solutions. The mode-based steady-state dynamic procedure is the
most computationally efficient alternative to compute the steady-state response
of structural-acoustic systems. Structural-acoustic coupling and damping
effects in these analyses depend on the type of modal procedure and the
eigensolver that was used to compute the eigenfrequencies.
Structural-Acoustic Coupling in Modal Analyses Using the Lanczos Eigensolver without the SIM Architecture
If coupled modes are computed using the Lanczos eigensolver, both the
mode-based and subspace projection steady-state dynamic procedures will include
structural-acoustic coupled effects. If uncoupled Lanczos modes are computed,
coupling can be restored only by using subspace projection. It is sufficient to
project at a single frequency (constant subspace) to resolve the acoustic
coupling for all frequencies.
Acoustic Medium Damping in Modal Analyses Using the Lanczos Eigensolver without the SIM Architecture
In subspace-based steady-state dynamic analysis, acoustic medium damping
and structural material damping are considered, and the structural-acoustic
interaction, infinite element, and impedance boundary terms are also included.
Acoustic medium damping is not considered in the procedures that base the
response prediction directly on the system's eigenmodes, such as transient
modal dynamic analysis or the mode-based steady-state dynamic procedure. These
methods should, therefore, be used with caution for problems with impedance
boundary conditions. Modal damping can be used in these procedures (Material Damping)
to model material damping and volumetric drag effects; however, modal damping
usually cannot be used to model the fluid-solid coupling or the impedance
boundary effects accurately.
Structural-Acoustic Coupling and Damping in Modal Analyses Using the Subspace Iteration Eigensolver
The subspace iteration eigensolver neglects the effects of
structural-acoustic coupling; therefore, coupling effects are not included in
subsequent modal procedures.
As with analyses using the Lanczos eigensolver, acoustic medium damping
and structural material damping are considered in subsequent subspace-based
steady-state dynamic procedures, but these damping effects are not considered
in subsequent transient modal or mode-based steady-state dynamic procedures.
Structural-Acoustic Coupling and Damping in Modal Analyses Using the AMS Eigensolver or the Lanczos Eigensolver Based on the SIM Architecture
The structural-acoustic modes, extracted using the
AMS eigensolver or the Lanczos eigensolver,
can be used in modal analyses using the SIM
architecture. When uncoupled modes are computed using the
AMS eigensolver or the Lanczos eigensolver
based on the SIM architecture with projection
of the structural-acoustic coupling specified, the coupling and acoustic
damping operators are projected and stored during the natural frequency
extraction. Subsequent coupled forced response analyses using modal
steady-state dynamics automatically restore the effects of structural-acoustic
coupling and damping by automatically using these projected matrices; if the
matrices were not projected, the steady-state dynamic step would not include
these effects. A mode-based steady-state dynamic step cannot use unsymmetric
damping, such as from acoustic flow velocity or infinite element effects. To
take these effects into account, a subspace-based steady-state dynamic analysis
should be used.
Defining Translational or Rotational Underlying Flow Velocity in Abaqus/Standard
As described above, acoustic analysis in
Abaqus/Standard
can be performed as a linear perturbation of a high-speed flow field. The flow
velocity field affects the propagation of acoustic waves in the medium through
the effect of the flow velocity on the speed of the wave propagation. Waves
travel faster along the direction of the local flow vector and are
correspondingly impeded in the direction against the flow direction. It is
sufficient for you to define the velocity field in the affected acoustic
region; the accelerations do not play a role in the formulation.
You specify the flow in the acoustic finite element region as history data
within a dynamic linear perturbation step. The flow field can be described
either by direct input of the velocity components or by defining rotating
motion associated with a reference frame. In the former case, each node in the
acoustic region where flow occurs is assigned a Cartesian velocity defined by
specifying the components of the velocity vector, . In the latter case,
the rotational velocity for the nodes in the acoustic region is defined by
specifying the magnitude of an angular rotation velocity,
, and the position
and orientation of the axis of rotation in the current configuration. The
position and orientation of the axis are applied at the beginning of the step
and remain fixed during the step.
The specified underlying flow is active only for acoustic finite elements;
other elements with acoustic degrees of freedom, such as acoustic infinite and
interface elements, are unaffected by the specified flow velocity. The effect
of underlying flow on the acoustic finite elements depends also on the
procedure used: the effects are present only in frequency-domain dynamic
procedures and natural frequency extraction. For complex-valued procedures,
such as complex frequency extraction and steady-state dynamics, the presence of
underlying flow affects the acoustic finite element stiffness matrices and adds
a significant contribution to the element damping matrix. For real-valued
procedures, such as eigenfrequency extraction and steady-state dynamics
analysis in which a real-only system matrix is factored, the presence of
underlying flow affects only the acoustic finite element stiffness matrices;
the damping matrix is ignored. Consequently, the effect of flow on the acoustic
field is fully realized only in complex-valued procedures.
For rotating systems, solid and acoustic materials are treated differently
in
Abaqus.
Flow of solid material through a mesh may induce significant deformation and is
handled by using steady-state transport; subsequent linear perturbation steps
are analyzed about this deformed state (see
Steady-State Transport Analysis).
Flow of material through an acoustic mesh is handled entirely within linear
perturbation steps by specifying an acoustic flow velocity; a preliminary
nonlinear steady-state transport analysis is not required. For coupled
acoustic-structural systems undergoing rotation, such as tires, the model may
be subjected to a steady-state transport step, which deforms the solid medium,
followed by linear perturbation dynamic steps. The effect of the rotation of
the solid is included in the linear perturbation steps in this case; to include
the effect of the rotation of the acoustic fluid, specify an acoustic flow
velocity in the linear perturbation steps.
Updating the Acoustic Domain during a Large-Displacement Abaqus/Standard Analysis
By default, the acoustic-structural coupling calculations are based on the
original configuration of the fluid domain. However, acoustic elements can also
be used in an analysis where the structural domain experiences large
deformation prior to the coupled analysis. A typical example is the interior
cavity of a tire subjected to structural loads such as inflation, rim mounting,
and footprint pressure.
The acoustic elements in
Abaqus
do not have displacement degrees of freedom and, therefore, cannot model the
deformation of the fluid when the structure undergoes large deformation.
Abaqus/Standard
solves the problem of computing the current configuration of the acoustic
domain by periodically creating a new acoustic mesh. The new mesh uses the same
topology (elements and connectivity) throughout the simulation, but the nodal
locations are adjusted so that the acoustic domain conforms to the structural
domain on the boundary.
A new acoustic mesh is computed when adaptive meshing is specified and
nonlinear geometric effects are considered in any non-perturbation
Abaqus/Standard
analysis procedure in which acoustic effects are ignored.
In
Abaqus/Standard
the initial acoustic static pressure (hydrostatic or ambient) is not modeled by
the acoustic formulation and cannot be specified as an initial condition.
In
Abaqus/Explicit
the initial acoustic pressure corresponding to the initial static equilibrium
(hydrostatic or ambient) can be specified (see
Initial Conditions)
and is meaningful only when the acoustic fluid is capable of undergoing
cavitation. In problems with possible fluid cavitation the initial acoustic
static pressure is taken into account in the cavitation condition; i.e., the
sum of the dynamic and static acoustic pressures needs to drop to the
cavitation pressure limit for the cavitation to occur. The specified acoustic
static pressure is used only in the cavitation condition and does not apply any
static loads to the acoustic or structural meshes at their common wetted
interface. In addition, the acoustic static pressure is not included in the
nodal acoustic pressure degree of freedom.
The initial temperature and field variable values can be specified (Initial Conditions)
for the direct time integration dynamic, explicit dynamic, dynamic fully
coupled temperature-displacement, and mode-based transient dynamic analysis
procedures. Changes in these variables during the analysis will affect any
temperature-dependent or field-variable-dependent acoustic medium properties.
Boundary Conditions
The various boundary conditions that can be applied to an acoustic medium
are described below. These include acoustic domain boundaries with stationary
rigid walls or symmetry planes, prescribed pressure values such as a free
surface with zero dynamic pressure, specified impedance (see
Acoustic and Shock Loads),
and structural interfaces such as the interface with a ship or a submarine. The
radiating (nonreflecting) boundary condition for exterior problems (such as a
structure vibrating in an acoustic medium of infinite extent) is implemented as
a special case of the impedance boundary condition (see
Acoustic and Shock Loads).
On any given part of the acoustic domain boundary only one boundary condition
type should be applied, except for the combination of the impedance boundary
condition and the acoustic-structural interface condition.
Boundary with a Stationary Rigid Wall or a Symmetry Plane
The default boundary condition for an acoustic medium is a boundary with a
stationary rigid wall or a symmetry plane. The “force” conjugate to pressure in
the acoustics formulation in
Abaqus
is the normal pressure gradient at the surface divided by the mass density;
dimensionally this is equal to a force per unit mass. In the absence of
volumetric drag this force per unit mass is equal to the inward acceleration of
the acoustic medium. The conjugate variable at a node on the surface is the
inward volume acceleration, which is the integral of the inward acceleration of
the acoustic medium evaluated over the surface area associated with the node. A
“traction-free” surface (one with no boundary conditions, no applied loads, no
surface impedance conditions, and no interface elements) is a surface normal to
which the acoustic medium undergoes no motion and, thus, corresponds to a
rigid, stationary surface adjacent to the fluid. A symmetry plane for the
acoustic medium is another “traction-free” surface.
Prescribed Pressure
The basic variable in the acoustic medium is pressure (degree of freedom 8).
Therefore, this variable can be prescribed at any node in the acoustic model by
applying a boundary condition (Boundary Conditions).
Setting the pressure to zero represents a “free surface,” where the pressure
does not vary because of the motion of the surface (to account for surface
motion effects, see the discussion of impedance below). Prescribing a nonzero
value for the pressure represents a sound source.
An amplitude variation can be used to specify the value of the pressure. In
a steady-state analysis you can specify both the in-phase (real) part of the
pressure (default) and the out-of-phase (imaginary) part of the pressure.
Boundary with a Structure
If the acoustic medium is adjacent to a structure, there will be a transfer
of momentum and energy between the media at the boundary. The pressure field
modeled with acoustic elements creates a normal surface traction on the
structure, and the acceleration field modeled with structural elements creates
the natural forcing term at the fluid boundary (for details, see
Coupled acoustic-structural medium analysis).
The surface-based coupling procedure and the user-defined acoustic interface elements differ
slightly in their theoretical implementation. In essence, the interface elements computed
internally by the surface-based procedure are discrete point elements computed at the
nodes of the secondary surface. A user-defined acoustic interface element, on the other
hand, distributes coupling effects across all of its nodes. Generally, the results
obtained using the two coupling methods will be very similar, but the difference in
discretization at the coupling boundary may create small differences in results.
Defining Acoustic-Structural Coupling with User-Defined Acoustic Interface Elements
In
Abaqus/Standard,
if the structural and acoustic meshes share nodes at the boundary, lining this
boundary with acoustic-structural interface elements (see
Acoustic Interface Element Library)
will enforce the required physical coupling condition. The interface element
normals must point into the acoustic medium, which forces continuity of the
normal accelerations of the acoustic medium and of the structure at the
boundary and ensures that the pressure of the acoustic elements is applied to
the structure. Displacements can also be prescribed at such a boundary.
Defining Acoustic-Structural Coupling Using a Surface-Based Coupling Procedure
Alternatively, a surface-based procedure can be used to enforce the
coupling; in
Abaqus/Explicit
the surface-based procedure is the only available method. This method requires
that the structural and acoustic meshes use separate nodes. You define surfaces
on the structural and fluid meshes and define the interaction between the two
meshes using a surface-based tie constraint (see
Mesh Tie Constraints).
No additional element definitions are required.
The secondary surface, the first of the two surfaces specified for the tie constraint, must be
element-based; whereas the main surface can be either element- or node-based. A surface
based on rigid element types (R3D4, etc.)
or an analytical rigid surface cannot be used as a main surface; instead, use a
deformable surface made rigid.
For surface-based tie constraints Abaqus automatically computes the region of influence for each internally generated
acoustic-structural interface element. If the user-defined secondary surface overhangs
the main surface significantly, the regions of influence may include parts of the
overhang. Consequently, the overhanging part of the secondary surface may exhibit
nonphysical coupled degrees of freedom: displacements if the secondary surface is
acoustic and acoustic pressures if the secondary surface is solid or structural. These
nonphysical results on the overhang do not affect the remainder of the solution, and it
should be understood that they are not meaningful.
Coupling Surfaces to Structures Using Acoustic Infinite Elements
Acoustic infinite elements may form surfaces that can be coupled to
structures by using a tie constraint in two different ways. The acoustic
infinite element surface may consist of the base (first) facets of the acoustic
infinite elements; in this case this surface should be tied to a topologically
similar structural surface. The acoustic infinite element edges may also be
used to define surfaces (see
Mesh Tie Constraints),
which can be tied to solid elements. This approach couples the semi-infinite
sides of acoustic infinite elements to solid elements.
Mesh Refinement
Although the meshes may be nodally nonconforming at the tied surfaces, mesh refinement affects
the accuracy of the coupled solution. In acoustic-solid problems the mesh refinement
depends on the wave speeds in the two media. The mesh for the medium with the lower wave
speed should generally be more refined and, therefore, should be the secondary surface.
If the details of the wave field in the vicinity of the fluid-solid interface are
important, the meshes should be of equally high refinement, with the refinement
corresponding to the lower wave speed medium. In this case the choice of the main
surface is arbitrary. An exception is the case where the acoustic medium must be updated
to follow the structure during a large-deformation analysis. In such a case the
secondary surface must be defined on the acoustic domain. Another exception is the case
of fluids coupled to both sides of shell or beam elements (as described below).
Solving the Structural System Sequentially Using the Submodeling Technique
In some applications the normal surface traction on the structure created
by the acoustic fluid may be negligible compared to other forces in the
structural system. For example, a metal motor housing may radiate sound into
the surrounding air, but the reaction pressure of the air on the motor may be
insignificant to the dynamics of the housing. In these cases the submodeling
technique (see
About Submodeling)
can be used to solve the system sequentially; that is, the structural analysis
(uncoupled from the fluid) is followed by the acoustic analysis (driven by the
structure). Usually, this decoupling of the analysis reduces computational
cost. The structural system plays the role of the “global” model, and the
acoustic fluid is the submodel. The structural displacements on the boundary of
the acoustic fluid must be saved to the results file in the global analysis.
Since
Abaqus
interpolates the fields between the global and submodels, acoustic-structural
interface elements can be used. They should be applied to the fluid boundary to
be driven by the global structural model.
Defining Acoustic-Structural Coupling on Both Sides of a Beam or Shell
In
Abaqus/Standard
there are two alternatives available for modeling a beam (in two dimensions) or
shell interacting with fluid on both sides: a surface-based procedure and an
element-based procedure. In
Abaqus/Explicit
the surface-based procedure must be used.
Use of the surface-based procedure is straightforward. Two surfaces must be defined on the beam
or shell: one on the SPOS side and one on the
SNEG side. Each surface is then coupled to the fluid
using a tie constraint. At least one of the two surfaces on the beam or shell must be a
main surface.
In
Abaqus/Standard,
if the same nodes are used for the fluid and the beam or shell, acoustic
interface elements must be used in the following manner to define
acoustic-structural coupling on both sides of a beam or shell element:
Define a second set of nodes coincident with the beam or shell nodes,
and constrain the motions of the two sets of nodes together using a PIN-type MPC (General Multi-Point Constraints).
Use the first set of nodes to line one side of the beam or shell
elements with acoustic interface elements (with the normals of the acoustic
interface elements pointing into the fluid).
Use the second set of nodes to line the other side of the beam or
shell elements with acoustic interface elements (with the normals pointing into
the fluid on the opposite side of the structure, as in Step 2).
The acoustic elements on the first side of the beam or shell elements
should be defined using the first set of nodes, and the acoustic elements on
the second side of the beam or shell elements should be defined using the
second set of nodes.
Defining the Virtual Mass Effect (Fluid-Structural Coupling) for Beam and Pipe Elements
In
Abaqus
virtual mass effects on submerged Timoshenko beam elements can be modeled by
specifying additional inertia for the beam. The virtual mass effects are
specified as part of the section definition of the beam.
The following types of loading can be prescribed in an acoustic analysis, as
described in
Acoustic and Shock Loads:
Concentrated pressure-conjugate loading.
An impedance condition that specifies the relationship between the
pressure of the acoustic medium and the normal motion at the boundary (either
element-based or surface-based). Such a condition is applied, for example, to
include the effect of small-amplitude “sloshing” in a gravity field or to
include the effect of a compressible, possibly dissipative, lining (such as a
carpet) between the acoustic medium and a fixed, rigid wall or a structure.
This type of condition can also be applied to edge facets of acoustic infinite
elements.
Nonreflecting radiation conditions on acoustic boundaries (either
element-based or surface-based). An impedance can be defined to select the
appropriate radiating boundary condition taking the radiating surface shape
into consideration.
Incident wave loading such as that caused by an underwater explosion or
a sound field. Since this type of loading is usually applied in conjunction
with semi-infinite acoustic regions, two alternative modeling formulations are
available in
Abaqus.
A total pressure-based formulation is provided when the incident wave loading
is applied to the exterior of a semi-infinite acoustic mesh. This formulation
must be used to handle the incident wave loading when the acoustic medium is
capable of cavitation, rendering the fluid material behavior nonlinear. The
scattered pressure formulation is typically used when cavitation is not part of
the fluid mechanical behavior and when the loads are applied to fluid-solid
interfaces. Sound transmission loss and acoustic scattering problems usually
fall into the latter category.
For both formulations, when incident wave loading is applied to a given
surface, a mathematical jump occurs between the pressures on both sides of the
surface because the side from which the incident pressure arrives is implicitly
a region of scattered pressure. This jump is handled automatically when the
incident wave load is applied to a surface with a nonreflecting impedance
condition and when the incident wave load is applied to a fluid-solid
interface. However, if the incident wave load is applied to a surface lying
between acoustic finite or infinite elements, the jump will not be modeled
properly because pressures are continuous between acoustic elements. For this
case, low-mass and low-stiffness membrane, shell, or surface elements should be
interposed between the acoustic elements to permit the jump in pressure to
exist.
Incident wave loading can be applied in time-harmonic problems, using
the direct solution steady-state dynamics and the subspace-based, steady-state
dynamic procedures. You can define individual spherical or planar sources
emitting waves, or you can use the deterministic diffuse field model in
Abaqus.
In the former case, usage is quite similar to transient analysis: the defined
sources correspond to distinct sound sources. The latter case models the sound
field incident on a surface exposed to a reverberant chamber: the field is
assumed to be equivalent to a number of plane waves arriving from directions
distributed on a hemisphere. Only the scattered wave formulation is supported
when using incident wave loading in steady-state dynamics.
Loading due to an incident shock wave caused by an air explosion.
Although this type of wave is highly nonlinear and complex, the pressure
loading due to the shock wave can be calculated readily from empirical data
provided by the CONWEP model available in
Abaqus/Explicit.
The main advantage of this model is that the loading is applied directly to the
structure subject to the blast; there is no need to include the fluid medium in
the computational domain. In the CONWEP model,
empirical data for two types of waves are available: spherical waves for
explosions in mid-air and hemispherical waves for explosions at ground level in
which ground effects are included.
The CONWEP model does not account for
effects of shadowing by intervening objects. In addition, it does not account
for effects due to confinement and, thereby, excludes incorporation of any
reflecting surfaces in the analysis. The model does account for the angle of
incident of the blast wave; see
Acoustic and Shock Loads
for incorporation of the incident angle in the pressure load calculation.
Predefined Fields
The following predefined fields can be specified in an acoustic analysis,
as described in
Predefined Fields:
Although temperature is not a degree of freedom in acoustic elements,
nodal temperatures can be specified. The specified temperature affects
temperature-dependent material properties.
The values of user-defined field variables can be specified. These
values affect field-variable-dependent material properties.
Material Options
Only the acoustic medium material model (Acoustic Medium)
is valid for use in an acoustic analysis. The structure in a coupled
acoustic-structural analysis can be modeled using any material model. Since
acoustic analyses are always performed using a dynamic procedure, the
structure's density (Density)
should usually be defined.
Porous materials are often modeled using an acoustic formulation when the
dilatational waves in the porous medium dominate the shear effects. A large
number of models exist for this category of phenomenon. In
Abaqus,
two categories of models are available for porous media modeled with acoustic
elements: phenomenological models and general frequency-dependent models.
Phenomenological models describe the dynamic characteristics using material
data related to the porous structure, such as porosity itself, tortuosity, etc.
Alternatively, you can specify the dynamic properties directly for the
material; usually, this is done using a table of frequency-dependent data. See
Acoustic Medium
for details on specifying acoustic materials in
Abaqus.
When the acoustic medium is capable of cavitation and the analysis includes
incident wave loading, a total pressure-based formulation must be used. Either
the default scattered wave formulation or the total wave formulation can be
used if the cavitation is absent or the problem has no incident wave loading.
For beam elements using the virtual mass approximation, the relevant data
are specified as part of the beam section definition.
In
Abaqus/Standard
the second-order acoustic elements are generally considerably more accurate
than first-order acoustic elements for a given number of degrees of freedom.
The acoustic elements in
Abaqus/Explicit
are limited to first-order interpolations.
Acoustic elements cannot be used together with hydrostatic fluid elements.
With the CONWEP model provided in
Abaqus/Explicit,
the analysis must be three-dimensional. The loading surface must be comprised
of solid, shell, or membrane elements only. In addition,
CONWEP loading cannot be applied to acoustic
elements.
Exterior Problems
We often need to model an exterior problem, such as a structure vibrating in
an acoustic medium of infinite extent. Impedance-type radiation boundary
conditions can be used to model the motions of waves out of the mesh.
Abaqus
provides acoustic infinite elements for this class of problems. In addition,
Abaqus/Standard
provides perfectly matched layers to truncate the acoustic infinite domain in a
direct-solution steady-state dynamic analysis.
Impedance-Type Radiation Conditions
In this case acoustic elements are used to model the region between the
structure and a simple geometric surface (located away from the structure), and
a radiating (nonreflecting) boundary condition is applied at that surface. The
radiating boundary conditions are approximate, so that the error in an exterior
acoustic analysis is controlled not only by the usual finite element
discretization error but also by the error in the approximate radiation
condition. In
Abaqus
the radiation boundary conditions converge to the exact condition in the limit
as they become infinitely distant from the radiating structure. In practice,
these radiation conditions provide accurate results when the distance between
the surface and the structure is at least one-half of the longest
characteristic or responsive structural wavelength.
Acoustic infinite elements are provided for modeling exterior problems
(Infinite Elements).
These elements have surface topology: line and quadratic segments in
two-dimensional and axisymmetric problems and triangles and quadrilaterals in
three-dimensional problems. Generally, the acoustic infinite elements are
defined on a terminating surface of a region of acoustic finite elements. The
infinite element formulation is considerably more accurate than the
impedance-type radiation boundary conditions in cases where the wave field
impinging on the terminating surface has many complex features. The radiation
boundary conditions are relatively simple, equivalent to a “zeroth-order”
infinite element; the acoustic infinite elements implemented in
Abaqus
are of variable order, up to ninth.
Acoustic infinite elements can be coupled directly to structural surfaces
by using a surface-based tie constraint: this may provide adequate accuracy in
some applications. In general cases the acoustic infinite elements are defined
on the terminating surface of the acoustic finite element mesh. The diameter of
the acoustic finite element mesh can be considerably smaller, for a given
solution accuracy, than is the case when using radiation boundary conditions.
The nodal connectivity on the acoustic infinite element defines the
element's surface topology. To complete the element formulation, the surface
topology must be mapped into the infinite domain. This mapping requires a
reference point, given in the element section property definition. The
reference point serves to define a characteristic length used in the coordinate
mapping. In the ideal case of acoustic radiation from a spherical surface, the
correct placement of the reference point is the center of the sphere. In
general, the acoustic infinite elements produce the most accurate results when
the reference node is located near the center of the region enclosed by the
infinite elements.
Nodal normal vectors are required for an accurate mapping of the infinite
domain. The nodal normal vectors must point into the infinite domain and are
used to define the portion of the infinite domain treated by a particular
infinite element. To cover the infinite domain without overlap, each node
attached to an infinite element must have a unique normal. The nodal normal
vectors are specified or calculated as follows.
User-specified alternative nodal normals (Normal Definitions at Nodes)
are ignored for acoustic infinite elements and, therefore, cannot be used to
define normal directions for acoustic elements. Over the element's surface
topology, the normal vectors must be divergent; that is, the area mapped (in
two dimensions) or the volume mapped (in three dimensions) must increase with
distance into the infinite domain. To ensure this criteria, the normal vectors
at each acoustic infinite element node are defined to lie along the vector
between that node and the reference point given in the element section property
definition. See
Infinite Elements
for more information.
Perfectly Matched Layers
Perfectly matched layers are provided for modeling exterior acoustic
problems during a direct-solution steady-state dynamic analysis. The perfectly
matched layer is modeled using the acoustic elements that are available in
Abaqus/Standard
whose behavior is modified appropriately to act as an absorbing layer. The
perfectly matched layer absorbs all the waves that are incident to it. For any
given problem, it is recommended to have 4–7 layers of elements in the
perfectly matched layer region. You specify the coefficients that are used to
define the absorbing properties of the perfectly matched layer and the outer
limits of the acoustic domain. These limits are used to compute the absorbing
properties for the perfectly matched layer.
You cannot use axisymmetric acoustic elements to model the perfectly
matched layer. The outer surface of the perfectly matched layer should have a
zero pressure boundary condition. To avoid reflections from the perfectly
matched layer region, the material properties used for the perfectly matched
layer elements should match those of the acoustic elements.
Mesh Refinement
Inadequate mesh refinement is the most common source of difficulties in
acoustic and vibration analysis. For reasonable accuracy, at least six
representative internodal intervals of the acoustic mesh should fit into the
shortest acoustic wavelength present in the analysis; accuracy improves
substantially if ten or more internodal intervals are used at the shortest
wavelength. In steady-state analyses the shortest wavelength will occur in the
medium with the lowest speed of sound, at the highest frequency analyzed. In
transient analyses the shortest wavelength present is more difficult to
determine before an analysis: it is reasonable to estimate this wavelength
using the highest frequency present in the loads or prescribed boundary
conditions.
An “internodal interval” is defined as the distance from a node to its
nearest neighbor in an element; that is, the element size for a linear element
or half of the element size for a quadratic element. At a fixed internodal
interval, quadratic elements are more accurate than linear elements. The level
of refinement chosen for the acoustic medium should be reflected in the solid
medium as well: the solid mesh should be sufficiently refined to accurately
model flexural, compressional, and shear waves.
The level of mesh refinement required depends on the application. Any finite
element discretization of a domain in which waves propagate introduces a
certain amount of error per wavelength. In meshes that are small in terms of
wavelengths, relatively coarse (for example, six internodal intervals per
wavelength) meshes may be adequate. For meshes that contain many wavelengths at
the frequency of interest, the per-wavelength finite element discretization
error accumulates, generally necessitating greater levels of refinement. In
these larger meshes the accumulated per-wavelength error may be present
throughout the mesh if refinement is inadequate.
The acoustic wavelength decreases with increasing frequency, so there is an
upper frequency limit for a given mesh. Let
represent the maximum internodal interval of an element in a mesh,
the number of internodal intervals we desire per acoustic wavelength
(
is recommended),
the cyclical frequency of excitation, and
the speed of sound, where
is the bulk modulus of the acoustic medium and
is its density. The requirements are then expressed as
The above expressions can be used to estimate the maximum allowable element
length if the frequency is given or the maximum frequency for which a given
mesh size is valid. For example, in air at room temperature,
meters per second. The following table gives some values for maximum internodal
distances to model given maximum frequencies
accurately:
Maximum Frequency of Interest,
Maximum Internodal Interval,
,
Maximum Internodal Interval,
,
100 Hz
< 430 mm
< 286 mm
500 Hz
< 86 mm
< 57 mm
1000 Hz
< 43 mm
<29mm
20 kHz
< 2.1 mm
< 1.4mm
For exterior problems the accuracy of an analysis also depends on the
accuracy of the absorbing boundary condition. As mentioned above, the absorbing
boundary impedance conditions implemented in
Abaqus
are used with a standoff thickness
of acoustic finite elements between the acoustic sources and the radiating
boundary. Since the approximate radiation conditions converge to the exact
condition in the limit of infinite standoff, a greater standoff thickness
improves the accuracy of the solution. The standoff thickness
is expressed as
wavelengths at the minimum frequency to be analyzed:
Continuing the example using the properties of air, we can calculate the
recommended minimum standoff thicknesses corresponding to a specified minimum
frequency of interest, using :
Minimum Frequency of Interest,
Radiation Boundary Standoff,
100 Hz
> 1140 mm
500 Hz
> 230 mm
1000 Hz
> 114 mm
20 kHz
> 5.7 mm
The computational requirements for an exterior problem thus depend on both
the radiation boundary standoff and the internodal distance. The number of
nodes N in a model depends on the volume of the mesh,
controlled by
and the spatial dimension d, and the mesh density,
controlled by .
The exact number of nodes depends on the details of the model, but the
expression
indicates the size of the model with respect to the ratio of the maximum to
minimum frequencies in a given analysis. Because the mesh size for an exterior
problem exhibits such strong dependence on the bandwidth,
,
you can control the size of an analysis by splitting the band. For example, if
the overall frequency range of interest is 100 to 10000 Hz, a single spherical
mesh covering this band in three dimensions has size
However, splitting the problem into two bands,
and ,
and creating an exterior mesh for each band, results in two analyses of size
In coupled acoustic-structural systems there usually exist different wave
speeds for the fluid and solid media. In the region of the acoustic-structural
interface, the wave phenomena in both media may exhibit length scales
characteristic of the slower medium; that is, the length scale of the wave
dynamics may be as short as the shorter wavelength, corresponding to the lower
wave speed. This result follows from the fact that the two media are coupled at
the boundary. The region near the acoustic-structural interface where these
effects are important is usually no thicker than the shorter wavelength.
For example, in an analysis involving water interacting with rubber, the
wave speed in the rubber may be much lower than that of water. A finite element
mesh used to model this problem in detail would require refinement down to six
(or more) nodes per shorter wavelength, on both sides of the interface. On the
water side (faster, longer wavelength) accuracy will probably not be
compromised significantly if this region of high refinement extends no further
into the water than one short wavelength. Of course, in some analyses the
effects in the vicinity of the interface may be unimportant. Then, the two
meshes can be refined only so far as to represent their own characteristic
wavelengths accurately.
Output
Nodal output variable POR (pressure magnitude at the nodes of the acoustic elements) is
available for an acoustic medium (in
Abaqus/CAE
this output variable is called
PAC). When the scattered wave formulation (default) is used
with incident wave loading, output variable POR represents only the scattered pressure response of the model
and does not include the incident wave loading itself. When the total wave
formulation is used, output variable POR represents the total dynamic acoustic pressure, which includes
contributions from both incident and scattered waves as well as the dynamic
effects of fluid cavitation. For either formulation output variable POR does not include the acoustic static pressure.
In
Abaqus/Explicit
an additional nodal output variable PABS (the absolute pressure, equal to the sum of POR and the acoustic static pressure) is available. When the
dynamic effects of fluid cavitation are of interest, you can specify the
acoustic static pressure in an acoustic analysis that uses the total wave
formulation. If the acoustic static pressure is not specified in an acoustic
region, it is assumed to be large; thus precluding cavitation in that region.
For general steps, including implicit and explicit dynamic steps, no energy
quantities are computed for acoustic elements. Consequently, these elements
will not contribute to the total energy balance.
Steady-State Dynamic Output
For steady-state dynamic analysis POR is complex and can be displayed in
several forms in
the Visualization module
of
Abaqus/CAE.
The phase angle (PPOR) is available as output to the data (.dat)
and results (.fil) files.
Several additional secondary quantities are available for multidimensional
acoustic finite elements in direct-solution steady-state dynamic or
subspace-based steady-state dynamic analysis. The “sound pressure level” is
defined as:
where
is defined as a physical constant in the model (see
Defining the Reference Pressure
below), and the
is computed from the complex-valued acoustic pressure
at any point using the formula:
The acoustic particle velocity at any material point is
The acoustic intensity vector, a measure of the rate of flow of energy at a
material point, is
In an acoustic medium the stress tensor is simply the acoustic pressure
times the identity tensor, so this expression simplifies to
The hats denote complex conjugation. The real part of the intensity is
referred to as the “active intensity,” and the imaginary part is the “reactive
intensity.” The acoustic pressure gradient is also available for acoustic
finite elements in steady-state dynamic analysis.
In steady-state dynamic analysis, additional nodal output quantities are
available for acoustic infinite elements.
PINF denotes the complex pressure coefficients of the infinite
element shape functions. These coefficients can be used to visualize the
exterior acoustic field (i.e., within the volume of the acoustic infinite
elements) using scripting in
the Visualization module of Abaqus/CAE;
see
Using infinite elements to compute and view the results of an acoustic far-field analysis.
INFN is the normal vector used by the acoustic infinite element to
define the element volume. INFR denotes the radius used for the element at that node, and INFC denotes the element cosine; that is, the minimum dot product
between the nodal normal vector and the acoustic infinite element facet normal
vectors attached to that node. See
Acoustic infinite elements
for more complete descriptions of these quantities. INFN, INFR, INFC are useful in debugging a model using acoustic infinite
elements; consequently, it is sometimes valuable to perform a steady-state
dynamics, direct analysis on a model to visualize this information.
For steady-state dynamic steps, energy quantities are available for acoustic
elements. These elements contribute to the total energy balance in steady-state
dynamics.
Defining the Reference Pressure
You must define the reference pressure, ,
used to compute the sound pressure level; there is no default value for the
reference pressure.
Input File Template
The following is an example of the step definition for a
direct-solution steady-state dynamic acoustic analysis that looks for the
response of a model at six frequencies ranging linearly from
to
cycles/time. The pressure at node set INPUT
(nodes at the boundary) is prescribed to have an in-phase component of 3.0 and
an out-of-phase component of −4.0 (i.e., a complex value of
).
An in-phase inward volume acceleration of 40.0 is specified at node 10.
On the surface LINER1 an impedance is
defined based on the impedance property named
CARPET1. On the second face of all of the
elements in element set PAD, another surface
impedance based on CARPET1 is defined. On the
fourth face of all of the elements in element set
END, the default plane wave boundary condition
is specified.
Printed output of pressure magnitude and phase is
requested for node set OUTPUT. Acoustic
pressure and displacement are written to the output database. All output is
written once for each of the six excitation frequencies.
HEADING
…
SURFACE, NAME=LINER1
10, S3
IMPEDANCE PROPERTY, NAME=CARPET1
Data describing impedance properties as a function of frequency
**
STEPSTEADY STATE DYNAMICS, DIRECT
10, 100, 6
SIMPEDANCE, PROPERTY=CARPET1
LINER1,
**
IMPEDANCE, PROPERTY=CARPET1
PAD, I2
IMPEDANCE
END, I4
** Apply complex pressure at node set INPUT
BOUNDARY, REAL
INPUT, 8, 8, 3.
BOUNDARY, IMAGINARY
INPUT, 8, 8, -4.
** Apply an in-phase inward volume acceleration at node 10
CLOAD
10, 8, 40.
** Output requests
NODE PRINT, NSET=OUTPUT, TOTALS=YESPOR, PPOROUTPUT, FIELDNODE OUTPUTU, PU, POREND STEP
The following is a template of the step definition for an
Abaqus/Explicit
acoustic analysis. On the surface SURF an
impedance is defined based on the impedance property named
IPROP. In addition, impedance is defined on
elements or element sets.
The following template is representative of a coupled
acoustic-structural shock problem using the preferred interface for applying
incident wave loading (see
Incident Wave Loading due to External Sources):
HEADING
…
ELEMENT, TYPE=…, ELSET=ACOUSTIC
Data lines to define acoustic elementsELEMENT, TYPE=…, ELSET=SOLID
Data lines to define solid elementsELEMENT, TYPE=…, ELSET=BEAM
Data lines to define beam elementsBEAM SECTION,ELSET=BEAM,MATERIAL=...
Data lines to define the beam stiffness section propertiesBEAM FLUID INERTIAData line to define the beam virtual mass propertySURFACE, NAME=IW_LOAD_ACOUSTIC
Data lines to define the acoustic surface loaded by the incident waveSURFACE, NAME=IW_LOAD_SOLID
Data lines to define the solid surface loaded by the incident waveSURFACE, NAME=IW_LOAD_BEAM
Data lines to define the beam surface loaded by the incident waveSURFACE, NAME=TIE_ACOUSTIC
Data lines to define the acoustic surface interface with the solid meshSURFACE, NAME=TIE_SOLID
Data lines to define the solid surface interface with the acoustic meshINCIDENT WAVE INTERACTION PROPERTY, NAME=IWPROP, TYPE=SPHEREData lines to define a spherical incident wave fieldUNDEX CHARGE PROPERTYData lines to define the underwater explosion parameters
** Tie the acoustic mesh to the solid mesh
TIE, NAME=COUPLING
TIE_ACOUSTIC, TIE_SOLID
STEPDYNAMIC, EXPLICIT or DYNAMIC
** Load the acoustic surface
INCIDENT WAVE INTERACTION, PROPERTY=IWPROP
IW_LOAD_ACOUSTIC, source node, standoff node, reference magnitude
** Load the solid surface
INCIDENT WAVE INTERACTION, PROPERTY=IWPROP
IW_LOAD_SOLID, source node, standoff node, reference magnitude
** Load the beam surface
INCIDENT WAVE INTERACTION, PROPERTY=IWPROP
IW_LOAD_BEAM, source node, standoff node, reference magnitudeEND STEP
The following template is representative of a coupled
acoustic-structural shock problem using the alternative interface for applying
incident wave loading:
HEADING
…
ELEMENT, TYPE=…, ELSET=ACOUSTIC
Data lines to define acoustic elementsELEMENT, TYPE=…, ELSET=SOLID
Data lines to define solid elementsELEMENT, TYPE=…, ELSET=BEAM
Data lines to define beam elementsBEAM SECTION,ELSET=BEAM,MATERIAL=...
Data lines to define the beam stiffness section propertiesBEAM FLUID INERTIAData line to define the beam virtual mass propertySURFACE, NAME=IW_LOAD_ACOUSTIC
Data lines to define the acoustic surface loaded by the incident waveSURFACE, NAME=IW_LOAD_SOLID
Data lines to define the solid surface loaded by the incident waveSURFACE, NAME=IW_LOAD_BEAM
Data lines to define the beam surface loaded by the incident waveSURFACE, NAME=TIE_ACOUSTIC
Data lines to define the acoustic surface interface with the solid meshSURFACE, NAME=TIE_SOLID
Data lines to define the solid surface interface with the acoustic meshINCIDENT WAVE PROPERTY, NAME=IWPROP, TYPE=SPHEREData lines to define a spherical incident wave fieldINCIDENT WAVE FLUID PROPERTYData lines to define the fluid properties for the incident wave fieldAMPLITUDE, DEFINITION=BUBBLE, NAME=PRESSUREVTIME
Data lines to define the underwater explosion parameters
** Tie the acoustic mesh to the solid mesh
TIE, NAME=COUPLING
TIE_ACOUSTIC, TIE_SOLID
STEPDYNAMIC or DYNAMIC, EXPLICIT
** Load the acoustic surface
INCIDENT WAVE, PRESSURE AMPLITUDE=PRESSUREVTIME,
PROPERTY=IWPROP
IW_LOAD_ACOUSTIC, {amplitude}
** Load the solid surface and the beam surface
INCIDENT WAVE, PRESSURE AMPLITUDE=PRESSUREVTIME,
PROPERTY=IWPROP
IW_LOAD_SOLID, {amplitude}
IW_LOAD_BEAM, {amplitude}
END STEP
The following template is representative of a coupled
acoustic-structural sound transmission problem using the preferred interface
for applying incident wave loading (see
Incident Wave Loading due to External Sources):
HEADING
…
ELEMENT, TYPE=…, ELSET=ACOUSTIC
Data lines to define acoustic elementsELEMENT, TYPE=…, ELSET=SOLID
Data lines to define solid elementsSURFACE, NAME=IW_LOAD_ACOUSTIC
Data lines to define the acoustic surface loaded by the incident waveSURFACE, NAME=IW_LOAD_SOLID
Data lines to define the solid surface loaded by the incident waveSURFACE, NAME=TIE_ACOUSTIC
Data lines to define the acoustic surface interface with the solid meshSURFACE, NAME=TIE_SOLID
Data lines to define the solid surface interface with the acoustic meshINCIDENT WAVE INTERACTION PROPERTY, NAME=FIRST, TYPE=SPHEREData lines to define a spherical incident wave fieldINCIDENT WAVE INTERACTION PROPERTY, NAME=SECOND, TYPE=PLANEData lines to define a planar incident wave field
** Tie the acoustic mesh to the solid mesh
TIE, NAME=COUPLING
TIE_ACOUSTIC, TIE_SOLID
STEPSTEADY STATE DYNAMICS, DIRECT or SUBSPACE PROJECTION
** Define the load on the acoustic and solid surfaces due to
** the first loading case:
LOAD CASE, NAME=FIRST_SOURCE
** Load the acoustic surface: define the real part at the
** standoff point
INCIDENT WAVE INTERACTION, PROPERTY=FIRST, REAL
IW_LOAD_ACOUSTIC, first source node, first standoff node, reference magnitude
** Load the acoustic surface: define the imaginary part at the
** standoff point
INCIDENT WAVE INTERACTION, PROPERTY=FIRST, IMAGINARY
IW_LOAD_ACOUSTIC, first source node, first standoff node, reference magnitude
** Load the solid surface: define the real part at the
** standoff point
INCIDENT WAVE INTERACTION, PROPERTY=FIRST, REAL
IW_LOAD_SOLID, first source node, first standoff node, reference magnitude
** Load the solid surface: define the imaginary part at the
** standoff point
INCIDENT WAVE INTERACTION, PROPERTY=FIRST, IMAGINARY
IW_LOAD_SOLID, first source node, first standoff node, reference magnitudeEND LOAD CASE
** Define the load on the acoustic and solid surfaces due to
** the next loading case:
LOAD CASE, NAME=SECOND_SOURCE
** Load the acoustic surface: define the real part at the
** standoff point
INCIDENT WAVE INTERACTION, PROPERTY=SECOND, REAL
IW_LOAD_ACOUSTIC, second source node, second standoff node, reference magnitude
** Load the acoustic surface: define the imaginary part at the
** standoff point
INCIDENT WAVE INTERACTION, PROPERTY=SECOND, IMAGINARY
IW_LOAD_ACOUSTIC, second source node, second standoff node, reference magnitude
** Load the solid surface: define the real part at the
** standoff point
INCIDENT WAVE INTERACTION, PROPERTY=SECOND, REAL
IW_LOAD_SOLID, second source node, second standoff node, reference magnitude
** Load the solid surface: define the imaginary part at the
** standoff point
INCIDENT WAVE INTERACTION, PROPERTY=SECOND, IMAGINARY
IW_LOAD_SOLID, second source node, second standoff node, reference magnitudeEND LOAD CASEEND STEP