Analyses performed with 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 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, Abaqus extracts real-valued coupled modes by default using the Lanczos and the subspace
iteration eigenfrequency extraction procedures. You can suppress coupling 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. You can also extract the coupled acoustic-structural modes when using the
AMS eigensolver.
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 and the subspace iteration eigensolvers
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.
Input File Usage
Use the following option to define a translating fluid velocity:
Acoustic flow velocity is not supported in Abaqus/CAE.
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.
Input File Usage
Use either of the following options to define the real (in-phase) part of the
boundary condition:
Load module: Create Boundary Condition: choose Other for the
Category and Acoustic pressure for the Types for Selected Step:
select regions: Magnitude: real (in-phase) part + imaginary (out-of-phase) parti
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.
Input File Usage
Use the following option in an analysis with the fluid mesh surface as the
secondary:
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.
Input File Usage
Use the following options in the global (structural) analysis to be followed by a
submodeling analysis:
Use the following input in the submodeling (fluid) analysis that uses an acoustic
interface on the fluid boundary to be driven:
Load module: Create Boundary Condition: choose Other for the
Category and Submodel for the Types for Selected Step:
select regions for fluid_boundary_to _be_driven: Exterior tolerance:
relative: tolerance; Degrees of freedom: 1, 3; Global step number: 1
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.
You cannot define a perfectly matched layer property in Abaqus/CAE.
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 PAC (pressure
magnitude at the nodes of the acoustic elements, alias of
POR) is available for an acoustic
medium (in Abaqus/CAE this output variable is called POR). 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.
You cannot define a reference pressure in Abaqus/CAE.
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