김경종
302 lines
26 KiB
Markdown
302 lines
26 KiB
Markdown
<!-- source-page: 171 -->
|
||
|
||
Input File Usage: \*DSECURRENT surface name, CS, current density magnitude
|
||
|
||
Abaqus/CAE Usage: Load module: Create Load: choose Electrical/Magnetic for the Category and Surface current for the Types for Selected Step: Distribution: Uniform, Magnitude: current density magnitude
|
||
|
||
# Prescribing electromagnetic loads for eddy current and/or magnetostatic analyses
|
||
|
||
In an eddy current analysis a distributed surface current density vector can be defined on surfaces and a distributed volume current density vector can be defined on elements.
|
||
|
||
# Specifying element-based distributed current density vectors
|
||
|
||
When you define a distributed volume current density vector, you must specify the element or element set, the current density vector label, the magnitude of the current density vector, the vector components of the current density, and an optional orientation name that defines the local coordinate system in which the vector components are specified. By default, the vector components of the current density are defined with respect to the global directions.
|
||
|
||
The specified current density vector direction components are normalized by Abaqus and, thus, do not contribute to the magnitude of the load.
|
||
|
||
Input File Usage: \*DECURRENT element number or element set name, CJ, current density vector magnitude, current density vector direction components, orientation name
|
||
|
||
Abaqus/CAE Usage: Load module: Create Load: choose Electrical/Magnetic for the Category and Body current density for the Types for Selected Step; Distribution: Uniform
|
||
|
||
# Specifying surface-based distributed current density vectors
|
||
|
||
When you specify distributed current density vectors on a surface, the element-based surface (see “Element-based surface definition,” Section 2.3.2) contains the element and face information. You must specify the surface name, the current density vector label, and the magnitude of the current density vector, the vector components of the current density, and an optional orientation name that defines the local coordinate system in which the surface current density is specified. By default, the vector components of the current density are defined with respect to the global directions.
|
||
|
||
The specified current density vector direction components are normalized by Abaqus and, thus, do not contribute to the magnitude of the load.
|
||
|
||
Input File Usage: \*DSECURRENT surface name, CK, current density vector magnitude, current density vector direction components, orientation name
|
||
|
||
Abaqus/CAE Usage: Load module: Create Load: choose Electrical/Magnetic for the Category and Surface current density for the Types for Selected Step; Distribution: Uniform
|
||
|
||
<!-- source-page: 172 -->
|
||
|
||
# Defining nonuniform current density vectors in a user subroutine
|
||
|
||
Nonuniform volume current density vectors can be defined with user subroutine UDECURRENT, and nonuniform surface current density vectors can be defined with user subroutine UDSECURRENT. If the magnitude and direction components are given, the values are passed into the user subroutine.
|
||
|
||
Input File Usage: Use the following option to define nonuniform element-based current density vectors:
|
||
|
||
\*DECURRENT
|
||
|
||
element number or element set name, CJNU, current density vector magnitude, current density vector direction components, orientation name
|
||
|
||
Use the following option to define nonuniform surface-based current density vectors:
|
||
|
||
\*DSECURRENT
|
||
|
||
surface name, CKNU, current density vector magnitude, current density vector direction components, orientation name
|
||
|
||
Abaqus/CAE Usage: Use the following option to define nonuniform volume current density:
|
||
|
||
Load module: Create Load: choose Electrical/Magnetic for the Category and Body current density for the Types for Selected Step; Distribution: User-defined
|
||
|
||
Use the following option to define nonuniform surface current density:
|
||
|
||
Load module: Create Load: choose Electrical/Magnetic for the Category and Surface current density for the Types for Selected Step; Distribution: User-defined
|
||
|
||
# Specifying real and imaginary components of current density vectors in a time-harmonic eddy current analysis
|
||
|
||
In a time-harmonic eddy current analysis, current density vectors are given in terms of their real (inphase) and imaginary (out-of-phase) components.
|
||
|
||
Input File Usage: Use the following options to define current density vectors:
|
||
|
||
\*DECURRENT, REAL or IMAGINARY
|
||
|
||
\*DSECURRENT, REAL or IMAGINARY
|
||
|
||
Abaqus/CAE Usage: Load module: Create Load: choose Electrical/Magnetic for the Category and Body current density or Surface current density for the Types for Selected Step; real components + imaginary components
|
||
|
||
<!-- source-page: 173 -->
|
||
|
||
# 34.4.6 ACOUSTIC AND SHOCK LOADS
|
||
|
||
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Applying loads: overview,” Section 34.4.1
|
||
• “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1
|
||
• \*AMPLITUDE
|
||
• \*BOUNDARY
|
||
• \*CLOAD
|
||
• \*CONWEP CHARGE PROPERTY
|
||
• \*IMPEDANCE
|
||
• \*IMPEDANCE PROPERTY
|
||
• \*INCIDENT WAVE
|
||
• \*INCIDENT WAVE FLUID PROPERTY
|
||
• \*INCIDENT WAVE INTERACTION
|
||
• \*INCIDENT WAVE INTERACTION PROPERTY
|
||
• \*INCIDENT WAVE PROPERTY
|
||
• \*INCIDENT WAVE REFLECTION
|
||
• \*SIMPEDANCE
|
||
• \*UNDEX CHARGE PROPERTY
|
||
• “Defining acoustic impedance,” Section 15.13.17 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
• “Defining incident waves,” Section 15.13.18 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
• “Defining an acoustic impedance interaction property,” Section 15.14.6 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
• “Defining an incident wave interaction property,” Section 15.14.7 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
|
||
# Overview
|
||
|
||
Acoustic loads can be applied only in transient or steady-state dynamic analysis procedures. The following types of acoustic loads are available:
|
||
|
||
• Boundary impedance defined on element faces or on surfaces.
|
||
• Nonreflecting radiation boundaries in exterior problems such as a structure vibrating in an acoustic medium of infinite extent.
|
||
|
||
<!-- source-page: 174 -->
|
||
|
||
• Concentrated pressure-conjugate loads prescribed at acoustic element nodes.
|
||
• Temporally and spatially varying pressure loading on acoustic and solid surfaces due to incident waves traveling through the acoustic medium.
|
||
|
||
# Specified boundary impedance
|
||
|
||
A boundary impedance specifies the relationship between the pressure of an acoustic medium and the normal motion at the boundary. Such a condition is applied, for example, to include the effect of smallamplitude “sloshing” in a gravity field or the effect of a compressible, possibly dissipative, lining (such as a carpet) between an acoustic medium and a fixed, rigid wall or structure.
|
||
|
||
The impedance boundary condition at any point along the acoustic medium surface is governed by
|
||
|
||
$$
|
||
\dot {u} _ {o u t} = \frac {1}{k _ {1}} \dot {p} + \frac {1}{c _ {1}} p,
|
||
$$
|
||
|
||
where
|
||
|
||
uout $\dot { u } _ { o u t }$ is the acoustic particle velocity in the outward normal direction of the acoustic medium surface,
|
||
|
||
$\pmb { p }$ is the acoustic pressure,
|
||
|
||
$\dot { p }$ is the time rate of change of the acoustic pressure,
|
||
|
||
$1 / k _ { 1 }$ is the proportionality coefficient between the pressure and the displacement normal to the surface, and
|
||
|
||
$1 / c _ { 1 }$ is the proportionality coefficient between the pressure and the velocity normal to the surface.
|
||
|
||
This model can be conceptualized as a spring and dashpot in series placed between the acoustic medium and a rigid wall. The spring and dashpot parameters are $k _ { 1 }$ and $c _ { 1 }$ , respectively, defined per unit area of the interface surface. These reactive acoustic boundaries can have a significant effect on the pressure distribution in the acoustic medium, in particular if the coefficients $k _ { 1 }$ and $c _ { 1 }$ are chosen such that the boundary is energy absorbing. If no impedance, loads, or fluid-solid coupling are specified on the surface of an acoustic mesh, the acceleration of that surface is assumed to be zero. This is equivalent to the presence of a rigid wall at that boundary.
|
||
|
||
Use of the subspace-based steady-state dynamics procedure is not recommended if reactive acoustic boundaries with strong absorption characteristics are used. Since the effect of $\dot { c } _ { 1 }$ is not taken into account in an eigenfrequency extraction step, the eigenmodes may have shapes that are significantly different from the exact solution.
|
||
|
||
# Sloshing of a free surface
|
||
|
||
To model small-amplitude “sloshing” of a free surface in a gravity field, set $1 / k _ { 1 } = 1 / ( \rho _ { f } g )$ and $1 / c _ { 1 } = $ , where $\rho _ { f }$ is the density of the fluid and g is the gravitational acceleration (assumed to be directed normal to the surface). This relation holds for small volumetric drag.
|
||
|
||
<!-- source-page: 175 -->
|
||
|
||
# Acoustic-structural interface
|
||
|
||
The impedance boundary condition can also be placed at an acoustic-structural interface. In this case the boundary condition can be conceptualized as a spring and dashpot in series placed between the acoustic medium and the structure. The expression for the outward velocity still holds, with $\dot { u } _ { o u t }$ now being the relative outward velocity of the acoustic medium and the structure:
|
||
|
||
$$
|
||
\dot {u} _ {o u t} = \mathbf {n} \cdot (\dot {\mathbf {u}} ^ {f} - \dot {\mathbf {u}} ^ {m}),
|
||
$$
|
||
|
||
where $\dot { \mathbf { u } } ^ { m }$ is the velocity of the structure, $\dot { \mathrm { ~ \bf ~ u ~ } } ^ { f }$ is the velocity of the acoustic medium at the boundary, and is the outward normal to the acoustic medium.
|
||
|
||
# Steady-state dynamics
|
||
|
||
In a steady-state dynamics analysis the expression for the outward velocity can be written in complex form as
|
||
|
||
$$
|
||
\dot {u} _ {o u t} = (\frac {1}{c _ {1}} + i \frac {\Omega}{k _ {1}}) p = \frac {1}{Z (\Omega)} p,
|
||
$$
|
||
|
||
where is the circular frequency (radians/second) and we define
|
||
|
||
$$
|
||
\frac {1}{Z (\Omega)} \equiv \frac {1}{c _ {1}} + i \frac {\Omega}{k _ {1}}.
|
||
$$
|
||
|
||
The term $1 / Z ( \Omega )$ is the complex admittance of the boundary, and $Z ( \Omega )$ is its complex impedance. Thus, a required complex impedance or admittance value can be entered for a given frequency by specifying the parameters $1 / c _ { 1 }$ and $1 / k _ { 1 }$ .
|
||
|
||
# Specifying impedance conditions
|
||
|
||
You specify impedance coefficient data in an impedance property table. You can describe an impedance table in terms of the admittance parameters, $1 / c _ { 1 }$ and $1 / k _ { 1 }$ , or in terms of the real and imaginary parts of the impedance. In the latter case Abaqus converts the user-defined table of impedance data to the admittance parameter form for the analysis.
|
||
|
||
The parameters in the table can be specified over a range of frequencies. The required values are interpolated from the table in steady-state harmonic response analysis only; for other analysis types, only the first table entry is used. The name of the impedance property table is referred to from a surface-based or element-based impedance definition. In Abaqus/CAE impedance conditions are always surface-based; surfaces can be defined as collections of geometric faces and edges or collections of element faces and edges.
|
||
|
||
In a steady-state dynamics analysis you cannot specify impedance conditions on a surface on which incident wave loading is applied.
|
||
|
||
<!-- source-page: 176 -->
|
||
|
||
<table><tr><td>Input File Usage:</td><td>Use the following option to specify an impedance using a table of admittance parameters (default):*IMPEDANCE PROPERTY, NAME=impedance property table name, DATA=ADMITTANCEUse the following option to specify an impedance using a table of the real and imaginary parts of the impedance:*IMPEDANCE PROPERTY, NAME=impedance property table name, DATA=IMPEDANCE</td></tr><tr><td>Abaqus/CAE Usage:</td><td>Use the following input to specify an impedance using a table of admittance parameters:Interaction module: Create Interaction Property: Name: impedance property table name and Acoustic impedance: Data type: AdmittanceUse the following input to specify an impedance using a table of the real and imaginary parts of the impedance:Interaction module: Create Interaction Property: Name: impedance property table name and Acoustic impedance: Data type: Impedance</td></tr></table>
|
||
|
||
# Specifying surface-based impedance conditions
|
||
|
||
You can define the impedance condition on a surface. The impedance is applied to element edges in two dimensions and to element faces in three dimensions. The element-based surface (see “Element-based surface definition,” Section 2.3.2) contains the element and face information.
|
||
|
||
Input File Usage: \*SIMPEDANCE, PROPERTY=impedance property table name surface name
|
||
|
||
Abaqus/CAE Usage: Interaction module: Create Interaction: Acoustic impedance: select surface: Definition: Tabular, Acoustic impedance property: impedance property table name
|
||
|
||
# Specifying element-based impedance conditions
|
||
|
||
Alternatively, you can define the impedance condition on element faces. The impedance is applied to element edges in two dimensions and to element faces in three dimensions. The edge or face of the element upon which the impedance is placed is identified by an impedance load type and depends on the element type (see Part VI, “Elements”).
|
||
|
||
Input File Usage: \*IMPEDANCE, PROPERTY=impedance property table name element number or set name, impedance load type label
|
||
|
||
Abaqus/CAE Usage: Element-based impedance conditions are not supported in Abaqus/CAE. However, similar functionality is available using surface-based impedance conditions.
|
||
|
||
<!-- source-page: 177 -->
|
||
|
||
# Modifying or removing impedance conditions
|
||
|
||
Impedance conditions can be added, modified, or removed as described in “Applying loads: overview,” Section 34.4.1.
|
||
|
||
# Radiation boundaries for exterior problems
|
||
|
||
An exterior problem such as a structure vibrating in an acoustic medium of infinite extent is often of interest. Such a problem can be modeled by using acoustic elements to model the region between the structure and a simple geometric surface (located away from the structure) and applying a radiating (nonreflecting) boundary condition at that surface. The radiating boundary conditions are approximate, so 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 surface is at least one-half wavelength away from the structure at the lowest frequency of interest.
|
||
|
||
Except in the case of a plane wave absorbing condition with zero volumetric drag, the impedance parameters in Abaqus/Standard are frequency dependent. The frequency-dependent parameters are used in the direct-solution and subspace-based steady-state dynamics procedures. In direct time integration procedures the zero-drag values for the constants $1 / c _ { 1 }$ and $1 / k _ { 1 }$ are used. These values will give good results when the drag is small. (Small volumetric drag here means $\gamma < < \rho _ { f } \Omega$ where $\rho _ { f }$ is the density of the acoustic medium and is the circular excitation frequency or sound wave frequency.)
|
||
|
||
A direct-solution steady-state dynamics procedure (“Direct-solution steady-state dynamic analysis,” Section 6.3.4) must include both real and complex terms if nonreflecting (also called quiet) boundaries are present, because nonreflecting boundaries represent a form of damping in the system.
|
||
|
||
Several radiating boundary conditions are implemented as special cases of the impedance boundary condition. The details of the formulation are given in “Coupled acoustic-structural medium analysis,” Section 2.9.1 of the Abaqus Theory Guide.
|
||
|
||
Element-based impedance conditions are not supported in Abaqus/CAE. However, similar functionality is available using surface-based impedance conditions.
|
||
|
||
# Planar nonreflecting boundary condition
|
||
|
||
The simplest nonreflecting boundary condition available in Abaqus assumes that the plane waves are normally incident on the exterior surface. This planar boundary condition ignores the curvature of the boundary and the possibility that waves in the simulation may impinge on the boundary at an arbitrary angle. The planar nonreflecting condition provides an approximation: acoustic waves are transmitted across such a boundary with little reflection of energy back into the acoustic medium. The amount of energy reflected is small if the boundary is far away from major acoustic disturbances and is reasonably orthogonal to the direction of dominant wave propagation. Thus, if an exterior (unbounded domain) problem is to be solved, the nonreflecting boundary should be placed far enough away from the sound source so that the assumption of normally impinging waves is sufficiently accurate. This condition would be used, for example, on the exhaust end of a muffler.
|
||
|
||
<!-- source-page: 178 -->
|
||
|
||
Input File Usage: Use either of the following options (default):
|
||
|
||
\*SIMPEDANCE, NONREFLECTING=PLANAR
|
||
\*IMPEDANCE, NONREFLECTING=PLANAR
|
||
|
||
Abaqus/CAE Usage: Use the following input to specify a surface-based planar nonreflecting boundary condition:
|
||
|
||
Interaction module: Create Interaction: Acoustic impedance: select
|
||
|
||
surface: Definition: Nonreflecting, Nonreflecting type: Planar
|
||
|
||
# Improved nonreflecting boundary condition for plane waves
|
||
|
||
For the planar nonreflecting boundary condition to be accurate, the plane waves must be normally incident to a planar boundary. However, the angle of incidence is generally unknown in advance. A radiating boundary condition that is exact for plane waves with arbitrary angles of incidence is available in Abaqus. The radiating boundary can have any arbitrary shape. This boundary impedance is implemented only for transient dynamics.
|
||
|
||
Input File Usage: Use either of the following options:
|
||
|
||
\*SIMPEDANCE, NONREFLECTING=IMPROVED
|
||
\*IMPEDANCE, NONREFLECTING=IMPROVED
|
||
|
||
Abaqus/CAE Usage: Use the following input to specify a surface-based improved planar nonreflecting boundary condition:
|
||
|
||
Interaction module: Create Interaction: Acoustic impedance: select
|
||
|
||
surface: Definition: Nonreflecting, Nonreflecting type: Improved planar
|
||
|
||
# Geometry-based nonreflecting boundary conditions
|
||
|
||
Four other types of absorbing boundary conditions that take the geometry of the radiating boundary into account are implemented in Abaqus: circular, spherical, elliptical, and prolate spheroidal. These boundary conditions offer improved performance over the planar nonreflecting condition if the nonreflecting surface has a simple, convex shape and is close to the acoustic sources. The various types of absorbing boundaries are selected by defining the required geometric parameters for the element-based or surface-based impedance definition.
|
||
|
||
The geometric parameters affect the nonreflecting surface impedance. To specify a nonreflecting boundary that is circular in two dimensions or a right circular cylinder in three dimensions, you must specify the radius of the circle. To specify a nonreflecting spherical boundary condition, you must specify the radius of the sphere. To specify a nonreflecting boundary that is elliptical in two dimensions or a right elliptical cylinder in three dimensions or to specify a prolate spheroid boundary condition, you must specify the shape, location, and orientation of the radiating surface. The two parameters specifying the shape of the surface are the semimajor axis and the eccentricity. The semimajor axis, a, of an ellipse or prolate spheroid is analogous to the radius of a sphere: it is one-half the length of the longest line segment connecting two points on the surface. The semiminor axis, b, is one-half the length of the longest line segment that connects two points on the surface and is orthogonal to the semimajor axis line. The eccentricity, , is defined as $\epsilon = \sqrt { 1 - ( b / a ) ^ { 2 } }$ .
|
||
|
||
<!-- source-page: 179 -->
|
||
|
||
See “Acoustic radiation impedance of a sphere in breathing mode,” Section 1.11.3 of the Abaqus Benchmarks Guide, and “Acoustic-structural interaction in an infinite acoustic medium,” Section 1.11.4 of the Abaqus Benchmarks Guide, for benchmark problems showing the use of these conditions.
|
||
|
||
# Input File Usage:
|
||
|
||
Use one of the following options:
|
||
|
||
\*SIMPEDANCE, NONREFLECTING=CIRCULAR
|
||
\*SIMPEDANCE, NONREFLECTING=SPHERICAL
|
||
\*SIMPEDANCE, NONREFLECTING=ELLIPTICAL
|
||
\*SIMPEDANCE, NONREFLECTING=PROLATE SPHEROIDAL
|
||
|
||
In each case, the \*IMPEDANCE element-based option can be used instead of \*SIMPEDANCE.
|
||
|
||
# Abaqus/CAE Usage:
|
||
|
||
Use the following input to specify surface-based geometric nonreflecting boundary conditions:
|
||
|
||
Interaction module: Create Interaction: Acoustic impedance: select surface: Definition: Nonreflecting, Nonreflecting type: Circular, Spherical, Elliptical, or Prolate spheroidal
|
||
|
||
# Combining different radiation conditions in the same problem
|
||
|
||
Since the radiation boundary conditions for the different shapes are spatially local and do not involve discretization in the infinite exterior domain, an exterior boundary can consist of the combination of several shapes. The appropriate boundary condition can then be applied to each part of the boundary. For example, a circular cylinder can be terminated with hemispheres (see “Fully and sequentially coupled acoustic-structural analysis of a muffler,” Section 9.1.1 of the Abaqus Example Problems Guide), or an elliptical cylinder can be terminated with prolate spheroidal halves. This modeling technique is most effective if the boundaries between surfaces are continuous in slope as well as displacement, although this is not essential.
|
||
|
||
# Concentrated pressure-conjugate load
|
||
|
||
Distributed “loads” on acoustic elements can be interpreted as normal pressure gradients per unit density (dimensions of force per unit mass or acceleration). When used in Abaqus, the applied distributed loads must be integrated over a surface area, yielding a quantity with dimensions of force times area per unit mass (or volumetric acceleration). For analyses in the frequency domain and for transient dynamic analyses where the volumetric drag is zero, this acoustic load is equal to the volumetric acceleration of the fluid on the boundary. For example, a horizontal, flat rigid plate oscillating vertically imposes an acceleration on the acoustic fluid and an acoustic “load” equal to this acceleration times the surface area of the plate. For the transient dynamics formulation in the presence of volumetric drag, however, the specified “load” is slightly different. It is also a force times area per unit mass; but this force effect is partially lost to the volumetric drag, so the resulting volumetric acceleration of the fluid on the boundary is reduced. Noting this distinction for the special case of volumetric drag and transient dynamics, it is nevertheless convenient to refer to acoustic “loads” as volumetric accelerations in general.
|
||
|
||
<!-- source-page: 180 -->
|
||
|
||
An inward volumetric acceleration can be applied by a positive concentrated load on degree of freedom 8 at a node of an acoustic element that is on the boundary of the acoustic medium. In Abaqus/Standard you can specify the in-phase (real) part of a load (default) and the out-of-phase (imaginary) part of a load. Inward particle accelerations (force per unit mass in transient dynamics) on the face of an acoustic element should be lumped to concentrated loads representing inward volumetric accelerations on the nodes of the face in the same way that pressure on a face is lumped to nodal forces on stress/displacement elements.
|
||
|
||
Input File Usage: Use the following option to define the real part of the load:
|
||
|
||
\*CLOAD, REAL
|
||
|
||
Use the following option to define the imaginary part of the load:
|
||
|
||
\*CLOAD, IMAGINARY
|
||
|
||
Abaqus/CAE Usage: Load module: Create Load: choose Acoustic for the Category and Inward volume acceleration for the Types for Selected Step
|
||
|
||
# Incident wave loading due to external sources
|
||
|
||
Abaqus provides a type of distributed load for loads due to external wave sources. Individual spherical monopole or individual or diffuse planar sources can be defined, subjecting the fluid and solid region of interest to an incident field of waves. Waves produced by an explosion or sound source propagate from the source, impinging on and passing over the structure, producing a temporally and spatially varying load on the structural surface. In the fluid the pressure field is affected by reflections and emissions from the structure as well as by the incident field from the source itself. The incident wave loads on acoustic and/or solid meshes depend on the location of the source node, the properties of the propagating fluid, and the reference time history or frequency dependence specified at the reference (“standoff”) node as indicated in Figure 34.4.6–1.
|
||
|
||
Several distinct modeling methods can be used in Abaqus with incident wave loading, requiring different approaches to applying the incident wave loads. For problems involving solid and structural elements only (for example, where the incident wave field is due to waves in air) the wave loading is applied roughly like a distributed surface load. This might apply to an analysis of blast loads in air on a vehicle or building (see “Example: airblast loading on a structure,” shown in Figure 34.4.6–6). In Abaqus/Explicit the CONWEP model can be used for air blast loading on solid and structural elements, without the need to model the fluid medium. “Deformation of a sandwich plate under CONWEP blast loading,” Section 9.1.9 of the Abaqus Example Problems Guide, is an example of a blast loading problem.
|
||
|
||
Incident wave loads (with the exception of CONWEP loading) can be applied to beam structures as well; this is a common modeling method for ship whipping analysis and for steel frame buildings subject to blast loads. Incident wave loads can be applied to surfaces defined on two- or three-dimensional beam elements. However, incident wave loads can be applied only to three-dimensional beams for transient dynamic analysis where beam fluid inertia is defined. Incident wave loads cannot be defined on frame elements, line spring elements, three-dimensional open-section beam elements, or three-dimensional Euler-Bernoulli beams.
|