김경종
32 KiB
transport; subsequent linear perturbation steps are analyzed about this deformed state (see “Steady-state transport analysis,” Section 6.4.1). 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, TRANSLATIONUse the following option to define a rotating fluid velocity:*ACOUSTIC FLOW VELOCITY, ROTATION |
Abaqus/CAE Usage: 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.
The adaptive meshing features for acoustic analysis are described in detail in “Defining ALE adaptive mesh domains in Abaqus/Standard,” Section 12.2.6, and “ALE adaptive meshing and remapping in Abaqus/Standard,” Section 12.2.7.
Initial conditions
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 in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) 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 in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) 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,” Section 34.4.6), 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,” Section 34.4.6). 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 in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1). 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:*BOUNDARY*BOUNDARY, REALUse the following option to define the imaginary (out-of-phase) part of the boundary condition:*BOUNDARY, IMAGINARY |
| Abaqus/CAE Usage: | 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) part i |
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,” Section 2.9.1 of the Abaqus Theory Guide).
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 slave 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,” Section 32.13.2) 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,” Section 35.3.1). No additional element definitions are required.
The slave surface, the first of the two surfaces specified for the tie constraint, must be element-based; whereas the master 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 master 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 slave surface overhangs the master surface significantly, the regions of influence may include parts of the overhang. Consequently, the overhanging part of the slave surface may exhibit nonphysical coupled degrees of freedom: displacements if the slave surface is acoustic and acoustic pressures if the slave 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 slave:
*TIE, NAME=fluidslave fluid_surf, struct_surface
Use the following option in an analysis with the solid mesh surface as the slave:
*TIE, NAME=solidslave
struct_surf, fluid_surf
Abaqus/CAE Usage: Interaction module: Create Constraint: Tie
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,” Section 35.3.1), 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 slave 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 master 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 slave 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 “Submodeling: overview,” Section 10.2.1) 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:
*NSET, NSET=solid_boundary_driving_the_fluid
*NODE FILE, NSET=solid_boundary_driving_the_fluid U
Use the following options in the subsequent submodeling (fluid) analysis that uses acoustic interface elements on the fluid boundary to be driven:
*NSET, NSET=fluid_boundary_to_be_driven
*SUBMODEL, EXTERIOR TOLERANCE=tolerance
fluid_boundary_to_be_driven
*BOUNDARY, SUBMODEL, STEP=1
fluid_boundary_to be_driven, 1, 3,
Abaqus/CAE Usage: 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 master 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,” Section 35.2.2).
- 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.
- Define the beam section (“Using a beam section integrated during the analysis to define the section behavior,” Section 29.3.6, or “Using a general beam section to define the section behavior,” Section 29.3.7), any additional internal inertia (“Adding inertia to the beam section behavior for Timoshenko beams” in “Beam section behavior,” Section 29.3.5), and the beam material properties.
- Define the virtual mass effect (“Additional inertia due to immersion in fluid” in “Beam section behavior,” Section 29.3.5).
- If the model is to be loaded using an incident wave (“Incident wave loading due to external sources” in “Acoustic and shock loads,” Section 34.4.6), define a surface or surfaces on the beam elements.
Loads
The following types of loading can be prescribed in an acoustic analysis, as described in “Acoustic and shock loads,” Section 34.4.6:
• 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.
See “Acoustic and shock loads,” Section 34.4.6, for several examples of incident wave loading.
• 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 midair 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,” Section 34.4.6, 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,” Section 34.6.1:
• 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-variabledependent material properties.
Material options
Only the acoustic medium material model (“Acoustic medium,” Section 26.3.1) 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,” Section 21.2.1) 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,” Section 26.3.1, 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.
Elements
Abaqus provides a set of elements for modeling an acoustic medium undergoing small pressure changes. In addition, Abaqus/Standard provides interface elements to couple these acoustic elements to a structural model (see “Choosing the appropriate element for an analysis type,” Section 27.1.3). If interface elements are used, only direct-solution steady-state harmonic (linear) response analysis (“Direct-solution steadystate dynamic analysis,” Section 6.3.4) and transient response analysis (“Implicit dynamic analysis using direct integration,” Section 6.3.2) can be performed.
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 directsolution 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.
For details, see “Acoustic and shock loads,” Section 34.4.6.
Acoustic infinite elements
Acoustic infinite elements are provided for modeling exterior problems (“Infinite elements,” Section 28.3.1). 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,” Section 2.1.4) 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,” Section 28.3.1, 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.
Input File Usage: *PERFECTLY MATCHED LAYER, ELSET=element set label, MATERIAL=material name *PML COEFFICIENT, VARIATION=LINEAR
Abaqus/CAE Usage: 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