김경종
279 lines
24 KiB
Markdown
279 lines
24 KiB
Markdown
<!-- source-page: 211 -->
|
||
|
||
Abaqus/CAE Usage: Load module: load editor: real (in-phase) part + imaginary (out-of-phase) part i
|
||
|
||
# Frequency-dependent loading
|
||
|
||
An amplitude definition can be used to specify the amplitude of a load as a function of frequency (“Amplitude curves,” Section 34.1.2).
|
||
|
||
Input File Usage: Use both of the following options: \*AMPLITUDE, NAME=name \*CLOAD or \*DLOAD, REAL or IMAGINARY, AMPLITUDE=name
|
||
|
||
Abaqus/CAE Usage: Load or Interaction module: Create Amplitude: Name: name Load module: load editor: real (in-phase) part + imaginary (out-of-phase) part i: Amplitude: name
|
||
|
||
# Predefined fields
|
||
|
||
Predefined temperature fields can be specified in direct-solution steady-state dynamic analysis (see “Predefined fields,” Section 34.6.1) and will produce harmonically varying thermal strains if thermal expansion is included in the material definition (“Thermal expansion,” Section 26.1.2). Other predefined fields are ignored.
|
||
|
||
# Material options
|
||
|
||
As in any dynamic analysis procedure, mass or density (“Density,” Section 21.2.1) must be assigned to some regions of any separate parts of the model where dynamic response is required. If an analysis is desired in which the inertia effects are neglected, the density should be set to a very small number. The following material properties are not active during steady-state dynamic analyses: plasticity and other inelastic effects, thermal properties (except for thermal expansion), mass diffusion properties, electrical properties (except for the electrical potential, , in piezoelectric analysis), and pore fluid flow properties—see “General and linear perturbation procedures,” Section 6.1.3.
|
||
|
||
Viscoelastic effects can be included in direct-solution steady-state harmonic response analysis. The linearized viscoelastic response is considered to be a perturbation about a nonlinear preloaded state, which is computed on the basis of purely elastic behavior (long-term response) in the viscoelastic components. Therefore, the vibration amplitude must be sufficiently small so that the material response in the dynamic phase of the problem can be treated as a linear perturbation about the predeformed state. Viscoelastic frequency domain response is described in “Frequency domain viscoelasticity,” Section 22.7.2.
|
||
|
||
# Elements
|
||
|
||
Any of the following elements available in Abaqus/Standard can be used in a steady-state dynamic procedure:
|
||
|
||
• stress/displacement elements (other than generalized axisymmetric elements with twist);
|
||
|
||
<!-- source-page: 212 -->
|
||
|
||
• acoustic elements;
|
||
• piezoelectric elements; or
|
||
• hydrostatic fluid elements.
|
||
|
||
See “Choosing the appropriate element for an analysis type,” Section 27.1.3.
|
||
|
||
# Output
|
||
|
||
In direct-solution steady-state dynamic analysis the value of an output variable such as strain (E) or stress (S) is a complex number with real and imaginary components. In the case of data file output the first printed line gives the real components while the second lists the imaginary components. Results and data file output variables are also provided to obtain the magnitude and phase of many variables (see “Abaqus/Standard output variable identifiers,” Section 4.2.1). In the case of data file output the first printed line gives the magnitudes while the second lists the phase angle.
|
||
|
||
The following variables are provided specifically for steady-state dynamic analysis:
|
||
|
||
Element integration point variables:
|
||
|
||
<table><tr><td>PHS</td><td>Magnitude and phase angle of all stress components.</td></tr><tr><td>PHE</td><td>Magnitude and phase angle of all strain components.</td></tr><tr><td>PHEPG</td><td>Magnitude and phase angles of the electrical potential gradient vector.</td></tr><tr><td>PHEFL</td><td>Magnitude and phase angles of the electrical flux vector.</td></tr><tr><td>PHMFL</td><td>Magnitude and phase angle of the mass flow rate in fluid link elements.</td></tr><tr><td>PHMFT</td><td>Magnitude and phase angle of the total mass flow in fluid link elements.</td></tr></table>
|
||
|
||
For connector elements, the following element output variables are available:
|
||
|
||
<table><tr><td>PHCTF</td><td>Magnitude and phase angle of connector total forces.</td></tr><tr><td>PHCEF</td><td>Magnitude and phase angle of connector elastic forces.</td></tr><tr><td>PHCVF</td><td>Magnitude and phase angle of connector viscous forces.</td></tr><tr><td>PHCRF</td><td>Magnitude and phase angle of connector reaction forces.</td></tr><tr><td>PHCSF</td><td>Magnitude and phase angle of connector friction forces.</td></tr><tr><td>PHCU</td><td>Magnitude and phase angle of connector relative displacements.</td></tr><tr><td>PHCCU</td><td>Magnitude and phase angle of connector constitutive displacements.</td></tr><tr><td>PHCV</td><td>Magnitude and phase angle of connector relative velocities.</td></tr><tr><td>PHCA</td><td>Magnitude and phase angle of connector relative accelerations.</td></tr></table>
|
||
|
||
Nodal variables:
|
||
|
||
<table><tr><td>PU</td><td>Magnitude and phase angle of all displacement/rotation components at a node.</td></tr><tr><td>PPOR</td><td>Magnitude and phase angle of the fluid, pore, or acoustic pressure at a node.</td></tr><tr><td>PHPOT</td><td>Magnitude and phase angle of the electrical potential at a node.</td></tr><tr><td>PRF</td><td>Magnitude and phase angle of all reaction forces/moments at a node.</td></tr><tr><td>PHCHG</td><td>Magnitude and phase angle of the reactive charge at a node.</td></tr></table>
|
||
|
||
<!-- source-page: 213 -->
|
||
|
||
The total kinetic energy of an element (ELKE) is not available for output in a direct-solution steadystate dynamic analysis.
|
||
|
||
The elastic strain energy density (SENER) is not available for output in a SIM-based steady-state dynamic analysis.
|
||
|
||
Whole model variables such as ALLIE (total strain energy) are available for direct-solution steadystate dynamic analysis by requesting energy output to the data, results, or output database files (see “Output to the data and results files,” Section 4.1.2, and “Output to the output database,” Section 4.1.3).
|
||
|
||
Input file template
|
||
```txt
|
||
*HEADING
|
||
...
|
||
*AMPLITUDE, NAME=loadamp
|
||
Data lines to define an amplitude curve as a function of frequency (cycles/time)
|
||
**
|
||
*STEP, NLGEOM
|
||
Include the NLGEOM parameter so that stress stiffening effects will
|
||
be included in the steady-state dynamic step
|
||
*STATIC
|
||
**Any general analysis procedure can be used to preload the structure
|
||
...
|
||
*CLOAD and/or *DLOAD
|
||
Data lines to prescribe preloads
|
||
*TEMPERATURE and/or *FIELD
|
||
Data lines to define values of predefined fields for preloading the structure
|
||
*BOUNDARY
|
||
Data lines to specify boundary conditions to preload the structure
|
||
...
|
||
*END STEP
|
||
**
|
||
*STEP
|
||
*STEADY STATE DYNAMICS, DIRECT
|
||
Data lines to specify frequency ranges and bias parameters
|
||
*BOUNDARY, REAL
|
||
Data lines to specify real (in-phase) boundary conditions
|
||
*BOUNDARY, IMAGINARY
|
||
Data lines to specify imaginary (out-of-phase) boundary conditions
|
||
*CLOAD, AMPLITUDE=loadamp
|
||
Data lines to specify sinusoidally varying, frequency-dependent, concentrated loads
|
||
*CLOAD and/or *DLOAD
|
||
Data lines to specify sinusoidally varying loads
|
||
...
|
||
*END STEP
|
||
```
|
||
|
||
<!-- source-page: 214 -->
|
||
|
||
<!-- source-page: 215 -->
|
||
|
||
# 6.3.5 NATURAL FREQUENCY EXTRACTION
|
||
|
||
Products: Abaqus/Standard Abaqus/CAE Abaqus/AMS
|
||
|
||
# References
|
||
|
||
• “Defining an analysis,” Section 6.1.2
|
||
• “General and linear perturbation procedures,” Section 6.1.3
|
||
• “Dynamic analysis procedures: overview,” Section 6.3.1
|
||
• \*FREQUENCY
|
||
• “Configuring a frequency procedure” in “Configuring linear perturbation analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
|
||
# Overview
|
||
|
||
The frequency extraction procedure:
|
||
|
||
• performs eigenvalue extraction to calculate the natural frequencies and the corresponding mode shapes of a system;
|
||
• will include initial stress and load stiffness effects due to preloads and initial conditions if geometric nonlinearity is accounted for in the base state, so that small vibrations of a preloaded structure can be modeled;
|
||
• will compute residual modes if requested;
|
||
• is a linear perturbation procedure;
|
||
• can be performed using the traditional Abaqus software architecture if appropriate, but the highperformance SIM architecture (see “Using the SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1) is used as the default; and
|
||
• solves the eigenfrequency problem only for symmetric mass and stiffness matrices; the complex eigenfrequency solver must be used if unsymmetric contributions, such as the load stiffness, are needed.
|
||
|
||
# Eigenvalue extraction
|
||
|
||
The eigenvalue problem for the natural frequencies of an undamped finite element model is
|
||
|
||
$$
|
||
(- \omega^ {2} M ^ {M N} + K ^ {M N}) \phi^ {N} = 0,
|
||
$$
|
||
|
||
where
|
||
|
||
MMN is the mass matrix (which is symmetric and positive definite);
|
||
|
||
<!-- source-page: 216 -->
|
||
|
||
KMN $K ^ { M N }$ is the stiffness matrix (which includes initial stiffness effects if the base state included the effects of nonlinear geometry);
|
||
|
||
N $\phi ^ { N }$ is the eigenvector (the mode of vibration); and
|
||
|
||
M and N are degrees of freedom.
|
||
|
||
When $K ^ { M N }$ is positive definite, all eigenvalues are positive. Rigid body modes and instabilities cause $K ^ { M N }$ to be indefinite. Rigid body modes produce zero eigenvalues. Instabilities produce negative eigenvalues and occur when you include initial stress effects. Abaqus/Standard solves the eigenfrequency problem only for symmetric matrices.
|
||
|
||
# Selecting the eigenvalue extraction method
|
||
|
||
Abaqus/Standard provides three eigenvalue extraction methods:
|
||
|
||
• Lanczos
|
||
• Automatic multi-level substructuring (AMS), an add-on analysis capability for Abaqus/Standard
|
||
• Subspace iteration
|
||
|
||
In addition, you must consider the software architecture that will be used for the subsequent modal superposition procedures. The choice of architecture has minimal impact on the frequency extraction procedure, but the default SIM architecture offers significant performance improvements over the traditional architecture for subsequent mode-based steady-state or transient dynamic procedures (see “Using the SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1). The architecture that you use for the frequency extraction procedure is used for all subsequent mode-based linear dynamic procedures; you cannot switch architectures during an analysis. The software architectures used by the different eigensolvers are outlined in Table 6.3.5–1.
|
||
|
||
Table 6.3.5–1 Software architectures available with different eigensolvers.
|
||
|
||
<table><tr><td rowspan="2">Software Architecture</td><td colspan="3">Eigensolver</td></tr><tr><td>Lanczos</td><td>AMS</td><td>Subspace Iteration</td></tr><tr><td>Traditional</td><td>√</td><td></td><td>√</td></tr><tr><td>SIM</td><td>√</td><td>√</td><td>√</td></tr></table>
|
||
|
||
The Lanczos solver with the SIM architecture is the default eigenvalue extraction method because it has the most general capabilities. However, the Lanczos method is generally slower than the AMS method. The increased speed of the AMS eigensolver is particularly evident when you require a large number of eigenmodes for a system with many degrees of freedom. However, the AMS method has the following limitations:
|
||
|
||
• All restrictions imposed on SIM-based linear dynamic procedures also apply to mode-based linear dynamic analyses based on mode shapes computed by the AMS eigensolver. See “Using the
|
||
|
||
<!-- source-page: 217 -->
|
||
|
||
SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1, for details.
|
||
|
||
• The AMS eigensolver does not compute composite modal damping factors.
|
||
• You cannot use the AMS eigensolver in an analysis that contains piezoelectric elements.
|
||
• You cannot request output to the results (.fil) file in an AMS frequency extraction step.
|
||
|
||
• The SIM-based architecture does not support the following capabilities: cyclic symmetry, fluid properties associated with an incident wave, transient dynamic procedures used for coupled structural-acoustic problems, symmetric model generation, and imperfections based on eigenmode data. It is recommended that you run random response analyses using the non-SIM architecture.
|
||
|
||
• At least one output request is required to run analyses using the SIM-based architecture.
|
||
|
||
If your model has many degrees of freedom and these limitations are acceptable, you should use the AMS eigensolver. Otherwise, you should use the Lanczos eigensolver. The Lanczos eigensolver and the subspace iteration method are described in “Eigenvalue extraction,” Section 2.5.1 of the Abaqus Theory Guide.
|
||
|
||
# Lanczos eigensolver
|
||
|
||
For the Lanczos method you need to provide the maximum frequency of interest or the number of eigenvalues required; Abaqus/Standard will determine a suitable block size (although you can override this choice, if needed). If you specify both the maximum frequency of interest and the number of eigenvalues required and the actual number of eigenvalues is underestimated, Abaqus/Standard will issue a corresponding warning message; the remaining eigenmodes can be found by restarting the frequency extraction.
|
||
|
||
You can also specify the minimum frequencies of interest; Abaqus/Standard will extract eigenvalues until either the requested number of eigenvalues has been extracted in the given range or all the frequencies in the given range have been extracted.
|
||
|
||
See “Using the SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1, for information on using the SIM architecture with the Lanczos eigensolver.
|
||
|
||
Input File Usage: \*FREQUENCY, EIGENSOLVER=LANCZOS
|
||
|
||
Abaqus/CAE Usage: Step module: Step→Create: Frequency: Basic: Eigensolver: Lanczos
|
||
|
||
Choosing a block size for the Lanczos method
|
||
|
||
In general, the block size for the Lanczos method should be as large as the largest expected multiplicity of eigenvalues (that is, the largest number of modes with the same frequency). A block size larger than 10 is not recommended. If the number of eigenvalues requested is n, the default block size is the minimum of (7, n). The choice of 7 for block size proves to be efficient for problems with rigid body modes. The number of block Lanczos steps within each Lanczos run is usually determined by Abaqus/Standard but can be changed by you. In general, if a particular type of eigenproblem converges slowly, providing more block Lanczos steps will reduce the analysis cost. On the other hand, if you know that a particular type of problem converges quickly, providing fewer block Lanczos steps will reduce the amount of in-core memory used. The default values are
|
||
|
||
<!-- source-page: 218 -->
|
||
|
||
<table><tr><td>Block size</td><td>Maximum number of block Lanczos steps</td></tr><tr><td>1</td><td>80</td></tr><tr><td>2</td><td>50</td></tr><tr><td>3</td><td>45</td></tr><tr><td>≥ 4</td><td>35</td></tr></table>
|
||
|
||
# Automatic multi-level substructuring (AMS) eigensolver
|
||
|
||
For the AMS method you need only specify the maximum frequency of interest (the global frequency), and Abaqus/Standard will extract all the modes up to this frequency. You can also specify the minimum frequencies of interest and/or the number of requested modes. However, specifying these values will not affect the number of modes extracted by the eigensolver; it will affect only the number of modes that are stored for output or for a subsequent modal analysis.
|
||
|
||
The execution of the AMS eigensolver can be controlled by specifying three parameters: $A M S _ { \mathrm { c u t o f f _ { 1 } } } , ~ A M S _ { \mathrm { c u t o f f _ { 2 } } }$ , and $A M S _ { \mathrm { c u t o f f _ { 3 } } }$ . These three parameters multiplied by the maximum frequency of interest define three cutoff frequencies. $A M S _ { \mathrm { c u t o f f _ { 1 } } }$ (default value of 5) controls the cutoff frequency for substructure eigenproblems in the reduction phase, while $A M S _ { \mathrm { c u t o f f _ { 2 } } }$ and $A M S _ { \mathrm { c u t o f f _ { 3 } } }$ (default values of 1.7 and 1.1, respectively) control the cutoff frequencies used to define a starting subspace in the reduced eigensolution phase. Generally, increasing the value of $A M S _ { \mathrm { c u t o f f _ { 2 } } }$ and $A M S _ { \mathrm { c u t o f f _ { 3 } } }$ improves the accuracy of the results but may affect the performance of the analysis.
|
||
|
||
# Requesting eigenvectors at all nodes
|
||
|
||
By default, the AMS eigensolver computes eigenvectors at every node of the model.
|
||
|
||
Input File Usage: \*FREQUENCY, EIGENSOLVER=AMS
|
||
|
||
Abaqus/CAE Usage: Step module: Step→Create: Frequency: Basic: Eigensolver: AMS
|
||
|
||
# Requesting eigenvectors only at specified nodes
|
||
|
||
Alternatively, you can specify a node set, and eigenvectors will be computed and stored only at the nodes that belong to that node set. The node set that you specify must include all nodes at which loads are applied or output is requested in any subsequent modal analysis (this includes any restarted analysis). If element output is requested or element-based loading is applied, the nodes attached to the associated elements must also be included in this node set. Computing eigenvectors at only selected nodes improves performance and reduces the amount of stored data. Therefore, it is recommended that you use this option for large problems. Abaqus/Standard can automatically select all the nodes that need to be included in the node set. These nodes are
|
||
|
||
• nodes at which a concentrated load is applied in the following mode-based procedures,
|
||
• nodes at which output is requested in the eigenvalue extraction analysis or in the following modebased procedures,
|
||
|
||
<!-- source-page: 219 -->
|
||
|
||
• nodes at which residual vectors are requested,
|
||
• nodes of elements at which a distributed load is applied,
|
||
• nodes of elements with frequency-dependent material properties, and
|
||
|
||
• nodes of elements at which output is requested in the eigenvalue extraction analysis or in the following mode-based procedures.
|
||
|
||
Input File Usage: Use the following option to specify a node set:
|
||
|
||
\*FREQUENCY, EIGENSOLVER=AMS, NSET=name
|
||
|
||
Use the following option to allow Abaqus/Standard to select the nodes automatically:
|
||
|
||
\*FREQUENCY, EIGENSOLVER=AMS, NSET
|
||
|
||
Abaqus/CAE Usage: You can only request eigenvectors at specific nodes by specifying a node set in Abaqus/CAE.
|
||
|
||
Step module: Step→Create: Frequency: Basic: Eigensolver: AMS:
|
||
|
||
Limit region of saved eigenvectors, select node set
|
||
|
||
# Controlling the AMS eigensolver
|
||
|
||
The AMS method consists of the following three phases:
|
||
|
||
• Reduction phase: In this phase Abaqus/Standard uses a multi-level substructuring technique to reduce the full system in a way that allows a very efficient eigensolution of the reduced system. The approach combines a sparse factorization based on a multi-level supernode elimination tree and a local eigensolution at each supernode.
|
||
|
||
Starting from the lowest level supernodes, we use a Craig-Bampton substructure reduction technique to successively reduce the size of the system as we progress upward in the elimination tree. At each supernode a local eigensolution is obtained based on fixing the degrees of freedom connected to the next higher level supernode (these are the local retained or “fixed-interface” degrees of freedom). At the end of the reduction phase the full system has been reduced such that the reduced stiffness matrix is diagonal and the reduced mass matrix has unit diagonal values but contains off-diagonal blocks of nonzero values representing the coupling between the supernodes.
|
||
|
||
The cost of the reduction phase depends on the system size and the number of eigenvalues extracted (the number of eigenvalues extracted is controlled indirectly by specifying the highest eigenfrequency desired). You can make trade-offs between cost and accuracy during the reduction phase through the $A M S _ { \mathrm { c u t o f f _ { 1 } } }$ parameter. This parameter multiplied by the highest eigenfrequency specified for the full model yields the highest eigenfrequency that is extracted in the local supernode eigensolutions. Increasing the value of $A M S _ { \mathrm { c u t o f f _ { 1 } } }$ increases the accuracy of the reduction since more local eigenmodes are retained. However, increasing the number of retained modes also increases the cost of the reduced eigensolution phase, which is discussed next.
|
||
|
||
• Reduced eigensolution phase: In this phase Abaqus/Standard computes the eigensolution of the reduced system that comes from the previous phase. Although the reduced system typically is two orders of magnitude smaller in size than the original system, generally it still is too large to solve directly. Thus, the system is further reduced mainly by truncating the retained eigenmodes
|
||
|
||
<!-- source-page: 220 -->
|
||
|
||
and then solved using a single subspace iteration step. The two AMS parameters, $A M S _ { \mathrm { c u t o f f _ { 2 } } }$ and $A M S _ { \mathrm { c u t o f f _ { 3 } } }$ , define a starting subspace of the subspace iteration step. The default values of these parameters are carefully chosen and provide accurate results in most cases. When a more accurate solution is needed, the recommended procedure is to increase both parameters proportionally from their respective default values.
|
||
|
||
• Recovery phase: In this phase the eigenvectors of the original system are recovered using eigenvectors of the reduced problem and local substructure modes. If you request recovery at specified nodes, the eigenvectors are computed only at those nodes.
|
||
|
||
# Subspace iteration method
|
||
|
||
For the subspace iteration procedure you need only specify the number of eigenvalues required; Abaqus/Standard chooses a suitable number of vectors for the iteration. If the subspace iteration technique is requested, you can also specify the maximum frequency of interest; Abaqus/Standard extracts eigenvalues until either the requested number of eigenvalues has been extracted or the last frequency extracted exceeds the maximum frequency of interest.
|
||
|
||
Input File Usage: \*FREQUENCY, EIGENSOLVER=SUBSPACE
|
||
|
||
Abaqus/CAE Usage: Step module: Step→Create: Frequency: Basic: Eigensolver: Subspace
|
||
|
||
# Structural-acoustic coupling
|
||
|
||
Structural-acoustic coupling affects the natural frequency response of systems. In Abaqus the AMS eigensolver and the Lanczos eigensolver can extract coupled modes to fully include this effect. The subspace eigensolver neglects the effect of coupling for the purpose of computing the modes and frequencies; the modes and frequencies are computed using natural boundary conditions at the structural-acoustic coupling surface. By default, the same is done for the AMS eigensolver; the coupling is projected onto the modal space and stored for later use.
|
||
|
||
# Structural-acoustic coupling using the Lanczos eigensolver
|
||
|
||
If structural-acoustic coupling is present in the model and the Lanczos method is used, Abaqus/Standard extracts the coupled modes by default. Because these modes fully account for coupling, they represent the mathematically optimal basis for subsequent modal procedures. The effect is most noticeable in strongly coupled systems such as steel shells and water. However, coupled structural-acoustic modes cannot be used in subsequent random response or response spectrum analyses. You can define the coupling using either acoustic-structural interaction elements (see “Acoustic interface elements,” Section 32.13.1) or the surface-based tie constraint (see “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1). It is possible to ignore coupling when extracting acoustic and structural modes; in this case the coupling boundary is treated as traction-free on the structural side and rigid on the acoustic side.
|
||
|
||
For frequency extractions that use the Lanczos eigensolver based on the SIM architecture, it is also possible to project structural-acoustic coupling operators onto the subspace of eigenvectors. The modes are computed using traction-free boundary conditions on the structural side of the coupling boundary and rigid boundary conditions on the acoustic side. Structural-acoustic coupling operators
|