김경종
283 lines
24 KiB
Markdown
283 lines
24 KiB
Markdown
<!-- source-page: 151 -->
|
||
|
||
# Abaqus/CAE Usage: Step module: Step→Create: Frequency: Use SIM-based linear dynamics procedures
|
||
|
||
# Example
|
||
|
||
The SIM architecture will be used for the entire linear dynamic analysis in the following input file template:
|
||
|
||
```txt
|
||
*STEP
|
||
*FREQUENCY, EIGENSOLVER=LANCZOS, SIM
|
||
Data line to control eigenvalue extraction
|
||
*COMPOSITE MODAL DAMPING
|
||
Data lines to define fraction of critical damping
|
||
*END STEP
|
||
**
|
||
*STEP
|
||
*MODAL DYNAMIC
|
||
Data line to control time incrementation
|
||
*SELECT EIGENMODES
|
||
Data lines to define the applicable mode ranges
|
||
*MODAL DAMPING, VISCOUS=COMPOSITE
|
||
Data lines to define composite modal damping
|
||
*END STEP
|
||
**
|
||
*STEP
|
||
*STEADY STATE DYNAMICS
|
||
Data lines to specify frequency ranges and bias parameters
|
||
*SELECT EIGENMODES
|
||
Data lines to define the applicable mode ranges
|
||
*END STEP
|
||
**
|
||
*STEP
|
||
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION
|
||
Data lines to specify frequency ranges and bias parameters
|
||
*SELECT EIGENMODES
|
||
Data lines to define the applicable mode ranges
|
||
*END STEP
|
||
```
|
||
|
||
# Output in a SIM-based analysis
|
||
|
||
Output is a fundamental factor in the performance of a linear dynamic analysis. Since it is difficult to predict the desired output quantities for a linear dynamic analysis, preselected output requests are ignored in SIM-based modal superposition procedures (except complex eigenvalue extraction). You must always specify output requests to the output database (.odb) file; otherwise, the analysis will not be performed.
|
||
|
||
<!-- source-page: 152 -->
|
||
|
||
There are several restrictions on available output requests that apply specifically to SIM-based analyses:
|
||
|
||
• You cannot request output to the results (.fil) file.
|
||
• Element variables cannot be output to the printed data (.dat) file except for random response analysis.
|
||
|
||
# Limitations of the SIM architecture
|
||
|
||
The cyclic symmetry modeling feature cannot be used in SIM-based analyses.
|
||
|
||
# Nonphysical material properties in dynamic analyses
|
||
|
||
Abaqus relies on user-supplied model data and assumes that the material’s physical properties reflect experimental results. Examples of meaningful material properties are a positive mass density per volume, a positive Young’s modulus, and a positive value for any available damping coefficients. However, in special cases you may want to “adjust” a value of density, mass, stiffness, or damping in a region or a part of the model to bring the overall mass, stiffness, or damping to the expected required levels. Certain material options in Abaqus allow you to introduce nonphysical material properties to achieve this adjustment.
|
||
|
||
For example, to adjust the mass of the model, you can define a nonstructural mass with a negative mass value, use mass elements with a negative mass over a region of nodes, or introduce additional elements with negative density. Similarly, to adjust damping levels, you can use negative damping coefficients or introduce dashpot elements with a negative dashpot constant to reduce the overall damping levels. Springs with negative stiffness can be defined to adjust the model stiffness.
|
||
|
||
If you specify nonphysical but allowed material properties, Abaqus issues a warning message. However, if you specify nonphysical material properties that are not allowed, Abaqus issues an error message. When introducing nonphysical material properties, you must be aware that the overall behavior should be “physical”; for example, the mass values at all nodes must be positive in an eigenvalue extraction procedure.
|
||
|
||
There are consequences of using nonphysical material properties that are easy to check and interpret, and there are others beyond the control of Abaqus. Therefore, you should fully understand the stated problem and the consequences of using nonphysical material properties before you specify the properties. This is particularly important in Abaqus/Explicit analyses, where the size of the time increment depends on material properties. For example, distributed mass-dependent loads are calculated based on the overall mass density (positive and negative) provided.
|
||
|
||
# Damping in dynamic analysis
|
||
|
||
Every nonconservative system exhibits some energy loss that is attributed to material nonlinearity, internal material friction, or to external (mostly joint) frictional behavior. Conventional engineering materials like steel and high strength aluminum alloys provide small amounts of internal material damping, not enough to prevent large amplification at or near resonant frequencies. Damping properties increase in modern composite fiber-reinforced materials, where the energy loss occurs through plastic or viscoelastic phenomena as well as from friction at the interfaces between the matrix and reinforcement.
|
||
|
||
<!-- source-page: 153 -->
|
||
|
||
Still larger material damping is exhibited by thermoplastics. Mechanical dampers may be added to models to introduce damping forces to the system. In general, it is difficult to quantify the source of a system’s damping. It usually comes from several sources simultaneously; e.g., from energy loss during hysteretic loading, viscoelastic material properties, and external joint friction.
|
||
|
||
Users that work with a specific system know the source of the energy loss from experience. A variety of methods are available in Abaqus to specify damping that accurately models the energy loss in a dynamic system.
|
||
|
||
# Sources of damping
|
||
|
||
Abaqus has four categories of damping sources: material and element damping, global damping, modal damping, and damping associated with time integration. If necessary, you can include multiple damping sources and combine different damping sources in a model.
|
||
|
||
# Material and element damping
|
||
|
||
Damping may be specified as part of a material definition that is assigned to a model (see “Material damping,” Section 26.1.1). In addition, Abaqus has elements such as dashpots, springs with their complex stiffness matrix, and connectors that serve as dampers, all with viscous and structural damping factors. Viscous damping can be included in mass, beam, pipe, and shell elements with general section properties; and it can also be used in substructure elements (see “Defining substructures,” Section 10.1.2). In direct steady-state dynamic analysis you can define the viscous and structural damping due to the interaction between the contacting surfaces by using user subroutine UINTER (see “UINTER,” Section 1.1.42 of the Abaqus User Subroutines Reference Guide). Contact damping is not applicable for linear perturbation procedures.
|
||
|
||
In acoustic elements, velocity proportional viscous damping is implemented using the volumetric drag parameter (see “Acoustic medium,” Section 26.3.1). Acoustic infinite elements and impedance conditions also add damping to a model.
|
||
|
||
# Global damping
|
||
|
||
In situations where material or element damping is not appropriate or sufficient, you can apply abstract damping factors to an entire model. Abaqus allows you to specify global damping factors for both viscous (Rayleigh damping) and structural damping (imaginary stiffness matrix).
|
||
|
||
# Modal damping
|
||
|
||
Modal damping applies only to mode-based linear dynamic analyses. This technique allows you to apply damping directly to the modes of the system. By definition, modal damping contributes only diagonal entries to the modal system of equations and can be defined several different ways.
|
||
|
||
# Damping associated with time integration
|
||
|
||
Marching through a simulation with a finite time increment size causes some damping. This type of damping applies only to analyses using direct time integration. See “Implicit dynamic analysis using direct integration,” Section 6.3.2, for further discussion of this source of damping.
|
||
|
||
<!-- source-page: 154 -->
|
||
|
||
# Damping in a linear dynamic analysis
|
||
|
||
Damping can be applied to a linear dynamic system in two forms:
|
||
|
||
• velocity proportional viscous damping; and
|
||
• displacement proportional structural damping, which is for use in frequency domain dynamics. The exception is SIM-based transient modal dynamic analysis, where the structural damping is converted to the equivalent diagonal viscous damping (see “Modal dynamic analysis,” Section 2.5.5 of the Abaqus Theory Guide).
|
||
|
||
An additional type of damping known as composite damping serves as a means to calculate a model average critical damping with the material density as the weight factor and is intended for use in modebased dynamics (excluding subspace projection steady-state analysis and SIM-based dynamic analyses). For additional information, see “Damping options for modal dynamics,” Section 2.5.4 of the Abaqus Theory Guide.
|
||
|
||
The types of damping available for linear dynamic analyses depend on the procedure type and the architecture (traditional or SIM) used to perform the analysis, as outlined in Table 6.3.1–1 and Table 6.3.1–2. For completeness, Table 6.3.1–1 also includes the damping options for a direct steady-state dynamic analysis. In addition to directly specified modal damping, global damping can be used in all linear dynamic procedures. Material and element damping can be used in subspace-based and SIM-based linear dynamic procedures.
|
||
|
||
Table 6.3.1–1 Damping sources for traditional architecture.
|
||
|
||
<table><tr><td rowspan="2">Traditional Architecture</td><td colspan="3">Damping Source</td></tr><tr><td>Modal</td><td>Global</td><td>Material and Element</td></tr><tr><td>Mode-based steady-state dynamics</td><td>√</td><td>√</td><td></td></tr><tr><td>Subspace-based steady-state dynamics</td><td></td><td>√</td><td>√</td></tr><tr><td>Transient modal dynamics</td><td>√</td><td>√</td><td></td></tr><tr><td>Random response analysis</td><td>√</td><td>√</td><td></td></tr><tr><td>Complex frequency</td><td></td><td>√</td><td>√</td></tr><tr><td>Response spectrum</td><td>√</td><td>√</td><td></td></tr><tr><td>Direct steady-state dynamics</td><td></td><td>√</td><td>√</td></tr></table>
|
||
|
||
<!-- source-page: 155 -->
|
||
|
||
Table 6.3.1–2 Damping sources for SIM architecture.
|
||
|
||
<table><tr><td rowspan="2">SIM Architecture</td><td colspan="3">Damping Source</td></tr><tr><td>Modal</td><td>Global</td><td>Material and Element</td></tr><tr><td>Mode-based steady-state dynamics</td><td>√</td><td>√</td><td>√</td></tr><tr><td>Subspace-based steady-state dynamics</td><td>√</td><td>√</td><td>√</td></tr><tr><td>Transient modal dynamics</td><td>√</td><td>√</td><td>√</td></tr><tr><td>Random response analysis</td><td>√</td><td>√</td><td></td></tr><tr><td>Complex frequency</td><td>√</td><td>√</td><td>√</td></tr><tr><td>Response spectrum</td><td>√</td><td>√</td><td></td></tr></table>
|
||
|
||
In a subspace-based or SIM-based linear dynamic analysis, material and element damping operators must first be projected onto the basis of mode shapes. This projection results in a full modal damping matrix for both viscous and structural damping; therefore, a modal steady-state response analysis requires the solution of a system of linear equations at each frequency point. The size of this system is equal to the number of modes used in the response calculation. In a mode-based transient analysis, the projected damping operator is treated explicitly in time by including it on the right-hand side of the system of equations.
|
||
|
||
Frequency-dependent damping is supported only for the subspace-based and direct-integration steady-state dynamic procedures.
|
||
|
||
Material and element damping is not supported for the response spectrum or the random response procedures. In these procedures, only modal and global damping are allowed, and material or element damping is ignored.
|
||
|
||
Damping in a mode-based steady-state and transient linear dynamic analysis using the SIM architecture
|
||
|
||
SIM-based linear dynamic analyses may include material and element damping contributions that introduce both diagonal and nondiagonal terms in the modal system of equations. The projection of material and element damping operators onto the basis of mode shapes is performed during the natural frequency extraction procedure, which enables a high-performance projection operation to be performed when used with the AMS eigensolver. If the damping operators depend on frequency, they will be evaluated at the frequency specified for property evaluation during the frequency extraction procedure.
|
||
|
||
When the structural and viscous damping operators are projected onto the mode shapes, the full modal damping matrix is stored in the linear dynamics data (.sim) file. The full modal damping matrix is combined with any diagonal contributions from global damping or traditional modal damping. The combined damping operator matrix is included in subsequent mode-based transient or steady-state dynamics steps. If there are nondiagonal (i.e., projected) damping contributions and a large number of modes are included, performance of the linear dynamics calculations will be impacted since a direct solve must be performed at each frequency point.
|
||
|
||
<!-- source-page: 156 -->
|
||
|
||
Acoustic damping due to impedance conditions is projected onto the subspace of acoustic eigenvectors. These contributions are taken into account in a subspace-based steady-state dynamics analysis that uses the SIM architecture.
|
||
|
||
The default behavior for a SIM-based frequency extraction step is to project any element and material damping onto the mode shapes. You can turn off this damping projection if it is not desired; however, in this case only diagonal damping is available for subsequent modal superposition steps. If the projected damping matrices are not desired in a particular mode-based linear dynamic step for performance reasons, they can be deactivated in that step using the damping control techniques discussed above in “Damping in dynamic analysis.”
|
||
|
||
Input File Usage: Use the following option to project material and element damping operators in a SIM-based analysis:
|
||
|
||
\*FREQUENCY, SIM, DAMPING PROJECTION=ON (default)
|
||
|
||
Use the following option to turn off damping projection in a SIM-based analysis:
|
||
|
||
\*FREQUENCY, SIM, DAMPING PROJECTION=OFF
|
||
|
||
Abaqus/CAE Usage: To control the projection of element and material damping in a SIM-based frequency extraction step that uses the Lanczos eigensolver:
|
||
|
||
Step module: Step→Create: Frequency: Eigensolver: Lanczos, Use SIM-based linear dynamics procedures, toggle Project damping operators
|
||
|
||
To control the projection of element and material damping in a frequency extraction step that uses the AMS eigensolver:
|
||
|
||
Step module: Step→Create: Frequency: Eigensolver: AMS, toggle Project damping operators
|
||
|
||
# Defining viscous damping
|
||
|
||
Abaqus allows you to choose a particular source of viscous damping, to add several sources, or to exclude viscous damping effects.
|
||
|
||
# Defining material/element viscous damping
|
||
|
||
You can choose to model the viscous damping matrix, $D _ { v i s c o u s } ^ { e l } .$ , by using material damping properties and/or damping elements (such as dashpot or mass elements). The viscous, mass, and/or stiffness proportional damping matrix will include the material Rayleigh damping factors, $\alpha _ { R } ^ { m a t }$ and $\beta _ { R } ^ { m a t }$ , as well as the element-oriented damping factor, $\alpha _ { R } ^ { e l }$ (e.g., for mass elements). The material/element-based viscous damping matrix can be written as
|
||
|
||
$$
|
||
\begin{array}{l} D _ {v i s c o u s} ^ {e l} = \sum_ {e l = 1} ^ {N u m e l e m s} \int_ {V} \pmb {\alpha} _ {R} ^ {m a t} N ^ {T} N \rho d v + \sum_ {e l = 1} ^ {N u m e l e m s} \pmb {\alpha} _ {R} ^ {e l} m ^ {e l} \\ + \sum_ {e l = 1} ^ {N u m e l e m s} \int_ {V} \beta_ {R} ^ {m a t} B ^ {T} D B d v + \sum_ {e l = 1} ^ {N u m e l e m s} d _ {v i s c o u s} ^ {e l}, \\ \end{array}
|
||
$$
|
||
|
||
<!-- source-page: 157 -->
|
||
|
||
where $d _ { v i s c o u s } ^ { e l }$ represents the viscous damping matrix for elements such as dashpots. In mode-based procedures projection of $D _ { v i s c o u s } ^ { e l }$ into the eigenmodes results in a non-diagonal matrix.
|
||
|
||
<table><tr><td rowspan="4">Input File Usage:</td><td>Use the following option to specify material viscous damping for elements with mechanical degrees of freedom:</td></tr><tr><td>*DAMPING, ALPHA= $\alpha_{R}^{mat}$ , BETA= $\beta_{R}^{mat}$ </td></tr><tr><td>Use the following option to specify material viscous damping for acoustic elements:</td></tr><tr><td>*ACOUSTIC MEDIUM, VOLUMETRIC DRAG</td></tr></table>
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: Mechanical→Damping:
|
||
|
||
Alpha: $\alpha _ { R } ^ { m a t }$ or Beta : βmat $\beta _ { R } ^ { m a t }$
|
||
|
||
Property module: material editor: Other→Acoustic Medium:
|
||
|
||
Volumetric Drag
|
||
|
||
# Defining global viscous damping
|
||
|
||
You can supply global mass and stiffness proportional viscous damping factors, $\alpha _ { g l o b a l }$ and $\beta _ { g l o b a l }$ , respectively, to create the global damping matrix using the global model mass and stiffness matrices, and , respectively:
|
||
|
||
$$
|
||
D _ {v i s c o u s} ^ {g} = \alpha_ {g l o b a l} M + \beta_ {g l o b a l} K.
|
||
$$
|
||
|
||
These parameters can be specified for the entire model (default), for the mechanical degree of freedom field (displacements and rotations) only, or for the acoustic field only.
|
||
|
||
Input File Usage: Use the following option to specify global viscous damping:
|
||
|
||
\*GLOBAL DAMPING, ALPHA= , BETA=
|
||
|
||
Abaqus/CAE Usage: Global viscous damping is not supported in Abaqus/CAE.
|
||
|
||
# Defining viscous modal damping
|
||
|
||
Rayleigh damping introduces a damping matrix, , defined as
|
||
|
||
$$
|
||
[ C ] = \alpha [ M ] + \beta [ K ],
|
||
$$
|
||
|
||
where is the mass matrix of the model, is the stiffness matrix of the model, and and $\beta$ are factors that you define.
|
||
|
||
In Abaqus/Standard you can define and $\beta$ independently for each mode, so that the above equation becomes
|
||
|
||
$$
|
||
c _ {M} = \alpha_ {M} m _ {M} + \beta_ {M} k _ {M} \quad (\text { no sum on M }),
|
||
$$
|
||
|
||
where the subscript M refers to the mode number and $c _ { M } , m _ { M }$ , and $k _ { M }$ are the damping, mass, and stiffness terms associated with the Mth mode.
|
||
|
||
<!-- source-page: 158 -->
|
||
|
||
<table><tr><td>Input File Usage:</td><td>Use the following option to define Rayleigh damping by specifying mode numbers:*MODAL DAMPING, VISCOUS=RAYLEIGH,DEFINITION=MODE NUMBERSUse the following option to define Rayleigh damping by specifying a frequency range:*MODAL DAMPING, VISCOUS=RAYLEIGH,DEFINITION=FREQUENCY RANGE</td></tr><tr><td>Abaqus/CAE Usage:</td><td>Use the following input to define Rayleigh damping by specifying mode numbers:Step module:Create Step: Linear perturbation:any valid step type:Damping:Specify damping over ranges of: Modes,Rayleigh:Use Rayleigh damping dataUse the following input to define Rayleigh damping by specifying frequency ranges:Step module:Create Step: Linear perturbation:any valid step type:Damping:Specify damping over ranges of: Frequencies,Rayleigh:Use Rayleigh damping data</td></tr></table>
|
||
|
||
Defining viscous modal damping as a fraction of the critical damping
|
||
|
||
You can also specify the damping in each eigenmode in the model or for the specified frequency as a fraction of the critical damping. Critical damping is defined as
|
||
|
||
$$
|
||
c _ {c r} = 2 \sqrt {m k},
|
||
$$
|
||
|
||
where m is the mass of the system and k is the stiffness of the system. Typical values of the fraction of critical damping, $\xi _ { i } ,$ are from 1% to 10% of critical damping, $c _ { c r } { \mathrm { i } }$ ; but Abaqus/Standard accepts any positive value. The critical damping factors can be changed from step to step.
|
||
<table><tr><td rowspan="4">Input File Usage:</td><td>Use the following option to define the fraction of critical damping by specifying mode numbers:</td></tr><tr><td>*MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING, DEFINITION=MODE NUMBERS</td></tr><tr><td>Use the following option to define the fraction of critical damping by specifying a frequency range:</td></tr><tr><td>*MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING, DEFINITION=FREQUENCY RANGE</td></tr></table>
|
||
|
||
<!-- source-page: 159 -->
|
||
|
||
<table><tr><td rowspan="4">Abaqus/CAE Usage:</td><td>Use the following input to define the fraction of critical damping by specifying mode numbers:</td></tr><tr><td>Step module: Create Step: Linear perturbation: any valid step type: Damping: Specify damping over ranges of: Modes, Direct modal: Use direct damping data</td></tr><tr><td>Use the following input to define the fraction of critical damping by specifying frequency ranges:</td></tr><tr><td>Step module: Create Step: Linear perturbation: any valid step type: Damping: Specify damping over ranges of: Frequencies, Direct modal: Use direct damping data</td></tr></table>
|
||
|
||
Viscous modal damping for uncoupled structural-acoustic frequency extractions
|
||
|
||
For uncoupled structural-acoustic frequency extractions performed using the AMS eigensolver, you can apply different damping to the structural and acoustic modes. This technique can be used only when damping is specified for a range of frequencies.
|
||
|
||
<table><tr><td>Input File Usage:</td><td>Use the following option to apply the specified damping to only the structural modes:*MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING, DEFINITION=FREQUENCY RANGE, FIELD=MECHANICALUse the following option to apply the specified damping to only the acoustic modes:*MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING, DEFINITION=FREQUENCY RANGE, FIELD=ACOUSTICUse the following option to apply the specified damping to both structural and acoustic modes (default):*MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING, DEFINITION=FREQUENCY RANGE, FIELD=ALL</td></tr><tr><td>Abaqus/CAE Usage:</td><td>The ability to specify different damping for structural and acoustic modes is not supported in Abaqus/CAE.</td></tr></table>
|
||
|
||
Controlling the sources of viscous damping
|
||
|
||
The material/element and global viscous damping sources can be controlled at the step level; controls are not available for modal damping. If both the material/element and global viscous damping matrices are supplied, both will be used as a combined damping matrix unless you request that only the element or global damping factor be used. The combined material/element and global viscous damping is
|
||
|
||
$$
|
||
D _ {v i s c o u s} = D _ {v i s c o u s} ^ {e l} + D _ {v i s c o u s} ^ {g}.
|
||
$$
|
||
|
||
<!-- source-page: 160 -->
|
||
|
||
<table><tr><td>Input File Usage:</td><td>Use the following option to activate only the material/element viscous damping matrix:*DAMPING CONTROLS, VISCOUS=ELEMENTUse the following option to activate only the global viscous damping matrix:*DAMPING CONTROLS, VISCOUS=FACTORUse the following option to activate the combined material/element and global viscous damping matrix:*DAMPING CONTROLS, VISCOUS=COMBINED</td></tr></table>
|
||
|
||
Abaqus/CAE Usage: Damping controls are not supported in Abaqus/CAE.
|
||
|
||
# Excluding viscous damping effects
|
||
|
||
You can choose to exclude the effects of viscous damping altogether at the step level.
|
||
|
||
Input File Usage: Use the following option to exclude the viscous damping matrix:
|
||
|
||
\*DAMPING CONTROLS, VISCOUS=NONE
|
||
|
||
Abaqus/CAE Usage: Damping controls are not supported in Abaqus/CAE.
|
||
|
||
# Defining structural damping
|
||
|
||
Abaqus allows you to choose a particular source of structural damping, to add several sources, or to exclude structural damping effects.
|
||
|
||
# Defining material/element structural damping
|
||
|
||
The material/element structural damping matrix (that represents the imaginary stiffness and is proportional to forces or displacements) is defined as
|
||
|
||
$$
|
||
K _ {s} ^ {m} = \sum_ {e l = 1} ^ {N u m e l e m s} \int_ {V} \mathbf {s} B ^ {T} D B d v + \sum_ {e l = 1} ^ {N u m e l e m s} \mathbf {s} ^ {e l} k ^ {e l},
|
||
$$
|
||
|
||
where represents the material structural damping, $\mathbf { s } ^ { e l }$ represents the structural damping coefficient for elements such as springs with complex stiffnesses and connectors, and $k ^ { e l }$ is the real element stiffness matrix. In mode-based procedures the projection of $K _ { s } ^ { m }$ onto the mode shapes results in a full modal damping matrix. When using SIM-based modal procedures, the projected material and element damping matrix may be combined with global and modal damping (see “Defining and using both global and modal diagonal damping,” below). Material/element structural damping is not available for acoustic elements.
|
||
|
||
Input File Usage: Use the following option to specify material structural damping:
|
||
|
||
\*DAMPING, STRUCTURAL=
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: Mechanical→Damping: Structural:
|