김경종
225 lines
16 KiB
Markdown
225 lines
16 KiB
Markdown
<!-- source-page: 1351 -->
|
||
|
||
# 16.1 Sequentially coupled multiphysics analyses
|
||
|
||
• “Predefined fields for sequential coupling,” Section 16.1.1
|
||
• “Sequentially coupled thermal-stress analysis,” Section 16.1.2
|
||
• “Predefined loads for sequential coupling,” Section 16.1.3
|
||
|
||
<!-- source-page: 1352 -->
|
||
|
||
<!-- source-page: 1353 -->
|
||
|
||
# 16.1.1 PREDEFINED FIELDS FOR SEQUENTIAL COUPLING
|
||
|
||
Products: Abaqus/Standard Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Defining an analysis,” Section 6.1.2
|
||
• “Sequentially coupled thermal-stress analysis,” Section 16.1.2
|
||
• “Predefined fields,” Section 34.6.1
|
||
• “Creating and modifying output requests,” Section 14.4.5 of the Abaqus/CAE User’s Guide
|
||
• “Defining a temperature field,” Section 16.11.9 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
|
||
# Overview
|
||
|
||
The time history of the following nodal output quantities, generated in an Abaqus/Standard analysis, can be read into subsequent Abaqus/Standard analyses as predefined fields for sequentially coupled multiphysics workflows:
|
||
|
||
• Temperature
|
||
• Normalized concentration
|
||
• Electric potential
|
||
|
||
A sequentially coupled multiphysics analysis can be used when the coupling between one or more of the physical fields in a model is only important in one direction—a special common case is a sequential thermal-stress analysis (“Sequentially coupled thermal-stress analysis,” Section 16.1.2). While the uncoupled thermal-stress analysis is the most common sequential multiphysics workflow, the predefined field capability in Abaqus/Standard directly supports similar sequential workflows involving normalized concentrations (“Mass diffusion analysis,” Section 6.9.1) and electric potentials (“Coupled thermal-electrical analysis,” Section 6.7.3). As with temperatures, normalized concentrations and electric potentials can be read from the output database (.odb) file into subsequent analyses as predefined fields.
|
||
|
||
When defined by results from a previous analysis, predefined fields typically vary with position and are time dependent—they are predefined because they are not changed by the current analysis. When predefined fields are read from a previous analysis, they are read in at the nodes. They are then interpolated within elements as needed (see “Interpolating data between meshes” in “Predefined fields,” Section 34.6.1). Any number of predefined fields can be read in, and material properties can be defined to depend on them. In addition, volumetric strain will arise in a stress analysis if thermal expansion (“Thermal expansion,” Section 26.1.2) or field expansion (“Field expansion,” Section 26.1.3) are included in the material property definition.
|
||
|
||
<!-- source-page: 1354 -->
|
||
|
||
Predefined fields may affect the system response through:
|
||
|
||
• the constitutive behavior, such as the yield stress defined as a function of temperature or field variables; or
|
||
• volumetric strains when thermal or field expansion behaviors (“Thermal expansion,” Section 26.1.2, and “Field expansion,” Section 26.1.3) are included in the material definition in a stress/displacement analysis.
|
||
|
||
# Saving temperatures, normalized concentrations, and electric potentials for predefined fields in subsequent analyses
|
||
|
||
Nodal temperatures, normalized concentrations, and electrical potentials can be stored as functions of time for use in subsequent analyses. Temperatures can be stored in either the results (.fil) file or the output database (.odb) file, but normalized concentrations and electrical potentials can be used only if they are stored in the output database file. Saved values must be read into the new analyses as predefined fields. See “Node output” in “Output to the data and results files,” Section 4.1.2, and “Node output” in “Output to the output database,” Section 4.1.3.
|
||
|
||
# Saving temperatures for predefined fields in subsequent analyses
|
||
|
||
To be read as a predefined field, nodal temperatures must be stored as functions of time in the results (.fil) file or output database (.odb) file. You can request nodal temperature output (NT) in an uncoupled heat transfer analysis or in a coupled thermal-electrical analysis.
|
||
|
||
# Saving normalized concentrations for predefined fields in subsequent analyses
|
||
|
||
To be read as predefined fields, normalized concentrations must be stored as functions of time in the output database (.odb) file—unlike nodal temperatures they cannot be read directly from a results file. You can request nodal normalized concentrations output (NNC) in a mass diffusion analysis.
|
||
|
||
# Saving electric potentials for predefined fields in subsequent analyses
|
||
|
||
To be read as predefined fields, electrical potentials must be stored as functions of time in the output database (.odb) file—unlike nodal temperatures they cannot be read directly from a results file. You can request nodal electric potential output (EPOT) in a coupled thermal-electrical analysis or a piezoelectric analysis.
|
||
|
||
# Transferring temperatures as temperature fields
|
||
|
||
To define the temperature field at different times in the current analysis, you read the nodal temperatures stored as a function of time in the heat transfer results or output database file. Nodes can be removed for the current problem; for example, in a sequential thermal-stress analysis elements that represent nonstructural parts of the heat transfer mesh (such as insulation or cooling fluid) can be omitted in the stress analysis. When the heat transfer results file or output database file is read, temperatures at nodes that are not present in the mesh for the current analysis are ignored.
|
||
|
||
<!-- source-page: 1355 -->
|
||
|
||
You must specify the name of the thermal analysis results file or output database file that contains the required nodal temperatures. The file extension is optional. If the heat transfer model and the current analysis model share the same mesh, the default is the results file. If the heat transfer model and the current analysis model have dissimilar meshes, the output database file must be used. See “Reading the values of a field from a user-specified file” in “Predefined fields,” Section 34.6.1, for more information.
|
||
|
||
If both models contain part and assembly definitions, the part (.prt) files from both analyses are required to transfer temperatures from the thermal analysis to the current analysis. If the thermal model is defined in terms of an assembly of part instances, the current analysis must be as well. The part instance names and local node numbers must be the same in both analyses for the nodes at which temperatures are transferred.
|
||
|
||
# Transferring temperatures, normalized concentrations, and electric potentials from the output database to predefined fields
|
||
|
||
To define predefined fields at different times in the current analysis, you can read nodal temperatures, normalized concentrations, or electric potentials stored as a function of time in the output database file. Nodes can be removed for the current problem. When the nodal output variables on the output database file are on nodes that are not present in the mesh for the current analysis, they are ignored.
|
||
|
||
You must specify the name of the output database file that contains the required nodal output variables as well as the nodal output label (NT, NNC, or EPOT) to identify the field that is being read. See “Defining fields using nodal scalar output values from a user-specified output database file” in “Predefined fields,” Section 34.6.1.
|
||
|
||
If both models contain part and assembly definitions, the part (.prt) files from both analyses are required to transfer nodal results from the original analysis to the current analysis. If the original model is defined in terms of an assembly of part instances, the current analysis must be as well. The part instance names and local node numbers must be the same in both analyses for the nodes at which nodal results are transferred.
|
||
|
||
# Initial conditions
|
||
|
||
Appropriate initial conditions for Abaqus/Standard procedures are discussed in Chapter 6, “Analysis Procedures.” You can read the nodal temperatures, normalized concentrations, or electric potentials from previous analyses to initialize predefined fields. See “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1, for details.
|
||
|
||
# Boundary conditions
|
||
|
||
Appropriate boundary conditions for Abaqus/Standard procedures are discussed in Chapter 6, “Analysis Procedures.” See also “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1.
|
||
|
||
# Loads
|
||
|
||
Appropriate loadings for Abaqus/Standard procedures are discussed in Chapter 6, “Analysis Procedures.” See also “Applying loads: overview,” Section 34.4.1.
|
||
|
||
<!-- source-page: 1356 -->
|
||
|
||
# Predefined fields
|
||
|
||
See “Predefined fields,” Section 34.6.1, for additional details on predefined temperatures and fields.
|
||
|
||
# Material options
|
||
|
||
See Part V, “Materials,” for details on the material models available in Abaqus/Standard.
|
||
|
||
Volumetric strain will arise in a stress analysis if thermal expansion (“Thermal expansion,” Section 26.1.2) or field expansion (“Field expansion,” Section 26.1.3) is included in the material property definition.
|
||
|
||
# Elements
|
||
|
||
Continuum and structural elements available in Abaqus/Standard are discussed in Chapter 28, “Continuum Elements,” and Chapter 29, “Structural Elements.” Details on how results from a previous analysis can be transferred to a current analysis are discussed in “Predefined fields,” Section 34.6.1.
|
||
|
||
# Output
|
||
|
||
Appropriate output variables for Abaqus/Standard are described in Part V, “Materials.” All of the output variables are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1.
|
||
|
||
# Input file template
|
||
|
||
A moisture-stress analysis is an example of a sequentially coupled multiphysics analysis. A typical sequentially coupled moisture-stress analysis consists of two Abaqus/Standard runs: a mass diffusion analysis and a subsequent stress analysis. Normalized concentrations are stored in the output database file for the mass diffusion analysis and read into the subsequent stress analysis as a predefined field.
|
||
|
||
The following template shows the input for the mass diffusion analysis massdiffusion.inp:
|
||
|
||
```txt
|
||
*HEADING
|
||
...
|
||
*ELEMENT, TYPE=DC2D4
|
||
(Choose the mass diffusion element type)
|
||
...
|
||
*STEP
|
||
*MASS DIFFUSION
|
||
...
|
||
Apply loads and boundary conditions
|
||
...
|
||
** Write all normalized concentrations to the output
|
||
** database file, massdiffusion.odb
|
||
*OUTPUT, FIELD
|
||
*NODE OUTPUT, NSET=NALL
|
||
```
|
||
|
||
<!-- source-page: 1357 -->
|
||
|
||
NNC
|
||
|
||
\*END STEP
|
||
|
||
The following template shows the input for the subsequent static structural analysis:
|
||
|
||
\*HEADING
|
||
|
||
\*ELEMENT, TYPE=CPE4R
|
||
|
||
(Choose the continuum element type compatible with the mass diffusion element type used)
|
||
|
||
\*MATERIAL
|
||
|
||
\*EXPANSION, FIELD=1
|
||
|
||
(Define field expansion for field 1 so that the normalized concentration causes volumetric strain in the stress analysis)
|
||
|
||
\*STEP
|
||
|
||
\*STATIC
|
||
|
||
Apply structural loads and boundary conditions
|
||
|
||
\*FIELD, FILE=massdiffusion.odb, OUTPUT VARIABLE=NNC, FIELD=1
|
||
|
||
Read in all normalized concentrations from the output database file into field variable 1
|
||
|
||
\*END STEP
|
||
|
||
<!-- source-page: 1358 -->
|
||
|
||
<!-- source-page: 1359 -->
|
||
|
||
# 16.1.2 SEQUENTIALLY COUPLED THERMAL-STRESS ANALYSIS
|
||
|
||
Products: Abaqus/Standard Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Defining an analysis,” Section 6.1.2
|
||
• “Heat transfer analysis procedures: overview,” Section 6.5.1
|
||
• “Predefined fields for sequential coupling,” Section 16.1.1
|
||
• “Creating and modifying output requests,” Section 14.4.5 of the Abaqus/CAE User’s Guide
|
||
• “Defining a temperature field,” Section 16.11.9 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
|
||
# Overview
|
||
|
||
A sequentially coupled heat transfer analysis:
|
||
|
||
• is used when the stress/deformation field in a structure depends on the temperature field in that structure, but the temperature field can be found without knowledge of the stress/deformation response; and
|
||
• is usually performed by first conducting an uncoupled heat transfer analysis and then a stress/deformation analysis.
|
||
|
||
A thermal-stress analysis in which the temperature field does not depend on the stress field is a common example of a sequential multiphysics workflow and is one case of the more general workflow described in “Predefined fields for sequential coupling,” Section 16.1.1. In such thermal-stress analyses, temperature is calculated in an uncoupled heat transfer analysis (“Uncoupled heat transfer analysis,” Section 6.5.2) or in a coupled thermal-electrical analysis (“Coupled thermal-electrical analysis,” Section 6.7.3).
|
||
|
||
# Saving the nodal temperatures
|
||
|
||
Nodal temperatures are stored as a function of time in the heat transfer results (.fil) file or output database (.odb) file by requesting output variable NT as nodal output to the results or output database file. See “Node output” in “Output to the data and results files,” Section 4.1.2, and “Node output” in “Output to the output database,” Section 4.1.3.
|
||
|
||
# Transferring the heat transfer results to the stress analysis
|
||
|
||
The temperatures are read into the stress analysis as a predefined field; the temperature varies with position and is usually time dependent. It is predefined because it is not changed by the stress analysis solution. Such predefined fields are always read into Abaqus/Standard at the nodes. They are then interpolated to the calculation points within elements as needed (see “Interpolating data between meshes” in “Predefined fields,” Section 34.6.1). The temperature interpolation in the stress elements is usually
|
||
|
||
<!-- source-page: 1360 -->
|
||
|
||
approximate and one order lower than the displacement interpolation to obtain a compatible variation of thermal and mechanical strain. Any number of predefined fields can be read in, and material properties can be defined to depend on them.
|
||
|
||
For more information, see “Transferring temperatures as temperature fields” in “Predefined fields for sequential coupling,” Section 16.1.1.
|
||
|
||
# Initial conditions
|
||
|
||
Appropriate initial conditions for the thermal and stress analysis problems are described in the heat transfer and stress analysis sections—for example, see “Heat transfer analysis procedures: overview,” Section 6.5.1; “Coupled thermal-electrical analysis,” Section 6.7.3; “Static stress analysis procedures: overview,” Section 6.2.1; and “Dynamic analysis procedures: overview,” Section 6.3.1. See also “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1.
|
||
|
||
# Boundary conditions
|
||
|
||
Appropriate boundary conditions for the thermal and stress analysis problems are described in the heat transfer and stress analysis sections—for example, see “Heat transfer analysis procedures: overview,” Section 6.5.1; “Coupled thermal-electrical analysis,” Section 6.7.3; “Static stress analysis procedures: overview,” Section 6.2.1; and “Dynamic analysis procedures: overview,” Section 6.3.1. See also “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1.
|
||
|
||
# Loads
|
||
|
||
Appropriate loading for the thermal and stress analysis problems is described in the heat transfer and stress analysis sections—for example, see “Heat transfer analysis procedures: overview,” Section 6.5.1; “Coupled thermal-electrical analysis,” Section 6.7.3; “Static stress analysis procedures: overview,” Section 6.2.1; and “Dynamic analysis procedures: overview,” Section 6.3.1. See also “Applying loads: overview,” Section 34.4.1.
|
||
|
||
# Predefined fields
|
||
|
||
In addition to the temperatures read in from the heat transfer analysis, user-defined field variables can be specified; these values only affect field-variable-dependent material properties, if any. See “Predefined fields,” Section 34.6.1.
|
||
|
||
# Material options
|
||
|
||
The materials in the thermal analysis must have thermal properties such as conductivity defined (see “Thermal properties: overview,” Section 26.2.1). Any mechanical properties such as elasticity will be ignored in the thermal analysis, but they must be defined for the stress analysis procedure. See Part V, “Materials,” for details on the material models available in Abaqus/Standard.
|
||
|
||
Thermal strain will arise in the stress analysis if thermal expansion (“Thermal expansion,” Section 26.1.2) is included in the material property definition.
|