Predefined fields for sequential coupling | ||||||||||
|
| |||||||||
ProductsAbaqus/StandardAbaqus/CAE
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 and Node output.
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.
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 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.
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 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 for details.
Boundary conditions
Appropriate boundary conditions for Abaqus/Standard procedures are discussed in Analysis Procedures. See also Boundary conditions in Abaqus/Standard and Abaqus/Explicit.
Loads
Appropriate loadings for Abaqus/Standard procedures are discussed in Analysis Procedures. See also About loads.
Predefined fields
See Predefined Fields for additional details on predefined temperatures and fields.
Material options
See Abaqus Materials Guide for details on the material models available in Abaqus/Standard.
Volumetric strain will arise in a stress analysis if thermal expansion (Thermal expansion) or field expansion (Field expansion) is included in the material property definition.
Elements
Continuum and structural elements available in Abaqus/Standard are discussed in Continuum Elements and Structural Elements. Details on how results from a previous analysis can be transferred to a current analysis are discussed in Predefined Fields.
Output
Appropriate output variables for Abaqus/Standard are described in Abaqus Materials Guide. All of the output variables are outlined in Abaqus/Standard output variable identifiers.
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:
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 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