16.1.1 Predefined fields for sequential coupling
Products: Abaqus/Standard Abaqus/CAE
References
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
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.
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.
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.
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:
*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