Predefined Fields for Sequential Coupling

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

Alternatively, the time history of a known pore fluid pressure field can be read into a subsequent Abaqus/Standard static or an Abaqus/Explicit dynamic stress analysis as a predefined field to perform a sequentially coupled pore pressure–stress analysis.

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). 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) and electric potentials (Coupled Thermal-Electrical Analysis). 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). 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) or field expansion (Field Expansion) 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 and Field Expansion) are included in the material definition in a stress/displacement analysis; or

  • a modification to the stress field when a pre-computed pore fluid pressure field is read into an Abaqus stress analysis as a predefined field variable.

This page discusses:

See Also
Analysis Procedures
Defining an Analysis
Sequentially Coupled Thermal-Stress Analysis
In Other Guides
Continuum Elements
Predefined Fields

ProductsAbaqus/Standard Abaqus/Explicit

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 Writing Nodal Output to the Output Database.

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.

Transferring Pore Fluid Pressure to a Predefined Field

In some geotechnical applications a fully coupled pore fluid diffusion and stress analysis can be approximated by a sequentially coupled approach that consists of two parts:

  1. A purely pore fluid flow analysis that computes the pore fluid pressure distribution in the porous medium without accounting for the deformation in the solid skeleton.
  2. A pure stress analysis that only computes the deformation of the solid skeleton, taking into account the effects of the pore fluid pressure field computed in the first part.

In such an approach, you must transfer a known pore fluid pressure field (computed in the first part of the sequential workflow) into a stress analysis (the current analysis, which is the second part of the sequential workflow).

To define the pore fluid pressure field at different times in the current analysis, you must first associate the pore fluid pressure field with a specific field variable (see Pore Fluid Pressure). Subsequently, you can use any of the available methods to read or define predefined fields to include the known pore pressure field in the stress analysis.

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. You can also read the stress, plastic strain, and damage initiation criteria from previous analyses to initialize predefined fields. When data are read from the output database (.sim) file, mapping is performed automatically between dissimilar meshes. See Initial Conditions for details.

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 ElementsContinuum Elements and Structural Elements. Details on how results from a previous analysis can be transferred to a current analysis are discussed in Predefined Fields.

Input File Template

Two examples of sequential workflows are shown.

The first example is a sequentially coupled moisture-stress analysis, which 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. An example problem is shown in Reading scalar nodal output from the output database into field variables.

The following template shows the input for the mass diffusion analysis massdiffusion2d.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, massdiffusion2d.odb
OUTPUT, FIELD
NODE OUTPUT
 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=massdiffusion2d.odb, OUTPUT VARIABLE=NNC, VARIABLE=1
Read in all normalized concentrations from the output database file into field variable 1 
…
END STEP

The second example shows a template for including a known pore fluid pressure field as a predefined field variable in a static or in an explicit dynamic step.

HEADING
…
ELEMENT, TYPE=element_type
(Choose the appropriate type of continuum element to carry out the stress analysis)
…
MATERIAL
PORE FLUID PRESSURE, FIELD=n
Associate pore fluid pressure field with the predefined field variable n
…
STEP
STATIC (or DYNAMIC, EXPLICIT)
…
Apply structural loads and boundary conditions
…
FIELD, VARIABLE=n
Read in known pore fluid pressure field into predefined field variable n 
…
END STEP