Sequentially Coupled Thermal-Stress Analysis

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. In such thermal-stress analyses, temperature is calculated in an uncoupled heat transfer analysis (Uncoupled Heat Transfer Analysis) or in a coupled thermal-electrical analysis (Coupled Thermal-Electrical Analysis).

This page discusses:

See Also
Defining an Analysis
About Heat Transfer Analysis Procedures
Predefined Fields for Sequential Coupling
In Other Guides
Creating and modifying output requests
Defining a temperature field

Products Abaqus/Standard Abaqus/CAE

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 and Writing Nodal Output to the Output Database.

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). The temperature interpolation in the stress elements is usually 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.

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.

Material Options

The materials in the thermal analysis must have thermal properties such as conductivity defined (see About Thermal Properties). Any mechanical properties such as elasticity will be ignored in the thermal analysis, but they must be defined for the stress analysis procedure. See Abaqus Materials Guide for details on the material models available in Abaqus/Standard.

Thermal strain will arise in the stress analysis if thermal expansion (Thermal Expansion) is included in the material property definition.

Elements

You can use any of the heat transfer elements in Abaqus/Standard in the thermal analysis. In the stress analysis, you must choose the corresponding continuum or structural elements. For example, if heat transfer shell element type DS4 is defined by nodes 100, 101, 102, and 103 in the heat transfer analysis, three-dimensional shell element type S4R or S4R5 must be defined by these nodes in the stress analysis procedure.

For continuum elements you can transfer heat transfer results from a mesh using first-order elements to a stress analysis with a mesh using second-order elements. For more information, see Using Second-Order Stress Elements with First-Order Heat Transfer Elements (the Midside Node Capability). You can activate the interpolation capability to map nodal temperatures between dissimilar meshes of matching element dimensionality (solid elements to solid elements or shell elements to shell elements). You cannot map nodal temperatures between heat transfer shell elements and structural membrane elements using the interpolation capability. For more information, see Interpolating Data between Meshes.

Output

The nodal temperatures must be written to the heat transfer analysis results or output database file by requesting the output variable NT (see Output to the Data and Results Files). These temperatures will be read into the stress analysis procedure.

Appropriate output variables are described in the heat transfer and stress analysis sections. All of the output variables are outlined in Abaqus/Standard Output Variable Identifiers.

Input File Template

A typical sequentially coupled thermal-stress analysis consists of two Abaqus/Standard runs: a heat transfer analysis and a subsequent stress analysis.

The following template shows the input for the heat transfer analysis heat.inp:

HEADING
…
ELEMENT, TYPE=DC2D4
(Choose the heat transfer element type)
…
STEP
HEAT TRANSFER
…
Apply thermal loads and boundary conditions
…
** Write all nodal temperatures to the results or
** output database file, heat.fil/heat.odb
NODE FILE, NSET=NALL
 NT
OUTPUT, FIELD
NODE OUTPUT, NSET=NALL
 NT
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 heat transfer element type used)
…
STEP
STATIC
…
Apply structural loads and boundary conditions
…
TEMPERATURE, FILE=heat
Read in all nodal temperatures from the results or output database file, heat.fil/heat.odb
…
END STEP