Sequentially coupled thermal-stress analysis | ||||||||||
|
| |||||||||
ProductsAbaqus/StandardAbaqus/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 Node output.
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.
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 About heat transfer analysis procedures, Coupled thermal-electrical analysis, About static stress analysis procedures, and About dynamic analysis procedures. See also Initial conditions in Abaqus/Standard and Abaqus/Explicit.
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 About heat transfer analysis procedures, Coupled thermal-electrical analysis, About static stress analysis procedures, and About dynamic analysis procedures. See also Boundary conditions in Abaqus/Standard and Abaqus/Explicit.
Loads
Appropriate loading for the thermal and stress analysis problems is described in the heat transfer and stress analysis sections—for example, see About heat transfer analysis procedures, Coupled thermal-electrical analysis, About static stress analysis procedures, and About dynamic analysis procedures. See also About loads.
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
Any of the heat transfer elements in Abaqus/Standard can be used in the thermal analysis. In the stress analysis the corresponding continuum or structural elements must be chosen. 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 heat transfer results from a mesh using first-order elements can be transferred to a stress analysis with a mesh using second-order elements (see Using second-order stress elements with first-order heat transfer elements (the midside node capability)).
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