Products: ABAQUS/Standard ABAQUS/CAE
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.
The most common type of thermal-stress analysis is one in which the temperature field does not depend on the stress field. In such cases temperature is calculated in an uncoupled heat transfer analysis (“Uncoupled heat transfer analysis,” Section 6.5.2) or in a coupled thermal-electrical analysis (“Coupled thermal-electrical analysis,” Section 6.6.2).
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.
| Input File Usage: | Use the following option to request nodal output to the results file: |
*NODE FILE NT Use the following options to request nodal output to the output database file: *OUTPUT *NODE OUTPUT NT |
| ABAQUS/CAE Usage: | You cannot write output to the results file in ABAQUS/CAE. Use the following options to request nodal output to the output database file: |
Step module: field or history output request editor: Select from list below, Thermal, NT, Nodal temperature |
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 temperatures between meshes” in “Predefined fields,” Section 27.6.1). 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.
To define the temperature field at different times in the stress 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 stress problem—for example, 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 or output database file is read during the stress analysis, temperatures at nodes that are not present in the mesh for the stress analysis are ignored.
You must specify the name of the thermal analysis results or output database file that contains the nodal temperatures required in the stress analysis. The file extension is optional. If the heat transfer model and the stress analysis model share the same mesh, the default is the results file. If the heat transfer model and the stress analysis model have dissimilar meshes, the output database file must be used. See “Predefined fields,” Section 27.6.1, 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 stress analysis. If the thermal model is defined in terms of an assembly of part instances, the stress 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.
| Input File Usage: | *TEMPERATURE, FILE=file_name |
| ABAQUS/CAE Usage: | Load module: Create Predefined Field: choose Other as the Category and Temperature as the Types for Selected Step: select the region to which the field is applied: Distribution: From results or database file: File name: file_name |
Appropriate initial conditions for the thermal and stress analysis problems are described in the heat transfer and stress analysis sections—for example, see “Heat transfer analysis procedures: overview,” Section 6.5.1; “Coupled thermal-electrical analysis,” Section 6.6.2; “Static stress analysis procedures: overview,” Section 6.2.1; and “Dynamic analysis procedures: overview,” Section 6.3.1. See also “Initial conditions,” Section 27.2.1.
Appropriate boundary conditions for the thermal and stress analysis problems are described in the heat transfer and stress analysis sections—for example, see “Heat transfer analysis procedures: overview,” Section 6.5.1; “Coupled thermal-electrical analysis,” Section 6.6.2; “Static stress analysis procedures: overview,” Section 6.2.1; and “Dynamic analysis procedures: overview,” Section 6.3.1. See also “Boundary conditions,” Section 27.3.1.
Appropriate loading for the thermal and stress analysis problems is described in the heat transfer and stress analysis sections—for example, see “Heat transfer analysis procedures: overview,” Section 6.5.1; “Coupled thermal-electrical analysis,” Section 6.6.2; “Static stress analysis procedures: overview,” Section 6.2.1; and “Dynamic analysis procedures: overview,” Section 6.3.1. See also “Applying loads: overview,” Section 27.4.1.
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,” Section 27.6.1.
The materials in the thermal analysis must have thermal properties such as conductivity defined (see “Thermal properties: overview,” Section 20.2.1). Any mechanical properties such as elasticity will be ignored in the thermal analysis, but they must be defined for the stress analysis procedure. See Part V, “Materials,” for details on the material models available in ABAQUS/Standard.
Thermal strain will arise in the stress analysis if thermal expansion (“Thermal expansion,” Section 20.1.2) is included in the material property definition.
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)” in “Predefined fields,” Section 27.6.1).
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,” Section 4.1.2). 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,” Section 4.2.1.
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