Defining a temperature field

You can define the magnitude and time variation of the temperature of the selected region for each analysis step; Abaqus will interpolate the temperatures to the material points. Alternatively, you can use the temperature values that Abaqus computed during a previous analysis with thermal components to define the temperatures in the current model.

Related Topics
Understanding symbols that represent prescribed conditions
Creating predefined fields
Using analytical expression fields
Creating expression fields
Creating discrete fields
In Other Guides
Predefined temperature

  1. Display the temperature field editor using one of the following methods:

    • To create a new temperature field, follow the procedure outlined in Creating predefined fields (Category: Other; Types for Selected Step: Temperature).

      Note:

      If you want to specify the temperature variation directly in the temperature field editor, in user subroutine UTEMP, or using an analytical field or discrete field, you must select a region for the temperature field. If you want to specify any other temperature distribution, you may click Done in the prompt area to use a calculated temperature.

    • To edit an existing temperature field using menus or managers, see Editing step-dependent objects.

  2. If you are editing a temperature field in any general analysis step other than the one in which the field was created, click the arrow to the right of the Status field, and select the option of your choice from the list that appears:

    • Select Propagated to indicate that the temperature field is active in the current step with temperatures values held constant from the previous step. No data can be specified; click OK to exit the editor. If you change the status of the current step from Modified to Propagated and click OK, all modifications to the current step are removed.

    • Select Modified to edit the field definition for the current step. Continue with Step 3.

    • Select Reset to initial to reset the field definition to the one that was prescribed in the initial step. No data can be specified; click OK to reset the field and to exit the editor.

  3. If you are creating a new temperature field, click the arrow to the right of the Distribution field, and select the option of your choice from the list that appears.

    Note:

    If you are creating a temperature field in the initial step, only the Direct specification, From results or output database file, analytical field, and discrete field distribution options are available.

    • Select Direct specification to specify the temperature variation over the selected region in the temperature field editor.

    • Select From results or output database file to read temperature values from the results or output database file of a previous Abaqus analysis with thermal components.

    • Select User-defined to define temperature values in user subroutine UTEMP. This option is available only for Abaqus/Standard analyses. See the following sections for more information:

    • Select From results or output database file and user-defined to read temperature values from the results or output database file of a previous Abaqus analysis with thermal components and modify them in user subroutine UTEMP. This option is available only for Abaqus/Standard analyses.

    • Select an analytical field, labeled with an (A), or a discrete field, labeled with a (D), to define a spatially varying temperature. The selection list contains all analytical fields and only discrete fields that are valid for temperature fields.

      Alternatively, you can click to create a new analytical field. (See The Analytical Field toolset for more information.)

  4. If you selected the Direct specification, analytical field, or discrete field distribution option, perform the following steps:

    1. Click the arrow to the right of the Section variation field, and select an option from the list that appears. Only options that are valid for the selected region appear in the list. Beam and shell gradient values are not affected by an analytical field or a discrete field. You should select an option that is consistent with the temperature variation method defined in the section definition associated with the region selected for this field as follows:

      • Select Constant through region to define a constant temperature over a section.

        In the Magnitude text field, enter the magnitude of the temperature across the section.

      • Select Gradient through shell section to define a temperature variation through a shell section. The Temperature variation method in the shell section editor must specify Linear through thickness.

        In the Reference magnitude text field, enter the magnitude of the temperature at the reference surface. In the Thickness gradient text field, enter the temperature gradient through the section.

      • Select Gradient through beam section to define a temperature variation through a beam section. (This method is not available for axisymmetric models.) The Temperature variation method in the beam section editor must specify Linear by gradients.

        In the Reference magnitude text field, enter the magnitude of the temperature at the cross-section origin. In the N1 gradient and N2 gradient text fields, enter the temperature gradients through the section in the n1- and n2-directions of the beam, respectively. For beams in a plane only the temperature magnitude and the N2 gradient must be specified.

      • Select Defined at shell/beam temperature points to define a piecewise linear temperature variation through a shell or beam section. The Temperature variation method in the shell section editor must specify Piecewise linear over n values. The Temperature variation method in the beam section editor must specify Interpolated from temperature points.

        Select the number of temperature points to be specified by either typing an integer in the Temperature points text field or using the arrows to the right of the text field to select a number, and enter the magnitude of the temperature at each point in the Section Data table. The number of values in the section definition should be less than or equal to the number of temperature data points given for this field. If the number of values is less, the last value will be repeated to match the number of temperature data points.

    2. If desired (for all steps other than the initial step), click the arrow to the right of the Amplitude text field, and select the amplitude of your choice from the list that appears. Alternatively, you can click to create a new amplitude. (See The Amplitude toolset for more information.) Beam and shell gradient values will be modified by the amplitude definition.
    3. Click OK to save your data and to exit the editor.

  5. If you selected the From results or output database file distribution option, perform the following steps:

    1. In the File name text field, enter the name of the results or output database file from which temperature data are to be read; or click to display the Select Results or Output Database File dialog box and select the file of your choice. (See Using file selection dialog boxes for more information.)
    2. If you are creating a temperature field in the initial step:

      • In the Step text field, enter the step number of the analysis whose results or output database file is being used as input from which the field data should be read.

      • In the Increment text field, enter the increment number of the analysis whose results or output database file is being used as input from which the field data should be read.

    3. Optionally, if you are creating a temperature field in an analysis step other than the initial step:

      • In the Begin step text field, enter the step number of the analysis whose results or output database file is being used as input that begins the field data to be read. By default, the first step available in the results or output database file will be used.

      • In the Begin increment text field, enter the increment number of the analysis whose results or output database file is being used as input that begins the field data to be read. By default, the first increment available in the results or output database file will be used.

      • In the End step text field, enter the step number of the analysis whose results or output database file is being used as input that ends the field data to be read. By default, the Begin step value will be used.

      • In the End increment text field, enter the increment number of the analysis whose results or output database file is being used as input that ends the field data to be read. By default, the last increment available for the End step value in the results or output database file will be used.

    4. Choose the Mesh compatibility.

      • Select Compatible if the meshes in the original analysis and the current analysis are the same or differ only in the element order.

        If the original and current meshes differ only in the element order, you must indicate that midside node temperatures in second-order elements are to be interpolated from corner node temperatures by toggling on Interpolate midside nodes.

      • Select Incompatible if the meshes in the original analysis and the current analysis are dissimilar. This option is valid only if the temperature values are being read from an output database file.

    5. If the original and current meshes are dissimilar, you can specify a value for the Exterior tolerance.

      • Specify the absolute value by which nodes of the current model may lie outside the region of the elements of the original model. If this value is not specified or is 0.0, the relative tolerance will apply.

      • Specify the relative fraction of the average element size by which nodes of the current model may lie outside the region of the elements of the original model.

      If both tolerances are specified, Abaqus uses the tighter tolerance.

    6. Click OK to save your data and to exit the editor.

  6. If you selected the User-defined distribution option, perform the following steps:

    1. Click OK to exit the editor.
    2. Enter the Job module, and display the job editor for the analysis job of interest. (For more information, see Creating, editing, and manipulating jobs.)
    3. In the job editor, click the General tab, and specify the file containing the user subroutine that defines the temperature field. For more information, see Specifying general job settings.

      Note:

      You can specify only one user subroutine file in the job editor; if your analysis involves more than one user subroutine, you must combine the user subroutines into one file and then specify that file.

  7. If you selected the From results or output database file and user-defined distribution option, follow the procedures outlined in Steps 5 and 6 for the From results or output database file and User-defined distribution options.