Creating Temperature Histories
Temperature histories represent the magnitude and time variation of temperature at the nodes throughout a body during an analysis.
Temperature histories can be applied only in mechanical steps.
A uniform temperature history distribution can be defined, or the temperature history data can be read from the results file or the output database file of a previous heat transfer analysis.
The magnitude of a temperature history can vary with time during a step according to an amplitude definition (see Amplitudes for more information on defining amplitudes).
You can prescribe the time variation of the magnitude of a temperature history in a user subroutine, which is sometimes preferable when the time history of the magnitude is complex. You can also apply knowledgeware techniques to control the value of a temperature history (for more information, see Applying Knowledgeware).
The temperature difference between the temperature field defined by a temperature history and the temperature field defined by an initial temperature will create thermal strains if a thermal expansion coefficient is given for the material. The temperature field specified by the temperature history also affects temperature-dependent material properties, if any.
You can import temperature data into a temperature history definition from a Microsoft Excel spreadsheet (.xls*) or a text file (.txt). The imported temperature data must satisfy the following criteria:
The data must be arranged in four columns in the following order: X-coordinate, Y-coordinate, Z-coordinate, and temperature value.
The data must include a header row in which the dimensional data are provided in parentheses. Temperature data can be provided without dimensions. The following sample header row provides one example of proper header row syntax:
X(mm) Y(mm) Z(mm) Temperature()
The actual temperature values created from imported data will be the product of the dimensionless temperature values multiplied by the value you provide for the Magnitude of the temperature. For example, if your imported data specify a dimensionless value of 10 at the location (0, 0, 0) and you specify a value of 20Kdeg for the temperature history object, the temperature at that location will be 200K for the analysis.
Temperature histories can be applied to volume or part supports or to mesh parts.
This task shows you how to create a temperature history on geometry.
Click the Temperature History icon
.The Temperature History dialog box appears, and a Temperature History object appears in the specification tree under the Fields objects set for the current step.
You can change the identifier of the field by editing the Name field.
Select the geometry support (a volume, part, or mesh part). Any selectable geometry is highlighted when you pass the cursor over it. You can select several supports to apply the field to all supports simultaneously.
The Supports field is updated to reflect your selection.
Select the Distribution Type for the temperature history:
Uniform: You will define a uniform temperature variation over the selected region.
From job: The temperature data will be obtained from the results file of a previous heat transfer analysis.
User-defined: The temperature data will be defined in user subroutine UTEMP. For more information, see Using User Subroutines and UTEMP in the Abaqus User Subroutines Guide.
From job and user-defined: The temperature data will be obtained from the results file of a previous heat transfer analysis and modified in user subroutine UTEMP.
If you selected the Uniform distribution type, enter a value for the temperature in the Magnitude field.
Right-click on the Magnitude field to add knowledgeware controls (for more information, see Applying Knowledgeware).
If you selected the Uniform distribution type, you can import and incorporate a temperature history by performing the following steps from the Uniform Distribution options:
Toggle on Data mapping, then click the ... button.
The Data Mapping dialog box appears.
Click Browse, then select the spreadsheet or text file from which you want to import temperature data.
Once you select a file, you can display the imported data in tabular form in the Imported Table dialog box by clicking Show.
If desired, toggle on Display Bounding Box to display a three-dimensional box incorporating the minimum and maximum values from the imported table. The bounding box enables you to confirm that the support you select lies completely within the space dictated by the imported data; if a portion of the support is outside this box, an error will be returned during the analysis.
Click OK to close the Data Mapping dialog box.
If you selected the From job or From job and user-defined distribution types:
In the specification tree, select the heat transfer job from which the temperature data should be read.
In the Begin Step and Begin Increment fields, enter the step and increment number, respectively, of the heat transfer job that begins the temperature data to be read.
In the End Step and End Increment fields, enter the step and increment number, respectively, of the heat transfer job that ends the temperature data to be read.
Toggle off Interpolate Midside Nodes to use thermal data from the midside nodes in your model, where they are available.
Click More to access additional temperature history options.
Toggle on Selected amplitude, and select an amplitude from the specification tree to define a nondefault time variation for the temperature history.
If you do not specify an amplitude in a Nonlinear Structural case, Abaqus applies the reference magnitude based on the option that you selected when you created the step. Abaqus either applies the reference magnitude linearly over the step (Ramp) or applies it immediately at the beginning of the step and subsequently holds it constant (Instantaneous).
If you do not specify an amplitude in an Explicit Dynamics case, Abaqus uses a linear interpolation to apply the reference magnitude over the step.
See About Prescribed Conditions in the Abaqus Prescribed Conditions Guide for more information.
Click OK in the Temperature History dialog box.
Symbols representing the applied field are displayed on the geometry.