Field Variables

Material data can be dependent on variables such as temperature, shear angle, degradation factor, or user-defined entries. These variables are termed as Field Variables and are only available for specific material properties and models, as listed below. For more information on this topic, see the discussion on User-Defined Field Variables in the Mechanical APDL Material Reference.

Engineering Data supports the following Field Variables:

The use of field variables to further define material properties enables you to simulate the effects of environmental conditions and manufacturing processes on material characteristics. This can be of particular importance when you are using the ANSYS Composite PrepPost application to model composites. See the Variable Material Data in Composite Analyses section of the ANSYS Composite PrepPost User's Guide for additional information.

The material properties and models supported by the field variable feature are based on the selected analysis system. Refer to the Supported Properties section of the documentation for a listing of all of the supported analysis types and the material properties that each analysis supports. You will note that certain properties are appended with a function notation to indicate supported fields. This includes:

The Shear Angle and Degradation Factor field variables are predefined user-defined variables. Based on this, isotropic elasticity supports all field variables and is denoted as: Isotropic Elasticity f(T,F,U).

However, for Modal Acoustic analysis system, only temperature is supported and so denoted as: Density f(T). For material properties that are defined with unsupported field variables, the application uses the default value for the unsupported field variables to calculate dependent values for the supported field variable(s) values. For example, during a Modal Acoustics analysis, you can enter frequency dependent and/or temperature dependent material properties, however:

Defining System Provided Field Variables

To implement a system provided field variable:

  1. Select one of the supported material properties (as listed above). The application displays the Field Variables category in the Toolbox.

  2. From the Field Variables category, select the desired system provided field variable:

    • Temperature

    • Frequency

    • Shear Angle

    • Degradation Factor

    The new field variable populates the Table pane. Enter appropriate values.

  3. Enter appropriate values into the Table Pane.

Creating User-Defined Field Variables

To implement a user-defined field variable:

  1. Select the Create Field Variable option from the Field Variables category in the Toolbox.

  2. The following dialog box displays. Enter a name for your new field variable and select a desired Quantity Type from the drop-down list. Dimensionless is the default. Once complete, click OK.

  3. The new field variable populates the Table pane. Enter appropriate values. Example entries are illustrated below for the user-defined field variable Example_Custom_Fld_Var.

  4. Select the Interpolation Options property to display the following Table pane. This table defines the algorithm the solver uses to interpolate between the data entered in the Table pane from Step 2 in order to get the values corresponding to the calculated field variable values on a given element. Please refer to the General Interpolation Library section of the ANSYS Composite PrepPost User's Guide for more details about the algorithms and options used when creating user-defined Field Variables.

  5. Select one of the following Algorithm Types from the drop-down menu:

  6. Refine the interpolation algorithm by activating one or more of the following options.

    • Normalize: scale the axes to achieve an unbiased distance metric. The ranges used to scale the axes are defined by the Lower Limit and Upper Limit values of the Material Field Variables table pane.

    • Cache: save previous queries in order to increase performance.

  7. Select the Material Field Variables property to display the following table pane.

    Field descriptions for the Interpolations Options property:

    • Default Data: this value is used by the interpolation algorithm when the corresponding field variable is not defined on a given element.

    • Lower Limit: this value defines the upper boundary on the range used when the data is normalized and/or quantized. When you use the Program Controlled setting, the value defaults to the minimum value of the data entered for all instances of the corresponding field variable in the selected material.

    • Upper Limit: this value defines the upper boundary on the range used when the data is normalized and/or quantized. When you use the Program Controlled setting, the value defaults to the maximum value of the data entered for all instances of the corresponding field variable in the selected material.

Usage Notes

The order in which you add field variables to a material property becomes important if:

Whichever field variable varies the most, is the variable that you should insert and define first. Consider the example illustrated below. In this case, the Temperature varies more than the Shear Angle, so it will be best to add temperature first and then shear angle. Adding the field variables in this order results in a table structure that, for each shear angle, there is data at multiple temperatures.

The drop-down menu on the Table pane for the field variable provides options (e.g., sorting and filtering). In order to remove a Field Variable from a property, you must use the Delete option from this drop-down menu.


Release 18.2 - © ANSYS, Inc. All rights reserved.