Importing Data into a Thermal or Structural (Static or Transient) Analysis

This feature enables you to perform a one-way Electromagnetics (EM) - Mechanical interaction problem by solving the electromagnetic analysis of the geometry in the HFSS, Maxwell, or Q3D Extractor applications, importing the thermal or structural results into the ANSYS Mechanical application where the defined load is applied to a thermal or structural analysis which is then solved and post processed.

For a thermal analysis, you can import Imported Heat Generation and Imported Heat Flux load types.

For a structural analysis you can import Imported Body Force Density (illustrated below) and Imported Surface Force Density load types.

Add the Imported Load

Follow these steps to add an imported load and associate it with parts of the geometry.

  1. Double-click the Model cell in your analysis system to open the Mechanical application.

  2. Click on the Imported Load group object. In the Details view, set the following field as needed:

    • If you want to suppress all of the loads under this Imported Load group, set the Suppressed field to Yes.

  3. For the Body Force Density and the Surface Force Density loading types, you can choose to import the Max Force Density or the DC Force Density, if the source provides the data, using the Data Type property. By default, the application imports the DC Force Density values. The application combines AC and DC values to calculate the Max Force Density value. Because the AC force is a complex vector, the peak vector among all phases of the AC force is taken and added to the DC force to obtain the Max Force Density.

  4. There are several ways to select an imported load and associate it with a part of your model.

    • Click an Imported Load Group object in the tree, click a part of the model, then right-click Imported Loads and from the Import menu item select the desired load type from the allowed imported load types. The load will be applied to the object you selected on the model.

    • Click on an Imported Load Group object in the tree, then click the Imported Loads button in the toolbar and select the desired load type from the allowed imported load types. In the Details view, click the Geometry field. Select the objects in the model to which you want to apply the load and click the Apply button in the Geometry field.

    • Right-click the Imported Loads Group object that was just added to the tree and select the desired load type from the allowed imported load types. In the Details view, click the Geometry field. Select the objects in the model to which you want to apply the load and click the Apply button in the Geometry field.


    Note:  Heat generation loads scoped to a surface body use the constant thickness value specified in the details view of the surface body object when data is imported. Surface body thickness defined using the thickness object is not accounted for when data is imported.


Set the Imported Load Options
  1. Click on the imported load object that you've added to the tree.

  2. Select the desired Ansoft solution you would like to import the load from. Some of the properties in the Details view and Data View tab are filtered based on this selection.

  3. Change any of the fields in the Details View as needed:

    • Scoping Method– Select the method of choosing objects to which the load is applied: Geometry Selection or Named Selection.

    • Geometry or Named Selection– Use these fields to choose the objects to which the load is applied, as appropriate from your Scoping Method choice.

    • Suppressed– Select Yes to suppress this load.

    • Ansoft Surface(s)– Select the Ansoft Surface(s) for a Heat Flux or Surface Force Density load.

      or

      Ansoft Volume(s)– Select the Ansoft Volume(s) for a Heat Generation or Body Force Density load.

Set the Imported Load Analysis Options

You can specify when the imported data should be applied and also modify the imported data, either by adding an offset or by using a scale factor.

To see the analysis setting for a load, click the object that you've added to the tree. The analysis options appear in the Data View tab of the window below the model. Make any changes to the load's analysis options as indicated below.

Change any of the columns in the Data View tab as needed:

You must re-solve after making any changes to the analysis options of a load.

You can define multiple rows in the Data View tab to import additional data from the selected Ansoft solution and apply the rows at different analysis times. If multiple rows are defined in the Data View tab, you can display imported values at different time steps by changing the Active Row option in the Details pane.

Right-click the Imported Load object and click Import Load to import the load. When the load has been imported successfully, a contour plot of the temperatures will be displayed in the Geometry window and a summary of the transfer is displayed as a comment in the particular load branch.


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