The Mechanical application enables you to apply velocities from a Structural Harmonic Response analysis as loads in an Acoustic analysis. The load transfer is applicable for the cases where the harmonic response and acoustic analyses are solved using different meshes. In this case, the velocity values are mapped and interpolated between the source and target meshes.
An acoustic analysis is performed via ACT. For information on creating optimization extensions, see the ANSYS ACT Developer's Guide.
Workflow for performing a one-way acoustic coupling analysis.
From the toolbox, drag and drop a Harmonic Response template onto the project schematic. Perform all steps to set up a Harmonic Analysis. Specify mesh controls, boundary conditions, and solution settings as you normally would and solve the analysis.
Drag and drop a Harmonic Response template onto the project schematic. Drag the Solution cell of the structural system onto the Setup cell of the acoustic system.

Double-click the acoustic system’s system Setup cell. In the Mechanical application, insert an Imported Velocity load into the acoustic system’s tree under an Imported Load folder.
Select appropriate geometry in the Details view of the imported velocity object using the Geometry or Named Selection scoping option.
The Source Bodies option in the Details view enables you to select the bodies, from the thermal analysis, that makeup the source mesh for mapping the data. You can choose one of the following options:
All- The source mesh in this case will comprise all the bodies that were used in structural analysis.
Manual- This option enables you to select one or more source bodies to make up the source mesh. The source body selections are made in the Material IDs field by entering the material IDs that correspond to the source bodies that you would like to use. Type material IDs and/or material ID ranges separated by commas to specify your selection. For example, type 1, 2, 5–10. The material IDs for the source bodies can be seen in Solution Information Object of the source analysis. In the example below, text is taken from a solver output,
***********Elements for Body 1 "coil" *********** ***********Elements for Body 2 "core" *********** ***********Elements for Body 3 "bar" ************
body ‘coil’ has material ID 1, body ‘core’ has material ID 2 and body ‘bar’ has material ID 3.
Change any of the columns in the Data View tab as needed:
Source Frequency- Frequency at which the velocities will be imported from the structural analysis.
Analysis Frequency- Choose the analysis frequency at which the load will be applied.
Note: The Data view can automatically be populated with the source and analysis frequencies using the Source Frequency property in the Details View. Use All to import data at all frequencies in the source analysis, or Range to import data for a range specified by a Minimum and Maximum. The default worksheet option requires users to manually input the Source Frequency and Analysis Frequency.
You can transform the source mesh used in the mapping process by using the Rigid Transformation properties. This option is useful if the source geometry was defined with respect to a coordinate system that is not aligned with the target geometry system.
You can modify the Mapper Settings to achieve the desired mapping accuracy. Mapping can be validated by using Mapping Validation objects.
Right-click the Imported Velocity object and click Import Load to import the load. When the load has been imported successfully, vectors plot (All), or contour plot (Total/X/Y/Z) of the real/imaginary components of velocities can be displayed in the Geometry window using the Component property in the details of imported load.
Note: The range of data displayed in the graphics window can be controlled using the Legend controls options. See Imported Boundary Conditions for additional information.
If multiple rows are defined in the Data view, it is possible to preview imported load vectors/contour applied to a given row or analysis frequency in the Data view. Choose Active Row or Analysis Frequency using the By property under Graphics Controls in the details of the imported load and then specify the Active Row/Analysis Frequency to preview the data.
Note: If the Analysis Frequency specified by the user does not match the list of analysis frequencies in the Data View, the data is displayed at the analysis frequency closest to the specified frequency.
Note: If the upstream (Structural) system is modified and re-solved after importing the load, a refresh operation on the Acoustic system’s Setup cell is required to notify Mechanical that source data has changed and re-import is required. Alternatively, the source data can be refreshed using the right-click operation on the Imported Load folder and choosing the Refresh Imported Load option.