In general, the program simulates interior problems or exterior problems as well as FSI problems.
For interior problems, a sound wave propagates or oscillates in a closed structure. The oscillating frequencies and transmission loss (TL) are usually investigated.
For exterior problems, a sound wave radiates into open space or it is scattered by a structural object in the open domain. The radiation sound power level (Lw), directive gain, or target strength (TS) is usually investigated. The program’s applications include, but are not limited to, sonar, noise investigation, acoustic design of architecture, underwater acoustics, and the design of acoustic devices.
An acoustic analysis involves most of the general steps found in any analysis. Following is the general process for performing an acoustic analysis:
Table 1.1: Acoustic Analysis Steps
| Step | Tasks | Comments |
| 1. | Build the model. |
An acoustic model generally consists of fluid domain, structural parts, FSI interfaces, sound excitations, and the truncation of the infinite domain. Ansys Workbench may help in building the model easily. |
| 2. | Set up the model environment. |
Acoustic analysis is supported by the FLUID30, FLUID220, FLUID221, FLUID243, and FLUID244 elements. The FLUID129 and FLUID130 elements can act as absorbing elements to truncate the infinite fluid domain. |
| 3. | Define material properties. |
Defining the material properties for an acoustic analysis is no different from any other analysis. Use the MP or TB commands to define linear or nonlinear material properties. The equivalent fluid model is defined by the TB command. For more information, see Defining Material Properties in the Basic Analysis Guide and Sophisticated Acoustic Media in the Mechanical APDL Theory Reference. |
| 4. | Mesh the model. |
Use meshing commands to mesh the different parts of the model. Certain areas may require more detailed meshing or special considerations. To ensure a reliable solution, either 10 elements per wavelength for low-order elements or 5 elements per wavelength for high-order elements are required at the highest working frequency. For more information, see the Modeling and Meshing Guide. |
| 5. | Define the boundary conditions. |
Define the boundary conditions using the D, SF, or BF command. The absorbing element FLUID130 or Artificially Matched Layers can achieve better accuracy for an open domain problem. For more information refer to Acoustic Boundary Conditions, Absorbing Boundary Condition (ABC), or Artificially Matched Layers in the Mechanical APDL Theory Reference. |
| 6. | Define the loads and excitations. |
Define the loads and excitations (D, SF, or BF). If the analytic wave sources are required, issue the AWAVE command. The DFSWAVE command specifies the diffuse sound field for random acoustics. An analytic acoustic mode is launched into the acoustic duct by the APORT command. The mean flow effect is taken into account via a defined mean flow velocity (BF command). The trim element with transfer admittance matrix is defined by the TB command for perforated structures. For more information, see Acoustic Excitation Sources and Sophisticated Acoustic Media in the Mechanical APDL Theory Reference. |
| 7. | Account for the FSI effect. |
Use the SF command to account for the acoustic fluid-structure interaction (FSI) effect. The solution for FSI with the strong coupled matrix is performed. For more information, see Acoustic Fluid-Structure Interaction (FSI) in theMechanical APDL Theory Reference. |
| 8. | Solve the model. |
The solution phase of an acoustic analysis adheres to standard Mechanical APDL conventions, although the FSI coupled matrices may not be symmetric. Modal, harmonic, and transient analyses may be performed. You may choose the symmetric algorithm for coupled matrices in a modal or harmonic analysis. The pure scattered pressure formulation is also available for the analytic incident wave, for more information see Pure Scattered Pressure Formulation in the Mechanical APDL Theory Reference. You can use structural results as the acoustic excitation source via the one-way coupling procedure (ASIFILE). You can impose Ansys Fluent CFD results (stored in a .CGNS file) on the structural surface via the one-way coupling procedure (FLUREAD). You can take the nonlinear static analysis into account and use a morphed mesh for the acoustic-structural coupled solution via a linear perturbation scheme. |
| 9. | Postprocess the acoustic analysis. |
Use the POST1 general postprocessor and the POST26 time history postprocessor to review results. Specific commands are available in POST1 for near- and far-field parameters (PRNEAR, PLNEAR, PRFAR, PLFAR, *GET), for sound power data (PRAS, PLAS), for various acoustic quantities (PRAS, PLAS), and for structural results as the acoustic excitation source (ASIFILE). |