Introduction
Mechanical enables you to perform a FSI Harmonic analysis on a pre-stressed structure using a Static Acoustics Analysis.
Points to Remember
To perform a prestressed Harmonic Acoustics analysis you need to first perform a Static Acoustics analysis and properly link it to the Harmonic Acoustics analysis. When performing this type of linked analysis, the Harmonic Acoustics analysis uses the Physics Regions (Acoustic and Structural) defined in the Static Acoustics analysis. Therefore, you need to remove the Acoustics Region from your Harmonic Acoustics analysis when you first create the linked systems.
Preparing the Analysis
Because this analysis is linked to (and based on) structural responses, a Static Acoustics analysis is a prerequisite. This setup allows the two analysis systems to share resources, such as material data, geometry, and the boundary condition type definitions that are defined the in the static acoustics analysis.
From the Workbench Toolbox, drag a Static Acoustics template to the Project Schematic. Then, drag a Harmonic Acoustics template directly onto the Solution cell of the Static Acoustics template.
Define Initial Conditions
The Pre-Stress object of the Harmonic Acoustics analysis must point to the linked Structural Acoustics analysis.
Note:
All structural loads, including Inertial loads, such as Acceleration and Rotational Velocity, are deleted from the harmonic analysis portion of the simulation once the loads are applied as initial conditions (via the Pre-Stress object). Refer to the Mechanical APDL command PERTURB,HARM,,,DZEROKEEP for more details.
For Pressure boundary conditions in the Structural Acoustics analysis: if you define the load with the Normal To option for faces (3D) or edges (2D), you could experience an additional stiffness contribution called the "pressure load stiffness" effect. The Normal To option causes the pressure acts as a follower load, which means that it continues to act in a direction normal to the scoped entity even as the structure deforms. Pressure loads defined with the or options act in a constant direction even as the structure deforms. For a same magnitude, the "normal to" pressure and the component/vector pressure can result in significantly different results in the follow-on Harmonic Acoustics analysis. See the Pressure Load Stiffness topic in the Applying Pre-Stress Effects for Implicit Analysis Help section for more information about using a prestressed environment.
If displacement loading is defined with Displacement, Remote Displacement, Nodal Displacement, or Bolt Pretension (specified as , , or ) loads in the Structural Acoustics analysis, these loads become fixed boundary conditions for the harmonic solution. This prevents the displacement loads from becoming a sinusoidal load during the Harmonic solution. If you define a Nodal Displacement in the harmonic analysis at the same location and in the same direction as in the structural analysis, it overwrites the previous loading condition and/or boundary condition in the harmonic solution.
Establish Analysis Settings
See the Establish Analysis Settings topic in the Harmonic Acoustics section for a complete listing of the Analysis Settings.
Apply Loads and Supports
See the Acoustics Loading Conditions as well as the Boundary Conditions section of the Mechanical User's Guide for a listing of all available loads, supports, etc. for this analysis type.
Solve
The Solution Information object provides some tools to monitor solution progress.
The setting for the Solution Output property continuously updates any listing output from the solver and provides valuable information on the behavior of the model during the analysis. Any convergence data output in this printout can be graphically displayed as explained in the Solution Information section.
Review Results
See the Acoustic Results section for descriptions of all supported result types.
Harmonic Acoustic results generally default to the setting . You can individually scope most of the Harmonic Acoustic analysis results to mesh or geometric entities on acoustic bodies.
Additional results are available for structural domain when solving Fluid Structural Interaction (FSI) problems. Refer to the Review Results topic in the Harmonic Response Analysis for more information regarding how to set up the harmonic results.