Harmonic Acoustics Analysis

Introduction

Harmonic Acoustics analyses are used to determine the steady-state response of a structure and the surrounding fluid medium to loads and excitations that vary sinusoidally (harmonically) with time. Examples of harmonic acoustics include Sonar (the acoustic counterpart of radar), the design of concert halls, the minimization of noise in a machine shop, noise cancellation in automobiles, audio speaker design, speaker housing design, acoustic filters, mufflers, and Geophysical exploration. Typical quantities of interest in the fluid and far-field location at different frequencies are pressure distribution, pressure gradient, sound power, and particle velocity of acoustic waves.

In Harmonic Response analyses, the following equation is resolved for pure acoustic problems:

For fluid structure interaction problems, the acoustic and the structural matrices are coupled using the following equation:

Points to Remember

The Harmonic Acoustics environment provides the following context menu (right-click) options:

Preparing the Analysis

Create Analysis System

  Basic general information about this topic

  ... for this analysis type:

If you have not already created a Harmonic Acoustics system in the Project Schematic, see the Harmonic Acoustics section in the Workbench User's Guide for the steps to create this system.

Define Engineering Data

  Basic general information about this topic

  ... for this analysis type:

All the acoustic bodies must be assigned a material containing Density and Speed of Sound.


Important:  Air, Water Liquid, and Water Vapor from the Fluid Materials include the Speed of Sound property. Any other material to be used in the Acoustics Region requires you to specify the Speed of Sound from the Toolbox > Physical Properties category of Engineering Data workspace.


Define Part Behavior

  Basic general information about this topic

  ... for this analysis type:

A Structural Physics Region may contain bodies with the Stiffness Behavior set to Rigid. Acoustics Regions do not support a Stiffness Behavior setting of Rigid.

If the Structural Region has the Stiffness Behavior property set to Rigid and if it is in contact with acoustic regions, then fluid-structure interaction may not behave as expected.

Define Connections

  Basic general information about this topic

  ... for this analysis type:

There are no specific contact considerations for this analysis.

Apply Mesh Controls/Preview Mesh

  Basic general information about this topic

  ... for this analysis type:

There are no specific mesh considerations for a harmonic acoustics analysis.

Establish Analysis Settings

  Basic general information about this topic

  ... for this analysis type:

For a Harmonic Acoustics analysis, the basic Analysis Settings include:

Options

The Options category enables you to specify the frequency range and the number of solution points at which the harmonic analysis will be carried out as well as the solution method to use and the relevant controls.

Only the Direct Integration (Full) Solution Method is available to perform a Harmonic Acoustics analysis.

Scattering Controls

The Scattering Controls category includes the Scattered Field Formulation property. The options for this property include:

  • Program Controlled (default)

  • Off: Selecting this option turns scattering controls off.

  • On: Selecting this option turns scattering controls on and also displays the Scattering Output Type property.

    The Scattering Output Type property is used to specify the output type for an acoustic scattering analysis. The options for this property include Total and Scattered. Select the Total option when you wish to output the total pressure field and the Scattered option when you want to output the scattered pressure field.

    If you specify an Incident Wave Source excitation and also specify the Incident Wave Location property as Inside the Model, then the application uses the Total setting for the Scattering Output Type property only.

    For more information, refer to the ASOL and ASCRES commands in the Mechanical APDL Command Reference.

Advanced

The Advanced category includes the property Far-Field Radiation Surface. Far-field result calculations are based on the Equivalent Source (Maxwell) Surfaces. Therefore, this field controls far-field result definitions and results. The options include:

  • Program Controlled (default): If your analysis does not include a user-defined Far-Field Radiation Surface boundary condition object, this setting identifies the Equivalent Source (Maxwell) Surfaces automatically created by the application using the environment option Create Automatic > Far-Field Radiation Surface. In this case, the application applies the surface flag MXWF on them. If the analysis does include a user-defined Far-Field Radiation Surface object, this settings defined by that object are used.

  • Manual: This option requires the definition of at least one user-defined Far-Field Radiation Surface object.

  • No: This setting invalidates all Equivalent Source (Maxwell) Surface objects and Far Field Result objects.

Output Controls

For Acoustic Region:

By default, the application calculates Acoustic Pressure. You can also request Acoustic Velocity and Acoustic Energy.

For Structural Region:

Additional Output Controls are available when solving an FSI problem in order to control the results calculated on structural domain. By default, only deformations are calculated. You can request Stress and Strain results. You can also specify to Calculate Reactions.

Damping Controls

The Damping Controls category is visible when Structural Physics is turned on. These properties enable you to specify damping for the structure in the Harmonic Acoustics analysis. Controls include: Structural Damping Coefficient, Stiffness Coefficient (beta damping), and a Mass Coefficient (alpha damping). They can also be applied as Material Damping using the Engineering Data tab.

Element Damping: You can also apply damping through spring-damper elements. The damping from these elements is used only in a Full method harmonic analysis.


Important:  If multiple damping specifications are made the effect is cumulative.


Analysis Data Management

These properties enable you to save solution files from the harmonic analysis. The default behavior is to only keep the files required for postprocessing. You can use these controls to keep all files created during solution or to create and save the Mechanical APDL application database (db file).

Define Physics Region(s)

  Basic general information about this topic

  ... for this analysis type:

To create a Physics Region:

  1. Highlight the Environment object and select the Physics Region button on the Environment toolbar or right-click the Environment object or within the Geometry window and select Insert > Physics Region.

  2. Define all of the properties for the new object. For additional information, see the Physics Region object reference section.

    A Structural Physics Region may contain bodies with the Stiffness Behavior set to Rigid. Acoustics Regions do not support a Stiffness Behavior setting of Rigid.

    If the Structural Region has the Stiffness Behavior property set to Rigid and if it is in contact with acoustic regions, then fluid-structure interaction may not behave as expected.

Apply Loads and Supports

  Basic general information about this topic

  ... for this analysis type:

The following loading conditions are supported for this analysis type:

Inertial

Acceleration

Acoustic Excitations

Mass Source
Surface Velocity
Diffuse Sound Field
Incident Wave Source
Port in Duct

Acoustic Loads

Temperature
Impedance Sheet
Static Pressure

Acoustic Boundary Conditions

Pressure
Impedance Boundary
Absorption Surface
Radiation Boundary
Absorbing Element
Free Surface
Thermo-Viscous BLI Boundary
Rigid Wall
Symmetry Plane
Far-Field Radiation Surface

Acoustic Models

Transfer Admittance Matrix

The following loading conditions are supported if the analysis has structural physics:

Loads

Pressure
Force
Remote Force
Moment
Line Pressure
Fluid Solid Interface: Use the Create Automatic FSI option on the Environment context menu to auto generate the applicable Fluid Solid Interfaces.

Supports

Fixed Support
Displacement
Remote Displacement
Frictionless Support
Compression Only Support
Cylindrical Support
Elastic Support

Conditions

Constraint Equation

Direct FE

Nodal Orientation
Nodal Force
Nodal Displacement

Solve

  Basic general information about this topic

  ... for this analysis type:

The Solution Information object provides some tools to monitor solution progress.

Solution Output 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

  Basic general information about this topic

  ... for this analysis type:

You can scope most of the Harmonic Acoustic analysis results to entities on acoustic bodies and, by default, all acoustic bodies compute results for display.

Additional results are available for structural domain when solving Fluid Structural Interaction (FSI) problems. Refer to the Review Results section of Harmonic Response Analysis for more information regarding how to set up the harmonic results.


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