A Modal Acoustic analysis models a structure and the surrounding the fluid medium to determine frequencies and standing wave patterns within a structure. Examples of 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.
A Modal Acoustic analysis usually involves modeling the fluid medium as well as the surrounding structure in order to determine frequencies and standing wave patterns within a structure. Typical quantities of interest are the pressure distribution in the fluid at different frequencies, pressure gradient, and particle velocity of acoustic waves.
Mechanical enables you to model pure acoustic problems and fluid-structure interaction (FSI) problems. A coupled acoustic analysis accounts for FSI. An uncoupled acoustic analysis simulates the fluid only and ignores any fluid-structure interaction.
Note that:
This analysis supports 3D geometries only.
If possible, model your fluid region as a single solid multibody part.
This analysis requires that the air surrounding the physical geometry be modeled as part of the overall geometry. The air domain can be easily modeled in DesignModeler using the Enclosure feature.
The Physics Regionobject(s) need to identify all of the active bodies that may belong to the acoustic and structural (if FSI) physics types. For your convenience, when you open a Modal Acoustics system, the application automatically inserts a Physics Region object and scopes it to all bodies. You need to specify the physics selection.
The following context menu (right-click) options are available for this object:
> : This selection creates a Fluid Solid Interface object with all possible Fluid Solid Interface face selection based on the physics region definitions.
> :
>
Create Analysis System
Basic general information about this topic
... for this analysis type:
If you have not already created a Modal Acoustics system in the Project Schematic, see the Modal 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.
Note: The acoustic damping material properties like Viscosity and/or Thermal Conductivity are applicable only for a damped modal solver. You need to set Damped property under Solver Controls to and select from the available damped modal solver types.
Attach Geometry
Basic general information about this topic
... for this analysis type:
There are no specific geometry considerations for a modal acoustic analysis.
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 . Acoustics Regions do not support a Stiffness Behavior setting of .
If the Structural Region has the Stiffness Behavior property set to 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:
Only the Bonded contact Type setting and the MPC Formulation are valid when defining contact between two acoustic bodies or an acoustic and a structural body (FSI contact) which have non-conforming meshes. In addition, for FSI contact, the Contact side must be on the acoustic body and the Target must be on the structural body.
Note: Contact settings other than Bonded using MPC are ignored and are overwritten with the following preferred key options of Bonded/MPC contact:
For fluid-fluid contact: keyo,cid,1,10 ! select only PRES dof
For FSI contact:
keyo,cid,8,2 ! auto create asymmetric contact
keyo,tid,5,2 ! For case of solid-shell body contact
keyo,tid,5,1 ! For case of solid-solid body contact
Bonded Always: keyo,cid,12,5
MPC Formulation: keyo,cid,2,2
Refer to Matrix-Coupled FSI Solutions section from the Mechanical APDL Acoustic Analysis Guide for more information.
As applicable, the application generates automatic contacts between fluid-fluid and fluid-solid bodies based on the criterion mentioned above.
Joints, Springs, Bearings, and/or Beams are not supported on acoustic bodies.
Apply Mesh Controls/Preview Mesh
Basic general information about this topic
... for this analysis type:
There are no special mesh considerations for this analysis type.
Establish Analysis Settings
Basic general information about this topic
... for this analysis type:
Basic Analysis Settings include:
- Options
Using the Max Modes to Find property, specify the number of frequencies of interest. The default is to extract the first 6 natural frequencies. The number of frequencies can be specified in two ways:
The first N frequencies (N > 0).
Or...
The first N frequencies in a selected range of frequencies.
Note: The Limit Search to Range property is set to by default and the Range Minimum property is set to greater than or equal to 0.01 Hz.
- Solver Controls
This Solver Controls includes the following properties:
Damped: Use this property to specify if the modal system is undamped or damped. Depending upon your selection, different solver options are provided. The default setting of the Damped property is , which assumes that the modal acoustics system is an undamped system.
Solver Type: It is generally recommended that you allow the application to select the solver type for your analysis, be it an undamped and damped system.
- Output Controls
For Acoustic region:
By default, the application calculates Acoustic Pressure. You can additionally request Acoustic Velocity and Acoustic Energy.
For Structural region:
Additional output controls are available when solving an FSI problem to control the results calculated on structural domain. By default, only mode shapes are calculated. You can request Stress and Strain results to be calculated but note that “stress” results only show the relative distribution of stress in the structure and are not real stress values. You can also specify to Calculate Reactions.
- Damping Controls (Structural Environment Only)
Damping Controls are supported when the Structural property of the Environment is set to . The options of the Stiffness Coefficient Defined By property, Direct Input or Damping vs. Frequency, enable you to define the method used to define the Stiffness Coefficient. If you select Damping vs. Frequency, the Frequency and Damping Ratio properties appear and require you to enter values to calculate the Stiffness Coefficient. Otherwise, you specify the Stiffness Coefficient manually. The Mass Coefficient property requires a manual entry
- Analysis Data Management
These properties enable you to define whether or not to save the Mechanical APDL application database as well as automatically delete unneeded files.
Define Physics Region(s)
Basic general information about this topic
... for this analysis type:
To create a Physics Region:
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 > .
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 . Acoustics Regions do not support a Stiffness Behavior setting of .
If the Structural Region has the Stiffness Behavior property set to 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 Loads
Temperature Impedance Sheet Static Pressure
Acoustic Boundary Conditions
Pressure Impedance Boundary Absorption Surface Radiation Boundary Absorbing Element Free Surface
The following loading conditions are supported if the analysis has structural physics:
Loads
Thermal Condition Fluid Solid Interface: Use the 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:
Selecting the Solution Information object enables you to view continuously updates any listing output from the solver and provides valuable information on the behavior of the fluid (and structure, if FSI) during the analysis.
Review Results
Basic general information about this topic
... for this analysis type:
You can scope Modal Acoustic analysis results to entities on acoustic bodies and, by default, all acoustic bodies compute results for display.
If you set the Amplitude property to for contour plots, you can see the amplitude contours at a specified frequency. This field is available only when complex results are available for a Modal Acoustics analysis while using the damped or unsymmetric Solver Type. The Amplitude calculation procedure for derived results when complex result sets are available for Modal analysis is similar to that of the Harmonic Analysis. For additional information about Amplitude calculation, see the Amplitude Calculation in Harmonic Analysis section of the Help.
Note: In a Modal Acoustic Analysis (and other eigenvalue-based analyses such as buckling), the solution consists of a deformed shape scaled by an arbitrary factor. The actual magnitudes of the pressures, deformations (if FSI) and any derived quantities, such as energy, strains and stresses, are therefore meaningless. Only the relative values of such quantities throughout the model should be considered meaningful. The arbitrary scaling factor is numerically sensitive to slight perturbations in the analysis; choosing a different unit system, for example, can cause a significantly different scaling factor to be calculated.