Introduction
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. You can also perform a FSI modal analysis on a prestressed structure using a Static Acoustics Analysis.
Points to Remember
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 Region object(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.
To perform a prestressed Modal Acoustics analysis you need to first perform a Static Acoustics analysis and properly link it to the Modal Acoustics analysis. When performing this type of linked analysis, the Modal 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 Modal Acoustics analysis when you first create the linked systems.
Automatic Boundary Condition Detection
In order to assist your analysis, the Environment object contains context menu (right-click) options that enable you to automatically generate interfaces based on physics region definitions. The Modal Acoustics analysis includes the option > . This selection automatically creates a Fluid Solid Interface object with all possible Fluid Solid Interface face selections.
Create Analysis System
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 Materials
All of your acoustic bodies must be assigned a material that contains the properties Density and Speed of Sound.
Important: The Fluid Materials library in the Engineering Data workspace includes the fluid materials Air and Water Liquid. Each of these materials includes the property Speed of Sound. Any other material to be used in the Acoustics Region requires you to specify the property Speed of Sound and Density in Engineering Data workspace (Toolbox > Physical Properties).
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.
Define Part Behavior
A Structural Physics Region may contain bodies with the Stiffness Behavior set to . cannot contain rigid bodies.
If the has the property set to and if it is in contact with acoustic regions, then fluid-structure interaction may not behave as expected.
Define Connections
To define contact between two acoustic bodies or an acoustic and a structural body (FSI contact) which have non-conforming meshes, you must set the:
Type property to .
Formulation property must be set to .
For FSI contacts:
The Contact side must be on the acoustic body and the Target must be on the structural body.
The Bonded contact type setting and the Pure Penalty formulation is supported in addition to MPC formulation.
Pure Penalty formulation is not supported for contact conditions between two acoustic bodies.
The Nodal-Dual Shape Function Projection (keyo,cid,4,4) option, of the Detection Method property, is used by default for FSI contact defined using the Pure Penalty formulation.
The Combined option (keyo,cid,4,5), of the Detection Method property, is not supported for the MPC formulation type
Note: Contact settings other than Bonded using MPC or Pure Penalty formulation (keyo,cid,2,1) are ignored and are overwritten with the following preferred key options of Bonded and 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
The application overwrites user-defined contact settings between fluid-fluid and fluid-solid bodies using the above criterion. Refer to Matrix-Coupled FSI Solutions section from the Mechanical APDL Acoustic Analysis Guide for more information.
Limitation: Joints, Springs, Bearings, and/or Beams are not supported on acoustic bodies.
Establish Analysis Settings
Basic Analysis Settings for this analysis include the following:
- 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
0.01Hz.- Solver Controls
This \ category 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
The properties of the Output Controls enable you to different quantities to be written to the result file for use during post-processing. During acoustics analyses, these quantities are based on the specified Acoustics or Structural Physics Regions.
- For specified Acoustics Regions:
By default, the application calculates and stores Acoustic Pressure in the result file. No specific property is associated with this quantity.
In addition, setting the Calculate Velocity and Calculate Energy properties to enables you to request acoustic velocity and acoustic energy.
- For specified Structural Regions:
When your analysis is solving an FSI problem in order to control the results calculated on structural domain, by default, only mode shapes are calculated. You can also request Stress and Strain results, using the corresponding properties. These properties only show the relative distribution of stress in the structure and are not real stress values. Furthermore, you can generate node-based force reactions using the Calculate Reactions property. This property requires you to set the Nodal Forces property to .
General Miscellaneous Property: This property includes options specific to Acoustics analyses based on the acoustics analysis type, either Harmonic or Modal, and enable you to produce element-based miscellaneous solution data.
- Damping Controls
The properties of the Damping Controls category depend upon the setting of the Damped property of the Solver Controls category.
- Undamped System
When the Damped property is set to the Ignore Acoustic Damping property displays. This property provides the options (default) and . Setting this property to instructs the application to ignore material properties that create damping effects, specifically Specific Heat, Thermal Conductivity, and Viscosity. Ignoring these material-based damping effects enables the application to use undamped eigensolvers without the need to suppress these material properties in Engineering Data.
- Damped System
When the Damped property is set to (Full Damped) and the Structural property of the Environment (Modal Acoustics) object is set to , the Stiffness Coefficient Defined By property displays. The options for this property include (default) or . The options of this property enable you to define the method used to define the . If you select , the Frequency and Damping Ratio properties display and require you to enter values to calculate the Stiffness Coefficient. Otherwise, you specify the Stiffness Coefficient manually. The Mass Coefficient property also 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 Pre-Stress Conditions
You can point to a Static Acoustics analysis in the Pre-Stress environment field if you want to include pre-stress effects. A typical example is the large tensile stress induced in a turbine blade under centrifugal load that can be captured by a static structural analysis. This causes significant stiffening of the blade. Including this pre-stress effect will result in much higher, realistic natural frequencies in a modal analysis.
If the Modal analysis is linked to a Static Acoustics analysis for initial conditions and the parent static analysis has multiple result sets (multiple restart points at load steps/sub steps), you can start the Modal analysis from any restart point available in the Static Acoustics analysis. By default, the values from the last solve point are used as the basis for the modal analysis. See the Restarts from Multiple Result Sets topic in the Applying Pre-Stress Effects for Implicit Analysis section for more information.
Note:
When you perform a prestressed Modal analysis, the support conditions from the static analysis are used in the Modal analysis. You cannot apply any new supports in the Modal analysis portion of a prestressed modal analysis. When you link your Modal analysis to a Structural Acoustics analysis, all structural loading conditions, including Inertial loads, such as Acceleration and Rotational Velocity, are deleted from the Modal 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 Static Acoustics analysis: if you define the load with the option for faces (3D) or edges (2-D), you could experience an additional stiffness contribution called the "pressure load stiffness" effect. The 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 modal results in the follow-on Modal Analysis. See the Pressure Load Stiffness topic in the Applying Pre-Stress Effects for Implicit Analysis 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 Lock, Adjustment, or Increment) loads in the Static Acoustics analysis, these loads become fixed boundary conditions for the Modal Acoustics solution.
Define Physics Region(s)
To specify a Physics Region object:
Highlight the Environment object and select the Physics Region button on the Environment Context Tab or right-click the Environment object or within the Geometry window and select > Physics Region.
Define all of the properties for the new object. For additional information, see the Physics Region object reference section.
A structural-based Physics Region may contain bodies with the Stiffness Behavior property 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.
Note: You may want to use the following context menu (right-click) options when specifying a Physics Region object:
> .
> .
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.
Review Results
This analysis type does not provide Acoustic Results. All structural result types are available. You can use a Solution Information object to track, monitor, or diagnose problems that arise during a solution.
Once a solution is available you can contour the results or animate the results to review the response of the structure.
As a result of a nonlinear static analysis you may have a solution at several time points. You can use probes to display the variation of a result item as the load increases. An example might be large deformation analyses that result in buckling of the structure. In these cases it is also of interest to plot one result quantity (for example, displacement at a vertex) against another results item (for example, applied load). You can use the Charts feature to develop such charts.