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:
Mesh Adaptation
During a purely harmonic acoustic analysis (all bodies in the Physics Region object set to ), use the Morphing Region object to perform mesh adaptation during the solution process.
This feature models an enclosure that includes an interior space. The surface (face) around this space defines a boundary. You also specify an external boundary surrounding the enclosure. The area between the two boundaries acts as an infinite acoustic space in the form of a mesh that will be adapted, per frequencies, during the solution process.
During the solution, the solver identifies if the mesh must be updated based on how you specify the object’s properties. Base mesh and morphing parameters include Base Frequency, Morphing Region Thickness, Minimum/Maximum Frequency, Morphing Intervals.
Mesh adaptations are based on an applied offset in the normal direction of the faces selected as the Moving Boundaries and as needed, the mesh is morphed/adapted. The offset is calculated as follows:
Offset = Morphing Region Thickness * ((Base Frequency/current frequency) – 1)
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 or Harmonic Acoustics system, the application automatically inserts a Physics Region object and scopes it to all bodies. You need to specify the physics selection.
Use the Morphing Region object to specify a domain in which the mesh is changed, or “morphed,” based on node locations and coordinates, during the solution process to adapt the mesh to the current frequency
Automatic Boundary Condition Detection
The Harmonic Acoustics Environment object provides the following context menu (right-click) options:
> : This selection creates a Fluid Solid Interface object with all possible Fluid Solid Interface face selections based on the physics region definitions.
> Far-field Radiation Surface: This selection automatically creates an Far-field Radiation Surface object that includes all possible Far-field Radiation Surfaces available in the analysis. Mechanical identifies the following faces as Far-field Radiation Surfaces:
Interface between the normal acoustic element and PML acoustic element (Interface between Normal Acoustic and PML Acoustic Region)
Face selections of Radiation Boundary (faces of elements flagged with SF,,INF)
Face selections of Impedance Boundary (faces of element flagged with SF,,IMPD)
Face selection of Absorption Element (faces of elements of type FLUID130)
Face selection of Absorption Surface (faces of element flagged with SF,,ATTN)
> : This selection performs both of the above object generation options.
Preparing the Analysis
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 Material Data
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 properties Density and Speed of Sound in Engineering Data workspace (Toolbox > Physical Properties).
Define Part Behavior
You cannot apply an acoustics-based Physics Region object to a body or part that has the Stiffness Behavior property set to .
Caution: If you scope a structural-based Physics Region to a body or part that has the Stiffness Behavior property set to , this body/part is in contact with an acoustic-based Physics Region, 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
For a Harmonic Acoustics analysis, the basic analysis settings include:
- Step Controls
Th e Step Controls category enables you to define step controls for an analysis that includes rotational velocities in the form of revolutions per minute (RPMs). You use the properties of this category to define RPM steps and their options. Each RPM load is considered as a load step, such as frequency spacing, minimum frequencies, maximum frequencies, etc. When you select the Analysis Settings object, the Step Controls category automatically displays in the Worksheet. You can modify certain properties in either the Worksheet or in the Details pane for the object.
- 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 () Solution Method is available to perform a Harmonic Acoustics analysis.
- Scattering Controls
The Scattering Controls category includes the property. The options for this property include:
(default): The application selects the desired setting.
: Scattering controls are off.
: Selecting this option turns scattering controls on and displays the Scattering Output Type property. You use the Scattering Output Type property to specify the output type for an acoustic scattering analysis. The options for this property include and . Select the option when you wish to output the total pressure field and the 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 , then the application uses the 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 Far-field Radiation Surfaces. Therefore, this field controls far-field result definitions and results. The options include:
(default): If your analysis does not include a user-defined Far-field Radiation Surface boundary condition object, this setting identifies the Far-field Radiation 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.
: This option requires the definition of at least one user-defined Far-field Radiation Surface object.
: This setting invalidates all Far-field Radiation Surface objects and Far-field Result objects.
- Output Controls
Summary
The properties of the Output Controls category 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 deformations are calculated. You can also request Stress and Strain results, using the corresponding properties. 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
The General Miscellaneous Property 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 Damping Controls category is visible when Structural Physics is turned . These properties enable you to specify damping for the structure in the Harmonic Acoustics analysis. Properties include: Structural Damping Coefficient, Stiffness Coefficient (beta damping), and Mass Coefficient (alpha damping). They can also be applied as Material Damping using the Engineering Data workspace.
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
The properties of the Analysis Data Management category 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 the solution or to create and save the Mechanical APDL application database (db file).
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 Insert > 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 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 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.
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.