Introduction
You use the Static Acoustics analysis as a method for applying stresses to a downstream analysis. This is a Fluid-Structure Interaction (FSI) analysis incorporating two different physics phenomena that can then interact with one another. The static analysis can be linear or nonlinear. It creates a pre-stress environment for the downstream dynamic acoustics analysis.
The Acoustics Regions of the Static Acoustics analysis do not effect the results of the downstream Modal or Harmonic Acoustics analysis, except that the mesh can be morphed during the solution.
Points to Remember
Note that:
This analysis supports 3D geometries only.
If possible, model your fluid region as a single solid multibody part.
The Physics Region object(s) need to identify all of the active bodies that may belong to the acoustic and structural physics types. For your convenience, when you open a Static Acoustics system, the application automatically inserts a Acoustics Region object and a Structural Region object.
Only Structural Results are supported for this analysis type.
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 Static 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 Static Acoustics system in the Project Schematic, see the Static 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).
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
For simple linear static analyses, you typically do not need to change the default Analysis Settings. For more complex analyses the basic Analysis Settings include:
- Large Deflection
Large Deflection is typically needed for slender structures. Use large deflection if the transverse displacements in a slender structure are more than 10% of the thickness.
Small deflection and small strain analyses assume that displacements are small enough that the resulting stiffness changes are insignificant. Setting the Large Deflection property to will take into account stiffness changes resulting from changes in element shape and orientation due to large deflection, large rotation, and large strain. Therefore, the results will be more accurate. However, this effect requires an iterative solution. In addition, it may also need the load to be applied in small increments. As a result, the solution may take longer to solve.
You also need to turn on large deflection if you suspect instability (buckling) in the system. Use of hyperelastic materials also requires large deflection to be turned on.
- Step Controls for Static and Transient Analyses
Step Controls are used to i) control the time step size and other solution controls and ii) create multiple steps when needed. Typically analyses that include nonlinearities such as large deflection or plasticity require control over time step sizes as outlined in the Automatic Time Stepping section. Multiple steps are required for activation/deactivation of displacement loads or pretension bolt loads. This group can be modified on a per step basis.
Note: Time Stepping is available for any solver.
- Output Controls
Output Controls enable you to specify the time points at which structural results should be available for postprocessing. In a nonlinear analysis it may be necessary to perform many solutions at intermediate load values. However i) you may not be interested in all the intermediate results and ii) writing all the results can make the results file size unwieldy. This group can be modified on a per step basis except for Stress and Strain.
- Nonlinear Controls
Nonlinear Controls enable you to modify convergence criteria and other specialized solution controls. Typically you will not need to change the default values for this control. This group can be modified on a per step basis. If you are performing a nonlinear Static Acoustics analysis, the Newton-Raphson Type property becomes available. This property only affects nonlinear analyses. Your selections execute the Mechanical APDL NROPT command. The default option, , allows the application to select the appropriate NROPT option or you can make a manual selection and choose , , or .
See the NROPT command in the Mechanical APDL Command Reference for additional information about the operation of the Newton-Raphson Type property.
- Damping Controls
When you pre-stress a Modal Acoustics analysis with a Static Acoustics analysis, the Damping Controls category of the Analysis Settings displays. It includes the property Ignore Acoustic Damping. 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 in your downstream Modal system. Ignoring these material-based damping effects enables the application to use undamped eigensolvers without the need to suppress these material properties in Engineering Data.
- Analysis Data Management
Settings enable you to save specific solution files from the Static Acoustics analysis for use in other analyses. You can set the Future Analysis property to if you intend to use the static acoustics results in a subsequent Modal or Harmonic analysis. If you link a structural system to another analysis type in advance, the Future Analysis property defaults to .
Note: Scratch Solver Files, Save Ansys db, Solver Units, and Solver Unit System are applicable to static systems only.
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.