Mechanical enables you to specify an upstream Coupled Field Static analysis whose effects are to be used to perform a downstream Coupled Field Modal analysis. The supported physics combinations include:
Coupling of Structural and Acoustics physics
Piezoelectric Coupling
Piezoelectric coupling with Acoustics physics
Coupling of Electrostatic and Structural physics
Electrostatic Structural coupling with Acoustics physics
Electrostatic Structural coupling with Piezoelectric coupling
See the Application Examples and Background section for an overview of types of problems that use coupled structural-electric solutions as well as some examples. Also see the Acoustics Analysis Overview section for more detailed information about performing an acoustics analysis.
Points to Remember
To perform a prestressed Coupled Field Modal analysis you need to first perform a Coupled Field Static analysis, and properly link it to the downstream coupled field analysis.
When beginning the analysis, you need to properly define the Physics Region object(s). The Physics Region object(s):
Is automatically included.
Requires each body of the model to be specified by a physics.
Defines the physics of the entire system/analysis.
Specifies physics type per body as needed.
Needs to be scoped to at least one body with more than one physics type or to an acoustic body.
Any change to the physics settings in the upstream analysis will be automatically reflected in the downstream analysis
The Thermal physics type is not supported. If this physics type is active in the upstream analysis, the downstream analysis will be invalid.
This section assumes that you have an understanding of the general workflow for performing a simulation. As needed throughout the analysis, refer to the Steps for Using the Application section for an overview of the workflow.
Create Analysis System
Because this analysis is linked to (and based on) structural responses, a Coupled Field Static analysis is a prerequisite. This setup enables the two analysis systems to share resources, such as Engineering Data, Geometry, and the boundary condition type definitions that are defined the in the structural analysis.
From the Toolbox, drag a Coupled Field Static template to the Project Schematic. Then, drag a Coupled Field Modal template directly onto the Solution cell of the structural template.
Tip: You can create a pre-stress environment in a Coupled Field Modal system that is already open in Mechanical by:
Selecting the option from the Analysis drop-down menu on the Home (or displayed) tab.
Setting the Pre-Stress Environment property (of the Pre-Stress object) to the Coupled Field Static system.
Specify Analysis Settings
The downstream Coupled Field Modal analysis supports the following Analysis Settings:
Define Initial Conditions
The Pre-Stress object of the Coupled Field Modal analysis must point to the upstream Coupled Field Static analysis.
Note:
When you perform a pre-stressed 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 pre-stressed modal analysis. When you link your Modal analysis to a Structural analysis, all structural loading conditions, including Inertial loads, such as Acceleration and Rotational Velocity, are deleted from the Modal portion of the simulation. This is a result of the Load Control property of the Pre-Stress object being set (by default) to the . You can modify this to property to control load generation. See the description of the Load Control property in the Pre-Stress object reference for more information. Also see the Mechanical APDL command PERTURB,MODAL,,,DZEROKEEP for more details.
For a Pressure load in the Coupled Field Static 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 to act 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 the 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 pre-stressed environment.
If displacement loading is defined with either the Displacement, Remote Displacement, Nodal Displacement, or Bolt Pretension (specified as a Lock, Adjustment, or Increment) in the Static Structural analysis, these loads become fixed boundary conditions for the Modal solution. If the Modal solution is followed by a Harmonic solution, these displacement loads become fixed boundary conditions for the Harmonic solution as well. This prevents the displacement loads from becoming a sinusoidal load during the Harmonic solution.
Apply Boundary Conditions
The Environment Context tab provides the following for the prestressed Coupled Field Modal analysis:
|
Acoustic Loads |
Acoustic Boundary Conditions |
Any structural and/or electric support used in the Coupled Field Static analysis persists. Therefore, you are not allowed to add new support in the pre-stressed Coupled Field Modal analysis.
Results
See the Using Results section for descriptions of all supported result types.
All results generally default to the corresponding physics setting, that is, , , or . You can individually scope most of the results to mesh or geometric entities on bodies.