Mechanical enables you to specify an upstream Coupled Field Static analysis whose effects are used to perform a downstream Coupled Field Harmonic 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 Harmonic 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 Harmonic template directly onto the Solution cell of the structural template.
Tip: You can create a pre-stress environment in a Coupled Field Harmonic 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 Harmonic analysis supports the following Analysis Settings:
Define Initial Conditions
The Pre-Stress object of the Coupled Field Harmonic analysis must point to the linked Coupled Field Static analysis.
Note:
All structural loads, including Inertial loads, such as Acceleration and Rotational Velocity, are deleted from the Harmonic analysis portion of the simulation once the loads are applied as initial conditions. 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,HARM,,,DZEROKEEP for more details.
For Pressure boundary conditions in the Static Structural 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 results in the follow-on Full-Harmonic Analysis. See the Pressure Load Stiffness topic in the Applying Pre-Stress Effects for Implicit Analysis Help Section for more information about using a pre-stressed environment.
If displacement loading is defined with Displacement, Remote Displacement, Nodal Displacement, or Bolt Pretension (specified as , , or ) loads in the Static Structural analysis, these loads become fixed boundary conditions for the Harmonic solution. This prevents the displacement loads from becoming a sinusoidal load during the Harmonic solution. If you define a Nodal Displacement in the Harmonic analysis at the same location and in the same direction as in the Structural Static analysis, it overwrites the previous loading condition and/or boundary condition in the Harmonic solution.
If a voltage is defined in the Coupled Field Static analysis, all non-zero voltages are set to zero for the Harmonic solution. If you define voltage at the same location in the Harmonic solution, the previous loading is overwritten.
Apply Boundary Conditions
The Environment Context tab provides the following for the prestressed Coupled Field Harmonic analysis:
|
| |||
| ||||
[a] If you apply a Voltage load, without the use of Voltage Coupling scoping option, to any of the geometries included in the Voltage Coupling condition defined in the upstream system, the entities will no longer be coupled and will be overwritten.
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 results to mesh or geometric entities on bodies.