The Coupled Field Static analysis simulates the steady state interaction of different physics types (see below). This section assumes that you have an understanding of the general workflow for performing a simulation. See the Application Examples and Background section for an overview of types of problems that use coupled structural-thermal solutions as well as some examples.
This analysis enables you to simulate the following physics types, independently or in combination, in a static environment:
Coupling of Structural and Thermal physics
Coupling of Structural and Acoustics physics
Piezoelectric (charge-based) coupling
Piezoelectric (charge-based) coupling with Acoustics physics
Coupling of Thermal and Electric conduction physics
Coupling of Structural and Thermoelectric conduction
Stand-alone Electrostatic
Coupling of Electrostatic and Structural physics
Electrostatic Structural coupling with Acoustics physics
Electrostatic Structural coupling with Piezoelectric coupling
Note: Piezoelectric (charge-based) analyses couple structural and electric physics with materials that have natural properties, such as quartz and ceramics.
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
When beginning the analysis, you need to properly define the:
The application automatically inserts an Initial Physics Options object in order to specify an initial and reference temperature for the analysis.
To simulate the thermoviscoelasticity coupling effect, the Viscoelastic Heating condition must be scoped to a body whose material assignment includes the Viscoelastic material properties Prony Shear Relaxation and Prony Volumetric Relaxation, as defined in Engineering Data.
To simulate the thermoplasticity coupling effect, the Plastic Heating condition object can be added and must be scoped to bodies whose material properties has the Plasticity effects
When performing an Electrostatic Structural analysis:
Set the Large Deflection property (Analysis Settings > Solver Controls) to .
Specify your mesh using a single layer of low-order elements (no mid-side nodes) to avoid air mesh distortion. A quadrilateral mesh that collapses uniaxially typically works best.
When you specify a Physics Region using only the Electric property, set to (electrostatic elements), make sure that the material assigned to the scoped bodies includes relative permittivity definition.
When your analysis includes electrostatic elements, the application automatically sets the electric charge reaction sign to negative. See the SOLID122 section (or PLANE121 and SOLID123) of the Mechanical APDL Element Reference for this KEYOPT setting.
When performing a standalone Electrostatic analysis, the application automatically specifies the Contact Region object property, Small Sliding as . This applies to all contact conditions.
As needed throughout the analysis, refer to the Steps for Using the Application section for an overview the general analysis workflow.
Define Initial Physics Options
Specify the temperature settings and values of the Initial Physics Options object. You use the Initial Physics Options object to specify the initial temperature and reference temperature of the parts/bodies specified as either Thermal or Structural (using the Physics Region object) during a Coupled Field Static analysis. For the Structural Settings, you specify a Reference Temperature. Typically for most other analysis types in Mechanical, you define a Reference Temperature from the Environment object.
Define Physics Region(s)
During a Coupled Field analysis, a Physics Region object is automatically included. All of the bodies of the model must have a physics type specified by a Physics Region object. You use this object to specify the geometry bodies that belong to the supported physics types. By default, the and properties are set to . The Coupled Field Static analysis provides the following physics types.
Structural
Acoustics
Thermal: Note that when the and properties are set to (default settings), the Coupling Options category displays. This category includes the Thermal Strain property. You use this property to specify the thermoelasticity coupled effects included through the Thermal Strain. Options include , , and .
Electric: The options for this property include , , and . Review the Physics Region object reference page for property descriptions.
You can add Physics Region objects as desired by:
Highlighting the Environment object and selecting the Physics Region option on the Environment Context Tab or right-click the Environment object or within the Geometry window and select > .
Define all of the properties for the new object.
For additional information, see the Physics Region object reference section.
Specify Analysis Settings
The analysis type supports the following Analysis Settings:
Recommendation: To improve convergence for thermal-electric coupling, set the Nonlinear Controls property, Line Search, to the setting.
Apply Boundary Conditions
The Environment Context tab provides the various groups of loads, supports, and conditions, including various Acoustic loads and boundary conditions and the following Electric loads and boundary conditions are specific to Coupled Field Static analyses:
Voltage (Supports Phase Angle)
In addition, and depending upon physics definitions, the following Conditions are specific to Coupled Field Static analyses:
See the Boundary Conditions section for additional information.
Results
The Solution Context tab provides the various groups of result options. The analysis supports Structural, Thermal, and Electric Probes. For many result objects, the default setting for geometry is either , , or , depending on the given result type.
See the Using Results section for more information.