This analysis enables you to simulate the following physics types, independently or in combination, in a transient environment:
Coupling of Structural and Thermal physics
Coupling of Structural and Acoustics physics
Coupling of Thermal and Electric Conduction physics
Coupling of Structural and Thermoelectric Conduction
Stand-alone Acoustics physics
Piezoelectric (charge-based) Coupling
Piezoelectric coupling (charge-based) with Acoustics physics
Coupling of Electrostatic and Structural physics
Electrostatic Structural coupling with Acoustics physics
Electrostatic Structural coupling with Piezoelectric coupling
Note: Piezoelectric 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
The application automatically inserts an Initial Physics Options object for this analysis type.
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.
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.
As needed throughout the analysis, refer to the Steps for Using the Application section for an overview the of 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 Transient analysis. For the thermal field, you specify an Initial Temperature as either Uniform or Non-Uniform (Transient only). For the Structural Setting, you specify a Reference Temperature. Typically for most other analysis types in Mechanical, you define a Reference Temperature from the Environment object.
Important: Currently, the Coupled Field Transient analysis only supports the option for the Initial Temperature property. However, the Non-Uniform Temperature setting is available when Beta Options are active.
Specify Analysis Settings
The analysis type supports the following Analysis Settings:
Step Controls (see below)
Recommendation: To improve convergence for thermal-electric coupling, set the Nonlinear Controls property, Line Search, to the setting.
For a Coupled Field Transient analysis when the Time Integration property is set to (default), based on the active physics of the environment, the following additional properties display and enable you to specify whether to turn a physics field on or off:
Structural Only: Options include and (default).
Thermal Only: Options include and (default) .
Electric Only: Options include and (default). Supported only for Electric (Conduction) physics only.
Note: For the Acoustics and Electric (Charge) physics properties, Time Integration property is automatically set to .
Note: For thermal-electric coupling and stand-alone acoustics physics, the application uses the Newmark Time integration method. For all other coupling and physics combinations, application uses the HHT time integration method. See the Transient analysis section of the Mechanical APDL Theory Reference for more information.
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 Transient 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 following properties:
Thermal Strain. You use this property to specify the thermoelasticity coupled effects included through the thermal strain. Options include (default), , and .
Thermoelastic Damping: Either or (default).
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.
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:
In addition, and depending upon physics definitions, the following Conditions are available:
Voltage Coupling (Electric)
Plastic Heating (Structural-Thermal)
Viscoelastic Heating (Structural-Thermal)
As needed, 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.