5.2. Coupled Field Analysis Types

Introduction

The Coupled Field analyses in Mechanical enable you to simulate interaction between multiple physics types. The availability of analysis settings, boundary conditions, results, etc. is based on the specified physics as well as the analysis type you select. For example, if you specify a Coupled Field Static analysis, all common features are available for structural physics, such as Force, Deformation, etc. Supported physics configurations include:

 Coupled Field HarmonicCoupled Field ModalCoupled Field StaticCoupled Field Transient
Structural✓✓✓✓
Acoustics✓✓✓✓
Electric✓[a]✓[a]✓[b]✓[b]
Thermal  ✓✓

[a] Supports charge-based formulation only.

[b] Supports charge-based and current-based formulation.

You can view the physics specified for your Coupled Field analysis from the properties of the Setup cell in Workbench.

And, in Mechanical, you can view the selected physics from the Environment object, and you can view and change the physics definition using the Physics Region object.

Coupling

The following table shows the interaction between the types of physics available in the application and the analysis types. You specify the interaction between the physics types and the analyses using either the 1) Physics Region, such as Thermal Strain, or through 2) coupling conditions, such as Plastic heating, or 3) the application always includes Piezoelectric coupling via Structural-Electric charge interaction.

Physics

Coupled Field Harmonic

Coupled Field Modal

Coupled Field Static

Coupled Field Transient

Structural Thermal

Not Supported

 

Thermal strain

Thermoplasticity

Thermoviscoelasticity

Thermal strain

Thermoelastic Damping

Thermoplasticity

Thermoviscoelasticity

Electrostatic Structural

Electrostatic Force[a]

Electrostatic Force[a]

Electrostatic Force

Electrostatic Force

Structural-Acoustics

Fluid Solid Interface

Fluid Solid Interface

Fluid Solid Interface

Fluid Solid Interface

Structural Electric (Charge)

Piezoelectric

Piezoelectric

Piezoelectric

Piezoelectric

Thermal Electric (Conduction)

  

Joule Heating

Seebeck

Peltier

Joule Heating

Seebeck

Peltier

[a] Requires prestress Coupled Field Static.

Important:  The Element Control property of the Geometry object is, by default, set to Program Controlled. This setting allows the application to choose the best Mechanical APDL element options (KEYOPTS). For example, if your coupled field analysis includes nonlinearities, the application could automatically (and without your knowledge):

  • Change the structural-thermal coupling from Strong to Weak.

  • Specify that all coupling types use a uniform reduced integration scheme instead of Full Integration (as defined by the Brick Integration Scheme property of Part/Body objects).

As a result, to make sure that the application does not automatically change the element options, use the Manual setting for the Element Control property.

See the Automatic Selection of Element Technologies and Formulations section of the Mechanical APDL Element Reference for more information.

Note:

  • The Physics Region supports the activation of more than two physics types and therefore, coupling. In this case, there is a cumulative effect for each individual physics interaction with the other supported physics.

  • If a body has more than two physics associated with its scoping, the interaction of the physics types is a combination of two different physics interactions.

  • You can set the Thermal Strain property, of Physics Region object, to Strong (Matrix) coupling or Weak (Load Vector) coupling. Review the Coupled Effects section of the Coupling documentation in the Mechanical APDL Theory Reference for more background information.

  • You can specify Thermoplasticity and Thermoviscoelasticity using the Plastic Heating and Viscoelastic Heating coupling conditions. Review the Thermoplasticity and Thermoviscoelasticity sections of the Coupling documentation in the Mechanical APDL Theory Reference for more background information.

  • Joule Heating is considered as a load vector. Review the Thermoelectrics section of the Coupling documentation in the Mechanical APDL Theory Reference for more background information.

  • For Piezoelectric coupling, the Piezoelectric matrix must be defined in the Engineering Data Workspace. You may want to review the Piezoelectrics section of the Coupling documentation in the Mechanical APDL Theory Reference for more background information.

  • Currently, linear elements generated by the application use element SOLID226 (a high-order element) with the mid-side nodes dropped, except for structural-thermal coupling and piezoelectric coupling. For structural-thermal coupling and piezoelectric coupling, the application uses element SOLID225.

Recommendation:  If your coupled field analysis includes an edge that you can more accurately measure in micrometers than meters, Ansys recommends that you use a unit system that supports this length, specifically the µMKS unit system.

Coupled Field Simulations

The following sections discuss the steps and requirements to perform, processing limitations of, and industry-based applications for, coupled field simulations.