### 12.4.6. Solid Models Tab

The Solid Models tab sets the models that apply to solid domains and to the solid material in a porous domain. The models chosen can vary between each domain, but if radiation is modeled, then all fluid domains must also model radiation. For details, see Using Multiple Domains.

#### 12.4.6.1. Heat Transfer

The `Thermal Energy` model and `Isothermal` model are available for the solid domain. If you do not want to model heat transfer for the domain, then set Heat Transfer > Option to `None`.

For details, see Conjugate Heat Transfer in the CFX-Solver Modeling Guide.

#### 12.4.6.2. Thermal Radiation Model

You can use only the `Monte Carlo` option to model radiation in a solid domain. The options available are the same as for the `Monte Carlo` model in a fluid domain. For details, see Thermal Radiation Model.

You cannot model radiation in a porous domain.

#### 12.4.6.3. Electromagnetic Model

The Electromagnetic Model enables you to define:

Electric Field Model

  Option can be set to `None`, `Electric Potential`, or `User Defined`.

  For a `User Defined` setting, you have to specify the electric field strength for the X, Y, and Z directions.

Magnetic Field Model

  Option can be set to `None`, `Magnetic Vector Potential`, or `User Defined`.

  For the `Magnetic Vector Potential` option, you can specify External Magnetic Field settings using Cartesian or cylindrical components. Using the `User Defined` option will enable you to specify the induced magnetic field model in the X, Y, and Z directions.

If a user-defined model is selected, you must make sure that the electromagnetic properties have been set in the Material details view. For details, see Material Properties Tab. Electromagnetic models are supported for multiphase simulations only if homogeneous.

For more information on electromagnetic theory, see Electromagnetic Hydrodynamic Theory in the CFX-Solver Theory Guide.

#### 12.4.6.4. Additional Variables Models

See Additional Variables.

#### 12.4.6.5. Solid Motion

You can model the motion of a solid that moves relative to its reference frame by selecting the Solid Motion option and specifying a velocity.

You can specify the velocity using one of the following methods:

- Cartesian velocity components

  You must specify values for U, V, and W.

- Cylindrical velocity components

  You must specify values for Axial Component, Radial Component, and Theta Component. You must also specify an Axis Definition.

- Rotating

  Specify an Angular Velocity and an Axis Definition.

The velocity that you specify is interpreted as being relative to the domain motion which is, in turn, relative to the coordinate frame; both of these are specified on the Basic Settings tab for the domain.

The motion of the solid is simulated by adding an advection term to relevant transport equations in the solid (for example, Energy and User Variables). For more details, see Conjugate Heat Transfer in the CFX-Solver Theory Guide.

On interfaces to other domains (fluid-solid or solid-solid interfaces) the solid must move only tangentially to its surface. On an external boundary, if the solid has a velocity component normal to the surface, then consider activating the advection term(s) on the boundary condition for that surface, by visiting the Boundary Details tab and selecting Solid Motion > Boundary Advection. For details on setting up boundary advection on a wall, see Solid Motion: Wall.

Note:

- Most solid motion cases will involve setting either non-stationary domain motion (on the Basic Settings tab) or activating the Solid Motion setting (on the Solid Models tab) but not both.

- If you have a solid with Solid Motion activated that meets a fluid domain at a fluid-solid interface, then you must explicitly set the wall boundary condition applied to the fluid side of the interface to have a wall velocity corresponding to the solid motion, as required.

Release 18.2 - © ANSYS, Inc. All rights reserved.