33.4. Guidelines For Using the Ansys Fluent MHD Model

This section provides a basic outline for installing the magnetohydrodynamics (MHD) module and solving MHD problems in Ansys Fluent.

Important:  While Using the Ansys Fluent MHD Module covers much of the same material in greater detail, this section presents a set of guidelines for solving typical MHD problems with Ansys Fluent, with occasional references to Using the Ansys Fluent MHD Module where more information can be found.

 

33.4.1. Installing the MHD Module

Before using the MHD module, you first need to install the necessary files onto your computer. These files are provided with your standard installation of Ansys Fluent. They can be found in your installation area in a directory called addons/mhd. The MHD module is loaded into Ansys Fluent through the text user interface (TUI)

define → models → addon-module

only after a valid Ansys Fluent case file has been set or read.

Once the MHD model is installed, beneath the mhd directory there are two subdirectories: a lib directory, and a directory corresponding to your specific architecture, ntx86 for example. The lib directory holds a Scheme code called addon.bin that contains the MHD module graphical interface. The specific architecture directory, ntx86 for example, contains the following subdirectories that hold various Ansys Fluent files:

 2d   2ddp   3d   3ddp
 2d_host  2ddp_host  3d_host  3ddp_host
 2d_node  2ddp_node  3d_node  3ddp_node
 

33.4.2. An Overview of Using the MHD Module

To use the MHD module in an Ansys Fluent simulation, follow the general guidelines:

  1. Start Ansys Fluent.

    To begin modeling your MHD simulation, you need to start an appropriate Ansys Fluent session. Choose from either the 2D, 3D, Double Precision, or the parallel version of Ansys Fluent.

  2. Read in a mesh file or a case file.

    You can have Ansys Fluent read in your mesh file, a previously saved non-MHD case file, or a previously saved MHD case file.

    Important:  Note that if you read in a new mesh file, you need to perform the appropriate mesh check and mesh scale procedures.

  3. Load the MHD module.

    The MHD module is loaded into Ansys Fluent using the text command

    define → models → addon-module

    and entering the corresponding module number (Loading the MHD Module).

  4. Set up the MHD model.

    The MHD Model dialog box is accessed using the graphical user interface (GUI):

     Setup → Models → MHD Model   Edit...

    If the MHD model is not enabled after the MHD module is loaded for the first time, you can enable it by clicking the Enable MHD button, which will display the expanded dialog box (Enabling the MHD Model).

  5. Select an MHD method.

    The method used for the MHD calculation can be selected under MHD Method. The two methods are

  6. Apply an external magnetic field.

    This is done by entering values for the B0 components in the External Field B0 tab. B0 input options can either be

    • Patched, or

    • Imported

    The Field Type will either be the DC Field or the AC Field. The Field Type is determined by the field data from the data file. Refer to Applying an External Magnetic Field for details on applying an external magnetic field.

  7. Set up the boundary conditions.

    Under the Boundary Condition tab, cell zones and wall boundaries can be selected as well as the corresponding zone type.

    Cell zone materials are selected from the Material Name drop-down list. The properties of the selected material can be modified by clicking on the Edit... button to the right of the material name. Note that the materials available in the list are set in the general Ansys Fluent case setup.

     Setup →   Materials

    The material properties that may be modified include the electrical conductivity and magnetic permeability.

    Wall boundary conditions can be set as an Insulating Wall, Conducting Wall, Coupled Wall or Thin Wall (see Setting Up Boundary Conditions).

  8. Set solution controls.

    Under the Solution Control tab:

    • The MHD equation is enabled or disabled.

    • Lorentz force and Joule heat sources are enabled or disabled.

    • under-relaxation factors are set (reasonable under-relaxation factors for the MHD equations are 0.8 0.9).

    • Scale factors can be used to adjust the strength of the imposed external magnetic field. As the calculation approaches convergence, the scale factor in the Solution Control tab can be increased gradually until the required external field strength is reached (Solution Controls).

    • The MHD model is initialized (MHD Model Initialization).

  9. Run the Ansys Fluent MHD simulation.

     Solution →   Run Calculation

    Set the number of iterations. It is often an effective strategy to begin your MHD calculations using a previously-converged flow field solution. With this approach, the induction equations themselves are generally easy to converge. For more information, see Iteration.

  10. Process the solution data.

    You can use the standard postprocessing facilities of Ansys Fluent to display the results of an MHD calculation. Contours of MHD variables can be displayed.

     Results → Graphics → Contours   Edit...

    The MHD variables can be selected from the variable list. Vectors of MHD variables, such as the magnetic field vector and current density vector, can be displayed using custom vectors.

     Results → Graphics → Vectors  Edit...

    For more information, see Postprocessing.