49.5. System Coupling Related Settings in Fluent

  • Double-Precision Solver

    System Coupling cases may benefit from the use of Fluent's double-precision solver. For coupling cases with moving and deforming meshes (MDM), it is a best practice to use Fluent's double-precision solver. For more information about Fluent's single- and double-precision solvers, see Single-Precision and Double-Precision Solvers in the Fluent User's Guide.

    • In the Fluent Launcher, select Double Precision to use Fluent's double-precision solver.

  • Dynamic Mesh

    • The System Coupling option must be selected on the desired moving and deforming wall boundaries in order to obtain displacements from other co-simulation participants taking part in the coupled analysis.

    • Make sure the appropriate solution stabilization options are selected in the Solver Options tab for the System Coupling boundary zone (and possibly other boundary zones nearby). Solution stabilization should be activated if you find that the Fluent solution is particularly sensitive to the data obtained through system couplings. For example, it is often beneficial for FSI problems in which the fluid is incompressible.

  • Heat Transfer

    • The via System Coupling option must be selected on the desired wall boundaries in order to obtain heat transfer data (temperature, heat flow, or heat transfer coefficient) from other participants taking part in the coupled analysis.

    • The Fluent coupling code has been extended to compute HTC based on Wall Functions and Y plus. By default, Fluent coupling code uses a wall adjacent based HTC method.

      All these HTC calculation methods and sub-stepping options can be accessed by TUI commands at this location:

      /define/models/system-coupling-settings/htc-calculation-settings> 

htc-calculation-method/    unsteady-statistics/

    • Two-way thermal coupling cases may experience slow convergence when the near wall temperature value used in the heat transfer coefficient calculation is close to the wall temperature and is not a good representation of the free stream temperature. This typically occurs when the first node of the mesh is well within the boundary layer.

      Convergence can be improved for such cases by allowing Ansys Fluent to send System Coupling a heat transfer coefficient value based on a constant, user-specified reference temperature. Note that this option results in the heat transfer coefficient having the same definition as the field variable Surface Heat Transfer Coef..

      Note:  Basing the heat transfer coefficient value on a constant reference temperature may not be suitable when there is a strong variation in the free stream temperature along the coupled wall.

      Specify that the heat transfer coefficient is based on a reference temperature by using the following text command:

      /define/models/system-coupling-settings/htc-calculation-settings/htc-calculation-methods/use-tref-in-htc-calculation?

      Define the reference temperature in the Temperature field of the Reference Values task page. It is recommended that you use a value that is close to the fluid free stream temperature.

       Setting Up Physics → Solver → Reference Values...

  • Custom Data Transfer Variables via User-Defined Memory (UDM)

    You can create user-defined data transfer variables using Zone-Based Memory Allocation. For details, see User-Defined Memory Storage in the Fluent Customization Manual.

    Once created you can enable the UDM for use as a System Coupling variable using the following text command:

    define/models/system-coupling-settings/user-defined-coupling-variables-via-udm

  • Run Calculation

    • When running as part of a transient coupled analysis, the step size for and duration of the analysis are controlled by System Coupling.

      • The Time Step Size specified in the Fluent setup is currently ignored; the Fluent solution will be advanced using the time step size specified as part of the System Coupling setup.

      • The Number of Time Steps is also ignored.

    • The specified Max Iterations/Time Step corresponds to the maximum number of nonlinear solver iterations performed per coupling iteration.

For steady-state, system-coupled Fluent analyses, the number of iterations specified in Fluent is equal to the maximum number of solver iterations solved per coupling iteration in a coupling step. Prior to ANSYS FLUENT 14.5, the number of iterations specified in Fluent was equal to the solver iterations solved in a coupling step and was divided equally between the coupling iterations in a coupling step. You can recover the previous behavior by using the following command: (rpsetvar ’sc/steady/default-iteration-method? #f).

For cases that use a pseudo time method, refer to Performing Calculations with a Pseudo Time Method in the Fluent User's Guide.

For steady-state dynamic mesh applications, refer to Steady-State Dynamic Mesh Applications in the Fluent User's Guide.