12.2.1. Solving Heat Transfer Problems

The procedure for setting up a heat transfer problem is described below. Note that this procedure includes only those steps necessary for the heat transfer model itself; you will need to define the other settings (for example, other models, boundary conditions) as usual.

  1. To activate the calculation of heat transfer, enable the energy equation by right-clicking Energy in the tree (under Setup/Models) and clicking On in the menu that opens.

     Setup → Models → Energy  On

    Figure 12.1:  Enabling the Energy Equation

    Enabling the Energy Equation

  2. (Optional, pressure-based solver only.) If you are modeling viscous flow and you want to include the viscous heating terms in the energy equation, enable the Viscous Heating option in the Viscous Model dialog box.

     Setup → Models → Viscous  Edit...

    As noted in Inclusion of the Viscous Dissipation Terms in the Theory Guide, the viscous heating terms in the energy equation are (by default) ignored by ANSYS Fluent when the pressure-based solver is used. They are always included for the density-based solver. Viscous dissipation should be enabled when the shear stress in the fluid is large (for example, in lubrication problems) and/or in high-velocity, compressible flows. See Equation 5–9 in the Theory Guide.

  3. Define thermal boundary conditions at flow inlets, flow outlets, and walls. The boundary condition dialog boxes can be opened by right-clicking the boundary name in the tree (under Setup/Boundary Conditions) and clicking Edit... in the menu that opens; alternatively, you can open them from the Boundary Conditions task page:

     Setup →   Boundary Conditions

    At flow inlets and exits you will set the temperature; at walls you may use any of the following thermal conditions:

    • specified heat flux

    • specified temperature

    • convective heat transfer

    • external radiation

    • combined external radiation and external convective heat transfer

    Thermal Boundary Conditions at Walls provides details on the model inputs that govern these thermal boundary conditions. The default thermal boundary condition at inlets is a specified temperature of 300 K; at walls the default condition is zero heat flux (adiabatic). See Cell Zone and Boundary Conditions for details about boundary condition inputs.


    Important:  If your heat transfer application involves two separated fluid regions, see the information provided below.


  4. Define material properties for heat transfer.

     Setup →   Materials

    Heat capacity and thermal conductivity must be defined, and you can specify many properties as functions of temperature as described in Physical Properties.

12.2.1.1. Limiting the Predicted Temperature Range

For stability reasons, ANSYS Fluent includes a limit on the predicted temperature range. The purpose of the temperature ceiling and floor is to improve the stability of calculations in which the temperature should physically lie within known limits. Sometimes intermediate solutions of the equations give rise to temperatures beyond these limits for which property definitions, and so on, are not well defined.

The temperature limits keep the temperatures within the expected range for your problem. If the ANSYS Fluent calculation predicts a temperature above the maximum limit, the stored temperature values are “pegged” at this maximum value. The default for the temperature ceiling is 5000 K. If the ANSYS Fluent calculation predicts a temperature below the minimum limit, the stored temperature values are “pegged” at this minimum value. The default for the temperature minimum is 1 K.

If you expect the temperature in your domain to exceed 5000 K, use the Solution Limits dialog box to increase the Maximum Static Temperature.

 Solution → Controls  Limits...

12.2.1.2. Modeling Heat Transfer in Two Separated Fluid Regions

If your heat transfer application involves two fluid regions separated by a solid zone or a wall, as illustrated in Figure 12.2: Typical Counterflow Heat Exchanger Involving Heat Transfer Between Two Separated Fluid Streams, you will need to define the problem with some care. Specifically:

  • You should not use outflow boundary conditions in either fluid.

  • You can establish separate fluid properties by selecting a different fluid material for each zone. For species calculations, however, you can only select a single mixture material for the entire domain.

Figure 12.2:  Typical Counterflow Heat Exchanger Involving Heat Transfer Between Two Separated Fluid Streams

Typical Counterflow Heat Exchanger Involving Heat Transfer Between Two Separated Fluid Streams


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