13.2.1 Steps in 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 set up other models, boundary conditions, etc. as usual.)

1.   To activate the calculation of heat transfer, enable the Energy Equation option in the Energy dialog box (Figure  13.2.1).

Models Energy Edit...

Figure 13.2.1: The Energy Dialog Box

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.

Models Viscous Edit...

As noted in this section in the separate 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 (e.g., in lubrication problems) and/or in high-velocity, compressible flows (see this equation in the separate Theory Guide).

3.   Define thermal boundary conditions at flow inlets, flow outlets, and walls.

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

Section  7.3.14 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 Chapter  7 for details about boundary condition inputs.

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

4.   Define material properties for heat transfer.

Materials

Heat capacity and thermal conductivity must be defined, and you can specify many properties as functions of temperature as described in Chapter  8.

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

Limiting the Predicted Temperature Range: The Temperature Floor and Ceiling

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, etc. 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, you should use the Solution Limits dialog box to increase the Maximum Temperature.

Solution Controls Limits...

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  13.2.2, 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 13.2.2: Typical Counterflow Heat Exchanger Involving Heat Transfer Between Two Separated Fluid Streams