[ANSYS, Inc. Logo] return to home search
next up previous contents index

13.2.4 Natural Convection and Buoyancy-Driven Flows

When heat is added to a fluid and the fluid density varies with temperature, a flow can be induced due to the force of gravity acting on the density variations. Such buoyancy-driven flows are termed natural-convection (or mixed-convection ) flows and can be modeled by ANSYS FLUENT.

For more information about the theory behind natural convection and buoyancy-driven flows, see this section in the separate Theory Guide.

Modeling Natural Convection in a Closed Domain

When you model natural convection inside a closed domain, the solution will depend on the mass inside the domain. Since this mass will not be known unless the density is known, you must model the flow in one of the following ways:


For a closed domain, you can use the incompressible ideal gas law only with a fixed operating pressure. It cannot be used with a floating operating pressure. You can use the compressible ideal gas law with either floating or fixed operating pressure.

See Section  9.4.4 for more information about the floating operating pressure option.

The Boussinesq Model

For many natural-convection flows, you can get faster convergence with the Boussinesq model than you can get by setting up the problem with fluid density as a function of temperature. This model treats density as a constant value in all solved equations, except for the buoyancy term in the momentum equation:

 (\rho - \rho_0) g \approx -\rho_0 \beta (T - T_0) g (13.2-2)

where $\rho_0$ is the (constant) density of the flow, $T_0$ is the operating temperature, and $\beta$ is the thermal expansion coefficient. Equation  13.2-2 is obtained by using the Boussinesq approximation $\rho = \rho_0 (1 - \beta \Delta T)$ to eliminate $\rho$ from the buoyancy term. This approximation is accurate as long as changes in actual density are small; specifically, the Boussinesq approximation is valid when $\beta(T-T_0)\ll 1$.

Limitations of the Boussinesq Model

The Boussinesq model should not be used if the temperature differences in the domain are large. In addition, it cannot be used with species calculations, combustion, or reacting flows.

Steps in Solving Buoyancy-Driven Flow Problems

The procedure for including buoyancy forces in the simulation of mixed or natural convection flows is described below.

1.   Activate the calculation of heat transfer, by enabling the Energy option in the Energy dialog box.

figure Models figure figure Energy figure Edit...

2.   Define the operating conditions in the Operating Conditions dialog box (Figure  13.2.3).

figure Cell Zone Conditions figure Operating Conditions...

Figure 13.2.3: The Operating Conditions Dialog Box

(a)   Enable the Gravity option under Gravity.

(b)   Enter the appropriate values in the X, Y, and (for 3D) Z fields for Gravitational Acceleration for each Cartesian coordinate direction. (Note that the default gravitational acceleration in ANSYS FLUENT is zero.)

(c)   If you are using the incompressible ideal gas law, check that the Operating Pressure is set to an appropriate (non-zero) value.

(d)   Depending on whether or not you use the Boussinesq approximation, specify the appropriate parameters described below:

  • If you are not using the Boussinesq model, the inputs are as follows:

    i.   If necessary, enable the Specified Operating Density option in the Operating Conditions dialog box, and enter a value for the Operating Density. See below for details.

    ii.   Define the fluid density as a function of temperature as described in Sections  8.2 and 8.3.

    figure Materials

  • If you are using the Boussinesq model (described in Section  13.2.4) the inputs are as follows:

    i.   Enter the Operating Temperature ( $T_0$ in Equation  13.2-2) in the Operating Conditions dialog box.

    ii.   Select boussinesq in the drop-down list for Density in the Create/Edit Materials dialog box as described in Sections  8.2 and 8.3, and enter a constant value.

    iii.   Also in the Create/Edit Materials dialog box, enter an appropriate value for the Thermal Expansion Coefficient ( $\beta$ in Equation  13.2-2) for the fluid material.

Note that if your model involves multiple fluid materials you can choose whether or not to use the Boussinesq model for each material. As a result, you may have some materials using the Boussinesq model and others not. In such cases, you will need to set all the parameters described above in this step.

3.   Define the boundary conditions.

figure Boundary Conditions

The boundary pressures that you input at pressure inlet and outlet boundaries are the redefined pressures as given by Equation  13.2-3. In general you should enter equal pressures, $p'$, at the inlet and exit boundaries of your ANSYS FLUENT model if there are no externally-imposed pressure gradients.

4.   Set the parameters that control the solution.

figure Solution Methods

(a)   Select Body Force Weighted or Second Order in the drop-down list for Pressure under Spatial Discretization in the Solution Methods task page.

(b)   If you are using the pressure-based solver, selecting PRESTO! as the Spatial Discretization method for Pressure is the recommended approach.

(c)   Add cells near the walls to resolve boundary layers, if necessary.

See also Section  13.2.1 for information on setting up heat transfer calculations.

Operating Density

When the Boussinesq approximation is not used, the operating density $\rho_0$ appears in the body-force term in the momentum equations as $(\rho - \rho_0) g$.

This form of the body-force term follows from the redefinition of pressure in ANSYS FLUENT as

 p'_{s} = p_s - \rho_0 gx (13.2-3)

The hydrostatic pressure in a fluid at rest is then

 p'_s = 0 (13.2-4)

Setting the Operating Density

By default, ANSYS FLUENT will compute the operating density by averaging over all cells. In some cases, you may obtain better results if you explicitly specify the operating density instead of having the solver compute it for you. For example, if you are solving a natural-convection problem with a pressure boundary, it is important to understand that the pressure you are specifying is $p'_s$ in Equation  13.2-3. Although you will know the actual pressure $p_s$, you will need to know the operating density $\rho_0$ in order to determine $p'_s$ from $p_s$. Therefore, you should explicitly specify the operating density rather than use the computed average. The specified value should, however, be representative of the average value.

In some cases the specification of an operating density will improve convergence behavior, rather than the actual results. For such cases use the approximate bulk density value as the operating density and be sure that the value you choose is appropriate for the characteristic temperature in the domain.

Note that if you are using the Boussinesq approximation for all fluid materials, the operating density $\rho_0$ does not appear in the body-force term of the momentum equation. Consequently, you need not specify it.

Solution Strategies for Buoyancy-Driven Flows

For high-Rayleigh-number flows you may want to consider the solution guidelines below. In addition, the guidelines presented in Section  13.2.2 for solving other heat transfer problems can also be applied to buoyancy-driven flows. Note, however that no steady-state solution exists for some laminar, high-Rayleigh-number flows.

Guidelines for Solving High-Rayleigh-Number Flows

When you are solving a high-Rayleigh-number flow ( ${\rm Ra} > 10^8$) you should follow one of the procedures outlined below for best results.

The first procedure uses a steady-state approach:

1.   Start the solution with a lower value of Rayleigh number (e.g., $10^7$) and run it to convergence using the first-order scheme.

2.   To change the effective Rayleigh number, change the value of gravitational acceleration (e.g., from 9.8 to 0.098 to reduce the Rayleigh number by two orders of magnitude).

3.   Use the resulting data file as an initial guess for the higher Rayleigh number and start the higher-Rayleigh-number solution using the first-order scheme.

4.   After you obtain a solution with the first-order scheme you may continue the calculation with a higher-order scheme.

The second procedure uses a time-dependent approach to obtain a steady-state solution [ 30]:

1.   Start the solution from a steady-state solution obtained for the same or a lower Rayleigh number.

2.   Estimate the time constant as [ 10]

 \tau = \frac{L}{U} \sim \frac{L^2}{\alpha} ({\rm Pr Ra})^{-1/2} = \frac{L}{\sqrt{g \beta \Delta T L}} (13.2-5)

where $L$ and $U$ are the length and velocity scales, respectively. Use a time step $\Delta t$ such that

 \Delta t \approx \frac{\tau}{4} (13.2-6)

Using a larger time step $\Delta t$ may lead to divergence.

3.   After oscillations with a typical frequency of $f \tau =$ 0.05-0.09 have decayed, the solution reaches steady state. Note that $\tau$ is the time constant estimated in Equation  13.2-5 and $f$ is the oscillation frequency in Hz. In general this solution process may take as many as 5000 time steps to reach steady state.

Postprocessing Buoyancy-Driven Flows

The postprocessing reports of interest for buoyancy-driven flows are the same as for other heat transfer calculations. See Section  13.2.3 for details.

next up previous contents index Previous: 13.2.3 Postprocessing Heat Transfer
Up: 13.2 Modeling Conductive and
Next: 13.2.5 Shell Conduction Considerations
Release 12.0 © ANSYS, Inc. 2009-01-29