13.2.2 Solution Strategies for Heat Transfer Modeling

Although many simple heat transfer problems can be successfully solved using the default solution parameters assumed by ANSYS FLUENT, you may accelerate the convergence of your problem and/or improve the stability of the solution process using some of the guidelines provided in this section.

Under-Relaxation of the Energy Equation

When you use the pressure-based solver, ANSYS FLUENT under-relaxes the energy equation using the under-relaxation parameter defined by you in the Solution Controls task page, as described in Section  26.3.2.

Solution Controls

If you are using the non-adiabatic non-premixed combustion model, you will set the energy under-relaxation factor as usual but you will also set an under-relaxation factor for temperature, as described below.

ANSYS FLUENT uses a default under-relaxation factor of 1.0 for the energy equation, regardless of the form in which it is solved (temperature or enthalpy). In problems where the energy field impacts the fluid flow (via temperature-dependent properties or buoyancy) you should use a lower value for the under-relaxation factor, in the range of 0.8-1.0. In problems where the flow field is decoupled from the temperature field (no temperature-dependent properties or buoyancy forces), you can usually retain the default value of 1.0.

Under-Relaxation of Temperature When the Enthalpy Equation is Solved

When the enthalpy form of the energy equation is solved (i.e., when you are using the non-adiabatic non-premixed combustion model), ANSYS FLUENT also under-relaxes the temperature, updating the temperature by only a fraction of the change that would result from the change in the (under-relaxed) enthalpy values. This second level of under-relaxation can be used to good advantage when you would like to let the enthalpy field change rapidly, but the temperature response (and its effect on fluid properties) to lag. ANSYS FLUENT uses a default setting of 1.0 for the under-relaxation on temperature and you can modify this setting using the Solution Controls task page.

Disabling the Species Diffusion Term

If you are solving for species transport using the pressure-based solver and you encounter convergence difficulties, you may want to consider disabling the Diffusion Energy Source option in the Species Model dialog box.

Models Species Edit...

When this option is disabled, ANSYS FLUENT will neglect the effects of species diffusion on the energy equation.

Note that species diffusion effects are always included when the density-based solver is used.

Step-by-Step Solutions

Often the most efficient strategy for predicting heat transfer is to compute an isothermal flow first and then add the calculation of the energy equation. The procedure differs slightly, depending on whether or not the flow and heat transfer are coupled.

Decoupled Flow and Heat Transfer Calculations

If your flow and heat transfer are decoupled (no temperature-dependent properties or buoyancy forces), you can first solve the isothermal flow (energy equation turned off) to yield a converged flow-field solution and then solve the energy transport equation alone.

Since the density-based solver always solves the flow and energy equations together, the procedure for solving for energy alone applies to the pressure-based solver, only.

You can temporarily disable the flow equations or the energy equation by disabling the Energy option in the Equations dialog box

Solution Controls Equations...

or

Models Energy Edit...

Coupled Flow and Heat Transfer Calculations

If the flow and heat transfer are coupled (i.e., your model includes temperature-dependent properties or buoyancy forces), you can first solve the flow equations before enabling energy. Once you have a converged flow-field solution, you can enable energy and solve the flow and energy equations simultaneously to complete the heat transfer simulation.