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

15.1.7 Solution Procedures for Chemical Mixing and Finite-Rate Chemistry

While many simulations involving chemical species may require no special procedures during the solution process, you may find that one or more of the solution techniques noted in this section helps to accelerate the convergence or improve the stability of more complex simulations. The techniques outlined below may be of particular importance if your problem involves many species and/or chemical reactions, especially when modeling combusting flows.



Stability and Convergence in Reacting Flows

Obtaining a converged solution in a reacting flow can be difficult for a number of reasons. First, the impact of the chemical reaction on the basic flow pattern may be strong, leading to a model in which there is strong coupling between the mass/momentum balances and the species transport equations. This is especially true in combustion , where the reactions lead to a large heat release and subsequent density changes and large accelerations in the flow. All reacting systems have some degree of coupling, however, when the flow properties depend on the species concentrations. These coupling issues are best addressed by the use of a two-step solution process, as described below, and by the use of under-relaxation as described in Section  26.3.2.

A second convergence issue in reacting flows involves the magnitude of the reaction source term. When the ANSYS FLUENT model involves very rapid reaction rates (reaction time scales are much faster than convection and diffusion time scales), the solution of the species transport equations becomes numerically difficult. Such systems are termed "stiff'' systems. Stiff systems with laminar chemistry can be solved using either the pressure-based solver with the Stiff Chemistry Solver option enabled, or the density-based solver (see Section  15.1.7). The laminar chemistry model may also be used for turbulent flames, where turbulence-chemistry interactions are neglected. However, for such flames, the Eddy-Dissipation Concept or PDF Transport models, which account for turbulence-chemistry interactions, may be a better choice.



Two-Step Solution Procedure (Cold Flow Simulation)

Solving a reacting flow as a two-step process can be a practical method for reaching a stable converged solution to your ANSYS FLUENT problem. In this process, you begin by solving the flow, energy, and species equations with reactions disabled (the "cold-flow'', or unreacting flow). When the basic flow pattern has thus been established, you can re-enable the reactions and continue the calculation. The cold-flow solution provides a good starting solution for the calculation of the combusting system. This two-step approach to combustion modeling can be accomplished using the following procedure:

1.   Set up the problem including all species and reactions of interest.

2.   Temporarily disable reaction calculations by turning off Volumetric in the Species Model dialog box.

figure Models figure figure Species figure Edit...

3.   Turn off calculation of the product species in the Equations dialog box.

figure Solution Controls figure Equations...

4.   Calculate an initial (cold-flow) solution. (Note that it is generally not productive to obtain a fully converged cold-flow solution unless the non-reacting solution is also of interest to you.)

5.   Enable the reaction calculations by turning on Volumetric again in the Species Model dialog box.

6.   Enable all equations in the Equations dialog box. If you are using the laminar finite-rate, finite-rate/eddy-dissipation, Eddy-Dissipation Concept or PDF Transport model for turbulence-chemistry interaction, you may need to patch an ignition source (as described below).



Density Under-Relaxation

One of the main reasons a combustion calculation can have difficulty converging is that large changes in temperature cause large changes in density, which can, in turn, cause instabilities in the flow solution. When you use the pressure-based solver, ANSYS FLUENT allows you to under-relax the change in density to alleviate this difficulty. The default value for density under-relaxation is 1, but if you encounter convergence trouble you may wish to reduce this to a value between 0.5 and 1 (in the Solution Controls task page).



Ignition in Combustion Simulations

If you introduce fuel to an oxidant, spontaneous ignition does not occur unless the temperature of the mixture exceeds the activation energy threshold required to maintain combustion. This physical issue manifests itself in an ANSYS FLUENT simulation as well. If you are using the laminar finite-rate, finite-rate/eddy-dissipation, Eddy-Dissipation Concept or PDF Transport model for turbulence-chemistry interaction, you have to supply an ignition source to initiate combustion. This ignition source may be a heated surface or inlet mass flow that heats the gas mixture above the required ignition temperature. Often, however, it is the equivalent of a spark: an initial solution state that causes combustion to proceed. You can supply this initial spark by patching a hot temperature into a region of the ANSYS FLUENT model that contains a sufficient fuel/air mixture for ignition to occur.

figure Solution Initialization figure Patch...

Depending on the model, you may need to patch both the temperature and the fuel/ oxidant/product concentrations to produce ignition in your model. The initial patch has no impact on the final steady-state solution--no more than the location of a match determines the final flow pattern of the torch that it lights. See Section  26.9.2 for details about patching initial values.



Solution of Stiff Laminar Chemistry Systems

When modeling stiff laminar flames with the laminar finite-rate model, you can either use the pressure-based solver with the Stiff Chemistry Solver option enabled as seen in the Species Model dialog box (Figure  15.1.1), or the density-based solver.

When using the pressure-based solver for unsteady simulations, the Stiff Chemistry Solver option applies a fractional step algorithm. In the first fractional step, the chemistry in each cell is reacted at constant pressure for the flow time-step, using the ISAT integrator. In the second fractional step, the convection and diffusion terms are treated just as in a non-reacting simulation.

For steady simulations using the pressure-based solver, the Stiff Chemistry Solver option approximates the reaction rate $R_{i}$ in the species transport equation (see this equation in the separate Theory Guide) as,


R^{*}_{i} = \frac{1}{\tau} \int_{0}^{\tau} R_{i} d t (15.1-5)

where $\tau$ is an appropriate time-step. Note that as ${\tau}$ tends to zero the approximation becomes exact but the stiff numerics will cause the pressure-based solver to diverge. On the other hand, as ${\tau}$ tends to infinity, the approximated reaction rate $R^{*}_{i}$ tends to zero and, while the numerical stiffness is alleviated, there is no reaction. In ANSYS FLUENT, the default value for ${\tau}$ is set to one-tenth of the minimum convective or diffusive time-scale in the cell. This value was found to be sufficiently accurate and robust, although it can be modified via the solve/set/stiff-chemistry text command. ISAT is employed to integrate the stiff chemistry in Equation  15.1-5.

Details about the ISAT algorithm may be found in this section in the separate Theory Guide and Section  19.6.2. For efficient and accurate use of ISAT, a review of this section is highly recommended.

Choosing the density-based implicit solver can provide further solution stability by enabling the Stiff Chemistry Solver option. This option allows a larger stable Courant (CFL) number specification, although additional calculations are required to calculate the eigenvalues of the chemical Jacobian [ 91]. When enabling the stiff-chemistry solver, the following must be specified:

If the density-based explicit solver is used, then the stiff-chemistry solver has to be enabled via the text command:

solve $\rightarrow$ set $\rightarrow$ stiff-chemistry

You will be prompted to specify the following:

The default values of these parameters are applicable in most cases.



Eddy-Dissipation Concept Model Solution Procedure

Due to the high computational expense of the Eddy-Dissipation Concept model, it is recommended that you use the following procedure to obtain a solution using the pressure-based solver:

1.   Calculate an initial solution using the equilibrium Non-premixed or Partially-premixed model (see Chapters  16 and 18).

2.   Import a CHEMKIN format reaction mechanism (see Section  15.1.9).

3.   Enable the reaction calculations by turning on Volumetric Reactions in the Species Model dialog box and selecting Eddy-Dissipation Concept under Turbulence-Chemistry Interaction. Select the mechanism that you just imported as the Mixture Material.

figure Models figure figure Species figure Edit...

4.   Set the species boundary conditions.

figure Boundary Conditions

5.   Disable the flow and turbulence and solve for the species and temperature only.

6.   Enable all equations and iterate to convergence. Note that the default numerical parameters for the solution of the Eddy-Dissipation Concept equations are set to provide maximum robustness with slowest convergence. The convergence rate can be increased by setting the Acceleration Factor in the Species dialog box or with the text command:

define $\rightarrow$ models $\rightarrow$ species $\rightarrow$ set-turb-chem-interaction

The Acceleration Factor can be set from 0 (slow but stable) to 1 (fast but least stable).

next up previous contents index Previous: 15.1.6 Defining Other Sources
Up: 15.1 Volumetric Reactions
Next: 15.1.8 Postprocessing for Species
Release 12.0 © ANSYS, Inc. 2009-01-29