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.
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 Setting Under-Relaxation Factors.
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 finite-rate chemistry should be solved using either the pressure-based or density-based solver together with either Stiff Chemistry Solver or the CHEMKIN-CFD Solver (see Solution of Stiff Chemistry Systems). Finite-rate chemistry may also be used for turbulent combustion. For turbulent combustion, turbulence-chemistry interactions can either be neglected (Finite-rate/No TCI model) or accounted for using Eddy-Dissipation Concept or PDF Transport models.
Solving a reacting flow as a two-step process is 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 thereby 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:
Set up the problem including all species and reactions of interest.
Temporarily disable reaction calculations by turning off Volumetric in the Species Model Dialog Box.
Setup → Models → Species
Edit...
Disable calculation of the product species in the Equations Dialog Box.
Solution →
Controls
→ Equations...
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.)
Enable the reaction calculations by turning on Volumetric again in the Species Model Dialog Box.
Enable all equations in the Equations dialog box. If you are using the Finite-Rate/No TCI, Finite-Rate/Eddy-Dissipation, Eddy-Dissipation Concept or PDF Transport model for the turbulence-chemistry interaction, you may need to patch an ignition source (as described in Ignition in Steady-State Combustion Simulations).
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 want to reduce this to a value between 0.5 and 1 (in the Solution Controls task page).
Note that if you are using a real-gas model the solution might converge at a slower rate than when running ideal-gas flow. To improve the convergence performance of your analysis, you need to reduce the underrelaxation for density to values as low as 0.1.
If you introduce fuel to an oxidant or have a premixed fuel/oxidant mixture, but you are not simulating the transient ignition process, then you must numerically force the solution to the burned state (rather than the unburned state). Generally, spontaneous ignition does not occur unless the temperature of the mixture exceeds the activation energy threshold required to maintain combustion. For steady-state ANSYS Fluent combustion simulations, whether you are using the species transport or PDF transport model and regardless of turbulence-chemistry interaction option, 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 an ignitable fuel/air mixture.
Solution →
Initialization → 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 Patching Values in Selected Cells for details about patching initial values.
When modeling stiff chemistry systems, such as flames with finite-rate kinetics, you can either use the pressure-based solver with the Stiff Chemistry Solver option enabled or CHEMKIN-CFD Solver selected as seen in the Species Model Dialog Box (Figure 14.1: The Species Model Dialog Box), or the density-based solver.
For steady simulations using the pressure-based solver, the Stiff Chemistry Solver option approximates the reaction
rate in the species transport equation
(see Equation 7–5 in the Theory Guide) as,
(14–8) |
where is an appropriate time-step. Note that
as
tends to zero the approximation becomes
exact but the stiff numerics will cause the pressure-based solver
to diverge. On the other hand, as
tends to infinity, the
approximated reaction rate
tends to zero and, while the numerical stiffness
is alleviated, there is no reaction. In ANSYS Fluent, the default value
for
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 using the
solve/set/stiff-chemistry text command. ISAT is employed
to integrate the stiff chemistry in Equation 14–8. Equation 14–8 is also applied for unsteady
simulations, with = flow time step.
Details about the ISAT algorithm may be found in Particle Reaction in the Theory Guide and Using ISAT Efficiently. For efficient and accurate use of ISAT, a review of this section is highly recommended.
The density-based implicit solver may also be used with either 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 system Jacobian [127]. When enabling the stiff-chemistry solver with the density-based solver, the following must be specified:
Temperature Positivity Rate Limit: limits new temperature changes by this factor multiplied by the old temperature. Its default value is 0.2.
Temperature Time Step Reduction: limits the local CFL number when the temperature is changing too rapidly. Its default value is 0.25.
Max. Chemical Time Step Ratio: limits the local CFL number when the chemical time scales (eigenvalues of the chemical Jacobian) become too large to maintain a well-conditioned matrix. Its default value is 0.9.
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:
Calculate an initial solution using the equilibrium Non-premixed or Partially-premixed model (see Modeling Non-Premixed Combustion and Modeling Partially Premixed Combustion).
Import a CHEMKIN format reaction mechanism (see Importing a Volumetric Kinetic Mechanism in CHEMKIN Format).
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.
Setup → Models → Species
Edit...
Set the species boundary conditions.
Setup →
Boundary Conditions
Disable the flow and turbulence and solve for the species and temperature only.
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 Aggressiveness Factor in the Species dialog box or with the text command:
define → models → species → set-turb-chem-interaction
The Aggressiveness Factor can be set from 0 (slow but stable) to 1 (fast but least stable). The default is 0.5