Modeling errors are the most difficult errors to avoid, as they cannot be reduced systematically. The most important factor for the reduction of modeling errors is the quality of the models available in the CFD package and the experience of the user. There is also a strong interaction between modeling errors and the time and space resolution of the grid. The resolution has to be sufficient for the model selected for the application.
In principle, modeling errors can only be estimated in cases where the validation of the model is ‘close’ to the intended application. Model validation is essential for the level of confidence you can have in a CFD simulation. It is therefore required that you gather all available information on the validation of the selected model, both from the open literature and from the code developers (vendors). In case that CFD is to be applied to a new field, it is recommended that you carry out additional validation studies, in order to gain confidence that the physical models are adequate for the intended simulation.
If several modeling options are available in the code (as is usually the case for turbulence, combustion and multi-phase flow models), it is recommended that you carry out the simulation with different models in order to test the sensitivity of the application with respect to the model selection.
In case you have personal access to a modeling expert in the required area, it is recommended that you interact with the model developer or expert to ensure the optimal selection and use of the model.
There are different methods for the treatment of turbulent flows. The need for a model results from the inability of CFD simulations to fully resolve all time and length scales of a turbulent motion. In classical CFD methods, the Navier-Stokes equations are usually time- or ensemble-averaged, reducing the resolution requirements by many orders of magnitude. The resulting equations are the RANS equations. Due to the averaging procedure, information is lost, which is then fed back into the equations by a turbulence model.
The amount of information that has to be provided by the turbulence model can be reduced if the large time and length scales of the turbulent motion are resolved. The equations for this so-called Large Eddy Simulation (LES) method are usually filtered over the grid size of the computational cells. All scales smaller than the resolution of the mesh are modeled and all scales larger than the cells are computed. This approach is several orders of magnitude more expensive than a RANS simulation and is therefore not used routinely in industrial flow simulations. It is most appropriate for free shear flows, as the length scales near the solid walls are usually very small and require small cells even for the LES method.
RANS methods are the most widely used approach for CFD simulations of industrial flows. Early methods, using algebraic formulations, have been largely replaced by more general transport equation models, for both implementation and accuracy considerations. The use of algebraic models is not recommended for general flow simulations, due to their limitations in generality and their geometric restrictions. The lowest level of turbulence models that offer sufficient generality and flexibility are two-equation models. They are based on the description of the dominant length and time scale by two independent variables. Models that are more complex have been developed and offer more general platforms for the inclusion of physical effects. The most complex RANS model used in industrial CFD applications are Second Moment Closure (SMC) models. Instead of two equations for the two main turbulent scales, this approach requires the solution of seven transport equations for the independent Reynolds stresses and one length (or related) scale.
The challenge for the user of a CFD method is to select the optimal model for the application at hand from the models available in the CFD method. In most cases, it cannot be specified beforehand which model will offer the highest accuracy. However, there are indications as to the range of applicability of different turbulence closures. This information can be obtained from validation studies carried out with the model.
In addition to the accuracy of the model, consideration has to be given to its numerical properties and the required computer power. It is often observed that more complex models are less robust and require many times more computing power than the additional number of equations would indicate. Frequently, the complex models cannot be converged at all, or, in the worst case, the code becomes unstable and the solution is lost.
It is not trivial to provide general rules and recommendations for the selection and use of turbulence models for complex applications. Different CFD groups have given preference to different models for historical reasons or personal experiences. Even turbulence experts cannot always agree as to which model offers the best cost-performance ratio for a new application.
A number of one-equation turbulence models based on an equation for the eddy viscosity have been developed over the last years. Typical applications are:
Airplane- and wing flows
External automobile aerodynamics
Flow around ships.
These models have typically been optimized for aerodynamic flows and are not recommended as general-purpose models.
The two-equation models are the
main-stand of industrial CFD simulations. They offer a good compromise
between complexity, accuracy and robustness. The most popular models
are the standard model and different versions of the 
model, see Wilcox [30]. The standard 
model of Wilcox is the most well
known of the 
based models, but shows a severe free-stream dependency.
It is therefore not recommended for general industrial flow simulations,
as the results are strongly dependent on the user input. Alternative
formulations are available, see for example, the Shear Stress
Transport (SST) model, Menter [9].
An important weakness of standard two-equation models is that they are insensitive to streamline curvature and system rotation. Particularly for swirling flows, this can lead to an over-prediction of turbulent mixing and to a strong decay of the core vortex. There are curvature correction models available, but they have not been generally validated for complex flows.
The standard two-equation models can also exhibit a strong build-up of turbulence in stagnation regions, due to their modeling of the production terms. Several modifications are available to reduce this effect, for instance by Kato and Launder [128]. They should be used for flows around rods, blades, airfoils, and so on.
SMC models are based on the solution
of a transport equation for each of the independent Reynolds stresses
in combination with the 
- or the 
-equation.
These models offer generally a wider modeling platform and account
for certain effects due to their exact form of the turbulent production
terms. Some of these models show the proper sensitivity to swirl and
system rotation, which have to be modeled explicitly in a two-equation
framework. SMC models are also superior for
flows in stagnation regions, where no additional modifications are
required.
One of the weak points of the SMC closure is that the same scale equations are used as in the two-equation framework. As the scale equation is typically one of the main sources of uncertainty, it is found that SMC models do not consistently produce superior results compared to the simpler models. In addition, experience has shown that SMC models are often much harder to handle numerically. The model can introduce a strong nonlinearity into the CFD method, leading to numerical problems in many applications.
SMC models are usually not started from a pre-specified initial condition, but from an already available solution from a two-equation (or simpler) model. This reduces some of the numerical problems of the SMC approach. In addition, it offers an important sensitivity study, as it allows quantifying the influence of the turbulence model on the solution. It is therefore recommended that you fully converge the two-equation model solution and save it for a comparison with the SMC model solution. The difference between the solutions is a measure of the influence of the turbulence model and therefore an indication of the modeling uncertainty. This is possible only in steady-state simulations. For unsteady flows, the models usually have to be started from the initial condition.
LES models are based on the numerical resolution of the large turbulence scales and the modeling of the small scales. LES is not yet a widely used industrial approach, due to the large cost of the required unsteady simulations. For certain classes of applications, LES will be applicable in the near future. The most appropriate area will be free shear flows, where the large scales are of the order of the solution domain (or only an order of magnitude smaller). For boundary layer flows, the resolution requirements are much higher, as the near-wall turbulent length scales become much smaller. The internal flows (pipe flows, channel flows) are in between, as they have a restricted domain in the wall normal direction, but small scales have to be resolved in the other two directions.
LES simulations do not easily lend themselves to the application of grid refinement studies both in the time and the space domain. The main reason is that the turbulence model adjusts itself to the resolution of the grid. Two simulations on different grids are therefore not comparable by asymptotic expansion, as they are based on different levels of the eddy viscosity and therefore on a different resolution of the turbulent scales. From a theoretical standpoint, the problem can be avoided, if the LES model is not based on the grid spacing, but on a pre-specified filter-width. This would enable reaching grid-independent LES solutions above the DNS limit. However, LES is a very expensive method and systematic grid and timestep studies are prohibitive even for a pre-specified filter. It is one of the disturbing facts that LES does not lend itself naturally to quality assurance using classical methods. This property of the LES also indicates that (nonlinear) multigrid methods of convergence acceleration are not suitable in this application.
On a more global level, the grid convergence can be tested using averaged quantities resulting from the LES simulation. The averaged LES results can be analyzed in a similar way as RANS solutions (at least qualitatively). Again, it is expensive to perform several LES simulations and grid refinement will therefore be more the exception than the rule.
Due to the high computing requirements of LES, modern developments in the turbulence models focus on a combination of RANS and LES models. The goal is to cover the wall boundary layers with RANS and to enable unsteady (LES-like) solutions in largely separated and unsteady flow regions (for example, flow behind a building, or other blunt bodies). There are two alternatives of such methods available in Ansys CFX.
The first alternative is called Scale-Adaptive-Simulation (SAS) model (Menter and Egorov [130], [131], [144], [145]). It is essentially an improved Unsteady RANS (URANS) method that develops LES-like solutions in unstable flow regimes.
The second alternative is called Detached Eddy Simulation (DES) (Spalart [146]), implemented in the version of Strelets [58]. The current recommendation is to use the SAS model, as it has less grid sensitivity than the DES formulation. In case that SAS does not provide an unsteady solution, the DES model should be applied. It should be noted that both model formulations require small timesteps with a Courant number of CFL<1. You are encouraged to read the original references before applying these models.
There are generally three types of boundary conditions that can be applied to a RANS simulation:
Standard wall functions are based on the assumption that the first grid point off the wall (or the first integration point) is located in the universal law-of-the-wall or logarithmic region. Wall functions eliminate the need to resolve the very thin viscous sublayer, leading to a reduction in the number of cells and to a more moderate (and desirable) aspect ratio of the cells (ratio of the longest to the smallest side in a structured grid). High aspect ratios can result in numerical problems due to round-off errors.
On the other hand, standard wall function formulations are difficult to handle, because you have to ensure that the grid resolution near the wall satisfies the wall function requirements. If the grid becomes too coarse, the resolution of the boundary layer is no longer ensured. If the resolution becomes too fine, the first grid spacing can be too small to bridge the viscous sublayer. In this case, the logarithmic profile assumptions are no longer satisfied. You have to ensure that both limits are not overstepped in the grid generation phase.
The lower limit on the grid resolution for standard wall functions is a severe detriment to a systematic grid refinement process, as required by the best practice approach. That is, instead of an improved accuracy of the solution with grid refinement, the solution will deteriorate from a certain level on, leading eventually to a singularity of the numerical method. Standard wall functions are therefore not recommended for systematic grid refinement studies. Recently, alternative formulations (scalable wall functions) have become available, Menter and Esch [142], which enable a systematic grid refinement when using wall functions.
The use of low-Reynolds (low-Re) number formulations of turbulence
models for the integration of the equations through the viscous sublayer
is generally more accurate, as no additional assumptions are required
concerning the variation of the variables near the wall. On the downside,
most low-Re extensions of turbulence models are quite complex and
can reduce the numerical performance or even destabilize the numerical
method. In addition, classical low-Re models require a very fine near-wall
resolution of 
at all wall nodes. This is very hard to ensure for all walls of
a complex industrial application. In the case that significantly coarser
grids are used, the wall shear stress and the wall heat transfer can
be reduced significantly below their correct values.
In Ansys CFX, hybrid methods are available for all 
-equation
based turbulence models (automatic near-wall treatment), which automatically
switch from a low-Re formulation to wall functions based on the grid
spacing you provide. These formulations provide the optimal boundary
condition for a given grid. From a best practice standpoint, they
are the most desirable, as they enable an accurate near-wall treatment
over a wide range of grid spacings. However, accurate boundary layer
simulations do not depend only on the 
near-wall spacing, but also require a minimum of
at least 10 grid nodes inside the boundary layer.
Avoid the use of classical wall functions, as they are inconsistent with grid refinement.
Avoid strict low-Re number formulations, unless it is ensured that all near-wall cells are within the resolution requirements of the formulation.
In combination with the
model, use scalable wall functions.
They can be applied to a range of grids without immediate deterioration
of the solution (default in Ansys CFX). For more accurate simulations, use an automatic wall treatment in combination with SST turbulence model (default in Ansys CFX).
The heat transfer formulation is strongly linked to the underlying turbulence model. For eddy viscosity models, the heat transfer simulation is generally based on the analogy between heat and momentum transfer. Given the eddy viscosity of the two-equation model, the heat transfer prediction is based on the introduction of a molecular and a turbulent Prandtl number. The treatment of the energy equation is therefore similar to the treatment of the momentum equations. No additional transport equations are required for the turbulent heat transfer prediction. The boundary conditions are the same as for the momentum equations and follow the same recommendations.
For SMC models, three additional transport equations must be solved for the turbulent heat transfer vector in order to be consistent with the overall closure level. Only a few CFD methods offer this option. In most cases, the heat transfer is computed from an eddy diffusivity with a constant turbulent Prandtl number.
Multi-phase models are required in cases where more than one phase is involved in the simulation (phases can also be non-miscible fluids). There is a wide variety of multi-phase flow scenarios, with the two extremes of small-scale mixing of the phases or a total separation of the phases by a sharp interface.
Depending on the flow simulation, different types of models are available. The main distinction of the models is given below.
Lagrange models solve a separate equation for individual particles, bubbles, or droplets in a surrounding fluid. The method integrates the three-dimensional trajectories of the particles based on the forces acting on them from the surrounding fluid and other sources. Turbulence is usually accounted for by a random motion, superimposed on the trajectory.
Lagrange models are usually applied to flows with low particle (bubble) densities. In these flows, the interaction between the particles can usually be neglected, thereby reducing the complexity of the problem significantly.
The Euler-Euler formulation is based on the assumption of interpenetrating continua. A separate set of mass, momentum, and energy conservation equations is solved for each phase. Interphase transfer terms have to be modeled to account for the interaction of the phases. Euler-Euler methods can be applied to separated and dispersed flows by changing the interface transfer model.
Additional models are required for flows with mass transfer between the phases (condensation, evaporation, boiling). These models can be applied in the form of correlations for a large number of particles (bubbles) in a given control volume, or directly at the interface between the resolved phase boundary.