Turbulence Models

Selection of the turbulence model mainly depends on the objective of a physical phenomenon that needs to be resolved. Reynolds-averaged Navier Stokes (RANS) and Large Eddy Simulation (LES) are two widely-used methods for calculating the effect of wind loads on buildings. A choice of a given model has a significant contribution on both accuracy and the computational cost. Therefore, the selection of the appropriate turbulence model is a very important decision in CWE simulations.

Reynolds-averaged Navier-Stokes equations (RANS): This is a widely- used model for most simulations due to its reduced computational resource requirement, and also provides a reasonable approximation for many simulations. RANS involves averaging of the turbulence terms, with various levels of approximations. The following are some of the variations in RANS turbulence models:

Spalart-Allmaras (one-equation model): This is the simplest RANS model that solves a modelled transport equation for the kinematic eddy (turbulent) viscosity (Spalart and Shur, 1997). The method is found to be effective at low Reynolds numbers, and allows the application of the model, independent of near-wall y* resolution (ANSYS Inc., 2020).

K-epsilon, K-e (two-equation model): The standard K-epsilon model involves solution of two transport equations based on turbulent kinetic energy and dissipation rate (Launder and Spalding, 1972). The two transport equations for К and e are given in Equations (16.18) and (16.19), respectively. This model is used widely in many engineering applications due to its simplicity, computational time, and reasonable solutions for most applications. However, the model has difficulty in resolving some flow regions.

In the above equations, Cle, С, and C}e are constants, о к is the turbulent Prandtl number for kinetic energy, and ae is the turbulent Prandtl number for dissipation rate. Gr is the generation of turbulent energy due to mean velocity gradient, Gi, is the generation of turbulent kinetic energy due to buoyancy. Sk and Se are source terms. The turbulent viscosity is


parameterized by pt = pCt,—.

There have been a number of proposed improvements to the standard K-e model. The most used variations of the standard model are: renormalisation group (RNG) and realizable K-e models. [1]

  • Transition SST (four-equation model): Shear-stress transport (SST) is a four-equation model which is an extension of the Menter (1992, 1994) two-equation model (Langtry and Menter, 2009). The model combines the SST K-co equations with gamma (y) and Re theta (Ree). The two additional transport equations are for intermittency and transition. The model gained a wide application and improvement. However, there are some limitations, as listed below (ANSYS Inc., 2020):
  • • The transition SST model is only applicable to wall-bounded flows. The model is not applicable to transition in free-shear flows and predicts free -shear flows as fully turbulent.
  • • The model should not be applied to a surface that moves relative to the coordinate system for which the velocity field is computed.
  • • The transition SST model is for flows with non-zero free-stream velocity like boundary layer flows.
  • • The model is not suitable for wall jet flows.
  • Reynolds stress model (RSM) (seven-equation model): This is a higher-level turbulence closures model also called ‘second-order closure’. The RSM does not use the eddy viscosity approach used in the RANS models described previously, but computes the Reynolds stress tensor directly (Chou, 1945; Rotta, 1951). The model accounts for the effect of streamline curvature, rapid change in strain rate, swirl and rotation to provide better prediction in complex flow. However, the results are limited to the assumptions made to form the transport equation for the Reynolds stress. The additional equations in RSM increase the required amount of computational resources. In addition, due to the assumption on closure model, it may not lead to accurate result in all cases. Thus, justification of its use may be required for simulation efficiency. However, for some flows, such as cyclone flows, highly swirling flows in combustors, rotating flow passages and the stress-induced secondary flows in ducts, it may provide a better result (ANSYS Inc., 2020).
  • Large eddy simulation (LES): LES is a method based on flow scaling, where large scales are resolved, while small scales are modelled. This method is different from the RANS model which is based on time averages or ensemble averaging. In direct numerical simulation (DNS), all the scales are resolved, and no modelling is required. However, this is computationally very expensive and not practical for high Reynolds number flows. In LES, large eddies are resolved directly, while small eddies are modelled. As turbulent modelling and range of resolved scales, LES can be considered to fall between DNS and RANS. Since LES models the large eddies, the requirement of mesh sizes is much lower than DNS. However, the requirement is impractical for most industrial applications.

Detached eddy simulation (DES): The DES model combines the RANS model with LES. This combination allows LES to be used for high Reynolds number by employing RANS for boundary layer resolution. The model still requires a considerable computational resource but much less extent than modelling with LES. The RANS model can be any one of the models discussed - one-, two-, three- or four- equation models.

Boundary Conditions

Unbounded computational domain changed to finite computational area by introducing artificial boundaries. The characteristics of these artificial boundaries need to be specified in order to solve the discretised algebraic equations. How the boundary conditions specified have a direct relation with the accuracy of the solution, computational time and numerical stability, is an area for study. Some common boundary conditions are presented below:

Wall boundary condition: This is the boundary condition used to represent the solid part of the computational domain. In external flow, the ground and the surfaces of buildings, or any solid structure, are represented by a wall boundary condition. In general, the wall boundary condition can be stationary or moving. The parameters specified by this boundary condition are no slip or slip condition, surface roughness, shear stress for velocity, stability, and unbounded domain as in external flow.

The wall boundary is one of the most difficult boundaries to handle, and the result of the difference between turbulent models. In turbulent flow near the wall, viscous damping reduces the tangential velocity fluctuations, while kinematic blocking reduces the normal fluctuations. Due to large gradients in mean velocity, the turbulence is rapidly increased by the production of turbulence kinetic energy toward the outer part of the near-wall region. Large changes of the variables gradient and momentum occur in the near-wall region. The near-wall region is divided into three layers: viscous sublayer, buffer layer and full turbulent region (log law region).

Viscous sublayer (y* < 5): This layer is the innermost layer where the flow is almost laminar, and viscosity plays a dominant role in momentum and heat or mass transfer. It can be assumed that the Reynolds shear stress is negligible. The “linear velocity law” is given by the following relation.

where у* = yu / v (u" is the friction velocity and v is the kinematic viscosity), and u+ = u/u, a non-dimensional velocity near the surface.

Buffer layer (5 < y* < 30): This layer is the transition region between the viscosity-dominated region and turbulence-dominated part of the flow.

Viscous and turbulent stresses are of similar magnitude, and since it is complex, the velocity profile is not well defined and the original wall functions avoid the first cell centre located in this region.

Log-law region (y* > 30): The turbulent stress dominates the flow in this region, and the velocity profile varies very slowly with a logarithmic function along the coordinate, y. The relation for this region, with a value of von Karman’s constant, k, of 0.41, is as follows:

The near-wall region can be modelled by two different methods. In the first method, the viscous affected region is resolved by a fine mesh all the way to the wall. The second method involves semi-empirical formula used to represent the viscous sublayer and buffer layer. This method is called the ‘wall-function’ method. These two methods are illustrated in Figure 16.9.

A wall function can be used to compute the wall shear stress instead of resolving the near-wall region. This approach reduces computational cost. However, the solution accuracy is reduced, or it can lead to instability if the model is used with a very fine mesh. Thus, the recommended value of y+ for first mesh point is between 30 and 500 (Franke et al., 2007).

Inlet boundary condition: Information on velocity and turbulent quantities is required to be specified at the inlet boundary. For steady-state simulation of synoptic-scale atmospheric boundary layers, the standard velocity profile described using power law, logarithmic law, friction velocity and roughness of the upwind terrain can be used. The turbulence characteristics can be specified by the turbulent kinetic energy, dissipation rate, intensity, specific dissipation rate, and length scale. The choice of turbulence parameters for the boundary conditions can be directly related to the turbulence

Near-wall region modelling

Figure 16.9 Near-wall region modelling.

model used in the flow modelling. For example, the following relationships for velocity and turbulence parameters can be used:

и is the friction velocity in the atmospheric boundary layer (ABL); к is von Karman’s constant (Section 3.2.1), Сц is the model constant for the K - e model, z is the height, and z0 is the roughness length (see Section 3.2.1).

A problem in steady-state simulation is that the inlet boundary conditions specified for mean velocity and turbulence will dissipate, and be modified, due to numerical dissipation and the wall function. Blocken et al. (2007) have discussed the boundary layer and wall function problem and provided some suggestions.

For unsteady simulations, an instantaneous inlet profile should be specified to reproduce the unsteady behaviour of the flow. There are a number of suggestions by researchers to impose unsteady inlet boundary conditions. Commercial software also provides alternate ways of generating unsteady inlet boundary condition (ANSYS Inc., 2020).

Outflow boundary condition: The boundary at downstream, leaving the computational domain, can be specified as an outflow or pressure outlet boundary condition.

With an outflow boundary condition, the derivatives of all flow variables are forced to vanish. Since no flow variable is specified in this condition, convergence can be a problem for the same flows. The pressure outlet boundary condition uses a constant static pressure at the outflow boundary. This boundary should be set far enough away from the region of interest during the computational domain construction, so that backflow does not affect the solution. For LES convective outflow boundary conditions, see Ferziger and Peric (2002).

Top boundary condition: The top boundary is specified as symmetry or inlet boundary condition. In the case of a symmetrical boundary, the assumption is that there is no convective flux across the boundary. The normal velocity component at the boundary is zero. There is no diffusion flux across the boundary, and the normal gradient of all flow variables is zero. There is a problem of sustaining equilibrium boundary layer profiles, as reported by Blocken et al. (2007). Thus, use of the inflow velocity and turbulent profile at the top boundary is recommended.

Lateral boundary condition: The sides of the computational domain are specified by a symmetrical boundary condition when these boundaries are parallel to the flow direction. They can be specified as outflow or pressure outlet boundary condition if they are located at the downstream of the flow. These boundaries should be away from the region of interest, with a blockage of 3% or less in order not to have any influence on solution variables.


CWE studies are usually done using commercial software such as ANSYS FLUENT, CFX, Star-CD, and others, or publicly-available codes, such as OpenFOAM, and rarely with codes developed ‘in-house’. There are three parts in every CWE study. The first part is called pre-processing. In the preprocessing stage, the definition of the problem, the method of simulation, the computational domain and the mesh generation will take place. The second step is simulation, computing. At this stage, some of the following steps are required to be implemented:

  • Computational resources: It is necessary to know the computing resources available. Without a proper consideration of the resources available, it is not possible to have a simulation. The size of the mesh directly goes to the memory capacity, and the processing time goes to the processor capacity, parallel computing capability and available processors. Adjusting the simulation requirement and what can be achieved with the available resources is the first step of a simulation. This decision is part of the pre-processing.
  • Time dependence: The study can be steady or unsteady simulation. Unsteady simulation is advanced in time using explicit or implicit time stepping. The order of accuracy can be of first order at the initial stage of the simulation for stability consideration and then be changed to a second-order approximation.
  • Level of accuracy: Numerical approximation introduces various errors at different levels of modelling and solution process. It is necessary to determine acceptable error for simulation and to tune the model accordingly. The numerical error can be the round-off error depending on whether single or double precision is used; the iteration error is needed to determine an acceptable convergence level; the mesh dependent error requires the solution to be independent of mesh density.
  • Initialization: The computational domain needs to be initialized to start an iterative process towards a solution. This initial value is very important in reducing computing time, stability and arriving at an accurate solution any approximate value can be used for the initial condition extending the boundary condition. First stage modelling uses first-order discretization, and one- or two-equation turbulence models can be used as initial condition for higher level modelling or unsteady simulation to achieve more stable solution and reduced time.
  • Solution monitoring: During the iterative process in steady or unsteady state simulation, the changes in solution variables are recorded to determine the convergence level. However, reducing the iteration error by order of magnitude may not always give accurate solution. Thus, monitoring solution variables at a few locations in the domain will add the confidence level and protect from unrealistic solution.
  • Data recording: During a solution process, solution variables can be recorded. For steady state simulation, recording during the solution process will help to use the data to continue the simulation, in case of unforeseen interruption or any other situation. For unsteady state simulations, recording of selected data, in addition to some full data, will help to analyse the time dependence of the solution variables.

Data Analysis and Results (Post Processing)

The advantage of CWE over experiments is the amount of data available. Processing data at the end of a simulation, or during the solution analyses, is called post-processing. Post-processing provides an insight into results of a CWE simulation. Post-processing can be the presentation of data by vector and contour plots, such as, 2D plots, animation, graphs and charts. The following are the main post-processing activities, according to the desired flow characteristics that need to be extracted from a solution:

  • • Calculation of integral parameters,
  • • Calculation of derived quantities,
  • • Data analysis by statistical tools,
  • • ID data plots of a variable trend,
  • • 2D contour and vector plots,
  • • 3D plots of iso surfaces and volumes,
  • • Particle tracing and animation.

Quality Assurance

Quality assurance is another important step in any CWE study, and the uncertainty in solutions is reduced by the use of a quality assurance procedure. There are a number of sources of advice on each step of a CFD study such as those by AIAA G-077-1998 (2002), AIJ (2006) and Franke et al. (2004, 2007). In addition, the procedures in Sections 16.3 and 16.4 can be adopted to ensure the quality of a CWE results. The following are the main considerations for a quality assurance process:

  • Computational domain: The computational domain needs to be in the recommended range.
  • Mesh: The density of mesh in a high-gradient area is critical, with very high stretching of a mesh often necessary. The solution should be mesh independent; thus, solutions of different mesh sizes need to be compared.
  • Level of uncertainty and error: The simulation incurs different levels of error, round-off, iterative, modelling and discretization. All errors have to be listed.
  • Assumptions: The modelling and solution process contain various assumptions. These assumptions needs to be listed.
  • Turbulence model: The choice of a turbulence model for a given problem can be very important. A solution should not be highly influenced by the type of turbulent model used.
  • Boundary conditions: Boundary conditions have a big influence in a solution. Thus, the solution needs to be scrutinized for the extent it is influenced by a boundary condition and if it is within the acceptable level.
  • Time step: Unsteady simulation marching in time and the total computational time has to be reported. Is the total time of simulation sufficient enough to characterize a flow? Is the time step taken reasonable? This question raised at the initial stage of modelling needs to be considered again.
  • Verification: The above points for quality assurance can be established through numerical verification. In addition to the numerical verification, comparing them with experimental data should be considered in all cases when opportunity is available.
  • Independent evaluation (peer review): The use of an independent reviewer, not involved in a modelling and solution process for the full modelling, solutions and post-processing process is important.

  • [1] K-omega, К-со (two-equation model)-. The standard K-omega modelrequires solution of two transport equations based on turbulencekinetic energy and specific dissipation rate (Wilcox, 1998). The modelincludes low Reynolds number effect, compressibility and shear flowspreading. It is sensitive for values outside the shear layer (ANSYSInc., 2020). There are variations of the original model which improvesits performance. • Transition K-Kt -(O (three-equation model): This model usesthree transport equations to predict boundary layer development.The transport equation uses turbulent kinetic energy (K), laminarkinetic energy (Ki) and inverse turbulent time scale (w) to establishthe transition of the boundary layer from a laminar to a turbulentregime.
< Prev   CONTENTS   Source   Next >