3.2.2.3 Advanced

Advanced

In this section of the dialog box, you decide whether you want to Consider turbulence. The effects of turbulent flow are characterised by chaotic changes of pressure and flow velocity (see the Chapter 'Turbulence'), contrasting laminar flow. As the air represents a "fluid" with low viscosity, excessive kinetic energy overcomes the damping of the fluid in areas with increased velocity.

The Model of turbulence can be based on the correlations between k and epsilon or between k and omega. The first option is set as default. Depending on the selection (see image to the left), you can specify either the turbulent dissipation rate ε or the specific dissipation rate ω. In general, the simulation using k_ω is more universal and more robust than the one using k_ε. The k_ε model of turbulence, though, gives better results for specific locations such as zones close to surfaces.

If you select the Calculate k-ε parameters from the intensity of turbulence option, you can define the intensity I as a percentage (ratio of root-mean-square of the turbulent velocity fluctuations and the averaged velocity at the same location over some time period) in the text box below.

The [Profile] button enables you to define the turbulence intensity as a function of the height. You can enter the chart values as described in the Chapter 'Wind Profile' above. The turbulent kinetic energy k and the turbulent dissipation rate ε (or the specific dissipation rate ω, respectively) are then determined by the program. Alternatively, you can define the parameters k and ε (or ω) manually as soon as you have cleared the option mentioned above.

An idealised flow of air with absolutely no fluctuations in air speed or direction would have a turbulence intensity value of 0%. For high-turbulence cases, the turbulence intensity is typically between 5% and 20% (see CFD Online). The turbulence intensity is set to 1% by default to cover most medium- and low-turbulence cases.

If the texture of the model surfaces has a major effect on the results, activate the Consider surface roughness check box. The roughness will then be taken into account for every surface of the model. Specific boundary conditions are applied to the surfaces or zones, providing surface constraints on the turbulent viscosity to account for roughness effects.

The approach to surface roughness in CFD models is described in the OpenFOAM User Guide.

For the program to determine the turbulent viscosity near the surfaces, the Sand-grain roughness height Ks needs to be specified. You can define the size of the sand grains in the text box. Note that the value is to be entered in meters.

The Roughness constant Cs controls the shape and spacing of the sand grains. This parameter is set as 0.5 by default, assuming a homogeneous distribution. If there is a non-uniform roughness, though, C_s can be increased up to 1.0.

The steady-state solver of RWIND Simulation does not fully capture "oscillating" effects as described in FAQ 4731.

In order to solve partial differential equations numerically, all differential terms (space and time derivatives) have to be discretized. There is a vast list of discretizations ("schemes"), with each scheme having its particular numerical behaviour in view of accuracy, stability and convergence.

The Use second-order numerical scheme check-box controls which numerical scheme is used for divergence terms (fluxes). It is not activated by default so that the calculation is carried out according to first order. If the check box has been selected, the solution is performed according to second order.

Basically, the order of the scheme indicates how accurate the numerical solution when compared to the solution of the original non-discretized equations is: