Wind Turbine SolidWorks Flow Simulation Premium Computational Fluid Dynamics: Verification and Validation

Numerical Methodology

Computational Fluid Dynamics analysis was performed using commercially available code SolidWorks Flow Simulation Premium© in the present study. SolidWorks Flow Simulation Premium© is a CAD embedded CFD tool; employs κ-ε turbulence model with damping functions, SIMPLE-R (modified) as the numerical algorithm and second order upwind and central approximations as the spatial discretization schemes for the convective fluxes and diffusive terms. The time derivatives are approximated with an implicit first-order Euler scheme. The Flow Simulation© solves the Navier-Stokes equations; mentioned below; which are formulations of mass and momentum conservation laws for fluid flows. To predict turbulent flows, the Favre-averaged Navier-Stokes equations are used.

∂ρ/∂t+∂(ρui)/∂xi=0

∂(ρui)/∂t+∂(ρuiuj)/∂xj+∂p/∂xi= ∂(τij+τijR)/∂xj+Si     i=1,2,3

where, Si is a mass-distributed external force per unit mass due to a porous media resistance (Siporous), a buoyancy (Sigravity=-ρgi is the gravitational acceleration component along the i-th coordinate direction) and the coordinate system’s rotation (Sirotation), i.e., Si=Siporous+Sigravity+Sirotation. The subscripts are used to denote summation over the three coordinate directions.

All the simulations were performed to predict three-dimensional transient flow over the wind turbine. The Local rotating region(s) (Sliding) feature within SolidWorks Flow Simulation Premium© software was employed to simulate the wind turbine’s rotation in standard atmosphere.

Validation and Verification

To ensure validation of the numerical methodology, the numerical results of the present study were compared with the experimental results. A total of six tip-speed ratios were selected for the present study, as mentioned in table 1. The NREL Phase VI wind turbine without contra-rotating technology was selected for validation and verification because there is no reliable experimental data available for the NREL Phase VI wind turbine incorporating the contra rotating technology. The operating rotational velocity for the NREL Phase VI wind turbine is 7.5 rad.s-1. The diameter of the wind turbine is 10.058 m.

Table 1; TSR and the corresponding wind speeds

TSR	Wind Speed [ms-1]
7.5	5
5.03	7.5
3.77	10
3.02	12.5
2.52	15
1.89	20

The comparison between the experimentally determined shaft torques and numerical results of the present study, along with the number of mesh cells and the time step employed at various wind speeds is shown in table 2. A comparison of the present study with other studies conducted on the NREL Phase VI wind turbine is presented in Figure 1.

The computational domain selected had a size of 4Dx4Dx2.8D. The computational domain had a large enough volume to accurately trace the fluid flow around the wind turbine and for the solver to operate without any reversed flow or unwanted vortex formation or any other numerical difficulties.

Flow Simulation© considers the real model created within SolidWorks© and automatically generates a Cartesian computational mesh in the computational domain distinguishing the fluid and solid domains. The resulting mesh, employs the immersed boundary method, has three types of cells, namely Fluid cells; the cells located entirely in the fluid, Solid cells; the cells located entirely in the solid and Partial cells are the cells which are partly in the solid and partly in the fluid [22]. The Cartesian mesh with immersed boundary method has certain advantages, like the mesh is very quick to generate and results in high quality elements. The solution converges faster and the mesh distortion and numerical errors are relatively lower. During the process of mesh generation, it was made sure that the region of interest; the region immediately surrounding the wind turbine; had a very fine mesh as compared to the boundaries of the computational domain, to make the simulations converge. The Local Mesh option within the SolidWorks Flow Simulation Premium© software was employed to increase the mesh density in the critical areas.

Table 2; Comparison of the Experimental and Numerical Results

Wind Speed [ms-1]	Experimental Power [W]	Numerical Power [W]	Percentage Difference	Mesh Cells [x105]	Time Step [x10-3 s]
5	2,000	2,043	2.1	3.77	5.41
7.5	6,000	6,105	1.72	3.77	5.41
10	10,000	10,230	2.25	3.77	5.41
12.5	9,500	9,343	1.65	7.79	1.9
15	9,000	7,606	15.49	7.79	1.9
20	8,500	8,696	2.25	9.21	1.96

Figure 1; Comparison of results from present study with previous works

Project Files and Illustrations
     The project files are available here. An illustration of the rotor is provided below.

CFD Post Processing