SolidWorks Flow Simulation: Internal Variable Velocity Inlet Boundary Condition

     This post is about an internal computational fluid dynamics simulation. The Simulation was performed in a pipe with a diameter of 1 in. The length of the inlet was 8 in away from the intersection. The two outlets were 4 in away from the intersection and were at an angle of 120° from the inlet, respectively. The flow entered the pipe in pulses with a period of 0.2 s. The peak velocity was at 2 m/s and the minimum velocity was kept at 0 m/s. This simulation setup can be analogous to the opening/closing of an IC engine valve simulation or simulation of cardiovascular systems etc.

     The part used in the simulation and the simulation setup is available here, as shown in Fig. 1.

Fig. 1, Part geometry.

 

     The mesh is shown in Fig. 2. The simulation assumed 2D simplification, to save time and computational resources. The mesh had a total of 15,512 cells. A simulation time step of 0.00625 s was employed.

 

Fig. 2, The computational mesh.

 

     The velocity profile at 0.9 s is shown in Fig. 3.

 

Fig. 3, Velocity Streamlines colored by velocity magnitude, superimposed by velocity vectors.

 

     An animation of the results is shown below. The results are, indeed, mesh and time independent.

 

 

     Thank you for reading. Reach out to collaborate in research projects.

Computational Fluid Dynamics (CFD) Analysis of a Horizontal Axis Tidal Turbine (Update 01)

     In this post, the results of numerical simulations carried out on a three-blade horizontal-axis tidal turbine blades are made available. These simulations are a part of larger project relating to a horizontal-axis tidal turbine.

 

     The turbine under investigation had a diameter of 4 m. The aero-foils employed include the NACA 4424 (chord length 0.25 m), NACA 4420 (chord length 0.2312 m), NACA 4418 (chord length 0.2126 m), NACA 4417 (chord length 0.1938 m), NACA 4416 (chord length 0.175 m), NACA 4415 (chord length 0.1562 m), NACA 4414 (chord length 0.1376 m), NACA 4413 (chord length 0.1188 m) and the NACA 4412 (chord length 0.1 m) at a distance of 0.4 m, 0.6 m, 0.8 m, 1 m, 1.2 m, 1.4 m, 1.6 m, 1.8 m, 2 m from the blade root, respectively [1].

 

     The numerical simulations were carried out on SolidWorks Flow Simulation Premium software. The software 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. To predict turbulent flows, the Favre-averaged Navier-Stokes equations are used. The software employs a Cartesian mesh which is created using the immersed boundary method.

 

     The simulations were carried out using the Local rotating region(s) (Sliding) technique. The mesh had a total of 589,763 cells. 132,045 cells were at the turbine blade-rotating region boundary. While the process of mesh generation, a mesh control was employed to refine the mesh near the turbine blades and at the boundary of the rotating region and the stationery computational domain. To refine the mesh for the mesh independent test, the curvature level was increased i.e. the mesh in the areas of interest was refined by a factor of 8. As a result, the refined mesh had a total of 916,577 cells. A total of 221,978 were present around the turbine blade. The computational mesh around the turbine blade is shown in Fig. 1. The refined mesh in the areas of high gradients is also clearly visible. The computational domain had dimensions of 2D x 2D x 2.4D, where D is the diameter of the turbine. The dimensions for the computational domain resemble to those in [2].

     Fig. 2 shows computational domain around the turbine blades. In Fig. 2, the curved teal arrow represents the direction of rotation of the turbine. The green arrows represent the respective co-ordinate directions. The brown arrow represents the direction of the force of gravity. The blue arrow represents the direction of the fluid velocity. The circular disc represents the rotating region.

 

Fig. 1, The computational mesh.

    

Fig. 2, The computational domain and the orientation of the boundary conditions.

 

     The simulations were carried out for a total of 5 tip-speed ratios for the turbine ranging from 2 to 10. The fluid; water, velocity was set at 2 m/s. The results are indeed, mesh independent. The mesh independence test was conducted on the design point of the turbine i.e. at the TSR of 6. The plot between the turbine tip-speed ratio; TSR, and the co-efficient of power is shown in Fig. 3. It can be clearly seen from Fig. 3 that the results are in close agreement with the results from [1, 3]. The CFD results from both studies are lower then the BEM, Blade-Element Momentum, results because the three-dimensional effects are not considered while implementing the BEM method.

 

Fig. 3, Turbine efficiency plot.

 

     Fig. 4 shows velocity streamlines colored by velocity magnitude, both of these features are drawn relative to the rotating reference frame, around the turbine blade cross-section at various tip-speed ratios. It can be seen from Fig. 4 that the turbine stalls at TSR of 2 due to a large positive angle of attack. It can also be seen that as the TSR increases, the angle of attack on the blade decreases, it is because of this reason that the power output from the turbine increases.

 

 

Fig. 4, Row 1, L-R; TSR of 2 and 4. Row 2, L-R; TSR of 6 and 8. Row 3, TSR of 10.

 

     Thank you for reading. If you would like to collaborate with research projects, please reach out.

     [1] Binoe E. Abuan, and Robert J. Howell, "The Influence of Unsteady Flow to the Performance of a Horizontal Axis Tidal Turbine," Proceedings of the World Congress on Engineering. London, 2018.

     [2] Ibrahim, I. H., and T. H. New, "A numerical study on the effects of leading-edge modifications upon propeller flow characteristics," Proceedings of Ninth International Symposium on Turbulence and Shear Flow Phenomena. Melbourne, 2015.
     [3] Bahaj, A., Batten, W., & McCann, J. (2007). Experimental verifications of numerical predictions for the hydrodynamic performance of horizontal axis marine current turbines. Renewable Energy, 2479-2490.

Update 01:

     CFD post processing added. One more TSR simulated.