[chengyu]

Dear all,

I have compiled SOWFA(https://nwtc.nrel.gov/SOWFA) in OpenFOAM-2.1.0. Following the guide of Matt Churchfield and Sang Lee, precursor simulation using LES is performed for atmospheric boundary layer flow and a plane has been sliced as the inflow boundary condition for the simulation of a single NREL 5MW wind turbine in the plant. During mesh generation, local refinement is adopted around the turbine. Unfortunately virtual numerical vorticity appears after the mesh interface of different density,see the attached figure. Does anybody have suggestions for removing the virtual vorticity?

Thank you for any comment.

[chengyu]

Hi all,
Since nobody has replied to this and I finally manage to solve the problem, I list my method here for the one who occurs the same problem.

1. About the reason: I used central difference scheme before which is less diffusive, the inpolation at the inreface between different levels of meshes causes too much vorticity since nusgs in LES is too small to diffuse it
2. Solving method: As used in many papers(for example:https://www.researchgate.net/publica..._Wind_Turbines), hybrid divergence scheme will help to eliminate the spurious vorticity. Here is the method I had followed: http://www.cfd-online.com/Forums/ope...alblended.html

At last, I attach the final result solved the problem. PS: it seems there is still some error downstream which I think is due to less weight of upwind scheme, I use 10% of upwind.

[bjc8z]

Thank you!!!!!

[Tim_]

Whilst using a blended scheme works well two points. 1st be careful as this will make the solver overly diffusive and you will loose some of the detail within the hub and tip vortices. Second i recommend using the functions in open foam to calculate lambda2 and vorticity rather than using a post processing function in paraview or tecplot.