Hello everyone,
I'm simulating a 2D flow past a I-beam using k-omega SST turbulence model and I'm having some trouble with the mesh (I guess). I've managed to get a solution with periodic vortex shedding, but I'm not very satisfied with my mesh.
I need very small elements near the beam flange (figure 2), but these elements keep its size through the entire domain along its horizontal line (figure 3). Therefore, I get some high aspect ratio cells as we get far away from the beam.
In addition to that, I once made a finer mesh with maximum y+ near 30, and the solution just blew up. As you can see from figures 4 to 7, there was a big problem with those high aspect ratio cells.
I had a new mesh idea (figure 8), but I'm not pretty sure if it's a good one.
Finally, my questions are:
1. Is it a mesh problem indeed?
2. Does anybody have some ideas how I could improve the mesh?
Thanks in advance.
P.S.: Boundary Conditions:
Inlet: velocity fixed value (1 m/s), pressure zero gradient;
Outlet: velocity zero gradient, pressure fixed value (0);
Beam: no slip wall;
Top and bottom walls: free slip
Your first grid appears to me much better than that reported in Fig.8. I don't think that you have a grid problem, first I suggest to let the flow develop for a sufficiently time to forget the intial condition. The fact that the solution on a finer grid blow up is more likely a numerical stability problem. Try to check the stability constraint.
However, this is a typical flow problem for which URANS can be problematic.
In case you have no restriction, you may obtain more acceptable results for the problem employing unstructured mesh(triangular elements) with sufficient inflation layers on the walls. You will have more controlled mesh density and growth rate.
Good luck!
Thank you all for the replies.
Filippo, I did so many tests with the interpolation schemes trying to increase stability and I used the "best" parameters I found in this simulation.
Mahdi, I have to use hexahedral mesh =)
You should provide all the details about your formulation, discretization, time integration... Apparently, the pressure field seems to have numerical wiggles, not a physical vortex shedding. Could you post the velocity field?
Then, I suggest starting with a laminar flow to check if the code run at lower Reynolds number without any turbulence model. You should see a vortex shedding also in laminar unsteady conditions.
In fact, I did manage to get a solution (With a coarser mesh and larger domain, I attached some figures), just want to know your opinion if everything seems "alright" or is there any way I could improove it.
I used the following schemes:
ddtSchemes: CrankNicolson 0.5;
gradSchemes: leastSquares;
divSchemes:
div(phi,U) Gauss linearUpwind grad(U);
div(phi,k) Gauss upwind;
div(phi,omega) Gauss upwind;
div((nuEff*dev2(T(grad(U))))) Gauss linear;
laplacianSchemes: Gauss linear orthogonal;
interpolationSchemes: linear;
snGradSchemes: orthogonal.
P.S.: I added the velocity field of the problematic simulation in the original post.
The velocity field appears quite regular (what is the Re number?), looking very smoothed by the numerical diffusion of the upwind along with the action of the turbulence model. But, as I wrote above, I suggest running first a laminar case without turbulence model.
Reynolds number = 275000, considering the beam height as the characteristic length
- Badges
- Science topic