Hi everybody:

Summary: My question is: How to avoid a non-physical growing of k and wiggles of all variables near the wake cut in a structured C-Mesh when using a 2D NavierStokes code with k-w turbulence model?

I am implementing a k-w turbulence model for a 2D Navier Stokes code (structured mesh, finite differencing scheme Beam&Warming+ADI, C-mesh around the airfoil). Near the wake cut boundary (where I just compute the mean of upper and lower values of variables explicitly after each step) there is a great production of k, and fluctuations of rho, rho*u,...Those wiggles don't cause troubles when using Balwin-Lomax or Spalart-Allmaras models, but the two equation model seems not to work properly due to them. Please, did you find this problem before? If you know the way to avoid it, or if you could help me with anything useful, THANKS!

Respeced sir,

I am an undergraduated engineering student doing a project on "development of a 2-D post processor for CFD applications".I do not have enough data to enhance my inroducion. So if you could plese send me some information on Introducion to CFD I would be much obliged to you as it would be of infinite help o me in completing my report.

Thanking you ,

Yours gratefully,

Rakesh.B.N

(1). For algebraic turbulence model like Baldwin-Lomax model, the eddy viscosity is calculated from the velocity field (or vorticity). (2). On the other hand, the two-equation turbulence models require the solutions of the TKE-equation and TKE dissipation equation. Sometimes, this set of equations require different solution procedure to obtain the converged solution. So, sometimes, it is a good idea to solve this set of equations separately. (3). The wake flow of an airfoil can have vortex shedding behavior, or transonic oscillation in it. It depends on the Mach number and the trailing edge geometry. (4). The mesh in this area also can have direct effect on the stability of the solution. (5). I would suggest that you try a case with symmetric airfoil having zero trailing edge thickness to avoid the effect from the geometry first. If it still does not work, then a finite flat plate wake flow problem should be tested to find out whether it is due to the turbulence model or the numerical method.

If the wiggles becomes larger and larger as the flow goes downstream, most probably, I think that the spatial size near the wake cut in normal direction of the mainstream is too large because 2-eq model requires finer grids than 0-eq and 1-eq models. Don't change the spatial size too rapidly in both directions, especially in the normal direction.

Z. Lei

Dear David I have not used k-w model so far, although I have a little knowledge about it. I wonder if your calculations are suffering from the liberties you have in specifying the boundary conditions of w. Menter(1994) (AIAA J., Vol.32, No.8, pp.1598-1605) has shown the dependance of Wilcox model on the boundary conditions of w. If you check it please let us know about the result.

Dear John:

Thanks for your reply. After reading it, I have tested the model with a different mesh and different conditions (transonic and subsonic). What I find is that not only in the wake cut, but in any part of the mesh where the grid spacing is small and jacobian changes rapidly (near leading and trailing edge) there is strong oscillation and growing of k. K shows strong mesh dependence, then I will have to review discretization of k-w equations. Things are worse in the wake cut, where it appears some discontinuity of variables before reaching convergence. I will test k-w model with a no-turbulence converged case, and I will freeze fluid variables only allowing turbulent variables to change.(as I don't know how to impose boundary condition inside the fluid cut for a better behaviour during the convergence!)

David

(1). Looks like that the formulation is sensitive to the mesh quality. (2). In general, FDM is more sensitive to mesh quality than the FVM. In certain region of mesh, you can set the stretching equal to one, to avoid the problem. In the area where you need the mesh stretching, try to keep the stretching factor less than 1.2 . (3). The idea is to isolate the problem, so that you can work out a solution.

Dear Dr. Sana:

Thanks for your reply. I know a 'little problem' of k-w model that makes it useless for practical purposes, unless you introduce cross-difussion term inside equations, proposed by Menter, in order to make it not so dependent of freestream B.C. I haven't done it yet, but I will do it, as research institutes advise using Menter's modified k-w better than Wilcox k-w. As soon as I test it, I will tell you about it.

Concerning with w: either using rugosity to define it near the wall as Menter does and having a good grid spacing in sub-viscous layer, or introducing analytical solution in sub-viscous layer directly as Wilcox proposes (but then the code is grid dependent), I found a good agreement with experimental data not only in sub-layer but also in log-layer.

David

Dear Zhong Lei:

Thanks for your answer. Maybe that is the problem, cause I have run the code with another mesh and shows that where there is fine grid (and spacing changes rapidly) is where k and turbulent viscosity explodes.

David,

I hope you get this one sorted out because I have had the same problem with k-w. I have run it in comparison with k-e for a variety of standard flows and often get the same explosion in k with the k-w but k-e behaves okay. I have run pipe flow, 2D mixing layer, plane jet. I have been over and over the transport equations and can find nothing amiss. These equations are very similar to k-e so its hard to believe that they are wrong. I am using a 3D formulation of the SIMPLE algorithm. Good luck. Larry