Hi Dear Friends,

In recent days, I have been simulated a Jet on flat surface by usind Low Re K-Epsilon model of Yang-Shih. The convective terms in the Reynolds equations were trated by SMART tecnique, and that the K-Epsilon model I used to first order UPWIND. I have noted that the calculations are strongly dominated by numerical difusion. Also, I used y+>>1.1 (perhaps 300). My question is:

Is the poor spatial resolution the problem?

Thanks. Valdemir.

(1). Normally there are two problems. (2). One is the turbulence model used, and the other is the coarse mesh used in the solution. (3). For the turbulence model part, you can check it out under simple environment to determine the mesh density, and the boundary conditions required to provide accurate solution. This will give you some ideas about the total number of mesh points or cells needed for accurate solution. (4). For the coarse mesh problem, all you need to do is to refine the mesh systematically until the solution is no longer changing as a function of the mesh density. (5). So, before one can answer your questions, you need to those two exercises first. (6). Also check the model specifications to see if the boundary condition is implemented properly. I have no idea whether Y+=300 is a good number for the turbulence model you used. (7). By the way, how do you know that the calculations are strongly dominated by the numerical diffusion? I mean, what kind of solutions will show strong numerical diffusion?

Dr. John C. Chien, Thanks for your considerations. About the question ``how do you know that the calcutions are strondly dominated by the numerical diffusion'', I have comparated whit the solution of the standard K-Epsilon model. By using the this model (standard), I have noted that the fluid layer on the flat surface is much more thin than that Low K-Epsilon model. Also, the number of the surface cells is great than the number of surface cells in the Low K-E model. This qualitatively behaviour supported my conclusion. In adition, perhaps the upwind method for the convective terms in the K-Epsilon equations was the problem.

Thanks. Valdemir.

(1)Were you saying that your first mesh point is Y+>=1.0 (around 300) ? when using the low Reynolds number model? (2). In general, you need to use Y+ <= 1.0 for the first mesh point when using the low Reynolds number model. Y+ =300 may be good for standard k-epsilon model (with wall function treatment). (3). But then I am not familiar with the particular model you used.

Yes, in fact, my Y+ is around 300. I have the impression that a Low Reynolds K-Epsilon model is valid in every place of the domain. The particular model uses a new time scale that is, the Kolmogorov time scale plus that of the standard K-Epsilon model. This Y+ is very good for standard K-Epsilon model, but I think it not correctely solves next to the wall. So, it is possible that the lack of resolution is the problem. In other words, the fluid layer is much diferent from that of the Standard K-E model.

1) I do agree with John. Whenever you are integrating to the wall, regardless of the turbulent model, your first node y^+ has to be within laminar sublayer, i.e. less than 4. That is to capture the right velocity profile at the wall.

Thanks. Mohammad