[abhi22]

Hi Ruiyan,

Yes, using vanDriest damping is the standard fix when using constant coefficient Smagorinsky model. See https://www.cfd-online.com/Wiki/Near...for_LES_models

However, using a dynamic model which follows the dynamic procedure of Germano et al. (1991) alleviates this near-wall limitation of the Smagorinsky model. Please refer to Germano's paper https://doi.org/10.1063/1.857955

Other LES models that performs well near-wall is the WALE model.

[cryabroad]

Thank you for the link. I think I will go with the Prandtl one because it (at least) looks similar to what ANSYS Fluent is using.

According to Fluent's manual, in the Smagorinsky-Lily model they are using, the eddy-viscosity is modeled by mu_t = rho* L_s^2*S with S being sqrt(2*Sij*Sij). L_s is determined by min(k*d,Cs*delta), where k is the von Karman constant, d is the distance to the closest wall, Cs is the Smagorinsky constant, and delta is cell volume cubed.

Fluent also recommends dynamic Smagorinsky model, but it seems like OpenFOAM doesn't have one, or at least an official one. The reason I'm using Fluent as a sort of "reference" is that I've been using it before for quite a long time and in general it gives satisfactory results.

[cryabroad]

Hi Abhi, hope you are doing well! I'm back with another question related to the LEMOS inflow generator.

I used this boundary condition to simulate flow inside a pipe with added passive scalar. What I found is that, other than the 0 folder, the refField, RField and R in the other time folders are all displayed as nonuniform List<scalar> instead of what they should be (like nonuniform List<vector> for refField and nonuniform List<symmTensor> for RField). Only the value entry is correct though, with nonuniform List<vector> in all the folders.

The reason I find this important is because in some files, I have very large and very small values in the resulting folder with the wrong data type, like +7e+200 for R at one cell, and I think those eventually cause my simulation to diverge.

Any ideas how to fix this kind of problem? Many thanks.

[cryabroad]

Here is a little tip I myself find useful.

When using the LEMOS inflow generator, to let my customized solver recognize this boundary condition, I included the header file (and associated libraries) when compiling my solver. However, due to some unknown reasons, the inflow generator behaves very strangely. For one thing, the refField for example, changes to type nonuniform List<scalar> instead of nonuniform List<vector>. (The RField and R behaves the same, i.e., their type are changed). For another thing, the values in e.g. refField are either very very small (0) or very very large.

The correct way of using this boundary condition should be, as pointed out in other posts, using

libs ("decayingTurbulence.so")

in the controlDict after compiling the code. This way the generated U file behaves correctly. A list of vortons are also written to the U file with their characteristics (length, location, omega, velocity and xmax), and paraview can read the U file just fine.

Hope this helps those who are using this boundary condition.