[johnblund]

Hi,

I am modeling atmospheric flows using a standard KE model. I have had some problems reproducing earlier results from e.g Hargreaves and Wright (2006) and Blocken et.al (2007)

I am sure that the differences are caused by different wall functions being applied, as I am sure inlet profiles are correct.

I have identified the wall functions used for k and epsilon (kqRWallFunctionFvPatchFIeld.C and epsilonWallFunctionFvPatchField.C), but I cannot find the wall function for velocity.

I want to make sure that the velocity is set according to the logarithmic law in the wall adjacent cells. I am only able to see that it is set to zero at the wall in the 0/U-file.

Does anyone know how the velocity is set in the wall-adjacent cells? And an easy way of defining a wall function for velocity close to the wall if it does not exist allready.

kind regads
John

[hectorgabriel85]

I cannot find wall function for velocity U in OpenFOAM. I am aware Fluent uses wall law for the velocity and not only for k or epsilon or omega.

[daylen]

is there a wall function in openFoam for velocity? if i put wall functions for k, nut and omega for k omega sst, how is velocity calculated? and how pressure is calculated? pressure needs a wall function or not? in openfoam tutorials velocity has noSlip and pressure zeroGradient, is this good enough when simulating using wallfunctions?

[SadBoySquad]

OpenFOAM indeed does not have wall functions explicitly for velocity. This is a matter of how OpenFOAM treats wall functions.

The desired near-wall behavior is achieved by modifying the turbulent viscosity and, thus, the wall functions are embedded in the turbulent viscosity boundary conditions file (nut) and not in the velocity file (U). Modifying near-wall turbulent viscosity essentially alters the shear stress which in turn will modify the velocity field.

Available boundary conditions (which include wall functions) for nut are described here:
https://www.openfoam.com/documentati...ived-wall.html.

In addition, I am happy to inform you that if you are working on the classic Hargreaves and Wright paper for downstream atmospheric development in a rectangular box, the complete case setup is available in the tutorials folder (at least for OpenFOAM v2112 or newer), since this is a classic validation case:
$FOAM_TUTORIALS/verificationAndValidation/atmosphericModels/atmDownstreamDevelopment