[immortality]

in mutkWallFunctionFvPatchScalarField the equation uses for y-plus is related to y-star not y-plus

Code:

y-star=pow(0.09,0.25)*sqr(k)*nearDist()/mu

Code:

y-plus=rho*u_star*y/mu which u*=aqrt(taw_w/rho)

y-star is related to turbulent kinetic energy while y-plus relates to friction velocity(that relates to wall skin friction in its own)

in the code of mut
:
Code:

forAll(mutw, faceI)     {         label faceCellI = patch().faceCells()[faceI];          scalar yPlus =             Cmu25*y[faceI]*sqrt(k[faceCellI])/(muw[faceI]/rhow[faceI]);          if (yPlus > yPlusLam_)         {             mutw[faceI] = muw[faceI]*(yPlus*kappa_/log(E_*yPlus) - 1);         }     }

thanks.

[vikramaditya91]

I believe I am very late to the party. I am currently using the OpenFOAM 2.4.0 and I have to say that they still have not made any changes to the code, even though I believe it would not be a involve a lot of coding. There was a post on the official openFOAM page, in case you might want to have a look, here it is http://www.openfoam.org/mantisbt/view.php?id=835

Well i was using the code Niklas had made, but I believe it requires a correction. Of course it needed to be edited slightly for the OpenFOAM 2.4 but that is not the correction I am talking about.
When it calculates the sqrt(viscosity*gradient of velocity), it has to consider the sum of kinematic viscosity+turbulent viscosity , but he has only used the turbulent viscosity (mut.boundaryField()[patchi]).
Practically, the turbulent viscoisty can be ignored and we are only left with the kinematic viscosisty. Very close to the wall i.e y+<3, the turbulent viscosity is negligible since it lies in the viscous laminar sub layer where there are negligible turbulent effects. The line I am talking about would be 3rd in the code attached which is from his Niklas's code.

yPlus.boundaryField()[patchi] = 
            y[patchi]           * sqrt              (            
mut.boundaryField()[patchi]       
   *  mag(U.boundaryField()[patchi].snGrad())       
   /  rho.boundaryField()[patchi]                 )     
      /  (RASModel->mu().boundaryField()[patchi]
/rho.boundaryField()[patchi]);

I would like to hear what you guys think about it. have a look at this for reference. Check out the section near equation (21) in this page http://www.cfd-online.com/Wiki/Intro...urbulent_flows