CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   komega turbulence model (http://www.cfd-online.com/Forums/openfoam/96350-komega-turbulence-model.html)

ahmed_khatibs January 20, 2012 05:19

komega turbulence model
 
hallo All,
I'm having a little trouble setting up the case in OpenFOAM 1.7 using k-omega SST turbulence model.
What are I need to define (Boundary Condition) for k-omega turbulent model in OpenFoam so as model has to compare with Ansys-Fluent (k-omega standard turbulence model).
Or
which solver I need to take in OpenFoam for compare with Ansys-Fluent (k-omega standard turbulence model).

Thank you

romant January 20, 2012 06:07

You will have to decide if you want to run the model in low Reynolds number mode or in high Reynolds number mode. The difference is to have the first cell y+<1 or between 30 and 100. You can then use the following boundary conditions

for low Reynolds mode
Code:

k:
all walls

type fixedValue;
value 1e-10;

omega:
all walls

type omegaWallFunction;

nut:
all wall

type nutLowReWallFunction;

high Reynold number mode
Code:

k:
all walls

type kqRWallFunction;

omega:
all walls

type omegaWallFunction;

nut:
all walls

type nutkWallFunction;

in case for the nutkWallFunction, there are different nut wall functions available, which you have to chose yourself in case you have a rough wall or some special wall behavior.


All times are GMT -4. The time now is 16:15.