CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Pre-Processing (http://www.cfd-online.com/Forums/openfoam-pre-processing/)
-   -   Turbulent flow in a rectangular duct foam vs fluent (http://www.cfd-online.com/Forums/openfoam-pre-processing/62147-turbulent-flow-rectangular-duct-foam-vs-fluent.html)

atzaru January 29, 2006 20:26

I am simulating a turbulent fl
 
I am simulating a turbulent flow in a square duct (0.2*0.2*6) in foam and fluent. I am concern about the velocity distribution difference between the two programs.

Reynolds number around 11 000.
in fluent i obtain a max velocity around 1.24 while in Foam the max velocity is 1.14. Does anybody know why and how i can correct this?

in both programs i introduced the same inlet (velocity, V=1m/s), the same initial k and epsilon, and outlet condition.

http://www.cfd-online.com/OpenFOAM_D...ges/1/1724.jpg
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif turb_flow_v2.tar.gz


ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
grad(U) Gauss linear;
}

divSchemes
{
default Gauss <>;
div(phi,U) Gauss upwind;
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div(phi,R) Gauss upwind;
div(R) Gauss linear;
div(phi,nuTilda) Gauss upwind;
div((nuEff*dev(grad(U).T()))) Gauss linear;
}

laplacianSchemes
{
default none;
laplacian(nuEff,U) Gauss linear corrected;
laplacian(1|A(U),p) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(DepsilonEff,epsilon) Gauss linear corrected;
laplacian(DREff,R) Gauss linear corrected;
laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}

interpolationSchemes
{
default linear;
interpolate(U) linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}


The boudary condition are:
(
wall
{
type wall;
physicalType wall;
startFace 97040;
nFaces 6720;
}

outlet
{
type patch;
physicalType pressureOutlet;
startFace 103760;
nFaces 400;
}

inlet
{
type patch;
physicalType inlet;
startFace 104160;
nFaces 400;
}

)

eugene January 30, 2006 08:25

What does the experimental dat
 
What does the experimental data say?

From what information you provided I would guess the source of inconsistency is either the turbulence model or the wall function. Please post which turbulence models and wall options you used for Fluent and Foam. Also, what is your y+ value.

atzaru February 2, 2006 11:51

hello thanks for your reply
 
hello

thanks for your reply

1 - in both programs Foam and Fluent I used the basic k-epsilon equations

2 the standard wall functions based on launder and spalding is used in both cases (the same Constants E =9.0 and kappa=0.4187)

3 The same k-eps coeff have been used cmu=0.009, c1=1.44, c2=1.92. I do not know why in Foam we do not have Tke=1 and TDR=1.3 but a coeff alphaEps = 0.7692. What is this coeff?

4 The y+ is 24

5 For the moment i do not have experimental data to compare with.

It is strange i obtain so different results.

eugene February 2, 2006 12:08

If you are using log the law o
 
If you are using log the law of the wall it is not valid at y+ = 24. My best guess is that fluent does something clever to improve at these intermediate values.

For Foam y+ needs to be around 100 with the standard k-epsilon model.

alberto February 2, 2006 14:28

FLUENT has different requireme
 
FLUENT has different requirements for its wall functions, according to its manual (30 < y+ < 60).

Also, in the OpenFOAM case files there is an error: in the 0\k dictionary the condition at the wall should be

wall
{
type zeroGradient;
}

instead of

wall
{
type fixedValue;
value uniform 0;
}

However it's strange that OpenFOAM 1.2 starts the calculation because it should quit and tell you the error.

Best regards,
Alberto

eugene February 3, 2006 06:01

Unfortunately/fortunately that
 
Unfortunately/fortunately that is one of the features of OpenFOAM. It allows you complete freedom in choosing individual boundary conditions, but at the same time, it wont tell you if you make an unwise choice.

alberto February 3, 2006 11:04

Sorry, I wasn't clear. I disco
 
Sorry, I wasn't clear. I discovered the error because trying to run the case with a grid I did, OpenFOAM 1.2 told me the problem in the BC ;-)

Regards,
Alberto

cesarbz February 13, 2007 15:42

Well... So the problem was jus
 
Well... So the problem was just de grid ? it's the same mesh for both programs?

Another questions...

What is the BC ?
And what represent de y+ value ?

thanks.


All times are GMT -4. The time now is 01:29.