Hello everyone, Happy Thank
 

Hello everyone,

Happy Thanksgiving for foamers!

I'm running the simulation for the circular cylinder flow.I'm using turbFoam solver which is recompiled to make it time-adaptive based on the max courant number. I found some problems when I set up the fvScheme dictionary. For the divScheme, the solver doesn't allow me to set default to "Gauss QUICK "or"Gauss upwind",it'll give

***********************************
Starting time loop

Time = 0.005

Courant Number mean: 0.00915807 max: 0.240009


attempt to read beyond EOF

file: /home/wuwei/OpenFOAM/wuwei-1.5/run/g2-scheme/system/fvSchemes::default at line 39.

From function ITstream::read(token& t)
in file db/IOstreams/Tstreams/ITread.C at line 64.

FOAM exiting

*****************************************

when I set it to "Gauss linear", it'll work.

Does anybody know the reason for this?

Thank you in advance.


Wei

Hello Wei, Check if you hav
 

Hello Wei,

Check if you have missed a ; at the end of the line.

You should have something like:
div(phi,U) Gauss upwind;

If it doesnt help, please post here your fvSchemes file.

Hi,Jose Thank you for your
 

Hi,Jose

Thank you for your reply.
I checked for the file I didn't miss a ; at the line.

here is my fvSchemes file, please check it for me, thanks

//**************************************************
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.4 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

FoamFile
{
version 2.0;
format ascii;

root "";
case "";
instance "";
local "";

class dictionary;
object fvSchemes;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
default CrankNicholson 1.0;
}

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

divSchemes
{
default Gauss upwind;

}

laplacianSchemes
{
default Gauss linear corrected;

}

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

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}
//************************************************** ***


after I executed the turbFoam command, it told me that

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
alphaEps 0.76923;
}


Starting time loop

Time = 0.005

Courant Number mean: 0.00915807 max: 0.240009


attempt to read beyond EOF

file: /home/wuwei/OpenFOAM/wuwei-1.5/run/g2-scheme/system/fvSchemes::default at line 39.

From function ITstream::read(token& t)
in file db/IOstreams/Tstreams/ITread.C at line 64.

FOAM exiting
************************************************** *******
line 39 is the one says "default Gauss upwind;"

if I change it into " default Gauss QUICK;"
same thing happens,but if I change it into "default Gauss linear;" , the code can run nicely.



Thank you

Most interpolation schemes inc
 

Most interpolation schemes including Upwind and QUICK require a flux, therefore you say

default Gauss upwind phi;

Read sections 4.4.5 and 4.4.1 of the User Guide for more information on this topic.

Henrik

Thank you so much, Henrik. It
 

Thank you so much, Henrik.
It worked after I added the " phi".