[wei_wu]

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

[santos]

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.

[wei_wu]

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

[henrik]

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

[wei_wu]

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