[g7fernandes]

I am new OpenFoam user I want to do something very simple:
There is a 2d pipe and in the middle there is a porous wall.
I used blockmesh with 3 blocks with equal sizes and the block in the middle should be the porous media.

How do I indicate to OpenFoam that there is a porous region?

I read about CellZone and Setset, but I can't find exactly what must I write and were

I'm using porousSimpleFoam and blockMesh.

If someone has the codes for such simulation to share, I and the Internet will be very thankfull to you and many people in the future will love you.

The "tutorials" that come with openFoam are very unclear.

[Antimony]

Hi,

Look at the topoSet utility: https://github.com/OpenFOAM/OpenFOAM...et/topoSetDict

You can define your cellZone using that. There are multiple options: boxToCell, cylinderToCell etc that you can use to get your cellZone.

Cheers,
Antimony

[g7fernandes]

Thank you for your reply!

I created the file topoSetDict and I put it in /system

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      topoSetDict;
}


actions
(
    // Load initial cellSet
    {
        name    porosity;
        type    cellSet;
        action  new;
        source boxToCell;
        sourceInfo
        {
            box (20 0 0) (40 20 1);
        }
    }
);

With this mesh

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.001;

vertices   // points in the flow space
(
    (0 0 0)  // 0
    (20 0 0)  // 1
    (20 20 0)  // 2
    (0 20 0)  // 3
    (0 0 1)  // 4
    (20 0 1)  // 5
    (20 20 1)  // 6
    (0 20 1)  // 7
    (40 0 0)  // 8 
    (40 20 0)  // 9 
    (40 0 1)  // 10
    (40 20 1)  // 11
    (60 0 0)  // 12 
    (60 20 0)  // 13 
    (60 0 1)  // 14
    (60 20 1)  // 15
);

blocks
(
    hex (0 1 2 3 4 5 6 7) (30 30 1) 

// the order of the numbers in hex ( ) defines the vertices of the tetrahedron (region of flow)
// Important: The first two digits in hex ( ) defines x-direction, the first and the third 
//            defines the Y, and the first and the fifth defines the Z 

    simpleGrading (1 1 1)  //defines the grid 

    hex (1 8 9 2 5 10 11 6) (30 30 1)
    simpleGrading (1 1 1)  //defines the grid 

    hex (8 12 13 9 10 14 15 11) (30 30 1)
    simpleGrading (1 1 1)  //defines the grid 

);    

edges  // used in the case of drawing curves
(
);

boundary   // names the faces 
(
    inlet
    {
        type patch; 
        faces
        (
            (0 3 4 7)  //face determinated by this vertices is the inlet
        );
    }


    outlet
    {
        type patch;
        faces
        (
            (12 13 15 14)
        );
    }

    walls
    {
        type wall;
        faces
        (
            (0 1 5 4)
            (2 3 6 7)
            (8 12 14 10)
            (9 13 11 15)
        );
    }    

    porosityWall
    {
        type wall;
        faces
        (
            (1 8 5 10) //
            (2 9 6 11) //
        );
    }

    frontAndBack
    {
        type empty;
        faces
        (
            (0 3 2 1)
            (4 5 6 7)
            (5 10 11 6)
            (1 8 9 2)
            (8 12 13 9)
            (10 14 15 11)
        );
    }

);

mergePatchPairs
(
);

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

but I get this error when I run porousSimpleFoam

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 3.0.1-119cac7e8750
Exec   : porousSimpleFoam
Date   : May 18 2016
Time   : 14:12:17
Host   : "ubuntu-mate-1510"
PID    : 29189
Case   : /home/ofuser/OpenFOAM/ofuser-3.0.1/run/sq_porous
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0


SIMPLE: no convergence criteria found. Calculations will run for 100 steps.

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    C3              -0.33;
    sigmak          1;
    sigmaEps        1.3;
}

No MRF models present

Creating porosity model list from porosityProperties

Porosity region porosity1:
    selecting model: DarcyForchheimer
    creating porous zone: porosity


--> FOAM FATAL ERROR: 
cannot find porous cellZone porosity

    From function Foam::porosityModel::porosityModel(const Foam::word&, const Foam::word&, const Foam::fvMesh&, const Foam::dictionary&, const Foam::word&)
    in file cfdTools/general/porosityModel/porosityModel/porosityModel.C at line 121.

FOAM exiting

What I'm doing wrong?

[Antimony]

Hi,

At the moment it is still a cellSet, not a cellZone. You will need to do one more step in your topoSet to get that. Look for setToCellZone to do the conversion.

Hope this helps.

Cheers,
Antimony