[yurifrey]

Hello!

I want to set a porous zone using fvOptions in OF 2.2.x, but it seems that the solver doesn't read the file.. I created a mesh with two separate zones and this is the first part of the cellZones file:

FoamFile
{
    version     2.0;
    format      ascii;
    class       regIOobject;
    location    "constant/polyMesh";
    object      cellZones;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

2
(
zone2
{
    type cellZone;
cellLabels      List<label> 
500
(
0
1

I create a file named fvOptions into the system folder with:

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvOptions;
}

porosity
{
    type          explicitPorositySource;
    active        yes;
    selectionMode cellZone;
    cellZone      zone2;

    explicitPorositySourceCoeffs
    {
        type DarcyForchheimer;

        DarcyForchheimerCoeffs
        {
              d    d [0 -2 0 0 0 0 0] (5e7 -1000 -1000);
              f    f [0 -1 0 0 0 0 0] (0 0 0);

              coordinateSystem
              {
                  e1    (1 0 0);
                  e2    (0 1 0);
              }
        }
    }
}

following what is said here:

http://www.openfoam.org/version2.2.0/fvOptions.php

but the solver (icoFoam) is unable to read it (if I change the values of the coefficients nothing changes in the solution..).

Do I need to specify something more?

Thank you,
Yuri

[yurifrey]

This is the answer I had from fredo490:

Hello,
I don't have any machine running openfoam next to me now so it's a bit hard to answer.

My guess is that icoFoam has not been updated to consider the fvOption files. The best way to check is to go to the icoFoam source code and check if you find any "+ fvOption" or something similar in one of the equation solved.

I have some source code on my computer but only simpleFoam and pimplefoam are up to date. If you look at the pimpleFoam UEqn.h you will find the following code to solve the momentum equation:

tmp<fvVectorMatrix> UEqn
(
    fvm::ddt(U)
  + fvm::div(phi, U)
  + turbulence->divDevReff(U)
 ==
    fvOptions(U)
);

The last term is the "fvOptions(U)" file that consider lthe porosity and so on.

Try to find the same for icoFoam... but I think you will not find it because icoFoam behave a bit differently.

Hope it helps you.

I checked it and it is exactly as he said. I had no problems using pimpleFoam.

[samiam1000]

Hi guys,

I am trying to use fvOption, as well.

What I would like to do is to add a body-force in certain cells of my domain.

Actually, what I did is something like

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

momentumSource
{
    type            vectorExplicitSetValue;
    active          on;            //on/off switch
    selectionMode   all;       //cellSet // points //cellZone

    vectorExplicitSetValueCoeffs
    {
        injectionRate
        {
            F    ( 0.1335 0 0 );
        }
    }
}


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

but I do not understand which are the right entries (I think that doing like what I did, I add a velocity, not a force).

Could you help, please?

Thanks a lot,
Samuele

[hfsf]

Hello all,

I'm sorry for such a noob question, but recently I started to model a flow over a porous media in OpenFOAM. In the OpenFOAM website I've stumbled upon a new feature since OF 2.x: the fvOptions dictionary.

The problem is: I cannot see any reference to the porosity of the medium. The example of a fvOptions dictionary configuration (from the very own OpenFOAM website) is:

porosity1 
{ 
    type          explicitPorositySource;                                                                                                                                                        
    active        yes; 
    selectionMode cellZone; 
    cellZone      porosity; 

    explicitPorositySourceCoeffs 
    { 
        type DarcyForchheimer; 

        DarcyForchheimerCoeffs 
        { 
              d    d [0 -2 0 0 0 0 0] (5e7 -1000 -1000); 
              f    f [0 -1 0 0 0 0 0] (0 0 0); 

              coordinateSystem 
              { 
                  e1    (0.70710678 0.70710678 0); 
                  e2    (0 0 1); 
              } 
        } 
    } 
}

But there's no mention of the porosity of the medium, as you can see!!!

In a post of Alberto Passalacqua's blog, he posted a similar procedure concerning the version 1.5 of the OpenFOAM. The posted code is as follows:

1 
(     
   porosity    
   {         
       coordinateSystem         
       {             
                origin (0 0 0);
                e1  (1 0 0);
                e2  (0 1 0);
        }          
        
        porosity 0.5;          
        Darcy         
        {             
                d   d [0 -2 0 0 0 0 0] (-1 1e7 -1);             
                 f   f [0 -1 0 0 0 0 0] (0 0 0);         
         }     
    } 
 )

The porosity field is there, after coordinateSystem definition. What have changed in the 2.2 version? How can I define the porosity of the medium?

Thanks in advance.

[olivierG]

Hello,

For pressure/velocity resolution, you don't need the porosity info (at least with Darcy model), only permeability.

However you need it for heat transfert, but in this case just add another fvOption for the heat transfert part (like "constantHeatTransfert" of "effectivenessHeatExchangerSource").

regards,
olivier

[openfoammaofnepo]

Dear Olivier,

For fvOptions, for those tutorials without the dictionary "fvOptions", the "fvOptions" related terms appears in the source files of the solvers actually are useless. These terms are only active when we specify the parameter in the fvOptions dictionary. Is what I am saying correct? Thank you so much.