CFD Online Discussion Forums - [TUTORIAL] Implementing porous zones to PisoFOAM

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Programming & Development (https://www.cfd-online.com/Forums/openfoam-programming-development/)

- - [TUTORIAL] Implementing porous zones to PisoFOAM (https://www.cfd-online.com/Forums/openfoam-programming-development/141181-tutorial-implementing-porous-zones-pisofoam.html)

[TUTORIAL] Implementing porous zones to PisoFOAM

Run the following to make a copy of the original pisoFoam

Code:

cp -r $WM_PROJECT_DIR/applications/solvers/incompressible/pisoFoam/ $WM_PROJECT_USER_DIR/applications/solvers/my_pisoFoamPOROUS

Change names

Code:

cd $WM_PROJECT_USER_DIR/applications/solvers/my_pisoFoamPOROUS

Code:

mv pisoFoam.C my_pisoFoamPOROUS.C

Change link options so that we can compile

Change Make/files to

Code:

my_pisoFoamPOROUS.C



EXE = $(FOAM_USER_APPBIN)/my_pisoFoamPOROUS

First line says which is the main file for the compilation, second line tells the compiler where to save the new solver and the new of the new solver (the name you will use to call the new solver)

Change Make/options to:

Code:

EXE_INC = \

    -I$(LIB_SRC)/turbulenceModels/incompressible/turbulenceModel \

    -I$(LIB_SRC)/transportModels \

    -I$(LIB_SRC)/transportModels/incompressible/singlePhaseTransportModel \

    -I$(LIB_SRC)/finiteVolume/lnInclude \

    -I$(LIB_SRC)/meshTools/lnInclude 



EXE_LIBS = \

    -lincompressibleTurbulenceModel \

    -lincompressibleRASModels \

    -lincompressibleLESModels \

    -lincompressibleTransportModels \

    -lfiniteVolume \

    -lmeshTools

The \ tells the compiler there is a new line, and we added meshTools library in order to access the mesh object during runTime

Remove old compiled files

Code:

rm -rf Make/linux* pisoFoam.dep

Create new file createPorousZones.H

Code:

touch createPorousZones.H

This will create the file. Then add to it the following

Code:

    porousZones pZones(mesh); //creates the object porousZones from the mesh object

    Switch pressureImplicitPorosity(false);// Sets the pressure solver as explicit

Open my_pisoFoamPOROUS.C and add this before the main function

Code:

...

#include "porousZones.H" // object porousZone 

int main(){

...

}

This is needed to have the porousZones constructor

Add the following after the main function

Code:

int main(){



    #include "CourantNo.H"

    #include "createPorousZones.H"

    

    // PISO LOOP

    ....



}

This will create the object porousZones as stated before

Inside the PISO corrector add the following

Code:

//PISO corrector



{

            fvVectorMatrix UEqn

            (

                fvm::ddt(U)

              + fvm::div(phi, U)

              + turbulence->divDevReff(U)

            );

           pZones.addResistance(UEqn);

          ...



}

Compile the solver

Code:

wmake

The solver is completed now you need to put inside your constant/ folder a file with name porousZones where you will write your porous properties. You can get one from

Code:

$WM_PROJECT_DIR/tutorials/incompressible/porousSimpleFoam/angledDuctExplicit/constant/
To set a porous zone inside your mesh

Run

Code:

topoSet

with your topoSetDict, example setting a box:

Code:

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2.1.0                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

FoamFile

{

    version     2.0;

    format      ascii;

    class       dictionary;

    object      topoSetDict;

}



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



actions

(

    {

        name    porosity;

        type    cellSet;

        action  new;

        source  boxToCell;

        sourceInfo

        {

           box (10 0 0) (35 2 0.5); //box (minVertex) (maxVertex)

        }

    }

After that run

Code:

setsToZones

because we have selected only Cells, but the solver needs zones.

At last call

Code:

my_pisoFoamPOROUS

inside your case folder, and it should hopefully run with porous zones.

Hope you found it helpful.

I get the error "fatal error: porousZones.H: No such file or directory
compilation terminated".

What can be the possible reasons?>

Hello
To make this work you either need to have the same version as OF that is used by ssss or get the right name of the include file for porousSimpleFoam.
#include "IOporosityModelList.H" in stead of
#include "porousZones.H"

This change also needs to be made in the code exchange porousZones by IOporosityModelList.

( I tried this with OF-dev and I had to change the tutorial also quite a lot because there are links to files that I could not copy)

Hope this helps
Wouter

Yeah I figured that out.

To add porous zones in any solver:

1. Create createPorousZones.H file.

Add

IOporosityModelList pZones(mesh); //creates the object porousZones from the mesh object

Switch pressureImplicitPorosity(false);// Sets the pressure solver as explicit

2. Add #include "IOporosityModelList.H" in header of .C
#include "createPorousZones.H" in main prog.

3. Add pZones.addResistance(UEqn); after the governing equations.

Peace!

Quote:

Originally Posted by wouter (Post 623876)

Is it necessary to multiply porosity explicitly in the Ueqn as given in various articles on porous media or OF takes care of it when you define darcyForchheimer type fvOptions?

Hello everyone.

Is there a similar method for including cellzones inside a solver, maybe icofoam or simplefoam??

what is the different if i want to implement porous zones to icoFoam? thanks