use of porous media with sonicFoam or rhoCentralFoam

Calmly · February 2, 2018, 15:54

Hello!

How can I use a porous media/cell zone with transient solver like sonicFoam or rhoCentralFoam? Do I need to implement the code for the porous zones in the solver or there is another way to do it?

I want to use the porous zone near the walls and the sonicFoam/rhoCentralFoam for the far-field domain.

Regards.

deepbandivadekar · February 8, 2018, 06:49

Were you able to use those sovlers (esp. sonicFoam) for your case? Could you share the outcome please?

rezaeimahdi · February 11, 2018, 01:02

Quote:

Originally Posted by Calmly

Hello!

How can I use a porous media/cell zone with transient solver like sonicFoam or rhoCentralFoam? Do I need to implement the code for the porous zones in the solver or there is another way to do it?

I want to use the porous zone near the walls and the sonicFoam/rhoCentralFoam for the far-field domain.

Regards.

Hello,

If I understand correctly your question, you want to simulate a porous zone with a transient solver? right?

you can define a porous zone in your mesh and then use fvOptions.

If my answer is what you are looking for and you need further information please don't hesitate to ask.

Bests

Calmly · February 13, 2018, 12:46

Quote:

Originally Posted by rezaeimahdi

Hello,

If I understand correctly your question, you want to simulate a porous zone with a transient solver? right?

you can define a porous zone in your mesh and then use fvOptions.

If my answer is what you are looking for and you need further information please don't hesitate to ask.

Bests

Hello,

Thank you for your answer.

Yeah, that's what I need, more or less.

I tried to define the porous zone with topoSetDict and then use the fvOptions as you said. It looks like it reads the porous zone when i run the solver but after 3 iterations i get this:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1706                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : v1706
Arch   : "LSB;label=32;scalar=64"
Exec   : rhoCentralFoam
Date   : Feb 13 2018
Time   : 19:16:39
Host   : "themistoklis-desktop"
PID    : 14946
Case   : /home/themistoklis/VKI/3D/LES/cases_folder/ss-LES-porosity1
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0

Reading thermophysical properties

Selecting thermodynamics package 
{
    type            hePsiThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleInternalEnergy;
}

Reading field U

Creating turbulence model

Selecting turbulence model type LES
Selecting LES turbulence model kEqn
Selecting LES delta type vanDriest
Selecting LES delta type cubeRootVol
LES
{
    LESModel        kEqn;
    turbulence      on;
    printCoeffs     on;
    delta           vanDriest;
    cubeRootVolCoeffs
    {
        deltaCoeff      1;
    }
    PrandtlCoeffs
    {
        delta           cubeRootVol;
        cubeRootVolCoeffs
        {
            deltaCoeff      1;
        }
        smoothCoeffs
        {
            delta           cubeRootVol;
            cubeRootVolCoeffs
            {
                deltaCoeff      1;
            }
            maxDeltaRatio   1.1;
        }
        Cdelta          0.158;
    }
    vanDriestCoeffs
    {
        delta           cubeRootVol;
        cubeRootVolCoeffs
        {
            deltaCoeff      1;
        }
        smoothCoeffs
        {
            delta           cubeRootVol;
            cubeRootVolCoeffs
            {
                deltaCoeff      1;
            }
            maxDeltaRatio   1.1;
        }
        Aplus           26;
        Cdelta          0.158;
    }
    smoothCoeffs
    {
        delta           cubeRootVol;
        cubeRootVolCoeffs
        {
            deltaCoeff      1;
        }
        maxDeltaRatio   1.1;
    }
    Ce              1.048;
    Ck              0.094;
}

Creating finite volume options from "system/fvOptions"

Selecting finite volume options model type explicitPorositySource
    Source: porosity_wall
    - selecting cells using cellZone porosity_wall
Porosity region porosity_wall:
    selecting model: DarcyForchheimer
    creating porous zone: porosity_wall
    coordinateSystem origin: (0 0 0)
    e1              (1 0 0);
    e2              (0 1 0);
    e3              (0 0 1);

    local bounds: (-2e+300 -2e+300 -2e+300)

fluxScheme: Kurganov

Starting time loop

--> FOAM Warning : 
    From function virtual void Foam::probes::findElements(const Foam::fvMesh&)
    in file probes/probes.C at line 122
    Did not find location (0.5 0.5 0.35) in any cell. Skipping location.
Mean and max Courant Numbers = 0.0011493 26.4788
deltaT = 1.8883e-10
Time = 1.8883e-10

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUx, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUy, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUz, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Ux, Initial residual = 5.90703e-08, Final residual = 2.44838e-17, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 1.26004e-08, Final residual = 6.01289e-18, No Iterations 2
smoothSolver:  Solving for Uz, Initial residual = 3.90837e-07, Final residual = 1.92179e-18, No Iterations 2
diagonal:  Solving for rhoE, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for e, Initial residual = 1.58267e-08, Final residual = 1.84018e-17, No Iterations 2
smoothSolver:  Solving for k, Initial residual = 1, Final residual = 9.37399e-20, No Iterations 2
ExecutionTime = 6.42 s  ClockTime = 7 s

Mean and max Courant Numbers = 2.14605e-05 0.466437
deltaT = 2.02418e-10
Time = 3.91248e-10

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUx, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUy, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUz, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Ux, Initial residual = 2.22091e-08, Final residual = 1.2556e-18, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 4.60887e-09, Final residual = 4.60887e-09, No Iterations 0
smoothSolver:  Solving for Uz, Initial residual = 2.09171e-07, Final residual = 6.71802e-18, No Iterations 2
diagonal:  Solving for rhoE, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for e, Initial residual = 5.00931e-09, Final residual = 5.00931e-09, No Iterations 0
--> FOAM Warning : 
    From function virtual void Foam::fv::option::checkApplied() const
    in file cfdTools/general/fvOptions/fvOption.C at line 125
    Source porosity_wall defined for field U but never used
--> FOAM Warning : 
    From function virtual void Foam::fv::option::checkApplied() const
    in file cfdTools/general/fvOptions/fvOption.C at line 125
    Source porosity_wall defined for field U but never used

This is my fvOption file:

Code:

porosity_wall 
{
    type           explicitPorositySource;
    active         true;

    explicitPorositySourceCoeffs
    {
        type           DarcyForchheimer;
        selectionMode  cellZone;
        cellZone       porosity_wall; // Specify the name of the cellZone

        DarcyForchheimerCoeffs
        {
            // Negative coeffs are multiplied by largest positive coeff,
            // taking the magnitude, e.g. for -1000, coeff = |1e7*-1000| = 1e10

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

            coordinateSystem // Cartesian coordinates for the cellZone
            {
                x          (1 0 0);
                y          (0 1 0);
                #includeEtc "caseDicts/general/coordinateSystem/cartesianXY"
            }
        }
     }
}

And this is my topoSetDict file:

Code:

actions
(
    {
        name    porosity_wall;//center
        type    cellZoneSet;
        action  new;//add
        source  boxToCell;
        sourceInfo
        {
            box (0.125 0 0)(0.12494365 0.75 0.1);//building_wall
        }
    }


);

rezaeimahdi · February 13, 2018, 23:50

Quote:

Originally Posted by Calmly

Hello,

Thank you for your answer.

Yeah, that's what I need, more or less.

I tried to define the porous zone with topoSetDict and then use the fvOptions as you said. It looks like it reads the porous zone when i run the solver but after 3 iterations i get this:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1706                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : v1706
Arch   : "LSB;label=32;scalar=64"
Exec   : rhoCentralFoam
Date   : Feb 13 2018
Time   : 19:16:39
Host   : "themistoklis-desktop"
PID    : 14946
Case   : /home/themistoklis/VKI/3D/LES/cases_folder/ss-LES-porosity1
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0

Reading thermophysical properties

Selecting thermodynamics package 
{
    type            hePsiThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleInternalEnergy;
}

Reading field U

Creating turbulence model

Selecting turbulence model type LES
Selecting LES turbulence model kEqn
Selecting LES delta type vanDriest
Selecting LES delta type cubeRootVol
LES
{
    LESModel        kEqn;
    turbulence      on;
    printCoeffs     on;
    delta           vanDriest;
    cubeRootVolCoeffs
    {
        deltaCoeff      1;
    }
    PrandtlCoeffs
    {
        delta           cubeRootVol;
        cubeRootVolCoeffs
        {
            deltaCoeff      1;
        }
        smoothCoeffs
        {
            delta           cubeRootVol;
            cubeRootVolCoeffs
            {
                deltaCoeff      1;
            }
            maxDeltaRatio   1.1;
        }
        Cdelta          0.158;
    }
    vanDriestCoeffs
    {
        delta           cubeRootVol;
        cubeRootVolCoeffs
        {
            deltaCoeff      1;
        }
        smoothCoeffs
        {
            delta           cubeRootVol;
            cubeRootVolCoeffs
            {
                deltaCoeff      1;
            }
            maxDeltaRatio   1.1;
        }
        Aplus           26;
        Cdelta          0.158;
    }
    smoothCoeffs
    {
        delta           cubeRootVol;
        cubeRootVolCoeffs
        {
            deltaCoeff      1;
        }
        maxDeltaRatio   1.1;
    }
    Ce              1.048;
    Ck              0.094;
}

Creating finite volume options from "system/fvOptions"

Selecting finite volume options model type explicitPorositySource
    Source: porosity_wall
    - selecting cells using cellZone porosity_wall
Porosity region porosity_wall:
    selecting model: DarcyForchheimer
    creating porous zone: porosity_wall
    coordinateSystem origin: (0 0 0)
    e1              (1 0 0);
    e2              (0 1 0);
    e3              (0 0 1);

    local bounds: (-2e+300 -2e+300 -2e+300)

fluxScheme: Kurganov

Starting time loop

--> FOAM Warning : 
    From function virtual void Foam::probes::findElements(const Foam::fvMesh&)
    in file probes/probes.C at line 122
    Did not find location (0.5 0.5 0.35) in any cell. Skipping location.
Mean and max Courant Numbers = 0.0011493 26.4788
deltaT = 1.8883e-10
Time = 1.8883e-10

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUx, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUy, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUz, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Ux, Initial residual = 5.90703e-08, Final residual = 2.44838e-17, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 1.26004e-08, Final residual = 6.01289e-18, No Iterations 2
smoothSolver:  Solving for Uz, Initial residual = 3.90837e-07, Final residual = 1.92179e-18, No Iterations 2
diagonal:  Solving for rhoE, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for e, Initial residual = 1.58267e-08, Final residual = 1.84018e-17, No Iterations 2
smoothSolver:  Solving for k, Initial residual = 1, Final residual = 9.37399e-20, No Iterations 2
ExecutionTime = 6.42 s  ClockTime = 7 s

Mean and max Courant Numbers = 2.14605e-05 0.466437
deltaT = 2.02418e-10
Time = 3.91248e-10

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUx, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUy, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUz, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Ux, Initial residual = 2.22091e-08, Final residual = 1.2556e-18, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 4.60887e-09, Final residual = 4.60887e-09, No Iterations 0
smoothSolver:  Solving for Uz, Initial residual = 2.09171e-07, Final residual = 6.71802e-18, No Iterations 2
diagonal:  Solving for rhoE, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for e, Initial residual = 5.00931e-09, Final residual = 5.00931e-09, No Iterations 0
--> FOAM Warning : 
    From function virtual void Foam::fv::option::checkApplied() const
    in file cfdTools/general/fvOptions/fvOption.C at line 125
    Source porosity_wall defined for field U but never used
--> FOAM Warning : 
    From function virtual void Foam::fv::option::checkApplied() const
    in file cfdTools/general/fvOptions/fvOption.C at line 125
    Source porosity_wall defined for field U but never used

This is my fvOption file:

Code:

porosity_wall 
{
    type           explicitPorositySource;
    active         true;

    explicitPorositySourceCoeffs
    {
        type           DarcyForchheimer;
        selectionMode  cellZone;
        cellZone       porosity_wall; // Specify the name of the cellZone

        DarcyForchheimerCoeffs
        {
            // Negative coeffs are multiplied by largest positive coeff,
            // taking the magnitude, e.g. for -1000, coeff = |1e7*-1000| = 1e10

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

            coordinateSystem // Cartesian coordinates for the cellZone
            {
                x          (1 0 0);
                y          (0 1 0);
                #includeEtc "caseDicts/general/coordinateSystem/cartesianXY"
            }
        }
     }
}

And this is my topoSetDict file:

Code:

actions
(
    {
        name    porosity_wall;//center
        type    cellZoneSet;
        action  new;//add
        source  boxToCell;
        sourceInfo
        {
            box (0.125 0 0)(0.12494365 0.75 0.1);//building_wall
        }
    }


);

Hello

Can you test your case with another solver like sonicFoam and let me know if it worked?

I have no idea about rhoCentralFoam, but just check the source code and it seems it doesn't care about fvOptions in momentum equation:

// --- Solve momentum
solve(fvm::ddt(rhoU) + fvc::div(phiUp));

U.ref() =
rhoU()
/rho();
U.correctBoundaryConditions();
rhoU.boundaryFieldRef() == rho.boundaryField()*U.boundaryField();

if (!inviscid)
{
solve
(
fvm::ddt(rho, U) - fvc::ddt(rho, U)
- fvm::laplacian(muEff, U)
- fvc::div(tauMC)
);
rhoU = rho*U;
}

And this could be the reason for this warning: Source porosity_wall defined for field U but never used

However, for the other solvers like sonicFoam momentum equation solve like this:

// Solve the Momentum equation

MRF.correctBoundaryVelocity(U);

fvVectorMatrix UEqn
(
fvm::ddt(rho, U) + fvm::div(phi, U)
+ MRF.DDt(rho, U)
+ turbulence->divDevRhoReff(U)
==
fvOptions(rho, U)
);

UEqn.relax();

fvOptions.constrain(UEqn);

if (pimple.momentumPredictor())
{
solve(UEqn == -fvc::grad(p));

fvOptions.correct(U);
K = 0.5*magSqr(U);
}

And as you can see, there is fvOptions in RHS of the equation as the source term.

Regards,

Calmly · September 15, 2018, 20:34

Quote:

Originally Posted by rezaeimahdi

Hello

Can you test your case with another solver like sonicFoam and let me know if it worked?

I have no idea about rhoCentralFoam, but just check the source code and it seems it doesn't care about fvOptions in momentum equation:

// --- Solve momentum
solve(fvm::ddt(rhoU) + fvc::div(phiUp));

U.ref() =
rhoU()
/rho();
U.correctBoundaryConditions();
rhoU.boundaryFieldRef() == rho.boundaryField()*U.boundaryField();

if (!inviscid)
{
solve
(
fvm::ddt(rho, U) - fvc::ddt(rho, U)
- fvm::laplacian(muEff, U)
- fvc::div(tauMC)
);
rhoU = rho*U;
}

And this could be the reason for this warning: Source porosity_wall defined for field U but never used

However, for the other solvers like sonicFoam momentum equation solve like this:

// Solve the Momentum equation

MRF.correctBoundaryVelocity(U);

fvVectorMatrix UEqn
(
fvm::ddt(rho, U) + fvm::div(phi, U)
+ MRF.DDt(rho, U)
+ turbulence->divDevRhoReff(U)
==
fvOptions(rho, U)
);

UEqn.relax();

fvOptions.constrain(UEqn);

if (pimple.momentumPredictor())
{
solve(UEqn == -fvc::grad(p));

fvOptions.correct(U);
K = 0.5*magSqr(U);
}

And as you can see, there is fvOptions in RHS of the equation as the source term.

Regards,

Thank you very much for your post, it really helped me.

You were right, rhocentralfoam couldn't 'read' the porous medium on the wall. In order to do so, I modified the momentum equation of rhocentralfoam and it works.

Sorry for the late reply.

shock77 · May 7, 2020, 11:12

Quote:

Originally Posted by Calmly

Thank you very much for your post, it really helped me.

You were right, rhocentralfoam couldn't 'read' the porous medium on the wall. In order to do so, I modified the momentum equation of rhocentralfoam and it works.

Sorry for the late reply.

Dear Calmly,

could you post your solution for rhoCentralFoam?
I am very interested how you changed the code to make it work.

Regards,
shock77

February 2, 2018, 15:54	use of porous media with sonicFoam or rhoCentralFoam	#1
Calmly New Member Join Date: Aug 2017 Posts: 18 Rep Power: 8	Hello! How can I use a porous media/cell zone with transient solver like sonicFoam or rhoCentralFoam? Do I need to implement the code for the porous zones in the solver or there is another way to do it? I want to use the porous zone near the walls and the sonicFoam/rhoCentralFoam for the far-field domain. Regards.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Thermal non-equilibrium porous media model with conjugate heat transfer	Hexahedron	FLUENT	9	February 22, 2023 02:55
Multiphase Porous Media Flow - Convergence Issues	VT_Bromley	FLUENT	7	May 14, 2020 16:34
Porous media setup issues in Fluent	Bernard Van	FLUENT	29	January 26, 2017 04:09
How to model granular flow through porous media	Axius	FLUENT	2	August 7, 2014 10:34
porous media: Fluent or Star-CD?	Igor	Main CFD Forum	0	December 5, 2002 15:16

February 8, 2018, 06:49		#2
deepbandivadekar Senior Member Deep Join Date: Oct 2017 Posts: 180 Rep Power: 8	Were you able to use those sovlers (esp. sonicFoam) for your case? Could you share the outcome please?