CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM

chtMultiRegionSimpleFoam with porous solid region.

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   February 5, 2018, 13:58
Default chtMultiRegionSimpleFoam with porous solid region.
  #1
New Member
 
Join Date: Nov 2017
Posts: 2
Rep Power: 0
srikanthallu is on a distinguished road
Hi,

In the tutorial/example for chtMultiRegionSimpleFoam i.e., heatExchanger, the porous region is modeled as fluid. I am trying to model this as a solid region since there is a volumetric heat source. The solver utilizes interRegionHeatTransferModel between regions using constantheatTransfer model. Does this model always expect the porous region to be fluid ?? Because it is expecting a surfaceField 'phi' and is giving me an error message:

request for surfaceScalarField phi from objectRegistry porous failed
available objects of type surfaceScalarField are
0()

If possible, please point me to appropriate location from where this error could be originating...


Thanks
srikanthallu is offline   Reply With Quote

Old   March 7, 2018, 07:35
Default
  #2
New Member
 
Adri
Join Date: Sep 2017
Posts: 24
Rep Power: 3
Adri_12 is on a distinguished road
Quote:
Originally Posted by srikanthallu View Post
Hi,

In the tutorial/example for chtMultiRegionSimpleFoam i.e., heatExchanger, the porous region is modeled as fluid. I am trying to model this as a solid region since there is a volumetric heat source. The solver utilizes interRegionHeatTransferModel between regions using constantheatTransfer model. Does this model always expect the porous region to be fluid ?? Because it is expecting a surfaceField 'phi' and is giving me an error message:
Hi, did you get more information about the way to consider the porous region? solid or fluid ?

Thanks,

Adrià
Adri_12 is offline   Reply With Quote

Old   March 8, 2018, 18:30
Default
  #3
Senior Member
 
Derek Mitchell
Join Date: Mar 2014
Location: UK, Reading
Posts: 160
Rep Power: 7
derekm is on a distinguished road
you cant model a porous region as a solid as you dont have the required fields e.g U . There is nothing stopping you having heat generation in a fluid using fvOptions.In fact it works very well.
__________________
A CHEERING BAND OF FRIENDLY ELVES CARRY THE CONQUERING ADVENTURER OFF INTO THE SUNSET
derekm is offline   Reply With Quote

Old   March 9, 2018, 03:48
Default chtMultiRegionFoam for porous regions
  #4
New Member
 
Adri
Join Date: Sep 2017
Posts: 24
Rep Power: 3
Adri_12 is on a distinguished road
Quote:
Originally Posted by derekm View Post
you cant model a porous region as a solid as you dont have the required fields e.g U . There is nothing stopping you having heat generation in a fluid using fvOptions.In fact it works very well.
Ok Thanks Derek,

in my case I would like to use chtMultiRegionFoam (transient) to look to heat transfers between a flow of hot air going through a porous bed (cf attachement). It's not for a heatexchanger it would be more for a thermal storage of heat in porous bed. So I don't need ther constantHeatSource but more a porosity modeling.

Do you think that I can introduce in constant/porous/fvOptions :
- a darcy forcheimer porosity model (with explicitPorositySource)
- with a radial porosity profile ?
- with a interfacial area density definition, (i.e the ratio of the area of the fluid / solid interface and the volume of the porous zone)
- heat transfer law modeling between fluid & porous bed (non-thermal equilibrium)

Thanks again for your help !

Adrià
Attached Images
File Type: png schéma_CFD_TES.PNG (12.9 KB, 22 views)
Adri_12 is offline   Reply With Quote

Old   August 3, 2018, 19:30
Default
  #5
Member
 
Colli, Alejandro
Join Date: Jan 2014
Posts: 75
Rep Power: 6
ancolli is on a distinguished road
Quote:
Originally Posted by Adri_12 View Post
Ok Thanks Derek,

in my case I would like to use chtMultiRegionFoam (transient) to look to heat transfers between a flow of hot air going through a porous bed (cf attachement). It's not for a heatexchanger it would be more for a thermal storage of heat in porous bed. So I don't need ther constantHeatSource but more a porosity modeling.

Do you think that I can introduce in constant/porous/fvOptions :
- a darcy forcheimer porosity model (with explicitPorositySource)
- with a radial porosity profile ?
- with a interfacial area density definition, (i.e the ratio of the area of the fluid / solid interface and the volume of the porous zone)
- heat transfer law modeling between fluid & porous bed (non-thermal equilibrium)

Thanks again for your help !

Adrià
I am facing a similar problem, did you solve it? Any hint?
ancolli is offline   Reply With Quote

Old   August 31, 2018, 11:14
Default
  #6
New Member
 
Adri
Join Date: Sep 2017
Posts: 24
Rep Power: 3
Adri_12 is on a distinguished road
Hi Alejandro,

Yes I am working on it. I manage to build a case considering fluid going accross a porous media and exchanging heat flux between both of them as 2 different regions (cf attached)

However I have some dimension troubles when I try to change the existing variableHeatTransfer function to calculate the h heat flux from the Nusselt number. I want to replace the proposed formula by a more adapted to my porous case adding 1 constant value :

Code:
Nu = a*pow(Re, b)*pow(Pr, c) --> Nu = 2 + 1.1*pow(Re, 0.6)*pow(Pr, 0.3)
PROBLEM : I have this error message when I use the new function (no problem for the compilation) :

Code:
--> FOAM FATAL ERROR: 
LHS and RHS of + have different dimensions
     dimensions : [0 0 0 0 0 0 0] + [0 -0.6 0 0 0 0 0]
ModifiedVariableHeatTransfer.C
Code:
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011-2016 OpenFOAM Foundation
     \\/     M anipulation  |
-------------------------------------------------------------------------------
License
    This file is part of OpenFOAM.

    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.

    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.

    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.

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

#include "WakaoCorrelationVariableHeatTransfer.H"
#include "addToRunTimeSelectionTable.H"
#include "turbulentFluidThermoModel.H"	

// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //

namespace Foam
{
namespace fv
{
    defineTypeNameAndDebug(WakaoCorrelationVariableHeatTransfer, 0);
    addToRunTimeSelectionTable
    (
        option,
        WakaoCorrelationVariableHeatTransfer,
        dictionary

    );
	
}
}


// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //

Foam::fv::WakaoCorrelationVariableHeatTransfer::WakaoCorrelationVariableHeatTransfer
(
    const word& name,
    const word& modelType,
    const dictionary& dict,
    const fvMesh& mesh
)
:
    interRegionHeatTransferModel(name, modelType, dict, mesh),
    UNbrName_(coeffs_.lookupOrDefault<word>("UNbr", "U")),
    a_(0), // 
    b_(0), // pow(Re,b)
    c_(0), // pow(Pr,c)
    ds_(0),
    //ds_("ds_", dimLength, 0.01),
    Pr_(0),
    AoV_()
{
    if (master_)
    {
	a_ = readScalar(coeffs_.lookup("a"));
        b_ = readScalar(coeffs_.lookup("b"));
        c_ = readScalar(coeffs_.lookup("c"));
        ds_ = readScalar(coeffs_.lookup("ds"));
        Pr_ = readScalar(coeffs_.lookup("Pr"));	
        AoV_.reset
        (
            new volScalarField
            (
                IOobject
                (
                    "AoV",
                    mesh_.time().timeName(),
                    mesh_,
                    IOobject::MUST_READ,
                    IOobject::AUTO_WRITE
                ),
                mesh_
            )
        );
    }
}



// * * * * * * * * * * * * * * * * Destructor  * * * * * * * * * * * * * * * //

Foam::fv::WakaoCorrelationVariableHeatTransfer::~WakaoCorrelationVariableHeatTransfer()
{}


// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //


void Foam::fv::WakaoCorrelationVariableHeatTransfer::calculateHtc()
{      
	if (master_)
	{
	   const fvMesh& nbrMesh =
		mesh_.time().lookupObject<fvMesh>(nbrRegionName());

	    const compressible::turbulenceModel& nbrTurb =
		nbrMesh.lookupObject<compressible::turbulenceModel>
		(
		    turbulenceModel::propertiesName
		);

	    const fluidThermo& nbrThermo =
		nbrMesh.lookupObject<fluidThermo>(basicThermo::dictName);

	    const volVectorField& UNbr =
		nbrMesh.lookupObject<volVectorField>(UNbrName_);

	    const volScalarField ReNbr(mag(UNbr)*ds_*nbrThermo.rho()/nbrTurb.mut());

	    const volScalarField NuNbr(2 + a_*pow(ReNbr, b_)*pow(Pr_, c_));
	}
}


bool Foam::fv::WakaoCorrelationVariableHeatTransfer::read(const dictionary& dict)
{
    if (interRegionHeatTransferModel::read(dict))
    {
        coeffs_.readIfPresent("UNbr", UNbrName_);

        coeffs_.readIfPresent("a", a_);
        coeffs_.readIfPresent("b", b_);
        coeffs_.readIfPresent("c", c_);
        coeffs_.readIfPresent("ds", ds_);
        coeffs_.readIfPresent("Pr", Pr_);

        return true;
    }
    else
    {
        return false;
    }
} 


// ************************************************************************* //
The original one : variableHeatTransfer.C :
Code:
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011-2016 OpenFOAM Foundation
     \\/     M anipulation  |
-------------------------------------------------------------------------------
License
    This file is part of OpenFOAM.

    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.

    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.

    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.

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

#include "variableHeatTransfer.H"
#include "turbulentFluidThermoModel.H"
#include "addToRunTimeSelectionTable.H"

// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //

namespace Foam
{
namespace fv
{
    defineTypeNameAndDebug(variableHeatTransfer, 0);
    addToRunTimeSelectionTable
    (
        option,
        variableHeatTransfer,
        dictionary
    );
}
}


// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //

Foam::fv::variableHeatTransfer::variableHeatTransfer
(
    const word& name,
    const word& modelType,
    const dictionary& dict,
    const fvMesh& mesh
)
:
    interRegionHeatTransferModel(name, modelType, dict, mesh),
    UNbrName_(coeffs_.lookupOrDefault<word>("UNbr", "U")),
    a_(0),
    b_(0),
    c_(0),
    ds_(0),
    Pr_(0),
    AoV_()
{
    if (master_)
    {
        a_ = readScalar(coeffs_.lookup("a"));
        b_ = readScalar(coeffs_.lookup("b"));
        c_ = readScalar(coeffs_.lookup("c"));
        ds_ = readScalar(coeffs_.lookup("ds"));
        Pr_ = readScalar(coeffs_.lookup("Pr"));
        AoV_.reset
        (
            new volScalarField
            (
                IOobject
                (
                    "AoV",
                    mesh_.time().timeName(),
                    mesh_,
                    IOobject::MUST_READ,
                    IOobject::AUTO_WRITE
                ),
                mesh_
            )
        );
    }
}


// * * * * * * * * * * * * * * * * Destructor  * * * * * * * * * * * * * * * //

Foam::fv::variableHeatTransfer::~variableHeatTransfer()
{}


// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //

void Foam::fv::variableHeatTransfer::calculateHtc()
{
    const fvMesh& nbrMesh =
        mesh_.time().lookupObject<fvMesh>(nbrRegionName());

    const compressible::turbulenceModel& nbrTurb =
        nbrMesh.lookupObject<compressible::turbulenceModel>
        (
            turbulenceModel::propertiesName
        );

    const fluidThermo& nbrThermo =
        nbrMesh.lookupObject<fluidThermo>(basicThermo::dictName);

    const volVectorField& UNbr =
        nbrMesh.lookupObject<volVectorField>(UNbrName_);

    const volScalarField ReNbr(mag(UNbr)*ds_*nbrThermo.rho()/nbrTurb.mut());

    const volScalarField NuNbr(a_*pow(ReNbr, b_)*pow(Pr_, c_));

    const scalarField htcNbr(NuNbr*nbrTurb.kappaEff()/ds_);

    const scalarField htcNbrMapped(interpolate(htcNbr));

    htc_.primitiveFieldRef() = htcNbrMapped*AoV_;
}


bool Foam::fv::variableHeatTransfer::read(const dictionary& dict)
{
    if (interRegionHeatTransferModel::read(dict))
    {
        coeffs_.readIfPresent("UNbr", UNbrName_);

        coeffs_.readIfPresent("a", a_);
        coeffs_.readIfPresent("b", b_);
        coeffs_.readIfPresent("c", c_);
        coeffs_.readIfPresent("ds", ds_);
        coeffs_.readIfPresent("Pr", Pr_);

        return true;
    }
    else
    {
        return false;
    }
}


// ************************************************************************* //
My questions :
1. Does anybody already used or validated this fvOption before ? There is no tutorial using it.
2. Do you agree that ds_ value would be declared as a dimensionedScalar [0 1 0 0 0 ...]. That would explain the dimension problem I found.
3. If it is the case, how can it works with the original function ?

I am quite surprised to have found such a mistake. I am waiting for your reactions !
Attached Files
File Type: gz AirAndBed_BORRAS_NADAL_CFDonline.tar.gz (8.9 KB, 2 views)
Adri_12 is offline   Reply With Quote

Old   September 1, 2018, 15:12
Default
  #7
Member
 
Colli, Alejandro
Join Date: Jan 2014
Posts: 75
Rep Power: 6
ancolli is on a distinguished road
why u removed the following 3 lines from the original function?

Code:
    const scalarField htcNbr(NuNbr*nbrTurb.kappaEff()/ds_);

    const scalarField htcNbrMapped(interpolate(htcNbr));

    htc_.primitiveFieldRef() = htcNbrMapped*AoV_;
ancolli is offline   Reply With Quote

Old   September 3, 2018, 03:42
Default
  #8
New Member
 
Adri
Join Date: Sep 2017
Posts: 24
Rep Power: 3
Adri_12 is on a distinguished road
Hi, Excuse me your right it's a mistake of copy/paste for the post.

the corrected version :

Code:
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011-2016 OpenFOAM Foundation
     \\/     M anipulation  |
-------------------------------------------------------------------------------
License
    This file is part of OpenFOAM.

    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.

    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.

    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.

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

#include "WakaoCorrelationVariableHeatTransfer.H"
#include "addToRunTimeSelectionTable.H"
#include "turbulentFluidThermoModel.H"	

// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //

namespace Foam
{
namespace fv
{
    defineTypeNameAndDebug(WakaoCorrelationVariableHeatTransfer, 0);
    addToRunTimeSelectionTable
    (
        option,
        WakaoCorrelationVariableHeatTransfer,
        dictionary

    );
	
}
}


// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //

Foam::fv::WakaoCorrelationVariableHeatTransfer::WakaoCorrelationVariableHeatTransfer
(
    const word& name,
    const word& modelType,
    const dictionary& dict,
    const fvMesh& mesh
)
:
    interRegionHeatTransferModel(name, modelType, dict, mesh),
    UNbrName_(coeffs_.lookupOrDefault<word>("UNbr", "U")),
    a_(0), // 
    b_(0), // pow(Re,b)
    c_(0), // pow(Pr,c)
    ds_(0),
    //ds_("ds_", dimLength, 0.01),
    Pr_(0),
    AoV_()
{
    if (master_)
    {
	a_ = readScalar(coeffs_.lookup("a"));
        b_ = readScalar(coeffs_.lookup("b"));
        c_ = readScalar(coeffs_.lookup("c"));
        ds_ = readScalar(coeffs_.lookup("ds"));
        Pr_ = readScalar(coeffs_.lookup("Pr"));	
        AoV_.reset
        (
            new volScalarField
            (
                IOobject
                (
                    "AoV",
                    mesh_.time().timeName(),
                    mesh_,
                    IOobject::MUST_READ,
                    IOobject::AUTO_WRITE
                ),
                mesh_
            )
        );
    }
}



// * * * * * * * * * * * * * * * * Destructor  * * * * * * * * * * * * * * * //

Foam::fv::WakaoCorrelationVariableHeatTransfer::~WakaoCorrelationVariableHeatTransfer()
{}


// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //


void Foam::fv::WakaoCorrelationVariableHeatTransfer::calculateHtc()
{      
	if (master_)
	{
	   const fvMesh& nbrMesh =
		mesh_.time().lookupObject<fvMesh>(nbrRegionName());

	    const compressible::turbulenceModel& nbrTurb =
		nbrMesh.lookupObject<compressible::turbulenceModel>
		(
		    turbulenceModel::propertiesName
		);

	    const fluidThermo& nbrThermo =
		nbrMesh.lookupObject<fluidThermo>(basicThermo::dictName);

	    const volVectorField& UNbr =
		nbrMesh.lookupObject<volVectorField>(UNbrName_);

	    const volScalarField ReNbr(mag(UNbr)*ds_*nbrThermo.rho()/nbrTurb.mut());

	    const volScalarField NuNbr(2 + a_*pow(ReNbr, b_)*pow(Pr_, c_));

            const scalarField htcNbr(NuNbr*nbrTurb.kappaEff()/ds_);

            const scalarField htcNbrMapped(interpolate(htcNbr));

            htc_.primitiveFieldRef() = htcNbrMapped*AoV_;
	}
}


bool Foam::fv::WakaoCorrelationVariableHeatTransfer::read(const dictionary& dict)
{
    if (interRegionHeatTransferModel::read(dict))
    {
        coeffs_.readIfPresent("UNbr", UNbrName_);

        coeffs_.readIfPresent("a", a_);
        coeffs_.readIfPresent("b", b_);
        coeffs_.readIfPresent("c", c_);
        coeffs_.readIfPresent("ds", ds_);
        coeffs_.readIfPresent("Pr", Pr_);

        return true;
    }
    else
    {
        return false;
    }
} 


// ************************************************************************* //
Any ideas about the dimension error ?

thanks for your help.

adrià
Adri_12 is offline   Reply With Quote

Old   September 3, 2018, 06:22
Default
  #9
Member
 
Colli, Alejandro
Join Date: Jan 2014
Posts: 75
Rep Power: 6
ancolli is on a distinguished road
can u upload the complete .H and .C code together with the make directory, then i can try to compile on my side. Which version of OF are u using?
ancolli is offline   Reply With Quote

Old   September 4, 2018, 05:22
Default
  #10
New Member
 
Adri
Join Date: Sep 2017
Posts: 24
Rep Power: 3
Adri_12 is on a distinguished road
Sure,

version : CFD-direct version OpenFOAM.5.0

you have the function to compile attached.

Adrià
Attached Files
File Type: gz WakaoCorrelationVariableHeatTransfer.tar.gz (86.0 KB, 3 views)
Adri_12 is offline   Reply With Quote

Old   September 4, 2018, 08:06
Default
  #11
Member
 
Colli, Alejandro
Join Date: Jan 2014
Posts: 75
Rep Power: 6
ancolli is on a distinguished road
Also, I ran ur example but, it is set for constantHeatTransfer. Did u run it with variableHeatTransfer? I would need the dictionary with your a, b, c, etc constant for your particular case.
ancolli is offline   Reply With Quote

Old   September 13, 2018, 09:52
Default
  #12
New Member
 
Adri
Join Date: Sep 2017
Posts: 24
Rep Power: 3
Adri_12 is on a distinguished road
Hi Alejandro,

Sorry for my late answer but I deal with other topics and I just come back to my porous heat transfer case.

Attached you 'll find the case with the modified library case. You will need to compile the Wakao lib to run it of course.

As I said before, I encountered a dimension error when I try to run it, and I don't know why.

here's the error when I take the following input coeffs :

Code:
solidToAir
{
    type            WakaoCorrelationVariableHeatTransfer;
    active          yes;

    WakaoCorrelationVariableHeatTransferCoeffs
    {
        interpolationMethod cellVolumeWeight;
        nbrRegionName   air;
        master          true;

        nbrModel       airToSolid;
        fields          (h);
        semiImplicit    no;

	a  1.1;
	b  0.6;//
	c  0.333;
	ds 0.01; //in m?
        Pr 0.7;

    }
}
Code:
--> FOAM FATAL ERROR:
LHS and RHS of + have different dimensions
     dimensions : [0 0 0 0 0 0 0] + [0 -0.6 0 0 0 0 0]


    From function Foam::dimensionSet Foam::operator+(const Foam::dimensionSet&, const Foam::dimensionSet&)
    in file dimensionSet/dimensionSet.C at line 501.
If you see where is my mistake, please let me know it.

Adrià
Attached Files
File Type: gz WakaoAirAndBed_BORRAS_NADAL_CFDonline.tar.gz (9.7 KB, 2 views)
Adri_12 is offline   Reply With Quote

Old   September 14, 2018, 08:46
Default
  #13
Member
 
Colli, Alejandro
Join Date: Jan 2014
Posts: 75
Rep Power: 6
ancolli is on a distinguished road
Hi Adri,
After studying a little bit the code. I think you are right in that ds_ value should be declared as a dimensionedScalar [0 1 0 0 0 ...]. That would explain the dimension problem. Otherwise, The Reynolds number would not be dimensionless and has no sense at all.

As u proposed by modifying:

.H
Code:
//scalar ds_; // error in the original code ?
	dimensionedScalar ds_;
and .C
Code:
//ds_(0),
ds_("ds_", dimLength, 0.01),
but also in .C (I am not 100% sure)
Code:
if (master_)
    {
	a_ = readScalar(coeffs_.lookup("a"));
        b_ = readScalar(coeffs_.lookup("b"));
        c_ = readScalar(coeffs_.lookup("c"));
        //ds_ = readScalar(coeffs_.lookup("ds"));
dimensionedScalar ds_ 
( 
"ds_",
dimLength,
readScalar(coeffs_.lookup("ds"))
);

I could compile and run without problems. The simulation is crashing after some iterations, but I have tried variableHeatTransfer and it is also crashing for the particular problem you are trying to solve (I think it is something related to numerical stability)

Maybe you should report the bug
ancolli is offline   Reply With Quote

Old   September 14, 2018, 08:59
Default
  #14
New Member
 
Adri
Join Date: Sep 2017
Posts: 24
Rep Power: 3
Adri_12 is on a distinguished road
Thanks Alejandro. I think it to.

The simulation runs but I think the solid region mesh resolution of the version I attached is not good enough.

Anyway I can update my case I attach the new one when it runs.

Apart from the code problem do you think that the case is adapted to consider heat transfer through porous media ? For the moment I am quite far from experiment results when looking the temperature evolution. But the behaviour is ok.

Adrià
Adri_12 is offline   Reply With Quote

Old   September 14, 2018, 11:23
Default
  #15
Member
 
Colli, Alejandro
Join Date: Jan 2014
Posts: 75
Rep Power: 6
ancolli is on a distinguished road
I think yes, you are doing something similar to the tutorial heat Exchanger. However, I can not see where to define the porosity in order to be taken into account by the heat equation either for porous zone and gas zone. Do you know how to set that variable in the present simulations?

Last edited by ancolli; September 28, 2018 at 20:10.
ancolli is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Can I use fvOptions to couple a solid region and a fluid region? titanchao OpenFOAM Running, Solving & CFD 1 March 7, 2018 07:46
Error - Solar absorber - Solar Thermal Radiation MichaelK CFX 12 September 1, 2016 05:15
Solid Temperature in porous Media iamsarthaknag STAR-CCM+ 1 May 23, 2016 07:14
Using starToFoam clo OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 33 September 26, 2012 04:04
CFX4.3 -build analysis form Chie Min CFX 5 July 12, 2001 23:19


All times are GMT -4. The time now is 01:51.