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

Modifying solidificationMeltingSource for Mushy zone phasechange

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

Like Tree4Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 30, 2017, 09:07
Post Modifying solidificationMeltingSource for Mushy zone phasechange
  #1
Member
 
a
Join Date: Oct 2014
Posts: 49
Rep Power: 8
cfd@kgp is on a distinguished road
Hi Foam experts,

I was trying to modify the solidificationMeltingSource (Isothermal ohase change source) for the mushy ploblems in OpenFoam version 3.0.

I was successful till defining the liquid fraction using Tsolidus and Tliquidus.

But some how I am unable to get the "Phi field" in order to add the term " fvc::div(phi, alpha1_))" in solidificationMeltingSourceTemplates.C.

Code:
\*---------------------------------------------------------------------------*/

#include "fvMatrices.H"
#include "fvcDdt.H"
#include "fvcDiv.H"


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

template<class RhoFieldType>
void Foam::fv::mushysolidificationMeltingSource::apply
(

    const RhoFieldType& rho,
    fvMatrix<scalar>& eqn
)
{
    if (debug)
    {
        Info<< type() << ": applying source to " << eqn.psi().name() << endl;
    }

    const volScalarField Cp(this->Cp());

    update(Cp);

    dimensionedScalar L("L", dimEnergy/dimMass, L_);

    // contributions added to rhs of solver equation
    if (eqn.psi().dimensions() == dimTemperature)
    {
        // isothermal phase change - only include time derivative
         eqn -= L/Cp*(fvc::ddt(rho, alpha1_) + fvc::div(phi, alpha1_)); //mushy phase change  
      //  eqn -= L/Cp*(fvc::ddt(rho, alpha1_));
    }
    else
    {
        // isothermal phase change - only include time derivative
         eqn -= L*(fvc::ddt(rho, alpha1_) + fvc::div(phi, alpha1_)); //mushy phase change  
       // eqn -= L*(fvc::ddt(rho, alpha1_));
    }
}


// ************************************************************************* //
I get following compilation error,

Code:
In file included from sources/derived/mushysolidificationMeltingSource/mushysolidificationMeltingSource.H:269:0,
                 from sources/derived/mushysolidificationMeltingSource/mushysolidificationMeltingSource.C:26:
sources/derived/mushysolidificationMeltingSource/mushysolidificationMeltingSourceTemplates.C: In member function ‘void Foam::fv::mushysolidificationMeltingSource::apply(const RhoFieldType&, Foam::fvMatrix<double>&)’:
sources/derived/mushysolidificationMeltingSource/mushysolidificationMeltingSourceTemplates.C:56:57: error: ‘phi’ was not declared in this scope
          eqn -= L/Cp*(fvc::ddt(rho, alpha1_) + fvc::div(phi, alpha1_)); //mushy phase change 
                                                         ^
sources/derived/mushysolidificationMeltingSource/mushysolidificationMeltingSourceTemplates.C:62:54: error: ‘phi’ was not declared in this scope
          eqn -= L*(fvc::ddt(rho, alpha1_) + fvc::div(phi, alpha1_)); //mushy phase change 
                                                      ^
sources/derived/mushysolidificationMeltingSource/mushysolidificationMeltingSource.C: In member function ‘void Foam::fv::mushysolidificationMeltingSource::update(const volScalarField&)’:
sources/derived/mushysolidificationMeltingSource/mushysolidificationMeltingSource.C:170:16: warning: unused variable ‘Cpc’ [-Wunused-variable]
         scalar Cpc = Cp[cellI];
                ^
make: *** [Make/linuxGccDPInt32Opt/sources/derived/mushysolidificationMeltingSource/mushysolidificationMeltingSource.o] Error 1
I have included the header file for the divergence term fvcDiv.H. should I include any other header file?

Thanks in advance.
kindly help
cfd@kgp is offline   Reply With Quote

Old   January 30, 2017, 11:46
Default
  #2
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 418
Rep Power: 19
cnsidero is on a distinguished road
The flux, phi, is not stored in that class (or parent classes) so you need to get a reference to it through the registry. Look in one of the other fvOptions sources that requires the flux for an example. The mesh is accessible so this should work:

Code:
const surfaceScalarField& phi =
        mesh_.lookupObject<surfaceScalarField>(phiName_);
-Chris
cnsidero is offline   Reply With Quote

Old   January 31, 2017, 04:46
Smile
  #3
Member
 
a
Join Date: Oct 2014
Posts: 49
Rep Power: 8
cfd@kgp is on a distinguished road
Quote:
Originally Posted by cnsidero View Post
The flux, phi, is not stored in that class (or parent classes) so you need to get a reference to it through the registry. Look in one of the other fvOptions sources that requires the flux for an example. The mesh is accessible so this should work:

Code:
const surfaceScalarField& phi =
        mesh_.lookupObject<surfaceScalarField>(phiName_);
-Chris
Thanks a lot cnsidero!
cfd@kgp is offline   Reply With Quote

Old   June 26, 2017, 02:19
Default
  #4
New Member
 
diwakar
Join Date: Sep 2016
Posts: 11
Rep Power: 6
janghel is on a distinguished road
hi cfd@kgp
were you able to run make the solver for solidificationMelting using fvOptions for mushy zone??
janghel is offline   Reply With Quote

Old   July 1, 2017, 13:44
Default
  #5
New Member
 
diwakar
Join Date: Sep 2016
Posts: 11
Rep Power: 6
janghel is on a distinguished road
Anyways I got it working for mushy zone ( both linear and schiel law case)
mikulo likes this.
janghel is offline   Reply With Quote

Old   September 6, 2017, 10:15
Default
  #6
New Member
 
Maurício Guilherme Alves dos Reis
Join Date: Feb 2015
Posts: 10
Rep Power: 8
MauricioReis is on a distinguished road
Quote:
Originally Posted by cnsidero View Post
The flux, phi, is not stored in that class (or parent classes) so you need to get a reference to it through the registry. Look in one of the other fvOptions sources that requires the flux for an example. The mesh is accessible so this should work:

Code:
const surfaceScalarField& phi =
        mesh_.lookupObject<surfaceScalarField>(phiName_);
-Chris
Hello,

I'm using OpenFOAM 4.1, I have made the proposed modifications, but the following error occurs during compilation:

error: ‘div’ is not a member of ‘Foam::fvc’
eqn -= L/Cp*(fvc::ddt(rho, alpha1_) + fvc::div(phi, alpha1_));


can anybody help me?
MauricioReis is offline   Reply With Quote

Old   September 14, 2017, 05:09
Default
  #7
Member
 
Bruno Lebon
Join Date: Dec 2012
Posts: 33
Rep Power: 10
blebon is on a distinguished road
Did you include fvcDiv.H?

My mushyZoneSourceTemplates.C file looks like this and it compiles fine:

Code:
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2014-2015 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 "fvMatrices.H"
#include "fvcDdt.H"
#include "fvcDiv.H"

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

template<class RhoFieldType>
void Foam::fv::mushyZoneSource::apply
(
    const RhoFieldType& rho,
    fvMatrix<scalar>& eqn
)
{
    if (debug)
    {
        Info<< type() << ": applying source to " << eqn.psi().name() << endl;
    }

    const surfaceScalarField& phi =
        mesh_.lookupObject<surfaceScalarField>(phiName_);

    const volScalarField Cp(this->Cp());

    update();

    dimensionedScalar L("L", dimEnergy/dimMass, L_);

    // contributions added to rhs of solver equation
    if (eqn.psi().dimensions() == dimTemperature)
    {
        // isothermal phase change - only include time derivative
        eqn -= L/Cp*(fvc::ddt(rho, alpha1_) + fvc::div(phi, alpha1_));
        // eqn -= L/Cp*(fvc::ddt(rho, alpha1_));
    }
    else
    {
        // isothermal phase change - only include time derivative
        eqn -= L*(fvc::ddt(rho, alpha1_) + fvc::div(phi, alpha1_));
        // eqn -= L*(fvc::ddt(rho, alpha1_));
    }
}


// ************************************************************************* //
blebon is offline   Reply With Quote

Old   September 14, 2017, 05:59
Default
  #8
New Member
 
diwakar
Join Date: Sep 2016
Posts: 11
Rep Power: 6
janghel is on a distinguished road
Quote:
Originally Posted by blebon View Post
Did you include fvcDiv.H?

My mushyZoneSourceTemplates.C file looks like this and it compiles fine:

Code:
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2014-2015 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 "fvMatrices.H"
#include "fvcDdt.H"
#include "fvcDiv.H"

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

template<class RhoFieldType>
void Foam::fv::mushyZoneSource::apply
(
    const RhoFieldType& rho,
    fvMatrix<scalar>& eqn
)
{
    if (debug)
    {
        Info<< type() << ": applying source to " << eqn.psi().name() << endl;
    }

    const surfaceScalarField& phi =
        mesh_.lookupObject<surfaceScalarField>(phiName_);

    const volScalarField Cp(this->Cp());

    update();

    dimensionedScalar L("L", dimEnergy/dimMass, L_);

    // contributions added to rhs of solver equation
    if (eqn.psi().dimensions() == dimTemperature)
    {
        // isothermal phase change - only include time derivative
        eqn -= L/Cp*(fvc::ddt(rho, alpha1_) + fvc::div(phi, alpha1_));
        // eqn -= L/Cp*(fvc::ddt(rho, alpha1_));
    }
    else
    {
        // isothermal phase change - only include time derivative
        eqn -= L*(fvc::ddt(rho, alpha1_) + fvc::div(phi, alpha1_));
        // eqn -= L*(fvc::ddt(rho, alpha1_));
    }
}


// ************************************************************************* //
Yes you have to include fvcDiv.H. your mushy template looks good to me. i think it will work.

-Diwakar Janghel
janghel is offline   Reply With Quote

Old   September 14, 2017, 06:03
Default
  #9
Member
 
Bruno Lebon
Join Date: Dec 2012
Posts: 33
Rep Power: 10
blebon is on a distinguished road
Thanks, I was replying to MauricioReis's error ... but since you are here, did you ever try to use a tabulated fraction liquid:

Code:
void Foam::fv::mushyZoneSource::update()
{
    if (curTimeIndex_ == mesh_.time().timeIndex())
    {
        return;
    }

    if (debug)
    {
        Info<< type() << ": " << name_ << " - updating phase indicator" << endl;
    }

    // update old time alpha1 field
    alpha1_.oldTime();

    const volScalarField& T = mesh_.lookupObject<volScalarField>(TName_);

    interpolationTable<scalar> fraction_curve("constant/fL");

    forAll(cells_, i)
    {
        label celli = cells_[i];

        scalar Tc = T[celli];
        scalar alpha1New;
        if (Tc < Tsolidus_)
        {
            alpha1New = 0.0;
        } else if (Tc < Tliquidus_) {
            alpha1New = fraction_curve(Tc);
        } else {
            alpha1New = 1.0;
        }

        alpha1_[celli] = max(0, min(alpha1New, 1));
    }

    alpha1_.correctBoundaryConditions();

    curTimeIndex_ = mesh_.time().timeIndex();
}
blebon is offline   Reply With Quote

Old   September 14, 2017, 06:13
Default
  #10
New Member
 
diwakar
Join Date: Sep 2016
Posts: 11
Rep Power: 6
janghel is on a distinguished road
Quote:
Originally Posted by blebon View Post
Thanks, I was replying to MauricioReis's error ... but since you are here, did you ever try to use a tabulated fraction liquid:

Code:
void Foam::fv::mushyZoneSource::update()
{
    if (curTimeIndex_ == mesh_.time().timeIndex())
    {
        return;
    }

    if (debug)
    {
        Info<< type() << ": " << name_ << " - updating phase indicator" << endl;
    }

    // update old time alpha1 field
    alpha1_.oldTime();

    const volScalarField& T = mesh_.lookupObject<volScalarField>(TName_);

    interpolationTable<scalar> fraction_curve("constant/fL");

    forAll(cells_, i)
    {
        label celli = cells_[i];

        scalar Tc = T[celli];
        scalar alpha1New;
        if (Tc < Tsolidus_)
        {
            alpha1New = 0.0;
        } else if (Tc < Tliquidus_) {
            alpha1New = fraction_curve(Tc);
        } else {
            alpha1New = 1.0;
        }

        alpha1_[celli] = max(0, min(alpha1New, 1));
    }

    alpha1_.correctBoundaryConditions();

    curTimeIndex_ = mesh_.time().timeIndex();
}
hii bruno

i did not get your question? are you talking about schiel law?
janghel is offline   Reply With Quote

Old   September 14, 2017, 06:23
Default
  #11
Member
 
Bruno Lebon
Join Date: Dec 2012
Posts: 33
Rep Power: 10
blebon is on a distinguished road
Yes, I implemented the fraction solid dependence on temperature using a temperature table ... which was itself calculated assuming Scheil solidification. Did you ever try this before? It converges fine ... to the wrong temperature profile.
blebon is offline   Reply With Quote

Old   September 14, 2017, 06:25
Default
  #12
New Member
 
diwakar
Join Date: Sep 2016
Posts: 11
Rep Power: 6
janghel is on a distinguished road
Quote:
Originally Posted by blebon View Post
Yes, I implemented the fraction solid dependence on temperature using a temperature table ... which was itself calculated assuming Scheil solidification. Did you ever try this before? It converges fine ... to the wrong temperature profile.
Can you share the formula which you are using to relate solid fraction with temperature..?
janghel is offline   Reply With Quote

Old   September 14, 2017, 06:35
Default
  #13
Member
 
Bruno Lebon
Join Date: Dec 2012
Posts: 33
Rep Power: 10
blebon is on a distinguished road
Not a formula, but a table:

Code:
(
    (  0   0)
    (873   0)
    (883.3 0.05)
    (884.7 0.1)
    (885.4 0.2)
    (886.8 0.3)
    (887.5 0.4)
    (891.6 0.5)
    (900.5 0.6)
    (907.4 0.7)
    (912.2 0.8)
    (913.6 0.9)
    (915.0 1.0)
   (9999   1.0)
)
blebon is offline   Reply With Quote

Old   September 14, 2017, 06:54
Default
  #14
New Member
 
diwakar
Join Date: Sep 2016
Posts: 11
Rep Power: 6
janghel is on a distinguished road
Quote:
Originally Posted by blebon View Post
Not a formula, but a table:

Code:
(
    (  0   0)
    (873   0)
    (883.3 0.05)
    (884.7 0.1)
    (885.4 0.2)
    (886.8 0.3)
    (887.5 0.4)
    (891.6 0.5)
    (900.5 0.6)
    (907.4 0.7)
    (912.2 0.8)
    (913.6 0.9)
    (915.0 1.0)
   (9999   1.0)
)
Sorry i did not try this. i just used the formula.
janghel is offline   Reply With Quote

Old   September 14, 2017, 08:59
Default
  #15
New Member
 
Maurício Guilherme Alves dos Reis
Join Date: Feb 2015
Posts: 10
Rep Power: 8
MauricioReis is on a distinguished road
Quote:
Originally Posted by blebon View Post
Did you include fvcDiv.H?

My mushyZoneSourceTemplates.C file looks like this and it compiles fine:

Code:
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2014-2015 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 "fvMatrices.H"
#include "fvcDdt.H"
#include "fvcDiv.H"

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

template<class RhoFieldType>
void Foam::fv::mushyZoneSource::apply
(
    const RhoFieldType& rho,
    fvMatrix<scalar>& eqn
)
{
    if (debug)
    {
        Info<< type() << ": applying source to " << eqn.psi().name() << endl;
    }

    const surfaceScalarField& phi =
        mesh_.lookupObject<surfaceScalarField>(phiName_);

    const volScalarField Cp(this->Cp());

    update();

    dimensionedScalar L("L", dimEnergy/dimMass, L_);

    // contributions added to rhs of solver equation
    if (eqn.psi().dimensions() == dimTemperature)
    {
        // isothermal phase change - only include time derivative
        eqn -= L/Cp*(fvc::ddt(rho, alpha1_) + fvc::div(phi, alpha1_));
        // eqn -= L/Cp*(fvc::ddt(rho, alpha1_));
    }
    else
    {
        // isothermal phase change - only include time derivative
        eqn -= L*(fvc::ddt(rho, alpha1_) + fvc::div(phi, alpha1_));
        // eqn -= L*(fvc::ddt(rho, alpha1_));
    }
}


// ************************************************************************* //
Thank you.
MauricioReis is offline   Reply With Quote

Old   November 15, 2017, 09:48
Default
  #16
Senior Member
 
Join Date: Sep 2013
Posts: 269
Rep Power: 16
Bloerb will become famous soon enough
Can someone explain to me why alpha is updated in the following fashion in the original solidificationMeltingSource? I understand that C*(Tc - Tmelt_) is basically the energy above the melt temperature. We devide by L to get a fraction....why is this needed though? Why not simple if T<Tmelt alpha=0 if T>Tmelt alpha=1...
Code:
        scalar alpha1New = alpha1_[celli] + relax_*Cpc*(Tc - Tmelt_)/L_;
And how would you update it for mushy problems? Something like this?
Code:
    alpha1 = 0.5*Foam::erf(4.0*(T-Tmelt)/(Tl-Ts))+scalar(0.5);
And again this would set it directly unlike the above method

Last edited by Bloerb; November 15, 2017 at 16:31.
Bloerb is offline   Reply With Quote

Old   April 12, 2018, 10:53
Smile
  #17
Member
 
a
Join Date: Oct 2014
Posts: 49
Rep Power: 8
cfd@kgp is on a distinguished road
Quote:
Originally Posted by Bloerb View Post
Can someone explain to me why alpha is updated in the following fashion in the original solidificationMeltingSource? I understand that C*(Tc - Tmelt_) is basically the energy above the melt temperature. We devide by L to get a fraction....why is this needed though? Why not simple if T<Tmelt alpha=0 if T>Tmelt alpha=1...
Code:
        scalar alpha1New = alpha1_[celli] + relax_*Cpc*(Tc - Tmelt_)/L_;
And how would you update it for mushy problems? Something like this?
Code:
    alpha1 = 0.5*Foam::erf(4.0*(T-Tmelt)/(Tl-Ts))+scalar(0.5);
And again this would set it directly unlike the above method

Bloerb/Stefan I am curious how did you implemented it using functions, please let us know your progress. meanwhile, I had send you a messege too, but not sure about its delivery so thought to get your response here.

Thanks in advance
cfd@kgp is offline   Reply With Quote

Old   May 10, 2018, 04:46
Default
  #18
Member
 
Bruno Lebon
Join Date: Dec 2012
Posts: 33
Rep Power: 10
blebon is on a distinguished road
Quote:
Originally Posted by Bloerb View Post
Can someone explain to me why alpha is updated in the following fashion in the original solidificationMeltingSource? I understand that C*(Tc - Tmelt_) is basically the energy above the melt temperature. We devide by L to get a fraction....why is this needed though? Why not simple if T<Tmelt alpha=0 if T>Tmelt alpha=1...
Code:
        scalar alpha1New = alpha1_[celli] + relax_*Cpc*(Tc - Tmelt_)/L_;
And how would you update it for mushy problems? Something like this?
Code:
    alpha1 = 0.5*Foam::erf(4.0*(T-Tmelt)/(Tl-Ts))+scalar(0.5);
And again this would set it directly unlike the above method
If you update melt_fraction using the if statement, energy is not conserved, because solution of the energy balance equation is based on previous values of melt fraction and hence inconsistent with the current temperature. If I am not mistaken, the correction process (i.e. what is implemented in solidificationMeltingSource) is based under the assumption that enthalpies is the same both for solving the energy balance equation and updating the melt fraction. Upon convergence of the iterative process, both energy is conserved and melt_fraction residuals should be very small.

When you have a mushy zone, you need to replace Tmelt_ but the temperature corresponding to alpha1_[celli] (either using a formula -- lever rule, Scheil or whatever --) or a lookup table.
blebon is offline   Reply With Quote

Old   May 10, 2018, 11:13
Default
  #19
Member
 
Tarang
Join Date: Feb 2011
Location: Delhi, India
Posts: 47
Rep Power: 12
gtarang is on a distinguished road
Hi,
I have made some changes in solidificationMeltingSource and I use it with tinkered buoyantPimpleSolver which I named as meltFoam. I basically solve energy equation before NS. Further, I solve Energy equation 'n' (nEnergyCorrector in PIMPLE dict) times so that energy equation converges reasonably before I move to next PIMPLE corrector. I am attaching both things here, feel free to comment or suggest improvements.
Attached Files
File Type: gz mySolidificationMeltingSource.tar.gz (5.3 KB, 63 views)
File Type: gz meltFoam.tar.gz (3.6 KB, 48 views)
Uyan, luks1910 and mikulo like this.
gtarang is offline   Reply With Quote

Old   January 25, 2021, 04:33
Smile Asking for which OF version?
  #20
New Member
 
michael villame
Join Date: Nov 2020
Posts: 11
Rep Power: 2
mikulo is on a distinguished road
Quote:
Originally Posted by gtarang View Post
Hi,
I have made some changes in solidificationMeltingSource and I use it with tinkered buoyantPimpleSolver which I named as meltFoam. I basically solve energy equation before NS. Further, I solve Energy equation 'n' (nEnergyCorrector in PIMPLE dict) times so that energy equation converges reasonably before I move to next PIMPLE corrector. I am attaching both things here, feel free to comment or suggest improvements.
Hi, thank you for your shared case files and solver. May I ask in which solver will it work? It would have been nice if it will work on OF 7. I will try it later..
mikulo is offline   Reply With Quote

Reply

Tags
melting openfoam, solidification, solidification/melting

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[Commercial meshers] Mesh conversion problem (fluent3DMeshToFoam) Aadhavan OpenFOAM Meshing & Mesh Conversion 2 March 8, 2018 01:47
Possible Bug in pimpleFoam (or createPatch) (or fluent3DMeshToFoam) cfdonline2mohsen OpenFOAM 3 October 21, 2013 09:28
[Commercial meshers] fluentMeshToFoam multidomain mesh conversion problem Attesz OpenFOAM Meshing & Mesh Conversion 12 May 2, 2013 10:52
Problem in running ICEM grid in Openfoam Tarak OpenFOAM 6 September 9, 2011 17:51
Problem in IMPORT of ICEM input file in FLUENT csvirume FLUENT 2 September 9, 2009 01:08


All times are GMT -4. The time now is 04:57.