[maruthamuthu_venkatraman]

Hello Foamers,
In order to check the heat flux balance i tried to use the utility wallHeatFlux. It seems it only works for Combustion solvers, when i run this utility for all those tutorial problems in heatTransfer it says as below:
-----------------------------------------------------------------------

Create time
Create mesh for time = 0
Time = 0
Selecting thermodynamics package hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>

Unknown hCombustionThermo type hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
Valid hCombustionThermo types are:
9
(
hPsiMixtureThermo<homogeneousMixture<sutherlandTra nsport<specieThermo<janafThermo<perfectGas>>>>>
hPsiMixtureThermo<reactingMixture<gasThermoPhysics >>
hPsiMixtureThermo<inhomogeneousMixture<constTransp ort<specieThermo<hConstThermo<perfectGas>>>>>
hPsiMixtureThermo<multiComponentMixture<gasThermoP hysics>>
hPsiMixtureThermo<veryInhomogeneousMixture<constTr ansport<specieThermo<hConstThermo<perfectGas>>>>>
hPsiMixtureThermo<homogeneousMixture<constTranspor t<specieThermo<hConstThermo<perfectGas>>>>>
hPsiMixtureThermo<inhomogeneousMixture<sutherlandT ransport<specieThermo<janafThermo<perfectGas>>>>>
hPsiMixtureThermo<veryInhomogeneousMixture<sutherl andTransport<specieThermo<janafThermo<perfectGas>> >>>
hPsiMixtureThermo<dieselMixture<sutherlandTranspor t<specieThermo<janafThermo<perfectGas>>>>>
)

From function hCombustionThermo::New(const fvMesh&)
in file combustionThermo/hCombustionThermo/newhCombustionThermo.C at line 66.
FOAM exiting
-----------------------------------------------------------------------

Then i tried to look at the wallHeatFlux utility and found "#include basicRhoThermo.H " is missing. I added to it and compiled the same. Again this doesnt solve the problem.

Any hints are welcome.

Thanks

[ulli]

Hello Maruthamuthu,
I did this like this
1. I copied the wallHeatFlux-dir into a new dir e.g. wallHeatFluxRho
2. I renamed the *c-File in dir wallHeatFluxRho to wallHeatFluxRho.c
3. I modified the name in "files" (Make –dir)
4. I replaced (with an editor) hCombustionThermo by basicPsiThermo (which is the base class, see Doxygen) in createFields.h and wallHeatFluxRho.c. I think this class has be renamed in 1.6
5. Than I complied with wclean/wmake
This should work.
Hope it helps
Ulrich

[maruthamuthu_venkatraman]

Thanks for your explanations.

Yes, it worked. I can able to run this utility for simpleRadiationFoam. I compiled BuoyantPisoRadiationFoam and tried to use wallHeatFluxRho utility. It doesnt work for that case. I will check it out in detail later.

[Pekka]

Hello Sir/Madam

I carried out benchmark calculations by using OF 1.6.x for cylinder on the cross flow and one interesting point is on the wall heat convection. Based on previous tips I do “wallHeatFluxRho” function so that I change “hCombustionThermo” to “basicRhoThermo” on wallHeatFluxRho.C and createFields.H files and complied with wclean/wmake. WallHeatFluxRho works on compressible e.g. BuoyantPisoFoam many different RASmodels but it works only realizableKE and LaunderSharmaKE models on the incompressible flow simulation (buoyantBoussinesqPisoFoam) . I use on the thermo physical models

“thermoType hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>;”.

How can I calculate wall heat flux on the incompressible case? WallHeatFluxRho function does not work with for example kOmegaSST model.

Thanks in advance

[maruthamuthu_venkatraman]

Hi Pekka,
I couldn't able to run thios utility wallHeatFluxRho for buoyantPisoFoam. The following error is showing up. Since you run this utility for buoyantPisoFoam , could you upload the sources. I will recompile and see my mistake.

Thanks.

-------------------------------Error Message---------------------------

Create time
Create mesh for time = 0
Time = 0
Selecting thermodynamics package hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>

Unknown basicPsiThermo type hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
Valid basicPsiThermo types are:
25
(
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
hhuMixtureThermo<veryInhomogeneousMixture<sutherla ndTransport<specieThermo<janafThermo<perfectGas>>> >>
hhuMixtureThermo<egrMixture<sutherlandTransport<sp ecieThermo<janafThermo<perfectGas>>>>>
hhuMixtureThermo<homogeneousMixture<constTransport <specieThermo<hConstThermo<perfectGas>>>>>
hPsiMixtureThermo<homogeneousMixture<sutherlandTra nsport<specieThermo<janafThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<eConstThermo<perfectGas>>>>>
hhuMixtureThermo<veryInhomogeneousMixture<constTra nsport<specieThermo<hConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
hPsiMixtureThermo<reactingMixture<gasThermoPhysics >>
hhuMixtureThermo<inhomogeneousMixture<sutherlandTr ansport<specieThermo<janafThermo<perfectGas>>>>>
hPsiMixtureThermo<inhomogeneousMixture<constTransp ort<specieThermo<hConstThermo<perfectGas>>>>>
hPsiMixtureThermo<multiComponentMixture<gasThermoP hysics>>
hPsiMixtureThermo<veryInhomogeneousMixture<constTr ansport<specieThermo<hConstThermo<perfectGas>>>>>
hhuMixtureThermo<egrMixture<constTransport<specieT hermo<hConstThermo<perfectGas>>>>>
hPsiMixtureThermo<homogeneousMixture<constTranspor t<specieThermo<hConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
hPsiMixtureThermo<inhomogeneousMixture<sutherlandT ransport<specieThermo<janafThermo<perfectGas>>>>>
hPsiMixtureThermo<veryInhomogeneousMixture<sutherl andTransport<specieThermo<janafThermo<perfectGas>> >>>
hPsiMixtureThermo<dieselMixture<sutherlandTranspor t<specieThermo<janafThermo<perfectGas>>>>>
ePsiThermo<pureMixture<constTransport<specieThermo <eConstThermo<perfectGas>>>>>
hhuMixtureThermo<homogeneousMixture<sutherlandTran sport<specieThermo<janafThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
hhuMixtureThermo<inhomogeneousMixture<constTranspo rt<specieThermo<hConstThermo<perfectGas>>>>>
)

From function basicPsiThermo::New(const fvMesh&)
in file psiThermo/basicPsiThermo/newBasicPsiThermo.C at line 64.
FOAM exiting
-----------------------------------------------------------------------

[Pekka]

Hi Maruthamuthu,


take a copy of wallHeatFlux folder and rename it, replace wallHeatFlux.C, createFiles.H and files to the new one and then compile. It should work with the BuoyantPisoFoam solver.


Has anybody any ideas how wall heat flux calculations are done for incompressible flow?

[Thomas Baumann]

Hi,

have a look at the discussion at
http://www.cfd-online.com/Forums/ope...oussinesq.html

Regards Thomas

[Pekka]

Hi,


thanks for the link and it clarified the problematics, but I have still the same problem with incompressible flow calculation. I change all kappaEff to alphaEff in the Tegn.H and recompiled it, but without success.

When I try post processing heat flux on the walls with wallHeatFluxRho function I get the following error:

----------Error message-------

Time = 0
Selecting thermodynamics package hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
Reading/calculating face flux field phi

Selecting RAS turbulence model kOmegaSST
--> Upgrading k to employ run-time selectable wall functions
Backup original k to k.old
Writing updated k
--> Upgrading omega to employ run-time selectable wall functions
Backup original omega to omega.old
Writing updated omega
--> Creating mut to employ run-time selectable wall functions
Writing new mut
--> Creating alphat to employ run-time selectable wall functions
Writing new alphat
#0 Foam::error::rintStack(Foam::Ostream&) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt at sigaction.c:0
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#5 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:erator/<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#6 Foam::compressible::RASModels::kOmegaSST::F2() const in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#7 Foam::compressible::RASModels::kOmegaSST::kOmegaSS T(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#8 Foam::compressible::RASModel::adddictionaryConstru ctorToTable<Foam::compressible::RASModels::kOmegaS ST>::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#9 Foam::compressible::RASModel::New(Foam::GeometricF ield<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#10 main in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/wallHeatFluxRho"
#11 __libc_start_main in "/lib64/libc.so.6"
#12 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/wallHeatFluxRho"
Floating point exception


Any ideas?


BR Pekka

[Pekka]

Hello Foamers,


The problem with wall flux calculation seems to be solved. On incompressible simulation modified wallHeatFlux utility gives “floating point exception” error when kOmegaSST model is used. I change pressure values from zero to 1e-12 on whole calculation field on first time step and then the wallHeatFluxRho utility works.


Can any OF guru tell me, is it possible to solve wall heat flux without any wall functions? What is the reason for changing the wall function to compressible wall function during run the wallHeatFlux utility?


Have I understood correctly that the RAS-model sets the wall functions on the wallHeatFlux utility? For example, if I use the kOmegaSST model the wallHeatFlux utility changes the wall functions to compressible:: omegaWallFunction; and low-Re models zeroGradient; boundary conditions be kept up, is it OK?


Thanks in advance

[mh.sedagaht@gmail.com]

hello
my new username is the next one

[M.H.Sedaghat]

hello
I change the wallHeatFlux files for laminar force and free convection heat transfer solvers(e.g. icoFoam with temperature for laminar force convection and boussinesqBuoyantFoam for laminar natural convection).
It works properly. I rename it wallHeatFluxLaminar. you can download it .

please visit our website:
http://sarreshtehdari.net/

[maddalena]

... and what about solvers that require multiple regions, as for example chtMultiRegionFoam? It can be interesting to evaluate the convective heat transfer at the interfaces...
Does someone has an application for this kind of problem as well?
regards,

mad

[crmccreary]

I've been mucking around trying to get a version of wallHeatFlux to work for CHT to no avail. If someone has a suggested roadmap or maybe some pointers, I'd be glad to do the coding.

[swahono]

Hello wallHeatFlux enthusiasts!

I have been also trying to modify the wallHeatFlux utility to work with chtMultiRegionSimpleFoam - however not successful yet.
The modified code compiled ok, but (i think) give wrong result.

Can anyone help us please.... Uncle Hrv?

This is my modified chtWallHeatFluxRho.C:

#include "fvCFD.H"
#include "basicPsiThermo.H"
#include "RASModel.H"
#include "fixedGradientFvPatchFields.H"
#include "wallFvPatch.H"
#include "regionProperties.H"

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

int main(int argc, char *argv[])
{
    timeSelector::addOptions();
    #include "setRootCase.H"
    #include "createTime.H"

    regionProperties rp(runTime);

    #include "createFluidMeshes.H"
//    #include "createSolidMeshes.H"

    #include "createFluidFields.H"
//    #include "createSolidFields.H"

    forAll(fluidRegions, i)
    {
    instantList timeDirs = timeSelector::select0(runTime, args);

    Info<< "\nSolving for fluid region " << fluidRegions[i].name() << endl;

    forAll(timeDirs, timeI)
    {
        runTime.setTime(timeDirs[timeI], timeI);
        Info<< "Time = " << runTime.timeName() << endl;
        fluidRegions[i].readUpdate();

        surfaceScalarField heatFlux =
            fvc::interpolate(KFluid[i])*fvc::snGrad(thermoFluid[i].h());

        const surfaceScalarField::GeometricBoundaryField& patchHeatFlux =
            heatFlux.boundaryField();

        Info<< "\nWall heat fluxes [W]" << endl;
        forAll(patchHeatFlux, patchi)
        {
            if (isA<wallFvPatch>(fluidRegions[i].boundary()[patchi]))
            {
                Info<< fluidRegions[i].boundary()[patchi].name()
                    << " "
                    << sum
                       (
                           fluidRegions[i].magSf().boundaryField()[patchi]
                          *patchHeatFlux[patchi]
                       )
                    << endl;
            }
        }
        Info<< endl;
        forAll(wallHeatFluxFluid[i].boundaryField(), patchi)
        {
            wallHeatFluxFluid[i].boundaryField()[patchi] = patchHeatFlux[patchi];
        }
        wallHeatFluxFluid[i].write();
    }
 }
    Info<< "End" << endl;
    return 0;
}

Basically, I just changed the #include createFields.H to createFluidFields.H by copying $FOAM_APP/solvers/heatTransfer/chtMultiRegionSimpleFoam to the directory where chtWallHeatFluxRho.C is

I also changed the 'mesh' to fluidRegions[i], by including the createFluidMeshes.H taken from the same directory above.

Oh, I also added declaration for the new variable 'wallHeatFluxFluid' in the copied createFluidFields.H file.

...
    PtrList<volScalarField> wallHeatFluxFluid(fluidRegions.size());

    // Populate fluid field pointer lists
    forAll(fluidRegions, i)
    {
...

Pleasee, can anyone verify/help and further correcting the modification?

Thank you very much.

Hopefully we can develop this marvelous utility to work with every solvers in OF 1.7.0.

Best regards,
Stefano

[swahono]

Hi Again,

Another thing with the chtWallHeatFluxRho above,

During runtime, it returns the following error:

Solving for fluid region bottomAir
Time = 0

Wall heat fluxes [W]
minY 0
minZ 0
maxZ 0
bottomAir_to_solidWall 345600


--> FOAM FATAL ERROR: 
hanging pointer, cannot dereference

    From function PtrList::operator[]
    in file /home/stefano/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/PtrListI.H at line 122.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/home/stefano/OpenFOAM/OpenFOAM-1.7.0/lib/linuxGccDPOpt/libOpenFOAM.so"
#1  Foam::error::abort() in "/home/stefano/OpenFOAM/OpenFOAM-1.7.0/lib/linuxGccDPOpt/libOpenFOAM.so"
#2  
 in "/home/stefano/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linuxGccDPOpt/chtWallHeatFluxRho"
#3  __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#4  
 in "/home/stefano/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linuxGccDPOpt/chtWallHeatFluxRho"
Aborted

Thank you future helper!

Cheers,
Stefano

[aerothermal]

Dear All,

I am running some flow cases around a circular cylinder with isothermal and rough surface and heat transfer.

So I picked your suggestions and put together an utility that worked with rhoSimpleFoam, RAS compreesible, kOmegaSST model and rough wall function.

See attached but I do not know if it works in other solvers.

Regards,

Guilherme

[Tobi]

Hey aerothermal,

nice tool it 's working fine but if i got the patchtype:

    siliziumoxid_to_ziegelstein
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value           uniform 730;
        neighbourFieldName T;
        K               K;
    }

Its not possible to solve it.
Any solutions ?

I ve used chtMultirRegionSimpleFoam


tobi

[NicolasB]

Hi!
Since I've got some problems using chtMultiRegionSimpleFoam, I'd like to check the heat fluxes. Obviously wallHeatFlux doesn't work in my case, therefore I've tried the wallHeatFluxRho utility.
Here is what I get :

$ wallHeatFluxRho 
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 1.7.0-113391ee57bd
Exec   : wallHeatFluxRho
Date   : Apr 20 2011
Time   : 11:08:16
Host   : caelinux-desktop
PID    : 4575
Case   : /home/caelinux/OpenFOAM/caelinux-1.7.0/Freyssinet3
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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

Create mesh for time = 0

Time = 0
Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>
#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam170/lib/linux64GccDPOpt/libOpenFOAM.so"
#1  Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam170/lib/linux64GccDPOpt/libOpenFOAM.so"
#2   in "/lib/libc.so.6"
#3  Foam::hPsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::calculate() in "/opt/openfoam170/lib/linux64GccDPOpt/libbasicThermophysicalModels.so"
#4  Foam::hPsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::hPsiThermo(Foam::fvMesh const&) in "/opt/openfoam170/lib/linux64GccDPOpt/libbasicThermophysicalModels.so"
#5  Foam::basicPsiThermo::addfvMeshConstructorToTable<Foam::hPsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > > >::New(Foam::fvMesh const&) in "/opt/openfoam170/lib/linux64GccDPOpt/libbasicThermophysicalModels.so"
#6  Foam::basicPsiThermo::New(Foam::fvMesh const&) in "/opt/openfoam170/lib/linux64GccDPOpt/libbasicThermophysicalModels.so"
#7  
 in "/home/caelinux/OpenFOAM/caelinux-1.7.0/applications/bin/linux64GccDPOpt/wallHeatFluxRho"
#8  __libc_start_main in "/lib/libc.so.6"
#9  
 in "/home/caelinux/OpenFOAM/caelinux-1.7.0/applications/bin/linux64GccDPOpt/wallHeatFluxRho"
Exception en point flottant

More details about my case on this thread

How may I fix this issue?
Thank you in advance for your help.

[Tobi]

Hey nikolas,

i think, you can't use the wallHeatFluxRho tool with chtMulti directly.
You have to change your case a little bit. Like you 've solve every region single.

Never have tried to use a wallHeatFlux Tool with cht Multi - but i ll test it if i 'd time

Regards Tobi

[NicolasB]

Hi Tobias,

Thanks to your hint, I've succeeded in computing the heat fluxes for the fluid zone (but at the inlet and outlet which are not walls).
When I prompt for the fluxes in solid region, I've got the next error:

$ wallHeatFluxRho 
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 1.7.0-113391ee57bd
Exec   : wallHeatFluxRho
Date   : Apr 20 2011
Time   : 14:03:58
Host   : caelinux-desktop
PID    : 6225
Case   : /home/caelinux/OpenFOAM/caelinux-1.7.0/Freyssinet3/beton
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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

Create mesh for time = 0

Time = 0


--> FOAM FATAL IO ERROR: 
cannot open file

file: /home/caelinux/OpenFOAM/caelinux-1.7.0/Freyssinet3/beton/constant/thermophysicalProperties at line 0.

    From function regIOobject::readStream()
    in file db/regIOobject/regIOobjectRead.C at line 61.

FOAM exiting

Obviously I miss the solid thermophysicalProperties file: I thought the files Cp, K, rho and T were sufficient. Can you give me a sample of such a file? There wasn't any in the multiRegionHeater tutorial, and I really don't know what to write in it.

Thanks again