CFD Online URL
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

chtMultiRegionSimpleFoam: strange error

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   October 9, 2013, 11:22
Default chtMultiRegionSimpleFoam: strange error
  #1
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 455
Rep Power: 9
samiam1000 is on a distinguished road
Dear all,

trying to run my chtMultiRegionSimpleFoam simulation, I get this error:

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.1-57f3c3617a2d
Exec   : chtMultiRegionSimpleFoam
Date   : Oct 09 2013
Time   : 16:09:54
Host   : "lab-laptop"
PID    : 7471
Case   : /home/lab/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create fluid mesh for region fluid for time = 0

Create solid mesh for region domain1 for time = 0

Create solid mesh for region domain2 for time = 0

Create solid mesh for region domain3 for time = 0



--> FOAM FATAL IO ERROR: 
keyword type is undefined in dictionary ".T"

file: .T from line 49 to line 66.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 402.

FOAM exiting

lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady$
The point is that it does not suggest me which is the corrupted file. Any idea? Is the error supposed to be in the domain3 region? Or domain3 is ok and I have to look in the next ones?

Thanks a lot,
Samuele
samiam1000 is offline   Reply With Quote

Old   October 12, 2013, 16:16
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 7,511
Blog Entries: 33
Rep Power: 74
wyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the rough
Hi Samuele,

Try this:
Code:
find . -name ".T"
It will tell you where the files named ".T" are located.

By the way, on Linux, files that start with "." are usually considered as hidden files. To see then, use the "-a" option with "ls" or "ll", for examples:
Code:
ls -a
ll -a
ls -la
The two last ones should be the same, because "ll" is an alias (when defined as such), as proved by this command:
Code:
alias ll
Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   October 14, 2013, 05:04
Default
  #3
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 455
Rep Power: 9
samiam1000 is on a distinguished road
I Bruno,

the point is that there was not such a file :-/..

..I've changed the folder case name and not I don't have this error.

But I have this new one:

Code:
lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady$ chtMultiRegionSimpleFoam 
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.1-57f3c3617a2d
Exec   : chtMultiRegionSimpleFoam
Date   : Oct 14 2013
Time   : 08:55:57
Host   : "lab-laptop"
PID    : 2667
Case   : /home/lab/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create fluid mesh for region fluid for time = 0

Create solid mesh for region domain1 for time = 0

Create solid mesh for region domain2 for time = 0

Create solid mesh for region domain3 for time = 0

Create solid mesh for region domain5 for time = 0

Create solid mesh for region packs for time = 0

*** Reading fluid mesh thermophysical properties for region fluid

    Adding to thermoFluid

Selecting thermodynamics package heRhoThermo<pureMixture<const<hConst<perfectGas<specie>>,sensibleEnthalpy>>>
#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
#4  Foam::rhoThermo::addfvMeshConstructorToTable<Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::New(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
#5  Foam::autoPtr<Foam::rhoThermo> Foam::basicThermo::New<Foam::rhoThermo>(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
#6  Foam::rhoThermo::New(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
#7  
 in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9  
 in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
Floating point exception (core dumped)
lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady$ 
lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady$ 
lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady$ 
lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady$
Could you help?

Thanks a lot,
Samuele
samiam1000 is offline   Reply With Quote

Old   October 14, 2013, 07:38
Default
  #4
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 988
Blog Entries: 4
Rep Power: 18
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi Samuel,

the first error is nice - never seen that befor.

The last error "Floating Point exeption" occure if you are dividing by Zero.

Check all your BC and set always the "value uniform X" keyword.

But hmmm ... it seems that you get the error while updating the thermodynamics. Maybe when the constructor is selected.

But first check my first hint.
Your meshes are okay?
Boundary files okay too?

Regards
Tobi
Tobi is offline   Reply With Quote

Old   October 14, 2013, 08:49
Default
  #5
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 455
Rep Power: 9
samiam1000 is on a distinguished road
Dear Tobi,

thanks for answering. Well, let me have a look at all the BC. Anyway, I am pretty confident it is ok! As far as the mesh is concerned, it should be alright.

I'll give you a feedback, soon.

Thanks a lot,
Samuele
samiam1000 is offline   Reply With Quote

Old   October 21, 2013, 06:39
Default
  #6
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 455
Rep Power: 9
samiam1000 is on a distinguished road
Dear Tobi,

I have checked all the BC and I have done some modifications.

The point is that now I have done a small step ahead, but there still is something wrong:

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.1-57f3c3617a2d
Exec   : chtMultiRegionSimpleFoam
Date   : Oct 21 2013
Time   : 11:26:34
Host   : "lab-laptop"
PID    : 4069
Case   : /home/lab/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create fluid mesh for region fluid for time = 0

Create solid mesh for region domain1 for time = 0

Create solid mesh for region domain2 for time = 0

Create solid mesh for region domain3 for time = 0

Create solid mesh for region domain5 for time = 0

Create solid mesh for region packs for time = 0

*** Reading fluid mesh thermophysical properties for region fluid

    Adding to thermoFluid

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

    Adding to rhoFluid

    Adding to UFluid

    Adding to phiFluid

    Adding to gFluid

    Adding to turbulence

Selecting turbulence model type RASModel
Selecting RAS turbulence model kEpsilon
--> Upgrading k to employ run-time selectable wall functions
    Backup original k to k.old
    Writing updated k
--> Upgrading epsilon to employ run-time selectable wall functions
    Backup original epsilon to epsilon.old
    Writing updated epsilon
--> Creating mut to employ run-time selectable wall functions
    Writing new mut
--> Creating alphat to employ run-time selectable wall functions
    Writing new alphat
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    C3              -0.33;
    sigmak          1;
    sigmaEps        1.3;
    Prt             1;
}

    Adding to ghFluid

    Adding to ghfFluid

--> FOAM Warning : 
    From function Field<Type>::Field(const word& keyword, const dictionary&, const label)
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.2.1/src/OpenFOAM/lnInclude/Field.C at line 262
    Reading "/home/lab/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady/0/fluid/p_rgh" from line 18 to line 20
    expected keyword 'uniform' or 'nonuniform', assuming deprecated Field format from Foam version 2.0.
--> FOAM Warning : 
    From function Field<Type>::Field(const word& keyword, const dictionary&, const label)
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.2.1/src/OpenFOAM/lnInclude/Field.C at line 262
    Reading "/home/lab/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady/0/fluid/p_rgh.boundaryField.intake" from line 55 to line 20
    expected keyword 'uniform' or 'nonuniform', assuming deprecated Field format from Foam version 2.0.
Selecting radiationModel none
    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region domain1

    Adding to thermos

Selecting thermodynamics package 
{
    type            heSolidThermo;
    mixture         pureMixture;
    transport       constIso;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

    Adding to radiations

Radiation model not active: radiationProperties not found
Selecting radiationModel none
    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region domain2

    Adding to thermos

Selecting thermodynamics package 
{
    type            heSolidThermo;
    mixture         pureMixture;
    transport       constIso;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

    Adding to radiations

Radiation model not active: radiationProperties not found
Selecting radiationModel none
    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region domain3

    Adding to thermos

Selecting thermodynamics package 
{
    type            heSolidThermo;
    mixture         pureMixture;
    transport       constIso;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

    Adding to radiations

Radiation model not active: radiationProperties not found
Selecting radiationModel none
    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region domain5

    Adding to thermos

Selecting thermodynamics package 
{
    type            heSolidThermo;
    mixture         pureMixture;
    transport       constIso;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigSegv::sigHandler(int) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::tmp<Foam::Field<double> > Foam::fvPatch::patchInternalField<double>(Foam::UList<double> const&) const in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#4  Foam::fvPatchField<double>::patchInternalField() const in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#5  Foam::basicSymmetryFvPatchField<double>::evaluate(Foam::UPstream::commsTypes) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#6  Foam::symmetryFvPatchField<double>::symmetryFvPatchField(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#7  Foam::fvPatchField<double>::adddictionaryConstructorToTable<Foam::symmetryFvPatchField<double> >::New(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#8  Foam::fvPatchField<double>::New(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#9  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::readField(Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#10  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::readFields(Foam::dictionary const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#11  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::readFields() in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#12   at basicThermo.C:0
#13  Foam::basicThermo::lookupOrConstruct(Foam::fvMesh const&, char const*) const in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
#14  Foam::basicThermo::basicThermo(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
#15  Foam::solidThermo::solidThermo(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libsolidThermo.so"
#16  Foam::heThermo<Foam::solidThermo, Foam::pureMixture<Foam::constIsoSolidTransport<Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie> >, Foam::sensibleEnthalpy> > > >::heThermo(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libsolidThermo.so"
#17  Foam::solidThermo::addfvMeshConstructorToTable<Foam::heSolidThermo<Foam::solidThermo, Foam::pureMixture<Foam::constIsoSolidTransport<Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::New(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libsolidThermo.so"
#18  Foam::autoPtr<Foam::solidThermo> Foam::basicThermo::New<Foam::solidThermo>(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libsolidThermo.so"
#19  Foam::solidThermo::New(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libsolidThermo.so"
#20  
 in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#21  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#22  
 in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
Segmentation fault (core dumped)
Any idea about this `new' (for me) error?
samiam1000 is offline   Reply With Quote

Old   October 21, 2013, 07:28
Default
  #7
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 988
Blog Entries: 4
Rep Power: 18
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi,

first of all post the p_rgh file (0/fluid/p_rgh).
And the second error (Segmentation fault) is in your domain5. You have an error there.
Tobi is offline   Reply With Quote

Old   October 21, 2013, 07:47
Default
  #8
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 455
Rep Power: 9
samiam1000 is on a distinguished road
Thanks Tobi.

Here is my p_rgh file:

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [ 1 -1 -2 0 0 0 0 ];

internalField   100000;

boundaryField
{
    wall-fluid
    {
        type            buoyantPressure;
        value           $internalField;
    }
    back
    {
        type            buoyantPressure;
        value           $internalField;
    }
    empty_1
    {
        type            buoyantPressure;
        value           $internalField;
    }
    empty_2-fluid
    {
        type            symmetryPlane;
    }
    glass
    {
        type            buoyantPressure;
        value           $internalField;
    }
    inlet_main
    {
        type            buoyantPressure;
        value           $internalField;
    }
    intake
    {
        type            fixedValue;
        value           $internalField;
    }
    pcm_surface
    {
        type            buoyantPressure;
        value           $internalField;
    }
    fluid_to_domain5
    {
        type            buoyantPressure;
        value           $internalField;
    }
    fluid_to_domain3
    {
        type            buoyantPressure;
        value           $internalField;
    }
    fluid_to_domain1
    {
        type            buoyantPressure;
        value           $internalField;
    }
    fluid_to_packs
    {
        type            buoyantPressure;
        value           $internalField;
    }
    fluid_to_domain2
    {
        type            buoyantPressure;
        value           $internalField;
    }
}


// ************************************************************************* //
and here the domain5 changeLogDict:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      changeDictionaryDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dictionaryReplacement
{
    boundary
    {
        empty_2-packs
        {
            type            symmetryPlane;
            nFaces          1342;
            startFace       47303;
        }
        wall_packs
        {
            type            wall;
            nFaces          705;
            startFace       48645;
        }
        domain5_to_fluid
        {
            type            mappedWall;
            nFaces          3997;
            startFace       49350;
            sampleMode      nearestPatchFace;
            sampleRegion    fluid;
            samplePatch     fluid_to_domain1;
            offsetMode      uniform;
            offset          (0 0 0);
        }
    }

    T
    {
        internalField   uniform 298;

        boundaryField
        {
            empty_2-packs
            {
                type            symmetryPlane;
            }
            wall_packs
            {
                type            zeroGradient;
            }
            domain5_to_fluid
            {
                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                value           uniform 298;
                neighbourFieldName T;
                kappa           solidThermo;
                kappaName       none;
            }
        }
    }

    p
    {
        internalField   uniform 100000;

        boundaryField
        {
            empty_2-packs
            {
                type            symmetryPlane;
            }
            wall_packs
            {
                type            calculated;
                value           uniform 0;
            }
            domain5_to_fluid
            {
                type            calculated;
                value           uniform 0;
            }
        }
    }
}
Thanks for answering and helping,
Samuele
samiam1000 is offline   Reply With Quote

Old   October 21, 2013, 10:26
Default
  #9
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 455
Rep Power: 9
samiam1000 is on a distinguished road
Hi Tobi,

following your advice, I solved an error, but I now get this message:

Code:
Attempt to cast type calculated to type compressible::turbulentTemperatureCoupledBaffleMixed
However, I think that my BC are properly set. Where may the error be, according to you?

Thanks a lot,
Samuele
samiam1000 is offline   Reply With Quote

Old   October 21, 2013, 12:02
Default
  #10
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 988
Blog Entries: 4
Rep Power: 18
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi

Code:
       domain5_to_fluid
        {
            type            mappedWall;
            nFaces          3997;
            startFace       49350;
            sampleMode      nearestPatchFace;
            sampleRegion    fluid;
            samplePatch     fluid_to_domain1;  // should be fluid_to_domain5 
            offsetMode      uniform;
            offset          (0 0 0);
        }
The other error... can you give me more information?
Tobi is offline   Reply With Quote

Old   October 21, 2013, 12:12
Default
  #11
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 455
Rep Power: 9
samiam1000 is on a distinguished road
Yeah: it's right.

About the `new error', here is the complete message:

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.1-57f3c3617a2d
Exec   : chtMultiRegionSimpleFoam
Date   : Oct 21 2013
Time   : 16:10:36
Host   : "lab-laptop"
PID    : 2401
Case   : /home/lab/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create fluid mesh for region fluid for time = 0

Create solid mesh for region domain1 for time = 0

Create solid mesh for region domain2 for time = 0

Create solid mesh for region domain3 for time = 0

Create solid mesh for region domain5 for time = 0

Create solid mesh for region packs for time = 0

*** Reading fluid mesh thermophysical properties for region fluid

    Adding to thermoFluid

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

    Adding to rhoFluid

    Adding to UFluid

    Adding to phiFluid

    Adding to gFluid

    Adding to turbulence

Selecting turbulence model type RASModel
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    C3              -0.33;
    sigmak          1;
    sigmaEps        1.3;
    Prt             1;
}

    Adding to ghFluid

    Adding to ghfFluid

--> FOAM Warning : 
    From function Field<Type>::Field(const word& keyword, const dictionary&, const label)
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.2.1/src/OpenFOAM/lnInclude/Field.C at line 262
    Reading "/home/lab/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady/0/fluid/p_rgh" from line 18 to line 20
    expected keyword 'uniform' or 'nonuniform', assuming deprecated Field format from Foam version 2.0.
--> FOAM Warning : 
    From function Field<Type>::Field(const word& keyword, const dictionary&, const label)
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.2.1/src/OpenFOAM/lnInclude/Field.C at line 262
    Reading "/home/lab/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady/0/fluid/p_rgh.boundaryField.intake" from line 55 to line 20
    expected keyword 'uniform' or 'nonuniform', assuming deprecated Field format from Foam version 2.0.
Selecting radiationModel none
    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region domain1

    Adding to thermos

Selecting thermodynamics package 
{
    type            heSolidThermo;
    mixture         pureMixture;
    transport       constIso;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

    Adding to radiations

Radiation model not active: radiationProperties not found
Selecting radiationModel none
    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region domain2

    Adding to thermos

Selecting thermodynamics package 
{
    type            heSolidThermo;
    mixture         pureMixture;
    transport       constIso;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

    Adding to radiations

Radiation model not active: radiationProperties not found
Selecting radiationModel none
    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region domain3

    Adding to thermos

Selecting thermodynamics package 
{
    type            heSolidThermo;
    mixture         pureMixture;
    transport       constIso;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

    Adding to radiations

Radiation model not active: radiationProperties not found
Selecting radiationModel none
    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region domain5

    Adding to thermos

Selecting thermodynamics package 
{
    type            heSolidThermo;
    mixture         pureMixture;
    transport       constIso;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

    Adding to radiations

Radiation model not active: radiationProperties not found
Selecting radiationModel none
    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region packs

    Adding to thermos

Selecting thermodynamics package 
{
    type            heSolidThermo;
    mixture         pureMixture;
    transport       constIso;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

    Adding to radiations

Radiation model not active: radiationProperties not found
Selecting radiationModel none
    Adding fvOptions

No finite volume options present

Time = 1


Solving for fluid region fluid
DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 0.00545361, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 0.018735, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 0.00880018, No Iterations 1


--> FOAM FATAL ERROR: 
Attempt to cast type zeroGradient to type compressible::turbulentTemperatureCoupledBaffleMixed

    From function refCast<To>(From&)
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.2.1/src/OpenFOAM/lnInclude/typeInfo.H at line 114.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  Foam::compressible::turbulentTemperatureCoupledBaffleMixedFvPatchScalarField::updateCoeffs() in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libcompressibleTurbulenceModel.so"
#3  Foam::mixedFvPatchField<double>::evaluate(Foam::UPstream::commsTypes) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#4  Foam::mixedEnergyFvPatchScalarField::updateCoeffs() in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
#5  Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#6  
 in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#7  
 in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9  
 in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
Aborted (core dumped)
samiam1000 is offline   Reply With Quote

Old   October 21, 2013, 13:02
Default
  #12
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 988
Blog Entries: 4
Rep Power: 18
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
T file of fluid please and the boundary file of your fluid domain.
Tobi is offline   Reply With Quote

Old   October 23, 2013, 03:56
Default
  #13
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 455
Rep Power: 9
samiam1000 is on a distinguished road
Tobi,

pardon for the late answer. I was out of office and I did not have the case with me. Sorry,

Anyway, the file that you want is here:

Code:
    T
    {
        internalField   uniform 298;

        boundaryField
        {
            wall-fluid
            {
                type            zeroGradient;
                value           uniform 273;
            }
            back
            {
                type            zeroGradient;
//                type            fixedValue;
                value           uniform 273;
            }
            empty_1
            {
                type            zeroGradient;
                value           uniform 273;
            }
            empty_2-fluid
            {
                type            symmetryPlane;
            }
            glass
            {
                type            fixedValue;
                value           uniform 298;
            }
            inlet_main
            {
                type            fixedValue;
                value           uniform 273;
            }
            intake
            {
                type            zeroGradient;
                value           uniform 273;
            }
            pcm_surface
            {
                type            fixedValue;
                value           uniform 275;
            }
            fluid_to_domain5
            {
                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                neighbourFieldName T;
                kappa           fluidThermo;
                kappaName       none;
                value           uniform 278;
            }
            fluid_to_domain3
            {
                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                neighbourFieldName T;
                kappa           fluidThermo;
                kappaName       none;
                value           uniform 278;
            }
            fluid_to_domain1
            {
                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                neighbourFieldName T;
                kappa           fluidThermo;
                kappaName       none;
                value           uniform 278;
            }
            fluid_to_packs
            {
                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                neighbourFieldName T;
                kappa           fluidThermo;
                kappaName       none;
                value           uniform 278;
            }
            fluid_to_domain2
            {
                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                neighbourFieldName T;
                kappa           fluidThermo;
                kappaName       none;
                value           uniform 278;
            }
        }
    }
Is there something strange?
samiam1000 is offline   Reply With Quote

Old   October 23, 2013, 05:37
Default
  #14
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 455
Rep Power: 9
samiam1000 is on a distinguished road
Tobi,

I have solved that problem, changing the BC. But I still have troubles: now I get this message:

Code:
Solving for solid region domain1


--> FOAM FATAL ERROR: 

    gradientInternalCoeffs cannot be called for a calculatedFvPatchField
    on patch domain1_to_fluid of field h in file "/home/lab/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady/0/domain1/h"
    You are probably trying to solve for a field with a default boundary condition.

    From function calculatedFvPatchField<Type>::gradientInternalCoeffs() const
    in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 199.

FOAM exiting
The point is that I don't have any h file, anywhere.

Any idea about this?
samiam1000 is offline   Reply With Quote

Old   October 23, 2013, 08:03
Default
  #15
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 988
Blog Entries: 4
Rep Power: 18
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi,

the T-file Looks good.
The Problem in the cht solver is always that the Domains are related to each other and the Problem could be in both. I worked a Long time with the cht but at the Moment I am not working anymore with it.

Therefor I am getting rusty in the error Messages

Is it possible to upload you 0 Folder and the constant Folder, best way would be the whole case.

Maybe its not possible for you (due to secret) it would be very good to have the 0 Folder and the constant/***/polyMesh/boundary files to have a look at the whole case. It would be the best way to give you a correct answer.

Otherwise you should always get more Information

So if you solving "domain1_to_fluid" it is interessting to have the related files of both Domains.



For your Problem it could be possible that you use "fluidThermo" in the T file for your solid Domain. there should be "solidThermo".

Regards Tobi
Tobi is offline   Reply With Quote

Old   October 23, 2013, 09:20
Default
  #16
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 455
Rep Power: 9
samiam1000 is on a distinguished road
I can share the case with you via Skype. I have tried to contact you there.

If you are online, please let me know. Otherwise, please write me at samuele.zampini@polimi.com and I'll send you tha case.

Thank you very much,
Samuele
samiam1000 is offline   Reply With Quote

Old   October 23, 2013, 09:39
Default
  #17
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 988
Blog Entries: 4
Rep Power: 18
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi Samuel,

i am online today evening (in 2 hours).
Otherwise you can send me the case Tobias.Holzmann@Holzmann-cfd.de

Regards

Tobi
Tobi is offline   Reply With Quote

Old   October 23, 2013, 12:10
Default
  #18
Senior Member
 
Ahmed Khattab's Avatar
 
ahmed
Join Date: Feb 2010
Posts: 161
Blog Entries: 1
Rep Power: 6
Ahmed Khattab is on a distinguished road
Quote:
Originally Posted by samiam1000 View Post
Tobi,

I have solved that problem, changing the BC. But I still have troubles: now I get this message:

Code:
Solving for solid region domain1


--> FOAM FATAL ERROR: 

    gradientInternalCoeffs cannot be called for a calculatedFvPatchField
    on patch domain1_to_fluid of field h in file "/home/lab/Documenti/Ethics/FRISBEE/CFD/testVerticalTN_PCM/PCMPacks/steady/0/domain1/h"
    You are probably trying to solve for a field with a default boundary condition.

    From function calculatedFvPatchField<Type>::gradientInternalCoeffs() const
    in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 199.

FOAM exiting
The point is that I don't have any h file, anywhere.

Any idea about this?

Hi,

i experienced such a problem before, already today. i found that my mistake was in changeDirectoryDict where i wrongly wrote than name of interface patch, i simply change uppercase letter to lowercase. that's it.

i hope it will be helpful for you.
samiam1000 likes this.
Ahmed Khattab is offline   Reply With Quote

Old   October 23, 2013, 12:24
Default
  #19
Senior Member
 
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 455
Rep Power: 9
samiam1000 is on a distinguished road
I'm pretty sure about the patch names, but I'll check them again!

Thanks!
samiam1000 is offline   Reply With Quote

Old   October 23, 2013, 14:09
Default
  #20
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 988
Blog Entries: 4
Rep Power: 18
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi,


1. your changeDict has a wrong entry like ahmed mentioned in your domain2
Code:
            domain2_to_fluid
            {
                type            mappedWall;
                nFaces          3997;
                startFace       49350;
                sampleMode      nearestPatchFace;
                sampleRegion    fluid;
                samplePatch     fluid_to_domain1;  //domain2
                offsetMode      uniform;
                offset          (0 0 0);
            }
        }
2. wrong schemes and solution for your solids

3. wrong changeDict in domain1
Code:
    T
    {
        internalField   uniform 298;

        boundaryField
        {
                    empty_2-packs
                    {
                        type            symmetryPlane;
                    }
                    wall_packs
                    {
                        type            zeroGradient        // forget ";"
                    }
                    domain1_to_fluid
                    {
                                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                                value           uniform 298;
                                neighbourFieldName T;
                                kappa           solidThermo;
                                kappaName       none;
                    }
        }
4. after changeDict on domain2 there are still one error in your "0/domain2/T" file:
Code:
   empty_2-packs
    {
        type            symmetryPlane;
    }
    wall_packs
    {
        type            zeroGradient 
    } 

    domain1_to_fluid 
    { 
       type compressible::turbulentTemperatureCoupledBaffleMixed;
        value           uniform 298;
        neighbourFieldName T;
        kappa           solidThermo;
        kappaName       none;
    }
    domain1_to_fluid                      // wrong - not needed
    {
        type            calculated; 
        value           uniform 0;
        neighbourFieldName T;
        kappa           solidThermo;
        kappaName       none;
    }
After the changes you will get the following output:
Code:
Time = 1


Solving for fluid region fluid
DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 0.0024031, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 0.0099621, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 0.0132661, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 1, Final residual = 0.0987243, No Iterations 4
Min/max T:269.145 301.75
DICPCG:  Solving for p_rgh, Initial residual = 0.999968, Final residual = 0.0094627, No Iterations 19
time step continuity errors : sum local = 22257.7, global = -0.00312494, cumulative = -0.00312494
Min/max rho:0.001 1.29413

Solving for solid region domain1
DICPCG:  Solving for h, Initial residual = 1, Final residual = 0.0184498, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 297.999 max(T) [0 0 0 1 0 0 0] 298.001

Solving for solid region domain2
DICPCG:  Solving for h, Initial residual = 1, Final residual = 0.0187101, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 276.999 max(T) [0 0 0 1 0 0 0] 277.003

Solving for solid region domain3
DICPCG:  Solving for h, Initial residual = 1, Final residual = 0.0906404, No Iterations 1
Min/max T:min(T) [0 0 0 1 0 0 0] 297.999 max(T) [0 0 0 1 0 0 0] 298.001

Solving for solid region domain5
DICPCG:  Solving for h, Initial residual = 1, Final residual = 0.0785481, No Iterations 1
Min/max T:min(T) [0 0 0 1 0 0 0] 297.999 max(T) [0 0 0 1 0 0 0] 298.002

Solving for solid region packs
DICPCG:  Solving for h, Initial residual = 1, Final residual = 0.0262329, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 297.999 max(T) [0 0 0 1 0 0 0] 298.001
ExecutionTime = 5.9 s  ClockTime = 6 s
- the second iteration is bad but I switched off the turbulence modelling and do not check the BC.

Have fun and good luck.

Regard
Tobi
samiam1000 likes this.

Last edited by Tobi; October 23, 2013 at 14:33. Reason: added one more error
Tobi 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
Compile calcMassFlowC aurore OpenFOAM Programming & Development 12 March 18, 2014 06:22
Saving ParaFoam views and case sail OpenFOAM Paraview & paraFoam 9 November 25, 2011 16:46
Version 15 on Mac OS X gschaider OpenFOAM Installation 120 December 2, 2009 11:23
How to get the max value of the whole field waynezw0618 OpenFOAM Running, Solving & CFD 4 June 17, 2008 06:07
user defined function cfduser CFX 0 April 29, 2006 11:58


All times are GMT -4. The time now is 08:04.