|
[Sponsors] |
October 9, 2013, 11:22 |
chtMultiRegionSimpleFoam: strange error
|
#1 |
Senior Member
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 520
Rep Power: 19 |
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$ Thanks a lot, Samuele |
|
October 12, 2013, 16:16 |
|
#2 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Hi Samuele,
Try this: Code:
find . -name ".T" 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 Code:
alias ll Bruno
__________________
|
|
October 14, 2013, 05:04 |
|
#3 |
Senior Member
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 520
Rep Power: 19 |
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$ Thanks a lot, Samuele |
|
October 14, 2013, 07:38 |
|
#4 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 52 |
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 |
|
October 14, 2013, 08:49 |
|
#5 |
Senior Member
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 520
Rep Power: 19 |
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 |
|
October 21, 2013, 06:39 |
|
#6 |
Senior Member
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 520
Rep Power: 19 |
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) |
|
October 21, 2013, 07:47 |
|
#8 |
Senior Member
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 520
Rep Power: 19 |
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; } } // ************************************************************************* // 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; } } } } Samuele |
|
October 21, 2013, 10:26 |
|
#9 |
Senior Member
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 520
Rep Power: 19 |
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 Thanks a lot, Samuele |
|
October 21, 2013, 12:02 |
|
#10 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 52 |
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); } |
|
October 21, 2013, 12:12 |
|
#11 |
Senior Member
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 520
Rep Power: 19 |
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) |
|
October 23, 2013, 03:56 |
|
#13 |
Senior Member
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 520
Rep Power: 19 |
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; } } } |
|
October 23, 2013, 05:37 |
|
#14 |
Senior Member
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 520
Rep Power: 19 |
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 Any idea about this? |
|
October 23, 2013, 08:03 |
|
#15 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 52 |
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 |
|
October 23, 2013, 09:20 |
|
#16 |
Senior Member
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 520
Rep Power: 19 |
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 |
|
October 23, 2013, 09:39 |
|
#17 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 52 |
Hi Samuel,
i am online today evening (in 2 hours). Otherwise you can send me the case Tobias.Holzmann@Holzmann-cfd.de Regards Tobi |
|
October 23, 2013, 12:10 |
|
#18 | |
Senior Member
|
Quote:
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. |
||
October 23, 2013, 12:24 |
|
#19 |
Senior Member
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 520
Rep Power: 19 |
I'm pretty sure about the patch names, but I'll check them again!
Thanks! |
|
October 23, 2013, 14:09 |
|
#20 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 52 |
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); } } 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; } } 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; } 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 Have fun and good luck. Regard Tobi Last edited by Tobi; October 23, 2013 at 14:33. Reason: added one more error |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Compile calcMassFlowC | aurore | OpenFOAM Programming & Development | 13 | March 23, 2018 08:43 |
[OpenFOAM] Saving ParaFoam views and case | sail | ParaView | 9 | November 25, 2011 16:46 |
Version 15 on Mac OS X | gschaider | OpenFOAM Installation | 113 | 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 |