|
[Sponsors] |
July 27, 2015, 10:06 |
wallHeatFlux utility with sonicFoam
|
#1 |
Senior Member
Huynh Phong Thanh
Join Date: Aug 2013
Location: Ho Chi Minh City
Posts: 105
Rep Power: 13 |
Hi everybody,
When I tried wallHeatFlux the buoyantSimpleFoam OF 2.1.1 in hotroom tutorial it was no problem with thermotype: Code:
thermoType hPsiThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>; pRef 100000; mixture { specie { nMoles 1; molWeight 28.9; } thermodynamics { Cp 1000; Hf 0; } transport { mu 1.8e-05; Pr 0.7; } } Code:
thermoType ePsiThermo<pureMixture<constTransport<specieThermo<eConstThermo<perfectGas>>>>>; mixture { specie { nMoles 1; molWeight 28.9; } thermodynamics { Cv 717.5; Hf 0; } transport { mu 1.8e-05; Pr 0.7; } } Code:
/*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 2.1.1-221db2718bbb Exec : wallHeatFlux -latestTime Date : Jul 25 2015 Time : 06:53:06 Host : "CompEng" PID : 2979 Case : /home/huynh/OpenFOAM/huynh-2.1.1/run/prism 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 mesh for time = 0.0003 Time = 0.0003 Selecting thermodynamics package ePsiThermo<pureMixture<constTransport<specieThermo<eConstThermo<perfectGas>>>>> --> FOAM FATAL ERROR: Not implemented From function basicThermo::h() in file basicThermo/basicThermo.C at line 260. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #1 Foam::error::abort() in "/opt/openfoam211/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #2 Foam::basicThermo::h() in "/opt/openfoam211/platforms/linuxGccDPOpt/lib/libbasicThermophysicalModels.so" #3 in "/opt/openfoam211/platforms/linuxGccDPOpt/bin/wallHeatFlux" #4 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6" #5 in "/opt/openfoam211/platforms/linuxGccDPOpt/bin/wallHeatFlux" Aborted Code:
/*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 2.1.1-221db2718bbb Exec : wallHeatFluxRho -latestTime Date : Jul 25 2015 Time : 22:05:09 Host : "CompEng" PID : 4590 Case : /home/huynh/OpenFOAM/huynh-2.1.1/run/prism 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 mesh for time = 0.0003 Time = 0.0003 Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>> Reading/calculating face flux field phi 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; } Wall heat fluxes [W] prismWall 0 End Code:
fvc::interpolate(RASModel->alphaEff())*fvc::snGrad(h) Thank you so much |
|
August 20, 2015, 00:34 |
|
#2 |
Senior Member
Huynh Phong Thanh
Join Date: Aug 2013
Location: Ho Chi Minh City
Posts: 105
Rep Power: 13 |
Hi everybody,
I modified the wallHeatFlux that can be calculated for ePsithermo. Here is the code: WallHeatFlux.C Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ License This file is part of OpenFOAM. OpenFOAM is free software: you can redistribute it and/or modify it under the terms of the GNU General Public License as published by the Free Software Foundation, either version 3 of the License, or (at your option) any later version. OpenFOAM is distributed in the hope that it will be useful, but WITHOUT ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License for more details. You should have received a copy of the GNU General Public License along with OpenFOAM. If not, see <http://www.gnu.org/licenses/>. Application wallHeatFlux Description Calculates and writes the heat flux for all patches as the boundary field of a volScalarField and also prints the integrated flux for all wall patches. \*---------------------------------------------------------------------------*/ #include "fvCFD.H" #include "hCombustionThermo.H" #include "basicPsiThermo.H" #include "RASModel.H" #include "turbulenceModel.H" #include "wallFvPatch.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // int main(int argc, char *argv[]) { timeSelector::addOptions(); # include "addRegionOption.H" #include "setRootCase.H" #include "createTime.H" instantList timeDirs = timeSelector::select0(runTime, args); #include "createNamedMesh.H" forAll(timeDirs, timeI) { runTime.setTime(timeDirs[timeI], timeI); Info<< "Time = " << runTime.timeName() << endl; mesh.readUpdate(); #include "createFields.H" surfaceScalarField heatFlux ( fvc::interpolate(turbulence->alphaEff())*fvc::snGrad(e) ); const surfaceScalarField::GeometricBoundaryField& patchHeatFlux = heatFlux.boundaryField(); Info<< "\nWall heat fluxes [W]" << endl; forAll(patchHeatFlux, patchi) { if (isA<wallFvPatch>(mesh.boundary()[patchi])) { Info<< mesh.boundary()[patchi].name() << " " << gSum ( mesh.magSf().boundaryField()[patchi] *patchHeatFlux[patchi] ) << endl; } } Info<< endl; volScalarField wallHeatFlux ( IOobject ( "wallHeatFlux", runTime.timeName(), mesh ), mesh, dimensionedScalar("wallHeatFlux", heatFlux.dimensions(), 0.0) ); forAll(wallHeatFlux.boundaryField(), patchi) { wallHeatFlux.boundaryField()[patchi] = patchHeatFlux[patchi]; } wallHeatFlux.write(); } Info<< "End" << endl; return 0; } // ************************************************************************* // Code:
Info<< "Reading thermophysical properties\n" << endl; autoPtr<basicPsiThermo> pThermo ( basicPsiThermo::New(mesh) ); basicPsiThermo& thermo = pThermo(); //volScalarField& p = thermo.p(); volScalarField& e = thermo.e(); //const volScalarField& psi = thermo.psi(); volScalarField rho ( IOobject ( "rho", runTime.timeName(), mesh ), thermo.rho() ); Info<< "Reading field U\n" << endl; volVectorField U ( IOobject ( "U", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::AUTO_WRITE ), mesh ); #include "compressibleCreatePhi.H" Info<< "Creating turbulence model\n" << endl; autoPtr<compressible::turbulenceModel> turbulence ( compressible::turbulenceModel::New ( rho, U, phi, thermo ) ); Code:
Create time Create mesh for time = 0.0090052 Time = 0.0090052 Reading thermophysical properties Selecting thermodynamics package ePsiThermo<pureMixture<constTransport<specieThermo<eConstThermo<perfectGas>>>>> Reading field U Reading/calculating face flux field phi Creating turbulence model Selecting turbulence model type RASModel Selecting RAS turbulence model kOmegaSST kOmegaSSTCoeffs { alphaK1 0.85034; alphaK2 1; alphaOmega1 0.5; alphaOmega2 0.85616; beta1 0.075; beta2 0.0828; betaStar 0.09; gamma1 0.05532; gamma2 0.4403; a1 0.31; c1 10; Prt 1; } Wall heat fluxes [W] bottom_heat -104748 Code:
Create time Create mesh for time = 0.0090052 Time = 0.0090052 Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>> Reading/calculating face flux field phi Selecting RAS turbulence model kOmegaSST kOmegaSSTCoeffs { alphaK1 0.85034; alphaK2 1; alphaOmega1 0.5; alphaOmega2 0.85616; beta1 0.075; beta2 0.0828; betaStar 0.09; gamma1 0.05532; gamma2 0.4403; a1 0.31; c1 10; Prt 1; } Wall heat fluxes [W] bottom_heat -146611 End Last edited by hiuluom; September 18, 2015 at 07:44. |
|
September 18, 2015, 00:33 |
|
#3 |
Senior Member
Huynh Phong Thanh
Join Date: Aug 2013
Location: Ho Chi Minh City
Posts: 105
Rep Power: 13 |
Dear all,
I know the difference result as I mention above. That is wrong at formula calculate heat flux in *.C. I check with paraview this formula after computing heat flux with ePsiThermo wallHeatFlux*(Cp/Cv) It will the same result when calculate heat flux with hPsiThermo. And then I modified the code wallHeatFlux.C by Code:
//molecular weight number // scalar W(thermo.lookup("molWeight")); //Heat capacity // scalar Cv(thermo.lookup("Cv")); surfaceScalarField heatFlux ( fvc::interpolate(turbulence->alphaEff())*(W + 8314/(Cv*W))*fvc::snGrad(e) ); Code:
Making dependency list for source file wallHeatFluxCompressible.C SOURCE=wallHeatFluxCompressible.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I.. -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/turbulenceModels -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/turbulenceModels/compressible/turbulenceModel -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/reactionThermo/lnInclude -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/basic/lnInclude -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/wallHeatFluxCompressible.o In file included from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/Field.H:360:0, from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/labelField.H:39, from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/primitiveFields.H:37, from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/pointField.H:36, from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/edge.H:40, from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/edgeList.H:32, from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/primitiveMesh.H:57, from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/polyMesh.H:44, from /opt/OpenFOAM/OpenFOAM-2.1.1/src/finiteVolume/lnInclude/fvMesh.H:50, from /opt/OpenFOAM/OpenFOAM-2.1.1/src/finiteVolume/lnInclude/fvCFD.H:7, from wallHeatFluxCompressible.C:34: /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/Field.C: In member function ‘void Foam::Field<Type>::operator=(const Foam::VectorSpace<Form, Cmpt, nCmpt>&)’: /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/Field.C:680:42: warning: typedef ‘VSType’ locally defined but not used [-Wunused-local-typedefs] typedef VectorSpace<Form,Cmpt,nCmpt> VSType; ^ In file included from /opt/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/eConstThermo.H:214:0, from wallHeatFluxCompressible.C:36: /opt/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/eConstThermoI.H: In member function ‘Foam::scalar Foam::eConstThermo<EquationOfState>::cp(Foam::scalar) const’: /opt/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/eConstThermoI.H:108:28: error: ‘specie’ has not been declared return Cv_*this->W() + specie::RR; ^ wallHeatFluxCompressible.C: In function ‘int main(int, char**)’: wallHeatFluxCompressible.C:61:24: error: missing template arguments before ‘.’ token scalar W(eConstThermo.lookup("molWeight")); ^ wallHeatFluxCompressible.C:64:25: error: missing template arguments before ‘.’ token scalar Cv(eConstThermo.lookup("Cv")); ^ wallHeatFluxCompressible.C:61:10: warning: unused variable ‘W’ [-Wunused-variable] scalar W(eConstThermo.lookup("molWeight")); ^ wallHeatFluxCompressible.C:64:10: warning: unused variable ‘Cv’ [-Wunused-variable] scalar Cv(eConstThermo.lookup("Cv")); ^ make: *** [Make/linux64GccDPOpt/wallHeatFluxCompressible.o] Error 1 Thank you, Thanh |
|
September 18, 2015, 07:39 |
|
#4 |
Senior Member
Huynh Phong Thanh
Join Date: Aug 2013
Location: Ho Chi Minh City
Posts: 105
Rep Power: 13 |
Finally, I compiled successfully wall heat flux for "ePsiThermo" thermal type for sonicFoam or rhoCentralFoam. Here is the code:
for "createFields.h" Code:
Info<< "Reading thermophysical properties\n" << endl; autoPtr<basicPsiThermo> pThermo ( basicPsiThermo::New(mesh) ); basicPsiThermo& thermo = pThermo(); //volScalarField& p = thermo.p(); const volScalarField& e = thermo.e(); const objectRegistry& db = mesh.thisDb(); //const IOdictionary& thermoProps = db.lookupObject<IOdictionary>("thermophysicalProperties"); const dictionary& thermoProps = db.lookupObject<IOdictionary>("thermophysicalProperties"); dictionary mixture ( thermoProps.subDict("mixture") ); dictionary specie ( mixture.subDict("specie") ); dictionary thermodynamics ( mixture.subDict("thermodynamics") ); const scalar Cv = readScalar(thermodynamics.lookup("Cv")); const scalar W = readScalar(specie.lookup("molWeight")); //double gamma = (Cv + 8314/(Cv*W)); //const volScalarField& Cv = thermo.Cv(); //const volScalarField& h = thermo.h(); //const volScalarField& psi = thermo.psi(); volScalarField rho ( IOobject ( "rho", runTime.timeName(), mesh ), thermo.rho() ); Info<< "Reading field U\n" << endl; volVectorField U ( IOobject ( "U", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::AUTO_WRITE ), mesh ); #include "compressibleCreatePhi.H" Info<< "Creating turbulence model\n" << endl; autoPtr<compressible::turbulenceModel> turbulence ( compressible::turbulenceModel::New ( rho, U, phi, thermo ) ); Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ License This file is part of OpenFOAM. OpenFOAM is free software: you can redistribute it and/or modify it under the terms of the GNU General Public License as published by the Free Software Foundation, either version 3 of the License, or (at your option) any later version. OpenFOAM is distributed in the hope that it will be useful, but WITHOUT ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License for more details. You should have received a copy of the GNU General Public License along with OpenFOAM. If not, see <http://www.gnu.org/licenses/>. Application wallHeatFlux Description Calculates and writes the heat flux for all patches as the boundary field of a volScalarField and also prints the integrated flux for all wall patches. \*---------------------------------------------------------------------------*/ #include "fvCFD.H" #include "hCombustionThermo.H" #include "basicPsiThermo.H" #include "turbulenceModel.H" #include "wallFvPatch.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // int main(int argc, char *argv[]) { timeSelector::addOptions(); # include "addRegionOption.H" #include "setRootCase.H" #include "createTime.H" instantList timeDirs = timeSelector::select0(runTime, args); #include "createNamedMesh.H" forAll(timeDirs, timeI) { runTime.setTime(timeDirs[timeI], timeI); Info<< "Time = " << runTime.timeName() << endl; mesh.readUpdate(); #include "createFields.H" surfaceScalarField heatFlux ( fvc::interpolate(turbulence->alphaEff())*(1 + 8314/(Cv*W))*fvc::snGrad(e) ); const surfaceScalarField::GeometricBoundaryField& patchHeatFlux = heatFlux.boundaryField(); Info<< "\nWall heat fluxes [W]" << endl; forAll(patchHeatFlux, patchi) { if (isA<wallFvPatch>(mesh.boundary()[patchi])) { Info<< mesh.boundary()[patchi].name() << ": Total " << sum ( mesh.magSf().boundaryField()[patchi] *patchHeatFlux[patchi] ) << " [W] over " << sum ( mesh.magSf().boundaryField()[patchi] ) << " [m2] (" << sum ( mesh.magSf().boundaryField()[patchi] *patchHeatFlux[patchi] )/ sum ( mesh.magSf().boundaryField()[patchi] ) << " [W/m2])" << endl; } } Info<< endl; volScalarField wallHeatFlux ( IOobject ( "wallHeatFlux", runTime.timeName(), mesh ), mesh, dimensionedScalar("wallHeatFlux", heatFlux.dimensions(), 0.0) ); forAll(wallHeatFlux.boundaryField(), patchi) { wallHeatFlux.boundaryField()[patchi] = patchHeatFlux[patchi]; } wallHeatFlux.write(); } Info<< "End" << endl; return 0; } // ************************************************************************* // Code:
Create time Create mesh for time = 0.0090052 Time = 0.0090052 Reading thermophysical properties Selecting thermodynamics package ePsiThermo<pureMixture<constTransport<specieThermo<eConstThermo<perfectGas>>>>> Reading field U Reading/calculating face flux field phi Creating turbulence model Selecting turbulence model type RASModel Selecting RAS turbulence model kOmegaSST kOmegaSSTCoeffs { alphaK1 0.85034; alphaK2 1; alphaOmega1 0.5; alphaOmega2 0.85616; beta1 0.075; beta2 0.0828; betaStar 0.09; gamma1 0.05532; gamma2 0.4403; a1 0.31; c1 10; Prt 1; } Wall heat fluxes [W] bottom_heat: Total -146673 [W] over 0.00909676 [m2] (-1.61237e+07 [W/m2]) End Best regards, Thanh |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
wallHeatFlux utility for an incompressible case | Mr.Jingles | OpenFOAM Post-Processing | 67 | April 6, 2023 03:25 |
wrong calculation of wallHeatFlux utility in solid patches | zfaraday | OpenFOAM Post-Processing | 6 | January 12, 2016 16:39 |
Something doens't work with wallHeatFlux utility or externalWallHeatFluxTemperat BC!! | zfaraday | OpenFOAM Post-Processing | 0 | February 5, 2015 16:47 |
wallHeatFlux utility and chtMultiRegionFoam solver | Lada | OpenFOAM Post-Processing | 4 | June 7, 2012 09:46 |
wallHeatFlux utility in OpenFoam1.6 | maruthamuthu_venkatraman | OpenFOAM | 29 | October 3, 2011 10:43 |