|
[Sponsors] |
February 14, 2014, 22:11 |
Error adding the temperature icoFoam
|
#1 |
Member
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 44
Rep Power: 12 |
Dear, good night.
I used the openfoamwiki's tutorial to edit the solve icoFoam and add the energy equation, however when trying to visualize the temperature field, it simply disappears. Below is example solver and edited example cavity. I appreciate everyone's attention. createFields.H Code:
Info<< "Reading transportProperties\n" << endl; IOdictionary transportProperties ( IOobject ( "transportProperties", runTime.constant(), mesh, IOobject::MUST_READ, IOobject::NO_WRITE ) ); dimensionedScalar nu ( transportProperties.lookup("nu") ); dimensionedScalar DT ( transportProperties.lookup("DT") ); Info<< "Reading field p\n" << endl; volScalarField p ( IOobject ( "p", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::AUTO_WRITE ), mesh ); Info<< "Reading field U\n" << endl; volVectorField U ( IOobject ( "U", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::AUTO_WRITE ), mesh ); Info<< "Reading field T\n" <<endl; volScalarField T ( IOobject ( "T", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::AUTO_WRITE ), mesh ); # include "createPhi.H" label pRefCell = 0; scalar pRefValue = 0.0; setRefCell(p, mesh.solutionDict().subDict("PISO"), pRefCell, pRefValue); Code:
/*---------------------------------------------------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | \\ / A nd | Copyright (C) 2011-2012 OpenFOAM Foundation \\/ M anipulation | ------------------------------------------------------------------------------- License This file is part of OpenFOAM. OpenFOAM is free software: you can redistribute it and/or modify it under the terms of the GNU General Public License as published by the Free Software Foundation, either version 3 of the License, or (at your option) any later version. OpenFOAM is distributed in the hope that it will be useful, but WITHOUT ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License for more details. You should have received a copy of the GNU General Public License along with OpenFOAM. If not, see <http://www.gnu.org/licenses/>. Application icoFoamTemp Description Transient solver for incompressible, laminar flow of Newtonian fluids. \*---------------------------------------------------------------------------*/ #include "fvCFD.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // int main(int argc, char *argv[]) { #include "setRootCase.H" #include "createTime.H" #include "createMesh.H" #include "createFields.H" #include "initContinuityErrs.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Info<< "\nStarting time loop\n" << endl; while (runTime.loop()) { Info<< "Time = " << runTime.timeName() << nl << endl; #include "readPISOControls.H" #include "CourantNo.H" fvVectorMatrix UEqn ( fvm::ddt(U) + fvm::div(phi, U) - fvm::laplacian(nu, U) ); solve(UEqn == -fvc::grad(p)); // --- PISO loop for (int corr=0; corr<nCorr; corr++) { volScalarField rAU(1.0/UEqn.A()); volVectorField HbyA("HbyA", U); HbyA = rAU*UEqn.H(); surfaceScalarField phiHbyA ( "phiHbyA", (fvc::interpolate(HbyA) & mesh.Sf()) + fvc::ddtPhiCorr(rAU, U, phi) ); adjustPhi(phiHbyA, U, p); for (int nonOrth=0; nonOrth<=nNonOrthCorr; nonOrth++) { fvScalarMatrix pEqn ( fvm::laplacian(rAU, p) == fvc::div(phiHbyA) ); pEqn.setReference(pRefCell, pRefValue); pEqn.solve(); if (nonOrth == nNonOrthCorr) { phi = phiHbyA - pEqn.flux(); } } #include "continuityErrs.H" U -= rUA*fvc::grad(p); U.correctBoundaryConditions(); } fvScalarMatrix TEqn ( fvm::ddt(T) + fvm::div(phi, T) - fvm::laplacian(DT, T) ); TEqn.solve(); runTime.write(); Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s" << " ClockTime = " << runTime.elapsedClockTime() << " s" << nl << endl; } Info<< "End\n" << endl; return 0; } Code:
Making dependency list for source file icoFoamTemp.C SOURCE=icoFoamTemp.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam222/src/finiteVolume/lnInclude -I/opt/openfoam222/src/sampling/lnInclude -IlnInclude -I. -I/opt/openfoam222/src/OpenFOAM/lnInclude -I/opt/openfoam222/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/icoFoamTemp.o icoFoamTemp.C: Na função ‘int main(int, char**)’: icoFoamTemp.C:100:19: erro: ‘rUA’ was not declared in this scope /opt/openfoam222/src/finiteVolume/lnInclude/readPISOControls.H:3:15: aviso: unused variable ‘nOuterCorr’ [-Wunused-variable] /opt/openfoam222/src/finiteVolume/lnInclude/readPISOControls.H:12:16: aviso: unused variable ‘momentumPredictor’ [-Wunused-variable] /opt/openfoam222/src/finiteVolume/lnInclude/readPISOControls.H:15:16: aviso: unused variable ‘transonic’ [-Wunused-variable] make: ** [Make/linux64GccDPOpt/icoFoamTemp.o] Erro 1 Last edited by wyldckat; February 16, 2014 at 09:49. Reason: Added [CODE][/CODE] |
|
February 14, 2014, 22:18 |
|
#2 |
Member
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 44
Rep Power: 12 |
fvSchemes
Code:
FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default Euler; } gradSchemes { default Gauss linear; grad(p) Gauss linear; } divSchemes { default none; div(phi,U) Gauss linear; //NOTICE: there is no space between the comma and the variables div(phi,T) Gauss upwind; } laplacianSchemes { default none; laplacian(nu,U) Gauss linear corrected; laplacian((1|A(U)),p) Gauss linear corrected; laplacian(DT,T) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(HbyA) linear; } snGradSchemes { default orthogonal; } fluxRequired { default no; p ; } Code:
FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { p { solver PCG; preconditioner DIC; tolerance 1e-06; relTol 0; } // GW Add a solver for T T { solver BICCG; preconditioner DILU; //GW or: none, GAMG, diagonal tolerance 1e-7; relTol 0; } U { solver PBiCG; preconditioner DILU; tolerance 1e-06; relTol 0; } } PISO { nCorrectors 2; nNonOrthogonalCorrectors 0; pRefCell 0; pRefValue 0; } Code:
FoamFile { version 2.0; format ascii; class volScalarField; object T; } //**********************************// dimensions [0 0 0 1 0 0 0]; internalField uniform 300; boundaryField { movingWall { type fixedValue; value uniform 350; } fixedWalls { type fixedValue; value uniform 300; } frontAndBack { type empty; } } Last edited by wyldckat; February 16, 2014 at 09:50. Reason: Added [CODE][/CODE] |
|
February 15, 2014, 11:45 |
|
#3 |
Member
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 44
Rep Power: 12 |
Can anyone help me identify the problem?
|
|
February 16, 2014, 02:58 |
|
#4 | |
Senior Member
|
Hi,
You got an error in compilation. How did you execute new solver? Error message says unknown word ‘rUA’ exists in line 100 of icoFoamTemp.C. Yes, its true. What is rUA? It will be rAU, isn't it? Quote:
|
||
February 16, 2014, 16:47 |
|
#5 |
Member
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 44
Rep Power: 12 |
Mr. Nakagawa,
Firstly thank you very much for your help. I modified the solver icoFOAM as the tutorial link: http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam Really, it was the correct rAU. But when running the modified ICOFOAM, the temperature field is still not appearing in the solution presented by PARAFOAM. Temperatures simply disappear. Wmake command again, we have: silvio@ubuntu:~/OpenFOAM/silvio-2.2.2/applications/solvers/icoFoamTemp$ wmake Making dependency list for source file icoFoamTemp.C SOURCE=icoFoamTemp.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam222/src/finiteVolume/lnInclude -I/opt/openfoam222/src/sampling/lnInclude -IlnInclude -I. -I/opt/openfoam222/src/OpenFOAM/lnInclude -I/opt/openfoam222/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/icoFoamTemp.o /opt/openfoam222/src/finiteVolume/lnInclude/readPISOControls.H: Na função ‘int main(int, char**)’: /opt/openfoam222/src/finiteVolume/lnInclude/readPISOControls.H:3:15: aviso: unused variable ‘nOuterCorr’ [-Wunused-variable] /opt/openfoam222/src/finiteVolume/lnInclude/readPISOControls.H:12:16: aviso: unused variable ‘momentumPredictor’ [-Wunused-variable] /opt/openfoam222/src/finiteVolume/lnInclude/readPISOControls.H:15:16: aviso: unused variable ‘transonic’ [-Wunused-variable] g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam222/src/finiteVolume/lnInclude -I/opt/openfoam222/src/sampling/lnInclude -IlnInclude -I. -I/opt/openfoam222/src/OpenFOAM/lnInclude -I/opt/openfoam222/src/OSspecific/POSIX/lnInclude -fPIC -Xlinker --add-needed -Xlinker --no-as-needed Make/linux64GccDPOpt/icoFoamTemp.o -L/opt/openfoam222/platforms/linux64GccDPOpt/lib \ -lfiniteVolume -lsampling -lOpenFOAM -ldl -lm -o /home/silvio/OpenFOAM/silvio-2.2.2/platforms/linux64GccDPOpt/bin/my_icoFoamTemp What can be the problem? I appreciate everyone's attention |
|
February 16, 2014, 20:48 |
|
#6 |
Member
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 44
Rep Power: 12 |
No suggestion?
|
|
February 16, 2014, 22:08 |
|
#7 |
Senior Member
|
Hi,
Questions: (1) Did you do "icoFoamTemp" instead of "icoFoam"? (2) what exactly happens? "Temperatures simply disappear. " Do you have a T file in time directories? Please provide clear, concise and complete information about what you did and what you got. |
|
February 17, 2014, 16:34 |
|
#8 |
Member
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 44
Rep Power: 12 |
(1) I used the command icoFoamTemp. I did not use command icoFoam .
(2) When displaying the simulated results by command paraFoam, check that the temperature disappears over time. That is, at time t = 0, s is the temperature field and as time goes by following the temperature disappears. What can be happening? Below, we have the result of ControlDict and icoFoamTemp command. I appreciate everyone's attention. ----------------------------------------------------------------------------------------------------------------------------------- Time = 0.495 Courant Number mean: 0.222159 max: 0.852134 DILUPBiCG: Solving for Ux, Initial residual = 3.77171e-08, Final residual = 3.77171e-08, No Iterations 0 DILUPBiCG: Solving for Uy, Initial residual = 8.93865e-08, Final residual = 8.93865e-08, No Iterations 0 DICPCG: Solving for p, Initial residual = 7.67456e-07, Final residual = 7.67456e-07, No Iterations 0 time step continuity errors : sum local = 7.3935e-09, global = -1.93974e-19, cumulative = -1.32121e-17 DICPCG: Solving for p, Initial residual = 9.33333e-07, Final residual = 9.33333e-07, No Iterations 0 time step continuity errors : sum local = 8.75324e-09, global = 8.34212e-19, cumulative = -1.23778e-17 ExecutionTime = 0.23 s ClockTime = 0 s Time = 0.5 Courant Number mean: 0.222159 max: 0.852134 DILUPBiCG: Solving for Ux, Initial residual = 3.10465e-08, Final residual = 3.10465e-08, No Iterations 0 DILUPBiCG: Solving for Uy, Initial residual = 7.20119e-08, Final residual = 7.20119e-08, No Iterations 0 DICPCG: Solving for p, Initial residual = 1.08094e-06, Final residual = 1.61882e-07, No Iterations 1 time step continuity errors : sum local = 2.42633e-09, global = 1.12397e-18, cumulative = -1.12539e-17 DICPCG: Solving for p, Initial residual = 4.79724e-07, Final residual = 4.79724e-07, No Iterations 0 time step continuity errors : sum local = 5.02954e-09, global = -1.26633e-18, cumulative = -1.25202e-17 ExecutionTime = 0.23 s ClockTime = 0 s ----------------------------------------------------------------------------------------------------------------------------------- FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ControlDict application icoFoamTemp; startFrom startTime; startTime 0; stopAt endTime; endTime 0.5; deltaT 0.005; writeControl timeStep; writeInterval 20; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression off; timeFormat general; timePrecision 6; runTimeModifiable true; |
|
February 17, 2014, 19:57 |
|
#9 |
Senior Member
|
hi,
I read your #5 post again and found the cause of the problem. http://www.cfd-online.com/Forums/ope...tml#post475242 Your new solver will be "my_icoFoamTemp" which is shown in the last line of wmake output. It is written in "files" file in Make subdirectory. Running my_icoFoamTemp will do what you want to do with your posted source code. I don't know what is icoFoamTemp in your system. Have you make a solver in that name before? It should be... This is the reason why you have been able to execute icoFoamTemp before you successfully compile the code, I think. |
|
February 17, 2014, 23:10 |
|
#10 |
Member
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 44
Rep Power: 12 |
Problem solved.
The error was in charge. Thank you for your attention. |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
whats the cause of error? | immortality | OpenFOAM Running, Solving & CFD | 13 | March 24, 2021 07:15 |
Problems adding temperature to icoFoam | sur4j | OpenFOAM Programming & Development | 8 | January 11, 2015 01:14 |
Calculation of the Governing Equations | Mihail | CFX | 7 | September 7, 2014 06:27 |
is internalField(U) equivalent to zeroGradient? | immortality | OpenFOAM Running, Solving & CFD | 7 | March 29, 2013 01:27 |
adding temperature field to icofoam | houkensjtu | OpenFOAM | 5 | September 26, 2012 22:20 |