|
[Sponsors] |
February 9, 2010, 09:39 |
wallHeatFlux utility in OpenFoam1.6
|
#1 |
Member
Maruthamuthu Venkatraman
Join Date: Mar 2009
Location: Norway
Posts: 80
Rep Power: 17 |
Hello Foamers,
In order to check the heat flux balance i tried to use the utility wallHeatFlux. It seems it only works for Combustion solvers, when i run this utility for all those tutorial problems in heatTransfer it says as below: ----------------------------------------------------------------------- Create time Create mesh for time = 0 Time = 0 Selecting thermodynamics package hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>> Unknown hCombustionThermo type hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>> Valid hCombustionThermo types are: 9 ( hPsiMixtureThermo<homogeneousMixture<sutherlandTra nsport<specieThermo<janafThermo<perfectGas>>>>> hPsiMixtureThermo<reactingMixture<gasThermoPhysics >> hPsiMixtureThermo<inhomogeneousMixture<constTransp ort<specieThermo<hConstThermo<perfectGas>>>>> hPsiMixtureThermo<multiComponentMixture<gasThermoP hysics>> hPsiMixtureThermo<veryInhomogeneousMixture<constTr ansport<specieThermo<hConstThermo<perfectGas>>>>> hPsiMixtureThermo<homogeneousMixture<constTranspor t<specieThermo<hConstThermo<perfectGas>>>>> hPsiMixtureThermo<inhomogeneousMixture<sutherlandT ransport<specieThermo<janafThermo<perfectGas>>>>> hPsiMixtureThermo<veryInhomogeneousMixture<sutherl andTransport<specieThermo<janafThermo<perfectGas>> >>> hPsiMixtureThermo<dieselMixture<sutherlandTranspor t<specieThermo<janafThermo<perfectGas>>>>> ) From function hCombustionThermo::New(const fvMesh&) in file combustionThermo/hCombustionThermo/newhCombustionThermo.C at line 66. FOAM exiting ----------------------------------------------------------------------- Then i tried to look at the wallHeatFlux utility and found "#include basicRhoThermo.H " is missing. I added to it and compiled the same. Again this doesnt solve the problem. Any hints are welcome. Thanks |
|
February 10, 2010, 09:17 |
|
#2 |
Member
Ulrich Heck
Join Date: Mar 2009
Location: Krefeld, Germany
Posts: 41
Rep Power: 17 |
Hello Maruthamuthu,
I did this like this 1. I copied the wallHeatFlux-dir into a new dir e.g. wallHeatFluxRho 2. I renamed the *c-File in dir wallHeatFluxRho to wallHeatFluxRho.c 3. I modified the name in "files" (Make –dir) 4. I replaced (with an editor) hCombustionThermo by basicPsiThermo (which is the base class, see Doxygen) in createFields.h and wallHeatFluxRho.c. I think this class has be renamed in 1.6 5. Than I complied with wclean/wmake This should work. Hope it helps Ulrich |
|
February 16, 2010, 13:11 |
|
#3 |
Member
Maruthamuthu Venkatraman
Join Date: Mar 2009
Location: Norway
Posts: 80
Rep Power: 17 |
Thanks for your explanations.
Yes, it worked. I can able to run this utility for simpleRadiationFoam. I compiled BuoyantPisoRadiationFoam and tried to use wallHeatFluxRho utility. It doesnt work for that case. I will check it out in detail later. |
|
February 20, 2010, 14:16 |
Problem with incompressible wall heat flux calculation
|
#4 |
New Member
Join Date: Feb 2010
Posts: 28
Rep Power: 16 |
Hello Sir/Madam
I carried out benchmark calculations by using OF 1.6.x for cylinder on the cross flow and one interesting point is on the wall heat convection. Based on previous tips I do “wallHeatFluxRho” function so that I change “hCombustionThermo” to “basicRhoThermo” on wallHeatFluxRho.C and createFields.H files and complied with wclean/wmake. WallHeatFluxRho works on compressible e.g. BuoyantPisoFoam many different RASmodels but it works only realizableKE and LaunderSharmaKE models on the incompressible flow simulation (buoyantBoussinesqPisoFoam) . I use on the thermo physical models “thermoType hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>;”. How can I calculate wall heat flux on the incompressible case? WallHeatFluxRho function does not work with for example kOmegaSST model. Thanks in advance |
|
February 23, 2010, 05:33 |
|
#5 |
Member
Maruthamuthu Venkatraman
Join Date: Mar 2009
Location: Norway
Posts: 80
Rep Power: 17 |
Hi Pekka,
I couldn't able to run thios utility wallHeatFluxRho for buoyantPisoFoam. The following error is showing up. Since you run this utility for buoyantPisoFoam , could you upload the sources. I will recompile and see my mistake. Thanks. -------------------------------Error Message--------------------------- Create time Create mesh for time = 0 Time = 0 Selecting thermodynamics package hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>> Unknown basicPsiThermo type hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>> Valid basicPsiThermo types are: 25 ( ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>> hhuMixtureThermo<veryInhomogeneousMixture<sutherla ndTransport<specieThermo<janafThermo<perfectGas>>> >> hhuMixtureThermo<egrMixture<sutherlandTransport<sp ecieThermo<janafThermo<perfectGas>>>>> hhuMixtureThermo<homogeneousMixture<constTransport <specieThermo<hConstThermo<perfectGas>>>>> hPsiMixtureThermo<homogeneousMixture<sutherlandTra nsport<specieThermo<janafThermo<perfectGas>>>>> ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<eConstThermo<perfectGas>>>>> hhuMixtureThermo<veryInhomogeneousMixture<constTra nsport<specieThermo<hConstThermo<perfectGas>>>>> hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>> hPsiMixtureThermo<reactingMixture<gasThermoPhysics >> hhuMixtureThermo<inhomogeneousMixture<sutherlandTr ansport<specieThermo<janafThermo<perfectGas>>>>> hPsiMixtureThermo<inhomogeneousMixture<constTransp ort<specieThermo<hConstThermo<perfectGas>>>>> hPsiMixtureThermo<multiComponentMixture<gasThermoP hysics>> hPsiMixtureThermo<veryInhomogeneousMixture<constTr ansport<specieThermo<hConstThermo<perfectGas>>>>> hhuMixtureThermo<egrMixture<constTransport<specieT hermo<hConstThermo<perfectGas>>>>> hPsiMixtureThermo<homogeneousMixture<constTranspor t<specieThermo<hConstThermo<perfectGas>>>>> hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>> hPsiMixtureThermo<inhomogeneousMixture<sutherlandT ransport<specieThermo<janafThermo<perfectGas>>>>> hPsiMixtureThermo<veryInhomogeneousMixture<sutherl andTransport<specieThermo<janafThermo<perfectGas>> >>> hPsiMixtureThermo<dieselMixture<sutherlandTranspor t<specieThermo<janafThermo<perfectGas>>>>> ePsiThermo<pureMixture<constTransport<specieThermo <eConstThermo<perfectGas>>>>> hhuMixtureThermo<homogeneousMixture<sutherlandTran sport<specieThermo<janafThermo<perfectGas>>>>> ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>> ePsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>> hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>> hhuMixtureThermo<inhomogeneousMixture<constTranspo rt<specieThermo<hConstThermo<perfectGas>>>>> ) From function basicPsiThermo::New(const fvMesh&) in file psiThermo/basicPsiThermo/newBasicPsiThermo.C at line 64. FOAM exiting ----------------------------------------------------------------------- |
|
February 23, 2010, 11:53 |
|
#6 |
New Member
Join Date: Feb 2010
Posts: 28
Rep Power: 16 |
Hi Maruthamuthu,
take a copy of wallHeatFlux folder and rename it, replace wallHeatFlux.C, createFiles.H and files to the new one and then compile. It should work with the BuoyantPisoFoam solver. Has anybody any ideas how wall heat flux calculations are done for incompressible flow? |
|
February 25, 2010, 03:45 |
|
#7 |
Senior Member
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 103
Rep Power: 17 |
Hi,
have a look at the discussion at http://www.cfd-online.com/Forums/ope...oussinesq.html Regards Thomas |
|
February 27, 2010, 14:48 |
|
#8 |
New Member
Join Date: Feb 2010
Posts: 28
Rep Power: 16 |
Hi,
thanks for the link and it clarified the problematics, but I have still the same problem with incompressible flow calculation. I change all kappaEff to alphaEff in the Tegn.H and recompiled it, but without success. When I try post processing heat flux on the walls with wallHeatFluxRho function I get the following error: ----------Error message------- Time = 0 Selecting thermodynamics package hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>> Reading/calculating face flux field phi Selecting RAS turbulence model kOmegaSST --> Upgrading k to employ run-time selectable wall functions Backup original k to k.old Writing updated k --> Upgrading omega to employ run-time selectable wall functions Backup original omega to omega.old Writing updated omega --> Creating mut to employ run-time selectable wall functions Writing new mut --> Creating alphat to employ run-time selectable wall functions Writing new alphat #0 Foam::error::rintStack(Foam::Ostream&) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so" #2 __restore_rt at sigaction.c:0 #3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so" #4 void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so" #5 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:erator/<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so" #6 Foam::compressible::RASModels::kOmegaSST::F2() const in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so" #7 Foam::compressible::RASModels::kOmegaSST::kOmegaSS T(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so" #8 Foam::compressible::RASModel::adddictionaryConstru ctorToTable<Foam::compressible::RASModels::kOmegaS ST>::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so" #9 Foam::compressible::RASModel::New(Foam::GeometricF ield<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so" #10 main in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/wallHeatFluxRho" #11 __libc_start_main in "/lib64/libc.so.6" #12 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/home/Pekka/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/wallHeatFluxRho" Floating point exception Any ideas? BR Pekka |
|
May 28, 2010, 14:28 |
|
#9 |
New Member
Join Date: Feb 2010
Posts: 28
Rep Power: 16 |
Hello Foamers,
The problem with wall flux calculation seems to be solved. On incompressible simulation modified wallHeatFlux utility gives “floating point exception” error when kOmegaSST model is used. I change pressure values from zero to 1e-12 on whole calculation field on first time step and then the wallHeatFluxRho utility works. Can any OF guru tell me, is it possible to solve wall heat flux without any wall functions? What is the reason for changing the wall function to compressible wall function during run the wallHeatFlux utility? Have I understood correctly that the RAS-model sets the wall functions on the wallHeatFlux utility? For example, if I use the kOmegaSST model the wallHeatFlux utility changes the wall functions to compressible:: omegaWallFunction; and low-Re models zeroGradient; boundary conditions be kept up, is it OK? Thanks in advance |
|
June 23, 2010, 09:43 |
|
#10 |
New Member
M.H.Sedaghat
Join Date: Jun 2010
Posts: 1
Rep Power: 0 |
hello
my new username is the next one Last edited by mh.sedagaht@gmail.com; June 23, 2010 at 16:45. |
|
June 23, 2010, 10:37 |
|
#11 |
New Member
Mohammad Hadi Sedaghat
Join Date: Jun 2010
Location: Iran
Posts: 1
Rep Power: 0 |
hello
I change the wallHeatFlux files for laminar force and free convection heat transfer solvers(e.g. icoFoam with temperature for laminar force convection and boussinesqBuoyantFoam for laminar natural convection). It works properly. I rename it wallHeatFluxLaminar. you can download it . please visit our website: http://sarreshtehdari.net/ |
|
August 12, 2010, 08:55 |
heat flux on multiRegion cases?
|
#12 |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
... and what about solvers that require multiple regions, as for example chtMultiRegionFoam? It can be interesting to evaluate the convective heat transfer at the interfaces...
Does someone has an application for this kind of problem as well? regards, mad |
|
September 17, 2010, 18:23 |
Any pointers on getting started for CHT?
|
#13 |
New Member
Charles McCreary
Join Date: Jun 2010
Posts: 12
Rep Power: 16 |
I've been mucking around trying to get a version of wallHeatFlux to work for CHT to no avail. If someone has a suggested roadmap or maybe some pointers, I'd be glad to do the coding.
|
|
October 7, 2010, 23:12 |
|
#14 |
Member
Stefano Wahono
Join Date: Aug 2010
Location: Melbourne, Australia
Posts: 42
Rep Power: 16 |
Hello wallHeatFlux enthusiasts!
I have been also trying to modify the wallHeatFlux utility to work with chtMultiRegionSimpleFoam - however not successful yet. The modified code compiled ok, but (i think) give wrong result. Can anyone help us please.... Uncle Hrv? This is my modified chtWallHeatFluxRho.C: Code:
#include "fvCFD.H" #include "basicPsiThermo.H" #include "RASModel.H" #include "fixedGradientFvPatchFields.H" #include "wallFvPatch.H" #include "regionProperties.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // int main(int argc, char *argv[]) { timeSelector::addOptions(); #include "setRootCase.H" #include "createTime.H" regionProperties rp(runTime); #include "createFluidMeshes.H" // #include "createSolidMeshes.H" #include "createFluidFields.H" // #include "createSolidFields.H" forAll(fluidRegions, i) { instantList timeDirs = timeSelector::select0(runTime, args); Info<< "\nSolving for fluid region " << fluidRegions[i].name() << endl; forAll(timeDirs, timeI) { runTime.setTime(timeDirs[timeI], timeI); Info<< "Time = " << runTime.timeName() << endl; fluidRegions[i].readUpdate(); surfaceScalarField heatFlux = fvc::interpolate(KFluid[i])*fvc::snGrad(thermoFluid[i].h()); const surfaceScalarField::GeometricBoundaryField& patchHeatFlux = heatFlux.boundaryField(); Info<< "\nWall heat fluxes [W]" << endl; forAll(patchHeatFlux, patchi) { if (isA<wallFvPatch>(fluidRegions[i].boundary()[patchi])) { Info<< fluidRegions[i].boundary()[patchi].name() << " " << sum ( fluidRegions[i].magSf().boundaryField()[patchi] *patchHeatFlux[patchi] ) << endl; } } Info<< endl; forAll(wallHeatFluxFluid[i].boundaryField(), patchi) { wallHeatFluxFluid[i].boundaryField()[patchi] = patchHeatFlux[patchi]; } wallHeatFluxFluid[i].write(); } } Info<< "End" << endl; return 0; } I also changed the 'mesh' to fluidRegions[i], by including the createFluidMeshes.H taken from the same directory above. Oh, I also added declaration for the new variable 'wallHeatFluxFluid' in the copied createFluidFields.H file. Code:
... PtrList<volScalarField> wallHeatFluxFluid(fluidRegions.size()); // Populate fluid field pointer lists forAll(fluidRegions, i) { ... Thank you very much. Hopefully we can develop this marvelous utility to work with every solvers in OF 1.7.0. Best regards, Stefano |
|
October 7, 2010, 23:17 |
|
#15 |
Member
Stefano Wahono
Join Date: Aug 2010
Location: Melbourne, Australia
Posts: 42
Rep Power: 16 |
Hi Again,
Another thing with the chtWallHeatFluxRho above, During runtime, it returns the following error: Code:
Solving for fluid region bottomAir Time = 0 Wall heat fluxes [W] minY 0 minZ 0 maxZ 0 bottomAir_to_solidWall 345600 --> FOAM FATAL ERROR: hanging pointer, cannot dereference From function PtrList::operator[] in file /home/stefano/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/PtrListI.H at line 122. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) in "/home/stefano/OpenFOAM/OpenFOAM-1.7.0/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::error::abort() in "/home/stefano/OpenFOAM/OpenFOAM-1.7.0/lib/linuxGccDPOpt/libOpenFOAM.so" #2 in "/home/stefano/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linuxGccDPOpt/chtWallHeatFluxRho" #3 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6" #4 in "/home/stefano/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linuxGccDPOpt/chtWallHeatFluxRho" Aborted Cheers, Stefano |
|
November 14, 2010, 00:36 |
wallHeatFlux for rhoSimpleFoam
|
#16 |
Senior Member
|
Dear All,
I am running some flow cases around a circular cylinder with isothermal and rough surface and heat transfer. So I picked your suggestions and put together an utility that worked with rhoSimpleFoam, RAS compreesible, kOmegaSST model and rough wall function. See attached but I do not know if it works in other solvers. Regards, Guilherme |
|
February 24, 2011, 09:52 |
|
#17 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 51 |
Hey aerothermal,
nice tool it 's working fine but if i got the patchtype: Code:
siliziumoxid_to_ziegelstein { type compressible::turbulentTemperatureCoupledBaffleMixed; value uniform 730; neighbourFieldName T; K K; } Any solutions ? I ve used chtMultirRegionSimpleFoam tobi |
|
April 20, 2011, 05:41 |
|
#18 |
Member
Nicolas
Join Date: Apr 2011
Location: Biarritz / France
Posts: 33
Rep Power: 15 |
Hi!
Since I've got some problems using chtMultiRegionSimpleFoam, I'd like to check the heat fluxes. Obviously wallHeatFlux doesn't work in my case, therefore I've tried the wallHeatFluxRho utility. Here is what I get : Code:
$ wallHeatFluxRho /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 1.7.0-113391ee57bd Exec : wallHeatFluxRho Date : Apr 20 2011 Time : 11:08:16 Host : caelinux-desktop PID : 4575 Case : /home/caelinux/OpenFOAM/caelinux-1.7.0/Freyssinet3 nProcs : 1 SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Time = 0 Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>> #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam170/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam170/lib/linux64GccDPOpt/libOpenFOAM.so" #2 in "/lib/libc.so.6" #3 Foam::hPsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::calculate() in "/opt/openfoam170/lib/linux64GccDPOpt/libbasicThermophysicalModels.so" #4 Foam::hPsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::hPsiThermo(Foam::fvMesh const&) in "/opt/openfoam170/lib/linux64GccDPOpt/libbasicThermophysicalModels.so" #5 Foam::basicPsiThermo::addfvMeshConstructorToTable<Foam::hPsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > > >::New(Foam::fvMesh const&) in "/opt/openfoam170/lib/linux64GccDPOpt/libbasicThermophysicalModels.so" #6 Foam::basicPsiThermo::New(Foam::fvMesh const&) in "/opt/openfoam170/lib/linux64GccDPOpt/libbasicThermophysicalModels.so" #7 in "/home/caelinux/OpenFOAM/caelinux-1.7.0/applications/bin/linux64GccDPOpt/wallHeatFluxRho" #8 __libc_start_main in "/lib/libc.so.6" #9 in "/home/caelinux/OpenFOAM/caelinux-1.7.0/applications/bin/linux64GccDPOpt/wallHeatFluxRho" Exception en point flottant How may I fix this issue? Thank you in advance for your help. |
|
April 20, 2011, 06:54 |
|
#19 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 51 |
Hey nikolas,
i think, you can't use the wallHeatFluxRho tool with chtMulti directly. You have to change your case a little bit. Like you 've solve every region single. Never have tried to use a wallHeatFlux Tool with cht Multi - but i ll test it if i 'd time Regards Tobi |
|
April 20, 2011, 08:22 |
|
#20 |
Member
Nicolas
Join Date: Apr 2011
Location: Biarritz / France
Posts: 33
Rep Power: 15 |
Hi Tobias,
Thanks to your hint, I've succeeded in computing the heat fluxes for the fluid zone (but at the inlet and outlet which are not walls). When I prompt for the fluxes in solid region, I've got the next error: Code:
$ wallHeatFluxRho /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 1.7.0-113391ee57bd Exec : wallHeatFluxRho Date : Apr 20 2011 Time : 14:03:58 Host : caelinux-desktop PID : 6225 Case : /home/caelinux/OpenFOAM/caelinux-1.7.0/Freyssinet3/beton nProcs : 1 SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Time = 0 --> FOAM FATAL IO ERROR: cannot open file file: /home/caelinux/OpenFOAM/caelinux-1.7.0/Freyssinet3/beton/constant/thermophysicalProperties at line 0. From function regIOobject::readStream() in file db/regIOobject/regIOobjectRead.C at line 61. FOAM exiting Thanks again |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Sample Utility not working in OpenFoam 1.6 | titio | OpenFOAM Post-Processing | 6 | November 15, 2014 18:04 |
problem with sampling Utility in openFOAM 1.6 | carmir | OpenFOAM Post-Processing | 10 | February 26, 2014 02:00 |
How to compile a new utility | rudy | OpenFOAM | 4 | October 1, 2011 22:48 |
wallHeatFlux BC not constant after restart | eelcovv | OpenFOAM Running, Solving & CFD | 26 | May 24, 2011 23:11 |
Sample Utility not working in OpenFoam 1.6 | titio | OpenFOAM Post-Processing | 0 | February 5, 2010 12:12 |