|
[Sponsors] |
October 6, 2008, 07:45 |
Hi all,
I want to simulate
|
#1 |
New Member
Volker Ludewig
Join Date: Mar 2009
Location: Chemnitz, saxony, germany
Posts: 12
Rep Power: 17 |
Hi all,
I want to simulate a flow through vent. The flow velocity is very small. So Reynold No. is below 2300 and I should have a laminar flow. The behavior of the fluid is similar to "Shear thinning" fluids. In the first step I simulated a Newtonian flow. I applied SimpleFoam and all was really fine. Now I am testing the CrossPower- law and at the moment at my wits' end: As soon as I set CrossPower- exponent n <> 0 then I get the following error: /*---------------------------------------------------------------------------*\ | ========= | | | \ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \ / O peration | Version: 1.4.1 | | \ / A nd | Web: http://www.openfoam.org | | \/ M anipulation | | \*---------------------------------------------------------------------------*/ Exec : simpleFoam /opt/OpenFOAM/volker-1.4.1/run Testsimplefoam2 Date : Oct 05 2008 Time : 23:53:16 Host : localhost PID : 5472 Root : /opt/OpenFOAM/volker-1.4.1/run Case : Testsimplefoam2 Nprocs : 1 Create time Create mesh for time = 0 Reading field p Reading field U Reading/calculating face flux field phi Selecting incompressible transport model CrossPowerLaw #0 Foam::error::printStack(Foam:stream&) in "/home/volker/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/home/volker/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Uninterpreted: [0xffffe420] #3 pow in "/lib/i686/libm.so.6" #4 Foam::pow(Foam::Field<double>&, Foam::UList<double> const&, double const&) in "/home/volker/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so" #5 Foam::tmp<foam::geometricfield<double,> > Foam::pow<foam::fvpatchfield,>(Foam::tmp<foam::geo metricfield<double,> > const&, Foam::dimensioned<double> const&) in "/home/volker/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libincompressibleTurbule nceModels.so" #6 Foam::viscosityModels::CrossPowerLaw::calcNu() const in "/home/volker/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libincompressibleTranspo rtModels.so" #7 Foam::viscosityModels::CrossPowerLaw::CrossPowerLa w(Foam::word const&, Foam::dictionary const&, Foam::GeometricField<foam::vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&) in "/home/volker/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libincompressibleTranspo rtModels.so" #8 Foam::viscosityModel::adddictionaryConstructorToTa ble<foam::viscositymodels::cro sspowerlaw>::New(Foam::word const&, Foam::dictionary const&, Foam::GeometricField<foam::vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&) in "/home/volker/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libincompressibleTranspo rtModels.so" #9 Foam::viscosityModel::New(Foam::word const&, Foam::dictionary const&, Foam::GeometricField<foam::vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&) in "/home/volker/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libincompressibleTranspo rtModels.so" #10 Foam::singlePhaseTransportModel::singlePhaseTransp ortModel(Foam::GeometricField< foam::vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&) in "/home/volker/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libincompressibleTranspo rtModels.so" #11 main in "/home/volker/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/simpleFoam" #12 __libc_start_main in "/lib/i686/libc.so.6" #13 Foam::regIOobject::readIfModified() in "/home/volker/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/simpleFoam" What could be wrong?? I am thankful about all suggestions. Kind regards |
|
October 7, 2008, 00:41 |
Hi,
Try to check your synt
|
#2 |
New Member
zhiwei liu
Join Date: Mar 2009
Posts: 22
Rep Power: 17 |
Hi,
Try to check your syntax in TransportModel. Maybe you have these errors: (1)lost a bracket or a semicolon; (2) m m [0 0 1 0 0 0 0] not m m [0 0 0 0 0 0 0]; |
|
October 8, 2008, 04:34 |
Yes it works.
The vector fo
|
#3 |
New Member
Volker Ludewig
Join Date: Mar 2009
Location: Chemnitz, saxony, germany
Posts: 12
Rep Power: 17 |
Yes it works.
The vector for the dimensions was wrong. Many thanks. I applied SimpleFoam in FoamX the GUI (graphic user interface) of OpenFoam. There is a programming error. The program produces script code. The dimension vectors in the script code for CrossPowerLaw and BirdCarreauLaw are without dimensions: Wrong CrossPowerLawCoeffs { nu0 nu0 [0 2 -1 0 0 0 0] ...; nuInf nuInf [0 2 -1 0 0 0 0] ...; m <> [0 0 0 0 0 0 0] ...; n <> [0 0 0 0 0 0 0] ...; } BirdCarreauCoeffs { nu0 nu0 [0 2 -1 0 0 0 0] ...; nuInf nuInf [0 2 -1 0 0 0 0] ...; k <> [0 0 0 0 0 0 0] ...; n <> [0 0 0 0 0 0 0] ...; } Works CrossPowerLawCoeffs { nu0 nu0 [0 2 -1 0 0 0 0] ...; nuInf nuInf [0 2 -1 0 0 0 0] ...; m m [0 0 1 0 0 0 0] ...; n n [0 0 0 0 0 0 0] ...; } BirdCarreauCoeffs { nu0 nu0 [0 2 -1 0 0 0 0] ...; nuInf nuInf [0 2 -1 0 0 0 0] ...; k k [0 0 1 0 0 0 0] ...; n n [0 0 0 0 0 0 0] ...; } dimension vector general: [a b c d e f g] a Mass kilogram in kg b Length metre in m c Time second in s d Temperature Kelvin in K e Quantity moles in mol f Current ampere in A g Luminous intensity candela in cd Example for nu in m^2/s: nu [0 2 -1 0 0 0 0] 0.0005 |
|
August 1, 2009, 21:17 |
|
#4 |
Senior Member
Sandy Lee
Join Date: Mar 2009
Posts: 213
Rep Power: 18 |
Hi everybody, where can I find those values nu0, nuInf, m, n, k to different phase names at different temperatures about CrossPowerLawCoeffs and BirdCarreauCoeffs??
|
|
January 14, 2010, 06:11 |
|
#5 | |
New Member
June
Join Date: Dec 2009
Posts: 18
Rep Power: 16 |
Quote:
i've also met this problem. There's so many keywords in openfoam, it's difficult to find out what do they mean. Is there guide for they too? |
||
Thread Tools | Search this Thread |
Display Modes | |
|
|