|
[Sponsors] |
May 5, 2008, 13:28 |
hi all,
i am trying to impl
|
#1 |
Member
Anthony Costa
Join Date: Mar 2009
Posts: 40
Rep Power: 17 |
hi all,
i am trying to implement the gammaContactAngle model for my problem, and i see the same error consistently. simple setup :: 0/gamma lowerWall { type gammaContactAngle; theta0 10; uTheta 0; thetaA 10; thetaR 10; value uniform 1; } :: constant/polyMesh/boundary type wall; physicalType wallContactAngle; i've tried other gammaContactAngle models (constant and dynamic) all to the same effect. any advice would be appreciated. thanks. error attached below. --> FOAM FATAL ERROR : Not implemented#0 Foam::error::printStack(Foam:stream&) in "/home/acosta/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::error::abort() in "/home/acosta/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #2 Foam::defaultFvPatchField<double>::defaultFvPatchF ield(Foam::fvPatch const&, Foam::DimensionedField<double,> const&) in "/home/acosta/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libfiniteVolume.so" #3 Foam::fvPatchField<double>::addpatchConstructorToT able<foam::defaultfvpatchfield <double> >::New(Foam::fvPatch const&, Foam::DimensionedField<double,> const&) in "/home/acosta/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libfiniteVolume.so" #4 Foam::fvPatchField<double>::New(Foam::word const&, Foam::fvPatch const&, Foam::DimensionedField<double,> const&) in "/home/acosta/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/interFoam " #5 Foam::GeometricField<double,>::GeometricBoundaryFi eld::GeometricBoundaryField(Fo am::fvBoundaryMesh const&, Foam::DimensionedField<double,> const&, Foam::List<foam::word> const&) in "/home/acosta/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/interFoam " #6 Foam::GeometricField<double,>::GeometricField(Foam ::IOobject const&, Foam::GeometricField<double,> const&, Foam::List<foam::word> const&) in "/home/acosta/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/interFoam " #7 main in "/home/acosta/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/interFoam " #8 __libc_start_main in "/lib/libc.so.6" #9 Foam::regIOobject::readIfModified() in "/home/acosta/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/interFoam " From function defaultFvPatchField<type>::defaultFvPatchField(con st fvPatch& p, const DimensionedField<type,>& iF) in file fields/fvPatchFields/basic/default/defaultFvPatchField.C at line 50. FOAM aborting Aborted |
|
May 5, 2008, 13:46 |
Hi Anthony
try this
type
|
#2 |
Senior Member
Join Date: Mar 2009
Posts: 248
Rep Power: 18 |
Hi Anthony
try this type constantGammaContactAngle; theta0 20; value uniform 0; similarly for your config above you need to write lowerWall { type dynamicGammaContactAngle; theta0 10; uTheta 0; thetaA 10; thetaR 10; value uniform 1; } and it shall work. Let me know if it didn't Hope that helps Jaswi |
|
March 3, 2010, 10:12 |
|
#3 |
Senior Member
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 17 |
Hi jaswi,
I have succesfully applied the condition: type constantGammaContactAngle; theta0 20; value uniform 0; I saw that theta0 is the contact angle in degrees, but I don't know what "uniform 0" means. I've worked with uniform 0 and uniform 1 and the results I've obtained are similar |
|
March 4, 2010, 04:21 |
|
#4 |
New Member
Malte
Join Date: Mar 2009
Posts: 2
Rep Power: 0 |
Hello Isabel,
with this parameter you are setting the value for gamma (or alpha1 if you are working with OF1.6) at your boundary. It probably didn't make a difference since you changed that value with "setFields" afterwards anyway. Malte |
|
March 4, 2010, 05:43 |
|
#5 |
Senior Member
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 17 |
Thank you very much, sinusmontis, but I didn't use "setFields" Is it neccesary?
|
|
November 9, 2010, 06:21 |
|
#6 |
Senior Member
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 17 |
Hello everybody,
In OpenFOAM 1.5, the boundary condition dynamic and constant gamma contact angle works Ok: lowerWall { type dynamicGammaContactAngle; theta0 10; uTheta 0; thetaA 10; thetaR 10; value uniform 1; } In OpenFOAM 1.7.1, I tried the same boundary condition as follows: lowerWall { type dynamicAlphaContactAngle; theta0 10; uTheta 0; thetaA 10; thetaR 10; value uniform 1; } But this time I have the following error: --> FOAM FATAL IO ERROR: keyword limit is undefined in dictionary "/home/isabel/OpenFOAM/OpenFOAM-1.7.1/tutorials/multiphase/interFoam/laminar/damBreak/0/alpha1::boundaryField::lowerWall" file: /home/isabel/OpenFOAM/OpenFOAM-1.7.1/tutorials/multiphase/interFoam/laminar/damBreak/0/alpha1::boundaryField::lowerWall from line 41 to line 46. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 395. FOAM exiting So I added the line I tipped in red, and the solver runs Ok: lowerWall { type dynamicAlphaContactAngle; theta0 10; uTheta 0; thetaA 10; thetaR 10; value uniform 1; limit alpha 1; } Does anybody knows what the line I added “limit alpha 1” means in OpenFOAM 1.7.1? |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Where is gSum implemented | cosimobianchini | OpenFOAM Running, Solving & CFD | 2 | June 7, 2022 15:27 |
Convective Schemes how are they implemented | nicasch | OpenFOAM Running, Solving & CFD | 1 | November 4, 2010 09:47 |
Calculated gradient boundary condition similar to gammaContactAngle | adona058 | OpenFOAM Running, Solving & CFD | 0 | September 26, 2007 16:23 |
Is it implemented the QUICK scheme in the CFX? | Viana | CFX | 2 | January 23, 2006 06:08 |
Format to specify gammaContactAngle | gopala | OpenFOAM Running, Solving & CFD | 1 | April 26, 2005 04:09 |