CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

GammaContactAngle not implemented

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By isabel

Reply
 
LinkBack Thread Tools Display Modes
Old   May 5, 2008, 12:28
Default hi all, i am trying to impl
  #1
Member
 
Anthony Costa
Join Date: Mar 2009
Posts: 40
Rep Power: 8
coastal593 is on a distinguished road
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
coastal593 is offline   Reply With Quote

Old   May 5, 2008, 12:46
Default Hi Anthony try this type
  #2
Senior Member
 
Join Date: Mar 2009
Posts: 248
Rep Power: 9
jaswi is on a distinguished road
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
jaswi is offline   Reply With Quote

Old   March 3, 2010, 10:12
Default
  #3
Senior Member
 
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 8
isabel is on a distinguished road
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
isabel is offline   Reply With Quote

Old   March 4, 2010, 04:21
Default
  #4
New Member
 
Malte
Join Date: Mar 2009
Posts: 2
Rep Power: 0
sinusmontis is on a distinguished road
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
sinusmontis is offline   Reply With Quote

Old   March 4, 2010, 05:43
Default
  #5
Senior Member
 
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 8
isabel is on a distinguished road
Thank you very much, sinusmontis, but I didn't use "setFields" Is it neccesary?
isabel is offline   Reply With Quote

Old   November 9, 2010, 06:21
Default
  #6
Senior Member
 
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 8
isabel is on a distinguished road
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?
yeyinglcn likes this.
isabel is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
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 15:23
Where is gSum implemented cosimobianchini OpenFOAM Running, Solving & CFD 0 September 19, 2007 12:35
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 03:09


All times are GMT -4. The time now is 19:26.