
[Sponsors] 
January 9, 2012, 13:02 
Strange boundary behaviour using interFoam

#1 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8 
Hi all,
I'm facing a strange behaviour using interFoam. I tried these set of boundary conditions: inlet p>fixedVale/totalPressure 1.1e5 u>pressureInletOutletVelocity/fluxCorrectedVelocity/zeroGradient outlet p>fixedVale/totalPressure 1e5 u>pressureInletOutletVelocity/fluxCorrectedVelocity/zeroGradient the rest of the domain are walls. The flow is driven by the pressure difference. I tried these BC in every combination but all give the same strange result. After a while the pressure at the inlet becomes not constant and the velocity does the same (see attached pictures). Has anyone else encountered the same problem? How can i solve it? thanks andrea 

January 9, 2012, 13:44 

#2 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8 
Just another information i forgot: at the inlet i'm injecting fluid one (fixedValue uniform 1 on alpha1 at the inlet)


January 10, 2012, 03:58 

#3 
Senior Member
Suresh kumar Kannan
Join Date: Mar 2009
Location: Luxembourg, Luxembourg, Luxembourg
Posts: 129
Rep Power: 9 
Hello Andrea,
I ran a similar setup when I started my PhD. It was injection of a liquid sheet in to a chamber, where i specified the pressure differences. But I was using OF1.5 and the boundary conditions that worked for me were: For pd: Inlet inlet { type fixedValue; value uniform 2e5; } outlet { type fixedValue; value uniform 0; } For U: { inlet { type pressureInletUniformVelocity; phi phi; rho rho; value uniform (0 0 0); } outlet { type pressureInletOutletVelocity; phi phi; value uniform (0 0 0); } and for U at walls i specified fixed value. for pd at walls i used zerogradient I am not sure if these bc's still exist in openfoam. But you can try them I hope they will work. bye regards K.Suresh kumar 

January 10, 2012, 05:25 

#4 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8 
Great!. It solved the problem.
The only difference with your configuration is that i'm using buoyantPressure for pressure at the wall (or fixedFluxPressure if the contactAngle is specified on alpha1). Thanks a lot! andrea 

January 10, 2012, 09:18 

#5 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8 
Hi again,
It seems that your suggestion has solved the first problem, but a new one now has appeared (otherwise it was too easy!). I got a floating point error: Code:
in "/opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so" [42] #1 Foam::sigFpe::sigFpeHandler(int) in "/opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so" [43] #1 Foam::sigFpe::sigFpeHandler(int) in "/opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so" [42] #2 in "/opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so" [43] #2 ???? in "/lib64/libc.so.6" [42] #3 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so" [42] #4 Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<double>&, Foam::Field<double> const&) const in "/lib64/libc.so.6" [43] #3 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so" [42] #5 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foa$ [43] #4 Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<double>&, Foam::Field<double> const&) const in "/opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so" [42] #6 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so" [43] #5 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foa$ [42] #7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so" [43] #6 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libfiniteVolume.so" [42] #8 in "/opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so" [43] #7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libfiniteVolume.so" [43] #8 main in "/opt/OpenFOAM/OpenFOAM1.7.1/applications/bin/linux64GccDPOpt/interFoam" [42] #9 __libc_start_main in "/lib64/libc.so.6" [42] #10 mainFoam::regIOobject::writeObject(Foam::IOstream::streamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/opt/OpenFOAM/OpenFOAM1.7.1/applications/bin/linux64GccDPOpt/inter$ [43] #9 __libc_start_main in "/opt/OpenFOAM/OpenFOAM1.7.1/applications/bin/linux64GccDPOpt/interFoam" [node03:02989] *** Process received signal *** [node03:02989] Signal: Floating point exception (8) [node03:02989] Signal code: (6) [node03:02989] Failing at address: 0x3f500000bad [node03:02989] [ 0] /lib64/libc.so.6 [0x2b0a630092d0] [node03:02989] [ 1] /lib64/libc.so.6(gsignal+0x35) [0x2b0a63009265] [node03:02989] [ 2] /lib64/libc.so.6 [0x2b0a630092d0] [node03:02989] [ 3] /opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so(_ZNK4Foam3PCG5solveERNS_5FieldIdEERKS2_h+0xe75) [0x2b0a621aa945] [node03:02989] [ 4] /opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so(_ZNK4Foam10GAMGSolver18solveCoarsestLevelERNS_5FieldIdEERKS2_+0x59f) [0x2b0a621c159f] [node03:02989] [ 5] /opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so(_ZNK4Foam10GAMGSolver6VcycleERKNS_7PtrListINS_9lduMatrix8smootherEEERNS_5FieldIdEERKS8_S9_S9_S9_RNS1_IS8_EESD_h+0xca1) [0x2b0a621c2e$ [node03:02989] [ 6] /opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so(_ZNK4Foam10GAMGSolver5solveERNS_5FieldIdEERKS2_h+0x48e) [0x2b0a621c44fe] [node03:02989] [ 7] /opt/OpenFOAM/OpenFOAM1.7.1/lib/linux64GccDPOpt/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE5solveERKNS_10dictionaryE+0x14b) [0x2b0a6166313b] [node03:02989] [ 8] interFoam [0x425a09] [node03:02989] [ 9] /lib64/libc.so.6(__libc_start_main+0xf4) [0x2b0a62ff6994] [node03:02989] [10] interFoam(_ZNK4Foam11regIOobject11writeObjectENS_8IOstream12streamFormatENS1_13versionNumberENS1_15compressionTypeE+0xf1) [0x41e419] [node03:02989] *** End of error message *** Code:
Courant Number mean: 0.000924621 max: 0.00771491 Interface Courant Number mean: 3.43381e07 max: 0.0011004 deltaT = 0.000601881 Time = 0.00398119 MULES: Solving for alpha1 Liquid phase volume fraction = 0.0330376 Min(alpha1) = 9.7801e57 Max(alpha1) = 1.00088 MULES: Solving for alpha1 Liquid phase volume fraction = 0.0330378 Min(alpha1) = 9.77621e57 Max(alpha1) = 1.00169 MULES: Solving for alpha1 Liquid phase volume fraction = 0.0330381 Min(alpha1) = 9.77228e57 Max(alpha1) = 1.0026 GAMG: Solving for p_rgh, Initial residual = 2.60679e06, Final residual = 1.76279e07, No Iterations 1 time step continuity errors : sum local = 1.31676e07, global = 6.14952e09, cumulative = 1.4974e07 GAMG: Solving for p_rgh, Initial residual = 5.02514e07, Final residual = 5.02514e07, No Iterations 0 time step continuity errors : sum local = 3.7534e07, global = 5.03656e09, cumulative = 1.54777e07 GAMG: Solving for p_rgh, Initial residual = 8.89208e07, Final residual = 8.89208e07, No Iterations 0 time step continuity errors : sum local = 6.64173e07, global = 2.40823e09, cumulative = 1.57185e07 ExecutionTime = 117.75 s ClockTime = 118 s Courant Number mean: 0.00111767 max: 0.0302757 Interface Courant Number mean: 4.14207e07 max: 0.0013322 deltaT = 0.000668757 Time = 0.00464995 MULES: Solving for alpha1 Liquid phase volume fraction = 0.0330384 Min(alpha1) = 9.7677e57 Max(alpha1) = 1.0035 MULES: Solving for alpha1 Liquid phase volume fraction = 0.0330387 Min(alpha1) = 9.7626e57 Max(alpha1) = 1.00543 MULES: Solving for alpha1 Liquid phase volume fraction = 0.0330389 Min(alpha1) = 9.75594e57 Max(alpha1) = 1.00734 GAMG: Solving for p_rgh, Initial residual = 6.52069e06, Final residual = 6.13259e07, No Iterations 1 time step continuity errors : sum local = 5.07027e07, global = 2.98245e08, cumulative = 1.27361e07 GAMG: Solving for p_rgh, Initial residual = 1.22576e06, Final residual = 2.2916e07, No Iterations 1 time step continuity errors : sum local = 1.89455e07, global = 2.48297e08, cumulative = 1.02531e07 GAMG: Solving for p_rgh, Initial residual = 4.76193e07, Final residual = 4.76193e07, No Iterations 0 time step continuity errors : sum local = 3.93663e07, global = 2.53955e08, cumulative = 7.71354e08 ExecutionTime = 120.63 s ClockTime = 121 s Courant Number mean: 0.00126773 max: 0.224444 Interface Courant Number mean: 4.68462e07 max: 0.00151491 deltaT = 0.000764293 Time = 0.00541424 MULES: Solving for alpha1 Liquid phase volume fraction = 0.0330393 Min(alpha1) = 9.74307e57 Max(alpha1) = 1.00901 MULES: Solving for alpha1 Liquid phase volume fraction = 0.0330396 Min(alpha1) = 9.71449e57 Max(alpha1) = 1.01605 MULES: Solving for alpha1 Liquid phase volume fraction = 0.0330399 Min(alpha1) = 9.6428e57 Max(alpha1) = 1.02287 regards andrea 

May 11, 2012, 06:06 

#6 
Senior Member
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 211
Rep Power: 9 
in OF 2.1.x a reflection of alpha1 at outlets appeared that wasn't the case in earlier versions. Using PISO instead of PIMPLE solved the problem, maybe this can help here, too.


January 17, 2013, 05:57 

#7 
New Member
Join Date: Dec 2012
Posts: 4
Rep Power: 5 
In my case I have also the problem of an unbounded alpha1. But I don't understand what you mean by saying I have to change PIMPLE to PISO, because PIMPLE is basically a combination of the PISO and SIMPLE alghorithm, and in interFoam you cannot change to PISO.


January 17, 2013, 09:52 

#8 
Senior Member
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 211
Rep Power: 9 
meanwhile I was told that setting zeroGradient for the pressure at the outlet lets both phases pass in interFoam. In OF 2.1 one cant change to PISO as in erlier releases and you are right, the reason must have been somwhere else. Do you use OF 2.1.1? It sais "Boundedness and consistency in the MULES algorithm has been improved for multiphase flows" at the release notes..


January 17, 2013, 11:47 

#9 
New Member
Join Date: Dec 2012
Posts: 4
Rep Power: 5 
Yes I use OF 2.1.1. I think it has to do with my buondary conditions. I have a fixed value for the inflow and the outflow of the domain, but also a fixed zero condition for a wall which is perpendicular and attach to the inflow and outflow. I think this imposes high pressure gradients locally and this maybe blows up my calculation.


January 20, 2013, 17:10 

#10  
Senior Member
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 211
Rep Power: 9 
Quote:


January 21, 2013, 10:17 

#11  
New Member
Join Date: Dec 2012
Posts: 4
Rep Power: 5 
Quote:


January 22, 2013, 16:09 

#12 
Senior Member
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 211
Rep Power: 9 
ok here is my last idea: Is the inflow area exactly the same as your outflow area, resp. are the inflow and outflow velocities adjusted accordingly up to a high precision? If for example due to rounding errors of the positions of the vertices in your blockMesh or whatever mesh generating file, the size of inflow and outflow does not match the specified inflow and outflow velocity up to a high precision, the continuity of mass could only be provided by changing the alpha1 value as the simulation proceeds...


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Implementation of boundary conditions for FVM  Tom  Main CFD Forum  7  August 26, 2014 05:58 
inlet velocity boundary condition  murali  CFX  5  August 3, 2012 08:56 
Outlet boundary condition for wave flume with interFoam solver  Arnoldinho  OpenFOAM  8  May 23, 2012 06:25 
Strange behaviour because of contact angle (interfoam)  Kim123  OpenFOAM Running, Solving & CFD  0  January 12, 2011 11:16 
Boundary conditions?  Tom  Main CFD Forum  0  November 5, 2002 02:54 