boundary conditions new case problem
Welcome everyone I have problem with new case..
When I translate mesh from icem I received mesh with 8 boundaries. then I try do standard simulation by solver icoFoam, but then I gets error : > FOAM FATAL IO ERROR: keyword PIPE_EDGE_0 is undefined in dictionary "/mnt/auto/people/plgsebaa/test_case/pipe_test1/0/p::boundaryField" file: /mnt/auto/people/plgsebaa/test_case/pipe_test1/0/p::boundaryField from line 25 to line 53. From function dictionary::subDict(const word& keyword) const in file db/dictionary/dictionary.C at line 456. FOAM exiting but in file p i defined Pipe egde.. version 2.0; format ascii; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 2 0 0 0 0]; internalField uniform 0; boundaryField { IN_OUT_0 { type zeroGradient; } IN_OUT_1 { type zeroGradient; } IN_OUT_2 { type zeroGradient; } BODY_HOT { type zeroGradient; } BODY_COLD { type zeroGradient; } PIPE_EGDE_0 { type empty; } PIPE_EGDE_1 { type empty; } PIPE_EGDE_2 { type empty; } } // ************************************************** *********************** // here in_out it's holes body hot it's internal mesh body cold it's external mesh and pipe edge it's surface at the hole http://img846.imageshack.us/img846/6995/pipej.jpg any Ideas how to do? greet Seba ;) 
i think your spelling is incorrect, you seem to have EDGE and EGDE

of course you're right.. :o
now another error.. may be badly defined ?? > FOAM FATAL IO ERROR: patch type 'wall' not constraint type 'empty' for patch PIPE_EDGE_0 of field p in file "/mnt/auto/people/plgsebaa/test_case/pipe_test1/0/p" file: /mnt/auto/people/plgsebaa/test_case/pipe_test1/0/p::boundaryField::PIPE_EDGE_0 from line 45 to line 45. From function emptyFvPatchField<Type>::emptyFvPatchField ( const fvPatch& p, const Field<Type>& field, const dictionary& dict ) in file fields/fvPatchFields/constraint/empty/emptyFvPatchField.C at line 100. FOAM exiting ?? 
check you boundary definition in constant/polyMesh/boundary
Do you also have patches specified as empty there? 
there I have:
boundary ( IN_OUT_0 { type wall; nFaces 7136; startFace 8976957; } IN_OUT_1 { type wall; nFaces 7286; startFace 8984093; } IN_OUT_2 { type wall; nFaces 6887; startFace 8991379; } BODY_COLD { type wall; nFaces 65467; startFace 8998266; } BODY_HOT { type wall; nFaces 123362; startFace 9063733; } PIPE_EDGE_0 { type wall; nFaces 12612; startFace 9187095; } PIPE_EDGE_1 { type wall; nFaces 12705; startFace 9199707; } PIPE_EDGE_2 { type wall; nFaces 12135; startFace 9212412; } 
you should have type empty in your constant/polyMesh/boundary file for your empty patches
take a look at the cavity tutorial: $FOAM_TUTORIALS/incompressible/icoFoam/cavity/ 
next problem..
You're right also :) and file U i also must edit. now it almost works but Starting time loop Time = 0.005 Courant Number mean: 0 max: 0.0551093 > FOAM FATAL ERROR: This mesh contains patches of type empty but is not 1D or 2D by virtue of the fact that the number of faces of this empty patch is not divisible by the number of cells. From function emptyFvPatchField<Type>::updateCoeffs() in file fields/fvPatchFields/constraint/empty/emptyFvPatchField.C at line 150. FOAM exiting is that because time step (deltaT = 0.005) is to big? 
no, sorry, did not look at your mesh before, empty patches are only used for 2D or 1D problems
Why do you want to use empty patches? Where are you PIPE_EDGES exactly in your mesh? Are they not just walls? 
pipe_edge is wall and it should be fixedValue I suppose. but then when flow influence in pipe by entry.. I got new error:
Time = 0.005 Courant Number mean: 0 max: 0.0551093 DILUPBiCG: Solving for Ux, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 5.26457e07, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0 > FOAM FATAL ERROR: Continuity error cannot be removed by adjusting the outflow. Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow. Total flux : 36.481 Specified mass inflow : 7539.44 Specified mass outflow : 0 Adjustable mass outflow : 0 From function adjustPhi(surfaceScalarField& phi, const volVectorField& U,const volScalarField& p in file cfdTools/general/adjustPhi/adjustPhi.C at line 115. FOAM exiting and then I try do "exit" from pipe by change wall into empty space :( 
OpenFOAM normally gives nice errors. In this case it tells you to use potentialFoam to initialize the flow, did you try this?

now, I change files little bit and something is running.. I will see is that correct ;)
greets Seba 
Hi stevenvanharen
I saw how helpful you were with Sebaj and I was wondering if you can help me as well. I am running a 2d case in OpenFoam using simpleFoam (incompressible 60m/s) and it gives me this error. DILUPBiCG: Solving for Ux, Initial residual = 0.324483, Final residual = 6.30403e06, No Iterations 5 #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam200/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam200/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #2 Uninterpreted: #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam200/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #4 in "/opt/openfoam200/platforms/linuxGccDPOpt/bin/simpleFoam" #5 in "/opt/openfoam200/platforms/linuxGccDPOpt/bin/simpleFoam" #6 in "/opt/openfoam200/platforms/linuxGccDPOpt/bin/simpleFoam" #7 __libc_start_main in "/lib/i386linuxgnu/libc.so.6" #8 in "/opt/openfoam200/platforms/linuxGccDPOpt/bin/simpleFoam" Do you have any idea y? Thank you in advance for your time, Sincerely, A.D.E 
me again.. :)
probably i have similiar problem.. Create time Create mesh for time = 0 Reading transportProperties Reading field p Reading field U Reading/calculating face flux field phi Starting time loop Time = 0.05 Courant Number mean: 0 max: 0.551093 DILUPBiCG: Solving for Ux, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 4.69515e08, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0 DICPCG: Solving for p, Initial residual = 1, Final residual = 9.60954e07, No Iterations 609 time step continuity errors : sum local = 4.2065e11, global = 1.63323e14, cumulative = 1.63323e14 DICPCG: Solving for p, Initial residual = 0.208382, Final residual = 9.50018e07, No Iterations 506 time step continuity errors : sum local = 2.39418e08, global = 5.87107e12, cumulative = 5.85473e12 ExecutionTime = 270.09 s ClockTime = 270 s Time = 0.1 Courant Number mean: 0.00498182 max: 0.880283 DILUPBiCG: Solving for Ux, Initial residual = 0.31478, Final residual = 5.87127e07, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.379635, Final residual = 1.43089e07, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0.333154, Final residual = 2.7084e06, No Iterations 2 DICPCG: Solving for p, Initial residual = 0.0603557, Final residual = 9.74963e07, No Iterations 538 time step continuity errors : sum local = 3.10184e08, global = 4.42633e11, cumulative = 3.84085e11 DICPCG: Solving for p, Initial residual = 0.68873, Final residual = 9.67525e07, No Iterations 522 time step continuity errors : sum local = 7.39548e09, global = 1.9175e11, cumulative = 1.92335e11 ExecutionTime = 516.3 s ClockTime = 516 s Time = 0.15 Courant Number mean: 0.00533215 max: 1.34034 DILUPBiCG: Solving for Ux, Initial residual = 0.0226568, Final residual = 2.8223e06, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.0133874, Final residual = 5.66317e06, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.116657, Final residual = 3.36112e07, No Iterations 3 DICPCG: Solving for p, Initial residual = 0.5099, Final residual = 9.89826e07, No Iterations 530 time step continuity errors : sum local = 2.90012e09, global = 1.72753e12, cumulative = 1.7506e11 DICPCG: Solving for p, Initial residual = 0.216951, Final residual = 9.63454e07, No Iterations 503 time step continuity errors : sum local = 1.80248e09, global = 1.18666e11, cumulative = 2.93726e11 ExecutionTime = 778.59 s ClockTime = 778 s Time = 0.2 Courant Number mean: 0.00529183 max: 3.17097 DILUPBiCG: Solving for Ux, Initial residual = 0.012159, Final residual = 7.18277e06, No Iterations 9 DILUPBiCG: Solving for Uy, Initial residual = 0.00836557, Final residual = 6.1792e06, No Iterations 3 DILUPBiCG: Solving for Uz, Initial residual = 0.0491227, Final residual = 2.08374e06, No Iterations 8 DICPCG: Solving for p, Initial residual = 0.287848, Final residual = 9.7348e07, No Iterations 552 time step continuity errors : sum local = 1.46002e09, global = 6.9727e13, cumulative = 2.86753e11 DICPCG: Solving for p, Initial residual = 0.121064, Final residual = 8.8766e07, No Iterations 557 time step continuity errors : sum local = 1.05088e09, global = 1.58428e12, cumulative = 3.02596e11 ExecutionTime = 1066.14 s ClockTime = 1066 s End and it's not write time files.. what's wrong? greets Seba 
Hello Seba,
data writing is specified in the controlDict, see http://www.openfoam.com/docs/user/controlDict.php Hope this helps. Florian 
Quote:

hi florian_krause
my controlDict file, here I think everything is ok :) problem is maybe in other file? FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application icoFoam; startFrom startTime; startTime 0; stopAt endTime; endTime 0.2; deltaT 0.05; writeControl timeStep; writeInterval 20; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression uncompressed; timeFormat general; timePrecision 6; runTimeModifiable yes; // ************************************************** *********************** // 
Hello Seba,
you specify: deltaT 0.05; writeControl timeStep; writeInterval 20; you write out your fields every 20 time steps, but you have only 4 time steps of deltaT=0.05 to reach endTime 0.2. Should be clear now. Florian 
hey florian_krause,
when I change writeInterval 20; to 1 how You advised, it's work :) thanks a lot :D now i try to visualize data :) 
Quote:
Hi Seba, I m getting the same error as your yours could you tell me how you corrected it ?? The error is Starting time loop Time = 0.0005 Courant Number mean: 0.000416667 max: 0.0416667 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 8.31588e07, No Iterations 3 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 1.21225e06, No Iterations 3 > FOAM FATAL ERROR: Continuity error cannot be removed by adjusting the outflow. Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow. Total flux : 2.89283e05 Specified mass inflow : 0.0005 Specified mass outflow : 0 Adjustable mass outflow : 0 From function adjustPhi(surfaceScalarField&, const volVectorField&,volScalarField&) in file cfdTools/general/adjustPhi/adjustPhi.C at line 118. FOAM exiting Thanks in advance 
Hi,
Try adding special small surface (inletoutlet without airflow velocity set) to compensate fot inequality between inflow and outflow :cool: 
All times are GMT 4. The time now is 15:30. 