 |
 |
 |
|
|
|
[Sponsors] | ||||
Heat transfer in liquid water suggestions for chioce of solver |
 |
|
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
October 17, 2008, 09:48
|
Hi Bernard,
I realised an h
|
#21 |
|
Member
Christian Lindbäck
Join Date: Mar 2009
Posts: 55
Rep Power: 17  |
Hi Bernard,
I realised an hour ago that pressure in compressible solvers is of dimension Pascal and that pressure in incompressible solvers is of dimension pressure/density. The solver is running now. Sorry, I should have posted a message that everything is well, for now  |
|
|
|
|
|
July 23, 2009, 06:32
|
|
#22 |
|
Senior Member
J. Cai
Join Date: Apr 2009
Posts: 180
Rep Power: 17 |
Hi, dear foamers, When I run the boussinesqBuoyantSimpleFoam solver on my own case, the following error appears:
Time = 0.05 DILUPBiCG: Solving for Ux, Initial residual = 0.989258, Final residual = 0.0103564, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.973745, Final residual = 0.0111817, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.975119, Final residual = 0.00821149, No Iterations 1 GAMG: Solving for p, Initial residual = 9.53872e-06, Final residual = 5.94514e-07, No Iterations 1 time step continuity errors : sum local = 1.07053e+17, global = -1.94455e+13, cumulative = -1.94455e+13 DILUPBiCG: Solving for epsilon, Initial residual = 1, Final residual = 0.00430228, No Iterations 1 bounding epsilon, min: -1.3712e+37 max: 4.32279e+38 average: 7.36798e+32 #0 _ZN4Foam5error10printStackERNS_7OstreamE-0xb34150 in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/lib/linuxIA64GccDPOpt/libOpenFOAM.so" #1 _ZN4Foam6sigFpe13sigFpeHandlerEi-0xad1820 in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/lib/linuxIA64GccDPOpt/libOpenFOAM.so" #2 Uninterpreted: [0xa0000000000107e0] #3 _ZNK4Foam13LimitedSchemeIdNS_14vanLeerLimiterINS_6 NVDTVDEEENS_10limitFuncs6magSqrEE7limiterERKNS_14G eometricFieldIdNS_12fvPatchFieldENS_7volMeshEEE-0x1d0538e in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/lib/linuxIA64GccDPOpt/libfiniteVolume.so" #4 _ZNK4Foam33limitedSurfaceInterpolationSchemeIdE7we ightsERKNS_14GeometricFieldIdNS_12fvPatchFieldENS_ 7volMeshEEE-0x1f1c680 in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/lib/linuxIA64GccDPOpt/libfiniteVolume.so" #5 _ZNK4Foam2fv21gaussConvectionSchemeIdE6fvmDivERKNS _14GeometricFieldIdNS_13fvsPatchFieldENS_11surface MeshEEERNS3_IdNS_12fvPatchFieldENS_7volMeshEEE-0x1f192a0 in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/lib/linuxIA64GccDPOpt/libfiniteVolume.so" #6 Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::div<double>(Foam::GeometricField<double , Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::word const&) in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxIA64GccDPOpt/boussinesqBuoyantSimpleFoam" #7 Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::div<double>(Foam::GeometricField<double , Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&) in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxIA64GccDPOpt/boussinesqBuoyantSimpleFoam" #8 _ZN4Foam10boussinesq9RASModels8kEpsilon7correctEv-0x28bce90 in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/lib/linuxIA64GccDPOpt/libboussinesqRASModels.so" #9 main in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxIA64GccDPOpt/boussinesqBuoyantSimpleFoam" #10 __libc_start_main-0x734df0 in "/lib/tls/libc.so.6.1" #11 _start in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxIA64GccDPOpt/boussinesqBuoyantSimpleFoam" Floating exception Any comments? thank you very much in advance. |
|
|
|
|
|
|
July 23, 2009, 07:09
|
|
#23 | |
|
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Quote:
- why do you have a timestep!=1 for a steady solver (not that it matters much, but it gives me the suspicion that the settings you're using were meant for a transient solver) - is this the first time-step where continuity explodes? - do you have relaxation? - was the vanLeer your idea? - what are the boundary conditions? Bernhard |
||
|
|
|
||
|
July 23, 2009, 07:51
|
|
#24 |
|
Senior Member
J. Cai
Join Date: Apr 2009
Posts: 180
Rep Power: 17 |
Hello, Bernhard, thank you very much for your precious comments.
About the relaxation, it is shown as follows. relaxationFactors { p 0.15; U 0.3; k 0.3; epsilon 0.3; R 0.7; nuTilda 0.7; T 0.3; } Sorry, I have to post the results in the follows for the reason of too many characters. Last edited by chiven; July 23, 2009 at 08:21. |
|
|
|
|
|
|
July 23, 2009, 07:52
|
|
#25 |
|
Senior Member
J. Cai
Join Date: Apr 2009
Posts: 180
Rep Power: 17 |
I changed the deltaT=1, and do calculation again, the results are shown in follows.
Create time Create mesh for time = 0 Reading transportProperties Reading environmentalProperties Reading field p Reading field T Reading field Q Reading field U Creating field alphaEff Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Selecting RAS turbulence model kEpsilon kEpsilonCoeffs { Cmu 0.09; C1 1.44; C2 1.92; Cb 1.44; alphaEps 0.76923; } Starting time loop Convergence criterion for U = 0.001 Convergence criterion for p = 0.01 Convergence criterion for T = 0.001 Time = 1 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.00959259, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0060194, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.00859174, No Iterations 1 GAMG: Solving for p, Initial residual = 1, Final residual = 0.00880705, No Iterations 9 time step continuity errors : sum local = 0.000515452, global = -1.32363e-05, cumulative = -1.32363e-05 DILUPBiCG: Solving for epsilon, Initial residual = 0.0516045, Final residual = 0.000326048, No Iterations 1 bounding epsilon, min: -1.05947 max: 85.5521 average: 2.55034 DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 0.0173683, No Iterations 1 DILUPBiCG: Solving for T, Initial residual = 0.000886871, Final residual = 2.99323e-06, No Iterations 1 ExecutionTime = 142.679 s ClockTime = 143 s Initial residual for U = 1 Initial residual for p = 1 Initial residual for T = 0.000886871 Time = 3 DILUPBiCG: Solving for Ux, Initial residual = 0.998546, Final residual = 0.0174537, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.999007, Final residual = 0.0185219, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.999519, Final residual = 0.0171578, No Iterations 1 GAMG: Solving for p, Initial residual = 0.984913, Final residual = 0.00683274, No Iterations 3 time step continuity errors : sum local = 904905, global = -7597.79, cumulative = -7597.66 DILUPBiCG: Solving for epsilon, Initial residual = 1, Final residual = 0.00633617, No Iterations 1 bounding epsilon, min: -2.0693e+12 max: 3.04074e+13 average: 2.12447e+08 DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 0.00279179, No Iterations 1 bounding k, min: -2.59096e+10 max: 1.58311e+12 average: 4.51853e+06 DILUPBiCG: Solving for T, Initial residual = 0.0518603, Final residual = 0.00156515, No Iterations 1 ExecutionTime = 357.442 s ClockTime = 358 s Initial residual for U = 0.999519 Initial residual for p = 0.984913 Initial residual for T = 0.0518603 Time = 5 DILUPBiCG: Solving for Ux, Initial residual = 0.989258, Final residual = 0.0103564, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.973745, Final residual = 0.0111817, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.975119, Final residual = 0.00821149, No Iterations 1 GAMG: Solving for p, Initial residual = 9.53872e-06, Final residual = 5.94514e-07, No Iterations 1 time step continuity errors : sum local = 1.07053e+19, global = -1.94455e+15, cumulative = -1.94455e+15 DILUPBiCG: Solving for epsilon, Initial residual = 1, Final residual = 0.00430228, No Iterations 1 bounding epsilon, min: -1.3712e+37 max: 4.32279e+38 average: 7.36798e+32 #0 _ZN4Foam5error10printStackERNS_7OstreamE-0xb34150 in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/lib/linuxIA64GccDPOpt/libOpenFOAM.so" #1 _ZN4Foam6sigFpe13sigFpeHandlerEi-0xad1820 in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/lib/linuxIA64GccDPOpt/libOpenFOAM.so" #2 Uninterpreted: [0xa0000000000107e0] #3 _ZNK4Foam13LimitedSchemeIdNS_14vanLeerLimiterINS_6 NVDTVDEEENS_10limitFuncs6magSqrEE7limiterERKNS_14G eometricFieldIdNS_12fvPatchFieldENS_7volMeshEEE-0x1d0538e in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/lib/linuxIA64GccDPOpt/libfiniteVolume.so" #4 _ZNK4Foam33limitedSurfaceInterpolationSchemeIdE7we ightsERKNS_14GeometricFieldIdNS_12fvPatchFieldENS_ 7volMeshEEE-0x1f1c680 in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/lib/linuxIA64GccDPOpt/libfiniteVolume.so" #5 _ZNK4Foam2fv21gaussConvectionSchemeIdE6fvmDivERKNS _14GeometricFieldIdNS_13fvsPatchFieldENS_11surface MeshEEERNS3_IdNS_12fvPatchFieldENS_7volMeshEEE-0x1f192a0 in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/lib/linuxIA64GccDPOpt/libfiniteVolume.so" #6 Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::div<double>(Foam::GeometricField<double , Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::word const&) in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxIA64GccDPOpt/boussinesqBuoyantSimpleFoam" #7 Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::div<double>(Foam::GeometricField<double , Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&) in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxIA64GccDPOpt/boussinesqBuoyantSimpleFoam" #8 _ZN4Foam10boussinesq9RASModels8kEpsilon7correctEv-0x28bce90 in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/lib/linuxIA64GccDPOpt/libboussinesqRASModels.so" #9 main in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxIA64GccDPOpt/boussinesqBuoyantSimpleFoam" #10 __libc_start_main-0x734df0 in "/lib/tls/libc.so.6.1" #11 _start in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxIA64GccDPOpt/boussinesqBuoyantSimpleFoam" Floating exception |
|
|
|
|
|
|
July 23, 2009, 08:16
|
|
#26 | |
|
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Quote:
- when starting a new case base the settings on a stable calculation with the same solver. Usually such settings can be found in $FOAM_TUTORIALS. So what I'd recommend is to use fvSchemes, fvSolution and controlDict from the buoyantSimple(!)Foam-hotroom as a first guess for your case. The references to vanLeer indicate that this is not the case for your calculation - for outflows that have zeroGradient for U don't use zeroGradient for transported quantities like k, epsilon and T. Use inletOutlet. Otherwise things might explode when you get a backflow there Bernhard |
||
|
|
|
||
|
|
|
Similar Threads
|
||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| Solver for heat transfer calculation with water media | benyamin1 | OpenFOAM Running, Solving & CFD | 6 | January 27, 2011 04:26 |
| Liquid Metals and Heat Transfer | juanltm | OpenFOAM Running, Solving & CFD | 7 | October 28, 2009 05:00 |
| Solid-Liquid heat transfer | Tu | CFX | 0 | August 17, 2008 17:42 |
| Heat transfer from solid to liquid | Richard | FLUENT | 2 | January 30, 2006 04:10 |
| Heat Transfer from Solid To Liquid! | Richard | FLUENT | 1 | January 20, 2006 05:43 |
Linear Mode
