|
[Sponsors] |
Error when running BuoyantBoussinesqSimpleFoam |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
June 18, 2020, 07:16 |
Error when running BuoyantBoussinesqSimpleFoam
|
#1 |
Member
Ben Simpson
Join Date: Dec 2019
Location: UK
Posts: 32
Rep Power: 7 |
Hi,
I am trying to run a simulation using the BuoyantBoussinesqSimpleFoam solver in OpenFOAM v-1812. The simulation is of a naturally ventilated building with space on the outside for the external environment. Currently when I try running BuoyantBoussinesqSimpleFoam the simulation is exiting due to an error. The error is as follows: Code:
------------------------------------------------------- Primary job terminated normally, but 1 process returned a non-zero exit code.. Per user-direction, the job has been aborted. ------------------------------------------------------- -------------------------------------------------------------------------- mpirun detected that one or more processes exited with non-zero status, thus causing the job to be terminated. The first process to do so was: Process name: [[5190,1],1] Exit code: 142 -------------------------------------------------------------------------- Any help on this issue would be much appreciated. Kind regards, Ben My boundary conditions are as follows: Code:
FoamFile { version 2.0; format ascii; class volScalarField; object p_rgh; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -2 0 0 0 0]; internalField uniform 1e5; boundaryField { "xmin|xmax|ymin|ymax|zmax" { type totalPressure; p0 $internalField; } "zmin|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ|Inlet" { type fixedFluxPressure; value $internalField; } #includeEtc "caseDicts/setConstraintTypes" } FoamFile { version 2.0; format ascii; class volScalarField; object T; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 0 1 0 0 0]; internalField uniform 293; boundaryField { "xmin|xmax|ymin|ymax|zmin|zmax|Ceiling|Floor|EWall|NWall|SWall|WWall|Inlet" { type fixedValue; value uniform 293; } PC { type fixedGradient; gradient uniform 100; } Occ { type fixedGradient; gradient uniform 130; } #includeEtc "caseDicts/setConstraintTypes" } FoamFile { version 2.0; format ascii; class volVectorField; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { "xmin|xmax|ymin|ymax|zmax" { type pressureInletOutletVelocity; value uniform (0 0 0); } "zmin|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ" { type noSlip; } Inlet { type fixedValue; value uniform (0 0.00047 0); //value uniform (0 1 0); } #includeEtc "caseDicts/setConstraintTypes" } FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object alphat; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -1 0 0 0 0]; internalField uniform 0; boundaryField { "xmin|xmax|ymin|ymax|zmax|Inlet" { type calculated; value uniform 0; } "zmin|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ" { type alphatJayatillekeWallFunction; Prt 0.85; value uniform 0; } #includeEtc "caseDicts/setConstraintTypes" } FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object CO2; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 0 0 0 0 0]; internalField uniform 0; boundaryField { "xmin|xmax|ymin|ymax|zmax" { type inletOutlet; inletValue $internalField; value $internalField; } "zmin|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ" { type zeroGradient; } Inlet { type fixedValue; value uniform 1.0; } #includeEtc "caseDicts/setConstraintTypes" } FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object epsilon; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // //epsilonInlet 0.03; // Cmu^0.75 * k^1.5 / L ; L =10 dimensions [0 2 -3 0 0 0 0]; internalField uniform 0.01; boundaryField { "xmin|xmax|ymin|ymax|zmax" { type inletOutlet; inletValue uniform 0.01; value uniform 0.01; } "zmin|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ" { type epsilonWallFunction; value $internalField; } Inlet { type fixedValue; value $internalField; } #includeEtc "caseDicts/setConstraintTypes" } FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object k; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // kInlet 1.5; // approx k = 1.5*(I*U)^2 ; I = 0.1 dimensions [0 2 -2 0 0 0 0]; internalField uniform 0.1; boundaryField { "xmin|xmax|ymin|ymax|zmax" { type inletOutlet; inletValue uniform 0.01; value uniform 0.01; } "zmin|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ" { type kqRWallFunction; value uniform 0.1; } Inlet { type fixedValue; value uniform 0.1; } #includeEtc "caseDicts/setConstraintTypes" } FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object nut; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -1 0 0 0 0]; internalField uniform 0; boundaryField { "xmin|xmax|ymin|ymax|zmax|Inlet" { type calculated; value uniform 0; } "zmin|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ" { type nutkWallFunction; value uniform 0; } #includeEtc "caseDicts/setConstraintTypes" } FoamFile { version 2.0; format ascii; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -2 0 0 0 0]; internalField uniform 1e5; boundaryField { "xmin|xmax|ymin|ymax|zmin|zmax|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ|Inlet" { type fixedFluxPressure; rho rhok; value uniform 0; } #includeEtc "caseDicts/setConstraintTypes" } |
|
June 19, 2020, 21:15 |
|
#2 |
Member
Lisandro Maders
Join Date: Feb 2013
Posts: 98
Rep Power: 13 |
Hello,
Can you run other cases in parallel (tutorials?).. Doesn't look like a case problem, but some wrong mpi setup or similar.. Also, did you remember to source OpenFOAM? Cheers, |
|
June 21, 2020, 16:36 |
|
#3 |
Member
Ben Simpson
Join Date: Dec 2019
Location: UK
Posts: 32
Rep Power: 7 |
Thank you Lisandro, for your response.
I have tried running one of my other cases and the windaroundbuildings tutorial case, both run in parallel. Both ran to an endTime of 5000 without any errors. I tried running my current case not in parallel and the solver stopped at a similar time to the parallel run, but without any error message or convergence message. I have copied the end of the log file below. Can you explain what you mean by source OpenFOAM? Kind regards, Ben Code:
Time = 499 DILUPBiCGStab: Solving for Ux, Initial residual = 4.2035517e-12, Final residual = 4.2035517e-12, No Iterations 0 DILUPBiCGStab: Solving for Uy, Initial residual = 1.3809356e-12, Final residual = 1.3809356e-12, No Iterations 0 DILUPBiCGStab: Solving for Uz, Initial residual = 3.4626842e-11, Final residual = 3.4626842e-11, No Iterations 0 DILUPBiCGStab: Solving for T, Initial residual = 5.7255095e-07, Final residual = 5.7255095e-07, No Iterations 0 DICPCG: Solving for p_rgh, Initial residual = 4.8174887e-29, Final residual = 4.8174887e-29, No Iterations 0 time step continuity errors : sum local = 4.7379025e+47, global = 6.7267478e+38, cumulative = 1.3690775e+39 DILUPBiCGStab: Solving for epsilon, Initial residual = 0.081559159, Final residual = 2.7467555e-07, No Iterations 1 bounding epsilon, min: -5.0589917e+76 max: 6.6333303e+104 average: 6.9901096e+98 DILUPBiCGStab: Solving for k, Initial residual = 9.7152148e-06, Final residual = 9.7152148e-06, No Iterations 0 ExecutionTime = 12550.98 s ClockTime = 12575 s fieldMinMax fieldMinMax write: min(mag(U)) = 0 in cell 0 at location (-2.9166667 -2.9166667 0) max(mag(U)) = 8.3277972e+51 in cell 58642 at location (-0.28756519 5.8448262 0.38346076) min(CO2) = -1.3654693e-08 in cell 2506767 at location (13.100119 16.077201 2.082341) max(CO2) = 1 in cell 471004 at location (7.8713678 2.5999999 1.2113401) min(p) = -3.6330321e+87 in cell 1506619 at location (-0.14127546 8.297961 3.4) max(p) = 1.0130987e+73 in cell 595727 at location (-0.018164488 7.8713315 3.1237291) min(T) = 292.99634 in cell 524500 at location (11.752019 15.324934 0.72123229) max(T) = 476.00394 in cell 267900 at location (13.908153 16.782254 3.3148686) scalarTransport execute: CO2 DILUPBiCGStab: Solving for CO2, Initial residual = 2.1732333e-28, Final residual = 2.1732333e-28, No Iterations 0 Time = 500 DILUPBiCGStab: Solving for Ux, Initial residual = 1, Final residual = 0.0032024424, No Iterations 1 DILUPBiCGStab: Solving for Uy, Initial residual = 1, Final residual = 0.0032024424, No Iterations 1 DILUPBiCGStab: Solving for Uz, Initial residual = 1, Final residual = 0.0032024579, No Iterations 1 DILUPBiCGStab: Solving for T, Initial residual = 1.1094197e-06, Final residual = 1.1094197e-06, No Iterations 0 |
|
June 21, 2020, 17:53 |
|
#4 |
Senior Member
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 931
Rep Power: 13 |
Hi
- The maximum magnitude of the velocity field is nonphysically large. Also, that of epsilon field. - Could you double-check the mesh metrics? `checkMesh -allGeometry -allTopology`? - Could you run your case with another turbulence closure model, e.g. omega-based model?
__________________
The OpenFOAM community is the biggest contributor to OpenFOAM: User guide/Wiki-1/Wiki-2/Code guide/Code Wiki/Journal Nilsson/Guerrero/Holzinger/Holzmann/Nagy/Santos/Nozaki/Jasak/Primer Governance Bugs/Features: OpenFOAM (ESI-OpenCFD-Trademark) Bugs/Features: FOAM-Extend (Wikki-FSB) Bugs: OpenFOAM.org How to create a MWE New: Forkable OpenFOAM mirror |
|
June 22, 2020, 17:14 |
|
#5 |
Member
Ben Simpson
Join Date: Dec 2019
Location: UK
Posts: 32
Rep Power: 7 |
Thank you for your response.
I have run check mesh and couldnt see any issues in the log file. Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Enabling all (cell, face, edge, point) topology checks. Enabling all geometry checks. Time = 0 Mesh stats points: 349461 faces: 1004544 internal faces: 961536 cells: 327680 faces per cell: 6 boundary patches: 7 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 327680 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 0 Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Topological cell zip-up check OK. Face-face connectivity OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology Bounding box xmin 2560 2709 ok (non-closed singly connected) (-3 -3 0) (18.7 -3 3.4) xmax 2560 2709 ok (non-closed singly connected) (-3 18.7 0) (18.7 18.7 3.4) ymin 2560 2709 ok (non-closed singly connected) (-3 -3 0) (-3 18.7 3.4) ymax 2560 2709 ok (non-closed singly connected) (18.7 -3 0) (18.7 18.7 3.4) zmin 16384 16641 ok (non-closed singly connected) (-3 -3 0) (18.7 18.7 0) zmax 7920 8360 ok (non-closed singly connected) (-3 -3 3.4) (18.7 18.7 3.4) zmax_ceiling 8464 8649 ok (non-closed singly connected) (0 0 3.4) (15.7 15.7 3.4) Checking faceZone topology for multiply connected surfaces... No faceZones found. Checking basic cellZone addressing... No cellZones found. Checking geometry... Overall domain bounding box (-3 -3 0) (18.7 18.7 3.4) Mesh has 3 geometric (non-empty/wedge) directions (1 1 1) Mesh has 3 solution (non-empty) directions (1 1 1) Boundary openness (4.4299191e-16 4.4299191e-16 -7.1450608e-15) OK. Max cell openness = 1.2245107e-16 OK. Max aspect ratio = 1.0239131 OK. Minimum face area = 0.027777776. Maximum face area = 0.029122167. Face area magnitudes OK. Min volume = 0.0047222218. Max volume = 0.0049507683. Total volume = 1601.026. Cell volumes OK. Mesh non-orthogonality Max: 0 average: 0 Non-orthogonality check OK. Face pyramids OK. Max skewness = 1.2789791e-13 OK. Coupled point location match (average 0) OK. Face tets OK. Min/max edge length = 0.16666666 0.17065218 OK. All angles in faces OK. Face flatness (1 = flat, 0 = butterfly) : min = 1 average = 1 All face flatness OK. Cell determinant (wellposedness) : minimum: 0.1249674 average: 0.93518669 Cell determinant check OK. Concave cell check OK. Face interpolation weight : minimum: 0.49409237 average: 0.49993708 Face interpolation weight check OK. Face volume ratio : minimum: 0.97664544 average: 0.99975127 Face volume ratio check OK. Mesh OK. End Here is the end of the log file before my computer died. Code:
Time = 1613 DILUPBiCGStab: Solving for Ux, Initial residual = 0.0022768434, Final residual = 3.8302314e-05, No Iterations 1 DILUPBiCGStab: Solving for Uy, Initial residual = 0.00087106937, Final residual = 1.5127342e-05, No Iterations 1 DILUPBiCGStab: Solving for Uz, Initial residual = 0.0016276516, Final residual = 2.8328342e-05, No Iterations 1 DILUPBiCGStab: Solving for T, Initial residual = 0.0012589984, Final residual = 6.7196765e-05, No Iterations 1 DICPCG: Solving for p_rgh, Initial residual = 0.0089650297, Final residual = 8.7014216e-05, No Iterations 55 time step continuity errors : sum local = 1.5389332e-05, global = -1.902396e-06, cumulative = -0.0041707033 smoothSolver: Solving for omega, Initial residual = 0.00039958681, Final residual = 2.8080538e-05, No Iterations 3 DILUPBiCGStab: Solving for k, Initial residual = 0.00018173884, Final residual = 4.1791532e-06, No Iterations 1 ExecutionTime = 17547.01 s ClockTime = 17682 s fieldMinMax fieldMinMax write: min(mag(U)) = 0 in cell 0 at location (-2.9166667 -2.9166667 0) on processor 0 max(mag(U)) = 1.049388 in cell 108330 at location (1.8558424 15.718582 3.3788139) on processor 2 min(CO2) = 0 in cell 0 at location (-2.9166667 -3 0.085) on processor 0 max(CO2) = 1 in cell 277850 at location (1.899056 7.5999999 1.2113291) on processor 0 min(p) = 99965.943 in cell 276497 at location (13.758831 15.718746 3.4) on processor 3 max(p) = 100000 in cell 135893 at location (12.521604 15.718749 0) on processor 3 min(T) = 293 in cell 0 at location (-2.9166667 -3 0.085) on processor 0 max(T) = 1186.3781 in cell 108330 at location (1.8558424 15.718582 3.3788139) on processor 2 scalarTransport execute: CO2 DILUPBiCGStab: Solving for CO2, Initial residual = 0.00036557033, Final residual = 6.8689503e-06, No Iterations 1 Time = 1614 DILUPBiCGStab: Solving for Ux, Initial residual = 0.0029013552, Final residual = 4.6281166e-05, No Iterations 1 DILUPBiCGStab: Solving for Uy, Initial residual = 0.0010731421, Final residual = 1.7715774e-05, No Iterations 1 DILUPBiCGStab: Solving for Uz, Initial residual = 0.0017262862, Final residual = 2.9371945e-05, No Iterations 1 DILUPBiCGStab: Solving for T, Initial residual = 0.0012577848, Final residual = 6.7378228e-05, No Iterations 1 DICPCG: Solving for p_rgh, Initial residual = 0.0090579121, Final residual = 8.7629514e-05, No Iterations 43 time step continuity errors : sum local = 1.5462643e-05, global = -1.1040759e-06, cumulative = -0.0041718074 smoothSolver: Solving for omega, Initial residual = 0.00039540712, Final residual = 2.8313504e-05, No Iterations 3 DILUPBiCGStab: Solving for k, Initial residual = 0.00017238916, Final residual = 4.1214014e-06, No Iterations 1 ExecutionTime = 17560.16 s ClockTime = 17698 s fieldMinMax fieldMinMax write: min(mag(U)) = 0 in cell 0 at location (-2.9166667 -2.9166667 0) on processor 0 max(mag(U)) = 1.046601 in cell 108330 at location (1.8558424 15.718582 3.3788139) on processor 2 min(CO2) = 0 in cell 0 at location (-2.9166667 -3 0.085) on processor 0 max(CO2) = 1 in cell 277850 at location (1.899056 7.5999999 1.2113291) on processor 0 min(p) = 99965.943 in cell 271108 at location (1.9411685 15.718749 3.4) on processor 2 max(p) = 100000 in cell 73613 at location (7.8713315 -0.018749525 0) on processor 1 min(T) = 293 in cell 0 at location (-2.9166667 -3 0.085) on processor 0 max(T) = 1180.8241 in cell 108330 at location (1.8558424 15.718582 3.3788139) on processor 2 scalarTransport execute: CO2 DILUPBiCGStab: Solving for CO2, Initial residual = 0.00036510744, Final residual = 6.8622869e-06, No Iterations 1 Kind regards, Ben |
|
June 22, 2020, 18:08 |
|
#6 |
Senior Member
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 931
Rep Power: 13 |
The culprit is the epsilon. There would be lots of reasons, I'm afraid. Please do search web - there should already be lots of insightful remarks about epsilon's numerical fragility.
Good luck. PS:Might be wise to check with other epsilon-based models, e.g. kepsilonphitf or rngkepsilon. etc.
__________________
The OpenFOAM community is the biggest contributor to OpenFOAM: User guide/Wiki-1/Wiki-2/Code guide/Code Wiki/Journal Nilsson/Guerrero/Holzinger/Holzmann/Nagy/Santos/Nozaki/Jasak/Primer Governance Bugs/Features: OpenFOAM (ESI-OpenCFD-Trademark) Bugs/Features: FOAM-Extend (Wikki-FSB) Bugs: OpenFOAM.org How to create a MWE New: Forkable OpenFOAM mirror |
|
June 23, 2020, 21:31 |
|
#7 |
Member
Lisandro Maders
Join Date: Feb 2013
Posts: 98
Rep Power: 13 |
You could try to under-relax the fields a little bit. The BC's looks fine. This could be a mesh problem, can you share some image of a slice of your mesh?
Also, can you share the fvSchemes and fvSolution files you are using? Did you use the same files for both k-epsilon and kOmega-SST? |
|
June 24, 2020, 09:05 |
|
#8 |
Member
Ben Simpson
Join Date: Dec 2019
Location: UK
Posts: 32
Rep Power: 7 |
Thanks for the replies.
I have been looking into better defining my BC's (especially for k and epsilon) previously they were just taken from tutorials. As for the fvSolutions and fvSchemes, I have copied them below. For the Omega run I used the same solutions and schemes as this but jut added Omega. For that I copied the Omega relevant parts from the motorbike tutorial. I will try a run with under-relaxing the fields. Code:
FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phi,U) bounded Gauss upwind; div(phi,T) bounded Gauss upwind; div(phi,k) bounded Gauss upwind; div(phi,epsilon) bounded Gauss upwind; div(phi,CO2) bounded Gauss upwind; div((nuEff*dev2(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } // ************************************************************************* // FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { p_rgh { solver PCG; preconditioner DIC; tolerance 1e-06; relTol 0.01; } "(U|T|h|k|epsilon|CO2)" { solver PBiCGStab; preconditioner DILU; tolerance 1e-05; relTol 0.1; } G { $p_rgh; tolerance 1e-05; relTol 0.1; } } SIMPLE { nNonOrthogonalCorrectors 0; pRefCell 0; pRefValue 0; residualControl { p_rgh 1e-4; U 1e-4; CO2 1e-4; T 1e-4; h 1e-4; G 1e-4; // possibly check turbulence fields "(k|epsilon|omega)" 1e-4; } } relaxationFactors { fields { rho 1.0; p_rgh 0.9; } equations { U 0.3; CO2 0.3; h 0.9; T 0.5; "(k|epsilon|R)" 0.7; P 0.8; G 0.7; } } // ************************************************************************* // Kind regards, Ben |
|
June 26, 2020, 10:18 |
|
#9 |
Member
Ben Simpson
Join Date: Dec 2019
Location: UK
Posts: 32
Rep Power: 7 |
I have been able to get my model running by adjusting the relaxation factors for epsilon as you suggested. A value of 1 allowed my model to run without errors.
I still need to go back a better define my BC's but at least I have a functioning model for the time being. Thanks for all the support with this issue. Regards, Ben |
|
Tags |
buoyancy driven flow, buoyantboussinesqsimple, openfoam 1812 |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Simulation just stops output writing, but keeps running | blaise | OpenFOAM Running, Solving & CFD | 6 | March 27, 2024 05:49 |
Running Case in Parallel | Typ | Main CFD Forum | 5 | May 11, 2020 04:43 |
[swak4Foam] swak4foam openfoam 7 installation problem | Andrea23 | OpenFOAM Community Contributions | 1 | February 17, 2020 19:11 |
Error problem while running sadia d lts tutorial | kane | OpenFOAM Running, Solving & CFD | 2 | May 26, 2018 04:38 |
Error Running Design of Experiments in ANSYS Fluent | tytrzecki | FLUENT | 0 | April 22, 2018 16:01 |