|
[Sponsors] |
Divergence in compressible LES, rhoPimpleFoam |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
New Member
Christopher Bruns
Join Date: Jun 2021
Posts: 6
Rep Power: 5 ![]() |
Dear Foamers,
I'm new to OpenFoam. However, I've got experiences using Ansys Fluent back in the days and more recent using Code_Saturne 7. The problem I've got is that Code_Saturne works well, but not using compressible flows since it is developed for majorly inkompressible flows. Furthermore, it is limited to compressible RANS models. LES is not possible because of the 1st order schemes. That is why I wanted to try OpenFoam. We try to solve the flow pattern in the hot air flow inside melt-blown nozzles. Therefore, we are facing velocities of Ma > 0.3 of more than 250 m/s. After checking some tutorials, I tried to solve the Code_Saturne model with was pre-processed using Salome 9. The mesh specs are: - 2 dimensions, 2 inlets, 1 outlet and fixed walls - min. element size: 0.1 mm - max. element size: 1 mm - viscous sublayer: 5, with 0.8 mm height However, while this simulation runs with RANS in Code_Saturne it diverges after 0.004 s in OpenFoam. I use OpenFoam Version 8 for Ubuntu 20.04. The chosen solver is rhoPimpleFoam. Basically, I adapted the pitzDaily example from compressible/LES/ with my boundaries etc. The simulation starts well but then diverges for some reason. Till now I tried: - decreased the time step from 1e-05 to 1e-07 - set adjustTimeStep to true - set maxCo from 0.4 to 0.25 - reduced the tolerance from 1e-06 to 1e-05 - increased the corrector iteration numbers - set the relaxationFactors from 1 to 0.7 to 0.3 - refined the mesh with Salome After running checkMesh everything seems to be fine despite the skewness: ***Max skewness = 5.47186, 22 highly skew faces detected which may impair the quality of the results <<Writing 22 skew faces to set skewFaces However, I’ve read that those higher values may impair quality (accuracy) of the results, anyway any reasonably high value (<20) of skewness parameter can be used for simulation. So, I continued. I run the simulation in parallel using “decomposePar” with 16 processors “mpirun -np 16 rhoPimpleFoam -parallel > log &” The error message after running OpenFoam is always the same: [8] #1 Foam::sigFpe::sigHandler(int) at ??:? [8] #2 ? in "/lib/x86_64-linux-gnu/libc.so.6" [8] #3 void Foam::fvc::surfaceIntegrate<double>(Foam::Field<do uble>&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/opt/openfoam8/platforms/linux64GccDPInt32Opt/bin/rhoPimpleFoam" [8] #4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::fvc::surfaceIntegrate<double>(Foam::Geometri cField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/opt/openfoam8/platforms/linux64GccDPInt32Opt/bin/rhoPimpleFoam" [8] #5 Foam::fv::gaussConvectionScheme<double>::fvcDiv(Fo am::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const at ??:? [8] #6 ? in "/opt/openfoam8/platforms/linux64GccDPInt32Opt/bin/rhoPimpleFoam" [8] #7 ? in "/opt/openfoam8/platforms/linux64GccDPInt32Opt/bin/rhoPimpleFoam" [8] #8 ? in "/opt/openfoam8/platforms/linux64GccDPInt32Opt/bin/rhoPimpleFoam" [8] #9 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" [8] #10 ? in "/opt/openfoam8/platforms/linux64GccDPInt32Opt/bin/rhoPimpleFoam" [simulationpc-desktop:3665676] *** Process received signal *** [simulationpc-desktop:3665676] Signal: Floating point exception (8) [simulationpc-desktop:3665676] Signal code: (-6) [simulationpc-desktop:3665676] Failing at address: 0x3e80037ef0c [simulationpc-desktop:3665676] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x46210)[0x7f12de0ab210] [simulationpc-desktop:3665676] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0xcb)[0x7f12de0ab18b] [simulationpc-desktop:3665676] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x46210)[0x7f12de0ab210] [simulationpc-desktop:3665676] [ 3] rhoPimpleFoam(_ZN4Foam3fvc16surfaceIntegrateIdEEvR NS_5FieldIT_EERKNS_14GeometricFieldIS3_NS_13fvsPat chFieldENS_11surfaceMeshEEE+0x3aa)[0x56117f1a308a] [simulationpc-desktop:3665676] [ 4] rhoPimpleFoam(_ZN4Foam3fvc16surfaceIntegrateIdEENS _3tmpINS_14GeometricFieldIT_NS_12fvPatchFieldENS_7 volMeshEEEEERKNS3_IS4_NS_13fvsPatchFieldENS_11surf aceMeshEEE+0x1d7)[0x56117f1f0fa7] [simulationpc-desktop:3665676] [ 5] /opt/openfoam8/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZNK4Foam2fv21gaussConvectionSc hemeIdE6fvcDivERKNS_14GeometricFieldIdNS_13fvsPatc hFieldENS_11surfaceMeshEEERKNS3_IdNS_12fvPatchFiel dENS_7volMeshEEE+0x52)[0x7f12e0c77682] [simulationpc-desktop:3665676] [ 6] rhoPimpleFoam(+0x7db51)[0x56117f1d7b51] [simulationpc-desktop:3665676] [ 7] rhoPimpleFoam(+0x7de74)[0x56117f1d7e74] [simulationpc-desktop:3665676] [ 8] rhoPimpleFoam(+0x33cef)[0x56117f18dcef] [simulationpc-desktop:3665676] [ 9] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xf3)[0x7f12de08c0b3] [simulationpc-desktop:3665676] [10] rhoPimpleFoam(+0x38d6e)[0x56117f192d6e] [simulationpc-desktop:3665676] *** End of error message *** -------------------------------------------------------------------------- Primary job terminated normally, but 1 process returned a non-zero exit code. Per user-direction, the job has been aborted. -------------------------------------------------------------------------- -------------------------------------------------------------------------- mpirun noticed that process rank 8 with PID 0 on node simulationpc-desktop exited on signal 8 (Floating point exception). -------------------------------------------------------------------------- I’ve attached two figures. One shows the simulation result and the other the convergence process. As you can see the flow pattern in the upper part looks fine. But where does this singularity in the down left come from? The velocity becomes infinite, the temperature is clipping (limitT is 200 K – 800 K) on both ends. Does anyone have a suggestion for me to overcome these issues? Thank you in advance. Best regards, Chris |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Senior Member
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 931
Rep Power: 12 ![]() |
Hi,
Could you attach the key files of settings, please? i.e. fvSchemes, fvSolution, BCs 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 |
|
![]() |
![]() |
![]() |
![]() |
#3 |
Senior Member
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 744
Rep Power: 15 ![]() |
LES is most demanding on the mesh. Don't even think about running this method with a mesh which gives warnings or errors with checkMesh. BTW: you should use at least 2,5D with LES, but this is only a point of accuracy and not of stability.
I recommend starting with laminar and get it run. You may this result use as a starting point for LES. If this crashes, use k-epsilon or k-omega first and look what happens. If all of these crash probably your physics is wrong.
__________________
Uwe Pilz -- Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950) |
|
![]() |
![]() |
![]() |
![]() |
#4 |
Senior Member
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 931
Rep Power: 12 ![]() |
I kindly disagree. I don't think the stability issues this user faces is related to LES, but compressible solver.
Also, I believe you can run LES models with bad-quality meshes since the LES of max-second-order spatiotemporal accuracy with non-cyclic boundary conditions (hence the commutation error) of OpenFOAM is not the LES the academia talks/knows about. I think the former is just an industrial LES, I would call it. Something better than RANS, but Trump-like in comparison to the actual well-defined well-implemented LES approaches. I also kindly disagree on the initialisation approach if the concern is only the LES model. I prefer hitting the LES right from the beginning - almost always more stable. Yet since I believe the issue is related to the transient compressible solver - the initialisation approach you suggest must be applied, I believe. I am more than happy to be proven incorrect.
__________________
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 |
|
![]() |
![]() |
![]() |
![]() |
#5 |
New Member
Christopher Bruns
Join Date: Jun 2021
Posts: 6
Rep Power: 5 ![]() |
Hi,
thanks's for your answers. Attached you will find the key files. Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application rhoPimpleFoam; startFrom latestTime; startTime 0; stopAt endTime; endTime 0.1; deltaT 1e-06; writeControl timeStep; writeInterval 1000; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression off; timeFormat general; timePrecision 6; runTimeModifiable true; adjustTimeStep yes; maxCo 0.4; functions { #includeFunc fieldAverage(U, p, prime2Mean = yes) } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default backward; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phi,U) Gauss LUST grad(U); div(phi,e) Gauss LUST grad(e); div(phi,K) Gauss linear; div(phiv,p) Gauss linear; div(phi,k) Gauss limitedLinear 1; div(phi,B) Gauss limitedLinear 1; div(phi,muTilda) Gauss limitedLinear 1; div(B) Gauss linear; div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { "(p|rho)" { solver PCG; preconditioner DIC; tolerance 1e-6; // 1e-6 relTol 0.01; } "(p|rho)Final" { $p; relTol 0; } "(U|e|k|nuTilda)" { solver smoothSolver; smoother symGaussSeidel; tolerance 1e-6; // 1e-6 relTol 0.01; } "(U|e|k|nuTilda)Final" { $U; relTol 0; } } PIMPLE { momentumPredictor yes; nOuterCorrectors 3; nCorrectors 1; // 1 nNonOrthogonalCorrectors 0; // 0 pMinFactor 0.5; pMaxFactor 2.0; } relaxationFactors { equations { ".*" 0.3; // 1 } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class polyBoundaryMesh; location "constant/polyMesh"; object boundary; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 5 ( inlet1 { type patch; nFaces 123; startFace 250133; } inlet2 { type patch; nFaces 123; startFace 250256; } outlet { type patch; nFaces 762; startFace 250379; } fixedWalls { type patch; nFaces 1468; startFace 251141; } frontAndBack { type empty; nFaces 330268; startFace 252609; } ) // ************************************************************************* // |
|
![]() |
![]() |
![]() |
![]() |
#6 |
Member
Julian
Join Date: Sep 2019
Posts: 32
Rep Power: 7 ![]() |
Try the Euler time integration scheme instead of backward.
What is your velocity initialization? |
|
![]() |
![]() |
![]() |
![]() |
#7 |
New Member
Christopher Bruns
Join Date: Jun 2021
Posts: 6
Rep Power: 5 ![]() |
Hi,
the initialization of velocity, pressure and temperature is as follows. Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volVectorField; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { inlet1 { type turbulentInlet; referenceField uniform (0 6 0); fluctuationScale (0.05 0.05 0.01); value uniform (0 6 0); } inlet2 { type turbulentInlet; referenceField uniform (0 -6 0); fluctuationScale (0.05 0.05 0.01); value uniform (0 -6 0); } outlet { type pressureInletOutletVelocity; inletValue uniform (0 0 0); value uniform (0 0 0); } fixedWalls { type noSlip; } frontAndBack { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 -1 -2 0 0 0 0]; internalField uniform 1; //1e5 boundaryField { inlet1 { type zeroGradient; } inlet2 { type zeroGradient; } outlet { type waveTransmissive; field p; psi thermo:psi; gamma 1.4; // 1.3 fieldInf 1; // 1e5 lInf 3; // 0.3 value $internalField; } fixedWalls { type zeroGradient; } frontAndBack { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object T; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 0 1 0 0 0]; internalField uniform 300; boundaryField { inlet1 { type fixedValue; value uniform 533; } inlet2 { type fixedValue; value uniform 533; } outlet { type inletOutlet; inletValue uniform 300; value uniform 300; } fixedWalls { type fixedValue; value uniform 300; } frontAndBack { type empty; } } // ************************************************************************* // |
|
![]() |
![]() |
![]() |
![]() |
#8 |
Member
Julian
Join Date: Sep 2019
Posts: 32
Rep Power: 7 ![]() |
Christopher,
Thanks for posting your case setup. I think it looks pretty good. My only suggestion would be to try some small velocity initialization or map a velocity field from for example an incompressible case. I am running some LES for a simple case and had a similar problem. I tried almost everything but it was changing the ddt scheme that resolved the instabilities. The difference is my Mach number is order 0.1. Please let me know if you resolve this. Thanks. |
|
![]() |
![]() |
![]() |
![]() |
#9 |
Senior Member
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 931
Rep Power: 12 ![]() |
Hi Chris,
Few suggestions: - I am almost certain that the instabilities arise from rhoPimpleFoam rather than LES modelling - or are you using a DES? - I kindly disagree with jmt on the temporal scheme. Do not use anything else than "backward" there if you use LES. - Could you attach also the output of "checkMesh -allTopology -allGeometry"? - Please use one of the limiters available in "gradSchemes" for velocity. Please search for "cellMDLimited" for the options. You have freedom not to apply limiters on other variables, and even so, please avoid limiters on "p" there. - LUST is a good choice for U in DES. If you use LES, please consider other options, e.g. linearUpwind. - Use "nNonOrthogonalCorrectors" at least 1. If the max non-orthogonality is severe, please consider to increase this number or regenerate the mesh. - Use the freestream value for the velocity's "internalField uniform (0 0 0);" rather than a zero field. - I am not sure if you intentionally set "turbulentInlet" boundary condition for velocity. If you aim to generate turbulent fluctuations, I am sad to inform you that "turbulentInlet" condition has a misleading name - it only generates random fluctuations. For synthetic turbulence, try to use "turbulentDFSEMInlet" or "turbulentDigitalFilterInlet" conditions. - Be careful with the pressure value in "rhoPimpleFoam" - it is the absolute pressure: so, "uniform 1; //1e5" is absolutely wrong. Set it to a freestream pressure value. - And this one is the key: for "rhoPimpleFoam", use limitTemperature and/or limitVelocity fvOptions. If you would be pissed of by stability problems despite these, just switch to the package HiSAFoam. ![]() Hope these help a bit.
__________________
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 |
|
![]() |
![]() |
![]() |
![]() |
#10 |
New Member
Christopher Bruns
Join Date: Jun 2021
Posts: 6
Rep Power: 5 ![]() |
Hi guys,
thank you very much for your suggestions. It is highly appreciated ![]() jmt, I've tried to use other schemes than "backward", e.g euler and crank nicolson. The simulation finished using both, but the physics was completely wrong. The flow starts correctly, but than stagnates after two or three iterations until finished. HPE, I am using LES. Attached you will find the log files from checkMesh. First I was using viscous boundary layer on my mesh which caused the skewness error (see log.checkMesh_vsl). Now, I deleted the boundary layer and employed a local mesh refinement on the fixedWalls. After running checkMesh, it says "Mesh OK". However, after running "checkMesh -allTopology -allGeometry", there is still an error called "Cells with small determinant". With viscous sublayer: Code:
/*---------------------------------------------------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ Build : 8-1c9b5879390b Exec : checkMesh -allTopology -allGeometry Date : Jul 02 2021 Time : 08:38:28 Host : "simulationpc-desktop" PID : 1626716 I/O : uncollated Case : /home/simulation-pc/OpenFOAM/simulation-pc-8/run/Exxon_Test2 nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10) allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 Enabling all (cell, face, edge, point) topology checks. Enabling all geometry checks. Time = 0 Mesh stats points: 196818 internal points: 0 edges: 659271 internal edges: 94644 internal edges using one boundary point: 0 internal edges using two boundary points: 94644 faces: 644477 internal faces: 276666 cells: 182023 faces per cell: 5.06059 boundary patches: 5 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 11028 prisms: 170995 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. <<Writing 2 cells with zero or one non-boundary face to set oneInternalFaceCells <<Writing 986 cells with two non-boundary faces to set twoInternalFacesCells Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology Bounding box inlet1 123 248 ok (non-closed singly connected) (-0.1262 -0.195998 0) (-0.0542 -0.16 0.001) inlet2 123 248 ok (non-closed singly connected) (-0.1262 0.16 0) (-0.0542 0.195998 0.001) outlet 762 1526 ok (non-closed singly connected) (0.0038 -0.1261 0) (0.2538 0.1261 0.001) frontAndBack 364046 196818 ok (non-closed singly connected) (-0.1262 -0.195998 -4.33681e-19) (0.2538 0.195998 0.001) fixedWalls 2757 5520 ok (non-closed singly connected) (-0.1262 -0.16 0) (0.0038 0.16 0.001) Checking geometry... Overall domain bounding box (-0.1262 -0.195998 -4.33681e-19) (0.2538 0.195998 0.001) Mesh has 2 geometric (non-empty/wedge) directions (1 1 0) Mesh has 2 solution (non-empty) directions (1 1 0) All edges aligned with or perpendicular to non-empty directions. Boundary openness (-4.7753e-19 -8.74247e-19 -1.20688e-13) OK. Max cell openness = 7.62907e-16 OK. Max aspect ratio = 25.9353 OK. Minimum face area = 1.15747e-08. Maximum face area = 1.74641e-06. Face area magnitudes OK. Min volume = 1.15747e-11. Max volume = 9.89927e-10. Total volume = 7.08515e-05. Cell volumes OK. Mesh non-orthogonality Max: 66.3308 average: 6.61413 Non-orthogonality check OK. Face pyramids OK. ***Max skewness = 4.32878, 13 highly skew faces detected which may impair the quality of the results <<Writing 13 skew faces to set skewFaces Coupled point location match (average 0) OK. Face tets OK. Min/max edge length = 2.31635e-05 0.00174641 OK. All angles in faces OK. Face flatness (1 = flat, 0 = butterfly) : min = 1 average = 1 All face flatness OK. Cell determinant (wellposedness) : minimum: 2.77556e-17 average: 2.16694 ***Cells with small determinant (< 0.001) found, number of cells: 2 <<Writing 2 under-determined cells to set underdeterminedCells Concave cell check OK. Face interpolation weight : minimum: 0.12137 average: 0.489786 Face interpolation weight check OK. Face volume ratio : minimum: 0.184169 average: 0.965087 Face volume ratio check OK. Failed 2 mesh checks. End Code:
/*---------------------------------------------------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ Build : 8-1c9b5879390b Exec : checkMesh -allTopology -allGeometry Date : Jul 02 2021 Time : 08:41:09 Host : "simulationpc-desktop" PID : 1632827 I/O : uncollated Case : /home/simulation-pc/OpenFOAM/simulation-pc-8/run/Exxon_Test2 nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10) allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 Enabling all (cell, face, edge, point) topology checks. Enabling all geometry checks. Time = 0 Mesh stats points: 207112 internal points: 0 edges: 714094 internal edges: 98160 internal edges using one boundary point: 0 internal edges using two boundary points: 98160 faces: 708697 internal faces: 299873 cells: 201714 faces per cell: 5 boundary patches: 5 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 0 prisms: 201714 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. <<Writing 20 cells with zero or one non-boundary face to set oneInternalFaceCells <<Writing 5356 cells with two non-boundary faces to set twoInternalFacesCells Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology Bounding box inlet1 119 240 ok (non-closed singly connected) (-0.1262 -0.195999 0) (-0.0542 -0.16 0.001) inlet2 120 242 ok (non-closed singly connected) (-0.1262 0.16 0) (-0.0542 0.195999 0.001) outlet 758 1518 ok (non-closed singly connected) (0.0038 -0.1261 0) (0.2538 0.1261 0.001) frontAndBack 403428 207112 ok (non-closed singly connected) (-0.1262 -0.195999 -4.33681e-19) (0.2538 0.195999 0.001) fixedWalls 4399 8804 ok (non-closed singly connected) (-0.1262 -0.16 0) (0.0038 0.16 0.001) Checking geometry... Overall domain bounding box (-0.1262 -0.195999 -4.33681e-19) (0.2538 0.195999 0.001) Mesh has 3 geometric (non-empty/wedge) directions (1 1 1) Mesh has 3 solution (non-empty) directions (1 1 1) Boundary openness (-1.38336e-18 -1.736e-18 1.49222e-13) OK. Max cell openness = 3.17955e-16 OK. Max aspect ratio = 10.2619 OK. Minimum face area = 3.11904e-08. Maximum face area = 1.67746e-06. Face area magnitudes OK. Min volume = 3.11904e-11. Max volume = 9.96512e-10. Total volume = 7.08517e-05. Cell volumes OK. Mesh non-orthogonality Max: 27.9673 average: 4.49526 Non-orthogonality check OK. Face pyramids OK. Max skewness = 0.401073 OK. Coupled point location match (average 0) OK. Face tets OK. Min/max edge length = 0.000216828 0.00167746 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 average: 2.46539e-34 ***Cells with small determinant (< 0.001) found, number of cells: 201714 <<Writing 201714 under-determined cells to set underdeterminedCells Concave cell check OK. Face interpolation weight : minimum: 0.322135 average: 0.490414 Face interpolation weight check OK. Face volume ratio : minimum: 0.47522 average: 0.964455 Face volume ratio check OK. Failed 1 mesh checks. End Maybe I initialized my physics incorrectly? I have a pressure of 1.25e5 Pa, a mass flow of 0.001 kg/s or velocity of 6 m/s and a temperature of 533 K at both inlets. Atmospheric pressure (1e5 Pa) and ambient temperature (300 K) at the outlet. No heat transfer to the walls. Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 -1 -2 0 0 0 0]; internalField uniform 100000; boundaryField { inlet1 { type freestreamPressure; freestreamValue uniform 125000; } inlet2 { type freestreamPressure; freestreamValue uniform 125000; } outlet { type waveTransmissive; field p; psi thermo:psi; gamma 1.4; // 1.3 fieldInf 100000; // 1e5 lInf 0.3; // 0.3 value $internalField; } fixedWalls { type zeroGradient; } frontAndBack { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volVectorField; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { inlet1 { type flowRateInletVelocity; massFlowRate 0.001; //mass flow rate [kg/s] value uniform (0 0 0); } inlet2 { type flowRateInletVelocity; massFlowRate 0.001; //mass flow rate [kg/s] value uniform (0 0 0); } outlet { type pressureInletOutletVelocity; inletValue uniform (0 0 0); value uniform (0 0 0); } fixedWalls { type noSlip; } frontAndBack { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object T; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 0 1 0 0 0]; internalField uniform 300; boundaryField { inlet1 { type fixedValue; value uniform 533; } inlet2 { type fixedValue; value uniform 533; } outlet { type inletOutlet; inletValue uniform 300; value uniform 300; } fixedWalls { type fixedValue; value uniform 300; } frontAndBack { type empty; } } // ************************************************************************* // |
|
![]() |
![]() |
![]() |
![]() |
#11 |
New Member
Christopher Bruns
Join Date: Jun 2021
Posts: 6
Rep Power: 5 ![]() |
Hello,
I have now tried your suggestions HPE. The simulation runs further than in the past. But no matter what I do, I always get these artifacts in the left and right corner below the free beam area. I have attached two images with U and UMean. Am I choosing the wrong output boundary condition? CheckMesh says Mesh OK. I took the same physical parameters that already worked with code_saturne in a RANS model. My mesh size is 1/10 mm to 1 mm. That should be ok for LES, right? With kind regards, Chris |
|
![]() |
![]() |
![]() |
![]() |
#12 |
Senior Member
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 744
Rep Power: 15 ![]() |
To see what happens I recommend to add glyphes. May be you have re-entering flow at output boundaries.
__________________
Uwe Pilz -- Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950) |
|
![]() |
![]() |
![]() |
![]() |
#13 | |
Member
Julian
Join Date: Sep 2019
Posts: 32
Rep Power: 7 ![]() |
Quote:
internalField uniform (0.1 0 0); This supplies an initial U_x of 0.1 m/s. Not sure if that's what HPE had in mind but I have also had trouble when starting a simulation with a zero initial velocity internal field. What solved my problem was mapping the developed flow field from a previous compressible simulation. |
||
![]() |
![]() |
![]() |
![]() |
#14 |
New Member
Christopher Bruns
Join Date: Jun 2021
Posts: 6
Rep Power: 5 ![]() |
Alright, I've already looked at the glyphes in Paraview.
And indeed, I need an inlet/outlet, because on the real system there are two vortexes left and right to the vertical freestream below the nozzle. This means that hot air streams out of the nozzle and entrains the surrounding cold air. Therefore, I have to face an air stream coming in from left and right in the upper part of the freestream area and an air stream streaming out in the lower part. Right now there is just chaos. Some glyphes point outwards some inwards randomly. jmt, thank you for your advice. However, I have a multi inlet (the two semicircles) single outlet (all faces in the freestream area) problem. The two inlets point in x and -x direction. So if I choose "internalField uniform (0.1 0 0);", I initialize a vector field that points in the wrong direction for one inlet. Or am I wrong? I guess there is something wrong with the outlet boundaries. I've got U: Code:
outlet { type pressureInletOutletVelocity; tangentialVelocity uniform (0 0 0); value uniform (0 0 0); } T (previously inletOutlet): Code:
outlet { type totalTemperature; gamma 1.4; T0 uniform 300; } p(previously waveTransmissive): Code:
outlet { type fixedValue; value 100000; } However, maybe I should try the mapping from a previous compressible RANS simulation to make a better initial guess for the solution. Thank you and kind regards, Chris |
|
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Problem with the running of compressible homogeneousDynOneEqEddy LES modle | Yupeng Qin | OpenFOAM Running, Solving & CFD | 3 | March 7, 2016 10:29 |
Divergence with Simulation using Embedded LES | CarlosGRR | FLUENT | 3 | October 2, 2014 17:52 |
Implementing DSM in compressible LES code | LES-newbie | Main CFD Forum | 0 | February 20, 2013 12:26 |
Compressible LES, yPlusLES problem. | fgal | OpenFOAM Post-Processing | 0 | June 3, 2010 10:02 |
LES NITA giving divergence problems | anindya | FLUENT | 0 | June 20, 2005 07:23 |