|
[Sponsors] |
[snappyHexMesh] Number of cells in mesh don't match with size of cellLevel |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
September 24, 2010, 02:37 |
Number of cells in mesh don't match with size of cellLevel
|
#1 |
Senior Member
Join Date: Aug 2010
Location: Groningen, The Netherlands
Posts: 216
Rep Power: 19 |
Hi Foamers,
I encountered an other error message which I couldn't get rid of (note that I deleted the header) Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Read mesh in = 17.04 s Overall mesh bounding box : (-185.25 0 -110.5) (185.25 247 6.5) Relative tolerance : 1e-06 Absolute matching distance : 0.0004604 Reading refinement surfaces. Read refinement surfaces in = 0.07 s Reading refinement shells. Refinement level 4 for all cells inside refinementBox Read refinement shells in = 0 s Setting refinement level of surface to be consistent with shells. Checked shell refinement in = 0 s Determining initial surface intersections ----------------------------------------- --> FOAM FATAL ERROR: Number of cells in mesh:1319790 does not equal size of cellLevel:1487102 This might be because of a restart with inconsistent cellLevel. From function hexRef8::getLevel0EdgeLength() const in file polyTopoChange/polyTopoChange/hexRef8.C at line 357. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::error::abort() in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Foam::hexRef8::getLevel0EdgeLength() const in "/opt/openfoam171/lib/linuxGccDPOpt/libdynamicMesh.so" #3 Foam::hexRef8::hexRef8(Foam::polyMesh const&, Foam::List<int> const&, Foam::List<int> const&, Foam::refinementHistory const&) in "/opt/openfoam171/lib/linuxGccDPOpt/libdynamicMesh.so" #4 Foam::meshRefinement::meshRefinement(Foam::fvMesh&, double, bool, Foam::refinementSurfaces const&, Foam::shellSurfaces const&) in "/opt/openfoam171/lib/linuxGccDPOpt/libautoMesh.so" #5 in "/opt/openfoam171/applications/bin/linuxGccDPOpt/snappyHexMesh" #6 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6" #7 in "/opt/openfoam171/applications/bin/linuxGccDPOpt/snappyHexMesh" Aborted According to further comparison of execution times the failure must be somwhere during the refinement but I couldn't figure out where. For complementation here the snappyHexMeshDict file (also without header): Code:
// Which of the steps to run castellatedMesh true; snap true; addLayers true; // Geometry. Definition of all surfaces. All surfaces are of class // searchableSurface. // Surfaces are used // - to specify refinement for any mesh cell intersecting it // - to specify refinement for any mesh cell inside/outside/near // - to 'snap' the mesh boundary to the surface geometry { kishinev.stl { type triSurfaceMesh; name kishinev; } refinementBox { type searchableBox; min (-5 0 -10); max (140 30 6.5); } }; // Settings for the castellatedMesh generation. castellatedMeshControls { // Refinement parameters // ~~~~~~~~~~~~~~~~~~~~~ // If local number of cells is >= maxLocalCells on any processor // switches from from refinement followed by balancing // (current method) to (weighted) balancing before refinement. maxLocalCells 10000000; // Overall cell limit (approximately). Refinement will stop immediately // upon reaching this number so a refinement level might not complete. // Note that this is the number of cells before removing the part which // is not 'visible' from the keepPoint. The final number of cells might // actually be a lot less. maxGlobalCells 60000000; // The surface refinement loop might spend lots of iterations refining just a // few cells. This setting will cause refinement to stop if <= minimumRefine // are selected for refinement. Note: it will at least do one iteration // (unless the number of cells to refine is 0) minRefinementCells 10; // Allow a certain level of imbalance during refining // (since balancing is quite expensive) // Expressed as fraction of perfect balance (= overall number of cells / // nProcs). 0=balance always. maxLoadUnbalance 0.10; // Number of buffer layers between different levels. // 1 means normal 2:1 refinement restriction, larger means slower // refinement. nCellsBetweenLevels 3; // Explicit feature edge refinement // ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~ // Specifies a level for any cell intersected by its edges. // This is a featureEdgeMesh, read from constant/triSurface for now. features ( //{ // file "someLine.eMesh"; // level 2; //} ); // Surface based refinement // ~~~~~~~~~~~~~~~~~~~~~~~~ // Specifies two levels for every surface. The first is the minimum level, // every cell intersecting a surface gets refined up to the minimum level. // The second level is the maximum level. Cells that 'see' multiple // intersections where the intersections make an // angle > resolveFeatureAngle get refined up to the maximum level. refinementSurfaces { kishinev { // Surface-wise min and max refinement level level (2 3); // 3 4 } } // Resolve sharp angles resolveFeatureAngle 30; // Region-wise refinement // ~~~~~~~~~~~~~~~~~~~~~~ // Specifies refinement level for cells in relation to a surface. One of // three modes // - distance. 'levels' specifies per distance to the surface the // wanted refinement level. The distances need to be specified in // descending order. // - inside. 'levels' is only one entry and only the level is used. All // cells inside the surface get refined up to the level. The surface // needs to be closed for this to be possible. // - outside. Same but cells outside. refinementRegions { refinementBox { mode inside; levels ((1E12 4)); // 1E15 4 } } // Mesh selection // ~~~~~~~~~~~~~~ // After refinement patches get added for all refinementSurfaces and // all cells intersecting the surfaces get put into these patches. The // section reachable from the locationInMesh is kept. // NOTE: This point should never be on a face, always inside a cell, even // after refinement. locationInMesh (75 0 0.1); } // Settings for the snapping. snapControls { //- Number of patch smoothing iterations before finding correspondence // to surface nSmoothPatch 3; //- Relative distance for points to be attracted by surface feature point // or edge. True distance is this factor times local // maximum edge length. tolerance 4.0; //- Number of mesh displacement relaxation iterations. nSolveIter 30; //- Maximum number of snapping relaxation iterations. Should stop // before upon reaching a correct mesh. nRelaxIter 5; } // Settings for the layer addition. addLayersControls { // Are the thickness parameters below relative to the undistorted // size of the refined cell outside layer (true) or absolute sizes (false). relativeSizes true; // Per final patch (so not geometry!) the layer information layers { solid { nSurfaceLayers 1; } } // Expansion factor for layer mesh expansionRatio 1.0; //- Wanted thickness of final added cell layer. If multiple layers // is the thickness of the layer furthest away from the wall. // See relativeSizes parameter. finalLayerThickness 0.3; //- Minimum thickness of cell layer. If for any reason layer // cannot be above minThickness do not add layer. // Relative to undistorted size of cell outside layer. minThickness 0.1; //- If points get not extruded do nGrow layers of connected faces that are // also not grown. This helps convergence of the layer addition process // close to features. nGrow 1; // Advanced settings //- When not to extrude surface. 0 is flat surface, 90 is when two faces // make straight angle. featureAngle 30; //- Maximum number of snapping relaxation iterations. Should stop // before upon reaching a correct mesh. nRelaxIter 3; // Number of smoothing iterations of surface normals nSmoothSurfaceNormals 1; // Number of smoothing iterations of interior mesh movement direction nSmoothNormals 3; // Smooth layer thickness over surface patches nSmoothThickness 10; // Stop layer growth on highly warped cells maxFaceThicknessRatio 0.5; // Reduce layer growth where ratio thickness to medial // distance is large maxThicknessToMedialRatio 0.3; // Angle used to pick up medial axis points minMedianAxisAngle 130; // Create buffer region for new layer terminations nBufferCellsNoExtrude 0; // Overall max number of layer addition iterations nLayerIter 50; } // Generic mesh quality settings. At any undoable phase these determine // where to undo. meshQualityControls { //- Maximum non-orthogonality allowed. Set to 180 to disable. maxNonOrtho 65; //- Max skewness allowed. Set to <0 to disable. maxBoundarySkewness 20; maxInternalSkewness 4; //- Max concaveness allowed. Is angle (in degrees) below which concavity // is allowed. 0 is straight face, <0 would be convex face. // Set to 180 to disable. maxConcave 80; //- Minimum projected area v.s. actual area. Set to -1 to disable. minFlatness 0.5; //- Minimum pyramid volume. Is absolute volume of cell pyramid. // Set to a sensible fraction of the smallest cell volume expected. // Set to very negative number (e.g. -1E30) to disable. minVol 1e-13; //- Minimum face area. Set to <0 to disable. minArea -1; //- Minimum face twist. Set to <-1 to disable. dot product of face normal //- and face centre triangles normal minTwist 0.02; //- minimum normalised cell determinant //- 1 = hex, <= 0 = folded or flattened illegal cell minDeterminant 0.001; //- minFaceWeight (0 -> 0.5) minFaceWeight 0.02; //- minVolRatio (0 -> 1) minVolRatio 0.01; //must be >0 for Fluent compatibility minTriangleTwist -1; // Advanced //- Number of error distribution iterations nSmoothScale 4; //- amount to scale back displacement at error points errorReduction 0.75; } // Advanced // Flags for optional output // 0 : only write final meshes // 1 : write intermediate meshes // 2 : write volScalarField with cellLevel for postprocessing // 4 : write current intersections as .obj files debug 0; // Merge tolerance. Is fraction of overall bounding box of initial mesh. // Note: the write tolerance needs to be higher than this. mergeTolerance 1E-6; Thanks for your trouble regards Colin |
|
September 24, 2010, 09:22 |
|
#2 |
Senior Member
Join Date: Mar 2009
Location: My oyster
Posts: 124
Rep Power: 17 |
Either remove the 1/ 2/ 3/ folders before you run again or implement the following settings in controlDict:
startFrom startTime; startTime 0; |
|
September 24, 2010, 10:06 |
|
#3 |
Senior Member
Join Date: Aug 2010
Location: Groningen, The Netherlands
Posts: 216
Rep Power: 19 |
Hi ziad,
unfortunately this seems to be not the problem for I don't have any 1/ 2/ 3/ folders and the starting time is already set to 0 too. However the case directory is indeed copied from an other case and contains some data from the original one. Could it be that I have to look for an other file/ folder that I have to change before I can run sHM? However thanks for your help ziad, I appreciate it. regards Colin |
|
September 24, 2010, 10:18 |
|
#4 |
Senior Member
Join Date: Mar 2009
Location: My oyster
Posts: 124
Rep Power: 17 |
Yeah that could be it. It helps to have your settings and cases in order anyway.
Do the blockMeshDict and snappyHexMeshDict correspond to each other? |
|
September 24, 2010, 10:29 |
|
#5 |
Senior Member
Join Date: Mar 2009
Location: My oyster
Posts: 124
Rep Power: 17 |
you also have pretty huge numbers in your original error message. Number of cells in mesh is 1319790 and cellLevel 1487102.
Is your original starting mesh already developed? If so delete it and reset blockMeshDict to give you the simplest possible mesh without any geometry detail inside. sHM takes care of that. It's explained very clearly in the user's guide. |
|
October 1, 2010, 06:30 |
|
#6 |
Senior Member
Join Date: Aug 2010
Location: Groningen, The Netherlands
Posts: 216
Rep Power: 19 |
Hi Ziad,
thanks again for your help, also for the hint with the user guide. Finally I managed to get rid of that error message. I just forgot to replace my alpha1 file by a new copy of my alpha1.org file and after doing so everything worked out fine. The number of cells is indeed very big, but this has something to do with the domain size which is also very big (somewhat about 4-5 mio m^3). best regards Colin |
|
October 1, 2010, 08:27 |
|
#7 |
Senior Member
Join Date: Mar 2009
Location: My oyster
Posts: 124
Rep Power: 17 |
Glad it worked out.
Enjoy! |
|
March 22, 2011, 00:26 |
|
#8 |
Member
Paul Reichl
Join Date: Feb 2010
Location: Melbourne, Victoria, Australia
Posts: 33
Rep Power: 16 |
I have also seen this before. Getting rid of the constant/polyMesh/refinementHistory file seemed to fix this for me.
|
|
November 2, 2011, 02:50 |
|
#10 |
Senior Member
Join Date: Aug 2010
Location: Groningen, The Netherlands
Posts: 216
Rep Power: 19 |
this has to do with the way OF saves the mesh. usually intermediate steps are stored in the 1 and 2 folder and the final mesh in the 3 folder as far as I understood. so when you open paraview you can click through the timeline and see different meshes from 0 to 3.
To supress this you have to type: snappyHexMesh -overwrite instead of only snappyHexMesh hope that helps regards Colin |
|
May 29, 2014, 11:49 |
|
#11 |
Senior Member
|
For anyone still struggling with such a problem, I solved mine by removing the 0 directory which was already containing data from a refined mesh.
Hope this can help. -Louis |
|
January 13, 2015, 11:47 |
|
#12 |
Member
Join Date: Dec 2012
Posts: 81
Rep Power: 13 |
hi,
I have the same error message when using sHM. I already tried the tips posted here but it is still not running :-( I have to say that Im new to OpenFOAM so it might be a really stupid mistake. Thank you very much in advance for your help -> FOAM FATAL ERROR: Number of cells in mesh:512000 does not equal size of cellLevel:5829368 This might be because of a restart with inconsistent cellLevel. From function hexRef8::getLevel0EdgeLength() const in file polyTopoChange/polyTopoChange/hexRef8.C at line 358. FOAM aborting #0 Foam::error:rintStack(Foam::Ostream&) at ??:? #1 Foam::error::abort() at ??:? #2 Foam::hexRef8::getLevel0EdgeLength() const at ??:? #3 Foam::hexRef8::hexRef8(Foam:olyMesh const&, bool) at ??:? #4 Foam::meshRefinement::meshRefinement(Foam::fvMesh& , double, bool, Foam::refinementSurfaces const&, Foam::refinementFeatures const&, Foam::shellSurfaces const&) at ??:? #5 at ??:? #6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #7 at ??:? Aborted (core dumped) I used the motorbike sHMDict file and changed it were needed (well at least the stl names). It now looks like this: /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.3.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object snappyHexMeshDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // // Which of the steps to run castellatedMesh true; snap true; addLayers false; geometry { UCAV.stl { type triSurfaceMesh; name UCAV; } // refinementBox // { // type searchableBox; // min (-1.0 -0.7 0.0); // max ( 8.0 0.7 2.5); // } }; // Settings for the castellatedMesh generation. castellatedMeshControls { // Refinement parameters // ~~~~~~~~~~~~~~~~~~~~~ maxLocalCells 100000; maxGlobalCells 2000000; minRefinementCells 10; maxLoadUnbalance 0.10; nCellsBetweenLevels 3; // Explicit feature edge refinement // ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~ features ( { file "UCAV.eMesh"; level 6; } ); // Surface based refinement // ~~~~~~~~~~~~~~~~~~~~~~~~ refinementSurfaces { motorBike { level (5 6); patchInfo { type wall; inGroups (motorBikeGroup); } } } // Resolve sharp angles resolveFeatureAngle 30; // Region-wise refinement // ~~~~~~~~~~~~~~~~~~~~~~ refinementRegions { refinementBox { mode inside; levels ((1E15 4)); } } // Mesh selection // ~~~~~~~~~~~~~~ locationInMesh (0 0 0); allowFreeStandingZoneFaces true; } // Settings for the snapping. snapControls { nSmoothPatch 3; / tolerance 2.0; nSolveIter 30; nRelaxIter 5; // Feature snapping nFeatureSnapIter 10; implicitFeatureSnap false; explicitFeatureSnap true; multiRegionFeatureSnap false; } // Settings for the layer addition. addLayersControls { relativeSizes true; layers { "(lowerWall|motorBike).*" { nSurfaceLayers 1; } } expansionRatio 1.0; finalLayerThickness 0.3; minThickness 0.1; nGrow 0; // Advanced settings featureAngle 60; slipFeatureAngle 30; nRelaxIter 3; nSmoothSurfaceNormals 1; nSmoothNormals 3; nSmoothThickness 10; maxFaceThicknessRatio 0.5; maxThicknessToMedialRatio 0.3; minMedianAxisAngle 90; nBufferCellsNoExtrude 0; nLayerIter 50; } meshQualityControls { #include "meshQualityDict" // Advanced nSmoothScale 4; errorReduction 0.75; } // Advanced / writeFlags ( layerFields ); mergeTolerance 1e-6; |
|
March 31, 2017, 23:12 |
did you solve this problem?
|
#13 |
New Member
Manuel Fermin Fonseca
Join Date: Nov 2014
Location: Valencia, Venezuela
Posts: 18
Rep Power: 11 |
did you solve this problem? i have the same problem with my OF 2.1 and the flange tutorial
|
|
July 4, 2017, 16:27 |
|
#14 |
New Member
Alwin
Join Date: Jun 2017
Posts: 11
Rep Power: 9 |
Sorry for updating this old thread, but I thought I might share my solution.
I had the same problem and deleted the folder "polyMesh" in /constant - now it works. I was using the case folder from an earlier project, that's probably why. |
|
December 12, 2018, 08:07 |
Solved
|
#15 |
Member
Akshay Patil
Join Date: Nov 2015
Location: Pune, India
Posts: 35
Rep Power: 10 |
Deleting the polyMesh directory solves the problem. There are some references ( Like the files celllevel, pointLevel etc. ) made about the mesh which do not hold when you re-run snappyHexMesh.
|
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Decomposing meshes | Tobi | OpenFOAM Pre-Processing | 22 | February 24, 2023 09:23 |
[snappyHexMesh] Help with Snappy: no layers growing | GianF | OpenFOAM Meshing & Mesh Conversion | 2 | September 23, 2020 08:26 |
parallel run OpenFoam | Srinath Reddy | OpenFOAM Running, Solving & CFD | 13 | February 27, 2019 09:15 |
[snappyHexMesh] crash sHM | H25E | OpenFOAM Meshing & Mesh Conversion | 11 | November 10, 2014 11:27 |
[Netgen] Import netgen mesh to OpenFOAM | hsieh | OpenFOAM Meshing & Mesh Conversion | 32 | September 13, 2011 05:50 |