[Eloise]

Hello Foamers,

I am working on the layer addition phase for a complex snappyHexMesh (sHM) mesh. I encountered a crash of sHM with the error message:

#1  Foam::sigFpe::sigHandler(int) in  "/share/apps/OpenFOAM-2.2.2//OpenFOAM-2.2.2/platforms/linux64Gcc46DPOpt/lib/libOpenFOAM.so"

which I overcame by unsetting FOAM_SIGFPE before generating my mesh.

Now that sHM runs until the end, I get a mesh with layers but it's quality is not sufficient. As shown by checkMesh output, I have some cells with minimum volume of magnitude e-300:

Checking geometry...
    Overall domain bounding box (-140 -140 -300) (140 140 0.000368027)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (-nan nan -nan) OK.
    Max cell openness = 6.65112e-16 OK.
    Max aspect ratio = 24.5205 OK.
    Minimum face area = 3.61586e-06. Maximum face area = 149.753.  Face area magnitudes OK.
    Min volume = 1.66667e-300. Max volume = 518.268.  Total volume = 1.83588e+07.  Cell volumes OK.
    Mesh non-orthogonality Max: 64.9964 average: -nan
    Non-orthogonality check OK.
    Face pyramids OK.
 ***Max skewness = 49.8663, 6557 highly skew faces detected which may impair the quality of the results
  <<Writing 6557 skew faces to set skewFaces
    Coupled point location match (average 0) OK.

Failed 1 mesh checks.

I run sHM layer phase with the following relaxed mesh quality:

    relaxed
    {
    maxNonOrtho 65; 
      maxBoundarySkewness -1; 
      maxInternalSkewness -1;
      maxConcave 180;
      minVol 1e-6;
        minArea 1e-6;
      minTetQuality -1e30; 
      minTwist -1e30;
      minDeterminant -1; 
      minFaceWeight -1;
    }

But at the end of sHM, I see in the output that 153 cells still don't respect the minimum volume criteria:

[...]
Setting up information for layer truncation ...

Checking mesh with layer ...
Checking faces in error :
    non-orthogonality > 65  degrees                        : 0
    faces with face pyramid volume < 1e-06                 : 153
    faces with area < 1e-06 m^2                            : 0
Detected 153 illegal faces (concave, zero area or negative cell pyramid volume)
Extruding 125954 out of 128858 faces (97.7%). Removed extrusion at 0 faces.
Added 125954 out of 128858 cells (97.7%).
Edge intersection testing:
    Number of edges             : 29892999
    Number of edges to retest   : 0
    Number of intersected edges : 2258776

Doing final balancing
---------------------

Writing 125954 added cells to cellSet addedCells
Writing 0 faces inside added layer to faceSet layerFaces
Layer mesh : cells:8664071  faces:29892999  points:12677767
Cells per refinement level:
    0    8664071
Writing mesh to time 3
Wrote mesh in = 346 s.
Layers added in = 346 s.
Finished meshing in = 391 s.
End

My questions are:
1. I would like to know where are the problematic faces/cells but checkMesh does not isolate them in a face or cell set. How can I create a set of cells which have a volume lower than 1e-6?
2. Which quality criteria or sHM criteria will force the cells volume to be above 1e-6?

Thanks for reading me
Regards,
Eloïse

[wyldckat]

Greetings Eloïse,

I have to say I found your post by accident, while searching for a very similar question.

The solution in your case is theoretically something like this:

1. Use the function object "writeRegisteredObject": http://openfoamwiki.net/index.php/Ti...gisteredObject - to write the field "V" which is the cell volume field.
2. I think you can use the utility writeCellCentres to trigger the usage of this function object. This way you also get a field with the cell centres, which could come in handy...
3. Then use setSet or topoSet to use the "fieldToSet" (found this explanation here: http://www.cfd-online.com/Forums/ope...tml#post431107). Additional details:
   • http://openfoamwiki.net/index.php/TopoSet
   • http://openfoamwiki.net/index.php/SetSet

Best regards,
Bruno