[s.m]

hi
when i run the "checkMesh" utility, it doen't complain anything, but when i execute "checkMesh -allGeometry -allTopology" it complains from concave cells, and report 1 failed mesh,
i put the report of checkMesh & checkMesh -allGeometry -allTopology and also some pics from my mesh in the following,
my question is, how can i improve my mesh to remove these concave cells from my mesh to have a good mesh?

Thanks in advance for any suggestion
""1. checkMesh""

 Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           206578
    internal points:  0
    faces:            403232
    internal faces:   199837
    cells:            99981
    faces per cell:   6.03184
    boundary patches: 6
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     96539
    prisms:        301
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     3141
    Breakdown of polyhedra by number of faces:
        faces   number of cells
            7   2798
            8   343

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
                   Patch    Faces   Points                  Surface topology
            topAndBottom      496      996  ok (non-closed singly connected)
                   inlet      176      354  ok (non-closed singly connected)
                  outlet      176      354  ok (non-closed singly connected)
                   front    99981   103289  ok (non-closed singly connected)
                    back    99981   103289  ok (non-closed singly connected)
               airfoil_solid     2585     5170  ok (non-closed singly connected)

Checking geometry...
    Overall domain bounding box (-5.97801 -11.4978 0.15) (21.0301 9.38239 0.25)
    Mesh (non-empty, non-wedge) directions (1 1 0)
    Mesh (non-empty) directions (1 1 0)
    All edges aligned with or perpendicular to non-empty directions.
    Boundary openness (1.33896e-18 5.41191e-21 3.12079e-14) OK.
    Max cell openness = 2.16716e-16 OK.
    Max aspect ratio = 2.51791 OK.
    Minimum face area = 2.51612e-07. Maximum face area = 0.0100472.  Face area magnitudes OK.
    Min volume = 2.51612e-08. Max volume = 0.00100472.  Total volume = 43.6397.  Cell volumes OK.
    Mesh non-orthogonality Max: 30.6861 average: 3.70862
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 1.17932 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

""2. checkMesh -allGeometry -allTopology ""

Create time

Create polyMesh for time = 0

Enabling all (cell, face, edge, point) topology checks.

Enabling all geometry checks.

Time = 0

Mesh stats
    points:           206578
    internal points:  0
    edges:            509829
    internal edges:   99856
    internal edges using one boundary point:   0
    internal edges using two boundary points:  99856
    faces:            403232
    internal faces:   199837
    cells:            99981                                                                                                                                                                     
    faces per cell:   6.03184                                                                                                                                                                   
    boundary patches: 6                                                                                                                                                                         
    point zones:      0                                                                                                                                                                         
    face zones:       0                                                                                                                                                                         
    cell zones:       0                                                                                                                                                                         
                                                                                                                                                                                                
Overall number of cells of each type:
    hexahedra:     96539
    prisms:        301
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     3141
    Breakdown of polyhedra by number of faces:
        faces   number of cells
            7   2798
            8   343

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 4 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
            topAndBottom      496      996  ok (non-closed singly connected) (-5.97801 -11.4978 0.15) (21.0301 9.38239 0.25)
                   inlet      176      354  ok (non-closed singly connected) (-5.97801 -8.04633 0.15) (-3.52856 9.38239 0.25)
                  outlet      176      354  ok (non-closed singly connected) (18.5806 -11.4978 0.15) (21.0301 5.9309 0.25)
                   front    99981   103289  ok (non-closed singly connected) (-5.97801 -11.4978 0.25) (21.0301 9.38239 0.25)
                    back    99981   103289  ok (non-closed singly connected) (-5.97801 -11.4978 0.15) (21.0301 9.38239 0.15)
           airfoil_solid     2585     5170  ok (non-closed singly connected) (-3.00658e-05 -0.14046 0.15) (0.990449 0.0593403 0.25)

Checking geometry...
    Overall domain bounding box (-5.97801 -11.4978 0.15) (21.0301 9.38239 0.25)
    Mesh (non-empty, non-wedge) directions (1 1 0)
    Mesh (non-empty) directions (1 1 0)
    All edges aligned with or perpendicular to non-empty directions.
    Boundary openness (1.33896e-18 5.41191e-21 3.12079e-14) OK.
    Max cell openness = 2.16716e-16 OK.
    Max aspect ratio = 2.51791 OK.
    Minimum face area = 2.51612e-07. Maximum face area = 0.0100472.  Face area magnitudes OK.
    Min volume = 2.51612e-08. Max volume = 0.00100472.  Total volume = 43.6397.  Cell volumes OK.
    Mesh non-orthogonality Max: 30.6861 average: 3.70862
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 1.17932 OK.
    Coupled point location match (average 0) OK.
    Face tets OK.
    Min/max edge length = 0.000483718 0.100434 OK.
    All angles in faces OK.
    Face flatness (1 = flat, 0 = butterfly) : average = 1  min = 1
    All face flatness OK.
    Cell determinant (wellposedness) : minimum: 1 average: 4.04297
    Cell determinant check OK.
 ***Concave cells (using face planes) found, number of cells: 1357
  <<Writing 1357 concave cells to set concaveCells

Failed 1 mesh checks.

End

[wyldckat]

Greetings Saeideh,

Without seeing where the concave cells are, it's hard to diagnose anything.

My suggestions are as follows:

• If you are using paraFoam and using the file extension ".OpenFOAM", then you should be able to see 2 options (I can't remember their exact names):
  • Include sets and/or zones
  • Use VTKPolyhedron
  With these options, you can select to see the sets "twoInternalFacesCells" and "concaveCells", as well as to view the real mesh.
• In case you are not using the files ".OpenFOAM", then you can use the following commands for exporting the sets to VTK:
  

  foamToVTK -cellSet twoInternalFacesCells
  foamToVTK -cellSet concaveCells

• Once you've seen the cells in question, you can decide if the concave cells are concave or not ( http://en.wikipedia.org/wiki/Concave ), because OpenFOAM's checkMesh algorithm sometimes has issues figuring it out if the cell is truly concave or not.
• From the wiki page http://openfoamwiki.net/index.php/SnappyHexMesh I suggest that you study the following two items:
  • The tutorial "A Comprehensive Tour of snappyHexMesh";
  • and section "Handling inclined surfaces" on the wiki: http://openfoamwiki.net/index.php/Sn...lined_surfaces

If after all of this you still have problems, we'll need more information about the mesh (namely what you see on each set), as well a description of what you've learned and tried from the mentioned study items.

Best regards,
Bruno

[s.m]

Originally Posted by wyldckat

Greetings Saeideh,

Without seeing where the concave cells are, it's hard to diagnose anything.

My suggestions are as follows:

• If you are using paraFoam and using the file extension ".OpenFOAM", then you should be able to see 2 options (I can't remember their exact names):
  • Include sets and/or zones
  • Use VTKPolyhedron
  With these options, you can select to see the sets "twoInternalFacesCells" and "concaveCells", as well as to view the real mesh.
• In case you are not using the files ".OpenFOAM", then you can use the following commands for exporting the sets to VTK:
  

  foamToVTK -cellSet twoInternalFacesCells
  foamToVTK -cellSet concaveCells

• Once you've seen the cells in question, you can decide if the concave cells are concave or not ( http://en.wikipedia.org/wiki/Concave ), because OpenFOAM's checkMesh algorithm sometimes has issues figuring it out if the cell is truly concave or not.
• From the wiki page http://openfoamwiki.net/index.php/SnappyHexMesh I suggest that you study the following two items:
  • The tutorial "A Comprehensive Tour of snappyHexMesh";
  • and section "Handling inclined surfaces" on the wiki: http://openfoamwiki.net/index.php/Sn...lined_surfaces

If after all of this you still have problems, we'll need more information about the mesh (namely what you see on each set), as well a description of what you've learned and tried from the mentioned study items.

Best regards,
Bruno

Dear bruno
Thank you very much, your explanation was very usefull and obvious
i am using paraFoam and the file extension ".OpenFOAM", so i checked the

• Include sets
• include zones
• Use VTKPolyhedron
• update GUI

as it can see in the pictures, after updating the GUI the "concaveCells -scellset" & "twoInternalFacesCells -cellset" appear, i check them, and uncheck the internalMesh, and what the paraFoam is seen to me, are the pictures that i attach in this post.
Thank you again for your nice attention
i study the references now, thank for introducing them too.

[s.m]

Dear Bruno, i don't understand anythig usefull from this pics, for solving my failed meshs, would you please guide me again?

Regards

[wyldckat]

OK, then can you please provide pictures where they only show the concave cells set on a few pictures, and the internal faces set on the other pictures?
Because I don't want to have to guess which ones are which ones

[s.m]

Originally Posted by wyldckat

OK, then can you please provide pictures where they only show the concave cells set on a few pictures, and the internal faces set on the other pictures?
Because I don't want to have to guess which ones are which ones

Thease are the pictures, here you are.
The twoInternalFacesCells are the cells that exit in the 4 corner of the domain.

[s.m]

When i unchecked the "use VTKpolyhedron " in object inspector, the pictures of concaveCell -cellSet change in this way, i attach them in the following.

[wyldckat]

From what I can see, the "concave cells" are fine. I think checkMesh is in this case complaining about the fact that those cells have 2 faces on the same side, leading to 180 between those two faces, leading to the diagnose those cells as likely being concave.

As for "twoInternalFacesCells": there isn't a zoom picture to see them properly


Without the VTK Polyhedron representation, what happens is that the cells are sliced (decomposed) into hexahedral or tetrahedral shaped cells, so that it's most likely to be properly represented on-screen. The polyhedral representation in ParaView is relatively more recent than the OpenFOAM/ParaView themselves, which is why the sliced cells is the standard representation.

[s.m]

Originally Posted by wyldckat

From what I can see, the "concave cells" are fine. I think checkMesh is in this case complaining about the fact that those cells have 2 faces on the same side, leading to 180 between those two faces, leading to the diagnose those cells as likely being concave.

As for "twoInternalFacesCells": there isn't a zoom picture to see them properly


Without the VTK Polyhedron representation, what happens is that the cells are sliced (decomposed) into hexahedral or tetrahedral shaped cells, so that it's most likely to be properly represented on-screen. The polyhedral representation in ParaView is relatively more recent than the OpenFOAM/ParaView themselves, which is why the sliced cells is the standard representation.

Excuse me
Thease pictures are the zoom of "twoInternalFacesCells" that are in the corner of the domain.
second without VTK Polyhedron checked third with VTK Polyhedron checked.
The "twoInternalFacesCells" don't change when i checked the VTK Polyhedron.

[wyldckat]

Hi Saeideh,

It shows a single face Problem is that I have not idea where in space is that face

You can open in that same ParaView, the same ".OpenFOAM" file, therefore having the same file opened twice. In the second one, you can choose to show the internal mesh, in wireframe mode. This should give us a better perception of where the faces.

Either way, my guess is that everything is fine with the mesh. The indications given by checkMesh are simply situations that the user should confirm for him/herself.

Best regards,
Bruno

[s.m]

Originally Posted by wyldckat

Hi Saeideh,

It shows a single face Problem is that I have not idea where in space is that face

You can open in that same ParaView, the same ".OpenFOAM" file, therefore having the same file opened twice. In the second one, you can choose to show the internal mesh, in wireframe mode. This should give us a better perception of where the faces.

Either way, my guess is that everything is fine with the mesh. The indications given by checkMesh are simply situations that the user should confirm for him/herself.

Best regards,
Bruno

Hi Bruno
Thank you very much
in the first picture, it can be seen 4 cells, that is located at 4 corner of the domain,

in the second and third one i zoom to show one of this 4 cells better, because of it you see only one cell in those pics.

why the cells that have 2 faces on the same side is created during meshing?

[wyldckat]

Isn't there another face perpendicular to the one you're showing?

I don't remember if you indicated the mesher you've used, so it's hard to ascertain as to why the faces are not properly done.

[s.m]

Originally Posted by wyldckat

Isn't there another face perpendicular to the one you're showing?

I don't remember if you indicated the mesher you've used, so it's hard to ascertain as to why the faces are not properly done.

yes it is, this cell that i zoom in, is in the front face, i extrude the front face 0.1, to have 3D mesh for analysis, but i set the front and back face to empty for 2D analysis.
i use the snappyHexMesh utility for creating my mesh.

[s.m]

some new pics from concaveCells

[wyldckat]

When in doubt, compare with OpenFOAM's tutorials.
If you look at the tutorial "incompressible/icoFoam/cavity" and run the same complete checkMesh, it will also tell you that:

  <<Writing 4 cells with with two non-boundary faces to set twoInternalFacesCells

So I guess this is normal when using 2D meshes.

edit: and like I wrote before, don't worry about these specific concave cells.

[s.m]

some new pics from concaveCell

[s.m]

Originally Posted by wyldckat

When in doubt, compare with OpenFOAM's tutorials.
If you look at the tutorial "incompressible/icoFoam/cavity" and run the same complete checkMesh, it will also tell you that:

  <<Writing 4 cells with with two non-boundary faces to set twoInternalFacesCells

So I guess this is normal when using 2D meshes.

edit: and like I wrote before, don't worry about these specific concave cells.

ok, Thank you, is concavecells ok too?

[wyldckat]

Originally Posted by s.m

ok, Thank you, is concavecells ok too?

I think they are OK. Because the detection that is occurring is actually only because each one of those cells has 2 faces on the same side, which each one of those faces is connected to smaller cell, which is normal for these larger cells that are next to smaller cells.

[s.m]

Originally Posted by wyldckat

I think they are OK. Because the detection that is occurring is actually only because each one of those cells has 2 faces on the same side, which each one of those faces is connected to smaller cell, which is normal for these larger cells that are next to smaller cells.

Ok, Thank you very much dear Bruno, Thank you for your attention to my questions.

i leave this 1 failed mesh that is reported from checkMesh -allGeometry because as i understand it doesn't effect on my analysis.

Best Regards,
Saeiseh.

[overdrive]

I noticed "two internalFacesCells" with "checkMesh -allTopology" in my 3D-case, too. I have an unstructured mesh generated with ICEM (export fluent_v6/nastran; import fluent3DMeshToFoam). These Cells are tetras and located along the border of two patches.
They have an effect on BCs, so it would be better to avoid this error. The error does not occur when I use a structured mesh or when I extrude a prism layer at the boundaries. Does someone know something about this problem?

Kind regards