[zfaraday]

Hi all,

I'm doing some tests with a geometry that is giving me some troubles according to what checkMesh says. This are the errors that the utility finds (using -allTopology -allGeometry options):

 ***Cells with small determinant (< 0.001) found, number of cells: 570
  <<Writing 570 under-determined cells to set underdeterminedCells
 ***Concave cells (using face planes) found, number of cells: 424
  <<Writing 424 concave cells to set concaveCells
    Face interpolation weight : minimum: 0.007427217 average: 0.4584105
 ***Faces with small interpolation weight (< 0.05) found, number of faces: 608
  <<Writing 608 faces with low interpolation weights to set lowWeightFaces
    Face volume ratio : minimum: 0.005415454 average: 0.8586378
 ***Faces with small volume ratio (< 0.01) found, number of faces: 304
  <<Writing 304 faces with low volume ratio cells to set lowVolRatioFaces

I would like to know what these errors exactly mean and how can they affect to the final result. I think that the concave cells are not a problem in my case taking into account all the information I've found out in the forum, but the other errors I have no clue what they mean nor how to solve them if its impact on the result is really significant.

Any hint about it will be much appreciated!

Regards,

Alex

[alexB]

Hi Alex,

can you look at your mesh with paraFoam?
Perhaps you can upload a picture here somehow (Dropbox etc. desribed here http://www.cfd-online.com/Forums/ope...-get-help.html ).

I am also just at the beginning of learning OF, so the errors dont mean much to me.

Greetings
Alex

[zfaraday]

Hi Alex,

The reason why I didn't upload any picture of my geometry is that the only think I want is to have a better understanding of this errors, I mean the theoretical background behind them so that I can detect more easily the cells/faces and how to proceed to correct the mesh on my own.

Greetings,

Alex

[Astrodan]

I can't help there either, but I have quite similar problems and would be interested.

However, maybe given images might help identify the "physical" problem, so I attached images for four different errors that occur in

checkMesh -allGeometry -allTopology

Result (excerpt):
    Face-face connectivity OK.
  <<Writing 117 cells with two non-boundary faces to set twoInternalFacesCells
    Number of regions: 1 (OK).

    Cell determinant (wellposedness) : minimum: 0 average: 109.741
 ***Cells with small determinant (< 0.001) found, number of cells: 117
  <<Writing 117 under-determined cells to set underdeterminedCells
 ***Concave cells (using face planes) found, number of cells: 4498
  <<Writing 4498 concave cells to set concaveCells
    Face interpolation weight : minimum: 0.0733659 average: 0.447134
    Face interpolation weight check OK.
    Face volume ratio : minimum: 0.0011126 average: 0.821268
 ***Faces with small volume ratio (< 0.01) found, number of faces: 3884
  <<Writing 3884 faces with low volume ratio cells to set lowVolRatioFaces

Failed 3 mesh checks.

What seems to be the case is that, the twoInternalFacesCell and underdeterminedCells are identical.

I also attached the concave cells, since I have a lot of them.

To have a better overview:

• underdeterminedCells/twoInternalFaces:
  underdeterminedCells.jpg twoInternalFaces.jpg
• lowVolRatio
  lowVolRatio.jpg
• concaveCells
  concaveCells.jpg

I also have 10 non-orthogonal cells, but I think they are not that bad, and I have a pretty good idea how to remove them.


Furthermore, for the mesh generation process, which I'm sure is quite important:

1. I Created the geometry with four regions (different mesh structures in screenshots) in ANSYS Meshing
   1. The left and both right parts are structured meshes, with some refinement done towards the walls
   2. the center part contains some ugly geometry, and the hex mesh tended to be messy, so I but a tet-mesh here.
2. Export the mesh as ACSII-msh
3. Import in OpenFOAM using fluent3DMeshToFoam
4. Merge all boundaries that are the same (e.g. walls) for different regions using createPatch utility
5. Stitch the regions using the stitchMesh utitiliy
6. Remove empty patches with the createPatch utility

So, if anyone has ideas what is going on there, I'd (we'd) appreciate help. And I hope you don't mind me using you thread, Alex .

[derekm]

Originally Posted by zfaraday

Hi Alex,

The reason why I didn't upload any picture of my geometry is that the only think I want is to have a better understanding of this errors, I mean the theoretical background behind them so that I can detect more easily the cells/faces and how to proceed to correct the mesh on my own.

Greetings,

Alex

have you read
ALGEBRAIC MESH QUALITY METRICS∗
PATRICK M. KNUPP SIAM J. SCI. COMPUT. Vol. 23, No. 1, pp. 193–218.
Derek

[zfaraday]

Hi Derek,

Many many many thanks for your information! I totally ignored the existence of this paper and I think it is exactly what I needed!

Again, thanks for sharing so useful information!

Best regards,

Alex

[franjo_j]

Hello,

These errors do not mean that you mesh is invalid, it just tells that it may cause problems to the numerics in the following ways:
1. Small determinants - generally this mean that the volume of some cells is very small compared to their area and that they are nearly planar or collinear. I would not expect convergence problems if these cells were in the right locations (and aligned with the gradient of the solution).
2. Concave cells - are a consequence of non-flat faces, and in general it does not cause convergence problems. It does affect accuracy, but it is not too worrying when it is difficult to generate any mesh in the first place.
3. Interpolation weights - are important for the convection term and implicitly for the diffusion term. Low weights mean that one of cell at a face dominates over the other. This is not a problem when the solution is uniform, and severely reduces accuracy and convergence is case of non-uniform fields.
4. Volume ratio - is important for the source terms and the pressure equation. Again, it might be a problem if the solution is not uniform at that location.

I hope this adds some value so that you can understand these quality metrics better. These are my experiences when dealing with adaptive refinement with high aspect ratio cells.

Regards,

Franjo

[zfaraday]

Hello Franjo,

Originally Posted by franjo_j

Hello,

These errors do not mean that you mesh is invalid, it just tells that it may cause problems to the numerics in the following ways:
1. Small determinants - generally this mean that the volume of some cells is very small compared to their area and that they are nearly planar or collinear. I would not expect convergence problems if these cells were in the right locations (and aligned with the gradient of the solution).
2. Concave cells - are a consequence of non-flat faces, and in general it does not cause convergence problems. It does affect accuracy, but it is not too worrying when it is difficult to generate any mesh in the first place.
3. Interpolation weights - are important for the convection term and implicitly for the diffusion term. Low weights mean that one of cell at a face dominates over the other. This is not a problem when the solution is uniform, and severely reduces accuracy and convergence is case of non-uniform fields.
4. Volume ratio - is important for the source terms and the pressure equation. Again, it might be a problem if the solution is not uniform at that location.

I hope this adds some value so that you can understand these quality metrics better. These are my experiences when dealing with adaptive refinement with high aspect ratio cells.

Regards,

Franjo

Wow! Thanks for this detailed and complete explanation! That was exactly what I needed!

However, I thought that the small determinant issue was an important point to take into account as Bruno Santos "wyldcat" suggested here in the forum in some other thread...

Again, thanks for taking your time with this very good answer!

Best regards,

Alex

[Astrodan]

As marango say here underdetermined cells apparently can also occur when they have multiple boundary faces, so maybe that is your problem, too.

Apart from that, thanks Franjo for the explanation. As helpful as the Paper might be, it is far too complex for me to understand any time soon..

[Howard]

Originally Posted by Astrodan

I can't help there either, but I have quite similar problems and would be interested.

However, maybe given images might help identify the "physical" problem, so I attached images for four different errors that occur in

checkMesh -allGeometry -allTopology
 
Result (excerpt):
    Face-face connectivity OK.
  <<Writing 117 cells with two non-boundary faces to set twoInternalFacesCells
    Number of regions: 1 (OK).
 
    Cell determinant (wellposedness) : minimum: 0 average: 109.741
 ***Cells with small determinant (< 0.001) found, number of cells: 117
  <<Writing 117 under-determined cells to set underdeterminedCells
 ***Concave cells (using face planes) found, number of cells: 4498
  <<Writing 4498 concave cells to set concaveCells
    Face interpolation weight : minimum: 0.0733659 average: 0.447134
    Face interpolation weight check OK.
    Face volume ratio : minimum: 0.0011126 average: 0.821268
 ***Faces with small volume ratio (< 0.01) found, number of faces: 3884
  <<Writing 3884 faces with low volume ratio cells to set lowVolRatioFaces
 
Failed 3 mesh checks.

What seems to be the case is that, the twoInternalFacesCell and underdeterminedCells are identical.

I also attached the concave cells, since I have a lot of them.

To have a better overview:

• underdeterminedCells/twoInternalFaces:
  Attachment 37940 Attachment 37941
• lowVolRatio
  Attachment 37942
• concaveCells
  Attachment 37943

I also have 10 non-orthogonal cells, but I think they are not that bad, and I have a pretty good idea how to remove them.


Furthermore, for the mesh generation process, which I'm sure is quite important:

1. I Created the geometry with four regions (different mesh structures in screenshots) in ANSYS Meshing
   1. The left and both right parts are structured meshes, with some refinement done towards the walls
   2. the center part contains some ugly geometry, and the hex mesh tended to be messy, so I but a tet-mesh here.
2. Export the mesh as ACSII-msh
3. Import in OpenFOAM using fluent3DMeshToFoam
4. Merge all boundaries that are the same (e.g. walls) for different regions using createPatch utility
5. Stitch the regions using the stitchMesh utitiliy
6. Remove empty patches with the createPatch utility

So, if anyone has ideas what is going on there, I'd (we'd) appreciate help. And I hope you don't mind me using you thread, Alex .

Hi, friend. Could I ask how to see the bad cells or points in paraview? I also have these problem. Thank you!

[Astrodan]

If you execute checkMesh it writes you cellSets with the erroneous cells in your polyMesh directory.

If you then view your case with paraFoam you can mark the checkbox "include sets" and choose the generated sets in the same list where you find the boundary conditions etc..

If you open the case twice in the same paraFoam window, you can use one instance to display the internal mesh (wired) and one to display the bad cells in surface rendering with a colour of your choice.

[ark704]

Hi all,

I have converted a fluent mesh (made in ICEM) to Openfoam format. I am facing 2 errors :
1. I am getting twoInernalfacecells problem at the edges of the geometry which is resulting in small determinant problem too.
2. underdetermined cells (<0.001).
The above problems were not shown in ICEM Quality patterns. How do I resolve this problem while meshing in ICEM?

How does the openfoam solver behaves if small determinant (< 0.001) and twoInternalfacecells are present in the mesh?

[franjo_j]

Hello,

Originally Posted by ark704

Hi all,

I have converted a fluent mesh (made in ICEM) to Openfoam format. I am facing 2 errors :
1. I am getting twoInernalfacecells problem at the edges of the geometry which is resulting in small determinant problem too.

There are some cells in the mesh that have mostly boundary faces and only two or one internal face. Do you maybe have columns of stacked hexes somewhere in the mesh?
By all means this is not an error.

Originally Posted by ark704

2. underdetermined cells (<0.001).
The above problems were not shown in ICEM Quality patterns. How do I resolve this problem while meshing in ICEM?

As was already mentioned, cells in oneInternalFaceCells and twoInternalFaceCells are also in the set of underdetermined cells. These cells may be problematic for evaluating gradients, and it depends on the boundary conditions applied there. Solution: refine the mesh or generate a boundary layer to reduce the number of boundary faces for each cells. Once again, this does not mean that you cannot run on this mesh.

Originally Posted by ark704

How does the openfoam solver behaves if small determinant (< 0.001) and twoInternalfacecells are present in the mesh?

With underDetermined cells I would only expect problems with Von Neumann type of boundary conditions, otherwise it should not cause problems.

Regarding the concave cells, all arbitrary polyhedra with a few faces in the same plane are classified are concave cells. These cells are the the boundary of becoming concave, and they are still not. Therefore, this is not a problem and I would not worry much about it.

[MaySea]

Originally Posted by franjo_j

Hello,

3. Interpolation weights - are important for the convection term and implicitly for the diffusion term. Low weights mean that one of cell at a face dominates over the other. This is not a problem when the solution is uniform, and severely reduces accuracy and convergence is case of non-uniform fields.

Hi,

My mesh has many faces with low interpolation weights.

Faces with small interpolation weight (< 0.05) found, number of faces: 141

Is there a way to reduce this with snappyHexMeshDict?
I confirm that these faces cause convergence (convection) problems... my simulations keep blowing up with this mesh.

Thanks,
Jan

[MaySea]

I fixed the problem by simply adding more layers.