[Rojj]

Hello

Is it possible to create a Mesh made by two blocks with different vertices and then use snappyHexMesh?

I have created the following mesh

// -*- C++ -*-
// File generated by PyFoam - sorry for the ugliness

FoamFile
{
 version 2.0;
 format ascii;
 class dictionary;
 object blockMeshDict;
}

convertToMeters 1;

vertices
  (
    (-595.82 -620.459 -5)
    (670.098 -620.459 -5)
    (670.098 645.459 -5)
    (-595.82 645.459 -5)

    (-595.82 -620.459 100)
    (670.098 -620.459 100)
    (670.098 645.459 100)
    (-595.82 645.459 100)

    (-595.82 -620.459 100)
    (670.098 -620.459 100)
    (670.098 645.459 100)
    (-595.82 645.459 100)

    (-595.82 -620.459 520)
    (670.098 -620.459 520)
    (670.098 645.459 520)
    (-595.82 645.459 520)
  );

  blocks
    (
      hex (0 1 2 3 4 5 6 7) (158 158 10) simpleGrading (1 1 1)
      hex (8 9 10 11 12 13 14 15) (79 69 28) simpleGrading (1 1 1)
    );

  edges
    (
    );

  boundary
    (
      sides
      {
        type patch;
        faces (
                (0 4 7 3)
                (8 12 15 11)
                (6 5 1 2)
                (14 13 9 10)
              );
      }

      inlet
      {
        type patch;
        faces (
                (3 7 6 2)
                (11 15 14 10)
              );
      }

      outlet
      {
        type patch;
        faces (
                (5 4 0 1)
                (13 12 8 9)
              );
      }

      ground
      {
        type wall;
        faces (
                (3 2 1 0)
              );
      }

      internalBottom
      {
        type patch;
        faces (
                (4 5 6 7)
              );
      }

      internalTop
      {
        type patch;
        faces (
                (8 11 10 9)
              );
      }

      sky
      {
        type patch;
        faces (
                (12 13 14 15)
              );
      }


    );

    mergePatchPairs (
      ( internalTop internalBottom ) );

but when I mesh with snappyHexMesh I receive the following error

Selected for refinement : 44456 cells (out of 404984)
hexRef8 : Dumping cell as obj to "/home/ubuntu/OpenFOAM/ubuntu-4.1/run/test02_base_Baseline/mesh/cell_251301.obj"


--> FOAM FATAL ERROR:
cell 251301 of level 0 uses more than 8 points of equal or lower level
Points so far:8(254492 254493 254572 254573 260092 260093 260172 260173)

    From function Foam::labelListList Foam::hexRef8::setRefinement(const labelList&, Foam::polyTopoChange&)
    in file polyTopoChange/polyTopoChange/hexRef8/hexRef8.C at line 3701.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::hexRef8::setRefinement(Foam::List<int> const&, Foam::polyTopoChange&) at ??:?
#3  Foam::meshRefinement::refine(Foam::List<int> const&) at ??:?
#4  Foam::meshRefinement::refineAndBalance(Foam::string const&, Foam::decompositionMethod&, Foam::fvMeshDistribute&, Foam::List<int> const&, double) at ??:?
#5  Foam::snappyRefineDriver::surfaceOnlyRefine(Foam::refinementParameters const&, int) at ??:?
#6  Foam::snappyRefineDriver::doRefine(Foam::dictionary const&, Foam::refinementParameters const&, Foam::snapParameters const&, bool, Foam::dictionary const&) at ??:?
#7  ? at ??:?
#8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9  ? at ??:?
Aborted (core dumped)

Cell 251301 is located at the interface internalTop/internalBottom.

I have tried to change slave and master, but the problem just happens in a different cell.

this picture shows the mesh and this one shows the cell

[Antimony]

Hi,

Nope. To the best of my knowledge, with snappyHexMesh you cannot do that. While blockMesh might merge the two meshes that you created, the resultant mesh is no longer purely hexahedral, which is a requirement to be able to run snappyHexMesh.

Instead you can do the following (assuming your geometry that you want to run your snappy on is less than the height of your first block):

1. Have a case and in that run blockMesh with only the first block
2. For the case from step 1, run snappyHexMesh
3. Have a separate case and in that run blockMesh with only the second block
4. Merge the two cases together using mergeMesh
5. Use either stitchMesh or cyclicAMI to take care of the overlapping patches.

Hope this helps.

Cheers,
Antimony

[Rojj]

Thanks Antimony. That certainly clarifies the issue.

Your proposed solution is interesting. As I am running everything programmatically, it might be relatively simple to implement.

I am now testing the cyclicAMI. I would like to better understand how it works (I will probably need it in the near future) and see if I can avoid the two step meshing.

Will report back.

[farzadmech]

Dear Antimony,
Thanks a lot for your suggestion. I am going to use it for my case to avoid huge cell numbers. I already posted my problem, I will be happy if you look at it.

Thanks,
Farzad

Originally Posted by Antimony

Hi,

Nope. To the best of my knowledge, with snappyHexMesh you cannot do that. While blockMesh might merge the two meshes that you created, the resultant mesh is no longer purely hexahedral, which is a requirement to be able to run snappyHexMesh.

Instead you can do the following (assuming your geometry that you want to run your snappy on is less than the height of your first block):

1. Have a case and in that run blockMesh with only the first block
2. For the case from step 1, run snappyHexMesh
3. Have a separate case and in that run blockMesh with only the second block
4. Merge the two cases together using mergeMesh
5. Use either stitchMesh or cyclicAMI to take care of the overlapping patches.

Hope this helps.

Cheers,
Antimony