Howdy, Stranger!

It looks like you're new here. If you want to get involved, click one of these buttons!

Sign In Apply for Membership

Internal volume mesh becoming coarser during layer creation
  • Arnoldinho January 2011
    Hi,

    maybe it's a stupid question, but I have a problem using engrid for the boundary layer generation in 3D cases. The orginally created internal (volume) mesh becomes coarser during the boundary layer or generally the volume mesh creation in engrid.

    Let's explain the procedure: I have a block of lets say 1x1x1m that is horizontally divided into several (volume) layers. The layers have different resolutions/edge lengths of tet elements. The mesh is created in Salome using the Netgen algorithm; boundary patches have been created and the mesh is exported into .unv format. After conversion with ideasUnvToFoam, the mesh is imported into engrid by Import -> OpenFOAM case. Then I do "edit boundary conditions", create a new volume and set all boundary patches (six, from the cube sides) to green. Then I do "create prismatic boundary layer", pick the boundary condition to refine and set the conditions. The boundary layer is calculated/created as intended. Then I export the new mesh via Export -> OpenFOAM case (grid only).

    No I come to the problem: When I open the mesh in Paraview, the surface mesh of the cube edges (outer 2D mesh) is still fine, but the internal (3D) volume mesh of the cube has become very coarse. No different resolutions of the volume layers can be found any more. So, where can I tell engrid to keep the former internal volume mesh resolutions?

    Best regards,
    Arne
  • Oliver January 2011
    Hello,

    enGrid will always create a new volume mesh (using NETGEN as well for the tetra part), even if you already have one. Hence you need to define your mesh resolution within enGrid, not by importing an existing volume mesh. After the prismatic layer has been created, the volume mesh needs to be improved in order to respect the desired mesh resolution (create/improve volume mesh).

    Generally it is better to create the whole mesh within enGrid -- including the surfaces. This is, however, not required for the volume meshing to work.

    You can also check the internal mesh density by using the clipping options before exporting to OpenFOAM.

    Cheers,
    Oliver
  • vaina74 January 2011
    I'm not so expert in enGrid, but maybe you can just mesh the surfaces of your domain in Salome (or Netgen or whatever you want) with your preferred critera, then import into enGrid and build the whole internal mesh by building a prismatic layer. If you're not satisfied with the resulting grid, you can improve and refine with enGrid tools.
    update:
    OK, while I was replying a REAL expert user (and developer) replied. Well, at leat I was correct :-)
  • Arnoldinho January 2011
    Thanks to both of you for your answers - and a special Thanks to Oliver for the great tool!

    I think I have to continue building my surface mesh in Salome as I sometimes need blended grid resolutions over my surfaces (and enGrid is only able to define a fixed value, right?). My second question now is: can I set some kind of resolution parameters, e.g. edge lengths, areas or volumes for my volume mesh in enGrid, as it is e.g. possible in Salome? I could not find any entry for this.
    If not, how can I know, after using the "improve volume mesh" option several times, that I reached my desired mesh resolution? By looking at the number of elements and knowing "what I need" from my former volume mesh?
    For this case, is any local volume mesh refinement possible?

    Btw: How does the "improving algorithm" work at all?

    Cheers,
    Arne
  • Oliver January 2011
    Arne,

    "I think I have to continue building my surface mesh in Salome as I sometimes need blended grid resolutions over my surfaces (and enGrid is only able to define a fixed value, right?)." My second question now is: can I set some kind of resolution parameters, e.g. edge lengths, areas or volumes for my volume mesh in enGrid, as it is e.g. possible in Salome? I could not find any entry for this.

    Not right ;-) You can define rules and sources for your mesh resolution and they will affect the surface and volume grids. If you are using version 1.2, please have a look at the tutorial from P. Bomke (see the comment which is linked below).

    http://engits.eu/vanilla/index.php?p=/discussion/comment/591/#Comment_591

    "If not, how can I know, after using the "improve volume mesh" option several times, that I reached my desired mesh resolution? By looking at the number of elements and knowing "what I need" from my former volume mesh? For this case, is any local volume mesh refinement possible?"

    Usually running it once after the initial prismatic layer process will give you a decent grid.

    "Btw: How does the "improving algorithm" work at all?"

    Based on a first coarse grid, local mesh densities are computed on that grid (using sources and the cell growth you specified). All mesh resolution parameters can be specified in . This is a bit of a misnomer because it also affects volume cells.

    'hope this helps a bit.

    Cheers,
    Oliver

  • Arnoldinho February 2011
    Oliver,

    thanks for your explanations. It indeed (almost) works as expected.