foamToVTK.C File Reference

Legacy VTK file format writer. More...

Go to the source code of this file.

Detailed Description

Legacy VTK file format writer.

Original source file foamToVTK.C

- Handles volFields, volFields::Internal, pointFields, surfaceScalarField and surfaceVectorField.

  • Mesh topo changes.
  • Both ascii and binary.
  • Single time step writing.
  • Write subset only.
  • Automatic decomposition of cells; polygons on boundary undecomposed since handled by vtk.
Usage
foamToVTK [OPTION]

Options:

  • -ascii
    Write VTK data in ASCII format instead of binary.
  • -mesh <name>
    Use a different mesh name (instead of -region)
  • -fields <fields>
    Convert selected fields only. For example, 
          -fields "( p T U )"
    The quoting is required to avoid shell expansions and to pass the information as a single argument.
  • -surfaceFields
    Write surfaceScalarFields (e.g., phi)
  • -cellSet <name>
  • -faceSet <name>
  • -pointSet <name>
    Restrict conversion to the cellSet, faceSet or pointSet.
  • -nearCellValue
    Output cell value on patches instead of patch value itself
  • -noInternal
    Do not generate file for mesh, only for patches
  • -noPointValues
    No pointFields
  • -noFaceZones
    No faceZones
  • -noLinks
    (in parallel) do not link processor files to master
  • poly
    write polyhedral cells without tet/pyramid decomposition
  • -allPatches
    Combine all patches into a single file
  • -excludePatches <patchNames>
    Specify patches (wildcards) to exclude. For example, 
          -excludePatches '( inlet_1 inlet_2 "proc.*")'
    The quoting is required to avoid shell expansions and to pass the information as a single argument. The double quotes denote a regular expression.
  • -useTimeName
    use the time index in the VTK file name instead of the time index

    Note: mesh subset is handled by vtkMesh. Slight inconsistency in interpolation: on the internal field it interpolates the whole volField to the whole-mesh pointField and then selects only those values it needs for the subMesh (using the fvMeshSubset cellMap(), pointMap() functions). For the patches however it uses the fvMeshSubset.interpolate function to directly interpolate the whole-mesh values onto the subset patch.

    new file format:
    no automatic timestep recognition. However can have .pvd file format which refers to time simulation if XML *.vtu files are available:
          <?xml version="1.0"?>
      <VTKFile type="Collection"
           version="0.1"
           byte_order="LittleEndian"
           compressor="vtkZLibDataCompressor">
        <Collection>
          <DataSet timestep="50" file="pitzDaily_2.vtu"/>
          <DataSet timestep="100" file="pitzDaily_3.vtu"/>
          <DataSet timestep="150" file="pitzDaily_4.vtu"/>
          <DataSet timestep="200" file="pitzDaily_5.vtu"/>
          <DataSet timestep="250" file="pitzDaily_6.vtu"/>
          <DataSet timestep="300" file="pitzDaily_7.vtu"/>
          <DataSet timestep="350" file="pitzDaily_8.vtu"/>
          <DataSet timestep="400" file="pitzDaily_9.vtu"/>
          <DataSet timestep="450" file="pitzDaily_10.vtu"/>
          <DataSet timestep="500" file="pitzDaily_11.vtu"/>
        </Collection>
      </VTKFile>

Definition in file foamToVTK.C.