Paraview unable to read lagrangian data (openFoam)

ParaView Support
8

@mwestphal Additionally we may wish to have a sticky FAQ (for the OpenFOAM question).

The problem (and confusion) originates from an internal OpenFOAM change to use barycentric coordinates in its lagrangian framework.

In the openfoam.com version:

  • The positions file contains tuples of (x,y,z, cellId). This file is generally ignored by OpenFOAM (in favour of the coordinates file), but is readable by ParaView. The format is consistent with what older versions of OpenFOAM generated.
  • The coordinates file contains the barycentric coordinates. This is used for OpenFOAM restarts but not by ParaView.

In the openfoam.org version:

  • The positions file was changed to contain the barycentric coordinates (identical contents to the openfoam.com coordinates file). Cannot be read by ParaView.

It is probably not realistic to expect support for the openfoam.org positions file. This would require shadowing the volume mesh in order to define the cells, additional tet decomposition of the volume cells, additional barycentric calculations to determine the corresponding x,y,z positions.

Available options, in any order of preference:

  • use the openfoam.com version that generates a positions file that can be read by ParaView.
  • use foamToVTK or foamToEnsight to convert the lagrangian fields only.