Known limitations with the built-in reader in ParaView

[wyldckat]

Over time, there have been several issues detected with using the internal .foam reader in ParaView that blueCFD-Core has to use on Windows OS. Here are the know issues and how to solve them.

[wyldckat]

1. Already answered in the FAQ entry No-slip surfaces show non-zero velocities in ParaView #203.

2. Certain inclusions of files will not work as intended, such as:

   #include ${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes
   

   Part of the problem is that the parenthesis are not unwrapped. The other problem is that it's not able to figure out that it's an absolute path.

   This means that patches that are not explicitly defined with boundary conditions in the respective field files, could either not have the correct value represented or could lead to the fields to not be loaded.

   For example, the following error message can occur:

   ERROR: In C:\bbd\5105004d\source-paraview\VTK\IO\Geometry\vtkOpenFOAMReader.cxx, line 6902
   vtkOpenFOAMReaderPrivate (000002029AB7BA90): boundaryField propellerTip not found in object U at time = 0
   

   • Fixed as of at least ParaView 5.4.0.

3. includeEtc may not be supported by ParaView. The expected error message is as follows:

   ERROR: In C:\bbd\5105004d\source-paraview\VTK\IO\Geometry\vtkOpenFOAMReader.cxx, line 6506
   vtkOpenFOAMReaderPrivate (000001FC17973640): Error reading line 25 of X:\ofuser-of4\run\tutorials\multiphase\interPhaseChangeDyMFoam\propeller\0/U: Unsupported directive includeEtc
   

   • Fixed as of at least ParaView 5.4.0.

4. Incomplete dimensionsentries such as this one:

   dimensions      [1 -1 -2 0 0];
   

   Will result in an error message such as this one:

   ERROR: In C:\bbd\5105004d\source-paraview\VTK\IO\Geometry\vtkOpenFOAMReader.cxx, line 6506
   vtkOpenFOAMReaderPrivate (000001FC17973640): Error reading line 18 of X:\ofuser-of4\run\tutorials\multiphase\interPhaseChangeDyMFoam\propeller\0/p_rgh: Expected a number, found a non-digit character ]
   

   • Fixed as of at least ParaView 5.4.0.

5. Boundary conditions that use tables or lists that rely on scalar or vector data may not be loaded properly. For example, the following boundary condition will not have its table data be loaded into ParaView or it could even simply break due to not recognizing the boundary condition itself:

   inlet
   {
       type            uniformFixedValue;
       uniformValue    table
       (
           (0     (0 0 0))
           (0.01  (0 -15 0))
           (100   (0 -15 0))
       );
       value           $internalField;
   }
   

   • It can give either just a warning for ParaView versions 5.1 and newer, due to the vectors within the table rows:

     Generic Warning: In C:\bbd\2d618e80\source-paraview\VTK\IO\Geometry\vtkOpenFOAMReader.cxx, line 4023
     Found a list containing scalar data followed by a nested list, but this reader only supports nested lists that precede all scalars. Discarding nested list data.
     

   • Or give an error message for not recognizing the boundary condition:

     ERROR: In ..\..\..\..\source\VTK\IO\vtkOpenFOAMReader.cxx, line 6481
     vtkOpenFOAMReaderPrivate (000000000EFD15F0): Error reading line 33 of X:\ofuser-of4\run\tutorials\multiphase\interPhaseChangeDyMFoam\propeller\0/U: Expected a number, found (
     

     • Possible solutions are given here: 'turbineSiting tutorial and paraview-3.98.0' thread at CFD-Online

     • Fixed as at least ParaView 5.1.0.