OpenFOAM

  1. ...
  2. ...
  3. CAE
  4. OpenFOAM
  1. Description
  2. Volume Conditions
  3. Poly-Voxel
  4. Related Commands
  5. Demonstration

Description

OpenFOAM is an open source solver that supports 3D hybrid grids including all cell types available in Fidelity Pointwise.

 

Caution: The presence of pole connectors and pole domains in structured blocks can result in degenerate hexahedral cells when exporting to an unstructured CAE format. Please refer to the Collapsed Cell Types section of this User Manual for more information on which structured topologies result in unsupported cell types.

Any baffle domains which have boundary conditions assigned to the faceSet type will not have their grid points cloned or "inflated" at export. On the other hand, baffle domains assigned to boundary conditions of any other type will have their points cloned.

Multiple volume conditions can be assigned and exported for interior, boundary, and complete volumes. Exporting volume conditions will result in additional files to the default five export files required by OpenFOAM. Additionally, solver attributes can be assigned so that Cell and Face data for the mesh can be exported as Sets, Zones, or both. Note that more OpenFOAM solver attributes are available in CAE, Solver Attributes, OpenFOAM

 

Tip: For more information about OpenFOAM, visit the official web site: https://www.opencfd.co.uk/openfoam

OpenFOAM Volume Conditions

Keep in mind that OpenFOAM does not support what is considered to be standard volume conditions. That being said, Fidelity Pointwise has defined a set of "special" OpenFOAM volume conditions that can be used to define different variations of face/cell sets and face/cell zones to be exported.

When the current CAE solver is OpenFOAM, you can define collections of faces in the CAE, Set Volume Conditions panel and use the volume condition Type options to define which cells and faces should be exported via the File, Export, CAE command. The table below, presents information regarding the specific meaning of each Fidelity Pointwise-defined OpenFOAM volume condition Type.

OpenFOAM Volume Conditions
Fidelity Pointwise-defined special OpenFOAM volume conditions allow you to define which cells and faces should be exported via the File, Export, CAE command.
Type Description
volumeToFace All faces are exported
interiorToFace Only interior faces are exported
boundaryToFace Only boundary faces are exported
interiorToFace+boundaryToFace Interior and boundary faces are exported separately
volumeToCell All cells are exported
volumeToCell+volumeToFace All cells and faces are exported
volumeToCell+interiorToFace All cells and interior faces are exported
volumeToCell+boundaryToFace All cells and boundary faces are exported
volumeToCell+interiorToFace+boundaryToFace All cells and interior and boundary faces are exported separately

Poly-Voxel Export

This CAE format supports exporting voxel cells as polyhedra. For more information on this topic, see the Poly-Voxel Export Options section of this User Manual.

Demonstration

Poly-Voxel Export