Description

When exporting to OpenFOAM, cell and face data can be exported as Sets, Zones, SetsAndZones, or not at all. The PointPrecision attribute can also be set via the Set Solver Attributes panel shown below.

CAE, Solver Attributes, OpenFOAM
The solver attributes for OpenFOAM include cell and face export format and point precision.

As required by OpenFOAM, all 2D grids are thickened (extruded) to a 1-cell-deep 3D grid during CAE export. The SideBCExport attribute controls how boundary conditions are applied to the base (original) domains and to the top domains of the thickened grid. The available options are:

Option Description
Unspecified No boundary conditions are applied.
Single (default) Both base and top boundary faces are placed in a single boundary condition named BaseAndTop with type Empty.
BaseTop The base boundary faces are placed in a boundary condition named Base with type Empty. On the other hand, the top boundary faces are placed in a boundary condition named Top with type Empty.
Multiple The base and top boundary faces are placed in a boundary conditions of type empty named <VCName>-base and <VCName>-top respectively. <VCName> denotes the name of the volume condition assigned to the original 2D grid.

The Thickness attribute controls the depth of the thickened grid; its default value is 0.0. Note that a Thickness of 0.0 will trigger an auto-compute functionality that will compute the optimal thickness for the 2D grid being exported.

 

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, 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 Pointwise-defined OpenFOAM volume condition Type.

OpenFOAM Volume Conditions
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