makeFaMesh

Overview

The makeFaMesh utility creates finite-area meshes from volume-mesh patches.

Usage

Synopsis

makeFaMesh [OPTIONS]

Examples

Run makeFaMesh and write the mesh as a VTK file for display:

makeFaMesh -write-vtk

Input

Arguments

No arguments required.

Options

-allAreas         Use all regions in finite-area regionProperties
  -area-region <name>
                    Specify area-mesh region. Eg, -area-region shell
  -area-regions <wordRes>
                    Use specified area region. Eg, -area-regions film
                    Or from regionProperties.  Eg, -area-regions '(film
                    "solid.*")'
  -case <dir>       Case directory (instead of current directory)
  -decomposeParDict <file>
                    Alternative decomposePar dictionary file
  -dict <file>      Alternative faMeshDefinition
  -dry-run          Create but do not write
  -empty-patch <name>
                    Specify name for a default empty patch
  -no-decompose     Suppress procAddressing creation and field decomposition
                    (parallel)
  -no-fields        Suppress field decomposition (parallel)
  -parallel         Run in parallel
  -region <name>    Specify mesh region (default: region0)
  -write-vtk        Write mesh as a vtp (vtk) file for display or debugging
  -doc              Display documentation in browser
  -help             Display short help and exit
  -help-compat      Display compatibility options and exit
  -help-full        Display full help and exit

Files

The makeFaMesh utility is configured using a <case>/system/faMeshDefinition, taking the form:

polyMeshPatches             ( <patch1> <patch2> ... <patchN> );

boundary
{
    <faPatch1>
    {
        type                <word>;
        neighbourPolyPatch  <word>;
        ownerPolyPatch      <word>;
    }
}

defaultPatch
{
    name    <word>;
    type    <word>;
}

Property	Description	Type	Required	Default
polyMeshPatches	List of volume mesh patches to use as the base of the finite area mesh	wordRes	yes	-
boundary	Dictionary providing list of edge-boundary conditions	dict	yes	-
type	Patch type, e.g. patch	word	yes	-
neighbourPolyPatch	Finite-volume patch neighbouring the finite-area	word	yes	-
ownerPolyPatch	Finite-volume patch corresponding to the finite-area patch	word	no	-
defaultPatch	Dictionary providing characteristics of default patches	dict	no	-
name	Name of default patches	word	yes	-
type	Patch type of default patches, e.g. empty	word	yes	-

Fields

No field input required.

Output

Logs

No log output.

Files

No file output.

Fields

The default path to write fields is <case>/constant/faMesh/.

Property	Description	Type
faBoundary	Finite-area boundary info	faBoundaryMesh
faceLabels	Finite-area mesh info	labelList

Further information

Tutorial:

• faMeshDefinition
• faMeshDefinition
• faMeshDefinition

Source code:

• makeFaMesh

History: Introduced in version v1712