OpenFOAM® v1612+: New Meshing Functionality

OpenFOAM® v1612+: New Meshing Functionality

23/12/2016

snappyHexMesh: updated locations in mesh

To seed multiple locations as volume regions to be meshed, the locationsInMesh keyword was first introduced in OpenFOAM-v3.0+. This has been improved, and the snappyMultiRegionHeater tutorial updated to show an example of its application.

The case includes five regions, whose locations in mesh are specified using:

locationsInMesh
(
    (( 0.005 0.005  0.005) heater)
    (( 0.05  0.005  0.005) rightSolid)
    ((-0.05  0.005  0.005) leftSolid)
    ((-0.05  0.015  0.005) topAir)
    ((-0.05 -0.015  0.005) bottomAir)
);

For the example case shown, this leads to the following mesh regions:

[Picture]

Source code
$FOAM_UTILITIES/mesh/generation/snappyHexMesh
Examples
$FOAM_TUTORIALS/heatTransfer/chtMultiRegionFoam/snappyMultiRegionHeater

snappyHexMesh: new region support

A new -region option has been added to snappyHexMesh to enable region-wise meshing:

snappyHexMesh -region <regionName>
To apply this option, there must already be a background mesh stored in the directory $FOAM_CASE/constant/<regionName>/polyMesh. This can be achieved by running the blockMesh utility with the -region option

blockMesh -region <regionName>
Note: the fvSolution, fvSchemes and snappyHexMeshDict files must be located in the region directory:

$FOAM_CASE/system/<regionName>

Source code
$FOAM_UTILITIES/mesh/generation/snappyHexMesh
Examples
$FOAM_TUTORIALS/heatTransfer/chtMultiRegionFoam/snappyMultiRegionHeater

Updated renumber mesh utility

The renumberMesh utility has been extended to enable renumbering of set information.

Cell, face and point sets are generated by many pre-processing utilities, typically to gain a more detailed insight into specific mesh regions, or to isolate regions for input into subsequent set-up phases. In prior releases this information was not updated during the renumbering, leading to inconsistent addressing and unpredictable behaviour.

Source code
$FOAM_UTILITIES/mesh/manipulation/renumberMesh

Updated surface check utility

The surfaceCheck utility has been extended to limit excessive output of OBJ files

In previous versions a separate OBJ file was written for each problematic part, with the potential to generate a huge number of files. By default, the utility limits the number of output files to ten. This is controlled using the new -outputThreshold command line option, e.g. for the $FOAM_TUTORIALS/incompressible/simpleFoam/motorBike tutorial the following commands:

surfaceCheck -outputThreshold 0 constant/triSurface/motorBike.obj.gz
will suppress writing any OBJ files.

Source code
$FOAM_UTILITIES/surface/surfaceCheck