In OpenFOAM, directories play a crucial role in organizing files and data for simulations. Here's an overview of common directories and their meanings:
Case Directory: This is the main folder for a specific simulation case. It contains all the files related to that simulation.
0 (Zero Directory): Contains initial conditions for the simulation. Files here specify the starting values for variables (e.g., velocity, pressure) at time zero.
constant Directory: Holds files related to the physical properties of the simulation. This includes:
transportProperties: Defines fluid properties like viscosity and density.
turbulenceProperties: Specifies turbulence models and parameters.
system Directory: Contains files that control the simulation execution, including:
controlDict: Manages the simulation time, output frequency, and solver settings.
fvSchemes: Defines numerical schemes for discretization.
fvSolution: Contains solver settings and tolerances.
Post-processing Directories: After running a simulation, results can be processed and visualized. Directories like results or output might be used for storing processed data.
Allrun and Allclean Scripts: Often found in the case directory, these scripts automate the running and cleaning processes for simulations.
Understanding these directories is essential for effectively using OpenFOAM, as each serves a specific purpose in the overall workflow of setting up, running, and analyzing simulations.
Usage: fluentMeshToFoam [OPTIONS] <Fluent mesh file> options: -2D <thickness> use when converting a 2-D mesh (applied before scale) -case <dir> specify alternate case directory, default is the cwd -fileHandler <handler> override the fileHandler -libs <(lib1 .. libN)> pre-load libraries -noFunctionObjects do not execute functionObjects -scale <factor> geometry scaling factor - default is 1 -writeSets write cell zones and patches as sets -writeZones write cell zones as zones -srcDoc display source code in browser -doc display application documentation in browser -help print the usage
Using: OpenFOAM-8 (see https://openfoam.org) Build: 8
Usage: fluent3DMeshToFoam [OPTIONS] <Fluent mesh file> options: -case <dir> specify alternate case directory, default is the cwd -cubit special parsing of (incorrect) cubit files -fileHandler <handler> override the fileHandler -ignoreCellGroups <names> specify cell groups to ignore -ignoreFaceGroups <names> specify face groups to ignore -includedAngle <angle> feature angle with which to split cyclics -libs <(lib1 .. libN)> pre-load libraries -noFunctionObjects do not execute functionObjects -scale <factor> geometry scaling factor - default is 1 -srcDoc display source code in browser -doc display application documentation in browser -help print the usage
Using: OpenFOAM-8 (see https://openfoam.org) Build: 8
Here's how to convert a .msh file to OpenFOAM format using fluentMeshToFoam:
Create a new empty directory for your case:
1 2
mkdir supersonic cd supersonic
Create the basic OpenFOAM directory structure:
1 2
mkdir constant mkdir system
and prepare all requried files,
Copy your .msh file to the case directory:
1 2 3 4
$ file supersonic_injet-stead.msh supersonic_injet-stead.msh: ASCII text
Mesh stats points: 20850 internal points: 0 faces: 40964 internal faces: 20116 cells: 10180 faces per cell: 6 boundary patches: 7 point zones: 0 face zones: 1 cell zones: 1
Overall number of cells of each type: hexahedra: 10180 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 0
Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK).
Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology inlet1 56 114 ok (non-closed singly connected) inlet2 2 6 ok (non-closed singly connected) top 182 366 ok (non-closed singly connected) outlet 56 114 ok (non-closed singly connected) bottom 180 364 ok (non-closed singly connected) obstacle 12 28 ok (non-closed singly connected) frontandback 20360 20850 ok (non-closed singly connected)
Checking geometry... Overall domain bounding box (-1.33333 0 0) (3 1 1) Mesh has 3 geometric (non-empty/wedge) directions (1 1 1) Mesh has 3 solution (non-empty) directions (1 1 1) Boundary openness (2.3102e-17 -4.76257e-17 4.86259e-16) OK. Max cell openness = 1.0842e-16 OK. Max aspect ratio = 62.3378 OK. Minimum face area = 0.00026736. Maximum face area = 0.03. Face area magnitudes OK. Min volume = 0.00026736. Max volume = 0.00054. Total volume = 4.32833. Cell volumes OK. Mesh non-orthogonality Max: 0 average: 0 Non-orthogonality check OK. Face pyramids OK. Max skewness = 5.92121e-14 OK. Coupled point location match (average 0) OK.
Mesh OK.
End
After conversion, you'll have: - constant/polyMesh/ directory containing the mesh files - Basic OpenFOAM mesh files: points, faces, cells, boundary, etc.
4 Comparison between fluentMeshToFoam and fluent3DMeshToFoam
From the release notes for OpenFOAM 1.4.1:
New fluent3DMeshToFoam converter for 3D meshes from Fluent format to OpenFOAM format including full support for all BCs, zones etc.;
Comparing the source code for fluentMeshToFoam and fluent3DMeshToFoam in OpenFOAM 1.4.1 and 1.5, the following main differences can be found:
fluentMeshToFoam supports 2D and 3D Fluent meshes, while fluent3DMeshToFoam only supports 3D.
fluent3DMeshToFoam deals with hanging nodes.
fluentMeshToFoam has the options to write sets and zones, while fluent3DMeshToFoam has the option to ignore a cell groups and face groups.
fluentMeshToFoam can only handle the following 3D cell types: tet, hex, pyramid, prism
fluent3DMeshToFoam can handle internal walls/patches, or at least it looks like it does. fluentMeshToFoam requires a workaround: Howto importing fluent mesh with internal walls
