OpenFOAM v12 User Guide

[version 12][version 11][version 10][version 9][version 8][version 7][version 6]

[chapter contents][previous topic][next topic][index]

3.7 Standard utilities

The utilities with the OpenFOAM distribution are in the $FOAM_UTILITIES directory. The names are reasonably descriptive, e.g. ideasToFoam converts mesh data from the format written by I-DEAS to the OpenFOAM format. The descriptions of current utilities distributed with OpenFOAM are given in the following sections.

3.7.1 Pre-processing

applyBoundaryLayer: Apply a simpliﬁed boundary-layer model to the velocity and turbulence ﬁelds based on the 1/7th power-law.
boxTurb: Makes a box of turbulence which conforms to a given energy spectrum and is divergence free.
changeDictionary: Utility to change dictionary entries, e.g. can be used to change the patch type in the ﬁeld and polyMesh/boundary ﬁles.
createExternalCoupledPatchGeometry: Application to generate the patch geometry (points and faces) for use with the externalCoupled boundary condition.
dsmcInitialise: Initialise a case for dsmcFoam by reading the initialisation dictionary system/dsmcInitialise.
engineSwirl: Generates a swirling ﬂow for engine calculations.
faceAgglomerate: Agglomerate boundary faces using the pairPatchAgglomeration algorithm. It writes a map from the ﬁne to coarse grid.
foamSetupCHT: Sets up a multi-region case using template ﬁles for material properties, ﬁeld and system ﬁles.
mapFields: Maps volume ﬁelds from one mesh to another, reading and interpolating all ﬁelds present in the time directory of both cases.
mapFieldsPar: Maps volume ﬁelds from one mesh to another, reading and interpolating all ﬁelds present in the time directory of both cases. Parallel and non-parallel cases are handled without the need to reconstruct them ﬁrst.
mdInitialise: Initialises ﬁelds for a molecular dynamics (MD) simulation.
setAtmBoundaryLayer: Applies atmospheric boundary layer models to the entire domain for case initialisation.
setFields: Set values on a selected set of cells/patchfaces through a dictionary.
setWaves: Applies wave models to the entire domain for case initialisation using level sets for second-order accuracy.
snappyHexMeshConﬁg: Preconﬁgures blockMeshDict, surfaceFeaturesDict and snappyHexMeshDict ﬁles based on the case surface geometry ﬁles.
viewFactorsGen: View factors are calculated based on a face agglomeration array (finalAgglom generated by faceAgglomerate utility).

3.7.2 Mesh generation

blockMesh: A multi-block mesh generator.
extrudeMesh: Extrude mesh from existing patch (by default outwards facing normals; optional ﬂips faces) or from patch read from ﬁle.
extrude2DMesh: Takes 2D mesh (all faces 2 points only, no front and back faces) and creates a 3D mesh by extruding with speciﬁed thickness.
extrudeToRegionMesh: Extrude faceZones (internal or boundary faces) or faceSets (boundary faces only) into a separate mesh (as a diﬀerent region).
snappyHexMesh: Automatic split hex mesher. Reﬁnes and snaps to surface.
zeroDimensionalMesh: Creates a zero-dimensional mesh.

3.7.3 Mesh conversion

ansysToFoam: Converts an ANSYS input mesh ﬁle, exported from I-DEAS, to OpenFOAM format.
ccm26ToFoam: Reads CCM ﬁles as written by Prostar/ccm using ccm 2.6
cfx4ToFoam: Converts a CFX 4 mesh to OpenFOAM format.
datToFoam: Reads in a datToFoam mesh ﬁle and outputs a points ﬁle. Used in conjunction with blockMesh.
ﬂuent3DMeshToFoam: Converts a Fluent mesh to OpenFOAM format.
ﬂuentMeshToFoam: Converts a Fluent mesh to OpenFOAM format including multiple region and region boundary handling.
foamMeshToFluent: Writes out the OpenFOAM mesh in Fluent mesh format.
foamToStarMesh: Reads an OpenFOAM mesh and writes a pro-STAR (v4) bnd/cel/vrt format.
foamToSurface: Reads an OpenFOAM mesh and writes the boundaries in a surface format.
gambitToFoam: Converts a GAMBIT mesh to OpenFOAM format.
gmshToFoam: Reads .msh ﬁle as written by Gmsh.
ideasUnvToFoam: I-Deas unv format mesh conversion.
kivaToFoam: Converts a KIVA3v grid to OpenFOAM format.
mshToFoam: Converts .msh ﬁle generated by the Adventure system.
netgenNeutralToFoam: Converts neutral ﬁle format as written by Netgen v4.4.
plot3dToFoam: Plot3d mesh (ascii/formatted format) converter.
sammToFoam: Converts a Star-CD (v3) SAMM mesh to OpenFOAM format.
star3ToFoam: Converts a Star-CD (v3) pro-STAR mesh into OpenFOAM format.
star4ToFoam: Converts a Star-CD (v4) pro-STAR mesh into OpenFOAM format.
tetgenToFoam: Converts .ele and .node and .face ﬁles, written by tetgen.
vtkUnstructuredToFoam: Converts ascii .vtk (legacy format) ﬁle generated by vtk/paraview.
writeMeshObj: For mesh debugging, writes mesh as three separate OBJ ﬁles for visualisation.

3.7.4 Mesh manipulation

autoPatch: Divides external faces into patches based on (user supplied) feature angle.
checkMesh: Checks validity of a mesh.
createBaﬄes: Makes internal faces into boundary faces. Does not duplicate points.
createEngineZones: Utility to create the cylinder head and piston bowl pointZones.
createNonConformalCouples: Utility to create non-conformal couples between non-coupled patches.
createPatch: Utility to create patches out of selected boundary faces. Faces come either from existing patches or from a faceSet.
deformedGeom: Deforms a polyMesh using a displacement ﬁeld U and a scaling factor supplied as an argument.
ﬂattenMesh: Flattens the front and back planes of a 2D cartesian mesh.
insideCells: Picks up cells with cell centre ’inside’ of surface. Requires surface to be closed and singly connected.
mergeBaﬄes: Detects faces that share points (baﬄes) and merges them into internal faces.
mergeMeshes: Merges two meshes.
mirrorMesh: Mirrors a mesh around a given plane.
moveMesh: Mesh motion and topological mesh changes utility.
objToVTK: Read obj line (not surface!) ﬁle and convert into vtk.
orientFaceZone: Corrects orientation of faceZone.
polyDualMesh: Calculates the dual of a polyMesh. Adheres to all the feature and patch edges.
reﬁneMesh: Utility to reﬁne cells in multiple directions.
renumberMesh: Renumbers the cell list in order to reduce the bandwidth, reading and renumbering all ﬁelds from all the time directories.
reorderPatches: Utility to reorder the patches of a case
setsToZones: Add pointZones, faceZones or cellZones to the mesh from similar named pointSets, faceSets or cellSets.
singleCellMesh: Reads all ﬁelds and maps them to a mesh with all internal faces removed (singleCellFvMesh) which gets written to region singleCell.
splitBaﬄes: Detects faces that share points (baﬄes) and duplicates the points to separate them.
splitMeshRegions: Splits mesh into multiple regions.
stitchMesh: Stitches a mesh.
subsetMesh: Selects a section of mesh based on a cellSet.
topoSet: Operates on cellSets/faceSets/pointSets through a dictionary.
transformPoints: Transforms the mesh points in the polyMesh directory according to the translate, rotate and scale options.
zipUpMesh: Reads in a mesh with hanging vertices and zips up the cells to guarantee that all polyhedral cells of valid shape are closed.

3.7.5 Other mesh tools

autoReﬁneMesh: Utility to reﬁne cells near to a surface.
collapseEdges: Collapses short edges and combines edges that are in line.
combinePatchFaces: Checks for multiple patch faces on same cell and combines them. Multiple patch faces can result from e.g. removal of reﬁned neighbouring cells, leaving 4 exposed faces with same owner.
PDRMesh: Mesh and ﬁeld preparation utility for PDR type simulations.
reﬁneHexMesh: Reﬁnes a hex mesh by 2x2x2 cell splitting.
reﬁnementLevel: Tries to ﬁgure out what the reﬁnement level is on reﬁned Cartesian meshes. Run BEFORE snapping.
reﬁneWallLayer: Utility to reﬁne cells next to patches.
removeFaces: Utility to remove faces (combines cells on both sides).
selectCells: Select cells in relation to surface.
splitCells: Utility to split cells with ﬂat faces.

3.7.6 Post-processing

engineCompRatio: Calculate the geometric compression ratio. Note that if you have valves and/or extra volumes it will not work, since it calculates the volume at BDC and TCD.
foamPostProcess: Execute the set of functionObjects speciﬁed in the selected dictionary (which defaults to system/controlDict) or on the command-line for the selected set of times on the selected set of ﬁelds.
noise: Utility to perform noise analysis of pressure data using the noiseFFT library.
pdfPlot: Generates a graph of a probability distribution function.
temporalInterpolate: Interpolate ﬁelds between time-steps e.g. for animation.

3.7.7 Post-processing data converters

foamDataToFluent: Translates OpenFOAM data to Fluent format.
foamToEnsight: Translates OpenFOAM data to EnSight format.
foamToEnsightParts: Translates OpenFOAM data to Ensight format. An Ensight part is created for each cellZone and patch.
foamToGMV: Translates foam output to GMV readable ﬁles.
foamToTetDualMesh: Converts polyMesh results to tetDualMesh.
foamToVTK: Legacy VTK ﬁle format writer.
smapToFoam: Translates a STAR-CD SMAP data ﬁle into OpenFOAM ﬁeld format.

3.7.8 Surface mesh (e.g. OBJ/STL) tools

surfaceAdd: Add two surfaces. Does geometric merge on points. Does not check for overlapping/intersecting triangles.
surfaceAutoPatch: Patches surface according to feature angle. Like autoPatch.
surfaceBooleanFeatures: Generates the extendedFeatureEdgeMesh for the interface between a boolean operation on two surfaces. Assumes that the orientation of the surfaces is correct.
surfaceCheck: Checks geometric and topological quality of a surface.
surfaceClean: Removes baﬄes - collapses small edges, removing triangles. - converts sliver triangles into split edges by projecting point onto base of triangle.
surfaceCoarsen: Surface coarsening using bunnylod
surfaceConvert: Converts from one surface mesh format to another.
surfaceFeatureConvert: Convert between edgeMesh formats.
surfaceFeatures: Identiﬁes features in a surface geometry and writes them to ﬁle, based on control parameters speciﬁed by the user.
surfaceFind: Finds nearest face and vertex.
surfaceHookUp: Find close open edges and stitches the surface along them
surfaceInertia: Calculates the inertia tensor, principal axes and moments of a command line speciﬁed triSurface. Inertia can either be of the solid body or of a thin shell.
surfaceLambdaMuSmooth: Smooths a surface using lambda/mu smoothing.
surfaceMeshConvert: Converts between surface formats with optional scaling or transformations (rotate/translate) on a coordinateSystem.
surfaceMeshExport: Export from surfMesh to various third-party surface formats with optional scaling or transformations (rotate/translate) on a coordinateSystem.
surfaceMeshImport: Import from various third-party surface formats into surfMesh with optional scaling or transformations (rotate/translate) on a coordinateSystem.
surfaceMeshInfo: Miscellaneous information about surface meshes.
surfaceMeshTriangulate: Extracts surface from a polyMesh. Depending on output surface format triangulates faces.
surfaceOrient: Set normal consistent with respect to a user provided ‘outside’ point. If the -inside option is used the point is considered inside.
surfacePointMerge: Merges points on surface if they are within absolute distance. Since absolute distance use with care!
surfaceRedistributePar: (Re)distribution of triSurface. Either takes an non-decomposed surface or an already decomposed surface and redistributes it so that each processor has all triangles that overlap its mesh.
surfaceReﬁneRedGreen: Reﬁne by splitting all three edges of triangle (‘red’ reﬁnement). Neighbouring triangles which are not marked for reﬁnement get split in half (‘green’ reﬁnement).
surfaceSplitByPatch: Writes regions of triSurface to separate ﬁles.
surfaceSplitByTopology: Strips any baﬄe parts of a surface. A baﬄe region is one which is reached by walking from an open edge, and stopping when a multiply connected edge is reached.
surfaceSplitNonManifolds: Takes multiply connected surface and tries to split surface at multiply connected edges by duplicating points. Introduces concept of - borderEdge. Edge with 4 faces connected to it. - borderPoint. Point connected to exactly 2 borderEdges. - borderLine. Connected list of borderEdges.
surfaceSubset: A surface analysis tool which sub-sets the triSurface to choose only a part of interest. Based on subsetMesh.
surfaceToPatch: Reads surface and applies surface regioning to a mesh. Uses boundaryMesh to do the hard work.
surfaceTransformPoints: Transform (scale/rotate) a surface. Like transformPoints but for surfaces.

3.7.9 Parallel processing

decomposePar: Automatically decomposes a mesh and ﬁelds of a case for parallel execution of OpenFOAM.
reconstructPar: Reconstructs ﬁelds of a case that is decomposed for parallel execution of OpenFOAM.
redistributePar: Redistributes existing decomposed mesh and ﬁelds according to the current settings in the decomposeParDict ﬁle.

3.7.10 Thermophysical-related utilities

adiabaticFlameT: Calculates the adiabatic ﬂame temperature for a given fuel over a range of unburnt temperatures and equivalence ratios.
chemkinToFoam: Converts CHEMKINIII thermodynamics and reaction data ﬁles into OpenFOAM format.
equilibriumCO: Calculates the equilibrium level of carbon monoxide.
equilibriumFlameT: Calculates the equilibrium ﬂame temperature for a given fuel and pressure for a range of unburnt gas temperatures and equivalence ratios; the eﬀects of dissociation on O2, H2O and CO2 are included.
mixtureAdiabaticFlameT: Calculates the adiabatic ﬂame temperature for a given mixture at a given temperature.

3.7.11 Miscellaneous utilities

foamDictionary: Interrogates and manipulates dictionaries.
foamFormatConvert: Converts all IOobjects associated with a case into the format speciﬁed in the controlDict.
foamListTimes: List times using timeSelector.
foamToC: Run-time selection table of contents printing and interrogation.
patchSummary: Writes ﬁelds and boundary condition info for each patch at each requested time instance.

OpenFOAM v12 User Guide - 3.7 Standard utilities