OpenFOAM v11 User Guide

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

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

7.3 Post-processing functionality

The packaged function objects are catalogued in this section. Each packaged function object is a conﬁguration ﬁle stored in $FOAM_ETC/caseDicts/postProcessing. As a reminder, they can be listed by the following command.

foamPostProcess -list

7.3.1 Field calculation

age: Calculates and writes out the time taken for a particle to travel from an inlet to the location.
components: Writes the component scalar ﬁelds (e.g. Ux, Uy, Uz) of a ﬁeld (e.g. U).
CourantNo: Calculates the Courant Number ﬁeld from the ﬂux ﬁeld.
ddt: Calculates the Eulerian time derivative of a ﬁeld.
div: Calculates the divergence of a ﬁeld.
enstrophy: Calculates the enstrophy of the velocity ﬁeld.
ﬁeldAverage: Calculates and writes the time averages of a given list of ﬁelds.
ﬂowType: Calculates and writes the flowType of velocity ﬁeld where: -1 = rotational ﬂow; 0 = simple shear ﬂow; +1 = planar extensional ﬂow.
grad: Calculates the gradient of a ﬁeld.
Lambda2: Calculates and writes the second largest eigenvalue of the sum of the square of the symmetrical and anti-symmetrical parts of the velocity gradient tensor.
log: Calculates the natural logarithm of the speciﬁed scalar ﬁeld.
MachNo: Calculates the Mach Number ﬁeld from the velocity ﬁeld.
mag: Calculates the magnitude of a ﬁeld.
magSqr: Calculates the magnitude-squared of a ﬁeld.
massFractions: Calculates mass-fraction ﬁelds from mole-fraction ﬁelds, or moles ﬁelds, and a multi-component thermophysical model.
moleFractions: Calculates mole-fraction ﬁelds from the mass-fraction ﬁelds of a multi-component thermophysical model.
PecletNo: Calculates the Peclet Number ﬁeld from the ﬂux ﬁeld.
Q: Calculates the second invariant of the velocity gradient tensor.
randomise: Adds a random component to a ﬁeld, with a speciﬁed perturbation magnitude.
reconstruct: Calculates the reconstruction of a ﬁeld; e.g. to construct a cell-centred velocity U from the face-centred ﬂux phi.
scale: Multiplies a ﬁeld by a scale factor
shearStress: Calculates the shear stress, outputting the data as a volSymmTensorField.
streamFunction: Writes the stream-function pointScalarField, calculated from the speciﬁed ﬂux surfaceScalarField.
surfaceInterpolate: Calculates the surface interpolation of a ﬁeld.
totalEnthalpy: Calculates and writes the total enthalpy $\text{[math]}$ as the volScalarField $\text{[math]}$ .
turbulenceFields: Calculates speciﬁed turbulence ﬁelds and stores it on the database.
turbulenceIntensity: Calculates and writes the turbulence intensity ﬁeld I.
vorticity: Calculates the vorticity ﬁeld, i.e. the curl of the velocity ﬁeld.
wallHeatFlux: Calculates the heat ﬂux at wall patches, outputting the data as a volVectorField.
wallHeatTransferCoeﬀ: Calculates the estimated incompressible ﬂow heat transfer coeﬃcient at wall patches, outputting the data as a volScalarField.
wallShearStress: Calculates the shear stress at wall patches, outputting the data as a volVectorField.
writeCellCentres: Writes the cell-centres volVectorField and the three component ﬁelds as volScalarFields; useful for post-processing thresholding.
writeCellVolumes: Writes the cell-volumes volScalarField
writeVTK: Writes out speciﬁed objects in VTK format, e.g. ﬁelds, stored on the case database.
yPlus: Calculates the turbulence y+, outputting the data as a yPlus ﬁeld.

7.3.2 Field operations

add: Add a list of ﬁelds.
divide: From the ﬁrst ﬁeld, divide the remaining ﬁelds in the list.
multiply: Multiply a list of ﬁelds.
subtract: From the ﬁrst ﬁeld, subtracts the remaining ﬁelds in the list.
uniform: Create a uniform ﬁeld.

7.3.3 Forces and force coeﬃcients

forceCoeﬀsCompressible: Calculates lift, drag and moment coeﬃcients by summing forces on speciﬁed patches for a case where the solver is compressible (pressure is in units M/(LTˆ2), e.g. Pa).
forceCoeﬀsIncompressible: Calculates lift, drag and moment coeﬃcients by summing forces on speciﬁed patches for a case where the solver is incompressible (pressure is kinematic, e.g. mˆ2/sˆ2).
forcesCompressible: Calculates pressure and viscous forces over speciﬁed patches for a case where the solver is compressible (pressure is in units M/(LTˆ2), e.g. Pa).
forcesIncompressible: Calculates pressure and viscous forces over speciﬁed patches for a case where the solver is incompressible (pressure is kinematic, e.g. mˆ2/sˆ2).

7.3.4 Sampling for graph plotting

graphCell: Writes graph data for speciﬁed ﬁelds along a line, speciﬁed by start and end points. One graph point is generated in each cell that the line intersects.
graphUniform: Writes graph data for speciﬁed ﬁelds along a line, speciﬁed by start and end points. A speciﬁed number of graph points are used, distributed uniformly along the line.
graphCellFace: Writes graph data for speciﬁed ﬁelds along a line, speciﬁed by start and end points. One graph point is generated on each face and in each cell that the line intersects.
graphFace: Writes graph data for speciﬁed ﬁelds along a line, speciﬁed by start and end points. One graph point is generated on each face that the line intersects.
graphLayerAverage: Generates plots of ﬁelds averaged over the layers in the mesh.
graphPatchCutLayerAverage: Writes graphs of patch face values, area-averaged in planes perpendicular to a given direction. It adaptively grades the distribution of graph points to match the resolution of the mesh

7.3.5 Lagrangian data

dsmcFields: Calculate intensive ﬁelds UMean, translationalT, internalT, overallT from averaged extensive ﬁelds from a DSMC calculation.
stopAtEmptyClouds: Stops the run when all clouds are empty, i.e. have no particles.

7.3.6 Volume ﬁelds

cellMax: Writes out the maximum cell value for one or more ﬁelds.
cellMaxMag: Writes out the maximum cell value magnitude for one or more ﬁelds.
cellMin: Writes out the minimum cell value for one or more ﬁelds.
cellMinMag: Writes out the maximum cell value magnitude for one or more ﬁelds.
volAverage: Writes out the volume-weighted average of one or more ﬁelds.
volIntegrate: Writes out the volume integral of one or more ﬁelds.

7.3.7 Numerical data

residuals: For speciﬁed ﬁelds, writes out the initial residuals for the ﬁrst solution of each time step; for non-scalar ﬁelds (e.g. vectors), writes the largest of the residuals for each component (e.g. x, y, z).

7.3.8 Control

adjustTimeStepToChemistry: Adjusts the time step to a chemistry model’s bulk chemical time scales
adjustTimeStepToCombustion: Adjusts the time step to a combustion model’s bulk reaction time scales
stopAtClockTime: Stops the run when the speciﬁed clock time in second has been reached and optionally write results before stopping.
stopAtFile: Stops the run when the ﬁle stop is created in the case directory.
stopAtTimeStep: Stops the run if the time-step drops below the speciﬁed value in seconds and optionally write results before stopping.
time: Writes run time, CPU time and clock time and optionally the CPU and clock times per time step.
timeStep: Writes the time step to a ﬁle for monitoring.
writeObjects: Writes out speciﬁed objects, e.g. ﬁelds, stored on the case database.

7.3.9 Pressure tools

staticPressureIncompressible: Calculates the pressure ﬁeld in normal units, i.e. Pa in SI, from kinematic pressure by scaling by a speciﬁed density.
totalPressureCompressible: Calculates the total pressure ﬁeld in normal units, i.e. Pa in SI, for a case where the solver is compressible.
totalPressureIncompressible: Calculates the total pressure ﬁeld for a case where the solver is incompressible, in kinematic units, i.e. $\text{[math]}$ in SI.

7.3.10 Combustion

Qdot: Calculates and outputs the heat release rate for the current combustion model.
XiReactionRate: Writes the turbulent ﬂame-speed and reaction-rate volScalarFields for the Xi-based combustion models.

7.3.11 Multiphase

populationBalanceMoments: Calculates and writes out integral (integer moments) or mean properties (mean, variance, standard deviation) of a size distribution computed with multiphaseEulerFoam. Requires solver post-processing.
phaseForces: Calculates the blended interfacial forces acting on a given phase, i.e. drag, virtual mass, lift, wall-lubrication and turbulent dispersion. Note that it works only in solver post-processing mode and in combination with multiphaseEulerFoam. For a simulation involving more than two phases, the accumulated force is calculated by looping over all phasePairs the phase is a part of.
phaseMap: Writes the phase-fraction map ﬁeld alpha.map with incremental value ranges for each phase e.g., with values 0 for water, 1 for air, 2 for oil, etc.
populationBalanceSizeDistribution: Writes out the size distribution computed with multiphaseEulerFoam for the entire domain or a volume region. Requires solver post-processing.
wallBoilingProperties: Looks up wall boiling wall functions and collects and writes out out ﬁelds of bubble departure diameter, bubble departure frequency, nucleation site density, eﬀective liquid fraction at the wall, quenching heat ﬂux, and evaporative heat ﬂux.

7.3.12 Probes

boundaryProbes: Writes out values of ﬁelds at a cloud of points, interpolated to speciﬁed boundary patches.
interfaceHeight: Reports the height of the interface above a set of locations. For each location, it writes the vertical distance of the interface above both the location and the lowest boundary. It also writes the point on the interface from which these heights are computed.
internalProbes: Writes out values of ﬁelds interpolated to a speciﬁed cloud of points.
probes: Writes out values of ﬁelds from cells nearest to speciﬁed locations.

7.3.13 Surface ﬁelds

faceZoneAverage: Calculates the average value of one or more ﬁelds on a faceZone.
faceZoneFlowRate: Calculates the ﬂow rate through a speciﬁed face zone by summing the ﬂux on patch faces. For solvers where the ﬂux is volumetric, the ﬂow rate is volumetric; where ﬂux is mass ﬂux, the ﬂow rate is mass ﬂow rate.
patchAverage: Calculates the average value of one or more ﬁelds on a patch.
patchDiﬀerence: Calculates the diﬀerence between the average values of ﬁelds on two speciﬁed patches. Calculates the average value of one or more ﬁelds on a patch.
patchFlowRate: Calculates the ﬂow rate through a speciﬁed patch by summing the ﬂux on patch faces. For solvers where the ﬂux is volumetric, the ﬂow rate is volumetric; where ﬂux is mass ﬂux, the ﬂow rate is mass ﬂow rate.
patchIntegrate: Calculates the surface integral of one or more ﬁelds on a patch.
triSurfaceAverage: Calculates the average on a speciﬁed triangulated surface by interpolating onto the triangles and integrating over the surface area. Triangles need to be small (¡= cell size) for an accurate result.
triSurfaceDiﬀerence: Calculates the diﬀerence between the average values of ﬁelds on two speciﬁed triangulated surfaces.
triSurfaceVolumetricFlowRate: Calculates volumetric ﬂow rate through a speciﬁed triangulated surface by interpolating velocity onto the triangles and integrating over the surface area. Triangles need to be small (¡= cell size) for an accurate result.

7.3.14 Meshing

checkMesh: Executes primitiveMesh::checkMesh to check the distortion of moving meshes.

7.3.15 ‘Pluggable’ solvers

particles: Tracks a cloud of parcels driven by the ﬂow of the continuous phase.
phaseScalarTransport: Solves a transport equation for a scalar ﬁeld within one phase of a multiphase simulation.
scalarTransport: Solves a transport equation for a scalar ﬁeld.

7.3.16 Visualisation tools

cutPlaneSurface: Writes out cut-plane surface ﬁles with interpolated ﬁeld data in VTK format.
isoSurface: Writes out iso-surface ﬁles with interpolated ﬁeld data in VTK format.
patchSurface: Writes out patch surface ﬁles with interpolated ﬁeld data in VTK format.
streamlinesLine: Writes out ﬁles of stream lines with interpolated ﬁeld data in VTK format, with initial points uniformly distributed along a line.
streamlinesPatch: Writes out ﬁles of stream lines with interpolated ﬁeld data in VTK format, with initial points randomly selected within a patch.
streamlinesPoints: Writes out ﬁles of stream lines with interpolated ﬁeld data in VTK format, with speciﬁed initial points.
streamlinesSphere: Writes out ﬁles of stream lines with interpolated ﬁeld data in VTK format, with initial points randomly selected within a sphere.

OpenFOAM v11 User Guide - 7.3 Post-processing functionality