In OpenFOAM version 4.0, the ‘non-GUI’ post-processing tools have been unified within a single command line interface (CLI). Post-processing functionality includes data processing, sampling (e.g. probes, graph plotting) visualisation, case control and run-time I/O. Functionality can be executed by:
- conventional post-processing, a data processing activity that occurs after a simulation has run;
- run-time processing, data processing that is performed during the running of a simulation.
Both approaches have advantages. Conventional post-processing allows the user to choose how to analyse data after the results are obtained. Run-time processing offers greater flexibility because it has access to all the data in the database of the run at all times, rather than just the data written during the simulation. It also allows the user to monitor processed data during a simulation and provides a greater level of convenience because the processed results can be available immediately to the user when the simulation ends.
There are 3 methods of post-processing that cover the options described above
- Every solver, e.g. simpleFoam can be configured to include run-time processing.
- The postProcess utility provides conventional post-processing of data written by a simulation.
- Every solver can be run with the -postProcess option, which only executes post-processing, but with additional access to data available on the database for the particular solver.
All modes of post-processing access the same functionality implemented in OpenFOAM in the function object framework. Function objects can be listed by running a solver with the -listFunctionObjects option, e.g.
The list represents the underlying post-processing functionality. Almost all the functionality is packaged into a set of configured tools that are conveniently integrated within the post-processing CLI. Those tools are located in $FOAM_ETC/caseDicts/postProcessing and are listed by running postProcess with the -list option.
This produces a list of tools that are described in the following sections.
- Calculates the Courant Number field from the flux field.
- 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.
- Calculates the Mach Number field from the velocity field.
- Calculates the Peclet Number field from the flux field.
- Calculates the second invariant of the velocity gradient tensor.
- Calculates the Reynolds stress tensor field and stores it on the database.
- Writes the turbulent flame-speed and reaction-rate volScalarFields for the Xi-based combustion models.
- Add a list of fields.
- Writes the component scalar fields (e.g. Ux, Uy, Uz) of a field (e.g. U).
- Calculates the divergence of a field.
- Calculates the enstrophy of the velocity field.
- Calculates and writes the flowType of velocity field where: -1 = rotational flow; 0 = simple shear flow; +1 = planar extensional flow.
- Calculates the gradient of a field.
- Calculates the magnitude of a field.
- Calculates the magnitude-squared of a field.
- Adds a random component to a field, with a specified perturbation magnitude.
- Writes the steam-function pointScalarField, calculated from the specified flux surfaceScalarField.
- From the first field, subtracts the remaining fields in the list.
- Calculates specified turbulence fields and stores it on the database.
- Calculates the vorticity field, i.e. the curl of the velocity field.
- Calculates the shear stress at wall patches, outputting the data as a volVectorField.
- Calculates the heat flux at wall patches, outputting the data as a volVectorField.
- Writes the cell-centres volVectorField and the three component fields as volScalarFields; useful for post-processing thresholding.
- Writes the cell-volumes volScalarField
- Writes out specified objects, e.g. fields, stored on the case database.
- Calculates the turbulence y+, outputting the data as a yPlus field.
- 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.
- 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.
- 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 (ˇ= cell size) for an accurate result.
- 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).
- 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).
- 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).
- Calculates pressure and viscous forces over specified patches for a case where the solver is incompressible (pressure is kinematic, e.g. mˆ2/sˆ2).
- Calculate intensive fields UMean, translationalT, internalT, overallT from averaged extensive fields from a DSMC calculation.
- Writes out the maximum cell value for one or more fields.
- Writes out the minimum cell value for one or more fields.
- Writes out the maximum face value for one or more fields.
- Writes out the minimum face value for one or more fields.
- Writes out the minimum and maximum values, by component for non-scalar fields, and the locations where they occur.
- Writes out the minimum and maximum values, by magnitude for non-scalar fields, and the locations where they occur.
- 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).
- Calculates the difference between the average pressures on 2 specified patches.
- Interpolates pressures onto 2 specified triangulated surfaces and calculates the difference between the average pressures.
- Calculates the pressure field in units M/(LTˆ2) (e.g. Pa) from kinematic pressure by scaling by a specified density.
- Calculates the total pressure field for a case where the solver is compressible (pressure is in units M/(LTˆ2), e.g. Pa).
- Calculates the total pressure field for a case where the solver is incompressible (pressure is kinematic, e.g. mˆ2/sˆ2).
- Writes out values of fields at a cloud of points, interpolated to specified boundary patches.
- 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.
- Writes out values of fields interpolated to a specified cloud of points.
- Writes out values of fields from cells nearest to specified locations.
- Writes out files of streamlines with interpolated field data in VTK format.
- Writes out surface files with interpolated field data in VTK format, e.g. cutting planes, iso-surfaces and patch boundary surfaces.
When a user wishes to process data during a simulation, they need to configure the case accordingly. The configuration process is as follows, using an example of monitoring flow rate at an outlet patch named outlet.
Firstly, the user should include the flowRatePatch function in functions sub-dictionary in the case controlDict file, using the #includeFunc directive.
… other function objects here …
That will include the functionality in the flowRatePatch configuration file, located in the directory hierarchy beginning with $FOAM_ETC/caseDicts/postProcessing.
The configuration of flowRatePatch requires the name of the patch to be supplied. Option 1 for doing this is that the user copies the flowRatePatch file into their case system directory by
and edits the patch name, in the copied file, as outlet. When the solver is run, it will pick up an included function in the local case system directory, in precedence over $FOAM_ETC/caseDicts/postProcessing. The flow rate through the patch will be calculated and written out into a file within a directory named postProcessing. Option 2 for specifying the patch name is to provide the name as an argument to the flowRatePatch in the #includeFunc directive, using the syntax keyword=entry.
… other function objects here …
In the case where the keyword is field or fields, only the entry is needed when specifying an argument to a function. For example, if the user wanted to calculate and write out the magnitude of velocity into time directories during a simulation they could simply add the following to the functions sub-dictionary in controlDict.
… other function objects here …
This works because the function’s argument U is represented by the keyword field, see $FOAM_ETC/caseDicts/postProcessing/fields/mag.
Some functions require the setting of many parameters, e.g. forces, forceCoeffs, surfaces, etc. For those functions, it is more reliable and convenient to copy and configure the function using option 1 (above) rather than through arguments.
The user can execute post-processing functions after the simulation is complete using the postProcess utility. Let us illustrate the use of postProcess using the pitzDaily case from the tutorials directory. The case can be copied, e.g. into the user’s run directory; the user can then go into the case directory, generate the mesh with blockMesh and then run simpleFoam
cp -r $FOAM_TUTORIALS/incompressible/simpleFoam/pitzDaily .
Now the user can run execute post-processing functions with postProcess. The -help option provides a summary of its use.
Simple functions like mag can be executed using the -func option; text on the command line generally needs to be quoted ("…") if it contains punctuation characters.
This operation calculates and writes the field of magnitude of velocity into a file named mag(U) in each time directory. Similarly, the flowRatePatch example can be executed using postProcess.
Let us say the user now wants to calculate total pressure for incompressible flow with kinematic pressure, . The function is available, named totalPressureIncompressible, which the user could attempt first to run as follows.
This returns the following error message.
The error message is telling the user that the pressure field p is not loaded; the same is true of the velocity field U. For the function to work, both fields can be loaded as comma separated arguments.
Alternatively the user can load a space separated list of fields using the -fields option, which the function can access.
Both options work effectively because the pressure and velocity data is available directly from the files, p and U.
A more complex example is calculating wall shear stress using the wallShearStress function.
Even loading relevant fields, the post-processing fails with the following message.
Unable to find turbulence model in the database
The message is telling us that the postProcess utility has not constructed the necessary models that the solver, simpleFoam, used when running the simulation, i.e. a turbulence model. This is a situation where we need to post-process (as opposed to run-time process) using the solver with the -postProcess option so that the modelling will be available that the post-processing function needs. Help for this operation can be printed with the following command.
It can be seen that the options for a solver with -postProcess are the same as when running postProcess utility. This means that the -func option can be used to execute the wallShearStress function effectively.
Note that no fields need to be supplied, either by function arguments ”(p,U)” or using ”-fields (p U)”, because simpleFoam itself constructs and stores the required fields. Functions can also be selected by the #includeFunc directive in functions in the controlDict file, instead of the -func option.