My first tutorial: pythonPalIcoFoam

You can watch a short videotutorial for this case, here.

In this tutorial, we create a modified version of icoFoam called pythonPalIcoFoam, where we use pythonPal to calculate the specific kinetic energy, \(k = \frac {1}{2} U \cdot U\)

Provided that pybind11 is installed (see installing), the steps to go from icoFoam to pythonPalIcoFoam are:

• Copy the icoFoam directory to a directory pythonPalIcoFoam, then rename the .C file inside it and the C file and executable file names inside Make/files ( Just replace icoFoam with pythonPalIcoFoam).

• Copy the pythonPal.H file to the pythonPalIcoFoam directory.

• Include pythonPal.H at the top of pythonPalIcoFoam.C;

#include "pythonPal.H"

• In createFields.H, construct a volScalarField called k, initialised to zero;

volScalarField k
(
    IOobject
    (
        "k",
        mesh.time().timeName(),
        mesh,
        IOobject::READ_IF_PRESENT,
        IOobject::AUTO_WRITE
    ),
    mesh,
    dimensionedScalar("k", dimensionSet(0, 2, -2, 0, 0, 0, 0), 0.0)
);

• In the parent folder, create a Python file and define a function that receives the U field from OpenFOAM and calculates k. We called that file python_script.py and the function calculatek.

def calculatek(field):
  return np.sum(field * field, axis = 1)[:, np.newaxis] / 2

• In pythonPalIcoFoam.C, create an object of type pythonPal and load the Python file python_script.py:

pythonPal myPythonPal("python_script.py", true);

• At the end of the time-loop, pass the U and k fields to Python via pythonPal:

myPythonPal.passToPython(U, "U");
myPythonPal.passToPython(k, "k");

• Calculate k via pythonPal:

myPythonPal.execute("k[:, :] = calculatek(U)");

• Finally, write the k field to disk, e.g. for viewing in ParaView.

k.write();

Figure shows the cavity case's velocity magnitude and specific kinetic energy field results.

To learn more about how pythonPal works, see How Does It Work?.