# Recent changes in the basics of the OpenFOAM solvers

 constrainHbyA

The boundary conditions of HbyA are now constrained by the new “constrainHbyA” function which applies the velocity boundary values for patches for which the velocity cannot be modified by assignment and pressure extrapolation is not specified via the new
“fixedFluxExtrapolatedPressureFvPatchScalarField”.

The member function assignable() is defined in the abstract base class of boundary conditions (fvPatchField):

It is overridden in the basic boundary condition classes (fixedValue, mixed, directionMixed and sliced):

 fvc::flux and dotInterpolate

dotInterpolate interpolates the field and “dots” the resulting face-values with the vector field provided which removes the need to create a temporary field for the interpolate. This reduces the peak storage of OpenFOAM caused by the divergence of the gradient of vector fields, improves memory management and under some conditions decreases run-time.

This development is based on a patch contributed by Paul Edwards, Intel.

 constrainPressure

In the case of compressible flow, the following relation \eqref{eq:1} holds for the velocity on the face:

\rho \boldsymbol{U}_f \cdot \boldsymbol{S}_f = \left(\frac{\rho \boldsymbol{H}}{A_p}\right)_f \cdot \boldsymbol{S}_f\;-\;\left(\frac{\rho}{A_p}\right)_f (\nabla p)_f \cdot \boldsymbol{S}_f. \tag{1} \label{eq:1}

Thus

(\nabla p)_f \cdot \boldsymbol{n}_f = \frac{1}{|\boldsymbol{S}_f|\left(\frac{\rho}{A_p}\right)_f} \left(\left(\frac{\rho \boldsymbol{H}}{A_p}\right)_f \cdot \boldsymbol{S}_f\;-\;\rho \boldsymbol{U}_f \cdot \boldsymbol{S}_f \right). \tag{2} \label{eq:2}

The fixedFluxPressure boundary condition calculates the boundary normal gradient of the pressure field using the Eq. \eqref{eq:2} so that the boundary fluxes satisfy the Eq. \eqref{eq:1}.

## Author: fumiya

CFD engineer in Japan

This site uses Akismet to reduce spam. Learn how your comment data is processed.