# OpenFOAM guide/H operator

The H operator is a form of shorthand notation that is not commonly used, but appears in OpenFOAM. It is comprised of a collection of terms from the momentum equation. A partially discretized form of the momentum equation is:

$A_p \mathbf U_p = \mathbf {S_m}_{,p} - \sum\limits_r A_r \mathbf{U}_r - \boldsymbol \nabla p^*$

Where:

• subscript p is the cell index;
• subscript r are related cells[1];
• A are the matrix coefficients;
• U is the uncorrected velocity;
• S is the discretization source term; and
• p* is the pressure from the previous timestep or initial guess.

The H operator is all terms on the right-hand side, excluding those involving pressure:

$\mathbf H_p = \mathbf {S_m}_{,p} - \sum\limits_r A_r \mathbf{U}_r$

Therefore the momentum equation becomes:

$A_p \mathbf U_p = \mathbf H_p - \boldsymbol \nabla p$

Due to its prevalence in solver algorithms, OpenFOAM implements the H operator directly in its matrix classes, including:

## Notes

1. What I'm calling related cells is conventionally called neighbours. But OpenFOAM has a different meaning for neighbours, so the term related cells is used.