potentialFoam

Solves for the velocity potential to provide velocity and incompressible flux fields, typically used to initialise viscous calculations.

Overview

• Category: Basic
• steady state
• incompressible

Equations

Solves for the velocity potential, $\Phi$, using the equation

$$\laplacian \Phi = \div \phi$$

where the volumetric flux, $\phi$ is given by dotting the interpolated velocity with the face area vectors:

$$\phi = \u_f \dprod \vec{S}_f$$

Finally the cell centre velocity is derived by reconstructing the volumetric flux.

Input requirements

Mandatory fields:

• p: kinematic pressure [m2/s2] or Phi: velocity potential [m2/s]
• U: velocity [m/s]

Physical models

• None

Solution controls

$FOAM_CASE/system/fvSchemes requirements:

• gradient schemes: grad(Phi)
• laplacian schemes: laplacian(1,Phi)

$FOAM_CASE/system/fvSolution requirements:

• solver entry for Phi

Command line options

• -pName <name>: name of the pressure field
• -initialiseUBCs: initialise the velocity boundary conditions prior to computing the volumetric flux
• -writePhi: write the velocity potential field
• -writep: write the Euler pressure field

Further information

Source code

• potentialFoam

See also

• simpleFoam

Tutorials

• potentialFoam