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

• $FOAM_SOLVERS/basic/potentialFoam

See also

• simpleFoam

Tutorials

• $FOAM_TUTORIALS/basic/potentialFoam