[hr_nt]

I recently an few multiphase scenarios using interFoam and found that fixedFluxPressure is more stable for the simulation than zeroGradient. What might be the issue for this ?

[vatavuk]

Hi HR,

At the 11th OpenFOAM Workshop there was a Training Course with the title "Learning how to use free surface flows in OpenFOAM 3.0" by Victoria Korchagova. This course is the only material that I found that explains this boundary condition. Is it for OF version 3, but I think that it also applies to newer versions. You can download the course material in this page:
https://openfoam-extend.sourceforge....s/courses.html

[Yann]

The OpenFOAM user guide also mention it, despite not giving much details:

5.2.3.3 Fixed flux pressure

In the above example, it can be seen that all the wall boundaries use a boundary condition named fixedFluxPressure. This boundary condition is used for pressure in situations where zeroGradient is generally used, but where body forces such as gravity and surface tension are present in the solution equations. The condition adjusts the gradient accordingly.

https://doc.cfd.direct/openfoam/user...v10/boundaries

There are also on old thread here discussing it: I need explanations about fixedFluxPressure

My personal experience with buoyantSimpleFoam is that I get a flowrate through the walls when using zeroGradient and it does not happen with fixedFluxPressure.

Yann

[hjasak]

Hi,

This is because when you’re solving for p, zero gradient isn’t the correct boundary condition. Consider additional forces, such as gravity: if you zero gradient the pressure, such terms will give you flux through a wall.

Fixed flux pressure compensates for it to achieve zero flux: you get a pressure gradient on the wall to balance all other flux contributions.

Hrv