[Outbound]

Greetings,

I'm working on a Master's thesis in which I'm continuing some work meant to validate the use of a porous medium to simulate dense submerged vegetation in compound channel flow.

The first stage is meant to replicate the initial study carried out using ANSYS-CFX in OpenFOAM using porousSimpleFoam. Initially I'm just using a wall with slip condition to simulate the free surface given the porousSimpleFoam doesn't do free surface interaction.

I'm having some trouble setting up the case based on the angleDuctExplicit tutorial.

I'm modifying the case for OpenFOAM 2.3.1 and using Gmsh to create the mesh.

Right now I'm having trouble setting the porosity value for the case. I used the "toposetDict" file to define the porous area, but I'm not sure where I set the actually porosity value.

I'm looking at some tutorials regarding porosity in OF but they relate to rhoPorousSimpleFoam and some of the case files are configured a bit differently.

Any help is appreciated,

[deepbandivadekar]

I stumbled at the same thing. Did you ever find anything about specifying porosity?

[Outbound]

Yes, enough to complete my dissertation.

It's not online yet but it is actually very simple so I'll try to describe it here.

If you're using blockMesh to build your mesh you basically set the internal volumes which are to be the zones with porosity by naming the corresponding block as porosity (or porosity1, 2 etc. depending on how many porous zones you have and if they're not continuous) and the rest of the internal volume as your free flow area. If you're using another program to generate the mesh you can use the topoSet utility (which runs like all other utilities, i.e., by setting up a topoSetDict and running the utility in the command line) to define the porosity zone in the mesh after it's built. It's only in theses zones of the mesh that the solver will apply the extra load loss term computed through the Darcy-Forchheimer equation (or PowerLaw if you set it to that) to the Navier-Stokes equation.

Then you change your porosity parameters in the /constant/porosityProperties (for as many porous zones as you set up in the mesh), setting up the Darcy and Forchheimer term with however the problem you're solving determines those two variables.

I hope this helps.

[deepbandivadekar]

Originally Posted by Outbound

Yes, enough to complete my dissertation.

It's not online yet but it is actually very simple so I'll try to describe it here.

If you're using blockMesh to build your mesh you basically set the internal volumes which are to be the zones with porosity by naming the corresponding block as porosity (or porosity1, 2 etc. depending on how many porous zones you have and if they're not continuous) and the rest of the internal volume as your free flow area. If you're using another program to generate the mesh you can use the topoSet utility (which runs like all other utilities, i.e., by setting up a topoSetDict and running the utility in the command line) to define the porosity zone in the mesh after it's built. It's only in theses zones of the mesh that the solver will apply the extra load loss term computed through the Darcy-Forchheimer equation (or PowerLaw if you set it to that) to the Navier-Stokes equation.

Then you change your porosity parameters in the /constant/porosityProperties (for as many porous zones as you set up in the mesh), setting up the Darcy and Forchheimer term with however the problem you're solving determines those two variables.

I hope this helps.

Thanks for your reply. I had figured out most of this (although not 100%). But I was rather enquiring something else. But I found my answers and I've mentioned about it here.

[Outbound]

OK,

So part of what I figured out about the porosity implementation in OF is that it's somewhat lacking. For e.g. it just applies the D and F coefficients like you said, and it doesn't ask for the porosity value (you just use it to calculate D and F). The problem here is that it then just uses the seepage velocity (which is the medium velocity of the fluid in the porous channels), and not the Darcy velocity it should use inside the porous medium.

The Darcy velocity is:

[m/s]

"Darcy velocity is a fictitious velocity since it assumes that flow occurs across the entire cross section of the [porous media]. Flow actually takes place only through interconnected pore channels (voids), at the seepage velocity" (Smart, 2013)

I don't know if this is why in the Darcy-Forchheimer equation it then applies a value in the nonlinear term, which is a formulation I didn't see anywhere else in the literature.

Also, it didn't apply any volumetric average to the porous medium (in versions of OF 2.x at least), which "allows considering the porous zones as continuous media, characterized by their macroscopic properties only, thus eliminating the need for a detailed description of their complex internal geometry. Hence, this technique can be thought of as a spatial filter to obtain an average flow behaviour inside porous zones, as already sketched in" (Higuera Caubilla, 2015). I think the first solvers to make use of volumetric averages for porous medium are IHFOAM, which if I'm not mistaken is now integrated into OF 5.x.

[deepbandivadekar]

Can anyone please clarify here? Anyone who knows more about porous media treatment in OpenFoam ?