[tehzap]

Hey,

I am pretty new to OpenFOAM. In my case i wanna simulate a multitubular reactor using the porousSimpleFoam solver. To get into OpenFOAM I started with a simulation of a 2 D plane with a porous zone in the middle. I reconfigured the angleDuctImplicit example to do so and it worked fine. Unfortunately I don't really get why.
The walls along the porosity zone are called "porosityWalls" just like in the example. Now there's the thing I don't get. How does OpenFOAM know, where the porous media is located at? In the porosityProperties file it looks something like this:

porosity1 {
cellZone: porosity;

Isn't it necessary to use the same names as in the blockMeshDikt file?

Thank you!
tehzap

[gooya_kabir]

As I know, it should be modified when you define the geometry, so you should define the porous zone in constant/polymesh/blockmesh directory.

[jprobst]

OpenFOAM will know which cells are porous medium from a so called cellSet. In the examples where the meshes are created using blockMesh, the blockMeshDict is already modified so you will get cellSets during mesh creation.

If you created the mesh without cellSets or if you don't use blockMesh you can always create a cellSet on an existing mesh using the onboard utility topoSet. In system/topoSetDict, try an entry like

actions
(
    {
        name    porosity;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box (-1 -1 -1) (1 1 1);
        }
    }
);

This will create a cellSet from all cells within the box described by the corner points (-1 -1 -1), (1 1 1) with the name 'porosity'. The same name must be used in constant/porosityProperties (more recent solvers use the file system/fvOptions) as value for the parameter 'cellZone'.

You can have several cellSets with different names and hence use different parameters on them. And you can define other geometries than a box. OpenFOAM has cylinders, spheres and the like.

[m5m5kh]

Hi
1. you should import your file to OF
for example for a fluent file you should you fluentMeshToFoam filename.msh (for 2D case) or fluent3DMeshToFoam filename.msh (for 3D case)
note: there is 2 space between command and file name
2. you should modify porous zone
for this step you should use topoSetdict file in your system folder in your case directory
you can see this link to choose what you want.it describes all forms of defining a zone
https://github.com/OpenFOAM/OpenFOAM...et/topoSetDict
then use setsToZones in terminal

3. you should modify D and F which are darcy and forchheimer coefficients.I describe it in this thread
http://www.cfd-online.com/Forums/ope...simplefom.html
you should define them in a porosityProperties file in your constant folder in your case directory
I suppose you can modify transportProperties and RASProperties.

4. finally you should use boundary condition in 0 folder and modify U and P.
then just use porousSimpleFoam and analyze your result

I wish you success !!!

Best Regards
Mohsen

[RygeltheXVI]

Hello All,

This Tech Report may prove helpful for those having difficulty understanding Darcy-Forchheimer settings in OpenFOAM.

Kind Regards,
RygeltheXVI