CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Pre-Processing

How does porousSimpleFoam work?

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 2 Post By m5m5kh

LinkBack Thread Tools Search this Thread Display Modes
Old   October 24, 2013, 13:59
Default How does porousSimpleFoam work?
New Member
Join Date: Oct 2013
Posts: 3
Rep Power: 8
tehzap is on a distinguished road

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 is offline   Reply With Quote

Old   October 25, 2013, 06:06
Default Hi
Join Date: Feb 2012
Posts: 67
Rep Power: 9
gooya_kabir is on a distinguished road
As I know, it should be modified when you define the geometry, so you should define the porous zone in constant/polymesh/blockmesh directory.
gooya_kabir is offline   Reply With Quote

Old   October 25, 2013, 15:49
New Member
Johannes Probst
Join Date: Aug 2013
Posts: 8
Rep Power: 8
jprobst is on a distinguished road
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

        name    porosity;
        type    cellSet;
        action  new;
        source  boxToCell;
            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.

Last edited by jprobst; October 26, 2013 at 05:04. Reason: formulated things a little bit clearer
jprobst is offline   Reply With Quote

Old   October 26, 2013, 03:52
Senior Member
mohsen kh
Join Date: Jan 2013
Location: Iran
Posts: 125
Rep Power: 9
m5m5kh is on a distinguished road
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 describes all forms of defining a zone
then use setsToZones in terminal

3. you should modify D and F which are darcy and forchheimer coefficients.I describe it in this thread
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
thiagopl and manuc like this.
m5m5kh is offline   Reply With Quote

Old   July 28, 2017, 01:50
Default Possibly useful reference
New Member
Join Date: Mar 2011
Posts: 16
Rep Power: 10
RygeltheXVI is on a distinguished road
Hello All,

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

Kind Regards,
RygeltheXVI is offline   Reply With Quote


Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
porousSimpleFoam aban OpenFOAM 9 January 6, 2019 08:47
How to work with constant pressure? Martin Siemens 2 February 25, 2009 14:23
Getting FoamX to work shaun OpenFOAM Installation 12 March 23, 2007 09:55
Why do the Plant library cases don't work? Alumna Phoenics 6 June 22, 2004 13:08
why my In-Form doesn't work? green Phoenics 2 May 27, 2004 22:03

All times are GMT -4. The time now is 13:51.