CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Meshing & Mesh Conversion (https://www.cfd-online.com/Forums/openfoam-meshing/)
-   -   How do you define a cell zone or region for porous? (https://www.cfd-online.com/Forums/openfoam-meshing/90632-how-do-you-define-cell-zone-region-porous.html)

bigbang July 16, 2011 10:12

How do you define a cell zone or region for porous?
 
I've solved my a model of my car using simpleFoam (KERealizable) but now I want to include the effects of the radiator because it is a FIA GT style car.

I understand that there are some tutorials using the porous code.

I've concluded that you need to define a cellZone or region to specify as a porous medium. I'm totally freeware so I use blender and snappyHexMesh to create the mesh.

The radiator is rectangular at a slight angle (Y).

Thank you.

bigbang July 21, 2011 13:41

Ok I found the answer to my own question (in part):

Steps:
1) Create your mesh with the volume in question (snappyHexMesh) and copy the final mesh in <case>/3 to <case>/constant. Delete <case>/1, <case>/2 and <case>/3.
2) run 'setSet' from your case directory and then at the prompt: 'cellSet <name> new boxToCell (minx miny minz) (maxx maxy maxz)' where min_ and max_ are the bounding values of your box.
3) run 'setsToZones'

And then you should have a cellZone created. You can verify this by looking for and reading the cellZones file in <case>/constant/polyMesh. It should list all the cells in your zone.

As far as creating a boxToCell at an angle to the coordinate system... I still have no idea, but luckily I found my car's radiator to be square :o

shipman November 16, 2014 10:51

Hi Alex,

Really nice info.

Thanks.

rafa13 March 25, 2015 12:51

Hi Alex,

Thanks a lot.

I was trying to define a porous zone on waves2foam and i used your description. The only thing that i did different was that i used topoSetDict an it works fine.

greetings

MaralMohajer March 11, 2016 05:55

hi Rafael,

could you please help me how did you define these cellzone using topoSetDict. My case Ždoesn't have anything to do with waves but I need to create cellzone in MRF and i cant Figure it out !

regards
Maral

rafa13 March 18, 2016 18:39

Hi Maral,

sorry that i responde only now.

Here that site will help you
https://openfoamwiki.net/index.php/TopoSet

First when you are creating the mesh you need to name the volume that you want to define as poros zone (here i call it porosity), then you need to define the field with setFieldDict (here i used Ihfoam, so i define this field as porosityIndex 1... this comes from the code)

FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
zoneToCell // Porous zone
{
name porosity;
fieldValues
(
volScalarFieldValue porosityIndex 1
);
}




after that you need to use the topoSetDict to define the the cellSet ( the zone that you called "porosity" during the mesh construction), and finally you need to use :setsToZones


FoamFile
{
version 2.0;
format ascii;
class dictionary;
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(

{
name porosity;
type cellSet;
action new;
source zoneToCell;
sourceInfo
{
name porosity1;
}
}


setsToZones




I hope that i was able to help you out.

Greets,
Rafa

rafa13 March 18, 2016 18:42

sorry guys i posted it 2 times

greets,
Rafa


All times are GMT -4. The time now is 06:32.