CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Meshing & Mesh Conversion

How do you define a cell zone or region for porous?

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

Like Tree12Likes
  • 11 Post By bigbang
  • 1 Post By rafa13

Reply
 
LinkBack Thread Tools Display Modes
Old   July 16, 2011, 10:12
Default How do you define a cell zone or region for porous?
  #1
Member
 
Alex
Join Date: Jun 2010
Location: Planet Earth
Posts: 43
Rep Power: 8
bigbang is on a distinguished road
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 is offline   Reply With Quote

Old   July 21, 2011, 13:41
Default
  #2
Member
 
Alex
Join Date: Jun 2010
Location: Planet Earth
Posts: 43
Rep Power: 8
bigbang is on a distinguished road
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
cutter, ehsan_am86, jherb and 8 others like this.
bigbang is offline   Reply With Quote

Old   November 16, 2014, 10:51
Default
  #3
Senior Member
 
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 130
Rep Power: 5
shipman is on a distinguished road
Hi Alex,

Really nice info.

Thanks.
shipman is offline   Reply With Quote

Old   March 25, 2015, 12:51
Default
  #4
Member
 
Rafael Marques
Join Date: Mar 2014
Location: Almada/Mülheim a.d. Ruhr, Portugal/Germany
Posts: 67
Rep Power: 4
rafa13 is on a distinguished road
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

Last edited by rafa13; March 25, 2015 at 12:52. Reason: forgot the name
rafa13 is offline   Reply With Quote

Old   March 11, 2016, 05:55
Default
  #5
New Member
 
Maral Mohajer
Join Date: Jan 2016
Location: Stuttgart
Posts: 18
Rep Power: 2
MaralMohajer is on a distinguished road
hi Rafael,

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

regards
Maral
MaralMohajer is offline   Reply With Quote

Old   March 18, 2016, 18:39
Default
  #6
Member
 
Rafael Marques
Join Date: Mar 2014
Location: Almada/Mülheim a.d. Ruhr, Portugal/Germany
Posts: 67
Rep Power: 4
rafa13 is on a distinguished road
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
mizzou likes this.
rafa13 is offline   Reply With Quote

Old   March 18, 2016, 18:42
Default
  #7
Member
 
Rafael Marques
Join Date: Mar 2014
Location: Almada/Mülheim a.d. Ruhr, Portugal/Germany
Posts: 67
Rep Power: 4
rafa13 is on a distinguished road
sorry guys i posted it 2 times

greets,
Rafa
rafa13 is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
CGNS converters available mbeaudoin OpenFOAM Meshing & Mesh Conversion 131 November 5, 2016 22:51
cgnsToFoam problems with "QUAD_4" cells lentschi OpenFOAM Meshing & Mesh Conversion 1 March 9, 2011 05:49
Pressure and Temperature UDF for Cell Zone elixer2104 FLUENT 0 February 24, 2011 12:54
Cells with t below lower limit Purushothama CD-adapco 2 May 31, 2010 21:58
Free surface boudary conditions with SOLA-VOF Fan Main CFD Forum 10 September 9, 2006 12:24


All times are GMT -4. The time now is 14:00.