CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Pre-Processing

Boundary conditions for Internal faces

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 16, 2013, 07:38
Default Boundary conditions for Internal faces
  #1
Member
 
Evangelos
Join Date: Sep 2011
Posts: 67
Rep Power: 5
Danath is on a distinguished road
Hello i want to set the boundary conditons for internal faces

i run simple
how to set the internal faces for P ,U i just want the fluid flow through the face and no special boundary condition

Last edited by Danath; April 16, 2013 at 08:04.
Danath is offline   Reply With Quote

Old   May 3, 2013, 05:02
Default
  #2
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Dear Evangelos,

did you find an answer ?

I have the same kind of problem. I want to set a boundary condition for a patch inside the flow domain. Let me know.

Regards,
Stephane.
openfoam_user is offline   Reply With Quote

Old   May 3, 2013, 11:51
Unhappy
  #3
Member
 
Evangelos
Join Date: Sep 2011
Posts: 67
Rep Power: 5
Danath is on a distinguished road
Quote:
Originally Posted by openfoam_user View Post
Dear Evangelos,

did you find an answer ?

I have the same kind of problem. I want to set a boundary condition for a patch inside the flow domain. Let me know.

Regards,
Stephane.
Hello ! No yet !

but if you want to connect volumes and eliminate the internal faces try " merge faces " using Gambit
Danath is offline   Reply With Quote

Old   May 4, 2013, 20:22
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,488
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings to all!

Quote:
Originally Posted by openfoam_user View Post
I want to set a boundary condition for a patch inside the flow domain.
It's possible to do this, but it depends on what exactly you want to do.

For example, there is a tutorial named "TJunctionFan", located in "incompressible/pimpleFoam/TJunctionFan", which creates a cyclic baffle. It then uses a special boundary condition of type "fan"... well, the specifics are in the file "system/createBafflesDict" and in "system/topoSetDict" you can see how the cell faces are selected for later converting to the cyclic baffles.

@Evangelos: creating a faceSet or faceZoneSet might be enough, if you want to calculate the mass-flow going through the selected faces, or some kind of value monitor. These are selected using topoSet, as described in the aforementioned tutorial.

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   January 13, 2014, 21:40
Default
  #5
Member
 
Dinesh Balaji
Join Date: Oct 2012
Posts: 43
Rep Power: 4
DineshramBalaji is on a distinguished road
Hi ,

I have created a solid sheet patch inside a fluid domain in salome and imported to fluent. the internal patch has been defined in face zones. I want to define it as a wall and specify some field values for it. Can someone help me on this?
DineshramBalaji is offline   Reply With Quote

Old   January 26, 2014, 15:01
Default
  #6
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,488
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Dinesh,

If you can provide a small example case, it would be easier to help you.

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   January 26, 2014, 15:03
Default
  #7
Member
 
Dinesh Balaji
Join Date: Oct 2012
Posts: 43
Rep Power: 4
DineshramBalaji is on a distinguished road
Hi Bruno,

Thanks for the help. I can work and see on it.
DineshramBalaji is offline   Reply With Quote

Old   January 26, 2014, 16:07
Default
  #8
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,488
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
By the way, doesn't this page explain what you are trying to do? http://openfoamwiki.net/index.php/Ho...internal_walls
wyldckat is offline   Reply With Quote

Old   January 26, 2014, 16:31
Default
  #9
Member
 
Dinesh Balaji
Join Date: Oct 2012
Posts: 43
Rep Power: 4
DineshramBalaji is on a distinguished road
Hi Bruno,

I created a large box. Inside which i created a duct, as a solid domain. Then I used partition operation for two bodies.

The boundaries are created in the face zone of the polymesh. I need to create a temperature boundary condition in the walls in the 0 directory. But I cant find the boundary condition for the walls.

This is my problem.
DineshramBalaji is offline   Reply With Quote

Old   January 26, 2014, 16:51
Default
  #10
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,488
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Dinesh,

Mmm... OK, then if the instructions at http://openfoamwiki.net/index.php/Ho...internal_walls don't do what you need, then I need an example case so that I can test this myself.

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   January 26, 2014, 17:05
Default
  #11
Member
 
Dinesh Balaji
Join Date: Oct 2012
Posts: 43
Rep Power: 4
DineshramBalaji is on a distinguished road
Hi,

If you can send ur email id, I can send the case to you directly.
DineshramBalaji is offline   Reply With Quote

Old   January 29, 2014, 23:34
Default
  #12
New Member
 
Steven
Join Date: Jan 2014
Posts: 14
Rep Power: 3
alientxtmsgs is on a distinguished road
Greetings everyone,

I have been running into a related issue with my simulation, although it may be an even simpler case. I've been following along the $FOAM_RUN/tutorials/incompressible/pimpleFoam/TJunctionFan tutorial to see if I can create a baffle in my domain.

My general procedure so far has been to first define my topoSetDict to create a faceZone that will then be converted into an internal wall with createBaffles.

The actions field inside my topoSetDict looks like:

PHP Code:
actions
(
    {
        
name    baffleFaces;
        
type    faceZoneSet;
        
action  new;
        
source  boxToFace;
        
sourceInfo
        
{
            
box (2.32 1.4 0) (5.6 1.4 1.15);
        }
    } 
However, I do not quite understand the boxToFace option. I want to convert a plane that coincides with cell faces in my domain. For this reason, I have attempted to define a plane in the "box" field and I am not sure if this is the correct way to proceed. It does not give me any errors when I run topoSet, but when I view the newly generated sets and zones in paraView, the plane seems to be defined in the correct location but it does not extend to the bottom of my domain like it should.

Any help would be greatly appreciated!

Regards,
Steven
alientxtmsgs is offline   Reply With Quote

Old   January 31, 2014, 00:28
Default
  #13
New Member
 
Steven
Join Date: Jan 2014
Posts: 14
Rep Power: 3
alientxtmsgs is on a distinguished road
Hello all,

I seem to have solved my problem. For those that are interested, I will explain what I did in order to create my infinitely thin wall. Please forgive me if my explanation isn't technically sound, it is merely how I understand it.

What I needed was essentially a vertical partition in my wave flume to create a 180 degree bend, essentially what is shown in my primitive drawing below (imagine the dots aren't there):
_________________________________________
|........ ___________________________________|
|_________________|

I needed it to behave as the external walls did with all the same initial and boundary conditions for k, epsilon, velocity, pressure, eddy viscosity, etc.

In the first step I created a topoSetDict with the following entries inside:
PHP Code:
{
        
name    baffleFaces;
        
type    faceSet;
        
action  new;
        
source  boxToFace;
        
sourceInfo
        
{
            
box (2.315 1.395 -0.05)(5.605 1.405 1.155);
        }
    }
    {
        
name    baffleFaces;
        
type    faceZoneSet;
        
action  new;
        
source  setToFaceZone;
        
sourceInfo
        
{
            
faceSet baffleFaces;
        }
    } 
The box I created in the topoSetDict enveloped the cell faces I needed to be converted into a faceZone (only slightly, by half a centimetre).

I ran topoSet after my mesh was created and was able to view the newly created "set" and "zone" in paraview (not yet a patch). To convert it to a wall I ran createBaffles with the following createBafflesDict entries:

PHP Code:
internalFacesOnly true;

baffles
{
    
baffleFaces
    
{
        
type        faceZone;
        
zoneName    baffleFaces;

        
patches
        
{
            
master
            
{
                
name            baffles;
                
type            wall;

                
patchFields
                
{
                    
epsilon
                    
{
                        
type            epsilonWallFunction;
                
value           uniform 0.1;
                    }
                    
k
                    
{
                        
type            kqRWallFunction;
                       
value           uniform 0.1;
                    }
                    
nut
                    
{
                        
type            nutkWallFunction;
                
value           uniform 0;
                    }
                    
nuTilda
                    
{
                        
type            zeroGradient;
                    }
                    
p_rgh
                    
{
                        
type            fixedFluxPressure;
                
value           uniform 0;
                    }
                    
U
                    
{
                        
type            fixedValue;
                        
value           uniform (0 0 0);
                    }
                }
            }
            
slave
            
{
                ${..
master}
            }
        }
    } 

After running createBaffles it output my new mesh to a new time directory so I changed my controlDict to start from the new time (0.001 sec). It now seems to be doing exactly as I hoped

If anyone who understands this better I would love to know if my procedure is standard, or if there is an easier way etc!

Hope it helps someone,
Steven


alientxtmsgs is offline   Reply With Quote

Old   February 2, 2014, 10:30
Default
  #14
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,488
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings to all!

@Dinesh:
Quote:
Originally Posted by DineshramBalaji View Post
If you can send ur email id, I can send the case to you directly.
Please use Dropbox or a similar service for uploading your case and then send me the link over private message: http://www.cfd-online.com/Forums/faq...ivate_messages
I ask this because otherwise your email will only get lost in the several other emails I get, which is why I like to keep OpenFOAM+forum related questions only on the forum itself, including private messages.


@Steven: Thanks for sharing the solution you've reached. And sorry, but I don't have time to go over the solution you've found .

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   April 15, 2015, 08:05
Unhappy Baffle boundary condition
  #15
Member
 
Naresh Yathuru
Join Date: Feb 2015
Posts: 54
Rep Power: 2
Naresh yathuru is on a distinguished road
Hi Foamers,

sorry for restarting the thread again. I need to implement baffles in my case. i have some basic question can some one please help me.
I m having a zero thickness surface in my geometry and i have read a lot of posts regarding how to implement baffles which helped me create a mesh with baffles in snappyHexMesh. (thanks to the changes in snappyhexmesh)

code in snappyHexmesh, refinementsurfaces
Code:
table
        {
        level (2 2);
        faceZone table;

        // Create baffles for all faces on the surface
        faceType baffle;

        cellZone table;
        cellZoneInside inside;
        }
In paraview i have two patches created, a master and a slave. so far its good.
and i have checked in the polymesh/boundary folder two boundaries are created of type wall.
Code:
table
    {
        type            wall;
        inGroups        1(wall);
        nFaces          588;
        startFace       653617;
    }
    table_slave
    {
        type            wall;
        inGroups        1(wall);
        nFaces          588;
        startFace       654205;
    }
now my questions are
1.How can i define B.C to these patches like U,P,K,epsilon
2. do i have to make a folder for "createbafflesDict" to specify boundary conditions or can i specify B.C like for other patches?
3. last and much important question is can i spesify different boundary conditions for the master and slave patch similar to twosidedwall in fluent?

I have looked in to couple of tutorials but could not get a clear answer.

I m using OF 2.3.0

I m banging my head on the wall. could someone please help me.

Regards,
Naresh
Naresh yathuru 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
ribbed channel / simpleFoam / boundary conditions beeo OpenFOAM Pre-Processing 20 July 17, 2013 08:39
Add Mesh Layers doesnt work on the whole surface Kryo OpenFOAM Native Meshers: snappyHexMesh and Others 8 September 13, 2012 09:28
mesh file for flow over a circular cylinder Ardalan Main CFD Forum 6 April 17, 2010 23:40
Please help with flow around car modelling! Tudor Miron CFX 17 March 19, 2004 20:23


All times are GMT -4. The time now is 02:06.