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

Faces of a cell

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 14, 2011, 11:04
Default Faces of a cell
  #1
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 275
Rep Power: 7
Andrea_85 is on a distinguished road
Hi all,

probably a very simple question. How can i access the faces of a particular cell?
I would like to loop over all the cell and for every cell[i] over all the face.

Thanks
Andrea
Andrea_85 is offline   Reply With Quote

Old   March 14, 2011, 11:20
Default
  #2
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,619
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
Hi Andrea

You can get the information as:

Code:
const labelListList & cellFaces = mesh.cellFaces();
Be aware that if you will access some surface<Type>Field given the faces, you need to check whether or not the face label is internal. If not, then you need to access the value of this boundary face through the boundary field.

Best regards,

Niels
ngj is offline   Reply With Quote

Old   March 14, 2011, 11:44
Default
  #3
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 275
Rep Power: 7
Andrea_85 is on a distinguished road
Hi Niels,

thanks for the answer. I need to know the values ​​of a variable (alpha1 using interFoam) belonging to the faces of a particular cell, and then loop for all the cell. Something like that:

forAll(alpha1,celli)
{
alpha[celli] = sum(alpha[facei]*Sf[facei])/sum(Sf[facei])
}

this does not work of course. I dont know where to put the loop on the correct faces belonging to the cell[i].

many thanks for any help

andrea
Andrea_85 is offline   Reply With Quote

Old   March 14, 2011, 12:00
Default
  #4
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 12
Bernhard is on a distinguished road
Isn't fvc able to calculate what you want? I suppose fvc:div does something similar you what you want? I cannot give you the correct syntax though, but maybe someone else can help you out.
Bernhard is offline   Reply With Quote

Old   March 14, 2011, 12:25
Default
  #5
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 275
Rep Power: 7
Andrea_85 is on a distinguished road
Hi,

basically a need to smooth alpha on every cell and i would like to do that by using alpha on the face times area divided by the total area. So i need to sum alpha on the 4 faces. The divergence is a difference between values on the faces divided by deltax and i dont know if is the same that i need.

andrea
Andrea_85 is offline   Reply With Quote

Old   March 14, 2011, 13:35
Default
  #6
Member
 
Duong A. Hoang
Join Date: Apr 2009
Location: Delft, Netherlands
Posts: 92
Rep Power: 8
duongquaphim is on a distinguished road
Send a message via Yahoo to duongquaphim
Hi Andrea,

Take a look at src/finiteVolume/finiteVolume/fvc/fvcSurfaceIntegrate.C and what they do is very similar to what you want.

I also did the smoothed alpha1, but I did not include the boundary value at all.
duongquaphim is offline   Reply With Quote

Old   June 8, 2011, 09:56
Default
  #7
New Member
 
Paweł Kuczyński
Join Date: Feb 2011
Location: Warsaw, Poland
Posts: 19
Rep Power: 6
kuczmas is on a distinguished road
Dear forumers,

I decided to post my question inside this thread, as it is also somehow connected with looping over faces in a given cell. What I try to achieve is to get the face normal vector at every face in the cell, regardless it is a boundary cell or internal.
I produced the following code...:

Code:
    const cell& faces = mesh_.cells()[cellI];

    forAll( faces, i )        // loop over all faces in cellID
    {
        vector faceINormal = mesh_.Sf()[i] / mesh_.magSf()[i] ; 
        Info << " i = " << i << ", faceINormal = " << faceINormal << endl ;
    }
...but the values of normal vectors I received are all of positive sign, all the components are of positive sign (on hexahedral mesh). I think in three normal vectors there should be at least one component of negative sign... Do you have any ideas?
__________________
Best regards
P. Kuczynski.
kuczmas is offline   Reply With Quote

Old   April 29, 2013, 11:36
Default
  #8
Senior Member
 
Anne Gerdes
Join Date: Aug 2010
Location: Hamburg
Posts: 152
Rep Power: 7
Anne Lincke is on a distinguished road
Hey,
have you solved your problem? I also would like to access the face normal vectors of internal faces....

Kind Regards
Anne
Anne Lincke is offline   Reply With Quote

Old   April 30, 2013, 02:23
Default
  #9
New Member
 
Paweł Kuczyński
Join Date: Feb 2011
Location: Warsaw, Poland
Posts: 19
Rep Power: 6
kuczmas is on a distinguished road
Yes, I solved the problem. The solution I got was correct. I.e. the components of normal vectors for an arbitrary cell can be in general of the same sign.

The reason for this are the normal vector direction rules. In OpenFoam mesh normal vectors:
- at boundary faces point out of the domain
- at internal faces they point from the cell of lower global ID number to higher.

Hope this helps,

Best regards,
kuczmas.
__________________
Best regards
P. Kuczynski.
kuczmas is offline   Reply With Quote

Old   April 30, 2013, 07:16
Default
  #10
Senior Member
 
Lieven
Join Date: Dec 2011
Location: Mol, Belgium
Posts: 295
Rep Power: 13
Lieven will become famous soon enough
Just a small note, I think

Code:
vector faceINormal = mesh_.Sf()[i] / mesh_.magSf()[i];
should be
Code:
 
vector faceINormal = mesh_.Sf()[faces[i]] / mesh_.magSf()[faces[i]] ;
Cheers,

L
Lieven is offline   Reply With Quote

Old   April 30, 2013, 08:36
Default
  #11
Senior Member
 
Anne Gerdes
Join Date: Aug 2010
Location: Hamburg
Posts: 152
Rep Power: 7
Anne Lincke is on a distinguished road
Thank you for this hint. I will keep on trying.
Kind Regards
Anne
Anne Lincke 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
SnappyHexMesh - no layer added bejbro OpenFOAM Mesh Utilities 4 October 16, 2014 19:24
DecomposePar unequal number of shared faces maka OpenFOAM Pre-Processing 6 August 12, 2010 09:01
external flow with snappyHexMesh chelvistero OpenFOAM 11 January 15, 2010 20:43
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15
Warning 097- AB CD-adapco 6 November 15, 2004 05:41


All times are GMT -4. The time now is 22:43.