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

bubbleInterTrackFoam tutorial

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 12, 2011, 04:48
Default bubbleInterTrackFoam tutorial
  #1
New Member
 
Kelvin Loh
Join Date: Mar 2009
Posts: 25
Rep Power: 8
kel85uk is on a distinguished road
Hi all,

Am still new to this free surface tracking solver, and I am trying to solve a similar problem as the one in the tutorial, but how do I change the size of the bubble to different initial diameters?

Thanks.

-kel85uk
kel85uk is offline   Reply With Quote

Old   May 12, 2011, 07:32
Default
  #2
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 12
Bernhard is on a distinguished road
The surface tracking solvers (I think you refer to bubbleInterTrackFoam?) are based on seperates meshes for different phases. For changing the bubble diameter, you need a different mesh. The easiest way to do this, is to rescale an existing mesh, you can use the utility transformPoints for that.
Bernhard is offline   Reply With Quote

Old   May 16, 2011, 00:19
Default
  #3
New Member
 
Kelvin Loh
Join Date: Mar 2009
Posts: 25
Rep Power: 8
kel85uk is on a distinguished road
Hi Bernhard,

Thank you very much. Will try that and see.

-kel85uk
kel85uk is offline   Reply With Quote

Old   May 17, 2011, 02:52
Default
  #4
New Member
 
Kelvin Loh
Join Date: Mar 2009
Posts: 25
Rep Power: 8
kel85uk is on a distinguished road
Hi,

Another quick question. How would I go about re-meshing the problem since scaling only changes the dimensions, and I might want to change the number of cells?

Many thanks.

Regards,
kel85uk
kel85uk is offline   Reply With Quote

Old   May 17, 2011, 04:06
Default
  #5
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 12
Bernhard is on a distinguished road
You can either use the refineMesh utility or make a mesh yourself.
Bernhard is offline   Reply With Quote

Old   May 19, 2011, 06:15
Default
  #6
New Member
 
Kelvin Loh
Join Date: Mar 2009
Posts: 25
Rep Power: 8
kel85uk is on a distinguished road
Quote:
Originally Posted by Bernhard View Post
You can either use the refineMesh utility or make a mesh yourself.
Yes, I'd probably want to make the mesh myself, but how to make the shadow zones? I have no idea how to start because the blockMeshDict is not present... Any help on this would be much appreciated.

Thank you.

Regards,
kel85uk
kel85uk is offline   Reply With Quote

Old   May 19, 2011, 06:46
Default
  #7
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 12
Bernhard is on a distinguished road
You need to make two seperate meshes (can be done with blockMesh). Define the interface twice, for one fluid, call it freeSurface for the one, and freeSurfaceShadow for the other.
Bernhard is offline   Reply With Quote

Old   May 23, 2011, 23:32
Default
  #8
New Member
 
Kelvin Loh
Join Date: Mar 2009
Posts: 25
Rep Power: 8
kel85uk is on a distinguished road
Quote:
Originally Posted by Bernhard View Post
You need to make two seperate meshes (can be done with blockMesh). Define the interface twice, for one fluid, call it freeSurface for the one, and freeSurfaceShadow for the other.
Hi Bernhard, sorry for the trouble again, but how do I make the refineMesh? I seem to get empty cells and the cellIDs are all over the place when I checked I converted it to VTK file format.

As for blockMesh, how do I merge the two separate meshes? Is it also possible if I can do the meshing in Gambit and then import it to OpenFOAM via the fluentMeshToFoam utility?

Thank you.

Regards,
kel85uk
kel85uk is offline   Reply With Quote

Old   May 24, 2011, 01:53
Default
  #9
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 12
Bernhard is on a distinguished road
To understand how to use refineMesh, copy refineMeshDict from utilities/mesh/manipulation/refineMesh to your case directory.

You don't have to merge the edges in blockMesh. And I don't see why you cannot make the mesh in gambit. Just give it a try. As long as you are consistent with naming the patches on the interface.
Bernhard is offline   Reply With Quote

Old   May 30, 2011, 06:41
Default
  #10
New Member
 
Kelvin Loh
Join Date: Mar 2009
Posts: 25
Rep Power: 8
kel85uk is on a distinguished road
Quote:
Originally Posted by Bernhard View Post
To understand how to use refineMesh, copy refineMeshDict from utilities/mesh/manipulation/refineMesh to your case directory.

You don't have to merge the edges in blockMesh. And I don't see why you cannot make the mesh in gambit. Just give it a try. As long as you are consistent with naming the patches on the interface.
Hi Bernhard,

Thank you for the guide, it works properly now in serial using the FLUENT meshes. Any idea how I can use decomposePar for this solver? I read in the OpenFOAM forums that the interface has to be in the master processor, and until now I have no clue as to how to make sure that is the case.

Thanks again.

Regards,
Kelvin
kel85uk is offline   Reply With Quote

Old   May 30, 2011, 06:51
Default
  #11
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 12
Bernhard is on a distinguished road
In decomposePar you have a subdictionary preservePatches. I've not tested this yet, but maybe this can help you. Please let me know if you get it done like this, because I'm also interested
Bernhard is offline   Reply With Quote

Old   May 31, 2011, 04:46
Default
  #12
New Member
 
Kelvin Loh
Join Date: Mar 2009
Posts: 25
Rep Power: 8
kel85uk is on a distinguished road
Hi Bernhard,

For the parallelization, it's easier to just use the manual decomposition method with funkysetfields to set the processor weights. However one more problem is with the fluidIndicator file. How do I create it? I searched the forums but they were unfortunately not very informative. Someone spoke about the setfluidindicator function but I have grepped it and found no files mentioning it in the src or even solver directories.

bubbleInterTrackFoam in parallel (fluidIndicator)

Any ideas on how to proceed from here?

Thanks.

Regards,
Kelvin
kel85uk is offline   Reply With Quote

Old   June 1, 2011, 05:38
Default
  #13
New Member
 
Kelvin Loh
Join Date: Mar 2009
Posts: 25
Rep Power: 8
kel85uk is on a distinguished road
Hi Bernhard,

I finally got it to work. The fluidIndicator file is nothing more like the alpha1, so, one can easily set it using funkySetFields. After that, it'll work.

-Kelvin
kel85uk is offline   Reply With Quote

Old   June 18, 2012, 14:02
Default
  #14
New Member
 
xiang chai
Join Date: Aug 2009
Posts: 13
Rep Power: 7
chai is on a distinguished road
Hi,
Can you explain the meaning of two seperate meshes. does it mean there is no connecting between these two meshese? for example, in my case that bubble rises in the water, there is a small gap between the grids occupied by water and grids for air. am i right?

Chai
chai is offline   Reply With Quote

Old   December 21, 2012, 10:10
Question How create 2 separated meshes
  #15
Member
 
Hanniel Freitas
Join Date: Jan 2012
Location: Natal, Brazil
Posts: 33
Rep Power: 5
hfsf is on a distinguished road
Quote:
Originally Posted by Bernhard View Post
You need to make two seperate meshes (can be done with blockMesh). Define the interface twice, for one fluid, call it freeSurface for the one, and freeSurfaceShadow for the other.
Sorry for the ressurection of a old thread and making a question that might sound too simple, but how can I create 2 separated meshes with the blockMesh utility? Once I run blockMesh with the configurations os the new mesh, the old one is replaced... I think I'm missing the point here, can anyone explain me please?
hfsf is offline   Reply With Quote

Old   December 21, 2012, 10:36
Default
  #16
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 12
Bernhard is on a distinguished road
Just put it in a single blockMeshDict. The vertices on the interface have to be defined twice, to make sure you get two patches. Then you create the patches freeSurface and freeSurfaceShadow.
Bernhard is offline   Reply With Quote

Old   December 21, 2012, 10:47
Default
  #17
Member
 
Hanniel Freitas
Join Date: Jan 2012
Location: Natal, Brazil
Posts: 33
Rep Power: 5
hfsf is on a distinguished road
Quote:
Originally Posted by Bernhard View Post
Just put it in a single blockMeshDict. The vertices on the interface have to be defined twice, to make sure you get two patches. Then you create the patches freeSurface and freeSurfaceShadow.
Thank you for so quick answer, Bernard. I will give it a try.
hfsf 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
[ANSYS Meshing] I need tutorial files colorful ANSYS Meshing & Geometry 5 September 19, 2014 01:21
Tutorial for subcooled nucleate boiling Asghari FLUENT 34 September 27, 2013 04:58
Problem on Fluent Tutorial: Horizontal Film Boilig Feng FLUENT 2 April 13, 2013 05:34
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52
STAR-CD Tutorial shekhar aryal STAR-CD 4 March 22, 2010 04:25


All times are GMT -4. The time now is 12:57.