
[Sponsors] 
October 11, 2012, 02:29 
How to compute surface area of rising bubble

#1 
Member
Tayo
Join Date: Aug 2012
Location: FL
Posts: 94
Rep Power: 5 
Hello,
Is there an accurate way to compute the surface area of a rising bubble as it deforms? I'm trying to compute the effective diameter using volumesurfaceArea ratio. I already computed the volume using (1gamma[cellI])*mesh.V()[cellI]. Or is there an alternative way to compute the diameter? Thanks in advance. 

October 18, 2012, 02:27 

#2 
Member
Tayo
Join Date: Aug 2012
Location: FL
Posts: 94
Rep Power: 5 
Hi Foamers,
I'm still expecting a response on how to compute bubble surface area at the interface. I read on page 29 of OF2.1.1 programmer's guide that Sf() is the access function for face area vector so I called the area of each mesh using mesh.sf()[cellI] but it won't even compile. Below is what I tried even though I should use an averaged value between 0<alpha1<1 of neighboring cells instead of (1alpha1) to represent the interface (I don't know how to do this either). (1alpha1[cellI])*mesh.Sf()[cellI] Any suggestions on how to go about computing this area? Thanks. 

October 18, 2012, 03:56 

#3 
Senior Member
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 13 
I am not sure if you can calculate this accurately with simple integration. Maybe by integration of (1gamma)*gamma, which is only nonzero at the interface (assuming you use interFoam). Howver, you will still get a volume, and not an area. Maybe if you divide this by the average interface thickness you get an estimate.
An alternative procedure, is to store the gamma=0.5 isosurface, and calculate the surface area of such a system by some external tools (I could not tell you how, however). 

October 18, 2012, 16:21 

#4 
Member
Tayo
Join Date: Aug 2012
Location: FL
Posts: 94
Rep Power: 5 
Thanks. I'll give your idea a little more thought.


October 18, 2012, 18:30 

#5  
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,916
Rep Power: 41 
Quote:
My proposal: let OpenFOAM calculate a sampledSurface on the isosurface of 0.5 (or whatever threshold you think is appropriate) then sum up area of the faces in that sampledSurface. The easiest way to do this (I think, but I'm extremely biased on this topic) is with swak4Foam: there is even a democase (a variation of the capillaryRisecase) where this (calculation of the interfacearea) is done
__________________
Note: I don't use "Friend"feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request 

October 23, 2012, 12:39 

#6  
Member
Tayo
Join Date: Aug 2012
Location: FL
Posts: 94
Rep Power: 5 
Quote:


October 23, 2012, 13:44 

#7 
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,916
Rep Power: 41 
Examples/other/capillaryRise
__________________
Note: I don't use "Friend"feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request 

October 23, 2012, 14:21 

#8 
Member
Tayo
Join Date: Aug 2012
Location: FL
Posts: 94
Rep Power: 5 
Thanks. I saw this link you gave from your Talk:Tip Surface elevation in time discussion. I've searched but all the links I found won't open for some reason. Few of these links are given below. That's why I requested you to provide the working link to the case. Thanks.
http://openfoamextend.hg.sourceforg.../capillaryRise http://openfoamextend.hg.sourceforg...em/controlDict 

October 23, 2012, 17:15 

#9  
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,916
Rep Power: 41 
Quote:
__________________
Note: I don't use "Friend"feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request 

October 23, 2012, 18:34 

#10 
Member
Tayo
Join Date: Aug 2012
Location: FL
Posts: 94
Rep Power: 5 
Oh, I get. I thought you meant that it was located at an online page. I've seen the case in the swak4Foam download that I use. I'll follow it to compute the interfacial area. Thanks for your awesome work on swak4Foam.
On a side note, I already some ran cases that takes days to complete. Is there a way to do some post processing using this tool without having to rerun my cases? 

October 30, 2012, 19:17 

#11  
Member
Tayo
Join Date: Aug 2012
Location: FL
Posts: 94
Rep Power: 5 
Quote:
Hi Bernard, I followed your advice to create an isosurface with alpha=0.5 and used this to compute the surface area of the bubble. I did a little test run copying the additional code from system/controlDict file of your capillaryRise example and added to my 2D bubble test case but I have few questions here: 1) The surface area computed is quite large (3.32e4) at 1st time step compared to (7.85e5) obtained if you check with pi*R^2 as initialized. I used "area()" instead of your "area()/0.001" in my controlDict expression. I initialized with funkysetFields with radius of 0.005. This bring me to why you used "area/0.001" in the surface expression? My guess is you probably divided by the cellsize. I checked your blockmesh and the zaxis mesh width is 0.001. So I simply used "area()" instead. 2) How can I compute the volume in swak4Foam, do I simply use "volume()"? I want to compare with using (1alpha[cellI])*mesh.V()[cellI]. 3) can I compute the bubble center velocity similarly? Thanks. libs ( "libOpenFOAM.so" // keeps paraFoam happy "libtwoPhaseInterfaceProperties.so" "libinterfaceProperties.so" "libsimpleSwakFunctionObjects.so" "libswakFunctionObjects.so" ); functions ( createInterface { type createSampledSurface; outputControl timeStep; outputInterval 1; surfaceName interface; surface { type isoSurface; isoField alpha1; isoValue 0.5; interpolate true; } surface { type swakExpression; valueType surface; surfaceName interface; verbose true; expression "area()/0.001"; accumulations ( sum ); ); Last edited by tayo; October 31, 2012 at 09:17. 

November 14, 2012, 18:37 

#12  
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,916
Rep Power: 41 
Quote:
About the discrepancy in size: no idea. Of course the isoSurface is naive about what you want to achive. So if in your simulation you have a bubble and a water surface then an isovalue of 0.5 will pick up the bubble AND the surface (that would explain the orderofmagnitude error). A bit creative playing around with the expressionFieldfunctionObject might help here Quote:
That depends on how you define the bubble center. The isosurface will only help you if you define it by the surface. If you define it by the volume something like "sum(pos()*vol()*(1alpha1))/(sum(vol()*(1alpha1)))" calculated on the internalField might be what you want
__________________
Note: I don't use "Friend"feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request 

January 30, 2013, 15:17 

#13 
Senior Member
Mieszko Młody
Join Date: Mar 2009
Location: POLAND, USA
Posts: 135
Rep Power: 9 
Hi
I am not sure if swak4FOAM is something I need, but I have a question which seems to be related to this thread. Do you know maybe how to extract isosurface of the field (e.g. field T, isosurface for T = 0) during runtime ? I would need it coordinate in my solver. Thanks ZM 

January 30, 2013, 18:59 

#14  
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,916
Rep Power: 41 
Quote:
BTW: T is NOT the temperature, right? Because then that isosurface wouldn't exist anyway
__________________
Note: I don't use "Friend"feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request 

January 30, 2013, 19:03 

#15 
Senior Member
Mieszko Młody
Join Date: Mar 2009
Location: POLAND, USA
Posts: 135
Rep Power: 9 
Thanks for your replay.
T is just some random field. But I need to do this during runtime, in my solver, for farther calculations in my solver. Not just passively to write on disc ... Best 

January 31, 2013, 05:19 

#16 
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,916
Rep Power: 41 
Then swak4Foam might be your thing. Have for instance a look in the swakdistribution at Examples/other/capillaryRise which calculates the properties of the surface. It is also possible to have these values feed back to boundary conditions etc (for details see the presentations that are linked from the swakpage in the Wiki). All this functionality is available in functionobjects: the advantage is that you don't have to modify the solver (disadvantage is that you can only influence/measure at the end of a timestep. But functionality from swak can also be incorporated into a solver. But usually the functionObjects are sufficient)
__________________
Note: I don't use "Friend"feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request 

January 6, 2014, 11:55 

#17  
New Member
Nazanin
Join Date: Sep 2013
Posts: 22
Rep Power: 4 
Quote:
I want calculate bubble diameter,bubble surface area,surface diameter and rising velocity for simulation rising bubble (2D&3D) .how I can calculate these parameters? I see ,in this thread that use swak4Foam but I don't find in capillaryRisecase about diameter and Are you sure this code (in capilary case) is correct?? 

January 7, 2014, 19:18 

#18  
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,916
Rep Power: 41 
Quote:
What do you mean with "is it correct"? You are doubting the expressions in the controlDict (I only sanitychecked them some time ago)? That's OK (doubting). These are just examples what can be done but the expressions for your application you've got to "develop" yourself
__________________
Note: I don't use "Friend"feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request 

January 8, 2014, 02:24 

#19  
New Member
Nazanin
Join Date: Sep 2013
Posts: 22
Rep Power: 4 
Quote:
I use capilarycase controldict for my case,and I have a question about that: 1I want calculate surface area bubble and in this code I think : Code:
functions ( createInterface { type createSampledSurface; outputControl timeStep; outputInterval 1; surfaceName interface; surface { type isoSurface; isoField alpha1; isoValue 0.5; interpolate true; } }surface { type swakExpression; valueType surface; surfaceName interface; verbose true; expression "area()"; accumulations ( sum ); 2for calculating changing diameter can I use this code??: Code:
Yheight { type swakExpression; valueType surface; surfaceName interface; verbose true; expression "pos().y"; accumulations ( min max ); } Thank you 

January 10, 2014, 09:37 

#20 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8 
Hi all,
i guess that the total interfacial area can be simply calculated using: \Sum_i=1:N \grad\alpha_i * \deltaV_i where N is total numer of cells in your domain. This gives you an area in m^2, so if your case is 2D and you just need the lenght of the interfacial line you have to normalized by the thickness. This is consistent with the CSF method implemented in interFoam. Best andrea 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Rising bubble with interFoam  tayo  OpenFOAM Running, Solving & CFD  15  December 5, 2014 04:49 
Water subcooled boiling  Attesz  CFX  7  January 5, 2013 04:32 
Layers don't fully surround surface  EVBUCF  OpenFOAM Native Meshers: snappyHexMesh and Others  14  August 20, 2012 04:31 
Cross section and surface area factor  Fabiana  CFX  0  January 10, 2006 00:51 
CFX4.3 build analysis form  Chie Min  CFX  5  July 12, 2001 23:19 