|
[Sponsors] |
|
May 20, 2008, 09:20 |
Hello.
Now I'm getting to m
|
#1 |
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 20 |
Hello.
Now I'm getting to my next problem: The rise of sperical bubble to it's terminal velocity. I used the test-setup described in http://test.interface.free.fr/Case01.pdf Unfortunately there is nothing about the boundary conditions in this case. As the boundary should not have an influence on the shape and even on the terminal veloctiy (if the computational domain is large enought), i chosed the following: left: symmetryPlane for all values (U,pd,gamma) (I use an axisymmetric description top: totalPressure (0) for pd, uniform (0 0 0) for U, zeroGradient for gamma left & bottom: zeroGradient for pd and gamma, uniform (0 0 0) for U To initialize the bubble I used funkySetFields to create a gamma-field at the center of the domain. Here is the image: I used the same function to initialize the pressure inside the bubble to the value defined by sigma/radius: Transport Properties were taken from the test-case description mentioned above. Sounds bad, but it's real: the solver is doing nothing: Exec : interFoam . . Date : May 20 2008 Time : 15:16:11 Host : M1530 PID : 6392 Root : /home/sega/OpenFOAM/sega-1.4.1/run/rise Case : . Nprocs : 1 Create time Create mesh for time = 0 Reading environmentalProperties Reading field pd Reading field gamma Reading field U Reading/calculating face flux field phi Reading transportProperties Selecting incompressible transport model Newtonian Selecting incompressible transport model Newtonian Calculating field g.h time step continuity errors : sum local = 0, global = 0, cumulative = 0 #0 Foam::error::printStack(Foam:stream&) So, there must be something wrong. Any ideas? My OpenFOAM-case is located here: http://therealsega.th.funpic.de/openfoam/rise.tar.gz
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" |
|
May 21, 2008, 11:07 |
My first setup was really bad.
|
#2 |
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 20 |
My first setup was really bad.
I have done this now: - used the complete computational domain (no symmetry) - boundary-condition: U: 0 at the bottom, zeroGradient at all other sides pd: totalPressure 0 at the top, zeroGradient at all other sides gamma: zeroGradient at all sides I initialized the bubble as a sphere of defined radius and defined pressure inside. All other transportProperties were chosen as in the literature mentioned above. The simulation is running, but is not computing as I have planned. - The bubble does not reach the "spherical cap sized" shape. It's more "skirted" at the sides. Is that due to wall effects (actually there is no wall to the sides)? Maybe I have to increade the computational domain? The bubble is rising very slowly. The image from above is after 30s Simulation time. From the literature the bubble should reach its final shape and terminal velocity round about 0.1 Seconds ...
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" |
|
May 31, 2017, 05:41 |
How to make 2D bubble region in openfoam?
|
#3 | |
New Member
David
Join Date: May 2017
Posts: 2
Rep Power: 0 |
Quote:
|
||
May 22, 2008, 01:36 |
Ok, of course I have chosen th
|
#4 |
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 20 |
Ok, of course I have chosen the wrong transportProperties, and size of the initial bubble. Thats why the bubble was rising too slow and getting "out of shape".
So, now that I did a check on all the numbers, there is another problem. The bubble is starting to disperse at the skirts. I have read about this phenomena in "Bubbles, Drops and Particles" (Clift, Grace, Weber. 2005) Do I have to chose an even smaller mesh-size to stop the bubble from further "divergence"?
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" |
|
May 22, 2008, 01:38 |
And now for the harder part:
|
#5 |
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 20 |
And now for the harder part:
How can I compute the actual rising velocity over time?
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" |
|
May 22, 2008, 03:41 |
Hi Sebastian
It looks nice.
|
#6 |
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,900
Rep Power: 37 |
Hi Sebastian
It looks nice. I do not know how to calculate the rising velocity. With respect to the dispersing bubble, I would try trial'n'error with a couple of different resolutions and see what happens. - Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request. |
|
May 22, 2008, 03:56 |
Hello,
Do you know about th
|
#7 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 |
Hello,
Do you know about the PhD Thesis from Henrik Rusche: Rusche, H: Computational fluid dynamics of dispersed two-phase flows at high phase fractions, Imperial College, University of London 2003. He has done a bunch of free-rising bubble simulations in 3-D. Incidentally, how big is your bubble? In 2-D it will only have approx half the curvature of a 3-D bubble, which will cause some break-up. Enjoy, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
May 22, 2008, 04:42 |
Dear Hrv.
The complete setu
|
#8 |
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 20 |
Dear Hrv.
The complete setup is described in http://test.interface.free.fr/Case01.pdf So, I used a spherical bubble of 0.02m diameter. An I have just downloaded the PhD from Henrik Rusche. I will have a look into it. @Niels: I will try some finer meshes later! Get back to you!
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" |
|
May 23, 2008, 05:08 |
I had a look into the PhD Thes
|
#9 |
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 20 |
I had a look into the PhD Thesis.
It's consistent with the other theoretical works I have read. What I'm still missing is a way of calculating the rise-velocity. The OpenFOAM-PostProcessing is still a mystery to me.
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" |
|
May 23, 2008, 06:40 |
I have set up a finer mesh by
|
#10 |
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 20 |
I have set up a finer mesh by now and the simulation is running.
The error between estimated and calculated liquid phase volume fraction is at 0.9 %. So I think the mesh is "good" enough. I have checked the results during the calculation and the bubble seems to be somehow "dented" at the apex. If you have a closer look at the mesh in this area you can see that it is finer there in an "uneven" way. I was not aware of this fact. Is it possible, that the mesh is causing this trouble? Maybe I should consider creating a more "balanced" mesh in this area concerning the grid spaces. P.S. With increasing calculation time the bubble is getting more thinner at the center line: I don't think thats good ...
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" |
|
May 23, 2008, 06:51 |
The bubble split up ...
htt
|
#11 |
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 20 |
The bubble split up ...
Looks like a smilie to me
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" |
|
May 25, 2008, 19:00 |
Now I could performe a full si
|
#12 |
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 20 |
Now I could performe a full simulation.
The terminal velocity is reached without significant "overshot". Have a look: terminalvelocity.pdf The shape is pretty good, allthought the bubble is still dispersing a little bit. BUT: First and graves problem: Compared to the literature the value of my terminal velocity is over 20% too low ...
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" |
|
May 26, 2008, 13:50 |
Hello.
I received a questio
|
#13 |
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 20 |
Hello.
I received a question about how I calculated the terminal velocity. I have used a post-processing tool I got from the university. I don't know in detail where it comes from, but it was really useful: barycenter.zip The tool calculates the location of the mass center of the phase gamma=0 at each timestep. I tun the tool over my case and put the results into a file named 'center'. barycenter . . >center Then I picked the times and positions of the masscenter and calculate the displacement over time which is representing the rising velocity. Greetings. S.
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" |
|
November 19, 2011, 08:26 |
barycenter and drop rise velocity
|
#14 | |
Member
Hrushikesh Khadamkar
Join Date: Jul 2010
Location: Mumbai
Posts: 68
Rep Power: 15 |
Quote:
I am able to simulate drop rise velocity using interFoam solver. Then I ran barycenter utility as posted above successfully. I am now stuck at how to extract the time and barycenter coordinate (say in .xy format)? So that I can calculate instantaneous drop rise velocity over a time. How did you pick the times and position of the masscenter from center file generated using barycenter utility? Hrushikesh |
||
January 7, 2012, 04:03 |
|
#15 | |
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 20 |
Quote:
Code:
barycenter > center
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" |
||
August 21, 2012, 10:53 |
Barycenter utility
|
#16 |
New Member
Angelo J. Chaves
Join Date: Aug 2012
Location: Itajubá, Brasil.
Posts: 3
Rep Power: 13 |
Hello
I am new here in the forum and I have been working with the same case of the bubble rising. I'm using interDyMFoam and an parallel processing to simulate the case. Now I want to calculate the barycenter of the bubble so I can get the velocity in each step of time. I downloaded the barycenter utility, but when I try to install it, an erro message occurs. ana@ana:~/OpenFOAM/OpenFOAM-2.1.0/applications/utilities/postProcessing/barycenter$ wmake Making dependency list for source file barycenter.C could not open file readEnvironmentalProperties.H for source file barycenter.C SOURCE=barycenter.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/home/ana/OpenFOAM/OpenFOAM-2.1.0/src/transportModels -I/home/ana/OpenFOAM/OpenFOAM-2.1.0/src/transportModels/incompressible/lnInclude -I/home/ana/OpenFOAM/OpenFOAM-2.1.0/src/transportModels/interfaceProperties/lnInclude -I/home/ana/OpenFOAM/OpenFOAM-2.1.0/src/finiteVolume/lnInclude -IlnInclude -I. -I/home/ana/OpenFOAM/OpenFOAM-2.1.0/src/OpenFOAM/lnInclude -I/home/ana/OpenFOAM/OpenFOAM-2.1.0/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/barycenter.o barycenter.C:49:44: error: readEnvironmentalProperties.H: Arquivo ou diretório não encontrado In file included from barycenter.C:52: createFields.H: In function ‘int main(int, char**)’: createFields.H:92: error: ‘g’ was not declared in this scope In file included from barycenter.C:55: /home/ana/OpenFOAM/OpenFOAM-2.1.0/src/finiteVolume/lnInclude/setInitialDeltaT.H:35: error: ‘CoNum’ was not declared in this scope /home/ana/OpenFOAM/OpenFOAM-2.1.0/src/finiteVolume/lnInclude/readPISOControls.H:3: warning: unused variable ‘nOuterCorr’ /home/ana/OpenFOAM/OpenFOAM-2.1.0/src/finiteVolume/lnInclude/readPISOControls.H:6: warning: unused variable ‘nCorr’ /home/ana/OpenFOAM/OpenFOAM-2.1.0/src/finiteVolume/lnInclude/readPISOControls.H:12: warning: unused variable ‘momentumPredictor’ /home/ana/OpenFOAM/OpenFOAM-2.1.0/src/finiteVolume/lnInclude/readPISOControls.H:15: warning: unused variable ‘transonic’ make: ** [Make/linux64GccDPOpt/barycenter.o] Erro 1 ana@ana:~/OpenFOAM/OpenFOAM-2.1.0/applications/utilities/postProcessing/barycenter$ I'm also a new user of the linux system but I guess the erro occurs because I'm using an new version of the OpenFoam (2.1.0) instead the original one that the utility were made for. If anyone could help me, I would be grateful. |
|
August 22, 2012, 01:09 |
|
#17 | |
Member
Hrushikesh Khadamkar
Join Date: Jul 2010
Location: Mumbai
Posts: 68
Rep Power: 15 |
Quote:
Yes, you are right. You need to make some minor changes in that code. I had done it a year back. I will have to look into my old files. If I get it, I will upload it here asap. |
||
September 21, 2012, 14:24 |
baryCenter
|
#18 |
Member
Hrushikesh Khadamkar
Join Date: Jul 2010
Location: Mumbai
Posts: 68
Rep Power: 15 |
Hi Angelo & Tayo
Here is the updated version of baryCenter baryCenter-of201.zip utility. I have tested it on OpenFoam-201. You can comapre the each file in zip archive with one that you have to recognise the changes one needs to make it usable in OF201. Hope it helps. Regards Hrushi |
|
September 21, 2012, 14:54 |
|
#19 | |
Member
Tayo
Join Date: Aug 2012
Posts: 94
Rep Power: 13 |
Quote:
Last edited by tayo; September 22, 2012 at 01:45. |
||
October 10, 2013, 15:45 |
|
#20 |
Member
Hrushikesh Khadamkar
Join Date: Jul 2010
Location: Mumbai
Posts: 68
Rep Power: 15 |
Hi,
Here is the updated version of baryCenter (for OF-2.2.1) baryCenter221.zip utility. I have tested it on OpenFOAM-2.2.1. Enjoy! |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Bubble rise velocity | Miguel | CFX | 1 | December 25, 2006 19:17 |
terminal velocity in spray dryer | weekendwarrior | Main CFD Forum | 1 | February 20, 2006 00:47 |
Query on VOF for Bubble rise | Vamsi | Main CFD Forum | 0 | December 22, 2005 00:02 |
Terminal velocity of 2D rising bubbles | Tony | Main CFD Forum | 0 | June 15, 2004 18:37 |
Terminal bubble shapes | Tony | Main CFD Forum | 0 | February 27, 2002 16:30 |