Rise of a spherical bubble terminal velocity

sega · May 20, 2008, 09:20

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

sega · May 21, 2008, 11:07

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 ...

sega · May 22, 2008, 01:36

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"?

sega · May 22, 2008, 01:38

And now for the harder part:

How can I compute the actual rising velocity over time?

ngj · May 22, 2008, 03:41

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

hjasak · May 22, 2008, 03:56

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

sega · May 22, 2008, 04:42

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!

sega · May 23, 2008, 05:08

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.

sega · May 23, 2008, 06:40

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 ...

sega · May 23, 2008, 06:51

The bubble split up ...

Looks like a smilie to me

sega · May 25, 2008, 19:00

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 ...

sega · May 26, 2008, 13:50

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.

sega · May 28, 2008, 02:28

How is it possible to get some numbers for the radius of the final shape?

ngj · May 28, 2008, 03:46

Hi Sebastian

What do you mean with radius? If you can find the periphery in some way as a function of a parameter t, you can easily find the radii of curvature as a function of t.
I would probably import the data in matlab and then find the curve.

- Niels

sega · May 28, 2008, 11:24

Yes, I'm talking about the curvation of the top front of the bubble.

I don't know how to export these things into MATLAB or similar.

Does anybody know, how this can be done?

Meanwhile I have used a different setup to calculate another bubble.
This time I used the properties of an airbubble in water - I have experimental data for these setups.

Unfortunately the bubble is starting to break up again. Any ideas how I can prevent this?

Have a look at the shape:
http://therealsega.th.funpic.de/openfoam/airbubble.jpg

ngj · May 28, 2008, 12:16

Hi Sebastian

You have your gamma field, and if you put that together with the informations contained in the files in the polyMesh-directory, you should be able to piece together a set of (x,y,z,gamma)-arrays.

It takes some thinking, especially with piecing the coordinate information together, but it is definitely doable.

/ Niels

sega · May 28, 2008, 13:33

Well, thats a lot of work.
But maybe I will try it.

Now, that the caluclation is finished I have some depressing results. The bubble broke up just about the end of the calculation:

And there is some variation in the rising velocity:

tvairwater.pdf

Taking the mean of the rising-velocity I'm round about the 20 % error I allready experienced with the first caluclation.

My next step will be a calculation of a smaller bubble of about 1 mm diameter. There should be no signifcant deformation and a rectilinear rise-path.

sega · May 29, 2008, 14:38

Dam it, this is not working.

I have tried different set-ups now, but this is still not working.

The test case with a 20mm diameter bubble described in the literature yields 20% error.

Testcase_400x200_de20mm.pdf

A 20mm diameter bubble in water has about 20 % error as well

water_de20mm.pdf

A 2mm diameter bubble in water about 30 % error.

water_de2mm.pdf

A 1mm diameter bubble in water is zickzacking in a transversal direction and the rise velocity is oscillating. So I can't really tell the terminal velocity. Funny thing: Helical paths are restricted to bubble of higher diameter ...

water_de1mm.pdf

It dawns me, that my results are void, because I'm doing 2D simulations.
What do you think? I'm comparing wrong ...?

ngj · May 29, 2008, 16:25

Hi Sebastian

I have discussed a lot with you, but this has become to subject specific, thus I will not be able to help you any further.

Good luck,

Niels

sega · June 3, 2008, 13:51

Hello again.

I revised the whole case of the rising bubble.
My first setup was complete crap!
I did completely wrong trying to compute in plane 2D.

Now I did a calculation on a axisymmetric 2D mesh and the results look pretty good.

risevelocity.pdf

BUT: As you may see, the bubble reaches the desired terminal velocity after the overshot, but is gaining speed after about 0.25 seconds.

Any ideas, why this is happening?

Greetings so far.

May 20, 2008, 09:20	Hello. Now I'm getting to m	#1
sega 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
sega 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 22, 2008, 01:36	Ok, of course I have chosen th	#3
sega 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:	#4
sega 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.	#5
ngj 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	#6
hjasak 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	#7
sega 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! BlnPhoenix likes this. __________________ 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	#8
sega 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	#9
sega 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	#10
sega 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 4siamak likes this. __________________ 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	#11
sega 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	#12
sega 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. BlnPhoenix likes this. __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

May 28, 2008, 02:28	How is it possible to get some	#13
sega Senior Member Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 20	How is it possible to get some numbers for the radius of the final shape? __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

May 28, 2008, 03:46	Hi Sebastian What do you me	#14
ngj Senior Member Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Copenhagen, Denmark Posts: 1,900 Rep Power: 37	Hi Sebastian What do you mean with radius? If you can find the periphery in some way as a function of a parameter t, you can easily find the radii of curvature as a function of t. I would probably import the data in matlab and then find the curve. - Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

May 28, 2008, 11:24	Yes, I'm talking about the cur	#15
sega Senior Member Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 20	Yes, I'm talking about the curvation of the top front of the bubble. I don't know how to export these things into MATLAB or similar. Does anybody know, how this can be done? Meanwhile I have used a different setup to calculate another bubble. This time I used the properties of an airbubble in water - I have experimental data for these setups. Unfortunately the bubble is starting to break up again. Any ideas how I can prevent this? Have a look at the shape: http://therealsega.th.funpic.de/openfoam/airbubble.jpg __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

Thread Tools	Search this Thread
Show Printable Version Email this Page	Search this Thread: Advanced Search
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

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

May 28, 2008, 12:16	Hi Sebastian You have your	#16
ngj Senior Member Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Copenhagen, Denmark Posts: 1,900 Rep Power: 37	Hi Sebastian You have your gamma field, and if you put that together with the informations contained in the files in the polyMesh-directory, you should be able to piece together a set of (x,y,z,gamma)-arrays. It takes some thinking, especially with piecing the coordinate information together, but it is definitely doable. / Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

May 28, 2008, 13:33	Well, thats a lot of work. Bu	#17
sega Senior Member Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 20	Well, thats a lot of work. But maybe I will try it. Now, that the caluclation is finished I have some depressing results. The bubble broke up just about the end of the calculation: And there is some variation in the rising velocity: tvairwater.pdf Taking the mean of the rising-velocity I'm round about the 20 % error I allready experienced with the first caluclation. My next step will be a calculation of a smaller bubble of about 1 mm diameter. There should be no signifcant deformation and a rectilinear rise-path. __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

May 29, 2008, 14:38	Dam it, this is not working.	#18
sega Senior Member Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 20	Dam it, this is not working. I have tried different set-ups now, but this is still not working. The test case with a 20mm diameter bubble described in the literature yields 20% error. Testcase_400x200_de20mm.pdf A 20mm diameter bubble in water has about 20 % error as well water_de20mm.pdf A 2mm diameter bubble in water about 30 % error. water_de2mm.pdf A 1mm diameter bubble in water is zickzacking in a transversal direction and the rise velocity is oscillating. So I can't really tell the terminal velocity. Funny thing: Helical paths are restricted to bubble of higher diameter ... water_de1mm.pdf It dawns me, that my results are void, because I'm doing 2D simulations. What do you think? I'm comparing wrong ...? __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

May 29, 2008, 16:25	Hi Sebastian I have discuss	#19
ngj Senior Member Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Copenhagen, Denmark Posts: 1,900 Rep Power: 37	Hi Sebastian I have discussed a lot with you, but this has become to subject specific, thus I will not be able to help you any further. Good luck, Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

June 3, 2008, 13:51	Hello again. I revised the	#20
sega Senior Member Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 20	Hello again. I revised the whole case of the rising bubble. My first setup was complete crap! I did completely wrong trying to compute in plane 2D. Now I did a calculation on a axisymmetric 2D mesh and the results look pretty good. risevelocity.pdf BUT: As you may see, the bubble reaches the desired terminal velocity after the overshot, but is gaining speed after about 0.25 seconds. Any ideas, why this is happening? Greetings so far. __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"