CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Rise of a spherical bubble terminal velocity (http://www.cfd-online.com/Forums/openfoam-solving/58449-rise-spherical-bubble-terminal-velocity.html)

sega May 20, 2008 09:20

Hello. Now I'm getting to m
 
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:

http://www.cfd-online.com/OpenFOAM_D...ges/1/7745.png

I used the same function to initialize the pressure inside the bubble to the value defined by sigma/radius:

http://www.cfd-online.com/OpenFOAM_D...ges/1/7746.png

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:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&)

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.
 
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?

http://www.cfd-online.com/OpenFOAM_D...ges/1/7774.png

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 th
 
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.

http://www.cfd-online.com/OpenFOAM_D...ges/1/7782.png

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:
 
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.
 
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 th
 
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 setu
 
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 Thes
 
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
 
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.

http://www.cfd-online.com/OpenFOAM_D...ges/1/7793.png

P.S. With increasing calculation time the bubble is getting more thinner at the center line:

http://www.cfd-online.com/OpenFOAM_D...ges/1/7794.png

I don't think thats good ...

sega May 23, 2008 06:51

The bubble split up ... htt
 
The bubble split up ...

http://www.cfd-online.com/OpenFOAM_D...ges/1/7796.png

Looks like a smilie to me http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

sega May 25, 2008 19:00

Now I could performe a full si
 
Now I could performe a full simulation.

The terminal velocity is reached without significant "overshot".

Have a look:
http://www.cfd-online.com/OpenFOAM_D...s/mime_pdf.gif terminalvelocity.pdf

The shape is pretty good, allthought the bubble is still dispersing a little bit.

http://www.cfd-online.com/OpenFOAM_D...ges/1/7811.jpg
http://www.cfd-online.com/OpenFOAM_D...ges/1/7812.jpg

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 questio
 
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:

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif 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
 
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 me
 
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 cur
 
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
 
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. Bu
 
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:

http://www.cfd-online.com/OpenFOAM_D...ges/1/7846.png

And there is some variation in the rising velocity:

http://www.cfd-online.com/OpenFOAM_D...s/mime_pdf.gif 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.
 
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.

http://www.cfd-online.com/OpenFOAM_D...s/mime_pdf.gif Testcase_400x200_de20mm.pdf

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

http://www.cfd-online.com/OpenFOAM_D...s/mime_pdf.gif water_de20mm.pdf

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

http://www.cfd-online.com/OpenFOAM_D...s/mime_pdf.gif 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 ...

http://www.cfd-online.com/OpenFOAM_D...s/mime_pdf.gif 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 discuss
 
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
 
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.

http://www.cfd-online.com/OpenFOAM_D...s/mime_pdf.gif 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.


All times are GMT -4. The time now is 10:49.