Hello World. I'm working to
 

Hello World.

I'm working to compute the following problem:

Concidering a liquid in the form of a SQUARE block in air with zero gravity.
Due to surface tension the liquid must obtain the contour of a sphere.

After meshing and setting the appropriate fields (gamma,U) I have a smooth silmulation of the deforming bubble.

It looks pretty well, but I doesn't come to rest.
Due to friction the liquid has to reach a state of rest. But it doesn't even after a endTime of 50.

How Do I implement friction?
Or Do I have even have to increase the running time ...

Hi Sebastian It sound like
 

Hi Sebastian

It sound like a very interesting experimenthttp://www.cfd-online.com/OpenFOAM_D...part/happy.gif Friction should be included in terms of the diffusion term laplacian(mu,U) in the UEqn, thus if you increase mu in your transportProperties dict in case/constant/, then the dissipation of energy will increase.

Hope it helps.

- Niels

I think I will have to take a
 

I think I will have to take a look at the corrosponding dimensionless description on this case.

I presume it's Re^2/We ...

I will write next time I get some results.

Hi Sebastian You inspired
 

Hi Sebastian

You inspired me to make some more visually pleasing bubbles, even though the simple cube in itself is very interesting, so please enjoy this small movie:

http://www.student.dtu.dk/~s001581/O.../cubeStick.mpg

In this I got the same problem as you, namely that the kinetic energy is very slow dissipating, the movie is 100s. Note that the smaller sphere is completely steady but the larger once are vibrating.

Best regards,

Niels

Well, that looks awesome... E
 

Well, that looks awesome...
Especially for a beginner, like me ...

Thankshttp://www.cfd-online.co
 

Thankshttp://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Obviously you are "very into i
 

Obviously you are "very into it".
Would you mind having a look at my post about seeting non-uniform fields?
http://www.cfd-online.com/cgi-bin/Op...how.cgi?1/7461

I'm really messed up with this problem.

Thanks, though I think you are
 

Thanks, though I think you are exaggerating a bithttp://www.cfd-online.com/OpenFOAM_D...part/happy.gif I have been reading that post as well, and unfortunately I cannot help you, because I have not tried to initialize fields with anything but setFields.
Though I like the way you tried to overcome the problem in creating a spherehttp://www.cfd-online.com/OpenFOAM_D...part/happy.gif Very creative.

- Niels

Actually the two problems are
 

Actually the two problems are not linked at all.
I have two different problems to perform:

1. This one: Deformation of a square under zero gravity.
2. Rise of a bubble to it's terminal velocity

For the second one I need the bubble...

Get it?

Ah, yes. But now that you know
 

Ah, yes. But now that you know how to create a bubble in zero gravity, then after doing that, add gravity to the system and it will rise. I know that it is computationally heavy, but it is a way out of the problem about generating the bubble.

- Niels

Now that it looks finaly that
 

Now that it looks finaly that I did the calculation right.
How can I compare the final shape of the fluid area with a circle?

I thought about creating the contour-plot for gamma=0.5, which does look really good like a cicle.
But how am I going to get addition data corrosponding to a circle inside this plot?
Or do I have to export the contour plot so I can handle the comparison in an other software - like MATLAB, or something similar?

Greetings.

Hello, Me again. I checked
 

Hello, Me again.

I checked some literature about how to set up this problem right:
Validation of Advanced Computational Methods for Multiphase Flow (ed. Lemonnier, Jamet, Lebaigue, 2005)

The simulation is running smoothly.
But I have some problem with the pressure inside the liquid.

Pressure-Difference should be delta_p = sigma / Radius for my 2D-case.
Unfortunately the simulation does not reach this state. The pressure inside the liquid is a little bit smaller - well, almost 6%.

The Radius of the liquid-circle is caluclated right.

Any ideas what went wrong?

http://www.cfd-online.com/OpenFOAM_D...ges/1/7615.jpg

Hi Sebastian I can come up
 

Hi Sebastian

I can come up with a couple of possibilities, which might explain what you see. I have put them in order, so the first is the one I think might have the largest impact:

1. I have experienced that you have to be careful when initializing the gamma-field. If the edges of your initial cube of water is not perfectly aligned with the faces in the grid you will get a larger or smaller amount water (gamma = 1) in your domain. As p < 1 suggest that you have to much water in your calculation. You could test it with a small command such as:

sum(mesh.V() * gamma) / sum(mesh.V())

and if this is not identical to "pi * thickness in z-direction" in your case, your radius cannot be 1, assumed sigma = 1.

2. Your circle is not perfectly circular, even though close, so in these flatter parts the curvature is smaller and thus the contribution to the internal pressure is smaller.

3. The surface tension is based on snGrad(), thus there is a numerical error and if your mesh does not represent the interface perfectly these would affect the surface tension and therefor the inner pressure.

Thanks for sharing the reference on the book, I will look into that.

Have a nice weekend,

Niels

Ooops, you should not divide b
 

Ooops, you should not divide by sum(mesh.V()).

- Niels

Thanks so far. But can you te
 

Thanks so far.
But can you tell me where I have to enter the calculation commands?
In a terminal windows?
Or in some kind of file?

I have some problems getting into the whole programming of OpenFOAM. I think I have to take a really close look into the programmers guide ...

BTW: I have come upon a web-site which contains most of the numerical test cases from the book mentioned above. Have a look at:
http://test.interface.free.fr/

Hi Sebastian After a second
 

Hi Sebastian

After a second thought, the information you are after is actually given to you directly in the log-file. Because the "Liquid phase volume fraction" is written each and every time step. Thus multiply that number with the total volume, and you will have the water volume.

Thanks for the link, it looks really goodhttp://www.cfd-online.com/OpenFOAM_D...part/happy.gif

- Niels

Hi Niels. Ok, there is too
 

Hi Niels.

Ok, there is too much liquid. Exactly 2.5 % plus.
The liquid phase volume fraction does work-
So, Do you have any ideas about how I can change this?

I'm using a 100x100 discretization.
Do you think it's necessary to increase this number to get a sharper interface?

Or can you think of an alternative way to make sure the gamma-field is set up to a face on the grid?

Well that is good, because tha
 

Well that is good, because that explains partly you underprediction of your pressure.
I have myself had problems with setting the gamma-field as no tool to set a fraction if the criterion is only partly fullfilled in a cell exists. I have considered making such a tool but it is far into the future.
My advise would be to go back to the cube initial field and then make you mesh out of 9 blocks, where the center block is [-sqrt(pi) / 2; sqrt(pi) / 2] x [-sqrt(pi) / 2; sqrt(pi) / 2]. This should give you a perfectly sharp interface, even though it is quite cumbersome.

- Niels

P.S. The book you mentioned is not available though my university library, so could you give a short description. I might consider buying it. Is it heavy on the mathematical treatment or is it more like a handbook with guidelines and test cases, i.e. with a more engineering kind of approach?

Well, that sounds like a good
 

Well, that sounds like a good solution.
I will try this one now.

About the book. The PDF-Files online are exactly the same as the cases in the book.
As the book is stuffed with about 30 problem problem setups there is not so much space for mathematics. Its more or less a handbook how to set up these problems right and which sections of the problem need higher attention.

Ok, the problems with the new
 

Ok, the problems with the new mesh are subject to this threat:
http://www.cfd-online.com/OpenFOAM_D...tml?1210424711