# Bubble in zero gravity conditions

 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 28, 2008, 12:34 Hello World. I'm working to #1 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 12 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 ... __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

 April 28, 2008, 15:24 Hi Sebastian It sound like #2 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,702 Rep Power: 27 Hi Sebastian It sound like a very interesting experiment 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 __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 April 29, 2008, 14:20 I think I will have to take a #3 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 12 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. __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

 April 29, 2008, 14:55 Hi Sebastian You inspired #4 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,702 Rep Power: 27 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 __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 April 29, 2008, 15:50 Well, that looks awesome... E #5 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 12 Well, that looks awesome... Especially for a beginner, like me ... __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

 April 30, 2008, 04:03 Thankshttp://www.cfd-online.co #6 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,702 Rep Power: 27 Thanks __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 April 30, 2008, 04:37 Obviously you are "very into i #7 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 12 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. __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

 April 30, 2008, 04:48 Thanks, though I think you are #8 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,702 Rep Power: 27 Thanks, though I think you are exaggerating a bit 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 sphere Very creative. - Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 April 30, 2008, 05:46 Actually the two problems are #9 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 12 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? __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

 April 30, 2008, 06:03 Ah, yes. But now that you know #10 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,702 Rep Power: 27 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 __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 May 4, 2008, 08:54 Now that it looks finaly that #11 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 12 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. __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

 May 9, 2008, 03:36 Hello, Me again. I checked #12 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 12 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? __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

 May 9, 2008, 04:15 Hi Sebastian I can come up #13 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,702 Rep Power: 27 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 __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 May 9, 2008, 04:25 Ooops, you should not divide b #14 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,702 Rep Power: 27 Ooops, you should not divide by sum(mesh.V()). - Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 May 9, 2008, 07:51 Thanks so far. But can you te #15 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 12 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/ __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

 May 9, 2008, 08:55 Hi Sebastian After a second #16 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,702 Rep Power: 27 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 good - Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 May 9, 2008, 13:53 Hi Niels. Ok, there is too #17 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 12 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? __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

 May 9, 2008, 16:46 Well that is good, because tha #18 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,702 Rep Power: 27 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? __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 May 10, 2008, 08:03 Well, that sounds like a good #19 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 12 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. __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

 May 10, 2008, 09:08 Ok, the problems with the new #20 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 12 Ok, the problems with the new mesh are subject to this threat: http://www.cfd-online.com/OpenFOAM_D...tml?1210424711 __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Lorenzo FLUENT 0 September 19, 2007 10:10 Shankar FLUENT 0 May 31, 2006 04:30 anjai FLUENT 12 October 17, 2005 06:34 Shankar FLUENT 4 November 26, 2003 16:45 cfd-novice FLUENT 0 April 14, 2003 01:50

All times are GMT -4. The time now is 09:31.