CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Seiche in a water basin

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 23, 2011, 11:33
Default Seiche in a water basin
  #1
New Member
 
Join Date: Dec 2010
Posts: 2
Rep Power: 0
maille is on a distinguished road
Hi,

I'm quite new at using OpenFoam. I've been looking for tutorials or examples applied to natural environments such as lakes/pounds without success.

I'm trying to model seiches in a water basin as a result of wind forcing.
I have started my project with a very simple basin, using (RAS)interFoam. My first results were not making much sense, so I set U to 0m/s and it appears that despite this set up significant velocities appear in the run, provoking some oscillation of the water body.

Would you have some advices or directions for me?

Thank you for your attention.
maille is offline   Reply With Quote

Old   March 4, 2011, 12:49
Default
  #2
Senior Member
 
Gijsbert Wierink
Join Date: Mar 2009
Posts: 383
Rep Power: 9
gwierink is on a distinguished road
Hi maille,

I think the problem are parasitic currents, which are more pronounced for greater viscosity and density ratios for the two fluids. These are usually quite difficult to deal with in a general way, although there are some tricks for specific situations. Have a look at this discussion for instance. More info on parasitic currents you can find here.

If you run the damBreak case in zero gravity (so that there is no driving force), you'll see parasitic currents as well. Do you have any pics of your lake? Have you tried interDyMFoam (dynamic meshing)?

One thing that may be of your interest is a report by Jan Potac. It's about snow drift, but there is some explanation on what BCs were used etc.
__________________
Regards, Gijs
gwierink is offline   Reply With Quote

Old   March 4, 2011, 15:37
Default
  #3
Senior Member
 
Gijsbert Wierink
Join Date: Mar 2009
Posts: 383
Rep Power: 9
gwierink is on a distinguished road
Right, I forgot to mention some other things ... Perhaps you know, but in any case there is an interface compression factor called cAlpha in system/fvSolution. Increasing cAlpha above 1 compresses the interface, which may help. Also, it may help to set momentumPredictor to yes in system/fvSolution.
This is all for inter(DyM)Foam, using the VoF method. You could also have a look at an interface tracking method like interTrackFoam.

P.S. I became curious and tried a simple 2D water basin with 10 m/s wind. The pics are after 60 s simulation in a 300 m domain. The water seems to start moving a bit, but I think the simulation time should be longer and/or higher wind velocity. The case lives here.

__________________
Regards, Gijs

Last edited by gwierink; March 5, 2011 at 04:09.
gwierink is offline   Reply With Quote

Old   March 9, 2011, 11:45
Smile
  #4
New Member
 
Join Date: Dec 2010
Posts: 2
Rep Power: 0
maille is on a distinguished road
Hi,
thank you for all your advices and help. I had found the second link on parasitic currents and tried to use some of the advices there but without sucess. The gravity seemed to be part of the trouble.
What would be the advantage of using interDyMFoam?
I have played around with cAlpha and momentumPredictor as well but without getting much improvements.
I have to put this project on break for a while but I will run your example with 10m/s (that should be more than sufficient to produce basin oscillations) and 0m/s to check the results, I will compare the configuration. I have already seen that you are using OpenFoam 1.6 while I'm on OpenFoam (p=>p_rgh), and you are also using the refineMeshDict that I have not used yet but seems extremely convenient here.
I will post a bit more details and results as soon as I can get back on this.
Thank you again.
maille is offline   Reply With Quote

Old   March 9, 2011, 12:09
Default
  #5
Senior Member
 
Gijsbert Wierink
Join Date: Mar 2009
Posts: 383
Rep Power: 9
gwierink is on a distinguished road
Hi,

Quote:
gravity seemed to be part of the trouble
In terms of parasitic currents you mean? Actually, if you're talking about parasitic currents, the problem is that if surface tension forces become dominant the VoF method freaks out and gives weird velocities at the interface.

Quote:
What would be the advantage of using interDyMFoam?
interDyMFoam is basically interFoam with dynamic meshing (this is what the "DyM" part stands for). The solver finds areas with string gradient in the colour function (alpha) and starts refining the mesh locally to resolve this strong gradient. Your interface will thus be sharper and better resolved.

I used OF-1.6 to set up this case, that's right. But it's not such a job to convert it to 1.7. Have a look and a try, I'm happy to help if I can
__________________
Regards, Gijs
gwierink is offline   Reply With Quote

Reply

Tags
interfoam, lake, parasitic velocities, seiche

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[GAMBIT] Creating the sea water basin domain (begginner) Muhammd Fikri ANSYS Meshing & Geometry 2 December 31, 2010 13:23
Water vapour condensation in CFX-5.7.1 hdj CFX 1 November 27, 2005 08:15
Separation phenomenon of water, droplet and air Raymond CFX 0 July 9, 2004 22:59
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11
uptodate water distribution network fredius,magige,tanzanian,(e.a) Main CFD Forum 0 January 27, 2002 08:10


All times are GMT -4. The time now is 18:18.