CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

Breaking Water Waves

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 4, 2007, 12:28
Default Breaking Water Waves
  #1
Erik Wickley-Olsen
Guest
 
Posts: n/a
I am interested in discussing the use of CFD for modeling of breaking water waves. Using Fluent, I have used a Volume of Fluid (VOF) model along with 1st, 2nd, and 3rd order solution schemes. Simulation were performed using laminar and standard k-e models. The smallest grid spacing has been 2cm X 1cm (the domain is approximately 2.5m X 23m).

My main concern is "energy" dissipation. The waves lose energy quickly (numerical dissipation is thought to cause this).

Has anyone had succesful, physical results? What sort of schemes have you used? Have you tried adjusting the constants in the k-e equations?

Thanks in advance for any advice.
  Reply With Quote

Old   May 4, 2007, 12:45
Default Re: Breaking Water Waves
  #2
Erik Wickley-Olsen
Guest
 
Posts: n/a
Before anyone asks, yes, the solution is transient.
  Reply With Quote

Old   May 5, 2007, 02:45
Default Re: Breaking Water Waves
  #3
to
Guest
 
Posts: n/a
1) your schemes may be good enough provided your mesh is fine enough ...

2) be sure to use a time step that ensures a good temporal resolution

3) just forget the turbulence model, at least at the begining; running it laminar will allow you to identify the problem more easily

regards
  Reply With Quote

Old   May 5, 2007, 12:25
Default Re: Breaking Water Waves *NM*
  #4
Phil
Guest
 
Posts: n/a
  Reply With Quote

Old   May 5, 2007, 12:26
Default Re: Breaking Water Waves
  #5
Phil
Guest
 
Posts: n/a
why not just leave it laminar throughout and obtain a DNS simulation?

Can't you just turn the energy dissipation down on the model you are using?
  Reply With Quote

Old   May 7, 2007, 09:50
Default Re: Breaking Water Waves
  #6
CFDtoy
Guest
 
Posts: n/a
Eric: What kind of test case are you running? Is it the Fluent 6.2 or 6.3 version that has been used?

Now here is the deal, Fluent 6.2 uses PLIC based geometric reconstruction schemes while the new 6.3 has front capturing method (CICSAM) completely different than PLIC (front tracking ! methods).

I have coded CICSAM etc and found that front tracking schemes work really nice to get all the breaking collapsing, colaescing of droplets, WAVES etc !!

I have seen lot of dissipation using Fluent's PLIC scheme. The interface is just isnt good enough. Smoothens rapidly !

Now, if you were using Fluent 6.2 I would suggest you play with the pressure velocity coupling. I have seen a huge variation in the interface computation using Fluent just by modifying the Pressure-Velocity Coupling.

Turbulence details, later ! Really, Laminar should give you more breakup and interfacial activity (remember no turbulence..no additional viscous effects !)

Reducing time steps is not a great idea in the sense that you shall be marching slower but without much variation in the interfacial activity. Try different p-v coupling and ofcourse, As I have done sometimes, do adaptive meshing based on gradients of VOF that would work just fine too.

Let me know how it works out for you.

CFDtoy
  Reply With Quote

Old   May 7, 2007, 11:53
Default Re: Breaking Water Waves
  #7
Phil
Guest
 
Posts: n/a
CFDtoy, I was having trouble getting my adaptive meshing to work. Do you know if having rotationally periodic boundaries should affect the ability in particular of 'dynamic' adaptive meshing?

thanks Phil
  Reply With Quote

Old   May 7, 2007, 13:07
Default Re: Breaking Water Waves
  #8
CFDtoy
Guest
 
Posts: n/a
I have had some problems combining periodic boundaries with dynamic meshing. Check Fluent manual. I guess I have seen some warning suggesting similar stuff ..Not to use periodic with dynamic meshes.

Thanks

CFDtoy
  Reply With Quote

Old   May 8, 2007, 11:23
Default Re: Breaking Water Waves
  #9
Erik Wickley-Olsen
Guest
 
Posts: n/a
Thanks for the replies!

I am running Fluent 6.2.

With regards to laminar solutions, I have run many in the past. I notice simiilar dissipation as in the k-e model, albeit not as severe. I am able to create breaking waves in this model, although only gentle spilling waves. My research is focused on the turbulent energy dissipation rate, so I am interested in developing a good turbulent simulation.

I have reduced the time step from 0.002s to 0.001s, and I have set turbulent energy dissipation and turbulent kinetic energy at the wave generator to 0 (although that doesn't seem too physical). The solution will take about a week.

CFDtoy: The simulation P-V coupling is PISO. I have not tried SIMPLE or SIMPLEC. Would PISO give more accuracy given it has velocity and pressure satisfy momentum during the solution process?

I have not had a chance to try grid adaption yet.
  Reply With Quote

Old   May 18, 2007, 10:50
Default Re: Breaking Water Waves
  #10
Erik
Guest
 
Posts: n/a
Update:

Smaller time discretization does not change the solution.

Can anyone comment on mesh size and numerical dissipation?
  Reply With Quote

Reply

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
CFD Animations of breaking waves Dommermuth Main CFD Forum 0 June 17, 2009 11:47
Papers request-Generation of water waves by source Mehdi BEN HAJ Main CFD Forum 0 June 11, 2007 12:55
Breaking Water Waves Erik Wickely-Olsen FLUENT 0 May 4, 2007 12:44
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 11:26.