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

Turbulence dissipates too much energy for interFoam to simulate wave breaking

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

Like Tree1Likes
  • 1 Post By brdvolde

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 21, 2013, 13:54
Default Turbulence dissipates too much energy for interFoam to simulate wave breaking
  #1
New Member
 
Hf
Join Date: Nov 2012
Posts: 25
Rep Power: 11
jasonchen is on a distinguished road
Hello everyone,

I'm using interFoam to simulate waves breaking on a sloping beach (two segments with slope 1:10 and 1:2). My problem is when the wave is about to break, the wave surface is not smooth anymore and small "ripples" seem to ride above the surface (refer to the 2nd link); and it's found that the final runup is not large enough when compared with expt data. This may be due to numerical errors, but I find most probably the turbulence model in openfoam dissipates too much energy and may cause the wave surface to deform in such a way. Does anybody encounter problems like this? I read on this forum that density missing in turbulenct transport equations may be responsible for such an issue. Any comments or suggestions on this? Thanks in advance.

The regular wave is generated using waves2Foam, and k-epsilon model is used as turbulence model. Mesh is refined uisng snappyHexMesh at swash zone and along the free surface area. Two plotts are given in the links below: one is for domain setup, another is a zoomup of free surface at swash zone when the wave is about to break.

Wave parameters: water depth=0.8m; wave period=1.0s; height=0.045m.
Inlet relaxation zone is adopted at wave generating boundary; surface elevation at the deep water is monitered and compare well with analytical solution.

https://www.dropbox.com/s/2sqnprqz4c...in%20setup.png

https://www.dropbox.com/s/vfn8y1accx...%20surface.png

Regards,
Jason
jasonchen is offline   Reply With Quote

Old   November 20, 2016, 06:21
Default
  #2
Member
 
Fei Fan
Join Date: Jun 2013
Location: NanJing, China
Posts: 54
Rep Power: 10
Fanfei is on a distinguished road
Quote:
Originally Posted by jasonchen View Post
Hello everyone,

I'm using interFoam to simulate waves breaking on a sloping beach (two segments with slope 1:10 and 1:2). My problem is when the wave is about to break, the wave surface is not smooth anymore and small "ripples" seem to ride above the surface (refer to the 2nd link); and it's found that the final runup is not large enough when compared with expt data. This may be due to numerical errors, but I find most probably the turbulence model in openfoam dissipates too much energy and may cause the wave surface to deform in such a way. Does anybody encounter problems like this? I read on this forum that density missing in turbulenct transport equations may be responsible for such an issue. Any comments or suggestions on this? Thanks in advance.

The regular wave is generated using waves2Foam, and k-epsilon model is used as turbulence model. Mesh is refined uisng snappyHexMesh at swash zone and along the free surface area. Two plotts are given in the links below: one is for domain setup, another is a zoomup of free surface at swash zone when the wave is about to break.

Wave parameters: water depth=0.8m; wave period=1.0s; height=0.045m.
Inlet relaxation zone is adopted at wave generating boundary; surface elevation at the deep water is monitered and compare well with analytical solution.

https://www.dropbox.com/s/2sqnprqz4c...in%20setup.png

https://www.dropbox.com/s/vfn8y1accx...%20surface.png

Regards,
Jason
Hi jason
I meet the same problem as you mentioned. I wanted to test Kirby's experiment in Neil's paper, and I have added the density into the turbulence model, but there is no improvment in the simulation result. Have you solve this problem, and can you give me some advices on that. Thanks.

Best regards
Fan Fei
Fanfei is offline   Reply With Quote

Old   March 21, 2018, 04:04
Default
  #3
Senior Member
 
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 234
Rep Power: 14
vonboett is on a distinguished road
Hi there

I am stuck at the same point. The formation of droplets as soon as one aproaches a thin film of fluid is a classic problem of VoF methods ond I guess refining the mesh at the interface is the only way out. However, playing around with the surface tension term may help a bit.
vonboett is offline   Reply With Quote

Old   July 26, 2018, 04:15
Default Buoyancy-modified turbulence models
  #4
New Member
 
Brecht Devolder
Join Date: Oct 2014
Posts: 2
Rep Power: 0
brdvolde is on a distinguished road
Hi

This might resolve your problem of wave damping when applying a RANS turbulence model using interFoam:
The buoyancy-modified turbulence models are developed to simulate offshore and coastal engineering processes. The buoyancy-modified turbulence models not only result in a stable wave propagation model without wave damping but they also predict the turbulence level inside the flow field more accurately in the surf zone.

The source code of the buoyancy-modified turbulence models is available on GitHub for various OpenFOAM distributions: https://github.com/BrechtDevolder-UG...rbulenceModels.
Cheers
Brecht
wdx_cfd likes this.
brdvolde is offline   Reply With Quote

Old   May 17, 2019, 04:23
Default Stable closure + isoAdvection
  #5
Member
 
Akshay Patil
Join Date: Nov 2015
Location: Pune, India
Posts: 34
Rep Power: 8
Akshay_11235 is on a distinguished road
Hello everyone,


For the overproduction of turbulence there is an excellent solution provided by stable closure develoepd by Larsen B et al. 2018 have a look at that


https://www.cambridge.org/core/journ...D197CC5A007CDD


The installation files can be found at


https://github.com/BjarkeEltardLarsen


The issue with run-up could be improved by using isoAdvection


https://github.com/isoAdvector/isoAdvector


Hope this helps!
Akshay_11235 is offline   Reply With Quote

Old   May 18, 2019, 09:21
Default
  #6
New Member
 
sebastien vilfayeau
Join Date: Feb 2012
Posts: 14
Rep Power: 12
sebastien_F1 is on a distinguished road
Hi,



Unless you go to a very fine mesh. You will not be able to solve the breaking correctly.



You have to use isoadvector method and the interIsoFoam solver, see https://www.openfoam.com/releases/op...cs-isoadvector


Best,
Sebastien
sebastien_F1 is offline   Reply With Quote

Reply

Tags
k-epsilon, sloping beach, turbulence, wave breaking, waves2foam

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Scaling up a wave energy converter - free surface flow mark_l CFX 3 February 17, 2010 16:57
free sw to model ocean wave energy device? Allen Main CFD Forum 0 August 31, 2009 16:59
How to simulate a sea wave striking a ship antenna Freeman FLUENT 0 February 25, 2009 14:17
Wave energy devices Rui CFX 0 February 18, 2008 12:44
simulation of breaking solitary wave mehdi icho Main CFD Forum 0 July 2, 2002 04:35


All times are GMT -4. The time now is 18:48.