[jasonchen]

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

[Fanfei]

Originally Posted by jasonchen

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

[vonboett]

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.

[brdvolde]

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

[Akshay_11235]

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!

[sebastien_F1]

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