[totalBeginner]

Hey Pablo,

thanks for your fast reply! I was thinking about using just two or three particles, but also in 3D, do you think that might work?

Cheers, Kryss

[Phicau]

Hi Kryss,

any small number of particles will work fine, I was talking about millions, each representing a sediment grain.

Hi Abas,

what you are experiencing here is the infamous build-up of turbulence. Basically your turbulence values grow and grow, pushing the turbulent viscosity to a very large value (check your nut field...), thus damping the waves significantly. A solution may be simulating the case without turbulence (laminar regime). You should also expect some degree of reflections at the outlet, not very high, though, since your wave conditions are in intermediate waters.

Best,

Pablo

[kmargaris]

Hi Pablo,

I am trying to model a solitary wave, but the wave generation doesn't work as expected. I have attached my case. The wave height is 5.18m and it is not above the breaking wave height for the water depth, but it seems that the wave breaks as it is generated.

Any thoughts as to what the issue is?

[smh]

Dear Pablo,
Hello

Thanks in advance for your time and patience.
I have two parameters from a series of irregular waves (Tp and Hmo).
I wanted to know whether is it possible to produce irregular waves with wave generation BC in OlaFoam or not?

Best regards,

Mahdi

[Phicau]

Hi kmargaris,

I will check it.

Hi Mahdi,

yes, you can. Get the parameters, apply your favourite spectral shape (e.g. JONSWAP), discretize it into individual components and apply random wave phases to these. Then you can feed them to the irregular wave type in olaFoam. You can also switch on second order wave generation for irregular waves. Check the reference materials for more info.

Best,

Pablo

[totalBeginner]

Hey Pablo,

I've watched this video: https://www.youtube.com/watch?v=dNffOs-1Esw
How did you implement the current? I have my problems with setting a velocity of the fluid in x-direction.

I'm using regular Stokes 1 waves.
Cheers,
Kryss

[Phicau]

Hi Kryss,

please research and read yourself; olaFoam includes simultaneous generation of wave and currents and there is an example that is ready to run (currentWaveFlume). The code is fully open source, so the implementation is in GitHub.

Cheers,

Pablo

[Phicau]

Hi kmargaris,

the problems are most likely caused by the low order solitary wave theory, plus maybe mesh issues.

I have included in the code a new type of solitary wave: Grimshaw. This is third order accurate.

I have tested the same wave and depth conditions, but with a homogeneous grid (20x20cm) and the wave looks OK. I suggest that you get the latest version of the code and try again with this new implementation:

waveType        solitary;
waveTheory      Grimshaw;
genAbs          1;
absDir          0.0;
nPaddles        1;
waveHeight      5.18;
waveDir         0.0;

Best,

Pablo

[kmargaris]

Hi Pablo,

Thanks for looking this further. I tested the new solitary wave theory in my model and the wave generation works much better now.

Do you have a reference of this new theory?

Best regards,
Kostas

[Phicau]

Hi Kostas,

the reference is "The solitary wave in water of variable depth. Part 2", Grimshaw (1971), but it is more understandable in "Measurement of velocities in solitary waves", Lee et al. (1982).

Best,

Pablo

[Peter&Anders]

Hi Pablo
We are two master students writing about waves propagating over a submerged breakwater and we are using OpenFOAM and OLAFOAM.
We have run into a problem in our model, where we are trying to recreate the experiment done by Beji and Battjes in “Experimental investigation of wave propagation over a bar” 1993 (see http://www.sciencedirect.com/science...7838399390022Z), to validate the use of OLAFOAM for our case. The problem lies in that for increasing mesh size, the waves (generated using Stokes V, with H=0.041, T=2.5s) does not converge after breaking but instead keep increasing in wave height and goes way beyond the experimental results, as seen in the figure attached (Convergence_Turbulence). We are using the k-epsilon turbulence model, a courant number of 0.3, a grading of 2 towards the water surface and snappyHexMesh to smooth the mesh near the bar.
We have tried to increase the length of the model before the bar, and also increased the height of the model to no real change in the results. We also tried to turn off the turbulence in “turburlenceProperties”, where there is a significant change in the wave trough and the waves gets offset after breaking for the coarse mesh and fluctuating results for the fine mesh, see “Turbulence_vs_no_turbulence” attached.
We would like to ask if you have any ideas as to what might be wrong in the model as it overestimate the wave height using turbulence, and seems unstable for cases without turbulence. We have attached a zip-file with the model-setup in OpenFOAM, a figure showing the model setup and position of wave gauges “Figure model setup.pdf” and the two figures mentioned above: “Convergence_turbulence”, “Turbulence_vs_no_turbulence”.
We hope you can help us J
Best regards
Anders and Peter
Aalborg University - Denmark
BejiBattjesTestOpenFOAM.pdf

Convergence_Turbulence.pdf

Turbulence_vs_no_Turbulence.pdf

OpenFOAMSetup.zip

[HosseinB]

I have recently modelled a near-breaking wave-structure interaction using OLAFOAM.


I had to neglect the turbulence because the turbulence led to unrealistic damping of waves travelling in the numerical tank.

Cheers,
Hossein

Originally Posted by Peter&Anders

Hi Pablo
We are two master students writing about waves propagating over a submerged breakwater and we are using OpenFOAM and OLAFOAM.
We have run into a problem in our model, where we are trying to recreate the experiment done by Beji and Battjes in “Experimental investigation of wave propagation over a bar” 1993 (see http://www.sciencedirect.com/science...7838399390022Z), to validate the use of OLAFOAM for our case. The problem lies in that for increasing mesh size, the waves (generated using Stokes V, with H=0.041, T=2.5s) does not converge after breaking but instead keep increasing in wave height and goes way beyond the experimental results, as seen in the figure attached (Convergence_Turbulence). We are using the k-epsilon turbulence model, a courant number of 0.3, a grading of 2 towards the water surface and snappyHexMesh to smooth the mesh near the bar.
We have tried to increase the length of the model before the bar, and also increased the height of the model to no real change in the results. We also tried to turn off the turbulence in “turburlenceProperties”, where there is a significant change in the wave trough and the waves gets offset after breaking for the coarse mesh and fluctuating results for the fine mesh, see “Turbulence_vs_no_turbulence” attached.
We would like to ask if you have any ideas as to what might be wrong in the model as it overestimate the wave height using turbulence, and seems unstable for cases without turbulence. We have attached a zip-file with the model-setup in OpenFOAM, a figure showing the model setup and position of wave gauges “Figure model setup.pdf” and the two figures mentioned above: “Convergence_turbulence”, “Turbulence_vs_no_turbulence”.
We hope you can help us J
Best regards
Anders and Peter
Aalborg University - Denmark
Attachment 54404

Attachment 54405

Attachment 54406

Attachment 54407

[Peter&Anders]

Hello Hossein.

Thanks for your answer. We have reached the conclusion that we have to exclude the turbulence as well. This seems like a reasonable assumption, as we assume smooth surfaces in the model.

Regarding the "spikes" in the model without turbulence, this seems to be caused by the definition of alpha, as the wave breaking mix water and air, leading to a large area of alpha between 0.2 and 0.8, fluctuating around 0.5. We are truing to solve this in a more elegant way than up until now.

Best regards
Peter and Anders

[totalBeginner]

Hey Pablo,
I've simulated cases with stokes I and with stokes II, besides the different wave theory, they were exacty the same. But when I compase those two cases, there's a phase shift in the X- and Z-velocity. So I was wondering, if OlaFoam coincidentally chooses to start with going down into a wave through or going up into a wave crest? If not, do you have any idea why it might behave that way?

And I also implemented a current of 1 m/s in x-direction, but there only seems to be a x-velocity of 0.5 m/s in the simulation? To implement it I've done exacty what this video (https://www.youtube.com/watch?v=dNffOs-1Esw) says...

Thanks a lot for your help!
Kryss

[Phicau]

Hi Kryss,

I will check tomorrow the Stokes I and II issue.

Just a quick check, have you changed the current velocity both in setFieldsDict and waveDict?

Best,

Pablo

[totalBeginner]

Hey Pablo,
no, i didnt do that I just changed it in the waveDict and the 0/U-file... Silly me!
But it still worked. How bad is it? Do you think the simulation has an informative power?
thanks!

[Phicau]

Hi Kryss,

thanks for reporting the discrepancy, I have been able to reproduce it and will try to correct this bug soon.

In the mean time, if you want the same phase in Stokes I case, use pi/2 value for wave phase instead of 3pi/2.

Best,

Pablo

[Phicau]

Hi Kryss and all,

I have fixed this issue, you can update your code from github and recompile it.

Be aware that now everything is consistent with StokesI theory. This means that, unlike before, phase pi/2 will start at still water level and generate a crest first. Phase 3pi/2 will start at still water level and generate a trough first.

Best,

Pablo

[zanis]

Hi Pablo,

I was generating wave in wavemakerflume, by changing H,T and h in flapWaveGen.py and of course increasing height of flume in blockMeshDict water level not changing at all and is stable at 0.4.
How can I increase water level?

Thanks in advance
Zahra

[challenger149]

Hello everyone,

Is it possible in olaFOAM to model a flume containing air, water and another fluid with different viscosity and density beneath it to track the interface between them?

Regards,
Mohammad