Learning Forum

[DanielOliveira]

Hello,

I would like to have some help with my study case on Fluent. I'm simulating wave propagation in a 2D wave flume model using VOF with open channel model, generating Stokes second order waves with H = 5 cm, T = 0.86 s (L = 1.07 m) and a water depth of 27.5 cm. I'm using a mesh refinement on the water surface envelope with 80 CPL-X direction, 20 CPH - Y direction and a time-step of T/200. The CFL condition is around 0.6. 

The problem is that the waves are losing energy (height) during the propagation phenomena in the domain. I'm analyzing the surface elevation at 0.5 m, 1 m, 2 m, 3 m and 6 m from the inlet. The results are presented in the attached file. 

Thank you in advance,

Best Regards

Daniel

[DanielOliveira]

[Amine Ben Hadj Ali]

For open channel flow you need to take care about domain extents and here you need to be very generous: Above the free surface you need at least 1.5 wavelength. At least 30-40 cells per wave height and length are required to reduce diffusion and dispersion errors and a time step to around T/100 or T/200. Also add a sort of sponge towards the outlet (coarse mesh)  and beach to reduce reflection.

 

[DanielOliveira]

My domain is 5 m length with regular mesh, 5 m length with a coarse mesh and 0.75 m height (I will try to increase it for 1.5 wavelengths, but since I set-up the upper boundary as pressure outlet with 0 gauge pressure, should it has so much influence?). I also refined the water zone below the water surface since in the future I will also have an obstacle there. In terms of the beach, would you suggest a numerical beach or it needs to be a geometrical beach? 

 

Thanks for your advices,

 

Best Regards,

Daniel   

 

 

 

 

[Amine Ben Hadj Ali]

Set up the top boundary to be symmetric if you are extending into the height (1.5 times wavelength is really a minimum). It might be you are getting some reversal flow of air from the top if pressure outlet is near the free surface.

 

I am talking about numerical beach + sponge coarse cell zone towards the outlet.

[DanielOliveira]

Hi,

 

I already set up the top boundary as symmetric and increase the height of the domain to 2 times the wavelength. The same level of damping is obtained. I also performed some simulations with a different number of cells per wavelength (50 and 70) and number of cells per wave height (20 and 30). The differences between the analysis are negligible. Do you have some more ideas about the origin of it? 

 

Best Regards

Daniel  

 

[Rob]

What's the bottom boundary set as? 

[DanielOliveira]

The bottom is set as a wall.

[Amine Ben Hadj Ali]

Are u using a fine time step resolution? Check if the deployed wave theory is appropriate.

Again dispersion and diffusion might dampen the wave evolution.

[DanielOliveira]

I'm using a time-step of T/200. I already tried with T/1000 but the results were the same. 

The deployed wave theory is correct. I also confirmed it in fluent. 

I'm checking the boxes of VoF: interfacial anti-diffusion and implicit body force. Is it correct?

I also tried to start the simulation with the wavy state, and after a few seconds, the waves start damping to the same values that I'm obtaining starting with the flat wave. 

Any advice?

 

Thanks

[Amine Ben Hadj Ali]

You can try making the domain much more longer and to check whether numerical beach is affecting the waves.

You need to compare for certain flow time the wave profile from the run with the analytical solution.

That is all what we can recommend or do without looking into the case on this open community.

[DanielOliveira]

Ok thanks.

Just one more questions before close the topic. Is it possible to create a report where I can check the wave profile at all domain at every time-step? if yes, how?

 

Best Regards

[Amine Ben Hadj Ali]

No there is no such an automatic report. What you can do is to record in a journal what you did in Fluent to create the plot and execute that at N time steps for example