[RenanJ]

Good afternoon, experts

I'm trying to simulate a planing hull against head waves to study vertical acelerations. I set a 5th order wave and I am using a inlet condition on the domain side, but as my simulation goes on the wave amplitude starts to get dampened, even though the damping function is turned OFF, I checked and rechecked if I wrote a wrong boundary condition but I found nothing wrong, I set for the velocity the wave field function, the same for the volume fraction of the light and heavy fluid, and hydrostatic pressure field function for my outlet.
the images attached are the wave scenes with a scalar Z position function

Thank you in advance.

[Ubuntu]

I believe the front is kept as velocity inlet and back as pressure outlet.
Can you tell me what are the conditions on top, bottom and side walls?

Originally Posted by RenanJ

...as my simulation goes on the wave amplitude starts to get dampened, even though the damping function is turned OFF...

I see some rise in wave height on the sides (2nd picture). Is that the problem?
Or you are not getting the wave height you entered (in wave properties) when you do simulation? (Say you kept wave height as 0.1 m but it gives only 0.05 m, measured at an appropriate location)

[RenanJ]

My Boundary conditions are pressure outlet for the back, velocity inlet for the front, bottom, top and side and symmetry plane at the diametral plane.

I am not getting the wave height that i prescribed at the inlet, thats why I guess the side still has the original height, since it's a boundary condition it has to satisfy the wave I prescribed. My teacher told me this is because I am using a first order discretization and it's very difusive.

Please enlighten me! the VOF solver is by default set to 2nd order, is there any other spacial parameter wichI have to change to 2nd order that I am missing?
Also I should switch my temporal discretization to 2nd order also? If so I have to change my time step so the wave propagate less than half a cell per time step right?
Sorry for so many questions, but so far I have dealt with tasks interested only in the permanent regime, I am using 40 cells to discretize the wave longitudinally and 20 cells for the wave height. Is that also not enough?

[Ubuntu]

Originally Posted by RenanJ

Also I should switch my temporal discretization to 2nd order also?

I think yes.

Originally Posted by RenanJ

I am not getting the wave height that i prescribed at the inlet...

How did you check that? Did you make a plot?

My suggestion is to keep your mesh settings at the free surface and time step according to your wave properties. There are some guidelines by ITTC. You can check them.

Like,
1.For volumetric control at free surface, 40 cells per wave height and 80 cells per wave length (you can try smaller values, may be during grid independence tests).
2.100 time steps per wave period

If you are using overset meshing, refinement at the free surface should be done considering the cell size in the overset region.

Hope this helps.

[raquelcfd]

Hello RenanJ,

I have the same problem. I am trying to simulate a wave model with a floating body and I am detecting that the created waves are not the ones that I specified in the wave model. My scenes show same problems as yours.

Have you tried to do the simulation without the body?
Cause I tried to do it, and even without the body i did not get the amplitudes.

Have you found any solution?


Regards

[RenanJ]

@Ubuntu i used a scalar function os position z at the free surface.

@raquelcfd Some people from other labs told me this happens because the vof model is very difusive and advised me to rerun The simulation using a second order discretization since we are interested in the transient behavior. I searched for star ccm+ guidelines and we have to set the time step so the wave don't advance more than half cell, also for this case we should optimally set the CFL at the free surface under 0.5 for optimal results but every value under 1 is fine. Finally, I was not yet able to test those settings since I'm simulating a classmate's final project. But I'll rerun the sim next week. If you have good results before me please share it!

[Ubuntu]

Originally Posted by RenanJ

i used a scalar function os position z at the free surface.

Please plot a wave height vs time graph (check this thread) and make your conclusions on this quantitatively. Colour bars in the scalar scene are not enough for this, I feel.

[raquelcfd]

@RenanJ I will try the recommendations. Even so, I have defined my tank’s sides as symmetry planes, not velocity inlet.
However, I still have problems with the wave amplitude at the end of the tank (red line). Now I am working without any floating body, then amplitude should be constant in the tank.

[raquelcfd]

Hello @RenanJ

Do you have any news on this matter?

[ksss]

Has anyone solved the problem regarding the damping..I am also facing the same situation regarding damping.. in my case the the wavve at the outlet has damped down to zero and on further running simulation the the whole pattern went below zero

[Marpole]

In your dynamicMeshDict, you might use scale which ramps down the wave amplitude over distance.

Originally Posted by ksss

Has anyone solved the problem regarding the damping..I am also facing the same situation regarding damping.. in my case the the wavve at the outlet has damped down to zero and on further running simulation the the whole pattern went below zero

[minh khang]

Originally Posted by Marpole

In your dynamicMeshDict, you might use scale which ramps down the wave amplitude over distance.

Charles,

Really?
Can you explain more about this?