Hi, I'm trying to get a correct wave profile along a ship hull but, although the general shape is correct, still I got a wave crest near the bow which is double than what measured in model tests.

Here is my coputational data: Ship lenght l=128 m Ship speed u=13.88 m/s Lenght scale 1:20 Domain shape: 1/4 cylinder - 1 ship lenght forward of ship bow, 2 ship lenght aft of ship stern and 1.6 ship lenght cylinder radius.

I have left 10 m of air (in full scale) above still sea surface.

Boundary conditions: similar to the one used in the tutorial "Free surface flow over a bump" with few exceptions.

Reference pressure = 1 [atm]- rho * g * z * VFWater

After few computations I noticed that I always obtain some dirt close to the lateral boundary (where it seems that an opening works better than a free slip wall) that probably affects the wave close to the hull.

Many thanks to anybody could give me a hint

Andrea

Hi Andrea,

your domain seems reasonable as discribed. The size of the air zone in the top is relatively unimportant so long as it is big enough to not touch any part of the wave. The momentum contributions there are 3 orders less than the water and therefore negligible.

You mention the scale? Are you running the real experimental conditions or some scaled result? I would strongly suggest running the experimental conditions and compare to raw data.

How fine is your mesh in the area of the bow wave? Have you done any refinement in the region of the interface? I would recommend a layer of 20 (or more) prisims (or hexes if you can?) along the calm-water line as a starting point.

What is your convergence like? On these problems one often must look (in addition to residulas) at some important integral quantity like drag or displacement, etc. You mention that some dirt (noise or wiggles) are entering the domain. What does this look like? Does it introduce reflecting waves? How big are the disturbances?

Regards,

Bak_Flow

Hi,

I am running the code at model scale which is 1:20 exactly equal to the scale used for towing tank tests. Velocity are scaled according to Froude number (Fr=0.4).

My grid is a structured grid (1.5 million nodes) and I have made refinements close to the water line. Consider that I have at least 40/50 layers in the interface region (from crest to hollow of the bow wave).

I have not monitored integral quantities but just RMS values of velocity residual which were decrising initially quite nicely although did not go below 10-3 (and oscillating with high frequency around this value).

Finally the problem developped from the boundary. In the far field on the side of the hull I have obtained a sea surface surge close to the boundary when I impose a free slip (it appears all along the boundary starting few lenght from the inlet and until the outlet). Imposing an opening (with prescribed pressure) things were a bit better. Note that the waves generated by the hull does not reach the boundary and therefore I think this problem is not related with a reflecting waves. However it probably does influence the wave pattern close to the hull.

I have noticed there is also a small transversal wave in between the inlet and the ship which I don't know from where it is generated.

I wonder if my problem is more related with the grid or with the imposed BC.

Thanks a lot regards, Andrea

Hi Andrea,

it seems as though your grid and domain are more than adequate...sounds like you know what you are doing ;-)

I have actually seen the problems you discribe for sub-critical flows (and they get worse as the Froude number decreases). I concluded that it was some error reflection from the outlet. I concluded this because when I artificially went super-critical....I dropped g to something small...the interface upstream of the hull was smooth as glass! Try that if you can? I would be interested to see some pictures if you can put them up here??

The problem is far less prominent if you have a coarse grid but since you are doing fine work it shows-up.

Regards,

Bak_Flow