Hi,

Has anyone done any ship resistance problems? I'm using CCM+ 2.06.004, and I'm trying to solve for the wave pattern as an implicit unsteady problem using VOF for the wave profile. The problem starts off ok, and the wave pattern starts to look about right, but i find the longer i run my problem, the further my resistance values decay, and i don't seem to be able to get a steady state solution at all. Any suggestions on these kind of problems?

... what time step is used? How many inner iterations?

... take care for high grid resolution where both phases are mixing!

I am using a time step of 0.025s, and 15 inner iterations.

I'm also using k-epsilon for turbulence, any thoughts if I should change that?

... may be try time step 0.01s to 0.0025! ... may be inner iteration of 10 will do!

... I have no arguments agains k-epsilon, but check if your boundary layer thickness is ok (use Y+)! This is a little bit difficult, because of the two layers! So may be try to optimize for the water area!

... have a look if your surface tension, gravity and buoyancy is on/correct! Otherwise you will get funny results!

... no more ideas so far!

Good luck!

Dan,

Seriously consider contacting CD-adapco and asking for advice and assistance in setting this up properly.

To calculate the wave pattern around a ship hull you have to calculate a sharp interface between the two fluids. Mixing the two fluids will at best smear the interface leading to poor results and at worst leave you with a two-phase mush and no wave pattern.

Also a ship is subject to dynamic sinkage and trim effects. How are you including these in the calculation? STAR-CCM+ currently does not support moving mesh.

The best advice you will receive today is to call CD-adapco.

Regards Peter

Could you describe your boundary conditions (eg. outlet domain)?

Regards, pp

Thanks for the help and input to everyone who's contributed, its much appreciated.

Just to give a brief description of my problem set-up to those who've asked, and a run down as to what I've figured out so far:

I use a user function for hydrostatic pressure on my outlet, and I define the water level at both my inlet & my outlet, and initialize it in initial conditions as well.

I had a refinement layer to capture the wave pattern locally for a few ship lengths around the hull, this was giving me problems, as it creates numeric waves where the refinement layer ends. This refinement layer needs to be extended as far upstream and to the side as the mesh goes!!!

Around the keel and bulbous bow, the extrusion layer tends to collapse around, I found that was contributing to my oscillating resistance values (still trying to figure out how to resolve this, any ideas?). I create my surfaces in a program called Rhino, then import to ProSurf to triangulate / fix the iges surfaces, before I can get it into Star CCM+ I need to find ways to improve this process.

Sinkage and trim are an issue. I have a large volume of experimental data for similar hulls, so I tend to approximate the sinkage and trim for each hull rather than ignore it or try to calculate it iteratively. Fortunately for large vessels at moderate Froude numbers, sinkage and trim can be quite small.

I've also been working with CD-Adapco as well. Thanks again everyone for your help.

Dan,

What sort of advice did CD-adapco provide on this issue?

Just curious ...

Regards Peter

In the end, my biggest problem was having refined cells around the hull to get low y+ values. This was giving me all sorts of problems at the free surface, and in general needs to be avoided. I've found that the free surface is extremely sensitive to mesh transitions. The guys at CD-adapco had quite a thorough look through my model, and this is the conclusion we came to. This of course leaves you with quite a few cells, but i've now finished quite a few different hull forms successfully, with accurate results compared to experimental work.

[Fn80]

so finally,how you proceed?
changing growth rate?