Submarine Free Surface
 

Hi,

I am attempting to simulate a submnarine travelling just bellow the surface at a constant speed and then compare the data to tank testing.

I am using ANSYS CFX, A homogenous free surface model, SST turbulence model, A structured 2.2mil mesh with a y+ less than 2.

I am modelling the submarine in the tank.

When I have not free surface it solves quiet quickly however when I add in a free surface the steady state will not converge and the transient state takes a very long time (weeks) I am running the solver on 8 parrallels.

Can anyone offer some advice from previous expeience? Do I need to run transient simulations or can I use steady state?

I can provide pictures if neccassary

Cheers,

Sam

Hi,

Yes, you can do free surface simulations steady state but they are tricky. Usually the problem is little transient waves away from the area of interest (often generated at the boundary conditions) which make converging to a steady state solution difficult. Running transient deals with this issue better but takes forever to run.

I think there is a boundary condition in CFX which may help, the non-reflecting boundary. Hopefully it can improve the way the surface waves are dealt with at the boundaries and make obtaining a steady state simulation much easier. I think it is a beta thing, I am not sure. If you cannot work it out you will have to talk to your CFX support person about this option.

Thanks very much Glenn that is exactly what I am finding.

My issue with the transient runs is that my drag coefficient oscillates and the amplitude is quite significant. I thought the issue was the size of my time step (Courant Number) however have found that it has little effect.

Can you make any suggestions?

Regards,

I would have a close look at it and try to determine whether the oscillation is real. Can you see the water surface rise and fall with the drag coefficient? In that case the oscillation is probably real.

Glenn,

I am more than happy to send you the post file. It does fluctuate even in a steady state run, I am aware CFX still uses a flase time step to increase stability maybe this is why?

In theory a standing kelvin wave pattern would develop which wouldn't cause the drag coefficent to fluctuate? But again this may be why my transient residuals converge a lot quicker than my steady state.

General information on this issue can be found here:
http://www.cfd-online.com/Wiki/Ansys...gence_criteria

But as I said I suspect the specific reason in this case is reflections off the outer boundaries. That is why I suggest investigating the non-reflecting boundary.

Another option I just remembered (I read a journal paper where a guy did this to make a non-reflecting boundary, it is a great idea) is to surround your mesh with some very coarse elements (say 10 or 20 time greater edge length than the actual mesh in your domain) and connect these coarse elements to your real domain with a GGI. Apply your normal boundary conditions to the outside coarse elements. The coarse elements damp out the waves which enter it through the large numerical diffusion in large elements and, in effect you end up with a non-reflecting boundary. I have never tried it but it sounds good.

Have you tried mesh adaption at the surface? This is also a way of eliminating spurious waves.

Mesh adaption reducing the spurious waves? A finer mesh will make it worse due to reduced dissipation. Also refinement has the usual general effects of making convergence harder and run times longer. It does not sound like the way to go for me (but please tell me why if you think I am wrong!)