Hello,

My problem is connected with the behaviour of the inteface capturing method in COMET. I am calculating flows around double ended ferries. The problem appears when the angle between bow of the ship and the free surface plane is smaller then about 15 deg. In such case the mixture of the water and the air appears under the hull and convergence ratio is affected. From my observations this "phenomenon" is somehow connected with the type of the disretization scheme used for convective terms in momentum equations ( UD or CD ) and time step size ( see manual for Comet and the dependence of HIRC scheme on the Courant number).

1. Does someone experienced this kind of problem ?

2. Is there exist any possible cure ?

Thank You for answers and explanations

T.W.

I can give you some general advices for running COMET with FS. Actually, the algorithm is very stable but you have to follow some rules concerning the general setup.

1) use as much CD as possible on the momentum equations. You can start with 100%UD and increase the amount of CD you use (20%,40%,60%,80%,90%,95%,...)

2) you can use 100%UD in the air and the default value for the discretisation scheme on momentum for water (see user subroutine blndfc.f)

3) use as much HRIC as possible (do not use UD) for the calculation with interface-capturing.

4) for the seek of accuracy, use a time-step that gives you a Courant number of max. ~1.0 (look at the his2-file). Else, the HRIC algorithm will give wrong results, because you will try to fill/empty cells within one time step with more fluid the cell can receive/give.

5) There is a technique employed for getting faster results which consits in making one outer iteration per time step. If you have a blunt body for the ship, you are more likely to have a breaking wave in the front of the ship. The only way to capture it is either to use more outer iterations per time step and/or to lower the time step.

6) Check also your boundary conditions. The normal procedure is to set an inlet BC, Slip walls everywhere else, except at the oulet boundary where you prescribe the static pressure according to the desired water level (via usercoding userbc.f)

7) The computational domain should exted at least 3 ship lengths in front of the ship, 3 ship length to the side and 7 at the back. Y should coarsen the cells near the outlet boundary in order to avoid any wave reflection coming from the boundary.

8) If nothing helps, try to call support. As far as I remember, they have a very experienced naval engineer.

Thank you for Yours explenations 4xF. Excluding the CD schemes with blending factor equals 1 ( I am using 0.7 ) for both the momentum and the mass fraction equations, the way in which I approach my solution ( a time marching procedure ) and in which the boundary conditions are specified is similar to this proposed by you. You are also right that this kind of the procedure leads to the reliable solutions for standart hulls forms.

The devil lies somewhere else. Unlike the regular ships, double ended ferries have small draught and flat bottom part of the hull. My problem is connected not with the stability of calculations but with artifical air-water mixture which appears when I am using procedure described earlier. I think that this phenomenon is not physical since it depends on the discretizations schemes employed during the calculations. For the UD scheme ( which we want to use at the begining of the simulation ) the boubles of the air are convected downwind along the hull and they do not preserve their sharpness ( bigger number of outer iterations per time step helps here but problem is still transient ). When the resistance force is more or less constant ( usually it oscillates ) I am switching to CD and this mixture slowly disapears but even though I can not achive the pure water on the hull ( the concentation of the species not everywhere equals 1. on the submerged part of the hull ). Additionally the resistance force oscillates stongly, and calculations are very slowly convergent (one week on 4 processor cluster, 1.5 milion CV´s ).

If this is possible, could you also explain me in more detail Yours second tip 2). How different blending factors for air and water can influence solution ?

Thank You for help

T.W.

Concerning the blending factor for the mass conservation equation: do NEVER change the value to something less than 1.0. Else, you will get really crap results.

Concerning the oscillatory behavior of the forces, the strong smearing of the interface and the rather slow convergence, they may have 2 reasons: 1) breaking waves at the bow (you get them for very full ships) and also along the hull. 2) flow pattern is unsteady.

Workaround: Lower the time step (for Godness' sake, look at the value of the Courant number in the his2 file!) and use more than one outer iteration per time step (3 to 5 should be OK). Residuals at the beginning of one time step should slowly decrease to 10^-1, 10^-2.

Concerning the subroutine blndfc.f, you will find it in the directory $COMETDIR/usrc/userprog. Copy it to your userprog directory and modify it. You have only to modify the exmaple so that you can change the blending factor value for the momentum equations according to the local value of the concentration. For example, if c=0, then you use pure UD (BLF=0.0), if c=1, you use the value provided by the default settings. For values inbetween, a linear interpolation is sufficient, but feel free to use anything else if you want to.

Have fun...

4xF

Do you know about FLUENT VOF method resoults for flow calculation past ship hull?