I have spent about two months trying to simulate a half wigley hull in a domain with 10m long x 2.25m width x 3m high with a half hull in a symmetry plane, 2 m from the inlet + 1m hull + 7m to the outlet = 10m long. The aspect ratio of the mesh is between 1.25 and 20. Determinant 3x3x3 is over 0.95. B.C. at inlet is normal velocity and Outlet is Static Pressure.

In the solver control when I select Upwind at Advection Scheme the simulation always crashes in less than 10 iterations with the message error "Floating point exception: Overflow"

It doesn't matter if I set a less Physical timescale for Volume Fraction. Any combination of timesteps end up crashing. Even following the CFX manual recommendations for timestep values as a fraction of the particle residence.

When I select High resolution at Advection Scheme and Physical timestep I obtain oscillatory results in RMS quantities.

Although, local timestep factor seems run the final solutions is far away of the expected results.

How could I figure out this parameters in the Solver Control in order to obtain a solution.

Thanks in advance,

Carlos Andrés.

"inlet is normal velocity and Outlet is Static Pressure."

You need to set a volume fraction weighted hydrostatic pressure BC at the outlet.

"In the solver control when I select Upwind at Advection Scheme the simulation always crashes in less than 10 iterations with the message error "Floating point exception: Overflow""

Getting convergence in free surface flows is hard. CFX11 has major improvements in this area.

Start with something simpler e.g. 2D breaking dam problem. Get this working well against experimental data to get a feel for the CFX free surface numerics.

Hi Joe, Thanks for answer,

Also with a VF weighted hydrostatic pressure at the outlet, the simulations crashes with the same message about overflow. I am running CFX11. Now I am playing with BC at the oultet with different physical timpesteps in both equations and Volume Fractions as a trial and error,after that suggestions on CFX manual didn't work. That's no the way, but there's no more options of trial and error.

It supposes that Wigley Hull is on of the straightforward benchmarks to valide simulations, but it really takes a lot of time to input the criteria both in ICEFM and CFX.

I will be grateful if you tell me more advice.

Get a simple damn break problem working first.

Dear Carlos Andres,

The numerics changes for multiphase flows in CFX 11.0 have shown remarkable improvements for free surface flows, in particular the Wigley hull case.

Since this case has already been solved/setup/benchmarked you are better off asking your help desk representative about CFX setup or any available information on how to run this particular case.

Opaque.

See this posting. Looks like they may be trying similar things.

http://www.cfd-online.com/Forum/main.cgi?read=51667

Hi Carlos,

there could be a number of things going wrong in your problem. I used CFX for some hulls a few years ago and it worked pretty well there are some tricks, however and lots of places to go wrong.

1. Do as Joe says and get the 2D bump working, play with mesh, numerics, time steps, etc

2. Set-up a channel flow without the hull and get that working. If you get your physics (reference density, outlet boundary condition, etc) mesh, discretization, time step, etc all working then you should see a nice level water channel. Get a feel for the how the mesh, discretizations and time steps affect your solution here.

3. Add your hull to 2 above and start playing with the domain size, mesh, discretization, time steps etc to validate your case

Some important things to think about:

- reference density: make sure your "reduced pressure" distribuion for hydrostatic pressure is set accordingly

- domain size there is a trade-off that too close of boundaries will affect the results due to waves reflecting, etc BUT too far of boundaries will waste cells that are better off resoving the boundary layers and interface!

- outlet boundary location and specification: the assumption of hydrostatic pressure distribution is slightly in error but this error decreases as you move into the far wake. I found about 3 hull lengths were adequate but that depends on wake shape, Froud number, etc.

- inlet boundary location: about 1 hull length is adequate but the levels of k and epsilon...really what you want is turbulent eddy viscosity specified at the hull depends on what you set at the boundary and how far away it is. Too far away and any level of k will dissipate to zero since there is a finite dissipation rate but no production.

- mesh: basically you need to resolve the boundary layers and the interface. Boundary layers you had better see the velocity profile. Interface you had better see red and blue for Volume fraction distribution at the interface.....not a lot of colours...keep refining at the interface till you see about 2 rows of cells that have volume fraction smearing.

Opaque,

what is new in the numerics?

Hope this helps,

Bak_Flow

Dear Bak_Flow,

ANSYS CFX 11.0 introduces a higher level of coupling between the multiphase equations. In particular, the volume fractions discretized equations are fully coupled with continuity and momentum equations while they were segregated in previous releases. This coupling has shown considerable convergence improvements for free surface flows.

In CFX-Pre, go to Solver Control/Advanced Options/Multiphase Control/Volume Fraction Coupling. Available options are Segregated and Coupled.

Hope this helps,

Opaque

Hi Carlos,

If you are still having trouble, have you tried, or are you using

(a) double precision-generally better for F-S calculations?

(b) to use the zero gradient outflow boundary condition

(c) to align the mesh with the initial free surface - this may mean using a hexa mesh

(d) have you compared RMS and MAX residuals (and written the residuals to the output file), this generally helps working out where it is all going wrong.

Can only agree with Joe and Bak_flow, get something simple to work and then go from there.

Good Luck

latslosh