
[Sponsors] 
April 12, 2007, 13:35 
Timestep in Free Surface Wigley Hull

#1 
Guest
Posts: n/a

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. 

April 12, 2007, 16:45 
Re: Timestep in Free Surface Wigley Hull

#2 
Guest
Posts: n/a

"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. 

April 12, 2007, 17:01 
Re: Timestep in Free Surface Wigley Hull

#3 
Guest
Posts: n/a

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. 

April 12, 2007, 17:23 
Re: Timestep in Free Surface Wigley Hull

#4 
Guest
Posts: n/a

Get a simple damn break problem working first.


April 12, 2007, 20:56 
Re: Timestep in Free Surface Wigley Hull

#5 
Guest
Posts: n/a

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. 

April 13, 2007, 09:11 
Re: Timestep in Free Surface Wigley Hull

#6 
Guest
Posts: n/a

See this posting. Looks like they may be trying similar things.
http://www.cfdonline.com/Forum/main.cgi?read=51667 

April 13, 2007, 09:15 
Re: Timestep in Free Surface Wigley Hull

#7 
Guest
Posts: n/a

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. Setup 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 tradeoff 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 

April 13, 2007, 13:30 
Re: Timestep in Free Surface Wigley Hull

#8 
Guest
Posts: n/a

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 CFXPre, go to Solver Control/Advanced Options/Multiphase Control/Volume Fraction Coupling. Available options are Segregated and Coupled. Hope this helps, Opaque 

April 29, 2007, 16:38 
Re: Timestep in Free Surface Wigley Hull

#9 
Guest
Posts: n/a

Hi Carlos,
If you are still having trouble, have you tried, or are you using (a) double precisiongenerally better for FS 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 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
free surface around a ship hull  Stephy  OpenFOAM Running, Solving & CFD  12  April 24, 2012 01:12 
CFX convergence issues with free surface  adenlan  CFX  3  September 2, 2011 06:43 
Can Flow3D plot the free surface area in Isosurface or colour variable?  therockyy  FLOW3D  1  June 20, 2010 19:36 
Free  Surface Flow: Split Fluid Forces acting on a Boat Hull  eee  CFX  2  August 28, 2009 08:36 
CFX4: Free surface grid movement algorithm  JEYA  CFX  0  November 7, 2007 08:47 