Hi, I am trying to simulate in CFX 5.6 a hull form in order to see the wave pattern. I always get an error message when trying to solve..'water and air is trying to get into the domain from the outlet' I tryed changing into an openning BC but still the same. I changed the dimensions, maybe it was to close to the action but still the same.

Does anybody have an idea? Thanks in advance! Joe

Hi,

Do you still get that message with an Openning BC? What is exactly the message?

How have you defined the other BCs? What are the hull and the domain dimensions?

Regards,

Rui

I ll answer your questions one at a time:

"Do you still get that message with an Openning BC? What is exactly the message?"

Yes i get it with the openning BC, the message is 'Fatal overflow in linear solver' and then says that water and air is trying to re-enter in the domain from outlet.

The other BC are: inlet, outlet, Top,Bottom & left -Free wall surface Right wall - Symmetry.

dimmensions are as in real life, there was no scale down made to it. 150m x 25m x 17.3m With a hull length of 41m.

Another thing is that CFX places walls by itself, is this normal?

Thanks

Hi,

CFX places a wall on an Outlet BC when the fluids try to enter the domain through that boundary. When the boundary is defined as Opening the fluids are allowed to leave and to enter the domain.

"Fatal overflow in linear solver" probably means that something is wrong in your simulation. Have you defined the initial pressure, and the pressure at the inlet and the outlet (Opening) boundaries, as in Tutorial 7 (Free surface flow over a bump)?

Regards,

Rui

I have defined the pressures as in tutorial 7.

But the only thing is that there is no water level difference in the inlet and outlet as in Tutorial 7, so from Tutorial 7 is not so much help with the Volume Fractions which may be the fault in my simulation.

This is my project in the university and i need to figure out a solution. Do you know any other tutorial or place to look for free surface simulations?

Thanks in advance!

A good diagnostic tool is to carefully check your inititial conditions.

You can do that by setting the EXPERT PARAMETER 'backup file at zero = t'.

You should also carefully check your inlet/outlet boundary conditions and make sure that the pressure profile you have specified makes sense for the approaching flow (especially to the outlet). If the profile you have specified is different than what the flow naturally wants to do then it can make the solver blow up.

Neale

Thanks for your message Neale! Using the expert parameter i did find an error with the volume fractions of the water and air. But i always get 'fatal overflow', there something with the pressure profile like you said.

Since is with a hull, there is no water level difference. I have defined the outlet-static pressure-Pressure depending on volume fractions. I can't seem to get anything correct with the pressures..

Thanks in advance!

Well, fundamentally there is not much different from a flow past a hull and flow over the free surface bump. For sure many free surface flows past hulls have been done before.

To figure it out you may have to get into the details of what is going on in the flow before the fatal overflow occurs. i.e. stop the solver a few timesteps before it happens and write a result and see what the flow looks like. If it looks ok then stop it right before and see where things are going crazy. This may give you some clue as to what is wrong in your setup.

Neale

Hi,

are you running in parllel?

There can be some issues if the interface and the parallel partition are co-incident. Have a look at the real partition number field in Post.

If the flow is in the x-direction then I would partition with direction specified slices along constant-x.

If things still are problematic, take it back a few iterations and then run serial to see if there are any differences around the failure point.

Let us know what works... ;-) or didn't

Good luck...........Bak_Flow

Thanks for your advices they were helpfull! I come accross another problem, when using k-epsilon model the simulation failed with 'fatal error in linear solver' but when using SST it could solve with no problem.

Has anyone have any suggestions? Thanks in advance!