CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Free surface in mixing vessel (http://www.cfd-online.com/Forums/cfx/109646-free-surface-mixing-vessel.html)

blubb1612 November 22, 2012 12:46

Free surface in mixing vessel
 
Hi all,
I'm quite new to CFX. I want to simulate the flow in a mixing vessel. It's a steady state simulation. The vessel has no inlet and no outlet. I only set boundary conditions for the walls and an opening boundary condition.
And here is my problem. It's a free surface problem and I don't know which opening boundary condition setting is the best for my problem.

The baffled vessel only contains water. The aim of the simulation is to determine the mixing time, so I want to include a scalar tracer after simulating the steady state flow. Later I also want to include a particle tracking.

I'm very thankful for every hints.

cdegroot November 22, 2012 13:01

Hi. It sounds like an interesting problem. Have you gone through the relevant CFX tutorials? There are some covering free surface flows, scalar transport, and particle tracking. If you haven't given those a try, you should. If you have some specific problems, post them here.

blubb1612 November 22, 2012 14:33

Thank you for your reply.

I already have done some tutorials concerning this problem...
My problem is that I don't reach convergence. I already read about this problem in relation with free surfaces.
I hope I can get a hint which mass and momentum options for the opening condition I should use to avoid this problem as much as possible. I think the air don't affect the fluid flow very much. On the other side I think it is not possible to model the liquid surface as wall because in this case the fluid flow in the vessel would definitly not be the real one.

cdegroot November 22, 2012 14:49

The easiest thing to converge will be if you use a homogeneous model (both water and air share the same velocity field). Start with this. At the top of the domain use an Opening boundary condition with a relative pressure of 0 Pa. Set the volume fraction of air to 1 and the volume fraction of water to 0.

brunoc November 22, 2012 14:50

Where is this opening boundary condition? Is it at the top of the vessel?

Also, you said you have a free surface problem but your vessel has water only. Do you intend to calculate the free surface position from the pressure level at the top? This might be valid only if the swirl in the fluid isn't too strong, otherwise the free surface height might be important and this simplification might deliver incorrect results. If swirl is not strong, them this can be a good first analysis simplification, but in this case it would be better to use a free-slip wall at the top boundary condition. After you get your results, you can estimate the actual free surface height from the pressure levels.

This simplification is only a good idea if you plan on doing this type of simulation several times and want to cut your total time, in which case I recommend you also do at least one simulation with an actual free surface to check how good your results are and tune your model. If you're only doing one simulation, than just use an actual free surface with the homogeneous model and the free surface algorithm turned on. The computational cost won't be that much higher and your results will be better.

Cheers

brunoc November 22, 2012 15:00

Quote:

Originally Posted by cdegroot (Post 393705)
The easiest thing to converge will be if you use a homogeneous model (both water and air share the same velocity field). Start with this. At the top of the domain use an Opening boundary condition with a relative pressure of 0 Pa. Set the volume fraction of air to 1 and the volume fraction of water to 0.

Hey Chris, looks like you pressed the 'Submit' button before I did :)

But I agree that an actual free surface simulation with the homogeneous model is the best option.

cdegroot November 22, 2012 15:02

Yes definitely do a real free surface simulation! There really shouldn't be any great difficulties getting this to converge.

ghorrocks November 22, 2012 16:04

Surface waves can often make steady state free surface simulations hard to converge. This simulation does not have inlets or outlets (which are a frequent source of small numerical noise which then become surface waves which cause convergence problems) so that might help a bit.

But in my experience you often have to do free surface simulations in transient simulations and run them out to steady state, rather than doing a steady state simulation.

blubb1612 November 28, 2012 10:16

Hi,

thank you for your advices.
At the moment I have made a free surface simulation as you described and it works. I have reached convergence.

Now I want to include an additional variable to simulate mixing times.
Therefore I definied an expression for the injection of the tracer: Tracerinjection=0.1*step((t-0.1[sec])/1 [sec]) [kg s^-1]
Because I had no inlet in my vessel I have defined a source point where I include the tracer.

I run this simulation as transient and set 'solve fluids', 'solve ernergy' and 'solve tubulence' to false. I use the result file from the steady state simulation as initial value. Is that right?
I have defined some monitor points. For this points I get a pulse response curve which I should analyse to get the mixing time. But the results are not these I predicted. There is a first peak and some smaller ones after that but it doesn't reaches a constant value at the end.

Are there any advices concering this problem with the additional tracer.


All times are GMT -4. The time now is 02:26.