[A_Prakash]

Hello there,

I would very much appreciate your advice in helping me set-up the following problem to get meaningful results:

Tank description (see attached figure):
> 35m L x 25 W x 7m High tank
> Water level at 3.5 m
> Constant steady flow from top (inlet BC) at roughly 100kg/s
> Outlet at bottom (100 kg/s)

Question:
Do I really need to have two different domains (air and water) in CFX in order to set-up a two phase problem?
I am using this approach. Specifying volume fractions of air and water. I am able to get the free-surface. However, there is something amiss..as solution starts to diverge. As in, water keeps circulating locally at inlet....there's hardly any action at outlet.


Could any of you here share your idea of best practice in such problem. My final objective is to estimate the extent of re-circulation for various baffle configs. I wish to refine my approach to be able to estimate average residence time, if possible.

[ghorrocks]

I assume you want the simulation to model the water surface level as it changes enough to be significant. In this case this is a single domain simulation, but with two phases. The free surface model will do it. You will also probably need to model this transient, even if you are looking for the final steady state condition.

Have you done the free surface over a bump tutorial? That shows the basics of how to set up these sort of simulations.

You should be able to get recirculations and residence times when this model is running correctly.

[A_Prakash]

Thanks Glenn. I will follow your tips. Yes, I will start from scratch by going over the tutorial. I will keep the forum posted!
Cheers and happy new year!

[A_Prakash]

Ok. I followed the philosophy outlined in the tutorial. The main difference between the tutorial and my problem is the closed tank.
With regard to setting up the approximate volume fraction, I specified the water height approximately half of the tank volume. Thereafter, I put in the appropriate expressions to specify the volume fractions as a function height (z coordinate).

For initial steady-state run, this is how I adapt the tutorial for my model:
1) Because the tutorial has an entertainment/opening BC; I knew that I couldn't go with downstream pressure (DownPres expression) for my problem-which is enclosed tank with specified flow in and mechanically extracted flow out. Therefore, I specified inlet with normal speed (0.1 m/s), VOFair=0 and VOFwater=1.
2) At outlet I put the same flow out (0.1 m/s).
3) Domain initialization for velocity and pressure = AUTOMATIC (unlike the case in tutorial)
4) VOF values were specified (same way as in tutorial)
5) UpH specified as per my water level. DownH= UpH-0.3m (just a rough guess)
*As far as mesh refinement goes, I had manually refined it at halfway mark..therefore, I did not activate it in the model...to keep it simple for now.

Here is my problem now:
My tanks seems to be progressively emptying. Water level keeps coming down. My objective is to model the steady-state water-in and water-out process. Examining the VOF contours, I can see that I have the initial water
and air VOF correct. Looking closely at the inlet, I see that there is no continous water stream through inlet. See pic. I suspect pressure BC isn't right.
Many thanks for your advise.

[ghorrocks]

As I said in my previous post, you are probably (almost certainly actually) going to need to run this transient. It will not work steady state due to gravity waves on the free surface.

1) OK
2) OK, but where do you set the pressure level? The pressure needs to be set somewhere.

There will always be an imbalance in inlet and outlet flow. This is another reason why you cannot run this steady state. At least in a transient simulation the level should only change slowly. Consider a pressure outlet where the pressure is the static head of the depth you want to maintain.

[A_Prakash]

Thanks you very much for your input. Yes, I better go the static pressure head option.
Also, I have to run it in transient mode.

From my previous experience with running the problem (before I posted here)..I found that time interval size has to be chosen carefully. For example, simu time of 60 sec with delta.t of 1s returned more meaningful result compared to running the model for 10 minutes with delta.t of 4s.
From tutorials they mention residence time(Rt). R(t)=Characteristic length/Velocity (makes more sense for uni-directional flow). For tanks with flow bends it better to use R(t)=WaterVolume/flowrate. Could you share some insights into how best to choose the time?

[ghorrocks]

Forget about residence time. That is not applicable for transient simulations. For a transient simulation you need to do a time step size sensitivity analysis to determine time step size. But for free surface simulations it is a really good idea to use adaptive time stepping to automatically find the time step - use 3-5 coeff loops per iteration with a max and min time step size wide enough that you never reach them.

[A_Prakash]

Sounds good! Will try it out. Thanks

[A_Prakash]

Nopes! Does not want to work I have attached the out file. There is 100% backflow at outlet (referenced as "OPEN" in attached ccl).

[ghorrocks]

The whole idea of the pressure outlet is that it can backflow if it needs to when the water level is low. So of course it is going to have backflow. So make it an opening to allow this.

Also - I suspect you are not setting the pressure on the outlet/opening correctly. Have a close look at it and make sure it is correct.

[A_Prakash]

Found one major mistake . I did not turn on the Homogeneous free surface tracking option. Redoing the analysis again now.

[A_Prakash]

Absolutely appreciate your advise, Glenn.
After chasing this for a couple of hours, I have managed to get my transient simulation going with adaptive time steps. Fixed some of the errors in my input. I am quite happy with the initial results of the run...Hope when I come back later... I don't have any surprises *fingers crossed*