Hi CFX users !

I have encountered an interesting problem with mass conservation in the multi fluid model in CFX 4.2.

Setup:

A box with 50 % water and 50 % air. The gravity separates the air and water. At the top of the box, there is a pressure boundary, where air can leave or enter. In the fully separated situation I start to blow air into a hole in the bottom of box (where the water is), in order to generate a column of bobles. The command file (*.fc) of the model is practical identical to example 23 (droplet sedimentation)

Problem:

Transient solution: Although the flowpattern seems resonable, the waterlevel slowly drops. The total volume of water decreases and is replaced with air. There is, however, no place where the water can leave the domain. At the pressure boundary, the volume fraction of water is 1E-10 (In CFX terms = zero). The massflow of water through this boundary (described in the output file) is practically zero.

Steady-State solution: No physical solution is reached. All the water leaves the domain (without a trace ? ).

Now, I have checked the dependency on the number of itterations, and as the steady state solution indicates, this cannot be solved by increasing the number of itteration.

Is this a problem when there is both a conservation equation for the mass in each phase and for the sum of volume in the two phases ? (Sum r_i = 1) ? I know that the sum of volumefractions ALLWAYS has to be 1.

Does anybody have a suggestion for the origin of my problem and a possible solution ?

Regards Michael

Hi,

I just came across your message. Quite interesting! I have done a lot of free-surface type simulations with CFX, and mass conservation was OK. Question: if you are using the homogeneous two-phase flows option in CFX to simulate your problem (i.e. segregated immiscible phases), did you use the surface sharpening algorithm? If not, your loss of mass could be explained by the smearing out of the interface due to the numerical diffusion across the interface? Let me know. I would be interested in getting your .fc files to have a try.

Cheers,

Thibauld

Hi Thibauld

Thank you for replying on my message.

The reason why we have investigated this is because we are implementing a microbiological process model for waste water treatment into a three phase CFX model. Individual mass balance for each phase is paramount in order to get the model to work. The two-phase simulation of air in water is only a test case for the final model. But if we can't get this to work, a three phase version is far out in the future.

I have no reason to doubt that CFX is able to achive mass conservation (I think thats the first thing they check for). What I meant with a "mass conservation error" is simply: When I sum over all the blocks, the average fraction of water should be the same as in the beginning of the simulation, as the water is not be able to leave the tank.

If the problem is simulated without air blowing in through the hole - mass conservation is perfect. The average water volume fraction is 0.50000. However, not all the time. As the simulation progresses, the average volume fraction can vary serveral procent to each side of 0.5, but at the equilibrium it is perfect. This suggest to me that the overall mass balance across the boundaries allways is preserved, while the distribution between the different volume fractions present can vary. I have no information about the inner workings of the model on this specific point - so this is just a guess. The "return of mass" also raises concerns. When the average volume returns for - say 0.49 to 0.5 - has the scalars within each phase also changed accordingly ?

What we have observed could just as well be our inability to setup the model correct. However, we have been working on this for the last 4 months and have tried a lot of different setup options. The nice people at the support desk at CFX is presently trying to figure out what can be wrong in our setup.

We are using the multi-fluid model and not the homogenous model. We have also wondered if the the mass loss is due to diffusion across the pressure boundary. We have performed simulations which indicates a gradient of water in the air. This could suggest a ordinary numerical problem. However, as stated above, when no air is blown into the tank - a steady-state mass balance is present. Using the honogenous model in a problem with a boble column in water is a problem. The algoithm will move water around in an unphyiscical way within the boble column itself, and we have had problems in achiving a steady-state solution.

In any case I think that the model should be able a calculate a simple problem as bobles in water, without significant changes in water volume. If numerical dispersion is responsible for the problems, it should be possible to correct this. But maybe the logic of the multi-fluid formulation makes this difficult, because the two phases dominates distinct different areas of the domain ? The volume fraction of water in the air (above the surface) is very low - but still the NS equations are still solved.

I will E-mail you my files as soon as I return to work , so you can have a go at them.

I will post the solution here as soon as I (or anybody else) figure one out.

Regards Michael

Hi CFX users

Well sometimes, I wish that I would wait just one more day before said my opinion about this case. But that's my nemesis !!!

I found the error - and it was (of course) in my own code. The mass conservation routine, we made for checking the phase error was developed in a system with constant grid size. In my test case, we have switched to a bodyfitted grid in order to have a good resolution around the air jet. However, the code did not take the variability of the grid into account when calculating the phase mass balance so when the air jet creates waves at the surface of the tank, mass is moved around in boxes of different sizes.

Thanks to Thibaud, CFX and anybody else who spent time thinking about this.

Regards

Michael