[GerhardHolzinger]

I have a bubble column which simulates just fine with twoPhaseEulerFoam-2.3.0. However, twoPhaseEulerFoam-2.3.x breaks the case.

I attached some images to illustrate my problem.

With OF-2.3.0 all turns out just fine. The screenshots of this case are at t=3s.

With OF-2.3.x, however, the simulation crashes at some point after t=0.2s.

I attached also the case for you to play around.


So, to repeat my problem or question:

How can I get my case running in twoPhaseEulerFoam-2.3.x with the fully conservative formulation (i.e. fvm::ddt(alpha1, rho1, U1) instead of fvm::ddt(alpha1, U1))?

[cutter]

Hi,

I'm currently investigating twoPhaseEulerFoam too. I have no idea what the reason for the crash is, but I can confirm that it's also crashing after 0.1301399s with my version of OF 2.3.x.

Just an idea: You could use 'git bisect' to find the patch that is causing the problem. This will take some time (depending on the number of git commits and your compile times), but it might help you finding the problem or maybe filing a bug report.

BTW: nice talk at the conference!

Cutter


http://git-scm.com/book/en/v2/Git-To...gging-with-Git

[alberto]

The new formulation couples the system of equations in a much tighter way. You must ensure that the whole system converges well.
The modification was introduced to ensure the conservation of the disperse phase, and to guarantee energy conservation when there are large gradients of the dispersed phase fraction.

In short, use multiple (20 - 40) outer correctors, and a sufficiently strict Courant condition.

[GerhardHolzinger]

Thanks for your reply and your note at my bug report (http://www.openfoam.org/mantisbt/view.php?id=1441#c3281).

Sorry, for being a whining baby, but is this the only way to get the cases to run?

Making the time step small by prescribing a small Co number and performing tens of outer iteration causes the case to take ages.

I know generalisation is a good thing, but I don't want my isothermal, incompressible cases to take x times as long just because I use a newer version of OpenFOAM.

Although I like the features introduced in OF-2.3.x such as the fvOptions mechanism in twoPhaseEulerFoam, I highly dislike the pain it causes me to get any case running.

[GerhardHolzinger]

I still don't manage to get the case running.

I use maxCo = 0.2 and the following residualControls.

To get to 0.1s simulated time, I had to wait for 2h and the result is still the same unphysical mess.

Does anybody get this bubble column to work?

PIMPLE
{
    nOuterCorrectors 40;
    nCorrectors      3;
    nNonOrthogonalCorrectors 0;
    
    residualControl
    {
        "(U|k|epsilon)"
        {
            relTol          0.0001;
            tolerance       0.0001;
        }
    }

    turbOnFinalIterOnly off;

}

[alberto]

I'm giving it a try now :-)

[alberto]

One question: is the inlet made by a central square and a small square in a corner?

That is what topoSet + createPatch seems to generate here.

[alberto]

Ok. Not sure how that happened. But I answered my question... just a square in the center.

[alberto]

Originally Posted by GerhardHolzinger

Although I like the features introduced in OF-2.3.x such as the fvOptions mechanism in twoPhaseEulerFoam, I highly dislike the pain it causes me to get any case running.

2.3.x is a development version. I would stick to 2.3.0 for production, if you don't need the features in 2.3.x.

Also, your case has some inconsistency which are independent from the problem you are encountering: you fill the column with water, water cannot go out (slip condition), but you add mass to the system. Also, Uwater at the inlet should be zero, being alpha.water zero.

[alberto]

I investigated a bit more, and run your simulation with Schiller-Naumann drag, obtaining reasonable results. Could you check that? Maybe it is a problem in the implementation of the drag law.

[GerhardHolzinger]

Thank you for having a look on my problem. I apologize for posting a messy case, that's clearly my homework to do.

This bubble column is based on the thesis and other publications of N. Deen, e.g. [1,2]


The problem with the water not being able to leave the domain is a tricky one. How could I model the upper boundary without including the free surface into my simulation domain?
Including the free surface introduces additional problems, e.g. phase-inversion.


I cleaned up and attached the case.

[1] N. G. Deen, T. Solberg, and B. H. Hjertager. Large eddy simulation of the gas-liquid flow in
a square cross-sectioned bubble column. Chemical Engineering Science, 56:6341–6349, 2001.

[2] Niels G. Deen. An experimental and computational study of fluid dynamics in gas-liquid
chemical reactors. PhD thesis, Aalborg University Esbjerg, 2001.

[alberto]

Thanks for the updated case. I will look into it.

Originally Posted by GerhardHolzinger

The problem with the water not being able to leave the domain is a tricky one. How could I model the upper boundary without including the free surface into my simulation domain?
Including the free surface introduces additional problems, e.g. phase-inversion.

The problem of phase inversion is well addressed in twoPhaseEulerFoam, so I would not worry about it. For stability, it is probably a good idea to actually include the free surface (it won't be resolved in detail, so it won't add computational cost) because it allows recirculation of water at the boundary to be avoided. Additionally, it lets you specify an easier boundary condition (constant pressure).

In any case, I will come back with additional comments once I look at the updated case :-)

[alberto]

I have come to the conclusion that the major culprit is the TomiyamaAnalytic drag. I ran the case with both Schiller-Naumann and Tomiyama-Kataoka-Zun-Sakaguchi drag law (I implemented it), and I don't see the very strange velocity profile that comes out with the TomiyamaAnalytic implementation.

Is the grid you are using here the same you had when you ran with 2.3.0 and obtained good results, or did you coarsen it? I don't see a lot of fluctuations in the bubble plume with the Schiller-Naumann drag. The case with Tomiyama-Kataoka-Zun-Sakaguchi is still running, so I will know soon.

[GerhardHolzinger]

Hi,

it is the same the mesh. I should definitely try other drag laws.

I will look into this issue.

Thanks for taking so many looks on my stuff.

It was definitely good to have a different pair of eyes on a problem I am stuck with.

[alberto]

Originally Posted by GerhardHolzinger

Hi,

it is the same the mesh. I should definitely try other drag laws.

I will look into this issue.

Thanks for taking so many looks on my stuff.

It was definitely good to have a different pair of eyes on a problem I am stuck with.

Any improvements?

[zandi]

Originally Posted by alberto

I have come to the conclusion that the major culprit is the TomiyamaAnalytic drag. I ran the case with both Schiller-Naumann and Tomiyama-Kataoka-Zun-Sakaguchi drag law (I implemented it), and I don't see the very strange velocity profile that comes out with the TomiyamaAnalytic implementation.

Is the grid you are using here the same you had when you ran with 2.3.0 and obtained good results, or did you coarsen it? I don't see a lot of fluctuations in the bubble plume with the Schiller-Naumann drag. The case with Tomiyama-Kataoka-Zun-Sakaguchi is still running, so I will know soon.

Dear Dr. Passalacqua
Is fluctuations in plume of bubble in this solver due to drag model? Schiller-Naumann can do fix it? in water and air mixing flow.

Really Thank you
Fatema

[smhosseini]

Hi everybody,

I want to simulate a bubble column. In this case, the gas phase is absorbed by the liquid phase and there is a reaction in the liquid phase. I'm going to use OpenFOAM. I want to combine twoPhaseEulerFoam and reactingFoam.

Could you tell me your idea about this case? Do you have any suggestion for me?

what is the term of + fvOptions(rho, Yi) in the YEqn.H of reactingFoam?

Looking forward to your answers.
Thanks in advance.

[zandi]

Originally Posted by zandi

Dear Dr. Passalacqua
Is fluctuations in plume of bubble in this solver due to drag model? Schiller-Naumann can do fix it? in water and air mixing flow.

Really Thank you
Fatema

O

I fixed it!! it is because of deltaT and maxCo
delta and courant number

[surya.tdr]

can any one help to simulate my bubble column which is having co-current flow of air and water. Is it possible to provide boundary conditions for inlet air and water or is it necessary to define a stagnant liquid column?

[zandi]

Originally Posted by surya.tdr

can any one help to simulate my bubble column which is having co-current flow of air and water. Is it possible to provide boundary conditions for inlet air and water or is it necessary to define a stagnant liquid column?

Hi
yes it is. I don't know alot about "co-current flow of air and water" but you can with different U files for water and air .