[raagh77]

@ Rachel,

As the simulation was not stable I tried using first order schemes for all variables and I changed the pressure tolerance to 1 e-04

Can I mail you the case setup files because I had some problems in attaching .rar files here in the forum

@ Alberto,

I am trying to simulate ladle-casting where Argon will be injected to the molten steel at the bottom.

As you said, the ratio of densities where too high I tried to increase the discrete phase density for stable simulation but I don't know how it will influence the flow physics..

Regards
Raghavendra

[alberto]

Hi,

increasing the tolerance on pressure is not going to help. It will make the code run a bit faster at the beginning, but you actually want to reduce that tolerance not to propagate errors.

About your application, I have to say I do not know much about the kind of system you are considering, however did you check if there are already works done using two-fluid models for that kind of application? My feeling is that it might not be the best approach. I saw casting simulations done mainly with VOF.

Best,
A.

[raagh77]

Hi Alberto,

I have few results done in CFX to validate my steel-argon case and it is based on two-fluid approach
also few literature where where steel argon simulation is performed based on two fluid modeling approach.

Finally my task is to compare results what I obtained in CFX and OF.

[alberto]

Hi,

could you point me to those references? I'm interested in taking a look at them. Is the melted steel newtonian?

Btw, I'm also interested in the comparison, so if you want and can stay in touch with me about that, I would be very grateful :-)

Best,
A.

[Rachel]

Good Morning Raghavendra,

I guess one problem with your case is that alpha is -ve and going more than 1.
Using a limiting scheme divScheme might solve the problem (it bounds variables between 0 and 1) which I suspect is that case with alpha.

I will try to find more about such schemes or if you find more pl update

[raagh77]

Hi Alberto,

Literatures what I am refering ..
1. Turbulent Flow of Liquid Steel and Argon Bubbles in Slide-Gate Tundish Nozzles: Part I. Model Development and Validation
by HUA BAI and BRIAN G. THOMAS

2. Mathematical simulation of fluid flow in gas-stirred liquid systems
by Lifeng Zhang Taniguchi Laboratory, Department of Metallurgy, Graduate School of Engineering, Tohoku University, Aoba-ku, Sendai 980-8579, Japan

Please check your mail, I have attached these to literatures

yes, I am eager to discuss the comparision results with you for steel-argon


Regards
Raghavendra

[raagh77]

Hi Rachel Vogl, Good morning

I used limiting scheme divScheme as you suggested but there was not much improvement (simulation still crashing for high density case and with free surface)

Also I increased nNonOrthogonalCorrectors to 8 as my mesh is not structured but still not much success


Regards
Raghavendra

[raagh77]

I am modelling steel as Newtonian fluid

[raagh77]

Hi Alberto and Rachel,

I tried injecting Steel-Argon with my earlier becker 3D case (rectangular bubblecolumn which I used to validate water-air case) and with some modification with pressure scheme the simulation was quite stable and also results seems to be quite good..

But with the same case setup (I mean with 0, constant and system) I tried with the cylindrical bubble column of unstructured grid (around 0.5 million cells) simulation is stable without turbulence being on.

When I switch on the turbulence simulation crashes after few iterations
this time because of the divergence in timestep continuity error.
the residual for timestep continuity error keeps on increasing as soon as I switch on turbulence and it explodes after few iterations.

Is that because of unstructured grid ? I tried increasing non-orthogonal correctors to 8 but the change what I noticed is the simulation crashes after performing few more iterations..
also I tried with non-orthogonal correctors 20 and the simulation runs for few more iterations and crashes again

and again the reason for instability is that timestep continuity error residual.

Regards
Raghavendra

[alberto]

Hi,

no, it's not the unstructured grid. If the grid is so bad to lead to instabilities you would notice it also in the laminar case.

We talked some time ago about stability problems with the turbulence model in twoPhaseEulerFoam. The problem is probably the same. Btw, are you using that turbulence model with the air-steel system?

P.S. What changes did you do to the pressure scheme, if you can share?

Best,

[raagh77]

Hi Alberto,

yes for the rectangular bubble column I used turbulence for steel-air also
but for the cylindrical case it is creating problem..

I changed the solver schemes for pressure

p PCG
{
preconditioner DIC;
tolerance 1e-10;
relTol 0;
};

and used first order (upwind) schemes for
k, epsilon and
limited alpha between 0 to 1 by Gauss limitedLinear01 1

these are the only changes I made and it worked fine for Steel-air in rectangular bubble column

..
Regards
Raghavendra

[alberto]

Hi,

thanks for your reply.

I have some doubt that with that difference in the fluid properties you can use the turbulence model based on the mixture. It sounds quite a strong assumption!

This said, if you suspect that the difference is actually given by the mesh, and not by the BC's or the numerics, you can still generate an hexhedral mesh for a cylinder. The typical configuration used in bubble columns is to split the section (circle) in a central square and four sides, and mesh them with hex cells. Axially you should not have any problem if the geometry is a simple cylinder without lateral inlets.

Best,

[raagh77]

Hello Alberto,

Yes you are right. I could have started with structured grids but I already had simulation running in CFX with this unstructured grids (of 0.5 Million cells) so I though to doing with the same mesh in OF also..

Now I have to try with structured grids..

Is it advisible to change pressure scheme from piso to simpleTransient in twoPhaseEulerFoam?

Regards
Raghavendra

[alberto]

Hi,

in my experience "multphase" and "non-hex grids" are not a good match. It takes a bit more time to generate a good hex grid, but with the same number of cells the result is typically a lot better, and the convergence too.

You can change the scheme from PISO to an unsteady SIMPLE, of course. This would allow you to under-relax inside each time step, and if you want to do something more refined, to check for residuals convergence and adapt the time step as a consequence. It has been on my to-do list for a long time (and it's not done yet, because I'm busy with other stuff) :-(

Best,

[alberto]

It is always interesting to see someone without anything better to do than spamming. User reported.

Update: Thanks for the cleanup to the CFD-Online people! :-)

Best,

[alberto]

Hi Raghavendra,

an additional hint: check the values of k, epsilon and the turbulent viscosity ratio (nutb/nub) where you have no liquid. I quickly took a look at those, and noticed the turbulent viscosity becomes large there.
It might be worth to limit the turbulent viscosity ratio (and as a consequence k) to some upper value.

Best,
Alberto

[raagh77]

Hi Alberto,

Thanks for your support

I will look into that..

Have a nice weekend



Regards
-
Raghavendra

[alberto]

You're welcome.

I actually coded the limiter in quite a rough manner, and I also added some submodels for gas-liquid flows (bubble pressure term, bubble induced turbulence, some drag correlation for contaminated water).

The turbulent viscosity limiter indeed plays an important role in my test case, which is Pfleger et al. bubble column. I represented it in 2D, with 45 cm of water in a 0.2m x 0.55m domain. If you look at the zone without liquid, the turbulent viscosity tends to become extremely high. Limiting the turbulent viscosity ratio to 10^5 there (value taken by FLUENT) stabilized the solution significantly.

Coding the limiter is very easy. Before correcting the effective viscosity in kEpsilon.H, simply add these lines:

scalar maxNutb = max(nutb).value();
Info << "Maximum turbulent viscosity of continuous phase = " << maxNutb << endl;

if (RASturbulence && (maxNutb/nub.value() > maxTurbulentViscosityRatio) && limitNuRatio)
{
   Info << "Warning: Limiting total viscosity ratio to " << 
           maxTurbulentViscosityRatio << endl;
   nutb.min(maxTurbulentViscosityRatio*nub);
   k = max(sqrt(nutb*epsilon/Cmu),dimensionedScalar("zero", k.dimensions(), 1.0e-8)) ;  
}

where

• "RASturbulence" is a switch called simply "turbulence" in twoPhaseEulerFoam
• maxTurbulentViscosityRation is a scalar I added to the RASproperties dictionary and I read in createFields.H
• limitNuRatio is a switch to turn the limiter on or off at will, which I added to the RASproperties dictionary

There is probably a better way to do this. It was just a few minutes thought

Best,

[raagh77]

Hi Alberto,

limiting nutb/nub seems to be interesting even I will try that in my Pfleger bubble column case for air-water.

Coming back to Steel-argon case yesterday I tried with structured mesh and simulation seems to be quite stable though it is really slow (for one second it took 4 hours with 70K cells..! I am limiting Co to 0.75 so the timestep is in the order of 0.1milliseconds)

I was really surprised unstructured grid (1.2Mcells) failing for a stable simulation. The same grid in CFX took less than 2 days to complete the simulation (200 seconds of simulation)

Anyways, going back to strucutred grid helped me a lot in my case.

I will try with limiting nutb/nub for 2D bubble column water-air case and
I will keep updating about this here

Regards
Raghavendra

[alberto]

Hi,

Originally Posted by raagh77

Hi Alberto,
limiting nutb/nub seems to be interesting even I will try that in my Pfleger bubble column case for air-water.

OK. It should keep in general, not only in the air-water system however. Where there is no continuous phase, the turbulence quantities are definetly too big.

Coming back to Steel-argon case yesterday I tried with structured mesh and simulation seems to be quite stable though it is really slow (for one second it took 4 hours with 70K cells..! I am limiting Co to 0.75 so the timestep is in the order of 0.1milliseconds)

A time step of 10^-4 is OK for this kind of simulations. The long time is probably due to the high number of iterations on the pressure equation. This seems to be significantly reduced using GAMG (but it might affect stability a bit).

Best,
Alberto