[su_junwei]

Hi raagh77

It seems that your simulation diverged, please try using a lower time step ?

regards, Junwei

[alberto]

Hi,

unfortunately issues when there are sharp interfaces in two-fluid simulations are very common, and when the plume reaches the top of the fluid phase might indeed give problems.

I don't think you need to change the turbulence parameters, if they work OK for a part of the simulation, just check that they are appropriate for you case. I'd try to reduce the time stop of one or two order of magnitudes to see what happens. You might want to reduce the tolerance on the pressure too.

Regards

[raagh77]

Hi..Alberto and Junwei

Just an hour back...finally

With the low relaxation parameters and piso correctors in fvSolution changed to 8 (from previous value 2 as suggested from my supervisor) the simulation was quite stable..

but I can say the simulation is successful only if the results are comparable with the experimental data..

before changing piso correctors I made following changes
. low time step (1e-4 !! )
. ddT schemes to backward from Euler
. applied pressure at the top of the outlet so that nutb doesn't create problem at the interface (as suggested by my supervisor)

and the same old result...simulation crashed.

Right now with piso correctors being increased simulation is quite stable and am waiting for the end results for compariying with the experiments..

Regards
Raghavendra

[alberto]

The solution you obtain with underrelaxation will be delayed in time, so don't expect time accurate predictions. As I told you before, you should not use under-relaxation in this solver because there is no mechanism to ensure that the solution will evolve up to the right point (no subiterations) in each time step.

Regards

[raagh77]

Hello Alberto,

yeah..I kept in mind before editing those relaxation parameters.
but there was no other go...I was totally exhausted.

Probably after a days break from OpenFOAM .. I though to make some changes in the turbulence model rather use K-omegaSST model as it is quite useful for low Re number flows..

Also mean time I would concentrate on other subjects of my course which I totally forgot..

Regards
Raghavendra..

[alberto]

Hehe, OK. But this might influence the comparison with the experimental data.

About the future developments, actually more than thinking to a SST-omega model, you might want to look into turbulence models developed for multiphase flows, or use an algebraic closure, which is worth to try, considering it doesn't require any effort to be implemented, being explicit, and it has been successfully used in other applications.

Best regards

[raagh77]

Hello Alberto,

Finally, my simulation is quite stable and I checked the intermediate results in paraFoam and seeems to be quite good..(though I haven't compared with Becker et al experiments yet)..

Thanks for the support

Now I am planning to compare with various turbulence model (as done in Dyanamic simulation of a 2D bubble column by Knut Bech). To begin with I am starting with k-omegaSST turbulence model (and also with other algerbric models which you suggested).

As I am very much new to openFOAM I couldn't implement k-omegaSST model direclty in twoPhaseEulerFoam solver as it is mainly focused on k-epsilon model (?). I tried to make some changes in twoPhaseEulerFoam.C file but it was not successful..(In some tutorial files I found other turbulence model coefficients being directly implemented in constant/RASproperties but in twoPhaseEulerFoam solver there is only k-epsilon)

Can you please tell me (in brief) what are the changes to made before compiling the solver ? (before wmake)..

Regards
Raghavendra

[alberto]

Hi,

twoPhaseEulerFoam implements the turbulence mixture model of Gosman (see H. Rusche thesis).The implementation is done completely in the code, where you can find also the implementation of the wall functions.

To implement a new model:

- Remove the current model equations, or add a switch to decide which turbulence model you want to use. Equations are in twoPhaseEulerFoam/turbulenceModel/kEpsilon.H. In the same directory you find the headers where wall functions are implemented.

- Assuming all turbulence models you want to try rely on the hypothesis of turbulence viscosity, you do not have to deeply change the structure of the solver. Simply change the parts where the turbulent and effective viscosities are computed.
For explicit closures, this is all what you need to do.

- For models involving transport equations, you should code them, following the example of the k-eps equations already in the code.

As a side note, to compile twoPhaseEulerFoam, you need to run ./Allwmake because there are additional classes to be compiled.

Best,
Alberto

[raagh77]

Hi Alberto,

I dont know how appropriate is to discuss this issue in this thread as it is related to post processing in paraFoam.

Now, the simulation is almost done (just around 100 seconds remaining) and to compare with Becker et al experiment, I have to start with velocity vs time plot at three different positions of x and y.

I was able to plot velocity vs position (x or y coordinate) with fixed time, T but I am looking for velocity vs time T plot in paraFoam (for fixed values of x and y co-ordinates).

I used plot selection over time in the filter menu but without any success..

Am looking forward for your suggestion on this..

and am sorry if this thread is not appropriate to discuss paraFoam and post processing results ..

Regards
Raghavendra

[alberto]

Hi,

let's say the procedure is not one of the simplest on the planet

• The first step is selecting the point in paraFoam, so after loading your case, do the following:
  • Show your case as usual, by clicking on "Apply" in the "Properties" tab.
  • Select the field you want to plot, for example the pressure "p", in the "Display" tab.
  • Now, go to the "View" menu, and choose "Selection inspector".
  • Click on "Create Selection".
  • In "Selection type", choose "Locations".
  • In "Field type", choose "POINT".
  • In the "Locations" table that appears, insert the coordinates of the point where you want to measure your data.
  • Now the selection is created.
• The next step is to plotting the selection:
  • Go to the "Filters -> Data Analysis -> Plot selection over time" menu.
  • On the left on the screen, you will see a button "Copy Active Selection", push it.
  • Click on "Apply" above that button.
  • You should now see your data plotted against time.

I hope this helps.

Regards,

[raagh77]

Hi Alberto,

I followed the steps you suggested in the previous but in the output window it says input and output array data types do not match.

I tried to plot lateral velocity (Uay) at the point (0.005, 0.25) close to the wall vs time.

One more thing which I noticed...

I plotted Uay along a horizontal line (from x,y = 0, 0.25 to 0.2, 0.25) to compare the velocity profile with the experimental data. In the experiments close to the wall shows the negative value (as it should be) but in my simulation results, close to the walls velocity is not negative !..
Is this due to the turbulence model what I am using (because of K-epsilon model) or may be something wrong!! .

Also in ppProperties g=0 thus I am neglecting particle particle interaction ..

Regards
Raghavendra

[raagh77]

Hi again,

Sorry, I think I fixed the other issue I was plotting particle velocity rather than plotting continuous phase velocity..

But the particle velocity Uay vs Time T is not fixed..which am working on that currently..
(Hope my posts are not flooding to your mail INBOX

Regards
Raghavendra

[alberto]

Originally Posted by raagh77

Hi Alberto,
I plotted Uay along a horizontal line (from x,y = 0, 0.25 to 0.2, 0.25) to compare the velocity profile with the experimental data. In the experiments close to the wall shows the negative value (as it should be) but in my simulation results, close to the walls velocity is not negative !

It might be to different factors. I'd suggest a search in the literature to see what settings do they use for similar simulations. Drag, lift coefficients, grid resolution and so on play a role in that.

Also in ppProperties g=0 thus I am neglecting particle particle interaction ..

That's not the problem. ppMagF has to be used only with gas-particle simulations.

Regards,

[raagh77]

Hi Alberto

Am back to this thread !

I just finished the 2D simulation of bubble column, becker case (with turbulence being on)

I would like to discuss the results here

.> The velocity variations at three positions after time averaging was quite compariable
.> K-epsilon model predicted higher turbulent viscosity (nutb)
.> Timeperiod of the lateral bubble movement around 70seconds which was far more greater than what specified in the paper (paper says 16 to 20seconds)

This increase in timeperiod is either because of high prediction of nutb by k-epsilon or due to the relaxation parameters used for twoPhaseEulerFoam solver (because I remember you saying with "realaxtion parameters its difficult to obtain time accruate predictions") ??

Regards
Raghavendra

[alberto]

Hi Raghavendr,

if you under-relax in twoPhaseEulerFoam without taking care of actually letting the solution evolve completely in the time step (= changing the code), you introduce a systematic time delay in the solution itself. That's what I meant.

I hope this helps.

Best,

[raagh77]

Hi Alberto

After this Water-air (Becker case) two phase flows

Now, I am tring to Simulate Steel-Argon flows as part of my master thesis work
(steel continuous phase and argon discrete phase) with free surface and the simulation is not stable.

I have limited the courant number to 0.85, after few iterations very small time steps will be used (of the order 1e-06) and simulation crashes with high courant number.

when I change the density of the continous phase from 1000 (from water) to 7000 (Steel density) simulation crashes.

Do I need to change the coefficients of Cvm, Cl and Ct in constant/transportProperties ?

awaiting for your suggestions

(I also posted this in a seperate thread earlier!)

Regards
Raghavendra

[Rachel]

HI Raghavendra,

I read somewhere in the forums: that Co = 0.2 is recommended. Many solvers use CO_max =0.1
You might consider running a case by limiting to 0.2 and see if it runs... I realize it will consure 4 times more time, but even I had a lot of problems with timestepping in OpenFOAM.

BR,

[raagh77]

Hi Rachel,
thanks for your reply.

currently I am limiting Co to 0.85 and the corresponding deltaT is 3.6e-07 seconds. When I decrease the upper limit to 0.2 then deltaT will be reduced further

but the problem is something in the pressure equation. It takes more iterations (around 250 to 300 and this keeps on increasing upto 1000) then the simulation crashes with high Co (of the order e10 !! ).

One thing which I just noticed is that
when I increase the discrete phase density to 100 simulation is quite stable (for initial few time iterations at least)

Regards
Raghavendra

[Rachel]

HI Raghavendra,

Did you play around with different Pressure schemes/solvers? Did it help?
What is the relTol and Epsilon are you solving ?

If its not an issue, can you email the case to have a look into the problem?

[alberto]

Hi,

the problem is that the density ratio becomes very big (7000 if the other phase is air) in your case, and this is a known reason of instability in the solution algorithm. When you increase the discrete phase density to 100, you actually bring that ration down to 70, which is a lot lower than the ratio you had in the air/water bubble column (1000).

To be honest I don't know an easy solution to the problem: you would need a more robust algorithm, but it is not trivial to implement, and, in my experience, OF adds some interesting complication to the problem when it comes to solving for the multiphase equations.

However, what kind of system are you trying to compute? Steel casting?

Best,
A.