Hi Muhammad,

People would need to know what kind of physics you are simulating before giving relevant suggestions in convergence improvement.

From your description it seems you are in serious trouble, so maybe you should consider strong simplifications like using a smaller domain size or try to take advantage of some flow symmetry to reduce your computational domain. The usage of 2D models or coarse meshes with wall functions may be very helpful in getting first approximations.

Regards,

Daniel

Hi Muhammad,

People would need to know what kind of physics you are simulating before giving relevant suggestions in convergence improvement.

From your description it seems you are in serious trouble, so maybe you should consider strong simplifications like using a smaller domain size or try to take advantage of some flow symmetry to reduce your computational domain. The usage of 2D models or coarse meshes with wall functions may be very helpful in getting first approximations.

Regards,

Daniel

Dear Daniel Fonseca de Carvalho e Silva,

Thank you for your suggestions. Can you please explain "coarse meshes with wall functions may be very helpful" ? I think coarse mesh reduce total Cell, Faces and Node size that leads to more divergence... Isn't it ??

About Physics I am applying Two phase flow Eulerian-Eulerian , PBM, Turbulence Models.

Regards

Dr. Malik M Barakathullah,

you are correct sir !! 10Million time steps !!! actually I used time step size is 1e-5 and for unsteady case 100second simulation needs 1e+7 time steps. I am trying to increase time step size to 1e-4 or 1e-3 that would definitely reduce the total number of time step to 100,000. ( when I use conventional air/water system I can run my simulation with step size is 0.01, completing within 1 day)

Today, I set convergence criteria for continuity is 0.01 ( it means solution will converge when residual drop to 10-3 magnitude. Then I notice almost every time step is converging at 15-16 iteration & completing in Average 5 Sec.

In my latest case , currently I am unable to use step size 0.001 or 0.0001.....It creates divergence every time. My problem would be solved if I use 1e-3 step size without divergence. So, I need you expert opinion about Mesh Quality, non-orthogonality, Remesh or refine cells which have large aspect ratio or large skewness.

I hope my problem will be solved if my mesh quality will be batter !! What is your suggestion sir !!

Regards

Hi Muhammad,

Coarse meshes do not necessarily increase your chance of getting divergence. The way you described, even solving your divergence problem, it doesn't seem you would get your solution in reasonable time duration, therefore I suggest a more "economical" numerical model.

With an appropriate verification of the CFL condition, you may be able to increase your time step by using appropriate under-relaxation factors, as it was mentioned by Malik.

If the problem is occurring in the simulation first steps, you may use a ramp to gradually increase the values in the boundary conditions. This procedure usually helps with stability issues.

Hope it helps,

Daniel

Hi Muhammad,

I don't have a lot of experience with multiphase flow in FLUENT (not good experience anyway, haha), but I did want to throw some questions/comments for you to consider.

1) Are you certain that mesh quality is the problem? Since you haven't mentioned what you are studying (aside from it being a two-phase problem), I was wondering if it is something in the physics of the fluids you are using, or something connected to your mesh size. The table you posted shows only 36,000 cells (and 4 partitions - you aren't utilizing 20 cores, it seems). Is your grid fine enough that you can resolve the features and physics that you're interested in? It could be that FLUENT is having issues calculating something because the cell size is very big. When I was even doing 2D VOF model of a jet, we needed many more cells to capture the behaviour even approximately.

2) Can you initialize the flow field better?  Maybe start it as a single phase flow, then have your second phase flow through the inlet?

3) I wouldn't recommend reducing the convergence criterion - having a poor solution at one time step may make it difficult to converge the next one.

4) Did you try tweaking the under-relaxation factors? I would probably only do this once your simulation has gone a few time steps and you are confident that it won't diverge, but it will help you at least get the continuity equation to resolve faster.

I think people would be able to offer better help if they knew exactly what you were modelling. You have this idea in your head that the problem is mesh quality, but from what you posted, it seems just as likely it could be something else.

Regards,

Derrick

hmmm... I am not sure that mesh quality is the problem. one of the previous author told me, " the time step is related to the mesh size and I should rebuild the mesh if I am interested to use 1e-4 step size"

From your suggestions I am considering the URF now. Before I was using default URF. 

Problem Statement :

By using a vertical 3D bubble column with single INLET and single Pressure outlet, hydrodynamics of air/water is under study. Eulerian Eulerian Multiphase and Viscus turbulent k-e model is used. INLET air velocity is 0.06 m/s. at Inlet water is static. column is open to atmosphere. For Bubble distribution , Population balance model is used. Phase interaction is defined by Drag( UDF ) , Lift , added mass, wall lubrication, surface tension and turbulence interactions. 

From my observation, continuity residual have poor convergence. So, can you understand this simulation and suggest me where is the problem ? If Mesh is the problem then how to solve it ? If URF is the problem then Which factor should I change ( increase/decrease) first !!

looking forward to your suggestions please !!!

Regards.

The URF was Malik's idea, but I do agree with it and recently experienced a lot of practical benefit from tuning it. FLUENT suggests leaving URF at default values if you are using SIMPLE but going to 1.0 for PISO. I suspect this is because PISO has additional sub-iterations to better match the continuity to pressure... Anyway, just also a note that increasing URF early on may also mess up your simulation. You should leave it as default until your simulation has started properly, or maybe even decrease it if you think there is a lot of oscillation in FLUENT's calculation of your flow field. Focus on the relaxation factors that are relevant to the field you are trying to improve your residuals on.

The time step being related to the mesh size is what Daniel was saying. In some schemes you have stability limitations due to CFL number, basically a ratio of how far a fluid element moves compared to your mesh size. CFL is a great concern for explicit time-marching methods, but usually it is a pretty soft requirement for implicit methods.

Anyway, hopefully someone with bubble column experience can chime in here, because I don't have experience with it. Until then, you're going to have to meddle with the simulation. Some stuff you can think about:

1) When I was doing the 2D VOF model, I found that surface tension effects behaved very strangely. The tube I was injecting water (into air) ended up creating very large droplets instead of a jet. Our Weber number was maybe a factor of 2 higher than dripping flow criterion, but this may be too close for FLUENT to resolve.

2) Can you simplify the models/physics and reach a situation where the simulation does work? Aside from replacing your drag UDF, maybe FLUENT is having trouble resolving something around a sharp corner.

3) It sounded Are you modelling your column as having a free surface? To reduce the complexity, you might try modelling without the free surface (unless this is what you are actually studying).

4) I'm still surprised you can get by with 36,000 cells. It seems like an extraordinarily small amount. If you use FLUENT's adaption function to go up to 300,000 cells, does it converge any better?

I think you should make a parallel question about bubble columns and resolving the physics of it with FLUENT - that may attract some more useful comments that will spark some progress for you.

Hi Experts,

After learning from your key suggestions, I worked on every aspects. I tried/changed 90+ models to solve my problem. * To change the URF , I did not find solution, *I was applying real case so that this time 2D was not desirable. * I was using a rectangular type geometry so that mesh quality ( skewness, orthogonality, aspect ratio) was pretty under control, * UDF was not a problem because it is used by others too. The turning point was "Coarse meshes do not necessarily increase your chance of getting divergence." and "Can you initialize the flow field better?"

So, I found little mistake when Initialize ( Boundary conditions of PBM module ) and Solution Method/algorithm what ever I used. Some time Second order upwind or QUICK creates more under and overshoots that makes divergence. These schemes are not unconditionally stable. So I tried to change these steps and got my solution !! Now 1 second simulation is taking 9-10 hours which is in under control because I can maximize time step size when solution reach to stable position.  

However, From this hit and trail, I learned that more fine mesh may not solve your problem because It takes more small time steps size to converge along with computationally expensive. For, Grid In-dependency and to catch complete phenomena I have to use more that than 100000 mesh size.

Thank you every one who gave me expert opinion to solve this problem.

Regards