[voingiappone]

Howdy!

I have been simulating a bubble column with the bubbleFoam but with no success (no convergence at all) and then decided to give a try to the VOF method. I have found papers about that and it seems to be adequate for what I need.

I created a mesh with 3505 cells and 1851 points simulating a flat 0.2x0.05x0.5 (WxDxH meters) reactor with a 0.003m inlet for injecting air at the bottom. The column is 3/5 filled with water (throug setFields run on alpha1 parameter). A very simple layout. I uploaded the case here so you can take a look at it.

Running the simulation this time is a breeze.... it takes centuries because the mesh is small and fine expecially around the inlet but it actually computes the bubbles coming out.

The problem:
when the bubble formed detaches from the inlet it travels few millimeters and "vanishes". Take a look to the attached pic to see what I mean. There you can see the alpha1 view of 3 bubbles: one forming on the bottom (blue core), one detached(green core) and one that has vanished (green mist).

My question this time is: why do the bubbles vanish instead of rising like an actual bubble towards the surface?

The only thing I could think about was that the mesh is still too coarse and, if the bubble splits in smaller ones, the actually calculated small bubbles cannot be described with the mesh cells (too big). As a result, the aplha becomes smaller and smaller ---> the green mist....

Can somebody help me with this? Meanwhile I'll try a mesh with 4 time more cells....

Thank you very much.

Luca

[akidess]

Try refining your mesh, and also try higher values of the interface compression coefficient cAlpha.

[voingiappone]

akidess, thank you for your prompt reply.
I am right now running the case with a decreased mesh cell size (now I have 24686 cells).

As soon as I will obtain some results, I'll try to change the compression coefficient. It is defaulted at 1 if I'm right; how much do you think it is safe to rise it without obtaining unphysical results and/or unrealistic time steps (if it impacts of course)? I'm currently "running" at 5.5e-5 s for having the C<0.5 condition respected.

[kathrin_kissling]

Hi Luca,

try interDyMFoam. There is a tutorial out there...
You can use cAlpha coefficients up to 4. But be careful this will influence the physical behaviour! You have to compare your results with experimental/analytical values for the rising velocity!

Always be aware: Your running DNS simulations. Therefore Co<0.5 is too high. I would go with 0.1, where I got decent results.


Best

Kathrin

[santiagomarquezd]

Hi Kathrin, I'm curious, What is the foundation of c_alpha<4? Do you have any theoretical or numerical explanation of that? I was analyzing alpha equation for a long while and it would be value to have more references or explanations.

Regards

[voingiappone]

Kathrin,

thank you for the answer. I fiddled with the cAlpha and indeed the situation got better, even at cAlpha=2 and even if the problem is "lifted" towards the surface.... where again the boundary gets lost. However, I relized that my mesh is indeed too "rude" for obtaining good results. I have to combine the two solutions. The reason why I can say this is that the bubbles are more or less well resolved where the cells are smaller... no surprise.

As santiagomarquezd pointed out (thanks a lot), it would be very nice to have a reference about the alpha upper limit value, just for having it handy when it comes to pointing out the parameter selection criteria.

[kathrin_kissling]

Hey guys,

have you tried to search through Henrik Rusche PHD Thesis. The link is out there in the forum. Moreover these values have been posted a lot of times before and there is always reference to a technical report of OpenCFD of which I dont have the exact reference handy right now.


Luca. I'm not sure whether simulating a bubble column with interFoam will work out. InterFoam is a DNS solver so you need to make sure everything is resolved resonably in space and time, what will cost you tons of computational effort for a technical buble colum. Search the internet for "OpenFOAM" and "bubble colum". I'm positive that there is tons of stuff out there.
If you are aming to focus on some single bubbles you might still want to test interFoam against the popular testcases! Again I would like to point you interDyMFoam which will reduce your computational cost.

I hope this being of some help!
Kathrin

[akidess]

Originally Posted by kathrin_kissling

Hey guys,

have you tried to search through Henrik Rusche PHD Thesis. The link is out there in the forum. Moreover these values have been posted a lot of times before and there is always reference to a technical report of OpenCFD of which I dont have the exact reference handy right now.

Hallo Kathrin,

I believe Henrik only writes about the compression coefficient in section 4.2.1, and recommends a coefficient of 1.5 for his case, but I haven't seen a condition of cAlpha < 4 anywhere in the thesis. Moreover, I follow the forums very closely, and I'm fairly certain this is the first time someone mentioned an upper bound for cAlpha. Would you mind pointing out more exactly where you found this? I'm aware of the technical report of OpenCFD that you're referring to, but I don't know of anyone other than the core developers that have had access to it. Did you get to read it?

- Anton

[kathrin_kissling]

Hi guys,

I'm thinking it was somewhere on the forum. I think I found it before the forum took over the new design. I'm not sure whether the really really old posts survived as a whole...

But: The values need to be adapted to your problem, because they will change the behaviour dramatically! I saw droplets moving with double the velocity they should have had!

Best

Kathrin

Some reference on the forum though
http://www.cfd-online.com/Forums/ope...flows-vof.html

[Andrea_85]

Hi all,

If you are aming to focus on some single bubbles you might still want to test interFoam against the popular testcases! Again I would like to point you interDyMFoam which will reduce your computational cost.

from what I know interDyMFoam is interFoam+meshRefinement (normally close to the interface to have a sharp interface), so i cannot figure out how the computational cost can be reduced. Normally it can take quite much computational time to respect to interFoam, or am i wrong?

Best

andrea

[akidess]

Originally Posted by Andrea_85

Hi all,
from what I know interDyMFoam is interFoam+meshRefinement (normally close to the interface to have a sharp interface), so i cannot figure out how the computational cost can be reduced. Normally it can take quite much computational time to respect to interFoam, or am i wrong?

Best

andrea

It depends. If you have a big area to simulate, but you're really only interested in having a good resolution at the interface, then the cost of the dynamic meshing can be small compared to the savings due to the overall lower number of cells.

- Anton

[kathrin_kissling]

It will reduce your cost esspeacially if you have large doamins since you have less cells! Otherwise you would have to resolve the whole domain with the decent resolution! With dynamic mesh only the part where your interface is located!

Look at the work of Popinet and Zaleski for example! I think there are descent evaluations of the computational cost regarding the dynamic mesh! Of course their code is effective and adapted to exatly that problem but the overall fact remains!

Best

Kathrin

PS: Seems two persons answered at the same moment

[voingiappone]

Kathrin, I have that Ph.D Thesis and as akidess poited out correctly I cannot find the conditition you mentioned. This doesn't in any way mean that I don't have to dig further in this subject to completely understand the meaning of the parameter....

Regarding the question of the interDyMFoam:

Originally Posted by Andrea_85

from what I know interDyMFoam is interFoam+meshRefinement (normally close to the interface to have a sharp interface), so i cannot figure out how the computational cost can be reduced. Normally it can take quite much computational time to respect to interFoam, or am i wrong?

I imagine (and think I once found here on the Forum) exactly the same.... It makes sense that the interface mesh refinement is done only on the interface itself, but that is nevertheless an addiction to the normal interFoam calculations... or not? I'm probably missing a crucial point here....
However, I'll give it a shot and try to do it the "practical" way, comparing the "time interFoam" and "time interDyMFoam" to see the results.
Of course I'll look for the Popinet and Zaleski paper and read it.

Thank you all for your precious help!

Luca

[kathrin_kissling]

Of course its an additional step.
BUT:
1. you can resolve your far field as coarse as possible
2. you have still sufficient resolution of the bubble with about 10-20% more computational
cost compared to the coarse resolution. Including both the flow calculation and the
dynamic mesh handling.

Otherwise you will have to refine the complete domain.

Best

Kathrin

[winsong]

Originally Posted by voingiappone

Howdy!

I have been simulating a bubble column with the bubbleFoam but with no success (no convergence at all) and then decided to give a try to the VOF method. I have found papers about that and it seems to be adequate for what I need.

I created a mesh with 3505 cells and 1851 points simulating a flat 0.2x0.05x0.5 (WxDxH meters) reactor with a 0.003m inlet for injecting air at the bottom. The column is 3/5 filled with water (throug setFields run on alpha1 parameter). A very simple layout. I uploaded the case here so you can take a look at it.

Running the simulation this time is a breeze.... it takes centuries because the mesh is small and fine expecially around the inlet but it actually computes the bubbles coming out.

The problem:
when the bubble formed detaches from the inlet it travels few millimeters and "vanishes". Take a look to the attached pic to see what I mean. There you can see the alpha1 view of 3 bubbles: one forming on the bottom (blue core), one detached(green core) and one that has vanished (green mist).

My question this time is: why do the bubbles vanish instead of rising like an actual bubble towards the surface?

The only thing I could think about was that the mesh is still too coarse and, if the bubble splits in smaller ones, the actually calculated small bubbles cannot be described with the mesh cells (too big). As a result, the aplha becomes smaller and smaller ---> the green mist....

Can somebody help me with this? Meanwhile I'll try a mesh with 4 time more cells....

Thank you very much.

Luca

Hi Luca,

Have you solved your problems?
I did some simulations recently, and there were some strange results.
1 I can get good bubbles in bubble column, just use the set of interFoam dam break tutorial. The inlet velocity is fixedValue [0 0.01 0], alpha1 for water is set to 1.
2 Use setFields to set the alpha1 as 4/5 of column is filled, then the air can not get into the column.
I have compared the pressure calculations, in the same time step (0.01), p is from 0 to -2000 (from bottom to top) in set 1, and p will go to balance after 5-6 time steps; p is form 2000 to 0, which is the balance situation. I think the different results at the beginning time steps make this strange result.

Any advice is welcomed!

Thank you!

Ted