[Santhosh91]

Hello All,


After looking out multiple threads, I didn't find my answer so I am asking here. I have trouble with solution convergence and I want to make sure I am using this ''constantAlphaContactAngle'' properly.


So I am modelling emulsions flowing in microchannel. Experimentally, we know that there is a thin liquid film between the walls and the emulsions. Therefore I used the following boundary condition for alpha at walls :
{
type constantAlphaContactAngle;
value uniform 1;
theta0 0;
limit gradient;
}


Knowing that alpha = 1 refers to the liquid film (water in my case).
I just don't properly understand if I should use ''gradient'' or ''zeroGradient'' for the limit and what it represents. Also, I don't get why we need to precise value and limit since the contact angle is provided.

If anyone could help me on this, it would be greatly appreciated.


Thanks for your time,
Sincerely,
Santhosh

[LuckyTran]

limit zeroGradient would be equivalent to using type zeroGradient and it is unlikely you would ever want to do that

value in this case would be an output. the list of value would give you the value of alpha on the wall at each cell on this wall. If you do 1 iteration, you will see this value replaced with non-uniform list containing a list of all the solution values.

so the question is whether you want to apply any limiter at all to keep your problem bounded physically. limit none is an option for no limiter. limit 0.5 would clip the field and allow phase fractions no higher than 0.5. limit gradient clips the gradient so that you don't have overshoots and undershoots.

[Santhosh91]

Hello Lucky,


Thanks a lot for the fast reply! So I guess my boundary condition is 'okay'' since I bound physically the solution using a limit on gradient.
Would you say that it would be best to put limit 1 if I am sure that there is a thin liquid film between the emulsions and the walls then ?

[LuckyTran]

alpha can't exceed 1 anyway so there is no point to limit 1. That's basically limit none. You misunderstand what and how it is being limited. limit number if you decide to use it should be used for numbers less than 1.

If you want to force there to always be alpha=1 on a boundary, then use type fixedValue and use value 1, you don't need a contact angle for this.

[arjun]

The fix value of alpha = 1 major contributor to the divergence. Not sure how much it is an replacement to the thin film there as far as solver goes. Thats because solver treats bc different than cells. The thin film is more like very thin shells of prisms.

I would just create very very thin prisms and force alpha to be 1 there mimicking a thin film. This in openfoam does come with very tight time stepping issues.

If you are not confined to only one solver then you can try it in wildkatze where it would work out much easily as far as stability and enforcing the values in thin shells goes.

[Santhosh91]

Hello Arjun,


Thanks for the input! Unfortunately I am confined to interFoam solver since I worked with it for most of my simulations.
Actually I see a thin liquid film with my B.C. for alpha but only when I am using an adptative mesh refinement along with refined cells near the walls. However it is computationally really expensive (especially for 3D scenario).

So I wanted to know if maybe an other B.C. for alpha would help me do the trick with keeping an uniform meshing but it seems not.

[arjun]

Originally Posted by Santhosh91

Hello Arjun,


Thanks for the input! Unfortunately I am confined to interFoam solver since I worked with it for most of my simulations.
Actually I see a thin liquid film with my B.C. for alpha but only when I am using an adptative mesh refinement along with refined cells near the walls. However it is computationally really expensive (especially for 3D scenario).

So I wanted to know if maybe an other B.C. for alpha would help me do the trick with keeping an uniform meshing but it seems not.

Unfortunately other than pointing out what is main cause of instability I can't help here. This is because fixing instability issue with openfoam is upto people who maintain it.

If the wall bc has water and next to it suddenly is air you have very sharp change in densty within 1 cell. Numerically it is challenging and perhaps this is what is causing the problems.

Now how it would be tackled in openfoam is hard to say for me specially when i do not have openfoam to even try such thing

[alancuberoab]

Originally Posted by arjun

Unfortunately other than pointing out what is main cause of instability I can't help here. This is because fixing instability issue with openfoam is upto people who maintain it. td {border: 1px solid #cccccc;}br {mso-data-placement:same-cell;}[FONT=Arial]td {border: 1px solid #cccccc;}br {mso-data-placement:same-cell;}https://pizzatower.io/puckdoku/][color=#td {border: 1px solid #cccccc;}br {mso-data-placement:same-cell;}f7f7ff]td {border: 1px solid #cccccc;}br {mso-data-placement:same-cell;}puckdoku[/COLOR]

If the wall bc has water and next to it suddenly is air you have very sharp change in densty within 1 cell. Numerically it is challenging and perhaps this is what is causing the problems.

Now how it would be tackled in openfoam is hard to say for me specially when i do not have openfoam to even try such thing

I also got this error and tried as you said it worked, thank you