[jason]

Hello,


I'm trying to understand multiphaseEulerFoam (and using OF v8.0) and hope someone can enlighten me. The attached case should also run with lower versions using reactingMultiPhaseEulerFoam and by changing the type of phase calculation in the file constant/phaseProperties.


Essentially, I have 3 phases, water, oil and air (water is the continuous phase). I have a vertical pipe with water entering at the bottom and travelling to the top. Later I want to introduce bubbles, but not yet.


I set alpha.air and alpha.oil to 0 everywhere. I run the case, converges nicely and I obtain results for the water phase passing through the pipe, however, even though alpha.air and alpha.oil are still zero, U.air and U.oil are not and are quite different from U.water (attached png shows profile across the centre of the pipe (not yet fully developed))

Eg
alpha.water = 1, U.water ~ 1 m/s as set in the U.water boundary condition
alpha.air = 0, U.air ~ 1.54 m/s
alpha.oil = 0, U.oil ~ 1.38 m/s

Why would I be obtaining non-zero velocities for phases that are not present, I understood that the momentum/continuity equations for each phase depend on the value of alpha.xxx?


Reference:
http://downloads.hindawi.com/journal...013/128936.pdf

Many thanks in advance
Jason


PS - I get the same effect in 3D also

[Ricky-11]

Hi Jason.

I'm working with same solver/version and wondering the same.

Did you come to any conclusion?

[jason]

Hi Ricky,
Unfortunately not yet
Did you have any ideas?
Jason

[Ricky-11]

Hi Jason.

I had this conversation on the bug tracking:

https://bugs.openfoam.org/view.php?id=3561

What's annoying is, at least in my experience, there could be situation where such artificial velocities have extreme values which may impact time step size if a Courant number limit is imposed.

Unfortunately, they tagged my report as user request so I don't think the developers will be willing to work on this...

[jason]

Thanks for the link, very interesting.


The comment by Henry ... in the simulations it will approach the velocity of the continuous phase as the phase-fraction -> 0 due to the drag.


.... gives me confidence that the solver is correct, although I'm also finding it difficult to get my head around.


In your case perhaps you could use or modify the fvOption limitVelocity in your region of interest or depending on the value of the phase fraction?

[andrea coletto]

Hi all,
I noticed this fact and I was wondering too.
Maybe the solution is here

twoPhaseEulerFoam - unphysical behaviour

I understood that multiphaseeulerfoam doesn't solve the traditional form of momentum equation, but their intensive form, i.e. the equation divided by volume fraction.
This causes the drag force not to tend to zero when alpha do it.

Unfortunately, this should be valid for old versions of OF, but I read in recent post that such implementation of momentum equations shouldn't be valid any longer.
I tried to read the solver code, but I'm not particulary good at it.

Can you help me please? According to your knowledge, is this formulation still implemented in OF?

Regards

[jason]

Hi,


Also still trying to understand why this occurs and also have trouble following the multiphaseEulerFoam code



I noticed that in the link you sent at the bottom post


"multiphaseEulerFoam (and compressibleTwoPhaseEulerFoam) uses the conservative form of the momentum equation"


Also, in this post, it seems to be confirmed.
Phase intensive momentum equation


The link to the paper by Venier et al provides interesting reading and also confirms the conservative form and explains why one might get non-zero velocities as alpha tends to zero, to avoid singularities, quote....the velocity of the disperse phase is set equal to the velocity of the continuous phase in those cells where the particle phase fraction gets below a certain critical value. A natural way to achieve this is to preserve the drag force as a non-zero term in the momentum equation when alpha tends to zero ...



Looking at the code for a couple of drag models this approach seems to be implemented.



In my application, I am concerned with obtaining the slip velocity, thus, if the velocity of the continuous phase = the velocity of the dispersed phase when alpha = 0 then slip velocity = 0 which is what I would expect if there is only the continuous phase present.



I think that might work for me


Thanks for pointing me in different directions.


Regards

[geth03]

Originally Posted by Ricky-11

Hi Jason.

I had this conversation on the bug tracking:

https://bugs.openfoam.org/view.php?id=3561

What's annoying is, at least in my experience, there could be situation where such artificial velocities have extreme values which may impact time step size if a Courant number limit is imposed.

Unfortunately, they tagged my report as user request so I don't think the developers will be willing to work on this...

hey,

i am currently simulating multiphase flow with OF version 7 and my courant number explodes for dispersed phases where the volume fraction is zero but the velocity becomes really high for the dispersed phase. I was able to fix it with different discretization schemes. but nevertheless when the volume fraction approaches zero it should not bother the courant number.

i am now investigating how the courant number is calculated for multiphase flow in the code and if it accounts for alphas.