Learning Forum

[AnthonyB08]

Hi all,

I am simulating a transient counter-flow two phase packed ped using the Eulerian-Eulerian multiphase model. The geometry and boundary conditions are listed below.

Bottom of domain ( z = 2.205m) pressure-outlet with the back flow volume fraction 1 for the gas phase

Top of the domain (z = 0 m) Velocity-Inlet  was placed with velocity of the gas phase as -0.25 m/s and a volume fraction of 1 for the gas phase.

Note these boundary conditions were instated to force the gas phase to enter the domain from the bottom uniformly.

Wall conditions for the walls.

At the liquid sparger a Velocity-Inlet was placed, with velocity of the liquid phase as 0.038 m/s and a volume fraction of 1 for the liquid phase.

 

This simulation iterates nicely up until the liquid phase enters the packed bed which is ~ 0.08 [m] from the top , as seen in the picture.

 

The simulation diverges because in the packed bed domain, which was spliced in design space, a fluid dispersion momentum source term is introduced, see below.

 

 

Most of these variables on constants, so the only variable that may cause issues is the division of volume fraction. So to avoid 1/0 in the source term I enforced a conditional statement with a volume fraction tolerance, see below.

 

However, my simulation still diverges when the liquid enters the packed bed domain. I have done a thorough investigation and found that my simulation works if the source term is removed. The fluid flows freely into the packed bed domain.

Other key simulation parameters:

1.       When initializing the gas phase occupies the entire domain

2.       Implicit Volume fraction parameters

3.       Time step is 1e-04

4.       Mesh size: Cells – 144,488, Faces – 365,148, Nodes – 83,839

5.       I have tried to refine the mesh at the interface ( still diverges)

So what does the community suggest?

[Rob]

What happens if you put a limiter on F_Disp_L to ensure it can't be non-physical? 

[AnthonyB08]

Okay so I have imposed limitations on variables that make the source term non-physical. The limitations constrain the force term similar to this graph I developed in MATLAB.

The simulation diverged once again. I changed the gradient volume fraction to the magnitude of the gradient... I am not sure about this. 

Also, do you think that the gradient of the volume fraction is respective of dimension? 

[AnthonyB08]

UPDATE: The simulation runs smoothly if I take the magnitude of the gradient.. which is confusing because it makes more sense to consider the gradient with respect to its dimension of the source term. 

[Rob]

Why does the dispersion force become non-zero for volume fraction below 0.1 and over 0.9 ?  It's also a very steep gradient, so maybe that's the cause of your problems: small change in volume fraction gives a very different force repsonse. With that you could trigger a feed back look that bounces the force between -10 and -60 for a negligble change in flow field. 

[AnthonyB08]

Because the division by a small number, say 0.01, makes the dispersion force extremely high. 

I am now working with a 3-D plot to see the gradient affects 

I will look into it, thanks!

[AnthonyB08]

This is what the graph looks like if I make the volume fraction and gradient of VOF a vector from 0 to 1 

[Rob]

Why would dispersion be so high? 

[AnthonyB08]

 

The first term in the liquid dispersion force 

has only the drift velocity of the liquid phase which is seen as : 

If the volume fraction of the liquid, at a given time step, is  0.001 then the U_D_L becomes 1000 * spread * grad _vof * mag of vel 

Essentially, the 1/alpha_L when alpha_L is very low causes the dispersion force to be excessive. 

[Rob]

And if the volume fraction is very low there's not much mass to add the force too so it'll be even less stable. Maybe add some limits? 

[AnthonyB08]

Okay, do you suggest limits to force itself or the variables? 

[Rob]

Treading carefully as I'm not permitted to use "engineering knowledge" or provide detailed insight.  I'd limit the returned source value and monitor where it's being capped. Typically, the solver may fail if source terms are excessive, or very rapidly changing due to whatever is controlling the source. In this case it's more obvious that the high & low volume fractions fall off a plateau: just because the maths says so it doesn't mean it's physically sensible. 

[AnthonyB08]

Okay , that makes sense - thanks. I will limit the force term gradually and see what this does