[Antanas]

Hello!

Is it possible to implement degassing boundary condition with algebraic slip model? What possibilities are there? Free slip wall with sinks and equations modifications? Maybe I can use opening boundary condition? But in this case I'm not sure about opening temperature if problem isn't isothermal. Or maybe wall deposition condition will do the trick?

[ghorrocks]

The documentation suggests that if you have a continuous liquid phase and a dispersed gas phase (either eularian or particles) then you can use a degassing boundary. In that case there will be no need for the walls, sinks or anything else.

[Antanas]

Originally Posted by ghorrocks

The documentation suggests that if you have a continuous liquid phase and a dispersed gas phase (either eularian or particles) then you can use a degassing boundary. In that case there will be no need for the walls, sinks or anything else.

Unfortunately degassing BC is available in case of full Euler multiphase model and unavailable when algebraic slip model is used.

[ghorrocks]

Yes, that would make sense - the continuous phase cannot have any motion normal to the degassing boundary (it is treated as a slip wall for the continuous phase), so that means the algebraic slip model cannot result in the disperse phase crossing the boundary.

So that means that if you are thinking of using a degassing boundary the algebraic slip model is not an appropriate model to use. You probably need to move to a inhomogenous multiphase model instead.

[Antanas]

Originally Posted by ghorrocks

Yes, that would make sense - the continuous phase cannot have any motion normal to the degassing boundary (it is treated as a slip wall for the continuous phase), so that means the algebraic slip model cannot result in the disperse phase crossing the boundary.

So that means that if you are thinking of using a degassing boundary the algebraic slip model is not an appropriate model to use. You probably need to move to a inhomogenous multiphase model instead.

Or I can extend my domain to include top gas region and model free surface, correct? Because in my case full Euler approach is too time consuming.

However I definitly saw papers where algebraic slip model was used to model bubble columns without modeling free surface of liquid.

Some guys used opening BC with liquid volume fraction = 1, and gas = 0. But the problem was isothermal and I'm not sure about temperature in non-isothermal case.

[ghorrocks]

Running a free surface model is likely to be far more expensive than an inhomogeneous model. And you cannot run algebraic slip with a free surface model anyway - unless you are going to make the liquid phase a variable composition mixture and then you have made the model far more complex.

The algebraic slip model is not suitable when non-drag forces are significant. If you have buoyancy then you have non-drag forces. At least with the algebraic slip model implemented in CFX that is the case.

[Antanas]

Originally Posted by ghorrocks

The algebraic slip model is not suitable when non-drag forces are significant. If you have buoyancy then you have non-drag forces. At least with the algebraic slip model implemented in CFX that is the case.

OK. I agree that if non-drag forces are significant ASM produces not best results. But are this forces always significant? It is said, for example, that lift force in most cases is insignificant compared to the drag force.

Anyway, even when we use full Euler model we not neccessarily account for non-drag forces. They may add problems, make model more computationally expensive, require fine meshes etc. Sometimes it is better to sacrifice accuracy a bit, but reduce computational time.

[ghorrocks]

You have to go further than saying "not the best results" - if non-drag forces are important then ASM cannot model them. So the key is to decide whether non-drag forces are important. If you want bubbles to exit via the top surface this is driven by gravity, not drag forces. So if you want the bubbles to exit via the top surface you cannot use ASM.

[oj.bulmer]

But are this forces always significant?

These are the excerpts from my thesis on bubble column simulations:

RADIAL FORCES:
For uniform slip velocity between bubble and liquid phase, the drag force is dominant. But for non-uniform slip velocity with rotational continuous phase, which is a characteristic of heterogeneous flow regime, other radial forces such as lateral lift and Magnus forces have to be accounted for. The difference between velocities of bubble and liquid plays a major role in deciding the lift force. Generally, smaller bubbles have smaller velocities and they are spherical because surface tension is highly influential; hence the flow structure in the wake of smaller bubble is steady and symmetric. This structure interacts with the shear layers around the bubble to generate a lift in the direction towards wall. Incidentally, compared to smaller bubbles, the large bubbles have higher velocities and are influenced by inertial and gravity forces as a result of which their shape is highly distorted. Thus the structure of flow in the wake of bigger bubbles is unsteady and highly asymmetric and hence when they interact with the shear layers, the net force generated is towards the centre of the tank. Essentially, for the bubbles above and below a certain critical diameter, the sign of lift coefficient is opposite. As a result, bigger bubbles tend to move towards centre while smaller bubbles move towards wall. Nevertheless, it is significant only in the shear layers that have widths comparable to mean diameter of bubbles. Thus, for bubbly flow in vertical pipe, where the pipe diameter is comparable to that of large bubbles, lift is significant. But for an industrial bubble column with diameter of the order of one meter or more, lift is not as significant.

VIRTUAL MASS FORCE:
When the slip velocity is not constant, the bubbles accelerate through the continuous phase.
This makes the surrounding fluid to accelerate with them, creating a drag which is termed as
added or virtual mass effect. Although this force is prominent when dispersed phase density is less than that of continuous phase density, it is generally significant only in the presence of large accelerated transient flows like flow through narrow restriction.

TURBULENT DISPERSION FORCE:
Dispersion is a mechanism that arises due to difference in concentrations of bubble phase at
different regions of the bubble column. On a macro scale, the turbulent dispersion creates a flux of bubbles from regions of higher concentration to the regions of lower concentration in an attempt to homogenise the volume fraction through the turbulent movement. This motion is influenced by turbulent disturbances and the inter-phase drag between the two phases. Its definition is analogous to diffusion in that it depends on gradient of volume fractions of both the continuous and dispersed phase. Essentially, the liquid eddies smaller than bubbles tend to break them, but the eddies larger than bubbles entrap them and transport them. Yet, owing to slip, often bubbles escape the eddies as well and hence the eddy motion is not strictly followed by all the bubbles.

WALL LUBRICATION FORCE:
It has been observed that, in vertical pipe flow, bubble concentrations tend to peak near the wall but not immediately adjacent to the wall. To accommodate this behaviour, an effect called wall lubrication force is modelled, that pushes the bubbles away from wall. The effect of this force is limited in very thin layers near wall and very fine mesh is required to effectively model it. Besides, for the walls with lubrication force active, no-slip boundary
condition has to be specified for gas phase, which is computationally taxing. Given that this
force is prominent only for vertical pipes with considerably smaller diameter as compared to
bubble column, its effect can be safely ignored in the current set-up to reduce the computational expense.

***

There is a lot of literature you can find on this, if you dig a bit.

Good luck!

[Antanas]

Originally Posted by oj.bulmer

These are the excerpts from my thesis on bubble column simulations:

I already saw such estimation, but thank you anyway!

In my case the domain dimensions are 0.33 [m] X 0.1 [m] X 0.82 [m]. And I have two dispersed phases which are produced in certain areas by electrochemical process and then moved upward by buoyancy. The movement of bubbles is major cause of primary phase movement.

The bubbles of first dispersed phase have mean diameter about 1 [mm] while that of the second dispersed phase is unknown. What is known is that this are relatively large bubbles that do not detach much from wall on which they arise and slip upward along it.

For now I want to take into account only small bubbles, because of unknown size and shape of large bubbles. And I don't want to use too fine mesh, because the problem is complex as it is (I have to model coupled processes of charge transfer, heat transfer, momentum transfer, mass transfer). So I think that in my case I can neglect most of non-drag forces, can't I?

[ghorrocks]

Your reply raises more questions than it answers.

The large bubble phase clearly needs a full inhomogenous eularian model as you said that both buoyancy and drag forces are important. It is impossible to tell what is the appropriate model for your small bubble phase as you have not told us anything about what you expect it to do or its characteristics.

How can you model the small bubble phase if you do not know the bubble size?

The mesh size you require should be determined by a mesh sensitivity study once you have all the physics working. Of course you don't want it to be too fine - but if it is required for accuracy then you will need it. But first things first - get the physics working first before you worry about the mesh.

You also imply the large bubbles do not detach from the wall. You will need to include this on the large bubble phase if it is important.

[Antanas]

Originally Posted by ghorrocks

Your reply raises more questions than it answers.

The large bubble phase clearly needs a full inhomogenous eularian model as you said that both buoyancy and drag forces are important. It is impossible to tell what is the appropriate model for your small bubble phase as you have not told us anything about what you expect it to do or its characteristics.

How can you model the small bubble phase if you do not know the bubble size?

The mesh size you require should be determined by a mesh sensitivity study once you have all the physics working. Of course you don't want it to be too fine - but if it is required for accuracy then you will need it. But first things first - get the physics working first before you worry about the mesh.

You also imply the large bubbles do not detach from the wall. You will need to include this on the large bubble phase if it is important.

Ah, yes! I did not mention that primary phase is liquid and secondary dispersed phases are relatively light gases.

The small bubbles is spherical with mean diameter equal to 1 [mm], their properties is similar to that of hydrogen gas. So size of small bubbles is known.

Because of lack of information about size of large bubble I don't want to model them at the moment. As I mentioned this bubbles slip along the wall and don't spread to the bulk of the domain. So maybe there will be no need to model them as bubbles but account for their motion through moving wall for example. But the problem then is the velocity of the wall which is unknown.

At present I don't model all the processes as coupled, on the contrary I decouple them and model in sequence. Right now I try to deal with fluids motion and the problem is that calculation is too slow. (Even though in reality the process must stabilize somehow, as I understand it is better to model this as transient, correct?) So the main task is to find balance between accuracy and calculation time.

[ghorrocks]

So maybe there will be no need to model them as bubbles but account for their motion through moving wall for example. But the problem then is the velocity of the wall which is unknown.

Comments like that suggest to me that you are guessing. If you want any hope of an accurate simulation you need to work out what controls their motion and what influence they have on the bulk flow. You could either generate a disperse bubble phase next to the wall and let them rise and pull the continuous phase by themselves (then what is the physics which keeps them near the wall?) Or you could replace the bubbles with a shear stress on the external wall (then the shear stress will be a function of the number of bubbles, their size, their velocity, wall proximity, entrained continuous phase fluid - do you know these things adequately to define a shear stress?)

Modelling this decoupled is always a good place to start and often you find it tells you enough and the fully coupled model is not required.

If you are interested in the steady flow then you should try to model it as steady.

[Antanas]

Originally Posted by ghorrocks

Comments like that suggest to me that you are guessing.

Yes you're right, I'm guessing. Because there is lack of data. The device that I'm trying to model is industrial device and nobody will experiment with it. It is not good situation when guys want you to model something but can't give you enough info about it, but it's reality.

Originally Posted by ghorrocks

If you want any hope of an accurate simulation you need to work out what controls their motion and what influence they have on the bulk flow. You could either generate a disperse bubble phase next to the wall and let them rise and pull the continuous phase by themselves (then what is the physics which keeps them near the wall?)

I think this is better choice because the answer to this

Originally Posted by ghorrocks

then the shear stress will be a function of the number of bubbles, their size, their velocity, wall proximity, entrained continuous phase fluid - do you know these things adequately to define a shear stress

is "NO, I don't".

About the physics which keeps bubbles near the wall I only know that they are formed on imperfections on the wall surface, inside pores and so on.
When pore is filled with gas, the gas spreads on the flat part all around the pore. Small bubble then coalesce and grow. When the size of the bubbles becomes large enough they begin to slip upward along the wall. This bubbles forms something like gaseous film. At the vicinity of the wall, the gaseous film interacts very strongly with the dense fluid and lifts it at the same velocity.

[Raijin Thunderkeg]

When the gas flowrate is large, the top free surface will fluctuate remarkably. Is it appropriate to use a degassing BC? When the degassing BC is used, a warning message appears during the solution like " A wall has been placed at portion(s) of an OUTLET ". How to solve this problem?

[Antanas]

Originally Posted by Raijin Thunderkeg

When the gas flowrate is large, the top free surface will fluctuate remarkably. Is it appropriate to use a degassing BC? When the degassing BC is used, a warning message appears during the solution like " A wall has been placed at portion(s) of an OUTLET ". How to solve this problem?

In CFX Help it is said that "When Degassing Boundary Condition is selected as the Flow Specification of an outlet, the continuous phase and any dispersed solid phases that may be present see this boundary as a free-slip wall and do not leave the domain. Dispersed fluid phases and Lagrange particles see this boundary as an outlet. However, the outlet pressure is not specified. Instead, a pressure distribution is computed on this fixed-position boundary, and can be interpreted as representing the weight of the surface height variations in the real flow."

So I think it is appropriate condition. The message "A wall has been placed at portion(s) of an OUTLET..." should usually disappear after a couple of iterations.

[Raijin Thunderkeg]

Thanks for ur reply.

I have some other questions about ASM.
1)How to set outlet boundary condition in ASM? A wall with free slip boundary for the continuous phase and deposition for dispersed phase?
2)Can ASM deal with the compressibility of dispersed phase? I get an initial field with constant property gas using ASM and the absolute pressure is correct, but when I try it with an ideal gas, the cfx5solve always exits with an error. What is the reason?

[Antanas]

Originally Posted by Raijin Thunderkeg

Thanks for ur reply.

I have some other questions about ASM.
1)How to set outlet boundary condition in ASM? A wall with free slip boundary for the continuous phase and deposition for dispersed phase?
2)Can ASM deal with the compressibility of dispersed phase? I get an initial field with constant property gas using ASM and the absolute pressure is correct, but when I try it with an ideal gas, the cfx5solve always exits with an error. What is the reason?

1)I have the same question. Actually that is why I started this topic. Wall deposition condition removes dispersed phase and adds liquid phase instead. So I'm not sure that this is what we need. We need something like degassing BC which acts like free slip wall for liquid phase and sink for gaseous. So we may impose free slip wall with sink term for gas phase continuity equation which will remove all gas from boundary during one time step. Also we may need to include additional force to momentum equation due to mass sink and probably do something with pressure.

Also I think that we may use opening BC with fluid volume fraction = 1 and gas volume fraction = 0. The problem is that if we model non-isothermal regime we also must specify opening temperature. And I'm not sure what to do in this case. I think that liquid should return into the domain with its exit temperature but don't know how to specify this.

2) I have not seen any limitations of ASM that relate to compressibility. What kind of error did you get?

[Raijin Thunderkeg]

The solver always crashes in the first 5 steps. The message is "The ansys cfx solver exited with return code 1". I know this must result from the variation of the property of the gas from constant to ideal gas. But I don't know how to adjust this. Do you have any ideas ?

[Antanas]

Originally Posted by Raijin Thunderkeg

The solver always crashes in the first 5 steps. The message is "The ansys cfx solver exited with return code 1". I know this must result from the variation of the property of the gas from constant to ideal gas. But I don't know how to adjust this. Do you have any ideas ?

Maybe you should use smaller timestep for several staring iterations.