Foam flow through a channel
 

Good day everyone,

I've been working on a project for the last month and it's been really hard to obtain anything from the CFX software. I've read all previous threads with similar problems and tried their solutions, but no one seems to work.

Problem:

Multiphase problem:
Air (Disperse fluid) + Water (Continuous fluid) (Foam Flow)
Square channel (21x1 mm) (2D problem)
Channel length: 315 mm
Mesh element size: 0,5 mm square
Walls at the top and bottom
Symmetry at both side faces
Inlet: 2 cm/s (Air Volume Fraction: 0.7 and Water Volume Fraction: 0.3)
Outlet: Average Static pressure 1 atm

The main objective is to determinate the pressure losses along the channel. I've tried it all: steady state, transient, turbulent, laminar, changing the timestep, prolonging the outlet, openings, specified blend factor, course mesh. The problem doesn't even start it makes 2 iterations and crashes.

If anyone can give me a clue of what to do, you'll relief me from a lot of suffering. :D

Thanks in advance

RChovet

When it crashes what does the .out file say?

Have you tried double precision?

Thanks for the answer RichochetJ,

I've always used double precision option checked.
In the first iteration it starts to put walls at the outlet (I understand why it does that), then crashes and says:
ERROR #004100018 has occurred in subroutines FINMES
Message:
Fatal overflow in linear solver

Greetings
RCH

This is a classic case of divergence. Moreover, the approach you took seems to be like taking all sorts of medicines to see which one gives you relief. Instead, I would first diagnose the disease and then decide the course of medication!

1) It's a multiphase problem, try using a nice hex mesh for faster progress.
2) Try local timescale in steady state and try increasing its value. This should facilitate different timescales through out the domain, depending on the local courant numbers, instead of auto timescale that uses universal timescale. Try value of 5, or increase if necessary.
3) If the solution still diverges, try transient state with adaptive timestep, minimum timestep being 1e-8 s and max being say 1000 s, min max coeff being 5 and 10. Let CFX decide the proper timescale, since you never know whether the timesteps you tried were sufficient, before ruling it out. Make sure you give reasonable convergence target.

OJ

Thanks a lot OJ,

I'll be back as soon as i finish the diagnose.

Greetings
RCH

The overflow is a FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

This is a very high air volume fraction. Are you sure your multiphase model is valid?

Glenn,

Thanks for the link, i've already read it. Trust me i've tried it all.
However, how do i know if the multiphase model is valid?

Regards
RCH

Read the CFX documentation on the multiphase models you are using and follow up the references listed - especially the momentum transfer models. These models are only valid for specific ranges of volume fraction.

Got it.
I'll be back with the answer
Greetings to all

Still Stuck!
 

Good day everyone,

So I'm back with the results from your previous recommandations.

I change the mesh... Still nothing
I tried a physical timestep and increasing its value... Nothing
Transient state with adaptative timestep... Nope

And finally re-read the whole multiphase model theory and find some interesting things:
There is no volume fraction limit... Only for some drag models (Schiller Nauman and Wen Yu) but this is not the case.
Some time convergence can be obtained by defining a minimum volume fraction bigger than the default (10e-18).... Still it did not work

The closest I've got to any result is using the multiphase homogeneous model... Because my bubbles diameter is 0.5mm so I assume is small enough to apply it. Is this correct? Anyways, it does not converges and results are far away from reality.

So any other suggestions?

Thanks in advance for any kind of idea... I'm getting desperate jejejeje.

Greetings

RCH

Rather than just try multiphase models at random, how you done some basic analysis to determine what is going on in your flow so you can choose an appropriate multiphase model? For instance, how much slip is there between the phases? Does each different phase require a different velocity field or can a single velocity field describe it? Or a velocity field with a defined slip? There are different multiphase models for each of these approaches.

We will worry about convergence after you have selected the correct multiphase model.

Thanks for the commitment glenn,
I truly appreciate it...

To answer the questions:

The horizontal foam flow should drain and a 2 mm slip liquid layer should form at the bottom while the top becomes "dryer". So there should be foam all along the conduct except at the bottom.

Because of the high air volume fraction, the air bubbles and the continuous liquid present the same velocity field. However, the velocity field of the liquid film at the bottom can present different values, depending on the total flow.

I tough that the eulerian-eulerian model should work fine.

Let me know what you think about it.

Thanks again

RCH

Yes, you will need to do this with a Eularian-Eularian model. But which one? MUSIG? Algebraic slip? homogenous/inhomogenous?

Foam characteristics
 

Thanks again for the answer Glenn,

So I read the theory (again, jejeje) and I'm a little confuse. We already stablished that it was a Eulerian-Eulerian model. Going through the specific model I got this:
MUSIG - depends on the bubbles diameter and their capacity to change its form
ASM - depends on the slip velocity equilibrium
Inhomogeneous and Homogeneous -are the classic ones that I've been trying to use.

From the description, It seems that all of them might work. Can you provide me a little of help here?

My foam properties are:
bubble diameter: 0.5 mm
dispersed phase: Air at 25
continuos phase: Water
Surface tension: 31.5 mN.m

I'll attach a picture of the foam.

Thanks again
Regards

RCH

Those photographs convince me that it is unlikely you are going to get this to work. The foam is showing some tricky rheology - the right hand image shows peaks, and the left image shows a short "beam" of foam hanging out the end of the duct. This means the foam has elastic/plastic properties for it to hold these shapes against its own weight. CFX does not have any multiphase models (that I am aware of) which can model elastic/plastic deformation. This elastic/plastic behaviour is caused by the bubbles acting like little rubber balls glued together - from the gas in the bubbles being compressed and the surface tension holding it together tightly.

So you have some choices:
* Model it anyway using CFX and you will probably be miles off as there is no appropriate physical model
* Model it using another software which has a good foam model. I have no idea if such a software exists.
* Simplify it down to some form of representative fluid with a representative viscosity, density, and possibly non-Newtonian properties to match the true multiphase flow. This will also probably be difficult to get anywhere near accurate.
* Give up and model something easier. Use experimental results to guide your designs as simulations are too difficult in this type of flow.

I had to do some foam modelling in CFX a few years ago and I chose the last option.

Thank you very much Glenn,

I knew it was going to be tricky... Anyways, I'll follow your suggestion and go for something easier. What really matters is the non-Newtonian properties and the pressure losses this type of fluid can creates.

Best regards
RCH