Species Mass Transfer, Multiphase setup problems..?

  • 273 Views
  • Last Post 03 February 2020
  • Topic Is Solved
taegyu87 posted this 22 January 2020

Hi

I am trying to simulate multiphase flow. Specifically, my inlet is carbonated water, and my geometry is venturi (converging diverging nozzle shape). So, through nozzle, the pressure will change, and solubility will be also changed. So, I want to see the CO2 in carbonated water is undissolved from carbonated water, and escape to ambient air.

I am trying to use multiphase Eulerian, species transport model, mass transfer from species to species with Henry's Law.

I am setting up...

  • fluids
    • mixture: CO2 and water
    • mixture: CO2 and air
    • air
  • mass transfer
    •    mixture (CO2 and water): CO2 --> mixture (co2 and air): co2
    • in order to represent undissolved co2 from carbonated water

Is this right setup to represent this phenomenon?

I keep getting divergence in residual...it says it is detecting floating point....

Could  anyone give me some advice?

Order By: Standard | Newest | Votes
taegyu87 posted this 22 January 2020

 FYI, I read these comments... and applied ....

https://studentcommunity.ansys.com/thread/dissolved-oxygen-in-water-1/?order=all#comment-7f7e6c45-1b8d-41b4-863f-ab430089a6c0

CO2 from mixture (water + CO2) --> CO2 from mixture (CO2 + dummy CO2)

in order to imitate co2 escaping from carbonated water as pressure change through nozzle shape geometry.

rwoolhou posted this 23 January 2020

What time step are you using?

taegyu87 posted this 23 January 2020

1. I am using steady state condition. I am trying to add lift force with Tomiyama or 0.53 as a constant, but it keeps diverging at 80 iteration. Now, I am trying to solve it without lift force, and run for 3000 iteration. Then, I will add lift force back to the system. Should I use transient solution?

2. I am thinking about using transient with 0.01 s time step if I need to use it. Should I use 0.001s or smaller?

 

taegyu87 posted this 23 January 2020

Here is my setup and geometry.

Top edge is inlet, and bottom edge is outlet. Mesh size is 0.00001m with triangle.

Virtual Mass: not applied

Drag: schiller-naumann

Lift: not applied

Surface Tension: constant=0.072

Interfacial Area: ia-symmetric

Mass Transfer is ....

 

This is my setup for mass transfer.

carb-water is mixture of water and co2, and undis-co2 is mixture of co2 and dummy co2.

 

Inlet condition:

   carb-water: vel=4.5m/s, species: mass fraction of water =0.992

   undis-co2: vel=4.5m/s, species: mass fraction of co2=0.999, multiphase: volume fraction=0.001

Outlet condition:

   air: back flow volume fraction =1

 

And my calculation method and setup is...

 

I keep getting divergence of the solution. Do you need any other information about my setup?

Do you have any feedback to improve solution convergence?

Did I do something wrong in setup?

 

Thank you for your help!

 

 

taegyu87 posted this 23 January 2020

The solution with transient 0.001 diverged.... and this is what fluent says...

 

 

 

 

rwoolhou posted this 23 January 2020

How does the solution look just before it diverges? Also, if the backflow vf is all air, what's stopping the domain filling with air?

taegyu87 posted this 23 January 2020

Thank you for getting back to me.

So, here is the screenshot of current stage. For this case, I turn off the lift force to get better divergent.

After initialization, I patched entire space with air volume fraction = 1. So, i think it will stop the air to come into the domain.

 

taegyu87 posted this 23 January 2020

I ran few more iteration and i got this error...

Do yo know why i am getting this error and how to fix this?

abenhadj posted this 24 January 2020

You should reduce the case into the backbone settings: Why do you have three phases? Why turbulence per phase? You are putting a lot of complexities into this case where the most important thing is based on something which is not really ideal as it assumes ideal solution and Henry's law. Use single turbulence field, two phases ( I do not know why air in this system) and transient run.

Best regards, Amine

taegyu87 posted this 24 January 2020

Thank you for your comment.

1. Why do you have three phases?What I eventually want to simulate when carbonated water pour into cup, how much CO2 is escaping. So, for that, I thought I should have mixture( water + CO2), CO2 (undissolved CO2 which is escaping to ambient), and ambient air.

My original simulation is carbonated water is coming out from the nozzle at the top and pour down into the cup, and I was trying to observe CO2 escaping from carbonated water stream into water. That is why I am trying to add air into my system. Do you suggest other way in order to have only two phase? Is mixture (water+co2) and mixture( CO2+ air) able to represent my system?

2. Why turbulence per phase? I thought this will help my simulation to be stabilized better. What do you suggest?

3. I do not need to run with transient. I was running Pseudo transient setting..

 

Could you please suggest some setting so that I can simplify my model?

 

Thank you so much for your help!

abenhadj posted this 24 January 2020

1/Suggest two phases: water mixture (+dissolved CO2) + gaseous mixture (Air+CO2) If the mass transfer occurs at the free surface probably your will probably require an UDF or at least to smear the interface and use that builtin model. This depends on the initial state. If all phases are mixed together than you might use Henry's law built in Fluent.

 

2/Single turbulence field

3/Run transient

Best regards, Amine

taegyu87 posted this 24 January 2020

Thanks Amine.

1. I will try two mixtures model. I do not have experience in writing UDF. I will start to study about it. Meanwhile, I will use builtin model. But can you specify what builtin model you are talking? Could you tell me some more details about the setting that I should do? I think initially all phases are mixed together very well, but i think they will not be mixed well as mass transfer phenomenon happening I think. So, in this case I should use Henry's law.. is it correct?

 

2. I will use mixture or dispersed.

 

3. I will run transient with 0.001 time step.

 

I will try what you told me, and let you know what happens.

 

Thank you for your help.

abenhadj posted this 24 January 2020

1/Henry's law is fine here (assuming ideal solution-...). I am talking about the case where you have stratified flows: gas over liquid. Here you probably need to write an UDF.

2/ok

3/ok

Best regards, Amine

taegyu87 posted this 24 January 2020

1. About the stratified flow... my inlet flow of mixture (water+co2) is carbonated water (co2 fully dissolved in water). Is my mixture setup of that correct? Or do I still need to write UDF for that?

abenhadj posted this 24 January 2020

You have a mixed flow at inlet. You need an UDF (probably) if you have a stratified flow: stratified flow regime is like this: 

 

Image result for stratified flow (Authors: Sketches of flow regimes for two-phase flow in a horizontal pipe. Source: Weisman, J. Two-phase flow patterns. Chapter 15 in Handbook of Fluids in Motion, Cheremisinoff N.P., Gupta R. 1983, Ann Arbor Science Publishers.)

Best regards, Amine

taegyu87 posted this 24 January 2020

I am running simulation as you told me to do. It is still running. I think it will take more than 48 hours. Also, it seems it is going to be diverged.

Is there a way to improve computational time?

And any recommendation to improve convergence?

 

Thank you so much for your help!

abenhadj posted this 27 January 2020

It does not look good. What is the initial state in your case? Add description of boundary conditions. Bad settings by the way un your Run Task Panel (why 200 iteration per time step? rather smaller time step sizes and just 10 iterations per time step).

Best regards, Amine

taegyu87 posted this 27 January 2020

1. my inlet conditions are...

inlet: top surface:

carb water = mixture of CO2 + Water

And also... as an initial seeding...

mixture of Air + CO2

Since I only want co2 interaction...air mass frac = 0

SInce it is an initial seeding I gave small vol fraction.

Outlet Conditon....

only air is coming back as a backflow

 

 

2. For initially zation, I did hybrid initiallization and patched air at entire region.

 

3. I will try smaller time-step and and 10 iteration at each step. I just put 200 iteration at each step only because I thought that would give me better convergence. But i will use your suggestion and run the simulation again.

 

4. Is there any wrong setting on my initial & boundary condition setup?

 

Thank you.

 

abenhadj posted this 27 January 2020

Both Co2 components need to be solved via transport equations.

 

Best regards, Amine

taegyu87 posted this 27 January 2020

Amine,

Do you mean that CO2 should be the secondary species in the mixture? Instead of adjusting air or water species mass fraction, do I need to adjust CO2 mass fraction at species tap? Is that what you mean?

Thank you.

abenhadj posted this 27 January 2020

Yes. It has be solved and not treated as ballast component. You do not require the seeding at inlet but in volume. I think I shared how to do that in another post.

Best regards, Amine

taegyu87 posted this 27 January 2020

Thank you, Amine. Yes, I read that post, and that is why I was trying to do seeding at inlet.

But I will not do seeding at inlet but patch at initiallization section. I think that is what I need to do accoring to the previous post.

So, this is modified setup...

I have one question... I am solving it with SIMPLE because I do not see any information says COUPLE is better than SIMPLE. Which solution method do you recommend?

Here is my setup for solution and under-relaxation factors.

Is my under-relaxation factor too low?

 

For seeding, is it right way?