CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT > Fluent Multiphase

Mass transfer between phases

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 10, 2016, 21:49
Smile Mass transfer between phases
  #1
New Member
 
Filipe de Menezes
Join Date: Feb 2012
Posts: 12
Rep Power: 9
filipemt is on a distinguished road
Hi everybody!

I am trying to simulate the mass transfer between two phases. Phisically, there is a gas (CO2) solved in both phases (oil and water), but with higher concentration in water. I want to discover the transfer of CO2 from one to another to obtain vof contours of CO2 as result. Am I clear?
Studying the help, I thought that I should set this gas as specie transport. Am I right? What about a massless discrete phase, does it make sense once this solved gas does not influence the flux?

Another issue, is that I already have a steady velocity field from a steady simulation wich I want to use as the start point to the transient one. So how can I disable all the equations that are not essential to this new stage (as turbulence)?

Thanks in advance for your patience.
filipemt is offline   Reply With Quote

Old   March 11, 2016, 04:41
Default
  #2
Senior Member
 
Cees Haringa
Join Date: May 2013
Location: Delft
Posts: 607
Rep Power: 13
CeesH is on a distinguished road
Hi Filipe,

How big is the domain you are studying? The best option if you are studying a large-scale gas liquid flow is likely the Euler-Euler model. This model, combined with species transport to model multi-species mixtures in each separate phase, should work for your case. Mass transfer can be set in the phase-interaction tab.

The discrete phase model is in essence an option too, but only useful for low gas fractions. If you want to study a very low number of bubbles, you can go for Volume of Fluid.

Good luck!
Cees
CeesH is offline   Reply With Quote

Old   March 11, 2016, 15:18
Default
  #3
New Member
 
Filipe de Menezes
Join Date: Feb 2012
Posts: 12
Rep Power: 9
filipemt is on a distinguished road
Thanks for your coment, CeesH!
My model is in laboratory scale, a 700mmx500mm mechanically stirred tank. The fraction of gas is low and there are too many bubbles. So I think is mixture model.
I tried to setup the simulation but some doubts appeared that I wasnt sure only with help. Could you help me?

In species model >> phases properties, wich fluid should I use? water?
I created a mixture as help demand, but I dont use it anywher, not even in mass transfer it appear (figure). Is it right? My simulation doesnt envolve reactions.

I thinhk to disable the solution of some equation is in solution controls >> equations. Do you agree?

Thank you so much for helping!
Attached Images
File Type: png forum 4.png (40.8 KB, 174 views)
filipemt is offline   Reply With Quote

Old   March 11, 2016, 15:59
Default
  #4
Senior Member
 
Cees Haringa
Join Date: May 2013
Location: Delft
Posts: 607
Rep Power: 13
CeesH is on a distinguished road
Hi Filipe,

Mixture model is a decent start, Euler-Euler 2 phase model may be more accurate - mixture is mostly good if the 2 phases are more or less co-flowing everywhere (bubble column), but not so much in situations where gas and liquid may exhibit different flow directions - which is certainly true near a stirrer.

For mass transfer, be sure to enable the species tracking option as well; otherwise you cannot distinguish between different molecular species in your air and water phases; so what you should do; make 2 species mixtures;

Mixture-liquid: dissolved-CO2 + water
Mixture-gas: CO2-gas + air (where air is basically everything that is not CO2)

Then, in mass transfer, set transfer
CO2-dissolved > CO2-gas

The default is constant rate, if you want to set up local mass transfer rates you will need to write a UDF.

Just out of curiosity, can you tell me a bit more about the project you're working on? I'm also doing some gas-liquid work in stirred reactors, so I'm interested in your experiences and applications!
CeesH is offline   Reply With Quote

Old   March 14, 2016, 23:28
Default
  #5
New Member
 
Filipe de Menezes
Join Date: Feb 2012
Posts: 12
Rep Power: 9
filipemt is on a distinguished road
Hi CeesH,


I am simulating the kanbara reactor, it is a desulphurization reactor in steel industry. Do you also work with metallurgical purposes?
I said in the first post that there were two phases, but it was just to simplify my question. Actually, there are three phases: water (hot metal), oil (slag) and air injection. One of my physical experiments is to study the surface contact area between air and water. So I initially inject co2 in water until saturation and then I measure the desortption by pH variation (from water to air). Am I clear?

1) I am trying to simulate the steady flow with vof model and open channel flow. To avoid overflow, I also had to use coupled pressure-velocity scheme, otherwise it was not going well. This model allows the setup of the "number of eulerian phases", but it is not the eulerian model itself. Is vof model ok in your opinion? I think eulerian could result in overflow.

2) I thought about mixture model on the transient simulation (because I read in a article). As you said, I will try vof or eulerian model.

3) Interaction>>mass>>mechanism>>constant-rate: Which unit is that?

4) I saw that is possible to specify CO2 mass fraction in inlet air, but how can I set the initial concentration of CO2 in water?

5) Pressure outlet>> species: if I dont know the CO2 mass fraction of the outflowing gas, what should I set here? I set 0 to inlet and 0,01 to outlet, just for test.

By the way, very precious your last comment, Thanks!!
filipemt is offline   Reply With Quote

Old   March 15, 2016, 00:08
Default
  #6
New Member
 
Filipe de Menezes
Join Date: Feb 2012
Posts: 12
Rep Power: 9
filipemt is on a distinguished road
Responding my question 5, ansys help says: "for pressure outlets you will set species mass fractions to be used in case of backflow".
So it is not an outflow mass fraction value, but an inflow. I will set 0, unless I have better idea.
filipemt is offline   Reply With Quote

Old   March 15, 2016, 03:59
Default
  #7
Senior Member
 
Cees Haringa
Join Date: May 2013
Location: Delft
Posts: 607
Rep Power: 13
CeesH is on a distinguished road
I'm working on aerated bioreactors; so dissolution of oxygen and venting of CO2 are among the problems I have to deal with

For your questions:

1 I am not sure what you mean with overflow, can you elaborate on that a bit? Anyway -the VOF model is advised if you have two continuous phases (such as is the case in the channel flow), or a dispersed flow where bubbles are much larger than your gridcells such that you can resolve the individual bubbles. The Eulerian model is good for dispersed flows at the large scale, where bubbles cannot be resolved. I am not sure which is best in your case; if you have a free surface flow, but a significant amount of air gets entrained, you may still need Eulerian - the bubbles you capture by entrainment likely contribute more to mass transfer than the free surface. I think the physics should be the major reason for picking VOF of E-E, not numerical considerations.

2: Mixture may be useable, but it depends on your flow patterns. As long as the gas and liquid predominantly flow in the same direction, go for it.

3: kg/m3 s

4) solution initialization> patch. There you can set the initial condition. If you want generation in your domain as well, you will either need to specify a chemical reaction, or a source term in cell zone conditions (the latter is rather artificial of course, but suffices if the generation of Co2 is time and location independent.)

5) The backflow fraction may best be based on some intuition I guess. It's always difficult to say upfront, and it may not matter than much (as long as there is no significant background). You could set it at the equilibrium value compared to the dissolved fraction or so, that's up to you.

Good luck!
CeesH is offline   Reply With Quote

Old   March 15, 2016, 22:44
Default
  #8
New Member
 
Filipe de Menezes
Join Date: Feb 2012
Posts: 12
Rep Power: 9
filipemt is on a distinguished road
Excelent answers! thank you!

About the overflow issue, I think it is a cfd beginner's problem, but I had some dificulties on simulating open channels. I used to patch the initial volumes of phases but it always diverged, like one phase volume increasing. The measures I took were setting the coupled velocity-pressure scheme; setting initial low under-relaxation factors and using open channel boundary condition. Maybe some of these measures are not necessary, but I am still investigating. I used not to solve free surfaces problems in previous works, but use degasing conditons. As I said, beginner's dificulties.

1) One question is: is patch less powerfull to convergence than open channel boundary condition? e.g.: does patch say to fluent that there are a particular level of the phase just initially, while free surface level (open channel) says it constantly?

2) My bubbles are smaller than the cells. So I should use the E-E model. The problem is I am not able to get convergence due to the issue I said. So, have you ever had this problem? What advices do you give me to simulate E-E model with free surface? I mistrust I just need set coupled p-v and maybe low initial U-R factors.

3) You said to use the patch to set the concentration of co2 in the mixture water-co2. But patch is usefull to set initial fraction of the mixture in the model and not of one specie in the mixture. Am I wrong?

Thanks in advance!
filipemt is offline   Reply With Quote

Old   March 16, 2016, 04:54
Default
  #9
Senior Member
 
Cees Haringa
Join Date: May 2013
Location: Delft
Posts: 607
Rep Power: 13
CeesH is on a distinguished road
I unfortunately have no experience with open channel flow, so I cannot help you on that front.

But, if bubble entrainment is an important phenomena, then I guess indeed you may need to go for an Euler-Euler simulation. My experiences with free surface Euler-Euler flow are eh, disappointing in terms of convergence, too. Are bubbles sparged in your domain, or entrained by surface aeration only?

Regarding patching, you can patch all basic fields; if you use a species tracking model the patching option will become available for that, too

and regarding the volume increase: the patch is of course only an initial value. So if you have an inflow or outflow, then the volume of 1 phase should increase (unless the volume fraction of the in- and outflow is exactly the same). My experience with euler-euler however shows that there are some instabilities, i.e. even if the in and outflow are 100% gas, the liquid volume is not constant (while it should be). From what I see, this mainly a problem at interfaces between cell zones in the domain. I have not yet found a reliable fix for this, but running transient instead of steady-state seems to reduce it largely.
CeesH is offline   Reply With Quote

Old   April 13, 2016, 18:17
Default
  #10
New Member
 
Filipe de Menezes
Join Date: Feb 2012
Posts: 12
Rep Power: 9
filipemt is on a distinguished road
Hello again CeesH!
Sorry for the late answer.. I was wating to come back with definitive good news of success, but they were not coming..
I think the problem was to demand too much of multiphase simulation.
At least the initial question of the topic (mass transfer) seems to be solved and I know more about my problem! Thank you for that.

The major problem now is: the problem doesnt converge when I insert the second phase. Initialy, I have only water rotating in the tank and it goes well. But when air is injected (through a surface only), it diverges after 600 iterations.
Can you give me some tips about that? I am using degasing boundary condition on top and low under-relaxation factors.
Thanks for helping!
filipemt is offline   Reply With Quote

Old   April 14, 2016, 14:42
Default
  #11
New Member
 
Join Date: May 2015
Posts: 3
Rep Power: 6
Ebimo is on a distinguished road
Hello filipemt and CeesH

I was reading your discussion and I think you guys can help me in my problem.
I am simulation a stirred tank reactor by ansys fluent 16.1. In the tank, I have a chemical reaction which create crystals. (actually crystallization happening in the tank). At the beginning, I have two species in water phase and every thing is liquid. Then, crystallization begin and I have some crystals( solid).

Based on the literature, I should use multiphase-eulerian method.
But now I am confused with defining my reaction. How can I define it? Is there any better option or template in fluent which can help me in crystallization problem better? (ACTUALLY THIS IS MY FIRST TIME THAT I WANNA USE REACTION IN FLUENT )

Thank you
Ebimo is offline   Reply With Quote

Old   April 15, 2016, 09:29
Default
  #12
New Member
 
Filipe de Menezes
Join Date: Feb 2012
Posts: 12
Rep Power: 9
filipemt is on a distinguished road
Hi Ebimo I would be glad on helping you, but I`ve never tried reactions..
Hope someone can answer you!
filipemt is offline   Reply With Quote

Old   November 15, 2019, 15:16
Default
  #13
New Member
 
HLFM
Join Date: May 2018
Posts: 1
Rep Power: 0
Hortencia is on a distinguished road
Quote:
Originally Posted by CeesH View Post
Hi Filipe,

Mixture model is a decent start, Euler-Euler 2 phase model may be more accurate - mixture is mostly good if the 2 phases are more or less co-flowing everywhere (bubble column), but not so much in situations where gas and liquid may exhibit different flow directions - which is certainly true near a stirrer.

For mass transfer, be sure to enable the species tracking option as well; otherwise you cannot distinguish between different molecular species in your air and water phases; so what you should do; make 2 species mixtures;

Mixture-liquid: dissolved-CO2 + water
Mixture-gas: CO2-gas + air (where air is basically everything that is not CO2)

Then, in mass transfer, set transfer
CO2-dissolved > CO2-gas

The default is constant rate, if you want to set up local mass transfer rates you will need to write a UDF.

Just out of curiosity, can you tell me a bit more about the project you're working on? I'm also doing some gas-liquid work in stirred reactors, so I'm interested in your experiences and applications!
hi CeesH,

I know this post is old, but if you or someone else in the forum can answer me, how do I enable the species tracking option in the fluent?

Thanks in advance for your help.
Hortencia is offline   Reply With Quote

Reply

Tags
disable equation, discrete phase, mass transfer, species transport, vof

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Difficulty In Setting Boundary Conditions Moinul Haque CFX 4 November 25, 2014 18:30
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 08:00
How to calculate Volumetric Mass transfer coefficient using CFX? tuks_123 CFX 2 July 22, 2010 02:15
Vof, udf and mass transfer panel Jay FLUENT 1 March 15, 2005 01:29
additional variable mass transfer in CFX5.6 john CFX 1 February 14, 2004 01:30


All times are GMT -4. The time now is 06:17.