Multicomponent DPM injection
Could anyone give me some information about DPM "multicomponent" injetcions.
I have a liquid (water) and solids (Coal) which are suspended in the liquid. The mixture is then sprayed and water evaporates from the suspended coal particles leaving behind only solid coal particles. Can i use "multicomponent" DPM injection in this case? or Multiocomponent injection can only be used for single phases, not solid and liquid.
In DPM model You can spray only liquid-liquid mixture. But there is simple way to cheat Fluent. You can easily copy properties of Coal from fluent materials library and create new liquid with properties of coal. But to evaporate water in multicomponent droplet model You need to include UDF with mass transfer equitations.
Thank you Jaskull
yes you are right but at first, I wanted to inject (spray) mixture of Soild particles and liquid (solid suspension in liquid). perhaps, that is not possible by FLUENT's in built functions. Probably some UDF may help.
As you recommended, the new liquid with properties of coal will actually be SOLID (like solid suspension)? For instance, I will cheat fluent by changing all the properties of liquid into the properties of solid coal particles, such as the bounday condtion called "reflect" will be used instead of trap etc (which is used for liquid bubble) with co-efficient of restitution=0.9. Also the density of Solid coal=1400kg/m3 (solid coal density) would be used instead of liquid density which must be lower than the solid. Hence, now it means the liquid is no longer liquid but a SOLID coal particle which is being sprayed. Right?
I'm sorry about those 2 days of silents but I was abroad.
You are right. In the same way I simulate spray drying of detergent. Now I'm preparing some changes into evaporation model. Default Fluent calculating evaporating process in first drying period all the time without internal resistance of the particles. I want to reduce the speed of evaporation of water during solidification of participles. In Your case, if I good understand, You have suspension so everything what stay after evaporation is already solid so You are drying in first period all the time.
My work is almost similar to your work.
I am simulating the drying of a solution containing liquid coal. The Liquid coal will become solid during spray drying and the solvent will evaporate.
However, to make things simpler, at first, i tried to simulate the suspensions rather than solution. Hence, as you said, whatever will be left after evaporation would be solid, so I will be drying in the first period all the time rather than the second period which includes the creation of solid crust over the surface of the particle and diffusion of vapors from the pores inside crust containing liquid.
For complete drying kinetics, papers written by M.Mezhericher, A. Levy and I. Border (2006-2010) are helpful as they explained clearly the droplet drying phenomenon and the numerical procedure. But to implement the numerical procedure in FLUENT seems to be very tough.
You're right our problems are almost similar. I know PhD Mezhericher and prof. Border personally. I met them in Finland on Nordic Drying Conference in April. I showed then results of simulations of dust explosions during spray drying. They have very interesting presentation, but their way looks rather complicated. In my simulations I use the method proposed by prof. Mujumdar and my supervisor prof Zbiciński. Tomorrow I will send you title of interesting article You will find it on web easily.
Now I starting write UDF to describe process of droplet agglomeration. Wish me a luck.
Droplet agglomeration is also a very interesting phenomenon for simulation. I wish you Good Luck.
Could you send me the title or paper on my email address:
I am prasad, from india doing Phd. im also working in the same area, spray dryer simulation. I have started working on this problem since 4 months. I have some doubts in spray dryer simulation. will you mail me to my mail ID. email@example.com.
Help me guys
I have a similar problem regarding my work
I will explain it in a few lines.
I have to simulate a very concentrated Brine solution entering in a tank where it is superheated to 410 degrees C and here the salt is separated since the water turns into water vapor. The vapor then just exits from the outlet at the top and the salt is deposited at the bottom.
My questions are
Can i use the idea that you suggested to Mohsin about fooling FLuent and creating a NaCl material using the properties of salt found online?
2) Can i use DPM for this or which other model will be best for this type of a problem
3) I will need to make sure the salt is dissolved in the water at the inlet. So can i do this using Species transport?
4) What about the actual evaporation process taking place? I need help with the UDF for the evaporation or is there any other way around it?
Please guys I am desperate. I really need help or else i am looking at another year wasted.
Donít worry, you have to study a little bit to solve your problem.
1. Firstly, you have to know what is the difference between Eulerian and Eulerian-Lagrangian approach. DPM model uses Eulerian-Lagrangian approach. This approach gives you the particle trajectory, residence time etc. This approach is suitable for dilute phases which means If volume fraction of your salt solution is less than 10-12 % of the total volume then this approach will give better results. I think, in your case DPM model is suitable. (also, you can read some research papers on what others are doing on this problem).
2. You have to use FLUENT "multi-component particle model" present in DPM. The first component being water and the other will be Nacl. But the fluent data base for multi-component mixture contains only liquid materials. So, you will fool fluent to make your Nacl as solid. You just will select 1 liquid material and change itís properties to solid.
3. You will have to use UDF because fluent cannot solve multi-component evaporation. Fortunately, it has given a code for this. You have to implement that code in FLUENT in order to solve the multi-component evaporation. This is the code:
4. Species transport will obviously be used.
Thank you sir
Thanks a lot for your help Mohsin,
I have been trying on the same lines and will implant the UDF as you suggested. But for another experiment,I have another model in which the brine solution is 25% so DPM won't work.
Also, in that method the salt is extracted through precipitation using the phenomenon of water losing its polarity after reaching a supercritical temperature of around 410 degree Celsius. And since there a pressure of around 3200 psi there wl not be any phase change in that model (thank god). But the issue over there is how do I make salt precipitate from water? Is there a way in which we can change the solubility of salt in water? Does fluent have solubility consideration?
I am not gonna ask you about the polarity because even I am pretty sure fluent doesn't have any provisions to add polarity as part of the fluids property.
In this case what is my best option?? I want the salt to separate out at temperatures around 410 (the brine solution inlet temp is 370 at which it is still a solution since water is polar at that temperature)
Any help regarding this will be a godsend.
So in short I want to know what to do in the case of the brine solution at 25% ratio.
Also whether there is a way to add solubility in fluent.
And whether fluent has a precipitation model that I could use.
Or can I use the temperature to somehow make the salt to separate out from water. Can I use a condensation model for this? I mean assume salt is liquid in the solution but at a certain temperature it condenses into solid? I know it sounds crazy since the temperature is increasing!but I meant to create fake precipitation process.
I am Saurabh from India and I have a similar problem. I want to use fluent to model a spray dryer in which brine is dried using hot air.
I am able to model the evaporation of pure water droplet but for the case of saline water droplet salinity will play an important role in drying kinetics. As I am new to fluent and have no experience with UDF could you please help me with this.
I am not quite confident in this area as of now so you might wanna create a new thread and ask this question. I can send you a message that I got from ansys tech support.
Hope that helps you in your work. I am completely engrossed in the heat transfer aspect of the work. I was trying to heat the water using heat flux but for a week couldn't get it. Turns out that was happening because of the 2 d drawing!!! And I used to think 2 d drawings should be used instead of 3d ones!
Anyway I tried a simple problem and got better heating results as per the
Q=m Cp dt. But work still going on..
Will try to get back once I start with multi component modeling.
Here is the Thread
@ SAURABH K
What is your simulation purpose? Do your want to know the precipitated salt concentration in a tank? If you want to know the concentration distribution of dissolved and precipitated salt distribution, you need to use our multiphase multispecies model. You need to define two phases.
Liquid phase: which is a mixture including water and dissolved salt species
Solid phase: precipitated solid salt.
We do not have any precipitation model in the code, as a user, you will have to find out a correlation about precipitation rate in a function of temperature or other variables and implement the model using a user defined function (UDF). The udf is used to consider the mass transfer between two phases. Maybe the most straightforward method is to treat precipitation as a heterogeneous reaction:
NaCl (liquid)--> NaCl (solid)
and use DEFINE_HET_RXN_RATE udf to implement the precipitation reaction rate. In the udf, you can implement the solubility and other info.
I hope this helps.
Thanks Abhijeet Shrawage
Thanks Abhijeet Shrawage for your reply.
Actually what I want to find out is what amount of salt will be precipitated inside the spray dryer? What will be the wall deposition? & what will be the temperature and humidity profile inside the spray dryer?
As of now, I am able to find out temperature and humidity profile inside the spray dryer for two cases: (i) when there is no spray (ii) when pure water is injected into the spray dryer.
Now I want to model for third case where there will a brine solution will be injected. As the drying will take place salinity inside the droplet will increase till it reaches the saturation value. After that salinity will remain constant as precipitation of salt will be taking place. In fluent the evaporation model is only for first drying stage. I need to model for second drying stage where there will be precipitation along with evaporation. Also for the case of first drying stage my saturation pressure will be lowered due to increased salinity. Thus I need to write a UDF for the same. But as I am new to fluent I have no experience with UDF.
So I wanted to ask if anyone has done this type of problem before.
I am a new member. Nice to joint in our forum!
I'm PhD student in Germany. I am going to simulate spray drying (material is multicomponent which contains sensitive ingredients in co-current prayer) in fluent. Because the model is more complicated than default model so I must use UDFs. I have already set up and run gas phase without droplet and run with multicomponent droplet as tutorial 17. However, when I try with DPM_HEAT_MASS example (in 2.5.5 of udf manual) as Mohsin talked above, it does not work: TP_N_COMPONENTS(p):structure reference not implemented; P_CELL_THREAD(p): undeclared variable, etc...
If you have any comment, please show me!
Thank you a lot,
I see that not only me and Mohsin working on spray drying simulations. I'm chemicals process engineer, now PhD student from Poland. I spend last six month preparing simulations of multicomponent spray drying and I have a few steps behind me. So if anyone has any questions let them write to my email (firstname.lastname@example.org). Maybe I can help.
Do you compiled your UDF to .dll library using virtual studio or just interpreted? Without compiling UDF won't work if you use the internal functions of FLUENT.
I have a question: Is the simulation of spray drying are the subject of your PhD? Germany is quite close to the Poland so maybe we can make some kind of cooperation?
Thank you for your reply. That's right, my topic is spray drying and now I try to simulate again PhD Mezhericher and prof. Border' model. However, Fluent is not easy to use!
I have intepreted the example (is this wrong???) and have not compiled yet. What is my mistake, please give me your advice?
I am PhD student at Otto von Guericke university, Magdeburg. I will be gleeful if I have chance to cooperate with you.
I think Maciej is well educated in multi-component simulations. I would just like to add some comments regarding your case.
1. You have to compile the UDF (multi-component vaporization) and then load it into your case file (not interpret).
2. The udf given is used for serial processing so please use serial processing (not parallel processing) for the UDF in question.
3. If you copy this UDF in notepad.c extension, then there comes some syntax errors which remains uncopied. This syntax error causes the FLUENT to give error when you "build". Please check the syntax thoroughly before use.
4. If nothing is working and you get the same problem. then, write back here.
P.S. This UDF gives linear evaporation rate i-e constant rate drying. It is unable to provide the drying for falling rate period. I would like to ask Maciej to put some light into how to simulate falling rate period. Thanks
|All times are GMT -4. The time now is 19:45.|