Modeling of Salt Separator
 

Hi everyone,
I'm using Ansys CFX 14.5 to model a salt-separator. I modelled water as a continuous fluid and the salt as "particle transport solid". Is there any way I can define a particle injection zone depending on the salt concentration in the water and more important, the temperature? I need to include the solubility in order to be able to know where the solid-salt particles need to be injected.
Or is there any other/better way to model a solution with salt/water accounting for dissolving and precipitation?

I would appreciate any help! Thanks
Stephan

Is the salt present as solid particles? If so then the model you selected is probably OK. Or is the salt dissolved in the water? If this is the case then you have not selected the correct physical model - in this case you should either use an additional variable to rack the salt, or use a multi-component mixture.

If the salt is both dissolved and present as particles then you have a multiphase and multicomponent simulation and things are getting complex.

Also note that you can model particles as lagrangian particles or as a eularian model.

HI
The salt separator is a multiphase and multicomponent problem in reality. But i assumed that the dissolved salt in the water is not important for my problem, since the concentration of the salt in the water is very low and has marginal impact on the flow of the stream. Therefore I'm trying to implement the salt only in its solid phase (as spheres). The problem is the particles should "magically" appear at locations depending on their solubility-temperature (on the isothermal of the solubility Temp. of the water). And I don't know yet how i can implement this in the "particle injection region" settings in CFX. Is there a way to detect the first solubility-Temperature-isothermal and set that location as the "injection region" for the salt particles?
greetings
Stephan

You might need to use a user fortran particle source for this.

But before you do - is Lagrangian particle tracking the best model for this? Would a Eularian particle model be better? You can easily seed particles anywhere with a Eularian model. Have a read of the documentation on the choice between Eularian and Lagrangian approaches, or if you give more detail on what you are modelling we can help you choose.

Thanks for the quick response!

I'm simulating a dip-tube salt separator where a superheated water/salt solution enters the device. As the solution cools down in the dip-tube, salt separates and due to the higher density settle down to the salt-brine exit. The remaining part of the feed reverses its flow direction and leaves the separator at the top (hopefully only water :)).

I probably need a Lagrangian approach since I am interested in tracking the path of the solid salt particles. The particle trajectories and deposition locations are the goal of the simulation.

Yesterday I had the idea of using the "reaction" option in CFX for a simplified dissolving-reaction of the salt: Salt_fluid -> Salt_solid.
I could implement a fluid phase of the salt with the density of water and let this particles react to their solid phase. I can choose the activation temperature and use a Arrhenius approach with negative heat release to model my reaction. Do you think that would work? Or do you have a better approach?

Thank you very much for your support!

You can use streamlines of the particle volume fraction velocity field to track representative particles in the Eularian approach as well.

The reaction model you describe is designed for chemical reactions, not phase change so I am a little concerned about using it for something it was not intended for. But if you think it might work then give it a go. But make sure you look at all the interphase mass transfer stuff which comes with CFX's multiphase model before you use a different model.

3 phase mixture model 0.5 Molar NaCl aqueous solution
 

https://drive.google.com/file/d/11rS...ew?usp=sharing
I need some help regarding the modeling of 0.5 Molar NaCl aqueous solution. I am using a 3 phase mixture model (nacl solution, water vaour and air). the problem is that i have a 2D cylinder and there is a membrane in the center which is modeled as a porous media jump .. now i want that only water vapour should pass through the membrane and the salt should be removed and rejected and should not pass through the membrane.

waiting for your helpful response.

First of all, let's get the basic physics right. If you are dealing with an NaCl aqueous solution then this is a single phase model. If the air interface is important as well it is a multiphase model, but only two phases (liquid and gas).

The NaCl should be modelled as an additional variable (if you are trying to be simple) or a multicomponent mixture (if you are trying to be accurate).

Yes Sir, I only need to deal with NACL solution... i want water to b evaporated from nacl solution and only collect vapour...

I wa unable to make a mixture of Nacl and water so i make a new fluid and changed its properties to that of NACL Solution...

what should i do ?

It would probably be worthwhile considering the purpose of what you are doing and looking at the basic approach to achieve the purpose.

Can you explain what you are doing and why you are modelling this? Please include an image of it, and the important physics you want to model.

I am using this apparatus.. NaCl solution will enter from the feed inlet ar 333K with mass flow rate of 2lpm and at the membrane surface i want water to b evaporated and only water vapor should pass from the membrane so on the permeate side i should only have pure water. The feed outlet is set to pressure outlet (atmospheric pressure) and the permeate outlet is also set to pressure outlet with vacuum pressure of 5.5KPa.

I want to calculate the Temperature Tfm (temp. in the feed side surface of the membrane) which I'll use to calculate the saturation pressure and partial pressure of water.

What should i do that only water vapour should pass from the membrane and NO salt water should pass?
Note: I am doing it in a 2D case not for 3D as shown in the image.

Image Link: https://drive.google.com/file/d/11rS...ew?usp=sharing

https://drive.google.com/file/d/11rS...ew?usp=sharing

If you are looking for the temperature at the membrane - isn't that a hand calculation with the heat of vapourisation working against thermal conduction? (probably with a bit of advection too)

But if you want to do this as CFD - it sounds like the air side plays little role in heat transfer so it can be ignored. This is very useful because this makes the simulation single phase. You then replace the membrane with source terms which gobbles up water but leaves the NaCl and uses a heat source to model the latent heat effects. You will have to think about how the source term works because by default mass sinks gobble up the additional variable (modelling the NaCl) along with the fluid.

You might also be able to do this using a porous material for the membrane with an outlet at the air face of the membrane. You then use a source term on the additional variable to set the NaCl in the membrane porous material to zero but puts the removed NaCl back into the simulation on the fluid side of the membrane. On second thoughts I suspect this is an easier and more physically correct approach.