Providing 0 mass fraction in vaccum condition

Member
in Fluids

Hello

I am trying to model flow of mixture of air and water vapor where vapor is pulled out into a vaccum domain

I want to provide an initial condition where mass fraction of vapor and air in the domain is 0 because the domain is in vaccum condition intially.

Fluent does not allow me to do this as sum of mas fractions of vapor and air in the domain should be 1. Is there any way i could assign this vaccum condition initially?

edited May 12

Have you used the patch option?

• Member
edited May 27

Yes, however the problem is fluent says sum of mass fraction of species should be 1 in the domain

edited May 27

You will not be able to define a real vacuum in Fluent. Fluent solves the NS equation assuming fluid continuity. Because the pressure is really low in a true vacuum, the fluid continuum assumption would break in such conditions. You have to have one of the materials defined in your cell zone at reduced pressure.

Is this does not agree well with your analysis, could you please elaborate on what you are modeling? Perhaps, we might be able to suggest an alternate approach.

Best,

Karthik

• Member

Hi Karthik

I am trying to model the evaporation and condensation process in vacuum. I want to understand what will be the velocity acceleration in the channel due to vacuum .

The geometry is a vertical rectangular channel with water vapor entering left hand side of channel at 0.5L/min and 70C which needs to evaporate depending on specific sat temperature and then condenses on other side of wall that is maintained at 50C. Fluent uses Lee condensation model and I dont know what should be the value of evaporation and condensation frequencies under vacuum conditions.

Also when I calculated Knudsen number for my channel pressure and dimension conditions, Kn was less than 0.01 which means continuity still holds . What do you think on this ?

• UKForum Coordinator

That sounds like a low pressure system rather than vacuum otherwise you'd not get any condensation. If Kn is in the continuity range it can't be a vacuum. Are you looking at freeze driers?

• GermanyForum Coordinator

In Fluent you can model near vacuum conditions or low slip region where the Knudsen number lies in the transition regime. Real vaccum cannot be solved with continuum equations used by Fluent for almost 99% of the cases.

If Kn << 0.01 then you might use NS equations. REgarding the frequencies you need to tune them to match experimental data or correlations. By the way you should rather write your own model for phase change or at least couple the saturation temperature of the Lee Model to "partial" pressure to have something consistent.

• Member

I am trying to model desalintaion process in vacuum. I have no idea on how to couple the Lee model sat temperature with vapor pressure.

Do you have any resources which guides on how to do this?

Is there any test cases which shows velocity or evaporation or condensation rate under vacuum conditions for any configuration and B.Cs? I would like to validate my simulation results (either velocity or condensation /evaporation rate) with a test case that has already been experimentally validated

• GermanyForum Coordinator

Can you explain the desalination process: which phases are involved and which components in the phases are involved?

• Member

Here is the process that I want to simulate

The feed solution is liquid water that is at high temperature say 80C. The region with lines next to the feed solution is a membrane that allows only water vapor to pass through it and not any other components like salts. The coolant on right hand side is maintained at cool temperature say 30C. The black region marked as polymer film is something similar to a copper plate. Due to difference in vapor pressure between feed and coolant streams, evaporation occurs at interface between membrane and feed solution. The white region in the middle is maintained at a vacuum (10000Pa absolute pressure) pressure using vacuum pump. Since vapor pressure due to evaporation process at membrane interface is high and there is vacuum in middle, the vapor would travel at high velocity towards the copper plate and condense.

For my current CFD model, I am trying to model only the middle region consisting of empty vacuum region, without the membrane on the left and instead and a copper plate on the right . I have given image of my computation geometry below

So I want to find 3 things from my simulation

1) Rate of condensation of vapor

2)Velocity magnitudes of vapor and velocity

Could you guide me in following aspects?

1) Which multiphase model should I consider for this scenario? (Eulerian homogeneous mixture or Eulerian inhomogeneous model or Eulerian VOF model)

2) How to model evaporation and condensation happening at vacuum ? Do I use the Lee evap/cond model with default coefficients (as I dont have values of these coefficients in real time at vacuum)? I dont have any UDF to define mass transfer as this is what I need to find from CFD

3) What should be the order of magnitude of velocity that I can expect from the simulation ?

4)Do you have any validation test cases from fluent that give evaporation/condensation rate /velocity in similar conditions ?

• UKForum Coordinator

You probably want to add the vapour using a source term, they're covered in the manuals. Remember to check heat & momentum sources at the same location. If the system is 10k Pa it's not a vacuum, it's just a lower pressure: you will need to check the Knudsen Number though to confirm the continuity equations are still valid.

Velocity will depend on the system. I'd expect it to be relatively low, simply because membranes tend to be quiet and desalination plants aren't usually high throughput systems.

If there aren't any examples in the Help system or on ansys.com (look in the Blogs) then we don't have anything we can share. There are references with most of the models so you can use those as a starting point for your literature review.

Re the mass transfer, you need to define conditions to then model the rate. Ie the relationships need to be provided, the solver will than calculate the conditions and rate of mass transfer. It's not a "magic box". Have a look at the options, but I suspect you want the Eulerian model, read the sections in the manual (User's and Theory) on multiphase and phase change.

• Member

Hello Bob

I have now built a simulation model of above geometry using ANSYS CFX Wall condensation model. The problem is the velocity values ,contours and the pressure values/contours dont make much sense to me. Could you help me understand if there is anything wrong I am doing with CFX wall condensation model and why I am getting these contours

The temperature values decrease gradually as expected and all residuals converge to 1E-04

The geometry is same as before with similar dimensions. The depth is 0.25mm. The Boundary conditions are as follows

Inlet mixture is a variable composition mixture of air and water vapor. Another mixture is homogeneous composition of water (liquid) and vapor. Saturation pressure is determined based on Anotinne equation. Condensation wall model is enabled on wall with 55C. Other walls are adiabatic except inlet and outlet. The only notice I get during the solution is " A wall has been placed at portion(s) of an INLET         |

| boundary condition (at 91.7% of the faces, 91.7% of the area)  |

| to prevent fluid from flowing out of the domain.         |

| The boundary condition name is: Inlet.              |

| The fluid name is: Fluid 1.                    |

| If this situation persists, consider switching          |

| to an Opening type boundary condition instead.          |"

On observing the velocity contours vectors, I see that most of flow at the inlet face of the geomerty from the top to somewhere near the bottom is directed in a downward vertical direction due to the pressure gradient difference between inlet and outlet. Only some part of the fluid at the bottom face of inlet moves normal towards the other wall resulting in condensation but very small amounts as shown below

• Member

Hi

Is there an option in CFX to provide an outlet B.C for the above geomtry such that only the fluid condensed out from the vapor leaves the domain while the vapor still remains inside the channel?