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

Liquid Water Free Surface Evaporation

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 31, 2015, 10:59
Default
  #21
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 14
JuPa is on a distinguished road
Quote:
Originally Posted by davide View Post
Hi everyone,

I do have the same problem (evaporation from a free-surface) which I would like to solve with CFX. This is a simple problem of a 2D domain with the domain occupied by water and air (water and air are separated with a clear interface). The water and air never mix, so the homogeneous free-surface model is enough. The interface will move due to evaporation (and mass conservation).

Please note I'm interested in CFD modeling of this problem not analytic solutions. I highly appreciate if anyone can let me know if they have ever solved this with CFX or are aware of any paper/article/video/tutorial that explains how to solve this with CFX.

Thanks :-)
This is quite wrong - you will need to use the inhomogeneous approach:
- Inhomogeneous momentum to allow the phases to separate during evaporation.
- Inhomogeneous energy for both phases to allow each phase to have its own temperature fields in order to correctly model evaporation
- You can get away with homogeneous turbulence

The particle and free surface models aren't sufficient in their formulation for the interfacial area density to model evaporation from the free surface. This means you'll need to go the mixture model route. What does this mean:
1. You need to specify the interfacial length scale (I should have a paper out soon documenting how to get the appropriate length scale for the mixture model in evaporation problems)
2. You need to specify the interfacial drag. The default is 0.44 - however this is for droplets and not a free surface.

And lastly, because you'll be using the mixture model you'll need to have two continuous phases (or in your case three!). Water, and water vapour and air above the free surface.

Essentially you're solving 3 sets of momentum equations (one set for each material), 2 sets of energy equations (assume the vapour is at Tsat and you don't need to solve the energy equation for vapour), the continuity and volume fraction equations, and your turbulence equations.

Basically, what you're after isn't easy.
JuPa is offline   Reply With Quote

Old   March 31, 2015, 12:36
Default
  #22
New Member
 
Join Date: Jan 2011
Posts: 5
Rep Power: 15
davide is on a distinguished road
Ricochet,

This is an interesting view. I understood all your points except the one that you said "Inhomogeneous momentum to allow the phases to separate during evaporation.". Can you please elaborate? Basically, I have water and vapor (lets's just say we have only two phases) which are separated by an interface (I use this as an initial condition). Then, I run the case, and ideally, the interface should move due to the conservation of mass.

btw, I did run some simulation with homogeneous approach and captured the interface movement (I am still working on it to make sure it is accurate).

Thanks
davide is offline   Reply With Quote

Old   April 1, 2015, 06:10
Default
  #23
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 14
JuPa is on a distinguished road
Quote:
Originally Posted by davide View Post
"Inhomogeneous momentum to allow the phases to separate during evaporation.". Can you please elaborate?
There is a sudden change of phase from water to vapour at the free surface. Well, it turns out the homogeneous momentum approach cannot model this correctly. If you do this homogeneously, significant mass of water gets "carried away" above the free surface. This is a physically unrealistic result since water is more dense than vapour and should just "fall back down".

You need an inhomogeneous approach to momentum to allow the two phases to "slip" past each other. You control the amount of slip via the drag coefficient.

Hint: look at the density ratio of water to vapour at your operating pressure. It's in the order of 1000s. Do you expect a homogeneous momentum approach will successfully model a sudden change in density from 998 kg/m^3 to 0.1 kg/m^3?
JuPa is offline   Reply With Quote

Old   May 19, 2016, 03:19
Default
  #24
New Member
 
Hilde
Join Date: May 2014
Location: Copenhagen, Denmark
Posts: 18
Rep Power: 11
hilde is on a distinguished road
Quote:
Originally Posted by JuPa View Post
1. You need to specify the interfacial length scale (I should have a paper out soon documenting how to get the appropriate length scale for the mixture model in evaporation problems)
This sounds extremely interesting. Could you please tell me when the paper is available? (or provide me with a title in order to set up a scholar alarm on it)

Thanks in advance
hilde is offline   Reply With Quote

Old   June 1, 2016, 04:53
Question related to fluent
  #25
New Member
 
Moscow
Join Date: Dec 2013
Posts: 4
Rep Power: 0
sawa25 is on a distinguished road
Quote:
Originally Posted by JuPa View Post
You need an inhomogeneous approach to momentum to allow the two phases to "slip" past each other. You control the amount of slip via the drag coefficient.
Can you please clarify, what mean inhomogeneous approach related to Fluent case setup. I model evaporation from free water surface in usual room conditions and need any information, how to do it.
sawa25 is offline   Reply With Quote

Reply

Tags
evaporation, free surface

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
Free water jet impinging hot solid surface, including boiling hamdy Fluent UDF and Scheme Programming 5 August 19, 2012 19:52
Can Flow-3D plot the free surface area in Iso-surface or colour variable? therockyy FLOW-3D 1 June 20, 2010 19:36
Patch type for free surface of liquid shchepan OpenFOAM Running, Solving & CFD 0 June 8, 2010 09:54
open channel problem (free surface) Andy Chen FLUENT 4 July 10, 2009 01:20
uptodate water distribution network fredius,magige,tanzanian,(e.a) Main CFD Forum 0 January 27, 2002 07:10


All times are GMT -4. The time now is 20:00.