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

Thermosyphon CFD calculation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 2, 2013, 04:40
Default Thermosyphon CFD calculation
  #1
New Member
 
Abhishek
Join Date: Nov 2011
Posts: 6
Rep Power: 5
abhishekchitvar is on a distinguished road
Hello Friends,

I want to model the vertical closed thermosyphon, it has three sections evaporation, adiabatic section and condenser section. The working of this device is first in evaporation section water boils as cause of heat input and the vapour phase is came into picture and then vapour flows towards condenser and latent heat of vapour gets release and water condensate come down to the evaporator section through walls and cycle continues.

I have to add the source terms to the transport equations. How to add this equation. Please find attached PNG file for equations.

Thanks in advance!
Attached Images
File Type: png Untitled.png (21.2 KB, 70 views)
abhishekchitvar is offline   Reply With Quote

Old   May 2, 2013, 05:43
Default
  #2
Senior Member
 
RicochetJ's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 291
Rep Power: 6
RicochetJ is on a distinguished road
I've read a bit about thermosyphon reboilers.

Simply adding sources and sinks to the transport equations may or may not do your problem any justice.

Also you're going to have issues with phase change in CFX (or any CFD code for that matter) if go down that route. The timesteps and computational expense required to solve a complex problem involving both condensation AND boiling will be immense.

Talk to us first abut the steps you have already done in CFX.

Additionally CFX has boiling and condensation models built in which take into consideration factors such as:
- Nucleation site density
- Quenching heat flux
- Bubble departure diameter

Also I'd be interested to know the source of the equations in your attachment.
RicochetJ is offline   Reply With Quote

Old   May 2, 2013, 06:20
Default Thermosyphon CFD calculation
  #3
New Member
 
Abhishek
Join Date: Nov 2011
Posts: 6
Rep Power: 5
abhishekchitvar is on a distinguished road
Dear Mr. RicochetJ

Many thanks for your valuable comments!

Following are the features of the problem:

It is basically multiphase simulation,

Water as continous phase and water vapour as dispersed phase

Buoyancy driven flow

Thermosyphon initially filled with water at some height i.e 0.3% water and 0.7% water vapour.

Heat transfer model is "Thermal Energry" as flow is buoyancy driven

Turbulence Model is set to none "Low Reynolds no"

Mass transfer is Interphase transfer>Phase Change

Initial and Saturation temp is defined.

Evaporator wall has Heat Flux provided.

Adibatic section "No heat Transfer"

Condenser section has Heat Transfer Coefficent applied as Boundary Condition.

As mentioned above, fractions of both the fluid as unity (0.7+0.3=1) is used.

setup of the problem is as mentioned above. But results are not acceptable.

For your kind reference I have attached the journal paper, It includes the detail equations.
Attached Images
File Type: png 1.png (27.6 KB, 45 views)
abhishekchitvar is offline   Reply With Quote

Old   May 2, 2013, 06:28
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,960
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Following on from Mr CFD's point - what are you trying to achieve with this model? If you are looking at things like flow resistance in the device then this can be modelled single phase and things get a lot easier. Alternately you might be able to use a simple mass source/sink approach if you just want to push the fluids around. Both of these approaches are much simpler than phase change. But whether they are appropriate depends on exactly what you are trying to acheive with the analysis.
ghorrocks is offline   Reply With Quote

Old   May 2, 2013, 06:43
Default Thermosyphon CFD calculation
  #5
New Member
 
Abhishek
Join Date: Nov 2011
Posts: 6
Rep Power: 5
abhishekchitvar is on a distinguished road
Dear Mr. Ghorrocks,

Thank your for your quick reply!

The objective is to find out the teperature distribution, pressure distribution and Liquid volume fraction at condenser wall.

If is there any simple approach please let me know.

Thanks in advance!
abhishekchitvar is offline   Reply With Quote

Old   May 2, 2013, 06:52
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,960
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Can you post an image of what it looks like?
ghorrocks is offline   Reply With Quote

Old   May 2, 2013, 07:02
Default Thermosyphon CFD calculation
  #7
New Member
 
Abhishek
Join Date: Nov 2011
Posts: 6
Rep Power: 5
abhishekchitvar is on a distinguished road
Please find attached picture of simple thermosyphon. It is cylinderical tube with three sections as shown in picture.

Thanking you!
Attached Images
File Type: jpg Picture2.jpg (29.7 KB, 59 views)
abhishekchitvar is offline   Reply With Quote

Old   May 2, 2013, 07:36
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,960
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The wall film is going to be very hard to model. Have a look at CFX's wall film model and see if it is suitable, I am not sure it is. If you have to explicitly model the film that will be pretty tricky to get working.
ghorrocks is offline   Reply With Quote

Old   May 2, 2013, 07:40
Default
  #9
Senior Member
 
RicochetJ's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 291
Rep Power: 6
RicochetJ is on a distinguished road
Similar work by Dr Abdelmadjid Alane has been done. He has written some papers on this topic - fairly recent papers. I suggest you read them.

Also which water material are you using? I'd recommend against using the default "Water" for this type of simulation. I suggest variable water properties such as IAPWS. In CFX pre you need to create a new material, select "Water Data,IAPWS IF97" for the material group and in material properties select your appropriate range. As IAPWS is a function of temperature and pressure the simulation will not use the Boussinesq approximation for buoyancy.

Also some analytical solutions exist for the wall film thickness. Have a look at Nusselt's formulation of film shear and thickness on a vertical flat plate to give you the sorts of orders of magnitude you expect for your simulation. HOWEVER bear in mind that those analytical solutions (and non that I know of)** don't account for the subcooling inside the liquid film.

**Adrian Bejan tries alleviate this problem by substituting the enthalpy of vaporisation in Nusselt's analysis with an augmented enthalpy of vaporisation which is now a function of the specific heat capacity and vapourside temperature difference in the condensate film layer. However this is a work around, and I'm not sure if it has been validated against experiment. Read Bejan Convective Heat Transfer for more information.

Last edited by RicochetJ; May 2, 2013 at 11:50.
RicochetJ is offline   Reply With Quote

Old   July 1, 2013, 20:41
Default What is a title of Alan's paper?
  #10
Member
 
Jeong Kim
Join Date: Feb 2010
Posts: 41
Rep Power: 7
enoch is on a distinguished road
To RiocochetJ
Could you please let me know a title of Alan's paper.
Thanks in advance.
enoch is offline   Reply With Quote

Old   July 2, 2013, 05:03
Default
  #11
Senior Member
 
RicochetJ's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 291
Rep Power: 6
RicochetJ is on a distinguished road
Quote:
Originally Posted by enoch View Post
To RiocochetJ
Could you please let me know a title of Alan's paper.
Thanks in advance.
Sure.
Paper 1. http://library.witpress.com/pages/pa...?paperid=16590

Paper 2. http://www.sciencedirect.com/science...63876211000451

There are a few others which I can't find right now. Do a key word search of the authors and you should find the other papers.
RicochetJ is offline   Reply With Quote

Old   December 16, 2013, 14:27
Default Closed loop thermosyphon
  #12
New Member
 
-Non-US-
Join Date: Dec 2013
Posts: 3
Rep Power: 3
rudolfkhalil is on a distinguished road
Hello!!
I am modeling the exact same model on gambit then simulate it on fluent.
i am finding abit of difficulties concerning some parameters and how to set boundarylayer multiphase and patching the solution....

can anyone help me?

Thank you

Quote:
Originally Posted by abhishekchitvar View Post
Hello Friends,

I want to model the vertical closed thermosyphon, it has three sections evaporation, adiabatic section and condenser section. The working of this device is first in evaporation section water boils as cause of heat input and the vapour phase is came into picture and then vapour flows towards condenser and latent heat of vapour gets release and water condensate come down to the evaporator section through walls and cycle continues.

I have to add the source terms to the transport equations. How to add this equation. Please find attached PNG file for equations.

Thanks in advance!
rudolfkhalil is offline   Reply With Quote

Old   December 16, 2013, 17:16
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,960
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Try the fluent forum.
ghorrocks is offline   Reply With Quote

Old   September 4, 2014, 20:06
Default volume fraction
  #14
Member
 
Muhammed Asmail
Join Date: Nov 2009
Location: Iraq
Posts: 36
Rep Power: 7
Muhammed_iraq is on a distinguished road
Hi all

what is the boundary condition of volume fraction in thrermosyphon by using ANSYS-FLUENT program? the path of the boundary conditions in this program?

Many Thanks
Muhammed_iraq is offline   Reply With Quote

Old   September 11, 2014, 16:23
Default
  #15
Member
 
Muhammed Asmail
Join Date: Nov 2009
Location: Iraq
Posts: 36
Rep Power: 7
Muhammed_iraq is on a distinguished road
Quote:
Originally Posted by abhishekchitvar View Post
Hello Friends,

I want to model the vertical closed thermosyphon, it has three sections evaporation, adiabatic section and condenser section. The working of this device is first in evaporation section water boils as cause of heat input and the vapour phase is came into picture and then vapour flows towards condenser and latent heat of vapour gets release and water condensate come down to the evaporator section through walls and cycle continues.

I have to add the source terms to the transport equations. How to add this equation. Please find attached PNG file for equations.

Thanks in advance!
Dear abhishekchitvar

How are you?
did you reach to solve heat and mass transfer equations by using UDF in ANSYS-FLUENT program?

Please also i need solution of these equations
Many Thanks
Muhammed_iraq is offline   Reply With Quote

Old   November 4, 2014, 17:11
Default
  #16
New Member
 
Xiaobing Zhang
Join Date: Apr 2014
Posts: 11
Rep Power: 3
xiaobingwill is on a distinguished road
Hello,

Did you solve this simulation? I'm dong similar simulation in FLUENT. But cannot see condensation after long time of calculation. Can you share your results and ways to simulate this problem?

Many thanks

Quote:
Originally Posted by abhishekchitvar View Post
Hello Friends,

I want to model the vertical closed thermosyphon, it has three sections evaporation, adiabatic section and condenser section. The working of this device is first in evaporation section water boils as cause of heat input and the vapour phase is came into picture and then vapour flows towards condenser and latent heat of vapour gets release and water condensate come down to the evaporator section through walls and cycle continues.

I have to add the source terms to the transport equations. How to add this equation. Please find attached PNG file for equations.

Thanks in advance!
xiaobingwill is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Entropy calculation using CFD MJK Main CFD Forum 5 May 12, 2003 02:33
STAR-Works : Mainstream CAD with CFD CD adapco Group Marketing CD-adapco 0 February 13, 2002 13:23
CFD for fans & blower housings David Carroll Main CFD Forum 8 August 24, 2000 17:25
PC vs. Workstation Tim Franke Main CFD Forum 5 September 29, 1999 15:01
Which is better to develop in-house CFD code or to buy a available CFD package. Tareq Al-shaalan Main CFD Forum 10 June 12, 1999 23:27


All times are GMT -4. The time now is 08:38.