Thermosyphon CFD calculation
1 Attachment(s)
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!:) 
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. 
Thermosyphon CFD calculation
1 Attachment(s)
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. 
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.

Thermosyphon CFD calculation
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!:) 
Can you post an image of what it looks like?

Thermosyphon CFD calculation
1 Attachment(s)
Please find attached picture of simple thermosyphon. It is cylinderical tube with three sections as shown in picture.
Thanking you!:) 
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.

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. 
What is a title of Alan's paper?
To RiocochetJ
Could you please let me know a title of Alan's paper. Thanks in advance. 
Quote:
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. 
Closed loop thermosyphon
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:

Try the fluent forum.

volume fraction
Hi all
what is the boundary condition of volume fraction in thrermosyphon by using ANSYSFLUENT program? the path of the boundary conditions in this program? Many Thanks 
Quote:
How are you? did you reach to solve heat and mass transfer equations by using UDF in ANSYSFLUENT program? Please also i need solution of these equations Many Thanks 
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:

All times are GMT 4. The time now is 06:03. 