evaporation-condensation model: 2D simulation of thermosyphon (closed-domain)

Hello

I'm using ANSYS Fluent 2019R1 to model a 2d thermosyphon (closed-domain). I'm planning to simulate simultaneous evaporation (of water) and condensation (of vapor) inside this 2d tube. I have the case setup and running without any problems.

However, I have a few questions regarding general procedure and Lee's model implementation in Fluent as the theory guide section dedicated to the Lee's model doesn't answer my question. The geometry and initial condition of water phase volume fraction is as follow:

  • Operating pressure location and reference pressure location

Due to the fact that the domain is closed, non of the boundaries fixes a value for pressure and thus a reference pressure level needs to be set. I have set the operating pressure location to (0, 0.2m). However when I initialize the simulation the following TUI command doesn't return any value and I can't check the actual location of the reference pressure:

define -> operating-conditions -> used-ref-pressure-location

Does fluent use reference pressure for this kind of simulations?

 

  • Lee's evaporation and condensation model

The theory guide section only describes the volume fraction formulation and its corresponding source term when the model is used. How the pressure and energy equations are modified when Lee's model is used? Do they include source terms due the mass transfer and latent heat during evaporation-condensation? It would be really helpful if you modify the theory guide section and provide both the modified pressure and energy equations.

 

Regards,

 

 

Comments

  • dp1106dp1106 Member
    edited May 2019

     Hello, 

             When you use the Lee model what do you define as the primary and the secondary phase? I believe the reference pressure location can be set through the operating conditions dialog box in Fluent. Do you see any of the condensation and evaporation occurring?

    Regards,

    DP

  • shadowfaxshadowfax Member
    edited May 2019

    thank you for the reply.

    The primary phase is water vapor and the secondary phase is liquid water. (As recommended in the user guide)

    Yes, I know the location can be set through the Operating condition dialog box. But in the following link, it is stated that you can check the actual reference pressure location being used by executing above mentioned TUI command.

    Actual Reference Pressure Location

    Since this command doesn't return anything, my advisor told me to check whether ANSYS fluent is actually setting a reference or not.

     

    Well I can see evaporation and condensation happening inside the tube. I just need more information to complete my thesis as requested by my advisor.

     

    Regards,

  • dp1106dp1106 Member
    edited May 2019

    Thanks! The Lee model is a kind of black box in terms of defining the mass source and the energy source terms in the conservation equations since not much information is provided in the theory guide. I presume you already have finished your simulations, therefore I won't recommend now to use UDF. The UDF subroutine can handle the source terms in a more convenient manner than the Lee model. Since you observe both evaporation and condensation you can presume that the source terms are implemented correctly. 

    Regarding the primary phase and the secondary phase in Lee model, I knew that liquid phase should be defined as a primary phase and vapor phase as a secondary phase in order to observe condensation (based on my experience and related posts in CFD online forum). People have reported not to observe condensation while using vapor phase as a primary phase although the evaporation does appear.

    Have you faced a similar situation like this before? Where in the user guide do you see the recommendation of having a vapor phase as the primary phase and liquid phase as a secondary phase. I would be grateful if you can kindly shed some views on this matter.

     

    Regards

  • shadowfaxshadowfax Member
    edited May 2019

    Well I'm now at validation level and I'm yet to finish my thesis but I need to gather basic information regarding how Fluent is handling my simulation.

    You mean that there is a UDF that can handle these type of simulation or I need to write one by myself?

     

    I haven't noticed that but I think in order to see condensation, one needs to use condensation coefficient which is several magnitude higher than evaporation coefficient. e.g. (coeffE = 0.1 and coeffC=1000)

     

    Regarding primary and secondary phase there is no rule of thumb but only recommendations:

    1- How to chose primary or secondary phase

    2- I remember to read in one of the ANSYS Fluent tutorials about setting the denser phase the secondary phase for better accuracy as the the volume fraction equation is not going to be solved for the primary phase.

     

    Regards

  • dp1106dp1106 Member
    edited May 2019

     Hello,

              Sorry for the delay in reply. Yes, you need to write an UDF that can handle the mass and energy transfers. However, you can get few UDF's code in the internet which I believe are correct although those are written for water-vapor to be primary phase and the water-liquid to be secondary phase. If you don't find one I can share it.

    Regarding the question you originally posted, yes the mass source terms are included in the volume fraction continuity equation and the energy source terms in the energy equation. The energy source terms are basically latent heat*mass source terms. Those are solved for the the secondary phase. The momentum equation is solved for the secondary phase with an additional surface tension force term as the source. The LEE model takes care of ebverything in FLUENT but still I feel UDF should be more accurate. Latent heat in fluent is computed using the differences in the specific enthalpies of the liquid phase and the vapor phase, divided the molar mass of the liquid water or vapor which is 18.01 kg/mol.

    As I am working on a similar problem, I have found that the default values of condensation and evaporation coefficient only works when you select water liquid as the primary phase and the water vapor as the secondary phase. Fine tuning those constants is an arduous task since it is purely based on trial and error approach.

    I have asked the ANSYS community regarding their suggestion on this matter but haven't got a reply yet.

    Please let me know if you have any questions regarding the validation or the accuracy % of the LEE model?

  • soumitra2102soumitra2102 Member
    edited June 2019

    you can get few UDF's code in the internet which I believe are correct although those are written for water-vapor to be primary phase and the water-liquid to be secondary phase. If you don't find one I can share it.

     

    Can you kindly share it here or @ [email protected] please?

    Thank You.

  • DrAmineDrAmine GermanyForum Coordinator
    edited June 2019
    Almost all UDF snippets which do know are generally another form of the Lee Model. I recommend to stick to Lee Model if you do have bulk phase change otherwise use an UDF to model free surfacec evaporation into gaseous mixture
  • DrAmineDrAmine GermanyForum Coordinator
    edited June 2019
    Problem with Lee Model are the tuneable coefficients which might range from 0.001 to 1000. If you do not have exp. data to compare with stick to Knudsen law to formulate them or keep the ratio equal to density ratio.
  • DrAmineDrAmine GermanyForum Coordinator
    edited June 2019
    And Fluent always set a preference pressure location. Please check after initialization. Let me know if this does not show the actual location (might be slightly different than from the user provided one)
  • shadowfaxshadowfax Member
    edited June 2019

    Well I have executed that command after the initialization step and yet Fluent doesn't show any value for the actual reference pressure location.

  • DrAmineDrAmine GermanyForum Coordinator
    edited June 2019

    The TUI command is working for me for VOF dummy case. 

  • rchristensenrchristensen Member
    edited August 2019

    Hello Amine, shadowfax and dp1106,

    It seems to me that there is a lot of confusion as to whether UDFs need to be used to model the mass and energy transfer appropriately or not, when it comes to modeling closed two-phase thermosyphons. Most research articles that I have read suggest the usage of UDFs, while ANSYS experts on the student community have advised to stick to the in-built Lee model. Maybe I'm beating a dead horse here, but I would appreciate if any one of you could clarify some of these things.  

    Has the in-built model in ANSYS been updated for newer versions (after Fluent 13.0) to model the mass and energy transfer more accurately? Because the UDF code snippets that most people are referring to are taken from the same resources, and those researchers have used either Fluent 6.2 or Fluent 13.0. 

    I would like to know your thoughts on this. 

    Rich 

     

  • DrAmineDrAmine GermanyForum Coordinator
    edited August 2019
    Yes no need to use any UDF if using Lee Model. All secondary fluxes are taken into account.
  • rchristensenrchristensen Member
    edited August 2019

    Thank you, Amine. 

    Rich

  • DrAmineDrAmine GermanyForum Coordinator
    edited August 2019
    You are Welcome.
  • pritam1688pritam1688 Member
    edited February 8

    Hello shadowfax and dp1106,

    Can you share a case setup information because  I am also not able to see any condensation with the lee model? 

    Please share some light on the primary and secondary phase and whether I need a 2 mass transfer lee mechanism or just one? 

Sign In or Register to comment.