
[Sponsors] 
Conjugate Heat Transfer in TwoPhase Flow 

LinkBack  Thread Tools  Search this Thread  Display Modes 
September 28, 2014, 11:31 
Conjugate Heat Transfer in TwoPhase Flow

#1 
Member
Parisa
Join Date: Feb 2013
Posts: 51
Rep Power: 13 
Hello everyone,
I a working on evaporation/condensation, using interPhaseChangeFoam. I could change the solver successfully, and right now I capture the physics. However, at the moment I would like to extend my model to a conjugate heat transfer. I know that I should replace interPhaseChangeFoam solver into chtMultiregionFoam. But, this is not as easy to say. Would you please guide me how I can make a twophase flow solver including conjugate heat transfer? Regards, Parisa 

September 28, 2014, 12:28 

#2 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128 
Greetings Parisa,
I'm going to try to give you a quick answer now to guide you in the right direction and hopefully you'll have more news for us during this week. First of all, practice this tutorial: http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam My strong advice is to not try to modify chtMultiRegionFoam directly, at least not until you've understood how it works. There is a modified/customized solver which might be useful to get some ideas from: http://www.cfdonline.com/Forums/ope...egionfoam.html  you can compare it to the source code for chtMultiRegionFoam on the variant OpenFOAM 1.6ext. After you've gotten a bit more familiar to those two solvers, you should look at the solvers rhoPimpleFoam and buoyantPimpleFoam, which should be the ones with the closest similarities to chtMultiRegionFoam. The point of reference for the core comparison is the code for the "fluid" part of the code on chtMultiRegionFoam. Then comes the bigger problem: how exactly does interPhaseChangeFoam compare to rhoPimpleFoam and/or buoyantPimpleFoam? It's possible that you might need to take a smaller step in between, for example, adapting compressibleInterFoam and/or compressibleMultiphaseInterFoam to the fluid section of chtMultiRegionFoam. Good luck! Best regards, Bruno
__________________


October 5, 2014, 13:40 
Source term in Energy Equation of interphaseChangeFoam

#3 
Member
Parisa
Join Date: Feb 2013
Posts: 51
Rep Power: 13 
Hi everyone,
I have a question in adding source term in energy equation due to evaporation/condensation. I am using interPhaseChangeFoam. I add the surce term as mdot*hl, that mdot is the net evaporation/condensation rate, and hl is the latent heat. However, I am wondering whether or not this source is only added on the interface of liquidvapor. Since the mass must be transferred only at the interface. I think by adding simply the source term, it will be considered for the whole domain, not only on the interface. Please correct me if I am wrong. Regards, Parisa Last edited by Parisa_Khiabani; October 7, 2014 at 16:35. Reason: Update about Heat Source at the Interface 

October 11, 2014, 11:04 

#4  
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128 
Greetings Parisa,
I've moved your post above from the "OpenFOAM Running, Solving & CFD" subforum, so that this can be discussed in a single topic. In addition, I hope you don't mind that I quote a part of what you sent me via PM: Quote:
I suggest following these steps:
Otherwise, personally I won't have nearly enough time to help you before late December. Best regards, Bruno
__________________


October 11, 2014, 12:16 

#5 
Member
Alex
Join Date: Jun 2011
Posts: 33
Rep Power: 15 
Hi Parisa,
I have also been working in thermally driven phase change phenomena, and I'm not sure that the model in interPhaseChangeFoam is really the one to follow. It seems to be geared towards cavitation type phenomena (pressure, not thermally driven), and applies the phase change everywhere, not just on the interface. For many practical evaporation and condensation problems, the compressibility of the flow is not important (as in compressibleInterFoam) since the total pressure and density of the liquid and vapor phases are pretty much constant. What I mean by this is that the density of a fluid element will not vary significantly (except at the infinitesimal interface). For example, if you have a smooth condensing film on a plate, the liquid and vapor densities will essentially be constants everywhere in the domain, even though the fluid is condensing. A better model is to apply a phase change source term on the interface which effects the phase fraction, energy, and pressure equations (e.g. the volumetric source). While I don't want to come across as too much of a self promoter, feel free to check out my JHT paper on the problem. If this seems like the right track to help with your problem, please message me. I can share my code, although I should caution that it is currently in the experimental stage, and I don't want to post it publicly just yet. 

October 13, 2014, 08:49 

#6 
Member
Parisa
Join Date: Feb 2013
Posts: 51
Rep Power: 13 
Thanks Bruno and Alex,
I really appreciate your helps. Would you please have a look at this post? http://www.cfdonline.com/Forums/ope...hangefoam.html In the above post, Jibran claimed that "Yes that is correct. Therefore I am using a modified phase change model. By including terms such as "alpha1*(1alpha1)" in the phase change equations one can ensure that the evaporation and condensation takes place just at the interface." I don't get exactly what he means. By the way, in my model in interPhaseChangeFoam, the phase change is thermally driven although it compares the saturation pressure. I'm saying that because saturation pressures in my model are obtained as a function of temperature. I appreciate if you guide me about those two comments (one from the post and one from the saturation pressure as a function of temperature) Best, Parisa 

October 13, 2014, 09:39 

#7 
Member
Alex
Join Date: Jun 2011
Posts: 33
Rep Power: 15 
Hi Parisa,
I cannot be 100% certain what Jibran meant. My instinct is that he might have meant to apply a source term like: pos( 0.9  alpha1)*pos( alpha1  0.1)*SOURCE . Something along this line looks like it would only apply the phase change on interface cells. This doesn't work out so well in practice. Some examples where it fails:
These are a few challenges that have been driving my own research and code development. 

October 13, 2014, 17:41 
Strange Results in InterPhaseChangeFoam

#8  
Member
Parisa
Join Date: Feb 2013
Posts: 51
Rep Power: 13 
One thing that is really strange for me:
When the inlet flow is subcooled, I see evaporation. However, I would like to see condensation but I cannot. I just set the inlet value for alpha as zero, also zero for internal field. Also I set p_grh less than saturation pressure, to make sure that I have vapor. I set the temperature of the walls much less than the inlet flow temperature (100 C less). However, although the pressure is higher than saturation pressure in some times, I don't see condensation. In fact, in all time directories, alpha is zero and intact. What do you think about this case? Please note that I set saturation pressure as a function of temperature. Regards, Parisa Quote:


October 16, 2014, 06:25 

#9 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 17 
Hello,
Parisa, i am not sure, but you need to check if your evaporation source term is not an expression linked with "alpha". This may block condensation, since alpha in vapour phase is "0". Alex, You say that compressibility of the flow is not important, but in a closed tank, with initial thermal condition far from equilibrium, like 90% of liquid phase, but T > 100° @ 1 atm, your total pressure will change. Or i am wrong ? By the way, is it possible to see your code, as in your paper you use an interesting way to solve evaporation ( interface selection and the pimple like loop for enthalpy) ? regards, olivier 

October 16, 2014, 08:43 

#10 
Member
Alex
Join Date: Jun 2011
Posts: 33
Rep Power: 15 
Hi Olivier,
You raise a very good point, and I should have been more specific. The case I was trying to make is that in many thermally driven phase change processes, there can be a tremendous change in fluid volume without a change in the individual phase densities. Some examples could be: boiling/condensation open to the atmosphere, or in a heat exchanger with relatively low frictional resistance. In your example of a closed pressure vessel, the compressibility of the vapor phase and variation of the saturation temperature with pressure would have to be considered. I can try to clean up my code a bit to share, and put together a couple example cases. It may take a few days to get around to it. In the meantime, here is a bit of a teaser on the energy model from a more recent version of the code focused on mixture phase change (where T_sat is a function of concentration). In this block, I use subcycling, like what is done for the alpha1 equation in interFoam. The energy equation transports H (enthalpy), but conduction is driven by the temperature field. So I use an artificial diffusion technique to stabilize this and prevent checkerboarding. The enthalpy equation for the mixture (H = f(x, T)) is userdefined at runtime, and I use GNU libmatheval to interpret it. In such general cases the temperatureenthalpy coupling is nonlinear, so it is corrected iteratively here (like the PIMPLE pressurevelocity coupling). Code:
for ( subCycle<volScalarField> ESubCycle(H, nESubCycles); !(++ESubCycle).end(); ) { for (int EEqnCount=0; EEqnCount < nEnergyLoops; EEqnCount++) { //Form and solve the energy equation fvScalarMatrix EEqn ( fvm::ddt(rho, H) + fvm::div(rhoPhi, H)  fvc::laplacian(kEff, T)  ChillaxFac*( fvm::laplacian(alphaEffRho, H)  fvc::laplacian(alphaEffRho, H) ) + phaseChangeModel>Q_pc() ); EEqn.solve(); //Now reevaluate T for the updated enthalpy fields T = twoPhaseProperties.T_HX()(); } //Update phase change rates: phaseChangeModel>correct(); alpha1Gen_accum += (runTime.deltaT()/totalDeltaT)*phaseChangeModel>alpha1Gen(); PCV_accum += (runTime.deltaT()/totalDeltaT)*phaseChangeModel>PCV(); } 

October 16, 2014, 09:42 

#11 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 17 
Hello,
So i am waiting for your code clean up and test case. I am not sure to catch what 's you are doing with your user defined enthalpy equation, is this similar to chris tabulated properties ? Btw, subcycling energy equation look like a good idea to avoid the too common "Maximum number of iterations exceeded" from the thermo Newton iteration. regards, olivier 

May 15, 2015, 05:48 

#12  
Senior Member
Join Date: May 2011
Posts: 231
Rep Power: 16 
Hi Parisa,
Did you get solver wring and any reasonable results until now? I am interested in similar problem as yours and I have started t follow the instructions in this thread...I am doing well until now..if you have any suggestions which will speed up the implementation, I will be very grateful! Thanks in advance! Kanarya Quote:


June 3, 2019, 04:07 

#13 
Senior Member

Hello everyone,
Sorry for initiating this post again. I am stuck with a problem, where I couldn't able to stop thinking about it. I have encountered the problem with phase change (adding source term in energy equation due to evaporation/condensation) Phase Change >> which solver ? >> met a problem I can't solve, please help me with it I have posted my query already in the above link Kindly someone look into it please. Thank you 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Conjugate Heat Transfer: Wall Heat Flux at Coupled Walls?  MaxHeat  FLUENT  4  September 14, 2017 10:44 
Quenching simulation : how to set up a conjugate heat transfer between solid&liquid  Rockda  FLUENT  24  August 30, 2016 06:33 
Heat transfer can't converge in the multiple phase flow  kiwishall  CFX  7  March 26, 2014 22:18 
Multiphase flow and conjugate heat transfer simulation  awacs  OpenFOAM Running, Solving & CFD  8  March 1, 2013 05:25 
Convective Heat Transfer  Heat Exchanger  Mark  CFX  6  November 15, 2004 15:55 