I have attempted a few tries of recreating a two-phase closed thermosyphon (heat pipe) in Fluent, but am unable to get condensation to work correctly. I have set up water liquid and water vapor as phases. I have also tried having air in addition to the two water phases. I have tried various tutorials on YouTube of evaporation/condensation mechanisms and have not been able to get any condensation. I've attached an example of a tutorial case from this YouTube video: https://www.youtube.com/watch?v=hPeGvczYHMM
Any insight would be greatly appreciated!
Hi,
I am interested about two phase flow. I am a newbie in this field. I see your simulation is different than Fadhl, et. al paper. I am curious about your CFD settings.
Thanks
Teguh
Hello,
The attached images are from the YouTube video linked. Fadhl was only mentioned to reference that that was my end goal.
Best,
Harrison
I'm not too familiair with the workings of ANSYS FLUENT, but generally speaking evaporation and condensation are modelled through source terms which act on the vapour-liquid interface. These terms 'subtract' mass and energy from one phase and 'add' it to the other phase. Unless you have specified these source terms, you can not expect condensation to occur spontaneously in your simulation.
An example of how this is implemented can be found in section 2.2 of the following paper (Ferrari et al 2018). Article Numerical analysis of slug flow boiling in square microchannels
Hello Leander,
Thank you for your input. I have set up an evaporation/condensation mass transfer mechanism within the multiphase model in Fluent. Both the evaporation frequency and condensation frequency are at 0.1 Hz, but have been modified on other attempts.
Best,
Harrison
Dear Mr. Bass,
Good to hear that you implemented a mass transfer model. Presuming that this model is correct, my next question would be: do you have an interface?
In a real thermosyphon condensation is initiated by the formation of minute liquid droplets on the cold wall. But numerically this means that an interface needs to be created before condensation can take place. Does your simulation have some sort of artificial 'starting point' for condensation? Of not, then that could become an issue.
Mr. Boer,
I am unsure what you mean by "interface." I have the condenser wall set as a 'wall' boundary condition which is where the liquid would condense. The water vapor gets cold (as seen by temperature contours) but no mass transfer occurs -- which is where your interface would come in?
Thanks,
Harrison
Yes, something special needs to be done here. We have encountered the same 'problem' in the past when trying to simulate pool boiling. In our case the local liquid temperature at the hot wall would keep increasing till far above the boiling point of the liquid, but no boiling would take place. Only when we initialized the simulation with a small nucleate bubble present on the wall, we could get a growing vapour bubble. This occurs because the simulation only describes transport between phases, but not the creation of a new phase (called nucleation).
In your case an amount of liquid needs to be present on the wall initially. Perhaps you can enforce this through an initial condition or boundary condition? I presume that you can find out more details on the treatment of this problem in existing literature on simulations of condensation heat transfer.
Mr. Boer,
I was curious about your statement about boiling without a nucleate bubble, so I ran it on Fluent, and it seems like Fluent can handle boiling without vapor bubble present. This was initialized as all liquid with a constant heat flux applied on the bottom third of the pipe.
Regardless, I tried a few cases of having a droplet present to induce condensation, but still I am not having luck. I think my issue is with picking the correct condensation frequency coefficient. Thankful for your input.
Modeling evaporation and condensation is a tricky business. You need to capture the interface first. Best way is write UDF for that
If you are considering water as a heat transfer fluid, use evaporation frequency 0.1 and condensation frequency 180.
In Fluent, evaporation frequency (Be), and condensation frequency (Bc) have been set equal to 0.1. However, Be and Bc should be set with being proportional to vapor density and liquid density. If they have the same value, the amount of the mass transfer in the phase change won't be able to keep the balance because of the difference between the liquid density and the vapor density. As a result, you might have a hard time in the convergence of continuity eq. as well. In the Fadhlstudy, the mass transfer time relaxation parameter for the condensation ( Bc ) has been calculated using the equation, Bc = Bv * ( liquid density / vapor density). = 0.1*( 1000/0.55) = 181 (approximate).)
I tried to solve vaporization of water flow in a pipe. The most important is to set the BCs right. I solved a SS problem, with inflow at certain inlet velocity, with zero VVF at inlet, and temperature at inlet below the boiling point. Set Outflow BC at exit. The pipe is heated at temperature greater than the boiling point temperature at the pipe walls. Make sure that the operating conditions are set right. I got a very reasonable results in terms of Volume fraction distribution, velocity and temperature distribution all over the flow domain.
Please, what is the reference of the mentioned equation?
Bc = Bv * ( liquid density / vapor density).
- Badges
- Science topic