[gartz89]

Hello If you followed the steps tutorial from the link below
the popular youtube channel on our colleague - CFD expert you will understand very fast the problem.

Film Condensation on Vertical Wall (Part-2)
https://www.youtube.com/watch?v=B_42GloChq8&t=45s

However first of all I have to confirm that this discussion has no conflict of interest and the only aim is for learning how to model film condensation on vertical wall with mixture model and evaporation. So I done the model and it works, but if you can’t open the link I’ll describe the problem.

This is vertical channel with fluid domain, pressure based solver and transient was specified with gravity -9.81 m/s^2. The fluid is mixture of air, water vapor and water liquid so we have to add and create them in the physical properties. After that in Multiphase models we define mixture model and specified the three phases: phase 1- air, phase 2-water vapor, phase 3 – water liquid. The mass transfer mechanism is evaporation/condensation with 0.1 frequency from default from liquid to vapor. In the BC we have velocity inlet 2.56 m/s and inlet temperature of the mixture 348.6 K. For the inlet water vapor we defined volume fraction 0.3 (humidity) velocity 2.56 m/s and for the water liquid the volume fraction is 0 and the inlet velocity again 2.56 m/s. The outlet is pressure outlet 0 Pa. The cooling wall temperature is 304 K. So the mesh is fine and is ok and everything looks good, but my question is not connect with this simulation … So if I want to use the solution of the model with film condensation for the initial condition for other model. For example I would like to simulate reverse flow with evaporating conditions and my outlet from the previous simulation will be inlet and the inlet will be outlet - reverse flow. The new BC are: the wall temperature will be more high 350 K and the reverse flow the inlet volume fraction of water vapor will be lower for example 0.03 and the velocity of the phases are the same 2.56 but the inlet temperature of the mixture is lower 300K. So I use the solution for the first model in edit automatic Initialization and Case modification I use the same transient steps and I used the new BC. Yes I have to tell you that there is evaporation, but the main problem is why the volume fraction of the water vapor is 0.03 constant only from the beginning of the inlet channel and stop to decrease longitudinally. And at the end of the simulation of the outlet I have the old value of volume fraction 0.3 from the first simulation. This is for example that I’ve got a lot of humid air from the first condensation model and after that in the reversal evaporation direction when I use dry air with very low humidity the flow can’t go out from the other side. Why this is happened can you give me more information or some advice, please? Thank you and regards!

[vinerm]

First of all, the tutorial is wrong in its entirety due to multiple reasons.

1. Air is being used as material for liquid water. Fluent does not care about the name of the material but its properties. So, the setup is wrong.

2. There is never a clear interface between two or more gases. Therefore, vapor and air cannot be different phases. These have to be part of same phase albeit as different components. The reason is not that these cannot be modeled as different phases, rather the models are inapplicable. Therefore, the system should have two phases, one containing water vapor and air and the other one containing water liquid.

3. The most important one is the physics being modeled. Though there are many reliable models for wall boiling yet there is hardly any model for wall condensation. CFX has a model but its pretty complicated and requires secondary fluxes to be modeled. The phenomenon itself is quite complex and has not really been easy on academicians. The model being used in the tutorial, Evaporation-Condensation, is meant for evaporation and condensation away from the walls or what is called pool boiling.

So, if you wish to model wall condensation, either write your own model or use CFX.

On a side, youtube is a social media channel and not a peer-reviewed resource. Therefore, be careful and verify before making use of anything. Personally, CFD tools are just tools; these are resources and just having resource available does not make someone expert. Validation, verification, and questioning are very important parts of scientific endeavor and there cannot be a compromise on that.

[gartz89]

Thank you Vinerm for your quick response. I really appreciate your comment and really thankful for the information. But as you said, the model is not quite accurate, but if I compare the results with some academic works, they are almost the same. Of course I'm sure you're right, but for now I won't check with other models or I will not validate with an experimental data. I will only use this model for approximatly estimates and some day if I want to do some experiment I will check this complicated CFX model and other models for verification and validation. Thank you again Vinerm and Regards!

[vinerm]

That's good. If the results are matching with some existing work, that means the model is appropriate for the phenomenon you want to simulate. All I stated was that model was invalid for wall condensation. However, if the condensation is not due to the wall, then the model is certainly valid.