[DnyanMiri]

I want to calculate the heat flux removal from a moving hot surface due to spray cooling. What thermal boundary condition should I give to the surface where I want to calculate the surface heat flux?
Heat flux, Temperature or coupled or anything else?

I am giving 0 heat flux boundary condition at the wall and while initialization assigned temperature(1053K) to the surface, am I doing it right?

Please give your valuable opinion. Let me know if you need any more info. Thanks in advance.

[vinerm]

If you wish to determine heat flux then applying heat flux doesn't make sense. You need to either apply a temperature or convection. For that, you should know the condition at the wall.

[DnyanMiri]

Thanks for the reply, Vinerm. Yes, I accept my mistake, it shouldn't be an adiabatic wall. The temperature boundary condition in the fluent means constant temperature, right?
In my case, the plate is initially at 1053K and after spray cooling, I want to calculate heat removal from the surface. I'm not understanding what should be my thermal boundary condition at the surface. I cannot give convection as I want to find the 'h' value from the heat flux. Do I need to write UDF for this? If you could give me any advice, I would be grateful.

[vinerm]

Though usually the thickness of the wall is not modeled or simulated, there are always two sides of a wall. So, you need to provide either a temperature (this would not be appropriate for your case) or convection condition (appears to be more appropriate for you). Fluent calculates convection on the side being included in the domain, such as, upper side if water is on top of the plate. But the bottom side is open to the atmosphere. So, you can provide a h value and a T value.

[DnyanMiri]

Thanks, Vinerm for replying back and sorry for the delay in replying. I've probably found out the right condition for the wall. As there is fluid-solid interaction, I have used it as a coupled wall temperature boundary condition. After initializing, using the patch I have given the initial temperature of the wall which is 1053 K.

This probably requires a new thread but still, it is related. I'm using ANSYS 18.2. When I use spray for cooling the plate/wall, at high temperature like 1053 K film boiling takes place. As the temperature decreases, it moves into transition then nucleate boiling regimes. I read through some related literature, I've found out 'wall jet' DPM boundary condition is used for simulating film boiling. Then lagrangian film model for nucleate boiling. I don't understand how to change between these two boundary conditions while simulation.

If you need any more info, please let me know.
Thanks and Regards,
Dnyanesh.

[vinerm]

That's good. As long as walls are coupled, you don't need to do anything.

For DPM, Wall-Jet boundary condition is nothing but an extension of reflect. It only models the momentum of a droplet hitting a hot wall, such as, droplets jumping on hot plate due to Leidenfrost effect. Wall jet model has no mass transfer mechanism.

Wall-Film on the hand provides you multiple options, including mass transfer. I have not checked in the newer version, however, until 16, there is no nucleate boiling option for droplets. For mass transfer, excluding reactions, evaporation and boiling are the only options. It is quite possible that you are referring to boiling and not nucleate boiling. Actually, nucleate boiling phenomenon may not even take place in a droplet because it is too small for a vapor bubble to form. So, most likely, you can use vaporization and boiling. This does not require any extra code or effort. Option is available within Fluent and switches automatically based on the input data.

[DnyanMiri]

Thanks a lot for the insights, Vinerm. This will help me move forward in my project.
I've found following paper which is closely related to my work, just incase if you want to refer
https://doi.org/10.1016/j.ijheatmass...er.2019.06.098

Thanks and Regards,
Dnyanesh

[vinerm]

It appears to be a good article, however, has mistakes in their representation, at least, if not in their understanding of the phenomenon. But what this paper shows is certainly doable using Wall Film model.

[DnyanMiri]

Hi Vinerm,
I'm right now stuck at a stage where the problem could be of meshing or implementation of the wall film model.
When droplets reach the surface, after a few iterations I get divergence in turbulent viscosity as well as temperature.
Could you help/advise on this problem? Thanks in advance. I can share the required files.

[vinerm]

It could be due to multiple reasons. First of all, droplets should be much smaller than cell sizes in terms of volume. Secondly, the values of the sources terms added to the continuous phase depend on the mass of the particles. If the mass being injected or reaching a surface is very high, it could lead to very high value of source term leading to convergence issues and eventually to divergence. You can plot source terms in Contour plots. Check for their variation as the simulation proceeds. If those values increase all of the sudden, then it could be numerical issue. However, if those increase gradually, then you may try with reduction in the mass being injected.

[DnyanMiri]

Thanks for the quick reply. I'll ensure these things are taken care of and see what happens.

[DnyanMiri]

Hi Vinerm, you have been a source of great help. I was able to solve the problem of divergence in turbulent viscosity by keeping smallest cell volume greater than volume of the droplet.
Right now, as I start my simulation every parameter converges with time step of 10^-4 but after like 100 time steps continuity residual does not go below 10^-3. How can I solve this? any suggestions are welcomed.
I'm using SIMPLEC with second order schemes. Let me know if you need any more info.
Thank you!

[vinerm]

Don't worry about that. 0.001 or 0.003 or even 0.005 are alright as long as there is good conservation of mass and energy as well as the monitors are stable.