## Ansys Products

Discuss installation & licensing of our Ansys Teaching and Research products

#### Periodic boundary condition for droplet evaporation

• Amir
Subscriber

Hi there

I wonder if somebody can help me with my problem

In  a cubic computational domain, for the evaporation of a droplet on a hot flat surface surrounded by pressure outlet boundaries on top and front surfaces, and the behind surface side is a symmetry BC,

1)for this problem, in practice, can we use periodic BC only between left and right surfaces to reduce the longitude size of the domain?
as the droplet moves in x direction when evaporating using a periodic BC can help if possible to be used

I am using VOF and the model of LEE

if this periodic setup is fine,
2)what should I set as the upstream bulk temperature in the periodic setup?

My initial setup as a test is as below

Gravity=-9.81 in Y

Boussinesq parameter: operating tempearure=the evaporation temperature

Operating density method=min phase average

--------------------------------

Periodic BC setup:

flow direction
x=1
y=0
z=0

for the upstream bulk temperature, I used two case studies

A)a little temperature (0.15 deg) less than evaporation temp

B) the same as the evaporation temp

------------------------------------

coupled +Body force weighted and GeoReconstruct,

3) is the setup you recommend for my simulation

--------------------------------------------

for the above setup, I did some simulations and faced a problem around the periodic surfaces, partially we see some hot and cold spots which is not realistic (there is no heat source/sink but the bottom hot surface with a fixed temperature) because all over the domain the temperature should not be more than the bottom fixed temperature hot base plate or less than initial/ and pressure outlet reverse flow temperature, but in the temperature contours on the symmetric plane, in below you can see, for the case A and B there are such hot and cold temperatures which I can not understand why

Amir

• Rob
Forum Moderator

No, as the droplet evaporates along the domain you don't conserve phase mass as you travel along the domain: it's not periodic.

• Amir
Subscriber

thank you so much Rob, so this problem is not possible to be simulated using periodic BC in any way?

what about my setup, is it fine?

Boussinesq parameter: operating tempearure=the evaporation temperature

Operating density method=min phase average

coupled +Body force weighted and GeoReconstruct,

• Amir
Subscriber

I used periodic BC to reduce the domain and computational cost, and symmetric as well

• Rob
Forum Moderator

If flow is travelling left to right (for example) the gas composition and liquid mass will change from right to left: mass per phase is not equal on both boundaries. From memory there are some multiphase specific notes in the Periodic boundary section(s) of the User's Guide.

Operating density needs to be reviewed if gravity is on when you have a vertical pressure boundary: how are you accounting for hydrostatic effects? Otherwise, the settings aren't wrong - note depending on what you're trying to do you may find alternative settings are "better". That's part of the skill with multiphase models, what is important, and what can we ignore?

• Amir
Subscriber

Please see the below image, a droplet on the surface surrounded by water vapor, the up and front BCs are pressure outlet and the back surface was symmetry, left and right was periodic which based on your answer is not correct,

the size of droplet is 500um

in this problem,

”Operating density needs to be reviewed if gravity is on when you have a vertical pressure boundary, how are you accounting for hydrostatic effects?”

yesI have a vertical pressure BC, what do you mean by hydrostatic pressure effects? so what should I set as the operating density and temperature?

yes gravity is on

• Rob
Forum Moderator

That's not periodic. You'll need to extend some boundaries if you're flowing gas over the domain. Set the downstream & "top" boundary as a pressure outlet.

The issue now is ensuring you have the pressure gradient set correctly up the sides. Fluent uses a "density-operating density" function , so setting the operating density to be exactly the value of the gas phase on the boundary (ie inflow temperature & pressure) reduces the density function to zero: it's explained in the Operating Conditions section of the User's Guide.

• Amir
Subscriber

thank you so much, for compressible flow, it is recommended to use total pressure and a zero operating pressure,

for incompressible flow, we break the total pressure into a non-zero operating pressure and a relative pressure (the static pressure), to reduce the numerical errors

1)what about evaporation in my problem, when using the VOF model, while the water vapor phase is considered to have a fixed density?

in evaporation, shall I still use a non-zero operating density+static pressure?

if so, or in my case as it is open to the atmosphere, the pressure outlet BCs would be zero

2)Also, in the below image, for the Boussinisque parameters, everything is correctly set (the minimum phase average method)?

3)what about the operating temperature?

shall I set the evaporation temperature (the saturation temperature) for that which 373.15 is

or the hot plat temperature which 373.15+8 is.

which one do you recommend?

4)Technically using a fixed density for the vapor water phase is correct for evaporation? (in this range of temperature 373.15+8=hotplate)

what if the evaporation frequency is high like 10^4, Does it influence your answer?

I read some discussions of your and DrAmine answers had about the evaporation frequency and LEE model

one that could find it now was this

https://forum.ansys.com/forums/topic/source-term-in-stefan-problem/

I wonder if you could help me with these questions, to save your time and other peoples will search and face the same questions, I numbered the questions

• Rob
Forum Moderator

I'd review the incompressibe ideal gas option for density. Unless the flow speed is sufficient that it's compressible.

No need to set operating pressure to zero, I generally leave it as "atmospheric" for whatever condition I'm modelling. Review the Bousinesq limitations re temperature range.