CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   Siemens (https://www.cfd-online.com/Forums/siemens/)
-   -   drop simulation (https://www.cfd-online.com/Forums/siemens/53399-drop-simulation.html)

Roxy July 24, 2003 07:19

drop simulation
 
Hii All!!!

I'm trying to simulate free fall of drop on a single tube, the area of interest is film thickness. for that i created geometry and solved that but not getting film over tube. does anyone suggest how to approach for that. Is any surface tension function need to be define, or a thin flow of stream would work for that.

thanks in advance for your invaluable suggestions and contribution of time for this problem.

4xF July 26, 2003 12:06

Re: drop simulation
 
Use the VOF model of STAR-CD (Free-surface flow). You have to define surface tension. For a first analysis, a constant value for the surface tension will do. Try to mesh finer at the walls. As far as I remember, there is a real constant for setting the contact angel at walls. Ask support to provide you the info.

Michiel July 29, 2003 04:55

Re: drop simulation
 
I also think you should use VOF on this topic, but take care of the resolusion. You should at least have about 20 computational within the drop but also in over the thickness of the film.

Roxy August 4, 2003 05:42

Re: drop simulation
 
Thank you for responce, I've completed that with very fine mesh and at a low time step. but I didn't specified any surface tension property as I took the default one for the two surface i.e. between air and water drop, it seems that we can't define surface tension simultaneously for drop and tube surface.

Do u have any suggestion on it, I think that will be help me further to get more realistic results.

Please do reply,

4xF August 4, 2003 08:41

Re: drop simulation
 
Do the following:

1) SWITCH 23 ON 2) Write the problem file 3) create the ufile directory by typing ufiles at the

command line 4) Goto to Utility -> User Subroutines and write out the

CAVPRO.F subroutine 5) Edit the CAVPRO.F subroutine and uncomment the lines

with SIGMA and CONTANG. This will pass the surface

tension coefficient (SIGMA) and the wall contact angle

(CONTANG) to the solver. Note that the values are

default ones for water. 6) Link your new star executable. Do not forget to

include user subroutines. 7) Run & enjoy :)

Roxy August 5, 2003 03:39

Re: drop simulation
 
Thank you very much, I will edit that Subroutine. Hope It will work. ;-)


All times are GMT -4. The time now is 09:23.