How to get the surface area between two phases in VOF model
 

Do anyone know if there has a macro to get the surface area between two phases in VOF model. I used Geo-Reconstrust Discretization for VOF.
I found C_VOF_S(c,t) and Get_Surface_Distance(cell_t c, Thread *t) in "sg_vof.h". I wanted to use them to found what did they return. But always fluent return errors:

Error:
FLUENT received fatal signal (ACCESS_VIOLATION)
1. Note exact events leading to error.
2. Save case/data under new name.
3. Exit program and restart to continue.
4. Report error to your distributor.

I tried mixture thread and one phase thread for t in C_VOF_S(c,t) and Get_Surface_Distance(cell_t c, Thread *t),but the errors still exist.

Hi, Cloud,
Have you solve you problem? I need to calculate the interface area in VOF model, and I'm wondering how to implement this. If you've solve this problem, plz help.
Thank you !

any luck?
 

Hi,

I just posted a similar question and I am wondering if you guys have found out how to obtain the area of the interface using an UDF?

Bradley

Interfacial area could be calculated by the following:

Magnitude of Gradient(Alpha) * Volume

Hope it helps.

Thanks! It's helpful. Another question: Which literature can I find this equation ?
Does the fluent help has this equation?

Hi,
I also confused with such a difficult question when i want to simulate the gas-liquid flow in a falling film reactor. how to get the the interface area in a cell using UDF micros? there were an equation in "help" to calculate the area density, area =2.0*[alpha]*the gradient of [alpha]. But this equation may be a wrong one. Besides of this, how to get the gradient of [alpha]? when you use the macro C_VOF_G, there will be notes: access violate.

Are you from China? Maybe we can discuss this problem in Chinese.my e-mail:classic1573@163.com:)

Hi vig,
I wonder if the equation is also applied to the wick-vapor interface?
Regards,
Bill

Finding interface area
 

Dear All
Hello
Finding the premier of the interface (in 2-D cases) or surface of interface (in 3-D simulations) is my concern also. I didn't found how I can use Ansys for calculating these parameters. using the equation Area = Magnitude of Gradient(Alpha) * Volume is not straightforward because in addition to non- constant valued of Gradient(Alpha) in all domain, finding its amount has been not predicted in Fluent. So now my question is how I can find the solution for this matter.
Thanks

UDF for surface between 2 phases
 

Here are 2 different ways of obtaining the area_density between 2 phases :
2.0 * magnitude(gradient(alpha)) * alpha
magnitude(gradient(alpha)) * Cell_Volume
I don't know which one is appropriate, but those 2 were mentioned across Fluent's help guide and within the previous posts :

/* ######################################
Steps to take to make it work
1. Read in the converged case and data
2. Link the udf (Define->User Defined->Functions->Compiled)
3. Hook adjust funtion (Define->User Defined->Function Hooks->Adjust Function)
4. Define UDM (Define->User Defined->Memory 3)
5. Define UDS (Define->User Defined->Scalars 2)
6. Turn off all equations (Solve->Controls->Solution)
7. Do one iterations
8. Execute store_gradient (Define->User Defined->Execute On Demand)
9. Execute store_area_density_1 (Define->User Defined->Execute On Demand)
10.Execute store_area_density_2 (Define->User Defined->Execute On Demand)
######################################*/
　
# include "udf.h"
# define domain_ID 2
　
DEFINE_ADJUST(adjust_gradient, domain)
{
Thread *t;
cell_t c;
face_t f;
　
domain = Get_Domain(domain_ID);
　
/* Fill UDS with the variable. */
thread_loop_c (t,domain)
{
begin_c_loop (c,t)
{
/* Obtains VOF at cell center and saves it as scalar */
C_UDSI(c,t,0) = C_VOF(c,t);
/* Obtains Cell Volume and saves it as scalar */
C_UDSI(c,t,1) = C_VOLUME(c,t);
}
end_c_loop (c,t)
}
　
thread_loop_f (t,domain)
{
if (THREAD_STORAGE(t,SV_UDS_I(0))!=NULL)
begin_f_loop (f,t)
{
F_UDSI(f,t,0) = F_VOF(f,t);
}
end_f_loop (f,t)
}
　
}
　
DEFINE_ON_DEMAND(store_gradient)
{
Domain *domain;
cell_t c;
Thread *t;
　
domain=Get_Domain(1);
　
/* Fill the UDM with magnitude of gradient. */
thread_loop_c (t,domain)
{
begin_c_loop (c,t)
{
C_UDMI(c,t,0) = NV_MAG(C_UDSI_G(c,t,0));
}
end_c_loop (c,t)
}
}
　
DEFINE_ON_DEMAND(store_area_density_1)
{
Domain *domain;
cell_t c;
Thread *t;
　
domain=Get_Domain(1);
　
/* Fill the UDM with are_adensity. */
thread_loop_c (t,domain)
{
begin_c_loop (c,t)
{

C_UDMI(c,t,1) = 2.0 * NV_MAG(C_UDSI_G(c,t,0)) * C_UDSI(c,t,0) ;
}
end_c_loop (c,t)
}
}
　
DEFINE_ON_DEMAND(store_area_density_2)
{
Domain *domain;
cell_t c;
Thread *t;
　
domain=Get_Domain(1);
　
/* Fill the UDM with are_adensity. */
thread_loop_c (t,domain)
{
begin_c_loop (c,t)
{

C_UDMI(c,t,2) = NV_MAG(C_UDSI_G(c,t,0)) * C_UDSI(c,t,1) ;
}
end_c_loop (c,t)
}
}

- JS

Thanks a lot. I will work on this UDF.

vof gradient
 

I am using this code, it works and you don't need UDS.

I looked for everywhere for the VOF area density functions in Fluent User Guide but I couldnt find these equations. Can anyone guide me to find those pages ?

Hi，have your problem been solved？ I need your help.

I am sorry but i also couldnt fix my problem

thank you. if you fix your problem someday, please tell me

interface surface area
 

Hi if you have fix the problem. Let me know also
I am also doing the same calculation

Why Fluent says that the periodic condition is not compatible with the VOF model ?
 

[QUOTE=LyngHoo;381000]Hi,
I realized a simulation of a free surface flow in the presence of periodic roughness with the VOF model. I remarked that when we impose the pressure gradient for the entire domain, the velocity of the air phase will be 100 x the velocity of the water phase.
Is it for this reason Fluent says that the periodic condition is not compatible with VOF?
To avoid this problem I used a UDF to impose this pressure gradient only in the water phase and I solved the problem.
Is the procedure I followed is logical?
How to contact Fluent for this problem?