[Harnoor]

I am working on my phD thesis that involves simulation of an ink droplet impacting a rigid surface. I am using a 2d planar multiphase VOF solver with surface tension modeling. So the primary phase is air and the secondary phase is the ink droplet. Now I wish to apply a constant volumetric heating source to the region where volume fraction of the droplet > 0.9 (cut off value). For this, I wrote a UDF. Even though I don't get any errors during interpretation, the UDF does not produce any volumetric heating. The UDF is pasted below:


#include "udf.h"
#include "mem.h" /* cell indexing header */

DEFINE_SOURCE(hgen_source,c,t,dS,eqn)
{
real source;
int phase_domain_index;
cell_t cell;
Thread *cell_thread;
Domain *subdomain;
Domain *mixture_domain;
mixture_domain = Get_Domain(1);

/* loop over all subdomains (phases) in the superdomain (mixture) */
sub_domain_loop(subdomain, mixture_domain, phase_domain_index)
{
/* loop if secondary phase */
if (DOMAIN_ID(subdomain) == 3) //DOMAIN_ID of: mixture =1, primary = 2, secondary = 3, by convention.
{
/* loop over all cell threads in the secondary phase domain */
thread_loop_c (cell_thread,subdomain)
{
/* loop over all cells in secondary phase cell threads */
begin_c_loop_all (cell,cell_thread)
{
if (C_VOF(cell,cell_thread)>0.9)
{
source = 8*pow(10,11);
dS[eqn] = 0;
}
else
{
source = 0;
dS[eqn] = 0;
}
}
end_c_loop_all (cell,cell_thread)
}
}
}

return source;
}


However when I remove the if condition inside c_loop_all and just set source equal to a constant value, I do get volumetric heating in the entire domain. I just can't find a way to apply the source term only to the region with droplet volume fraction > 0.9. Is there something wrong with the UDF? I am really new to UDF's so any help will be greatly appreciated.

[Harnoor]

Hey guys, I would really appreciate any insights into the problem. I am stuck and need some help to proceed.

[AlexanderZ]

did you hook your functions in Fluent GUI?
try to compile instead of interpret

best regards

[obscureed]

Hi Harnoor,

Quoting from the ANSYS Fluent Customization Manual:
Your UDF will need to compute the real source term only for a single cell and return the value to the solver

So you don't need a cell loop at all. On each call to the UDF, you only need to consider the cell defined by the values of c,t that are passed into the function.

By the way, when a publication writes 8×10^11, you should use 8.e11 in a program, not 8*pow(10,11). They arrive at the same answer, but 8.e11 goes straight there. It's a bit like not knowing how decimal points work, so writing 93.3 as (93+3./10.).

I am uneasy about the physical basis for defining a volume-based energy source. Are you relying on a uniform cell height for the wall-adjacent cells?

Good luck!
Ed