The DEFINE_TURB_SCHMIDT macro can be
used to specify the turbulent Schmidt numbers of all transported species
in ANSYS Fluent, for single-phase flows.
The turbulent Schmidt number, denoted ,
controls the turbulent diffusion of species transported in ANSYS Fluent.
You can use
DEFINE_TURB_SCHMIDT to specify for each species solved.
DEFINE_TURB_SCHMIDT (name, c, t, i)
|
Argument Type |
Description |
|---|---|
|
|
UDF name. |
|
|
Index of cell on which the Turbulent Schmidt number function is to be applied. |
|
|
Pointer to cell thread. |
|
|
Species index. |
Function returns
real
There are four arguments to DEFINE_TURB_SCHMIDT: name, c, t and i. You supply name, the name of the UDF. c, t and i are variables
that are passed by the ANSYS Fluent solver to your UDF. Your UDF will
need to return the real value for the turbulent
Schmidt number to the solver.
The following example sets to
be inversely proportional to the species index. Hence, the first species
in the materials list will have the smallest turbulent diffusion,
and the last species will have the largest turbulent diffusion.
#include "udf.h"
DEFINE_TURB_SCHMIDT(udf_sct, c, t, i)
{
return 1./((real)i+1.);
}
After the UDF that you have defined using DEFINE_TURB_SCHMIDT is interpreted (Interpreting UDFs)
or compiled (Compiling UDFs), the name
of the argument that you supplied as the first DEFINE macro argument (for example, udf_sct in
the above example) will become visible and selectable in the Viscous Model dialog box in ANSYS Fluent. See Hooking DEFINE_TURB_SCHMIDT UDFs for details.