You can use DEFINE_DPM_DRAG to specify
the drag between particles and fluid as a dimensionless group () as it appears in the
drag force per unit particle mass:
(2–19) |
| where | |
|
| |
|
| |
|
| |
|
| |
|
|
DEFINE_DPM_DRAG (name, Re, tp)
|
Argument Type |
Description |
|---|---|
|
|
UDF name. |
|
|
Particle Reynolds number based on the particle diameter and relative gas velocity. |
|
|
Pointer to the |
Function returns
real
There are three arguments to DEFINE_DPM_DRAG: name, Re, and tp. You supply name, the name
of the UDF. Re and tp are variables that are passed by the ANSYS Fluent solver to your UDF.
Your UDF will need to return the real value
of the drag force on a particle. The value returned to the solver
must be dimensionless and represent 18 * Cd * Re / 24.
Important: Pointer tp can be used as an argument
to the macros defined in DPM Macros to
obtain information about particle properties (for example, injection
properties).
The following UDF, named particle_drag_force, computes the drag force on a particle and is a variation of the
body force UDF presented in
DEFINE_DPM_BODY_FORCE
. The flow is the same,
but a different curve is used to describe the particle drag. DEFINE_DPM_DRAG is called at every particle time step
in ANSYS Fluent, and requires a significant amount of CPU time to execute.
For this reason, the UDF should be executed as a compiled UDF.
/***********************************************************************
UDF for computing particle drag coefficient (18 Cd Re/24)
curve as suggested by R. Clift, J. R. Grace and M. E. Weber
"Bubbles, Drops, and Particles" (1978)
************************************************************************/
#include "udf.h"
DEFINE_DPM_DRAG(particle_drag_force,Re,tp)
{
real w, drag_force;
if (Re < 0.01)
{
drag_force=18.0;
return (drag_force);
}
else if (Re < 20.0)
{
w = log10(Re);
drag_force = 18.0 + 2.367*pow(Re,0.82-0.05*w) ;
return (drag_force);
}
else
/* Note: suggested valid range 20 < Re < 260 */
{
drag_force = 18.0 + 3.483*pow(Re,0.6305) ;
return (drag_force);
}
}
After the UDF that you have defined using DEFINE_DPM_DRAG is interpreted (Interpreting UDFs)
or compiled (Compiling UDFs), the name
of the argument that you supplied as the first DEFINE macro argument will become visible in the Set Injection
Properties dialog box in ANSYS Fluent. See Hooking DEFINE_DPM_DRAG UDFs for details on how to hook your
DEFINE_DPM_DRAG UDF to ANSYS Fluent.