2.5.3 DEFINE_DPM_DRAG

Description

You can use DEFINE_DPM_DRAG to specify the drag coefficient, $C_D$, between particles and fluid defined by the following equation:

$$\begin{eqnarray*} F_D = \frac{18 \mu} {\rho_p D^2_p} \frac{C_D {\rm Re}} {24} \end{eqnarray*}$$

Usage

DEFINE_DPM_DRAG( name, Re, p)

Argument Type	Description
symbol name	UDF name.
real Re	particle Reynolds number based on the particle diameter and
	relative gas velocity.
Tracked_Particle *p	Pointer to the Tracked_Particle data structure which
	contains data related to the particle being tracked.
Function returns
real

There are three arguments to DEFINE_DPM_DRAG: name, Re, and p. You supply name, the name of the UDF. Re and p 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.

Pointer p can be used as an argument to the macros defined in Section  3.2.7 to obtain information about particle properties (e.g., injection properties).

Example

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 Section  2.5.2. 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,p)
{
  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);
    }
}

Hooking a DPM Drag Coefficient UDF to ANSYS FLUENT

After the UDF that you have defined using DEFINE_DPM_DRAG is interpreted (Chapter  4) or compiled (Chapter  5), the name of the argument that you supplied as the first DEFINE macro argument will become visible in the Discrete Phase Model dialog box in ANSYS FLUENT. See Section  6.4.3 for details on how to hook your DEFINE_DPM_DRAG UDF to ANSYS FLUENT.