2.5.8 DEFINE_DPM_OUTPUT

Description

You can use DEFINE_DPM_OUTPUT to modify what is written to the sampling device output. This function allows access to the variables that are written as a particle passes through a sampler (see this chapter in the separate User's Guide for details).

Usage

DEFINE_DPM_OUTPUT( name, header, fp, p, t, plane)

Argument Type	Description
symbol name	UDF name.
int header	Variable that is equal to 1 at the first call of the function
	before particles are tracked and set to 0 for subsequent calls.
FILE *fp	Pointer to the file to or from which you are writing or reading.
Tracked_Particle *p	Pointer to the Tracked_Particle data structure which
	contains data related to the particle being tracked.
Thread *t	Pointer to the thread that the particle is passing through if the
	sampler is represented by a mesh surface. If the sampler is not
	defined as a mesh surface, then the value of t is NULL.
Plane *plane	Pointer to the Plane structure (see dpm.h) if the sampling
	device is defined as a planar slice (line in 2d). If a mesh surface
	is used by the sampler, then plane is NULL.
Function returns
void

There are six arguments to DEFINE_DPM_OUTPUT: name, header, fp, p, t, and plane. You supply name, the name of the UDF. header, fp, p, t, and plane are variables that are passed by the ANSYS FLUENT solver to your UDF. The output of your UDF will be written to the file indicated by fp.

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 discrete_phase_sample samples the size and velocity of discrete phase particles at selected planes downstream of an injection. For 2d axisymmetric simulations, it is assumed that droplets/particles are being sampled at planes (lines) corresponding to constant $x$. For 3d simulations, the sampling planes correspond to constant $z$.

To remove particles from the domain after they have been sampled, change the value of REMOVE_PARTICLES to TRUE. In this case, particles will be deleted following the time step in which they cross the plane. This is useful when you want to sample a spray immediately in front of an injector and you don't wish to track the particles further downstream.

This UDF works with unsteady and steady simulations that include droplet break-up or collisions. Note that the discrete phase must be traced in an unsteady manner.

#include "udf.h"
/******************************************************************/
/* UDF that samples discrete phase size and velocity distributions*/ 
/* within the domain.                                             */          
/******************************************************************/
#define REMOVE_PARTICLES FALSE

DEFINE_DPM_OUTPUT(discrete_phase_sample,header,fp,p,t,plane)
{  

#if RP_2D

  real y; 

  if(header)
  {
      par_fprintf_head(fp,"  #Time[s]   R [m]   X-velocity[m/s]");
      par_fprintf_head(fp," W-velocity[m/s]  R-velocity[m/s]  ");
      par_fprintf_head(fp,"Drop Diameter[m]  Number of Drops   ");
      par_fprintf_head(fp,"Temperature [K]  Initial Diam [m]  ");
      par_fprintf_head(fp,"Injection Time [s]  \n");
  }

  if(NULLP(p))
    return;

  if (rp_axi && (sg_swirl || rp_ke))
    y = MAX(sqrt(SQR(P_POS(p)[1]) + SQR(P_POS(p)[2])),DPM_SMALL);
  else
    y = P_POS(p)[1];

  par_fprintf(fp,"%d %d  %e %f %f  %f  %f  %e  %e  %f  %e  %f  \n",
       P_INJ_ID(P_INJECTION(p)),p->part_id, P_TIME(p),y,P_VEL(p)[0],
       P_VEL(p)[1],P_VEL(p)[2],P_DIAM(p),P_N(p),
       P_T(p), P_INIT_DIAM(p),p->time_of_birth);

#else 

  real r, x, y; 

  if(header)
  {
    par_fprintf_head(fp,"  #Time[s]  R [m]  x-velocity[m/s]  ");
    par_fprintf_head(fp,"y-velocity[m/s]  z-velocity[m/s]   ");
    par_fprintf_head(fp,"Drop Diameter[m]   Number of Drops  ");
    par_fprintf_head(fp,"Temperature [K]   Initial Diam [m]    ");
    par_fprintf_head(fp,"Injection Time [s]  \n");
  }

  if(NULLP(p))
    return;

  x = P_POS(p)[0];
  y = P_POS(p)[1];
  r = sqrt(SQR(x) + SQR(y));

  par_fprintf(fp,"%d %d %e %f  %f %f  %f %e %e %f %e %f \n",
	 P_INJ_ID(P_INJECTION(p)), p->part_id, P_TIME(p), r,P_VEL(p)[0],
         P_VEL(p)[1],P_VEL(p)[2],P_DIAM(p),P_N(p),
         P_T(p), P_INIT_DIAM(p), p->time_of_birth);

#endif

#if REMOVE_PARTICLES
  p->stream_index=-1;
#endif
}

Hooking a DPM Output UDF to ANSYS FLUENT

After the UDF that you have defined using DEFINE_DPM_OUTPUT 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 Sample Trajectories dialog box in ANSYS FLUENT. See Section  6.4.8 for details on how to hook your DEFINE_DPM_OUTPUT UDF to ANSYS FLUENT.