CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   Fluent UDF and Scheme Programming (https://www.cfd-online.com/Forums/fluent-udf/)
-   -   UDF for deleting particles in DPM (https://www.cfd-online.com/Forums/fluent-udf/107304-udf-deleting-particles-dpm.html)

imanmirzaii September 23, 2012 18:49
UDF for deleting particles in DPM
 
Hi all,

I am trying to solve the motion of particles in bubbles. The particles along with air are injected from an inlet into water. Therefore the air, which includes the particles, generates the bubble and the particles are trapped in the bubble. For the bubble motion I used VOF and for the particle motion DPM model. Now for the last step of my project I have to delete the particles in the bubble as soon as they impact the bubble surface... I wanna do this with UDF... The idea for this UDF is that I want to delete the particles as soon as the particles are in a cell with f>=0.5 This is the UDF I am using:

#include "udf.h"
#define REMOVE_PARTICLES TRUE
DEFINE_DPM_OUTPUT(discrete_phase_counter,header,fp ,p,t,plane)
{
cell_t c;
Thread *t;
#if REMOVE_PARTICLES /*This if loop removes the particles*/
if(C_VOF(c,t)<=0.5)
p->stream_index=-1;
#endif
#endif
}

I can compile this UDF in Fluent, however, it does not remove the particles... Since I have been working with self developed codes in FORTRAN and I am not an expert in writing UDFs, would you please let me know how I should change this UDF to delete the particles in cells with VOF fractions greater than 0.5. It should be mentioned that in VOF model in liquid f=1 and in air f=0.

With Regards,
Iman.

alexsatan October 8, 2012 03:31
Quote:
Originally Posted by imanmirzaii (Post 383238)
Hi all,

I am trying to solve the motion of particles in bubbles. The particles along with air are injected from an inlet into water. Therefore the air, which includes the particles, generates the bubble and the particles are trapped in the bubble. For the bubble motion I used VOF and for the particle motion DPM model. Now for the last step of my project I have to delete the particles in the bubble as soon as they impact the bubble surface... I wanna do this with UDF... The idea for this UDF is that I want to delete the particles as soon as the particles are in a cell with f>=0.5 This is the UDF I am using:

#include "udf.h"
#define REMOVE_PARTICLES TRUE
DEFINE_DPM_OUTPUT(discrete_phase_counter,header,fp ,p,t,plane)
{
cell_t c;
Thread *t;
#if REMOVE_PARTICLES /*This if loop removes the particles*/
if(C_VOF(c,t)<=0.5)
p->stream_index=-1;
#endif
#endif
}

I can compile this UDF in Fluent, however, it does not remove the particles... Since I have been working with self developed codes in FORTRAN and I am not an expert in writing UDFs, would you please let me know how I should change this UDF to delete the particles in cells with VOF fractions greater than 0.5. It should be mentioned that in VOF model in liquid f=1 and in air f=0.

With Regards,
Iman.
HI:

Did you solve your problem? I have the same problem with you .In my oponion, "#include `dpm.h`" shuold be included in the head file, but my UDF like this and it does not work:

# include "udf.h"
# include "dpm.h"
DEFINE_DPM_SCALAR_UPDATE (reDPM,c,t,in,p)
{
Thread **pt；
real vof_g = C_VOF (c,pt[0]);

if (vof_g>=0.1)
p-> reDPM = -1;
else
return vof_g;
}

imanmirzaii October 8, 2012 12:05
Hi alexsantan,

Yeah I solved the problem, this is the UDF I used and it works perfect:


#include "udf.h"

DEFINE_DPM_SCALAR_UPDATE(charge,c,t,initialize,p)
{
Thread *phase_t = THREAD_SUB_THREAD(t,1);

if(C_VOF(c,phase_t)>=0.5)
p->stream_index = -1;
}

/*
0 in phase_t represents primary phase. If you want to find VOF for
secondary phase, you will have to change 0 to 1.
*/

fluentsimulation November 20, 2012 05:08
hi, Iman

do you know how to use this code in a parallel server ?

thanx a lot!

gearboy November 20, 2012 20:31
Quote:
Originally Posted by imanmirzaii (Post 383238)
Hi all,

I am trying to solve the motion of particles in bubbles. The particles along with air are injected from an inlet into water. Therefore the air, which includes the particles, generates the bubble and the particles are trapped in the bubble. For the bubble motion I used VOF and for the particle motion DPM model. Now for the last step of my project I have to delete the particles in the bubble as soon as they impact the bubble surface... I wanna do this with UDF... The idea for this UDF is that I want to delete the particles as soon as the particles are in a cell with f>=0.5 This is the UDF I am using:

#include "udf.h"
#define REMOVE_PARTICLES TRUE
DEFINE_DPM_OUTPUT(discrete_phase_counter,header,fp ,p,t,plane)
{
cell_t c;
Thread *t;
#if REMOVE_PARTICLES /*This if loop removes the particles*/
if(C_VOF(c,t)<=0.5)
p->stream_index=-1;
#endif
#endif
}

I can compile this UDF in Fluent, however, it does not remove the particles... Since I have been working with self developed codes in FORTRAN and I am not an expert in writing UDFs, would you please let me know how I should change this UDF to delete the particles in cells with VOF fractions greater than 0.5. It should be mentioned that in VOF model in liquid f=1 and in air f=0.

With Regards,
Iman.
DEFINE_DPM_SCALAR_UPDATE(remove_particle,c,mix_t,i nitialize,p)
{
cell_t c;
int water_index = 0; /* primary phase index is 0 */
Thread *water_t = THREAD_SUB_THREAD(mix_t,water_index);
if(REMOVE_PARTICLES) /*This if loop removes the particles*/
{
if(C_VOF(c,water_t)>=0.5) p->stream_index=-1;
}
}

rk_k67 January 29, 2013 07:02
Storing the particles
 
Hi everyone,

stream_index gets rid of the particles from the domain. Does anyone know if there is there a way to get the properties and number of the removed particles removed from the flow ? Do we need to store them in an array or sth ? Thanks!

Cheers,

kanglele November 16, 2020 02:19
I don't know what's wrong？
 
Quote:
Originally Posted by imanmirzaii (Post 385574)
Hi alexsantan,

Yeah I solved the problem, this is the UDF I used and it works perfect:


#include "udf.h"

DEFINE_DPM_SCALAR_UPDATE(charge,c,t,initialize,p)
{
Thread *phase_t = THREAD_SUB_THREAD(t,1);

if(C_VOF(c,phase_t)>=0.5)
p->stream_index = -1;
}

/*
0 in phase_t represents primary phase. If you want to find VOF for
secondary phase, you will have to change 0 to 1.
*/
I copy you code into fluent16.1，it shows“line 8: structure reference not implemented”，I don't know what's wrong？

AlexanderZ November 16, 2020 04:43
compile code

kanglele November 17, 2020 03:58
Quote:
Originally Posted by AlexanderZ (Post 787877)
compile code
Thank you very much for your answer.
Yes， I compile code，but I meet new difficulty，the fluent16.1 show “fluent16.1.0\win64\2d\fl1610.lib : fatal error LNK1113: invalid machine type”.

AlexanderZ November 19, 2020 00:37
most likely, you've installed visual studio in wrong way

read this information
https://www.cfd-online.com/Wiki/Flue...UDF.29_Related

kanglele November 25, 2020 05:38
Quote:
Originally Posted by AlexanderZ (Post 788166)
most likely, you've installed visual studio in wrong way

read this information
https://www.cfd-online.com/Wiki/Flue...UDF.29_Related
I installed visual studio 2019 ，and from visual studio 2019 enter into fluent 16.1,the code could be build and load . Thank you very much.
But I have new problem. After adding the UDF, and I want fluent16.1 to show the particle trajectories. the following error occurs :
Error: received a fatal signal (Segmentation fault).
Error Object: #f.
(If I didn't add the UDF, there's no problem)

pakk November 25, 2020 14:23
And you are really using the VOF model?

kanglele November 25, 2020 19:27
Quote:
Originally Posted by pakk (Post 788859)
And you are really using the VOF model?
Yes，For the bubble motion I used VOF and for the particle motion DPM model. I have to delete the particles in the bubble as soon as they impact the bubble surface.


All times are GMT -4. The time now is 23:51.