[Boh]

Hi!
In my simulation I have three different materials that constitute three different cell zones...if I want to loop over the cell zone of only one of the materials how should I do? Thanks!

[pakk]

In which context do you want to loop over the cell zones?

If for example you want to put a source term only in a certain cell zone, you are thinking too complex, because then you can just attach the udf only to that cell zone...

[Boh]

I need to calculate the mass of water that accumulates in a porous media...I did a thread loop over all domain's thread and inside a loop over all the cells of the thread and imposed the limitations on the domain using the x,y coordinates...but I thought that maybe there was a smarter way

[pakk]

Yes, there is a smarter way: use THREAD_ID.

thread_loop_f(f_thread, domain) {
 if (THREAD_ID(f_thread) == ID) {
  ... your code ...
 }
}

Replace "ID" by the number of the cell zone that you can find in Fluent.

[Boh]

Thanks for your help!

[macfly]

You can use Lookup_Thread instead and loop directly on the desired thread (no need for a conditional statement).

From the UDF manual:

You can use Lookup_Thread when you want to retrieve the pointer t to the thread that is associated with a given integer zone ID number for a boundary zone. The zone_ID that is passed to the macro is the zone number that ANSYS Fluent assigns to the boundary and displays in the boundary condition dialog box (for example, Fluid).

/*******************************************************************/
    Example of an adjust UDF that uses Lookup_Thread.
    Note that if this UDF is applied to a multiphase flow problem,
    the thread that is returned is the mixture-level thread
 ********************************************************************/
 #include "udf.h"
 /* domain passed to Adjust function is mixture domain for multiphase*/
 DEFINE_ADJUST(print_f_centroids, domain)
 {
    real FC[2];
    face_t f;
    int ID = 1;
    /* Zone ID for wall-1 zone from Boundary Conditions task page */
    Thread *thread = Lookup_Thread(domain, ID);
    begin_f_loop(f, thread)
    {
       F_CENTROID(FC,f,thread);
       printf("x-coord = %f y-coord = %f", FC[0], FC[1]);
    }
    end_f_loop(f,thread)
 }

For DEFINE_EXECUTE_AT_END or DEFINE_ON_DEMAND you need to add the Domain... line:

DEFINE_ON_DEMAND(on_demand_0)
{
#if !RP_HOST /* action not performed on host, only on compute nodes */
Domain *domain = Get_Domain(1); /* declare domain pointer since it is not passed as an argument to the DEFINE macro */
int Cell_Zone_ID = 13;
cell_t c;
Thread *t = Lookup_Thread(domain, Cell_Zone_ID);
begin_c_loop(c,t)
    {
    Message("looping over cells...\n");
    }
end_c_loop(c,t)
#endif
}

[vidyadhar]

Hello François Grégoire,


I want to apply energy source on one layer of liquid cells which are lying next to the liquid vapor interface.

Can you let me know how to do this.

I guess I cannot use LookupThread and Adjacent Cell thread (THREAD_T0) for this.


Thanks in advance!
Vidyadhar

[AlexanderZ]

as far as I know, you can get liquid-vapor interface if you are using Volume Of Fluid model (VOF). May be, you may get adjusted cells using macros for c1,t1

best regards

[vidyadhar]

Originally Posted by AlexanderZ

as far as I know, you can get liquid-vapor interface if you are using Volume Of Fluid model (VOF). May be, you may get adjusted cells using macros for c1,t1

best regards

Hello Alexander,


Thanks for the reply.


I am using VOF model. I can visualize interface. The interface is of the type "interior" in the fluid zone.

I request you to elaborate on "May be, you may get adjusted cells using macros for c1,t1"


Thanks & Regards,
Vidyadhar

[macfly]

Hi Vidyadhar,


I'm not working with Fluent anymore, don't have it on my computer, can't really help you, sorry.


François

[AlexanderZ]

make a loop over all face/threads, check F_VOF(f, t); value
if it varies in range 0 .. 1 , than this cell is interface

than you can check

if (BOUNDARY_FACE_THREAD_P(t))
{} // do nothing, because there is no cell outside the face
else
{
c1 = F_C1(f,t);
t1 = THREAD_T1(t);
F_UDMI(c1,t1,0) = your_source;
}

something like this

best regards

[ViLaks]

Hi,

Sorry for restarting the thread.
I am simulating flow through a capillary tube (3D) in Fluent and I would like to understand the variation in temperature and pressure across the length of the capillary.
The simple and tedious option would be to create multiple faces across the capillary (varying in 2 directions, say x and y) and report values at each face.

Is it possible to do this through UDFs?
I would like inputs in looping through cells in a particular domain and write values at fixed intervals, say 0.1 m or so

PS: My geometry is a coiled capillary

Thanks in Advance!!!

[AlexanderZ]

from your explanation it seems, that you don't need udf at all
you may create monitor points at locations you are interested in

if there are too many points, you may use TUI commands and journal file to make points by script