[JannisSif]

Hi!

I am trying to create a udf which finds the average temperature at the outlet of the domain and then applies it to the inlet (increased by 7.58). I wrote the following udf but in the DEFINE_PROFILE the c_udmi returns zero and thus the F_PROFILE(f,t,nv) gets equal to 7.58 constantly......can someone help please??



DEFINE_EXECUTE_AT_END(average_exit_temp)
{
face_t f;
cell_t c0;
Domain *d=Get_Domain(1);
Thread *t=Lookup_Thread(d,8), *t0;
real vol=0, tavg=0, temp=0, vol_tot=0;
t0=THREAD_T0(t);

begin_f_loop(f,t)
{
c0=F_C0(f,t);
vol=C_VOLUME(c0,t0);
vol_tot+=vol;
temp=C_T(c0,t0);
tavg+=temp*vol;
}
end_f_loop(f,t)

tavg/=vol_tot;

begin_f_loop(f,t)
{
c0=F_C0(f,t);
C_UDMI(c0,t,0)= tavg;
printf("\n Average temperature is: %g\n",C_UDMI(c0,t,0));
}
end_f_loop(f,t)
}




DEFINE_PROFILE(inlet_temperature, t, nv)
{
face_t f;
Thread *t0;
cell_t c0;
real tavg;
t0=THREAD_T0(t);

begin_f_loop(f,t)
{
c0=F_C0(f,t);
F_PROFILE(f,t,nv)= C_UDMI(c0,t0,0) + 7.58;

printf("\n Inlet temperature is: %g\n",F_PROFILE(f,t,nv));
}
end_f_loop(f,t)

}

[blackmask]

You just need to store one value "tavg", what do you need a "UDM" for? You can simply declare "tavg" in the file scope.

The "c0" in "DEFINE_PROFILE" is the cell index adjacent to inlet boundary, which has no overlap with cell index adjacent to outlet boundary. Suppose there is a grid with 100*100 cells and is number from top left to bottom right. The inlet and outlet boundary are located at the left and right ends, respectively. Then in the "DEFINE_EXECUTE_AT_END" you assigned values for cells with index ranging 9900 to 9999, then in the "DEFINE_PROFILE" you obtain values from cells with index ranging 0 to 99.

[JannisSif]

Originally Posted by blackmask

You just need to store one value "tavg", what do you need a "UDM" for? You can simply declare "tavg" in the file scope.

Hi blackmask and thank you very much for the reply. I am very new to udfs and so I am a little confused....


So as far as I understood from what you wrote, in my case, I could use the following code, wright?


#include "udf.h"

real tavg=280.;

DEFINE_EXECUTE_AT_END(average_exit_temp)
{
face_t f;
cell_t c0;
Domain *d=Get_Domain(1);
Thread *t=Lookup_Thread(d,8), *t0;
real vol=0, temp=0, vol_tot=0;
t0=THREAD_T0(t);

begin_f_loop(f,t)
{
c0=F_C0(f,t);
vol=C_VOLUME(c0,t0);
vol_tot+=vol;
temp=C_T(c0,t0);
tavg+=temp*vol;
}
end_f_loop(f,t)

tavg/=vol_tot;
}



DEFINE_PROFILE(inlet_temperature, t, nv)
{
face_t f;

begin_f_loop(f,t)
{
F_PROFILE(f,t,nv)= tavg + 7.58;
printf("\n Inlet temperature is: %g\n",F_PROFILE(f,t,nv));
}
end_f_loop(f,t)

}


The problem is though that although it is interpreted without a problem, when I start the calculation I get a "floating poitn axception error". Also the "printf" I used says that "Inlet temperature is: inf"......what could be the problem?

Thank you very much for your time!

[blackmask]

You should check whether the thread is empty or the sum of volume is non-zero. What is the output of the code below?

#include "udf.h"

real tavg=280.0;

DEFINE_EXECUTE_AT_END(average_exit_temp)
{
    face_t f;
    cell_t c0;
    Domain *d=Get_Domain(1);
    Thread *t=Lookup_Thread(d,8), *t0;
    real vol=0, temp=0, vol_tot=0;
    t0=THREAD_T0(t);

    Message("number of faces: %d\n", THREAD_N_ELEMENTS(t));

    begin_f_loop(f,t)
    {
        c0 = F_C0(f,t);
        vol = C_VOLUME(c0,t0);
        vol_tot += vol;
        temp = C_T(c0,t0);
        tavg += temp*vol;
    }
    end_f_loop(f,t);

    Message("sum of volumes: %g\n", vol_tot);

    tavg /= vol_tot;
}



DEFINE_PROFILE(inlet_temperature1, t, nv)
{
    face_t f;

    begin_f_loop(f,t)
    {
        F_PROFILE(f,t,nv)= tavg + 7.58;
        printf("\n Inlet temperature is: %g\n",F_PROFILE(f,t,nv));
    }
    end_f_loop(f,t)

}

[JannisSif]

So I run the code (actually changed the "message" with "printf" because I could not interpret it) and it printed this:

number of faces: 0
sum of volumes: 0
number of faces: 0
sum of volumes: 0
number of faces: 0
sum of volumes: 0
number of faces: 6
sum of volumes: 1.33696e-07
number of faces: 0
sum of volumes: 0

[blackmask]

The thread id (8) could be wrong. Please check.

[JannisSif]

I just checked, it is correct (8) for the outlet of the domain.....

[blackmask]

You can use the following code (just paste them to the the fluent TUI, i.e., the console below the graphics window)

(rp-var-define 'jos-thread-id-list () 'list #f) 
(rpsetvar 'jos-thread-id-list ()) 
(for-each (lambda (t) (rpsetvar 'jos-thread-id-list (list-add 
(rpgetvar 'jos-thread-id-list) (thread-id t)))) 
(get-all-threads)) 
(rpgetvar 'jos-thread-id-list) 


(rp-var-define 'jos-thread-name-list () 'list #f) 
(rpsetvar 'jos-thread-name-list ()) 
(for-each (lambda (t) (rpsetvar 'jos-thread-name-list (list-add 
(rpgetvar 'jos-thread-name-list) (thread-name t)))) 
(get-all-threads)) 
(rpgetvar 'jos-thread-name-list)

to get the list of zone names and their ids. What is the output?

[AlexanderZ]

Originally Posted by JannisSif

So I run the code (actually changed the "message" with "printf" because I could not interpret it) and it printed this:

number of faces: 0
sum of volumes: 0
number of faces: 0
sum of volumes: 0
number of faces: 0
sum of volumes: 0
number of faces: 6
sum of volumes: 1.33696e-07
number of faces: 0
sum of volumes: 0

why do you have 5 output messages?
Are you using 5 cores?

best regards

[JannisSif]

Originally Posted by blackmask

to get the list of zone names and their ids. What is the output?

The output is:

jos-thread-id-list

> jos-thread-id-list

>
> (6 3 14 2 8 7 13 1 9 10 11 12 5)

> adapt/ file/ solve/
adjoint/ mesh/ surface/
close-fluent parallel/ views/
define/ plot/
display/ report/

> adapt/ file/ solve/
adjoint/ mesh/ surface/
close-fluent parallel/ views/
define/ plot/
display/ report/

> jos-thread-name-list

> jos-thread-name-list

>
> (zone_wall part_4-surface_body interior-zone_wall-shadow interior-zone_wall outlet inlet symmetry interior-part_4-surface_body wall_tank-part_4-surface_body-zone_wall wall_tank-zone_wall plates-part_4-surface_body plates-zone_wall wall_tank-part_4-surface_body-zone_wall-shadow)

>

[JannisSif]

Originally Posted by AlexanderZ

why do you have 5 output messages?
Are you using 5 cores?

best regards

Hi Alexander,

I am running on 4 cores (not sure why I have 5 messages....)

thank you.

[blackmask]

Did not see that coming. Please try the following code:

#include "udf.h"

real tavg=280.0;

DEFINE_EXECUTE_AT_END(average_exit_temp)
{
    face_t f;
    cell_t c0;
    Domain *d=Get_Domain(1);
    Thread *t=Lookup_Thread(d,8), *t0;
    real vol=0, temp=0, vol_tot=0;
    t0=THREAD_T0(t);

    tavg = 0.0;
#if RP_NODE || !PARALLEL
    begin_f_loop(f,t)
    {
        c0 = F_C0(f,t);
        vol = C_VOLUME(c0,t0);
        vol_tot += vol;
        temp = C_T(c0,t0);
        tavg += temp*vol;
    }
    end_f_loop(f,t);

    tavg = PRF_GRSUM1(tavg);
    vol_tot = PRF_GRSUM1(vol_tot);
    tavg /= vol_tot;

    Message("processor: %d,tavg: %g\n", myid, vol_tot);
#endif
}



DEFINE_PROFILE(inlet_temperature1, t, nv)
{
    face_t f;
#if RP_NODE || !PARALLEL
    begin_f_loop(f,t)
    {
        F_PROFILE(f,t,nv)= tavg + 7.58;
        printf("\n Inlet temperature is: %g\n",F_PROFILE(f,t,nv));
    }
    end_f_loop(f,t)
#endif
}

[JannisSif]

Originally Posted by blackmask

Did not see that coming. Please try the following code:

Thank you so much for your help! I tried the code you sent me but I got an error "MPT_gssum1: no function prototype"

[blackmask]

The error does not occur if you can use compiled UDF. Otherwise it might need a work-around.

[JannisSif]

Originally Posted by blackmask

The error does not occur if you can use compiled UDF. Otherwise it might need a work-around.

Yes you are absolutely right! It worked fine!!! Thank you so much!

So just to understand exactly what happened, the problem was that each core was calculating a different value? Or something else?

[blackmask]

The solver processes are composed of one host node plus n (n=4 in your case) computing nodes. The host process definitely have no data of your outlet thread, so it will always result in 0./0. (i.e., FPE error you have encountered). Depending on the mesh partition, the computing node may or may not have data of your outlet thread, so it may cause FPE. Besides, the (temperature*volume) and (volume) should be summed from all computing nodes and then compute the average value, which is done with PRF_GRSUM1.

[JannisSif]

Originally Posted by blackmask

The solver processes are composed of one host node plus n (n=4 in your case) computing nodes. The host process definitely have no data of your outlet thread, so it will always result in 0./0. (i.e., FPE error you have encountered). Depending on the mesh partition, the computing node may or may not have data of your outlet thread, so it may cause FPE. Besides, the (temperature*volume) and (volume) should be summed from all computing nodes and then compute the average value, which is done with PRF_GRSUM1.

Thank you very much for your time and help!! Have a nice day!

Best regards,
Jannis