[erfan2000]

Hello dear all
I have a case that consists of several parts. I want to get the maximum temperature in each time step and if it is over 320K I want to increase my inlet velocity. would you please help me to get the maximum temperature of all zones as tmax?
thanks a lot
Here is my UDF until now:

DEFINE_PROFILE(InletVelocity, t, i)
{
face_t f;
begin_f_loop (f,t)
{
	if (tmax>=320)
		F_PROFILE(f,t,i) = 0.005;
	else
		F_PROFILE(f,t,i) = 0.002;
}
end_f_loop(f,t)
}

[AlexanderZ]

you may find the example to start with in ansys fluent customization manual
look for DEFINE_ON_DEMAND

[erfan2000]

Thank you dear Alexander
I changed my code to this:

real tmax = 0.;

DEFINE_ON_DEMAND(on_demand_calc)
{
Domain *d; /* declare domain pointer since it is not passed as an
argument to the DEFINE macro */
real temp,volume,vol_tot;
Thread *t;
cell_t c;
d = Get_Domain(34); /* Get the domain using ANSYS Fluent utility */
/* Loop over all cell threads in the domain */
thread_loop_c(t,d)
{
/* Compute max, min, volume-averaged temperature */
/* Loop over all cells */
begin_c_loop(c,t)
{
volume = C_VOLUME(c,t); /* get cell volume */
temp = C_T(c,t); /* get cell temperature */
if (temp > tmax || tmax == 0.) tmax = temp;
}
end_c_loop(c,t)
printf("\n  Tmax = %g",tmax);
}
} 

DEFINE_PROFILE(InletVelocity, t, i)
{
face_t f;
begin_f_loop (f,t)
{
	if (tmax>=320)
		F_PROFILE(f,t,i) = 0.005;
	else
		F_PROFILE(f,t,i) = 0.002;
}
end_f_loop(f,t)
}

Is everything OK?
thanks for helping

[AlexanderZ]

to check if your UDF is OK or not you should:
1. compile code
2. run it
3. read log in console

few modifications were made on assumption that under Get_Domain(34) you wanted to check the temperature of zone 34
that id must be the the id of zone not boundary, because you are using loop over cells (volumes) but not faces, in case id 34 belongs to boundary you should change begin_c_loop to begin_f_loop

compile code

#include "udf.h"
real tmax = 0.;

DEFINE_ON_DEMAND(on_demand_calc)
{
Domain *d;
real temp;
int ID = 34;
Thread *t;
cell_t c;
d = Get_Domain(1); /* Get the domain using ANSYS Fluent utility */
t = Lookup_Thread(domain, ID);
/* Loop over all cell threads in the domain */

begin_c_loop(c,t)
{
temp = C_T(c,t); /* get cell temperature */
if (temp > tmax || tmax == 0.) tmax = temp;
}
end_c_loop(c,t)
# if RP_NODE /* Perform node synchronized actions here. Does nothing in Serial */
tmax = PRF_GRHIGH1(tmax);
# endif /* RP_NODE */
Message0("\n  Tmax = %g",tmax);
} 

DEFINE_PROFILE(InletVelocity, t, i)
{
face_t f;
begin_f_loop (f,t)
{
	if (tmax>=320)
		F_PROFILE(f,t,i) = 0.005;
	else
		F_PROFILE(f,t,i) = 0.002;
}
end_f_loop(f,t)
}

[erfan2000]

I’m so grateful for your help. It was a challenging time but you made it easier. Thank you.

[erfan2000]

Dear Alexander
I face this error: "MPT_gdhigh1: no function prototype" in the line

tmax = PRF_GRHIGH1(tmax);

do you know how can I fix it?
thank in advanced

[pakk]

That sounds like an error message when you interpret. You should not interpret, you should compile.