[teguhtf]

Dear all,
I am new in UDF. I am trying to make different initial guess of temperature distribution in solid by using #DEFINE_INIT CODE in Fluent 17.2. I took the whole code from UDF Fluent Customization sample. I just make little modification. The case is 2D and the solid is in y- direction.
Do you have any advice?
However when the code is interpreted the error shows
Error: E:/profile_temp.c: line 8: parse error.
Thank you for your help
Here is my code


/************************************************** *********************
UDF for initializing flow field variables
************************************************** **********************/

#include "udf.h"
#define d 5

DEFINE_INIT(temp_prof_init,d)

{
cell_t c;
Thread *t;
real xc[ND_ND];
/* loop over all cell threads in the domain */
thread_loop_c(t,d)
{
/* loop over all cells */
begin_c_loop_all(c,t)
{
C_CENTROID(xc,c,t);
y = xc[1]
if (y < 0) /* y < 0 */
C_T(c,t) = 10.578*y +302.26;

else if (y <-5 )
C_T(c,t) = 4.6277*y + 300.46; /* y < -5 */

else
C_T(c,t) = 290;
}
end_c_loop_all(c,t)
}
}

[obscureed]

Hi Teguh,

Out of paranoia, I recommend you delete the blank line after the DEFINE_INIT line.

However, the problem is the "#define d 5" -- as you probably know, this is a preprocessor directive. It is basically a "find and replace". I am not sure what you intended this to achieve, but the result is that "DEFINE_INIT(my_init_func,d)" becomes "DEFINE_INIT(my_init_func,5)", which is not valid. Fluent needs a variable name d (and arranges for it to have type Domain*).

Good luck!
Ed

[teguhtf]

Dear obscureed,


Thank you for your suggestion. I have repaired the code. It works if the only one zone. Actually, I have two zones (Solid and Liquid zone). If I do not define zone ID the initial temperature of solid and fluid will be same. I attach the inital temperature and zone ID (Zone ID 4 is solid and zone ID -1 is liquid. I want to make the DEFINE_INIT works only in solid zone. What should I do for this problem?


Thank you for your help


Here is my new code


/************************************************** *********************
UDF for initializing flow field variables
************************************************** **********************/

#include "udf.h"

DEFINE_INIT(my_init_func,domain)

{
cell_t c;
Thread *t;
real xc[ND_ND];
real y;

/* loop over all cell threads in the domain */
thread_loop_c(t,domain)
{
/* loop over all cells */
begin_c_loop_all(c,t)
{
C_CENTROID(xc,c,t);
y = xc[1];

if ( y >= -0.293) /* 12-13 */
C_T(c,t) = 300;

else if ( y >= -0.984) /* 12-13 */
C_T(c,t) = 290;

else if ( y >= -2.992) /* 12-13 */
C_T(c,t) = 280;

else if ( y >= -9.98) /* 12-13 */
C_T(c,t) = 270;

else
C_T(c,t) = 260;

}
end_c_loop_all(c,t)
}
}

[obscureed]

Hi Teguh,

In UDFs, a "thread" is a cell zone or a face zone. (This becomes more complicated in multiphase models, but it will be OK for now.) So you are asking about how to find a specific thread, based on its ID number. For this, you do not want "thread_loop_c(t,domain){ /*... use t ...*/ }", which repeatedly evaluates the contents with each possible cell thread in t. Instead you want

t = Lookup_Thread(domain, 4);
/*... use t ...*/

By the way, a negative value for a cell ID would be very surprising to me. Please could you check this? Is it different after a mesh check and/or initialization?

Good luck!
Ed

[teguhtf]

Dear obscureed,

Thank you for your advice. It works good on several time. But, in the initial condition contour, fluent makes the same temperature field in every threat. How to solve that?

Best regards

[obscureed]

Hi Teguh,

I do not completely understand your question, but it sounds like you need to debug your own UDF code.

Good luck!
Ed