[Saman95]

hello all dear

I want to calculate area weighted average of heat flux along the surface, so I write a udf to calculate temperature gradientin every cell adjacent to the surface, but it is wrong because the answer of ansys fluent is different
my udf is :

DEFINE_EXECUTE_AT_END(Direct)
{
int i,ID,zone[7] = { 10,9,8,7,6,5,4 };
float T_i=300.0,T_f=500.0;
float ds, A_by_es, flux,DTX=0.0,DTY=0.0;
float H_flux[7], A[ND_ND], es[ND_ND], dr0[ND_ND];
face_t f;
cell_t c0,c;
Thread *t0, *t;
Domain *d = Get_Domain(1);
FILE *fp;
fp = fopen("Data.txt", "w");
for (i = 0;i < 1;i++){
flux = 0.0;
ID = zone[i];
t = Lookup_Thread(d, ID);

begin_f_loop(f, t)
{
BOUNDARY_FACE_GEOMETRY(f, t, A, ds, es, A_by_es, dr0);
c0 = F_C0(f, t);
t0 = THREAD_T0(t);
C_T_RG(c0, t0);
DTX += C_T_RG(c0, t0)[0];
DTY+= C_T_RG(c0, t0)[1];
flux += fabs(C_T_RG(c0, t0)[0] * es[0]) + fabs(C_T_RG(c0, t0)[1] * es[1]);
}
end_f_loop(f, t)
H_flux[i] = (202.4*flux);

please help

[obscureed]

Hi Saman95,

A few points:
(1) You are only calculating the first zone in the current UDF, because of "for (i = 0;i < 1;i++){".
(2) We cannot see what you do with the data, because you have not included the end of the UDF. Don't forget to fclose.
(3) I think that fabs is inappropriate here.
(4) You are not currently getting an area-weighted average, nor a total integrated flux, because you are not making any use of the face area. "es" is a unit vector.
(5) I'm not sure where 202.4 comes from -- something to do with conductivity?
(6) The flux through the boundary face is not guaranteed to be related exactly to the temperature gradient in the cell, though you might hope that they would be closely correlated. Things get more complicated with turbulence, since a boundary-adjacent cell can contain both bulk fluid and a boundary layer -- but maybe your case is laminar (since you are using a single value of conductivity)?

If Fluent's calculations are what you want, then you will save yourself all sorts of trouble by using Fluent's version.

Good luck,
Ed

[Saman95]

Thanks
1-202.4 is conductivity.
2- my case is laminar.
3-I want to show just for one face,not all, so i use "for (i = 0;i < 1;i++)"
4-also, I use fclose and I finish my udf by }.(I wrote only main program)

[Saman95]

It's better to show my udf file:

#include"udf.h"
#include"sg.h"

DEFINE_EXECUTE_AT_END(Direct)
{
int i, ID, zone[7] = { 14,12,11,10,9,8,7 };
double ds, A_by_es, flux,DTX,DTY,Area;
double H_flux[7], A[ND_ND], es[ND_ND], dr0[ND_ND];
face_t f;
cell_t c0,c;
Thread *t0, *t;
Domain *d = Get_Domain(1);
FILE *fp;
fp = fopen("Data.txt", "w");
for (i = 0;i < 1;i++){
flux = 0.0;
DTX = 0.0;
DTY = 0.0;
Area = 0.0;
ID = zone[i];
t = Lookup_Thread(d, ID);

begin_f_loop(f, t)
{
BOUNDARY_FACE_GEOMETRY(f, t, A, ds, es, A_by_es, dr0);
Area += NV_MAG(A);
c0 = F_C0(f, t);
t0 = THREAD_T0(t);
C_T_RG(c0, t0);
DTX += C_T_RG(c0, t0)[0] * es[0] * NV_MAG(A);
DTY+= C_T_RG(c0, t0)[1] * es[1] * NV_MAG(A);
fprintf(fp, "%f\t %f\n", DTX,DTY);
flux += (C_T_RG(c0, t0)[0] * es[0]+ C_T_RG(c0, t0)[1] * es[1])* NV_MAG(A);
}
end_f_loop(f, t)
DTX /= Area;
DTY /= Area;
flux /= Area;
H_flux[i] = (202.4*flux);
Message("Wall %d:\t DTX=%f\t DTY=%f\t heat flux=%f\n", ID, DTX, DTY, H_flux[i]);
//fprintf(fp, "%f\n", H_flux[i]);
}
fclose(fp);
}


please give your Idea about this

[obscureed]

I think, bearing in mind my point (6), you should investigate BOUNDARY_HEAT_FLUX(f,t).

[Saman95]

Thank u

can u tell me how I can find this macro in ansys help. I can't find it.

where is it?

please write it's part

[obscureed]

Hi Saman95,

Unfortunately, it is not documented anywhere. I found it by looking in the Fluent header files -- it is in sg_mem.h.

I think you will find that it contains the thermal power [in watts] entering through the face, not a flux [in W/m2]. If you are aiming for a sum in parallel, you should only look at threads that pass the test:

if (BOUNDARY_FACE_THREAD_P(t) && !(THREAD_TYPE(t) == THREAD_F_JUMP)) { ... }

and you should only count the faces that pass the test:

if (PRINCIPAL_FACE_P(f, t)) { ... }

Obviously you need to check that it gives results that match Fluent's. (If your model is axi-symmetric, you might or might not need to multiply by a factor of 2*M_PI to get it to match.) Good luck!

Ed

[Saman95]

ok

I can't find it and have two questions

1- can u tell me how i can find (Fluent header files -- it is in sg_mem.h.)

2- Do u know how fluent calculate Area weighted average of heat flux o a wall, I saw theory guide of fluent for this, But my answer is different