[Alex90]

Hi Guys, I am relativeley new to Ansys Fluent UDF Scripting and so far I did not get very far with my code ...

So what is my problem. I want to define an axial profile of the wall heat flux. I have a 4000mm long cylinder within Ansys the axis is orientated into z direction. The crux is that I have a constant wall heat flux within specific distances. For example from z>=0 to z<=300mm the heat flux q=0 and from z>300 to z<=600 the heat flux q=4738.666 .... and so on ....

Here is what I scripted so far :

#include "udf.h"
Define_Profile(heat_flux,thread,i)
{
face_t f;
begin_f_loop(f,thread)
{
if(x[2] <= 300)
F_PROFILE(f,thread,i) = 0;
else if(x[2] <= 600 && x[2] > 300)
F_PROFILE(f,thread,i) = 3500.955;
else if(x[2] <= 1050 && x[2] > 600)
F_PROFILE(f,thread,i) = 4738.666;
else if(x[2] <= 2100 && x[2] > 1050)
F_PROFILE(f,thread,i) = 4971.053;
else if(x[2] <= 2850 && x[2] > 2100)
F_PROFILE(f,thread,i) = 5092.298;
else if(x[2] <= 3300 && x[2] > 2850)
F_PROFILE(f,thread,i) = 4738.666;
else if(x[2] <= 3600 && x[2] > 3300)
F_PROFILE(f,thread,i) = 3500.955;
else if(x[2] <= 3900 && x[2] > 3600)
F_PROFILE(f,thread,i) = 2121.791;
else
F_PROFILE(f,thread,i) = 0;
}
end_f_loop(f,thread);
}


Unfortanetley this does not work. I wrote this with the code blocks editor and saved it as heat_flux.c , afterwards I compiled this within Fluent.
I got the following failure :
line 1 parse error ....

Can someone please help me with finding the failure. Thank you ...

[ghost82]

Hi
you didn't hold the position vector.
Add

real x[ND_ND];

before face_t f

Define_Profile(heat_flux,thread,i) should be uppercase DEFINE_PROFILE(....)

Daniele

[flotus1]

After you added this, I think you still need to write the current face position to the variable x by adding

F_CENTROID (x,f,thread);

at the beginning of the face loop.

[Alex90]

Hi guys, i added what ghost82 wrote and tried it again. This time Fluent compiled it without failure. I did a steady calculation which finished after 1 iteration ... Post-Processing the results their is no single Heat Flux all over my geometry. I have the feeling that i did not specify geometry as flotus1 suggested ... so here is my second code :


#include "udf.h"
DEFINE_PROFILE(heat_flux,thread,i)
{
real x[ND_ND];
face_t f;
begin_f_loop(f,thread)
{
F_CENTROID (x,f,thread);
if(x[2] <= 300)
F_PROFILE(f,thread,i) = 0;
else if(x[2] <= 600 && x[2] > 300)
F_PROFILE(f,thread,i) = 3500.955;
else if(x[2] <= 1050 && x[2] > 600)
F_PROFILE(f,thread,i) = 4738.666;
else if(x[2] <= 2100 && x[2] > 1050)
F_PROFILE(f,thread,i) = 4971.053;
else if(x[2] <= 2850 && x[2] > 2100)
F_PROFILE(f,thread,i) = 5092.298;
else if(x[2] <= 3300 && x[2] > 2850)
F_PROFILE(f,thread,i) = 4738.666;
else if(x[2] <= 3600 && x[2] > 3300)
F_PROFILE(f,thread,i) = 3500.955;
else if(x[2] <= 3900 && x[2] > 3600)
F_PROFILE(f,thread,i) = 2121.791;
else
F_PROFILE(f,thread,i) = 0;
}
end_f_loop(f,thread);
}


Thank you for your fast answers and your support

[ghost82]

1 iteration??
Adjust number of iterations in the run tab and adjust residual values in the monitor tab to let the solution converge.

[Alex90]

I addjusted the iterations number before the calculation to 100 ... I will try the residuals now ...

[flotus1]

Did you add what I suggested? Otherwise the heat flux will be zero everywhere and it comes as no surprise that the solution of the energy equation converges after 1 iteration.

[Alex90]

Hi Flotus you mean F_CENTROID ? ....


#include "udf.h"
DEFINE_PROFILE(heat_flux,thread,i)
{
real x[ND_ND];
face_t f;
begin_f_loop(f,thread)
{
F_CENTROID (x,f,thread);
if(x[2] <= 300)
F_PROFILE(f,thread,i) = 0;

[flotus1]

Yes.
Additionally, keep in mind that Fluent expects values to be in SI-units. So "if(x[2] <= 300)" checks if the z-value is smaller than 300m.
Just to be sure I would rather enter these values with a decimal point, so 300.0 instead of 300 and F_PROFILE(f,thread,i) = 0.0; instead of F_PROFILE(f,thread,i) = 0;

[SHREEKANT]

I went through all your healthy discussions...
I want to give different heat flux values in a pipe in a angular way like,upper part of pipe receiving more heat than lower part.

That is, upper portion of 270 deg. receiving 550W/m2 and lower 90 deg. receiving 20000W/m2 of heat.

can anyone help me out of this issue?

[brunoc]

Originally Posted by SHREEKANT

I went through all your healthy discussions...
I want to give different heat flux values in a pipe in a angular way like,upper part of pipe receiving more heat than lower part.

That is, upper portion of 270 deg. receiving 550W/m2 and lower 90 deg. receiving 20000W/m2 of heat.

can anyone help me out of this issue?

No need to use UDFs here. Just split your pipe into upper and lower regions, then set different boundary conditions at those.

[SHREEKANT]

Originally Posted by brunoc

No need to use UDFs here. Just split your pipe into upper and lower regions, then set different boundary conditions at those.

Hi Brunoc,
Thank you for the reply. In that case, I am afraid about the ways by which inlet and outlet boundary condition can be given, as it is split as two halves. I have a mass flow inlet at the entrance section.

[hussein92]

hi !!
my module is cooling PV cell
so the heat flux will be q*(1-efficiency of pv )
but the efficiency is function of temperature of pv T cell
efficincy= efficincy-ref *(1-0.004(T of cell -T ref))
how i can defined that in fluen

[Shamoon Jamshed]

I want to test two models. One model is full circular pipe with solid wall modeled and has a heat flux of 3500 on its top wall.
Second model is 1/10 th of the circumference extruded in third dimension to get the pipe length. This also contains the solid mesh. The outer wall is again supplied with 3500 heat flux. The sides are periodic (rot. periodic)
Now I want to compute Tw at the interface and Tout at outlet and difference between the two. such that delta T = (Tw- (298.15+To)*0.5). 298.15 K is the inlet temperature.
Q: Why the delta T is different for two cases? Should I take some other flux value when modeling 1/10th of the geometry.