[cfdworker]

Hello, I have a problem with the definition of a boundary condition with UDF to simulation of the wind in a terrain. I have to define a velocity inlet in a 3d domain; this condition is a logarithmic velocity profile. I can define the logarithmic velocity profile with UDF, like this:



#include "udf.h"

DEFINE_PROFILE(log_velocity,thread,index)
{
real x[ND_ND];
real z;
face_t f;

begin_f_loop(f,thread)
{
F_CENTROID(x,f,thread);
z = x[2];
F_PROFILE(f,thread,index) = 3*log(z/0.01)/log(10/0.01);
}
end_f_loop(f,thread)
}


My domain is this:



I have to impose the logarithmic profile in the front face that is shown in figure.
My question is how I define in the UDF so that the velocity in bottom of the face is equal 0.
My problem is the coordinates that I use in UDF are absolute and I don’t know how to define relative coordinates, in order to the z in the equation that defines the velocity profile, is the height relatively to the bottom of the face and not the absolute height.

I would appreciate any suggestions.

[lalula2]

hi, i need help on creating UDF for logarithmic velocity profile for my final year project also. But i am not very familiar with c programming language...any good example for me to follow??
thanks

[lalula2]

Hi cfdworker....
since ur simulation problem is 3D, then how about the y vector??
and for the array part,shudnt it be 3D array??
Any pro or expert here mind to share their suggestion and opinion?
thanks.

[Häwimeddel]

I guess your boundary condition for the landscape ist WALL. To estimate the distace from any cell to the nearest WALL, you could maybe use C_WALL_DIST(c,t).

[cfdworker]

Hi, thanks for the reply. I tried to use the C_WALL_DIST(c,thread) macro like this:


#include "udf.h"

DEFINE_PROFILE(log_velocity,thread,index)
{
real z;
face_t f;
cell_t c;

begin_f_loop(f,thread)
{
z = C_WALL_DIST(c,thread);
F_PROFILE(f,thread,index) =3*log(z/0.01)/log((10)/0.01);
}
end_f_loop(f,thread)
}



But when i selected the udf in velocity inlet in boundary condition, fluent gave me this message:


Error:
FLUENT received fatal signal (ACCESS_VIOLATION)
1. Note exact events leading to error.
2. Save case/data under new name.
3. Exit program and restart to continue.
4. Report error to your distributor.
Error Object: ()



I think the problem is that the boundary condition that I set is to a face and I use a macro for cells in the udf.

I don’t know how to use this macro for my situation. Can anyone help me with this issue ?

Thanks in advance

[cfdworker]

Someone can help me. Please I need someone who is patient to help me with this problem.

Thanks.

[cfdworker]

I tried to make another udf, as shown:


#include "udf.h"

DEFINE_PROFILE(inlet_x_velocity, thread, position)
{
cell_t c;

begin_c_loop(c, thread)
{
C_PROFILE(c, thread, position) = 3.*log(C_WALL_DIST(c,thread)/(0.01))/log(10./(0.01));
}
end_c_loop(c, thread)
}

But gave me the same error message.
I want to use the distance between the faces centroids that were determined by the F_CENTROID(f,thread) macro in the first udf and the terrain, in the face where I have to impose the velocity profile. But the only macro i know that give an distance is the C_WALL_DIST(c,thread), and this is applied to cells. I don't Know how to determine the distance for faces, for my problem.

Please, i beg for help.

[coglione]

Hello,

try this one and let me know if it works. Having a look at the UDF-Manual section 3.2.5 might also help.

#include "udf.h"

DEFINE_PROFILE(log_velocity,thread,index)
{
real z;
face_t f;
cell_t c;
Thread *tc;

begin_f_loop(f,thread)
{
c = F_C0(f,thread);
tc = THREAD_T0(f,thread);
z = C_WALL_DIST(c,tc);
F_PROFILE(f,thread,index) =3*log(z/0.01)/log((10)/0.01);
}
end_f_loop(f,thread)
}

cheers

[cfdworker]

hello, thanks for the reply. I used your udf, but still gives the same error message, when I do init to start iterate.

Error:
FLUENT received fatal signal (ACCESS_VIOLATION)
1. Note exact events leading to error.
2. Save case/data under new name.
3. Exit program and restart to continue.
4. Report error to your distributor.
Error Object: ()

[coglione]

Hm,
seems like Fluent does not recognize C_WALL_DIST() at all. Is your case laminar or turbulent? It might be that C_WALL_DIST() is only available if a turbulence model is activated.

cheers

[cfdworker]

My case is turbulent. I think that the fluent recognizes the macro, i think that the problem is in using macro for cells in a boundary condition that is imposed in a face. I do not know if this is the problem. What do you think ?

Thanks

[coglione]

No, F_C0 and THREAD_T0 give you cell index and cell thread of the adjacent cell to each face at your boundary which is o.k. You can try the following:

type solve/set/expert in the text user interface of Fluent and enter yes if asked to keep temporary memory from being freed. Maybe a DEFINE_PROFILE macro for velocity i.e. applied for momentum equation does not has default access to C_WALL_DIST which is relevant for turbulence.

Hope this helps

[cfdworker]

I already did what you said, but even so it gives the same error message.

Thanks for the replys.

[coglione]

Hi again,

it seems like you have to do some testing what the actual problem is.

If you replace C_WALL_DIST with for example C_CENTROID: does it work? This would indicate that C_WALL_DIST is to blame

If so, try to hook your DEFINE_PROFILE for one of the turbulence variables, e.g. k, and check whether it works then. If yes you could iterate one single iteration/timestep, store the cell wall distance in a UDM and proceed with your velocity-profile-udf using this values.

cheers

[cfdworker]

Hello. I did what you said. I replace C_WALL_DIST for C_CENTROID, but still gives the same error.

[coglione]

Well, then something more fundamental is wrong with your udf. If you compile your udf, what does the log-file say? Everything ok or some warnings?

cheers

[cfdworker]

Hello.
I found a alternative way to define the velocity profile for my problem.
What I did was, first write out a profile file at the inlet boundary, then obtain a profile file, which contains vectores of x,y,z,cell wall distance and velocity magnitude, then I read the file with excel and replace the velocity magnitude by a function of cell wall distance (which is the logarithmic function for velocity profile). Then i save the altered data and read this back to fluent as profile. Finally, then I used these profiles as boundary conditions for the inlet.

Thanks for the replys.

[lalula2]

hi there, how to use fluent to read the altered data??
mind to share??
Thanks.

[mrn]

dear cfdworker,
i have a problem same as your case and i have to define logarithmic velocity inlet at the beginning of cylindrical pipe.but unfortunately i have a error when i want to hook this udf and set as velocity inlet in boundary condition panel or it doesn't iterate( error is invalid number?!).please tell me how i can solve my problem.i have wrote the udf as below.velocity inlet is in y direction.

#include "udf.h"

DEFINE_PROFILE(inlet_y_velocity, thread, position)

{

real xc[ND_ND];

real ro,mu_t,visc_t,x,y,z,a,r,rw,utaw,rbi,yplus,b;

cell_t c;
face_t f;
ro = C_R(c,thread);
mu_t = C_MU_T(c,thread);
visc_t=mu_t/ro;

begin_f_loop(f, thread)

{

F_CENTROID(xc,f,thread);

x = xc[0];
y = xc[1];
z = xc[2];

rw=0.5;
utaw=0.0176;
r=sqrt(pow(x,2)+pow(z,2));
rbi=r/rw;
yplus=utaw*r/visc_t;

b=(1.5*yplus*(1+rbi))/(1+2*pow(rbi,2.));


F_PROFILE(f, thread, position) = utaw*(2.5*log(b)+5.5);

}

end_f_loop(f, thread)

}