[MiBe]

Hello everyone,
I have been trying for hours to write a DEFINE_PROFILE UDF which takes the Species Mass Fraction of 4 out of 5 species from boundary-adjacent cells and imposes the same concentration on the boundary. This is to simulate a flow with one wall of a 2d-duct replaced by a velocity-inlet with normal velocity=0. Imposing the concentrations from the steady case as profiles on the boundary does not give the desired results. I have been working with a c_face_loop. Here is my UDF. It compiles and runs, but does not give the desired results. I am thankful for any suggestion!

#include "udf.h"

DEFINE_PROFILE(O2_concentration, thread, position)
{

cell_t c;
Thread *t;
face_t f;
Thread *tf;
int n;

c_face_loop(c,t,n)
{
c0_thread=THREAD_T0(thread);
if(THREAD_TYPE(tf) == THREAD_F_WALL)
{
f = C_FACE(c,t,n);
t = C_FACE_THREAD(c,t,n);
F_PROFILE(f, thread, position) = C_YI(c0,c0_thread,n);
}
}
}

[MayTheFlowBeWithYou]

I have had the same issue a while back, spend days on it, I'll save you from this. Here is the answer:


#include "udf.h"
#include "mem.h"
#include "metric.h"
#include "sg_mem.h"

/* MODEL FOR OUTLET PROFILES*/

DEFINE_PROFILE(Outlet_UDS, t, i)
{
Thread *t0;
face_t f;
cell_t c, c0;

begin_f_loop(f, t)
{
t0 = THREAD_T0(t);
c0 = F_C0(f, t);

/********** DEFINING PROFILE **********/
F_PROFILE(f, t, i) = C_UDSI(c0, t0, i); /* Lets hope this works. */
}
end_f_loop(f, t)
}


P.S. I know I probably #include too much stuff, I just never cared to optimize.
P.P.S. c_face_loop will loop over all the faces of the cells (in a 2d situation, each cell will have 4 faces). Looping over all 4 faces of each cell of your boundary and then setting the adjacent cell to each of those faces will indeed not give you the desired results. Frankly, I'm amazed it didn't just crash.
P.P.P.S. The last term in DEFINE_PROFILE is not a position, it's an index given by fluent to each UDS.

[MiBe]

Hello,

thank you very much for your detailed explanation and especially for the provided example code. I have been trying to use this function both, as is and with different minor changes, as an input for the species mass fractions on a velocity-inlet. The compiled function can be read, but as soon as I try to impose it as a boundary condition in the velocity-inlet toolbox, I get the error message shown in the screenshot: <received fatal signal (Segmentation fault).>
do you remember how you solved this problem? I have tried

F_PROFILE(f, thread, position) = F_YI(f,thread,i);

but without getting a good result. The velocity magnitude is set to 0, could this cause the problem?

Thank you very much for your help so far!
Michael

[MayTheFlowBeWithYou]

Well, first of all, the "segmentation error" can be caused by 100's of different things, and practically doesn't tell you much more than "something doesn't work". I have found stupid things like the order in which variables are defined to even cause this sometimes. In my opinion it just shows that ANSYS did a lazy job in the error reporting of Fluent, and thus everything was just shoved under "segmentation error".

My code was intended for when you used a User-Defined Scalar instead of species, perhaps using:

F_PROFILE(f, t, i) = C_YI(c0, t0, i);

instead of

F_PROFILE(f, t, i) = C_UDSI(c0, t0, i);

will make it work for you? What the code is basically trying to do now is to impose the values of the cells next to the boundary upon the faces of the boundary itself. Chapter "1.6. Mesh Terminology" of the Customization guide for Fluent has a nice explanation of the difference between cells, faces and nodes. This might help you in choosing the correct macros in the future as well.