[a.apostoli]

Hi guys!
I would like to extract the shear stress of a precise region of my fluid domain at every time step of the simulation run on ANSYS Fluent. I'm used to do it defining the region of interest with an iso-surface or iso-clip and use the automatic export command to write the values on an ASCII file. In this particular simulation the mesh is moving (the motion is imposed by an UDF grid motion). So the iso-sufrace or iso-clip do not follow the movement. Does anybody know how to extract the values of stresses for moving nodes in the mesh? Is it possible to use a pointer (or something similar) to point a cell of the domain?
Thanks in advance for the help!

[D.M]

hi
i dont know if your region is a surface or not
but u can use the udf below to find the shear stress on a particular surface:

DEFINE_EXECUTE_AT_END(wall_shear_stress)
{
..............
BOUNDARY_FACE_GEOMETRY(f,tf,A,ds,es,A_by_es,dr0);
C_UDSI(c, t, 0) = sqrt(NV_MAG(F_STORAGE_R_N3V(f, tf, SV_WALL_SHEAR)) / (NV_MAG(A) * C_R(c, t)));
}

C_UDSI(c, t, 0) = sqrt(NV_MAG(F_STORAGE_R_N3V(f, tf, SV_WALL_SHEAR)) / (NV_MAG(A) * C_R(c, t))); this part calculate the shear stress on the face element of your face thread and save them in the center of the cell that the face element is already a part of it.

[Prikane]

Hello a.apostoli,

Since you are using UDF for dynamic mesh, somewhere in your UDF you should put the following part of code:

begin_f_loop(f, tf)
{
f_node_loop (f, tf, n)
{
node_p = F_NODE(f, tf, n) ;
X[f]=(NODE_X(node_p)) ;
Y[f]=(NODE_Y(node_p)) ;
}
sumshear += NV_MAG(F_STORAGE_R_N3V(f,tf, SV_WALL_SHEAR)) ;
}
end_f_loop(f, tf)

After you do this, you can extract ''sumshear'' variable in text file (e.g sumshear.txt) which you will create and locate in your Fluent folder, where are your case and data file located. For extraction, you can use the following code:

fx=fopen("sumshear.txt","w+") ;
fprintf(fx,"%E",sumshear) ;
fclose(fx) ;

Hope this will help you,

Prikane