[enry]

Hi, I have a question:
I wanna calculate the entire force on a blade with Fluent for linux. The problem is a 2d rotating blade. Blade are modelling as an edge (and edge-shadow).
I write this UDF (It's my first UDF!!!! :-S ):

#include "udf.h"

DEFINE_ON_DEMAND(force_on_demand)
{
real force = 0.;
real NV_VEC(A);
int IDblades = 10;

face_t f;
Thread *f_thread;
Domain *d;

d = Get_Domain(3); /* Fluid ID */
f_thread = Lookup_Thread(d, IDblades);


begin_f_loop(f,f_thread)
{
F_AREA(A,f,f_thread);
force += F_P(f,f_thread) * NV_MAG(A);
}
end_f_loop(f,f_thread)

printf("\n FORCE = %g \n", force); */
}

but Fluent stamp an error :
fluent.6.3.26 received a fatal signal (segmentation violation)
Error Object: #f

Can somebody help me??!?!?!??!?!
Thanks!

[dmoroian]

Try to replace

d = Get_Domain(3); /* Fluid ID */
f_thread = Lookup_Thread(d, IDblades);

with

d = Get_Domain(3); /* Fluid ID */

if(NULL == d)
   Error("Something wrong with your domain id!\n");

f_thread = Lookup_Thread(d, IDblades);

if(NULL == f_thread || 
   !BOUNDARY_FACE_THREAD_P(f_thread))
       Error("Something wrong with your face id!\n");

But there is an already implemented force reporting facility accessible through the menus (report-forces).

[enry]

HI dmoroian;

I replace it, but Fluent finds an error in:

if(NULL == f_thread ||
!BOUNDARY_FACE_THREAD_P(f_thread))
Error("Something wrong with your face id!\n");

So I write replace it only with:

d = Get_Domain(3); /* Fluid ID */

if(NULL == d)
Error("Something wrong with your domain id!\n");

f_thread = Lookup_Thread(d, IDblades);

if(NULL == f_thread)
Error("Something wrong with your face id!\n");
This code runs on Fluent, but before running Fluent show this Error:


Error: C:\Documents and Settings\Enrico\Desktop\UDF windows\define_on_demand.c: line 32: function "CX_Primitive_Error" not found (pc=39).
Error: C:\Documents and Settings\Enrico\Desktop\UDF windows\define_on_demand.c: line 32: function "CX_Primitive_Error" not found (pc=67).
.entry




Of course I can do it through menu, but I have to calculate the mean-time moment coefficient on the blades, so I'm starting with easier code. (Do you know if there is any way to do it through menu?).
Thanks!

[enry]

HI! Sorry... I'm a beginner with UDF! Now I write this code :





#include "udf.h"

DEFINE_ON_DEMAND(force_on_demand)
{
real force = 0.;
real NV_VEC(A);
int IDblades = 10;

face_t f;
Thread *f_thread;
Domain *d;

d = Get_Domain(3); /* Fluid ID */

if(NULL == d)
printf("Something wrong with your domain id!\n");


f_thread = Lookup_Thread(d, IDblades);

if(NULL == f_thread)
printf("Something wrong with your face id!\n");


begin_f_loop(f,f_thread)
{
F_AREA(A,f,f_thread);
force += F_P(f,f_thread) * NV_MAG(A);
}
end_f_loop(f,f_thread)

/*printf("\n FORCE = %g \n", force);*/
}



Then I compile it (Define User-Defined Function Interpreted), and Fluent doesn't report any errors.
When I do "Execute on demand" Fluent report this message:

Something wrong with your domain id!
Something wrong with your face id!

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: ()






SO... something wrong! .... :-S

[enry]

I replace ID fluid domain with ID default-interior domain, and Fluent report FORCE!!!! =)

I have another question: do you know how can I calculate the moment-coefficient of the blade? ( the blade is a 1d blade, so I have also the blade-shadow). I have to calculate it in order to get the mean-time moment coefficient of the blade.

THANKS!

[qiyang860908]

I want to the process of the evaporation of water .So fluent may be a good tool.The problem is there is a interior cavitation model in fluent,and you can also write your own C files ,in other words ,the UDF program.BUt is there any difference between them?

[enry]

Sorry but, I can't answer... I never solve problem like that.

I have a question for you. Is it possible to match to the VISCOUS FORCE by UDF script?
I need to sum viscous force and pressur force. The command for pressur force is F_P(..), are there any command for viscous force?

[O.D.Y.]

you can let Fluent caluclate the moment-coefficient -> monitors
but you have to set proper reference values and the depth of the blade before....

[enry]

Yes, of course I can do that through Moment-coefficient - monitors, but I need Moment coefficient in a UDF in order to obtain the time average cm.
So I wrote a UDF function and I'm able to calculate the PRESSURE force through the command F_P (then I multiply F_P * moment arm = MOMENT), but I'm unable to calculate the VISCOUS force.
Do you know how I can do it?

[enry]

I solve my own problem with

Wall_Shear_Force_X = F_STORAGE_R_N3V(f,f_thread,SV_WALL_SHEAR)[0];
Wall_Shear_Force_Y = F_STORAGE_R_N3V(f,f_thread,SV_WALL_SHEAR)[1];

( I find these funcions on the web; they are NOT on UDF manual!!!! )

[Atze]

Hi enry,

i have to calculate pressure moment on my body. I've written
begin_f_loop(f,t)
{
F_CENTROID(x,f,t);
F_AREA(A,f,t);
NV_D(force, = ,A[0]*F_P(f,t),A[1]*F_P(f,t),0);
NV_CROSS(Mp,x,force);
NV_V(Mp_t,+=,Mp);
}
end_f_loop(f,t)

but something is wrong.... how did you calculate your pressure moments?

thanks