CFD Online Discussion Forums - how to set up and write a cosine UDF

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- Fluent UDF and Scheme Programming (https://www.cfd-online.com/Forums/fluent-udf/)

- - how to set up and write a cosine UDF (https://www.cfd-online.com/Forums/fluent-udf/107169-how-set-up-write-cosine-udf.html)

how to set up and write a cosine UDF

Hello everybody,

i ve got a problem with my inlet boundary conditions. i want to implement a cosine (or sine) function because, i got a pulsative flow at the inlet. my flow changes every second from 0 to 20 m/s.
one possible function would be 10*cos(x*pi)+10 with 0<x<2.

Now, i just dont know how to setup this function in fluent and how and where to wirte it. I know that i have to define this function somewhere and upload it after in fluent. and how can i tell fluent that one period is like 4 seconds?

Would be really great if someone can help me with this.

regards, chris

You should read the Fluent UDF manual here:
http://hpce.iitm.ac.in/website/Manua...f/main_pre.htm

Alternatively you can create a Profile file with discrete velocity vs. time data and use that. See here:
http://hpce.iitm.ac.in/website/Manua...ug/node301.htm

ok thanks i`ll try it!

Quote:

Originally Posted by chriskit (Post 382563)

Hi,
I don't understand very well: your function should be time dependent but there isn't time in your function..what is x?time?
From what I understand I think you want to change velocity at inlet with a time dependent cos function.
If so, try this udf.

Code:

#include "udf.h"

#include "math.h"

#include "mem.h"



DEFINE_PROFILE(my_velocity, thread, position)

{

  face_t f;

  real t = CURRENT_TIME;



  begin_f_loop(f, thread)

    {

          F_PROFILE(f, thread, position) = 10.*cos(t*3.14159)+10.;

    }

  end_f_loop(f, thread)

}

Am I right?
If so copy this udf in a textedit file and save it as somename.c (not txt extension but c extension) and put it in the folder of your cas and dat files.
Open fluent and go to define->user-defined->functions->interpreted.
Choose the c file and interpret it.
Then in your velocity boundary condition choose your interpreted udf ("my_velocity").
Choose an appropriate time step for your unsteady simulation and stop it after some periods (you know 1 period is 2 seconds).

Also, I don't understand this:
..and how can i tell fluent that one period is like 4 seconds?

your period is 2 seconds not 4.
If I don't understand post a sketch of your domain and explain better.

Daniele

Hey Daniele,

thanks a lot! You understood it absolute right. And really thanks for the code, my knowledge at C and C++ isn´t that big...

So now, i made it like your proposal but the new problem is that "my_velocity" doesn`t appear at the boundary conditions. I think interpreting worked well but i can`t choose this condition.

Do you know what kind of problem could be the reason for that?

Thank you and regards,

chris

Quote:

Originally Posted by chriskit (Post 382946)

Hi Chris,
after interpreting your udf, go to boundary condition panel, choose your inlet, then change from "constant" to udf my_velocity.

PS: if you start your simulation with your function velocity at time=0 s is 20 m/s; you should perform a steady state simulation first, with v=constant=20 m/s than switch to unsteady and apply your cosine udf.

Daniele

ok great, thank you, now it works!!!