UDF for 2d translational motion
 

Hi all,

I am relatively new to ANSYS Fluent and am trying to impose a simple UDF to move a disturbance through a fluid. I only require the disturbance to move in the x direction with a constant velocity.

Could anyone please point me in the right direction about how to write this UDF?

Thanks

Profiles instead
 

This is a udf for X-velocity (3D)

#include<udf.h>
DEFINE_CG_MOTION(velo_needle, dt, cg_vel, cg_omega, time, dtime)
{

cg_vel[0] = -0.6; /* x-velocity*/
cg_vel[1] = 0.0;
cg_vel[2] = 0.0;
NV_S (cg_omega, =, 0.0); /* no angular motion */
/* Messages in Fluent TUI */
Message(" \n");
Message("velocity \n");
Message("%5.6f\t\n",cg_vel[0]);
Message(" \n");
}

However, Fluent support advised me to use profiles files for this kind of motion (i.e. non force driven motions)... It's easier since you do not have to compile your udf or have to keep the files together, etc.

Since I discovered the use of profiles for transient motions my life has changed :D

Marion.

Hi Saeed, I have emailed you.
Thanks.

Marion:
'Fluent support advised me to use profiles files for this kind of motion'

Thanks for the reply. Do you have any resources on using profiles to specify translation?

Its pretty frustrating it seems like a relatively simply problem to move an object at a constant velocity in one dimension however the simulation is becoming difficult and cumbersome.

Have you tried the udf I gave you yesterday and it is not working? Maybe you have an issue with compiling udfs?
For the profile files, there is a section about this in the user guide, but here is a copy of a recent reply I posted on this forum:

For the profile:
you have to write it like this and save it as filename.prof:
disp_needle 2 10 0
time x
0.00000E+00 0.00000E+00
1.00000E-06 -1.20000E-07
2.00000E-06 -2.40000E-07
3.00000E-06 -3.60000E-07
4.00000E-06 -4.80000E-07
5.00000E-06 -6.00000E-07
6.00000E-06 -7.20000E-07
7.00000E-06 -8.40000E-07
8.00000E-06 -9.60000E-07
9.00000E-06 -1.08000E-06

where
*disp_needle--> name of the profile
*2 --> number of columns
*10 --> number of points
*0 --> for periodicity - 0=not periodic and 1=periodic

once you've created this file, within Fluent TUI you type
file
rtt
filename.prof
(make sure everything is in your working directory)

and then in the fluent dynamic mesh panel, choose disp_needle in the drop down list under "profile/udf".

As it is displacement vs. time the 1st column has to be time. the 2nd column can be displacement (x,y,z) velocity (v_x, v_y, v_z) , etc...

I hope this helps,

Marion.

Simple UDF motion
 

Like Carlos, I'm trying to impose a simple UDF for moving a body through a fluid. I require only your body moving in the X direction with a constant speed, this movement is caused by fluid entering the duct. Carlos, you could help in achieving this UDF, or guide in performing the same.

I leave a picture

Like you I would like to learn the use of profiles for transient motions :).
Thanks !!

I am trying to use profile by entering the velocity_y and time data points from matlab using step time as 0.000041667s. To get the rigid body motion as needed.
I use the layering - dynamic mesh type

When I see the zone motion - preview it work 254mm distance in 60millisec(30 millisec it move remaining 30 ms it zero velocity.)

But when i try mesh motion - preview - it moves little bit only.. not 254mmm for same time steps.

can you tell what may be issue with mesh notion


. I tried the UDF but it shows error: warning unable to read the udf file

#include "udf.h"
DEFINE_CG_MOTION(oscillate, dt, vel, omega, time, dtime)
{
Thread *t;
face_t f; /* define the variables */

t = DT_THREAD(dt); /* get the thread pointer for which the motion is defined */

/* if (!Data_Valid_P())
/* return; /* check if the values of the variables are accessible before you compute the function */

begin_f_loop(f, t) /* loop over each face in the zone to create an array of data */
{
if (time <= 0.02)
vel[0] = (673* time); /* define the velocity of the moving zone---*/
else if (0.02 < time < 0.027)
vel[0] = 14;
else if (0.027 < time < 0.03)
vel[0] = 3 - 2800*(time-0.03);
else if (0.03 < time)
vel[0] = 0;
}
end_f_loop(f, t)
}

If we have to give displacement, velocity, and time then do we have to make three columns?

velocity is implied by displacement.
or what direction of the velocity.

profile cannot be read
 

I write a profile, but it doesn't work, motion profile not recognizeit can you help? thank you.
what I wrote as below:

disp_piston 2 20 1
time x
0 0
1 0.1
2 0.2
3 0.3
4 0.4
5 0.5
6 0.6
7 0.7
8 0.8
9 0.9
10 1
11 0.9
12 0.8
13 0.7
14 0.6
15 0.5
16 0.4
17 0.3
18 0.2
19 0.1

It's format more like in Fluent 17.0:

((moveVel transient 3 0)

(time 0 1 2)

(v_x 0.05 0.05 0.05)

)

I am asking one point with profiles, I seen three point for continuation of profile. Does ansys make its own calculation for the continuation of the profile? For example my time step is 1e-7 and my velocity is fix for 0.05.(total time is 13 s) Should I use time when writing the profile or time step?
And is it necessary write in the three point for continuation time/velocity

The profile you write should be smaller than your time step. so it gives enough velocity information. The data is much more than three.

((moveVel transient 5 0) %% red 5 is you give 5 data; Bule 0 means not periodic, if you make it 1, that will be periodic.

(time 0.00000005 0.00000001 0.00000015 0.00000002 0.00000025) %% smaller than your time step

(v_x 0.05 0.05 0.05 0.05 0.05) %% define your velocity

)

example of 5 time points, fix velocity 0.05, periodic by define 0.

But I don't understand, if your velocity is fixed, why you need a transient profile? I use it to define the changing velocity/pressure.

Another suggestion, you can define cycle/periodic if your total time is periodic.

Hi, if I use "periodic", should I add some about my periodicity?

((movevel transient 5 1) of course ,

and then in addition to time and vel_x?

Thank you!