I need to write a UDF for a boundary condition of a gas flow rate. In my simulation using Fluent, I need to simulate a process lasts for ~ 5 hours. During the process a specific gas flow rate (1.6389 kg per hour) is injected through pipes to the fluid domain. The gas flow rate is injected when the process starts (i.e. when flow time is zero in the simulation) and repeats every one hour. The injection process lasts for few seconds.
So how can I write the suitable UDF for this flow rate?. I wrote a simple code and would be so much grateful if anyone has experience with UDF can give me a feedback. Any help is greatly appreciated.
#include "udf.h"
DEFINE_PROFILE(transient_mf, thread, position)
{
face_t f ;
real t = RP_Get_Real("flow-time"); /* to calculate the physical time step*/
begin_f_loop(f, thread)
{
if (t==0,3600, 2*3600, 3*3600, 4*3600, 5*3600)
{
F_PROFILE(f, thread, position) = 1.6389;
}
else
{
F_PROFILE(f, thread, position) = 0;
}
}
end_f_loop(f, thread)
}
From a conceptual viewpoint, the gas-flow with this UDF is non-zero only if the flow-time exactly matches said time, which is unlikely (since time is a real number, the odds of it exactly matching an integer are minimal), and even if it matches, the velocity is only held for a single timestep. So the amount of gas dosed depends on your timestep size. In reality, I assume you set a gas flow for a certain amount of time (x seconds or so) - this is not reflected in your current UDF. You should specify the flowrate for a certain range of time, not for fixed timepoints.
More specific points, check the unit. I believe the gas flow rate is set in kg/s if you use a mass-flow inlet, so do the conversion. Also I don't think your if-stament will work like this, you need if (t == 0 || t == 3600 || t == 2*3600 ) etcetera.
The amount of gas delivered depends on your size of time. I propose to determine the flow of time for a certain period of time, and not for fixed time options.
you need to confirm the boundary condition you want to use for the mass flow rate, because the udf
DEFINE_PROFILE(transient_mf, thread, i)
is usually used to specify the value of the variable on the boundary condition,
for example
(1) if you use "mass-flow-inlet" as your boundary, you need to specify the mass flow rate in the unit of kg/s, so maybe you can write udf like this:
#include "udf.h"
DEFINE_PROFILE(transient_mass_flow_rate, thread, i)
{
face_t f ;
const real delta_t = 10; /* the duration of your injection process. */
real t = RP_Get_Real("flow-time"); /* to calculate the physical time step*/
begin_f_loop(f, thread)
{
if (
(t > 0 && t < delta_t)
||
(t > 3600 && t < 3600 + delta_t)
||
(t > 2*3600 && t < 2*3600 + delta_t)
||
(t > 3*3600 && t < 3*3600 + delta_t)
||
(t > 4*3600 && t < 4*3600 + delta_t)
||
(t > 5*3600 && t < 5*3600 + delta_t)
)
{
F_PROFILE(f, thread, i) = 1.6389/delta_t;
}
else
{
F_PROFILE(f, thread, i) = 0;
}
}
end_f_loop(f, thread)
}
(2) if you use velocity-inlet as your boundary condition, you need to convert the mass flow rate to velocity in unit of m/s, like this:
velocity = mass_flow_rate/cross_area_of_inlet/density, you can write your udf like this
#include "udf.h"
DEFINE_PROFILE(transient_velocity, thread, i)
{
face_t f ;
const real area_inlet = 0.1; /* the area of your injector jet. */
const real delta_t = 10; /* the duration of your injection process. */
real rho = 0.0;
real t = RP_Get_Real("flow-time"); /* to calculate the physical time step*/
begin_f_loop(f, thread)
{
if (
(t > 0 && t < delta_t)
||
(t > 3600 && t < 3600 + delta_t)
||
(t > 2*3600 && t < 2*3600 + delta_t)
||
(t > 3*3600 && t < 3*3600 + delta_t)
||
(t > 4*3600 && t < 4*3600 + delta_t)
||
(t > 5*3600 && t < 5*3600 + delta_t)
)
{
rho = F_R(f,t);
F_PROFILE(f, thread, i) = 1.6389/delta_t/area_inlet/rho
}
else
{
F_PROFILE(f, thread, i) = 0;
}
}
end_f_loop(f, thread)
}
this is just a general ideal, you need to check the details. hopes this can help you with your problem
Dear Cees Haringa and Dušan Regodić thank you so much for answering my question. You both recommended me to specify the flow of gas for a certain range of time and not for fixed time points, this is quite interesting. As I'm an absolute beginner in UDF I need further assist with this, so can you recommend me any tutorial or a code that I can refer to help me to build my code?Any help will be greatly appreciated.
Regards
Hi Xu Kailong
Thank you so much for your answer. Also many thanks for providing these codes, they are quite interesting and helpful. Just one more question, can I apply same function to two inlets?
Regards
I would not seek a specific UDF tutorial, rather, look for a course on C coding. If you can do that to a sufficient extent, you can make UDFs.
Oula Fatla you can check fluent help on how to write udfs. you can apply same function to two inlets if they have the same boundary conditions. if the flow rates are different, you can write udfs with different names.
Many thanks Cees Haringa . I will, definitely consider taking a course in C coding
Thanks again for your valuable comments.
Best Regards
- Badges
- Science topic