[mj2malik]

I am simulating a 2D axisymetrical combustor. I have a boundary condition on the wall of the combustor for temperature, which is varying with length . the length (Y) of the combustor wall is 2.4 metres and temperature is in K.

please see the temperature variation in the attachment.

Can someone help me define these boundary conditions in ANSYS Fluent, either through GUI or through UDF.

Thanks

[annan]

Hello
You can try to compile the following udf, I wrote quickly and didn't have time to verify it works. But basically, your UDF should look like this one.
Once you compiled it in Fluent, go to your boundary conditions panel, select the velocity inlet boundary you want to change, and set the velocity (x,y or z depending on your case) to udf inlet_velocity.
Hope this will help.
Good luck

#include "udf.h"

DEFINE_PROFILE(inlet_velocity, thread, position)
{
real x[ND_ND]; /* this will hold the position vector */
real y;
face_t f;

begin_f_loop(f, thread)
{
F_CENTROID(x,f,thread);
y = x[1];
if (y>0 & y<=0.046)
{ F_PROFILE(f, thread, position) = 925; }
else if (y>0.046 & y<=0.553)
{ F_PROFILE(f, thread, position) = 358.88*y^2-54.615*y+925.6; }
else if (y>0.553 & y<=1.4)
{ F_PROFILE(f, thread, position) = -567.89*y^2+1115.1*y+564.02; }
else
{ F_PROFILE(f, thread, position) = 953; }
}
end_f_loop(f, thread)
}

[mj2malik]

Thanks Annan for your help. I just want to clarify one thing, in your post you suggested to select inlet velocity.

Since I want to vary the wall temperature, should I go in the boundary condition panel and select wall and set the temperature in the thermal setting using new input parameter.

Your input will be highly appreciated.

[annan]

My bad sorry, I thought it was a velocity inlet condition. In your case, you should implement it in "Boundary conditions => select your boundary => wall => thermal => select temperature" and then try to specify it as the UDF.

[mj2malik]

Thank for your help. Just a quick question, in the UDF, what should i replace inlet_velocity with in the DEFINE_PROFILE(inlet_velocity, thread, position)

Should it be temperature or wall_temperature

Your input will be highly appreciated.

[annan]

That is just the name of the udf so that you can recognize it in Fluent GUI. You can put whatever you want, it doesn’t really matter. Therefore, you may put temperature or wall_temperature, it’s really just a name.

[mj2malik]

I have interpreted the file and i get the following error

line 16: invalid type for integral binary expression: double ^ double.

Line 16 in this case is
{ F_PROFILE(f, thread, position) = 358.88*y^2-54.615*y+925.6; }


Any suggestions how I can fix the error. Should I replace y^2 with y*y ?

[annan]

Yes either put y*y or replace y^2 by pow(y,2)

[mj2malik]

Now, I want to apply the same boundary condition for a horizontal combustor, where the wall boundary condition changes in the x-axis instead of y.

Should I swap the x and y in the udf ? Or do i need some additional changes ?

Please, see the attachment for more clarity.

[annan]

In the udf I’ve written, x[ND_ND] is your domain. x[0] is the x-axis and x[1] is the y-axis. If you want to apply the same udf on a horizontal boundary, you just need to set y=x[0], which means that your condition statements will be set for x values.
Hope I was clear and that it will help
Let me know if you need more details

[mj2malik]

Thanks alot. I really appreciate your help. it worked without any problem

[annan]

My pleasure

Good luck