I have a gas in a steel pipe surrounded by heat insulator. There is forced convection between gas and pipe, conduction in steel pipe, conduction between steel and heat insulator, conduction in heat insulator, and then free convection between heat insulator and ambiant air. The inlet temperature is given by an udf. It change for each step time. I don't know how it's possible to simulate the conduction between steel and heat insulator with Fluent. My boundaries conditions are a wall at the limit of the steel zone and an other one at the begining of the heat insulator zone. I thought about using an udf method to get temperatures values at the limit of the steel zone and put them as boundary condition for the heat insulator zone. Is that a good way? If yes, can you give me the udf program.

thanks

Is there any need to model the pipe wall? The conductivity of the steel pipe is about 100 times higher than a normal insulator so it play no (or very little) role in the heat transfer to the outside. The limiting factors are the insulator and the free convection. You can model only the fluid zone and set the boundary condition at the wall to "convection".

RoM

Thanks for your idea but i absolutly need to model all the elements. The aim of my study is to know the temperature value at the steel/heat insulator interface, on heat insulator side. I have to compare the adiabatic case (without heat insulator but no heat flux on steel pipe boundary with outside) and the real one. So I have to make an UDF to get steel pipe limit temperature value and an other one to calculate heat flux between steel and heat insulator.

thanks for your help.

You dont need an udf to model the solid zones. You can run the Gambit journal below to see the basic geometry setup.
If you mesh the 3 volumes and export the mesh to Fluent, Fluent will create some interface zones between the different fuid/sold zones. Dont change those interfaces. Assign the porper materials to the steel and insulator solid zones, define a convection bc for the wall (wall material is not important, thickness = 0.) and set up the gas flow. If everything works right Fluent will calculate a heat flow through both solid zones.

Good luck,
RoM


default set "GRAPHICS.GENERAL.CONNECTIVITY_BASED_COLORING" numeric 1
volume create height 100 radius1 5 radius3 5 offset 0 0 50 zaxis frustum
volume create height 100 radius1 6 radius3 6 offset 0 0 50 zaxis frustum
volume create height 100 radius1 7 radius3 7 offset 0 0 50 zaxis frustum
volume split "volume.3" volumes "volume.2" connected bientity
volume split "volume.2" volumes "volume.1" connected bientity
physics create "gas" ctype "FLUID" volume "volume.1"
physics create "steel" ctype "SOLID" volume "volume.2"
physics create "insulator" ctype "SOLID" volume "volume.3"
physics create "wall" btype "WALL" face "face.8"
physics create "inlet" btype "WALL" face "face.12"
physics create "outlet" btype "WALL" face "face.13"

I made this UDF to get steel boundary temperature but when i initialize in fluent, i have an error message: "segmentation violation". Do you know what the problem is?

#include "udf.h" #define tid 1 /*the ID of steel boundary*/

DEFINE_PROFILE(conduction, thread, position){

face_t f, f1;

real temperature1;

Thread *thread1;

Domain *d;

d = Get_Domain(2); /*the steel domain*/

thread1=Lookup_Thread(d, tid);

begin_f_loop(f1, thread1){

temperature1=F_T(f1,thread1);

}

end_f_loop(f1, thread1)

begin_f_loop(f, thread){

F_PROFILE(f,thread,position)=temperature1;

}

end_f_loop(f, thread)

}

If your problem is not multiphase you should always use Get_Domain(1). But as i said in my previous post, there is no need for an udf in this case. Fluent can calculate heat transfer between different solid zones. All you have to do is set up the geometry right (make shure everything is connected).

RoM