[Boone]

Hi,



I am trying to study heat transfer in pipe flow with solid shell but it seems that the conduction in the solid is not taken into account in my setup (see in attached picture the external shell is homogeneous blue).


I draw 2 frozen bodies corresponding to the fluid and the solid with design modeler and I make 1 piece with those two parts as recommanded for the mesh generation.



I defined the surface that is common to both fluid and solid (commun_fluide_solide) as a wall (I also tried to use the shell conduction on this layer but it does not change anything). Note that, after importing the mesh, Fluent created an extra wall commun_fluide_solide-shadow: I appllied the same boundary conditions on it than on the original commun_fluide_solide nammed selection.


My fluid is water and my solid aluminium. The heat transfer coefficent is 400 W/m2/K and the free stream temperature is 300K. The inlet water temperature is 400K.


Can you help me to figure out why the temperature in the solid is homogeneous and remains equal to the external temperature ?


Thanks a lot !

[CFDKareem]

Make sure you use Share Topology in geometry generation. The interface wall should be defined as a "Coupled Wall" in fluent. Since it created a shadow face this should be correct.

If you plot the heat transfer rate in the flux reports does it show any heat transfer at your interface wall?

[Boone]

Hi, thanks for your answer.

I shared the topology in design modeler and the interface wall is defined as coupled wall. The heat fluxes in the interface wall is not null and I see that the temperature in the solid region depend on the longitudinal location. However for a given location in the longitudinale location, the solid temperature is homogeneous in the thickness (see the temperature plot at different longitudinal locations).

As I am drawing and meshing the solid region I do not use the shell conduction option for the external wall of solid. I checked convection, select aluminium and give a heat transfer coefficient as well as freestream temperature. I have the possibility to give the wall thickness but it seems weird to give the wall thickness while the solid thickness is given in the geometry and meshed so I set it to 0. Is this the correct setting ?

For the interface "commun_fluide_solide" I set it as a wall and do not check the shell conduction option (only "Coupled"). I choose the same setting for the automatically created "commun_fluide_solide_shadow". Is that ok?

Also, I defined my solide volume as internal and remesh with boundary layer cells (see picture).

Can you explain me why there is no temperature gradient in the solid thickness ? What I am doing wrong ?


Thanks again !

[CFDKareem]

Originally Posted by Boone

Hi, thanks for your answer.

I shared the topology in design modeler and the interface wall is defined as coupled wall. The heat fluxes in the interface wall is not null and I see that the temperature in the solid region depend on the longitudinal location. However for a given location in the longitudinale location, the solid temperature is homogeneous in the thickness (see the temperature plot at different longitudinal locations).

As I am drawing and meshing the solid region I do not use the shell conduction option for the external wall of solid. I checked convection, select aluminium and give a heat transfer coefficient as well as freestream temperature. I have the possibility to give the wall thickness but it seems weird to give the wall thickness while the solid thickness is given in the geometry and meshed so I set it to 0. Is this the correct setting ?

For the interface "commun_fluide_solide" I set it as a wall and do not check the shell conduction option (only "Coupled"). I choose the same setting for the automatically created "commun_fluide_solide_shadow". Is that ok?

Also, I defined my solide volume as internal and remesh with boundary layer cells (see picture).

Can you explain me why there is no temperature gradient in the solid thickness ? What I am doing wrong ?


Thanks again !

I believe your setup is correct. The wall should be coupled and there is no need for a thickness on the outer wall. A few suggestions...

First, refine your post processing to just the wall and confirm the temperature is equal on the inner and outer wall. Although it looks flat in the XY plot your provided, it may actually have a slight gradient if you only plot a line through the thickness, and not through the fluid. You can also plot a contour on just the pipe and uncheck "global range" to get a more relevant scale. Finally, use surface integrals to check the area-weighted-average on the inner wall vs. the outer wall and see if they are different.

Second, this may be a perfectly reasonable result. I would suggest trying to validate with some simple hand calculations from heat transfer first principles. Just looking at your boundary conditions, 400 W/m2-k is a really high HTC. It's not too surprising that your pipe has only a very small temperature gradient through the thickness.

Finally, if you want to trust your simulation you should analyze potential error sources. I would say the first source, human error, looks okay. I believe your boundary conditions are set correctly. The second source I would check is your spatial discretization error, or mesh size. A mesh refinement analysis would be useful to test mesh independence. Looking at your mesh it looks pretty coarse for the high temperature gradients you are trying to resolve. Other sources of error can be checked, but should be minimal for this simple problem.

Hope this helps! Let me know if you're still having issues.

[Boone]

Hi,



I changed the HTC and the solid with wood and there is a temperature gradient in the thickness. The setup is good you were right.



Yes the mesh needs to be adapted but it was just to see if the conduction is well considered with this type of setup.



Thanks !