[adi10]

Dear CFD Community,

I hope this message finds you well. I am currently working on a CFD simulation of a Compound Parabolic Collector (CPC) solar collector with conjugate heat transfer. The model consists of a receiver tube enclosed between parabolic reflectors and a rectangular glass cover at the aperture of the CPC. Water flows through the tube, and air surrounds it inside the enclosure. Figure for model has been shared in the attachment.
Copper receiver Tube is geometrically given a thickness of 1mm in space claim. While modelling them in space claim, shared topology was also applied.
So there are 2 fluid zones (air and water) and one solid zone (copper) in the model. In fluent, sets of wall & wall-shadow are obtained each for air-copper and copper-water interfaces.

I have encountered a warning message in Fluent that appears during the mesh reading process. The warning states:

"Warning: materials in neighbor cell threads (6 and 7) of interior zone 4 are of different types (water-liquid and copper). This problem MUST be fixed before solving!
Warning: materials in neighbor cell threads (7 and 8) of interior zone 5 are of different types (copper and air). This problem MUST be fixed before solving!"

This message is repeated 55 times in the console. Subsequently, Fluent performs mesh operations such as "Change Zone Type" and "Slitting wall zone," creating shadow zones for the interfaces between air-copper and copper-water. The following messages are displayed in console for such mesh operations performed.


Applying mesh operation "Change Zone Type"
Slitting wall zone 5 into a coupled wall.
creating receiver_air_side-shadow
Applying mesh operation "Change Zone Type [ 2 ]"
Slitting wall zone 4 into a coupled wall.
creating receiver_water_side-shadow
Applying mesh operation "Change Zone Type [ 3 ]"
Setting zone id of fff-1-copper_tube to 7.
Setting zone id of fff-1-water to 6.
Setting zone id of fff-1-air to 8.
….
So on and finally
“Preparing mesh for display...
Done.”

Despite these warnings, my simulations are running smoothly with convergence observed in terms of residuals, steady-state conditions, and consistent physical quantities such as receiver outlet temperature and heat flux.

I am reaching out to seek your expertise on whether these warnings pose a significant issue. I am uncertain about the implications of these warnings and whether any corrective actions are necessary.

I have gone through various discussions on similar topics within this platform, but I am still seeking a clearer understanding of the steps that can be taken to address or eliminate these warnings.

Your valuable insights and guidance on how to interpret and potentially resolve these warnings would be greatly appreciated. Thank you for your time and assistance.

[MKuhn]

You have defined the wall between fluid and solid as interior. This is only possible for two fluid domains, so FLUENT changes the boundary to a coupled wall. One side ist attached to the fluid domain and the other side (shadow) to the solid domain.
Regarding the 1 mm copper wall, I would recommend to neglected it in the CAD-Modell and just define it at the boundary settings in fluent a thin cooper wall. If the heat flow along the copper pipe is not negligible use also shell conduction.

[adi10]

I had changed the already defined wall between fluid and solid zone from interior to wall, which had resulted in wall and wall-shadow.
The problem is :

Say i want to change the element size in mesh file, so I change the size, generate the mesh and update it.

now I run the fluent which is now reading the updated mesh, so in console of fluent that warning message is displayed.

"Warning: materials in neighbor cell threads (6 and 7) of interior zone 4 are of different types (water-liquid and copper). This problem MUST be fixed before solving!

Warning: materials in neighbor cell threads (7 and 8) of interior zone 5 are of different types (copper and air). This problem MUST be fixed before solving!"

. Now, if i reset the fluent (deleting all previous settings done in fluent) and read the updated mesh, this warning does not appear.

it solves the problem, however, it takes a lot of time and effort to again setup the fluent for every refined mesh case.

Regarding the use of shell conduction, i will try as heat flow through copper pipe is important in my case.

[MKuhn]

The best way is to define the boundary between copper and air already as wall in your meshing tool. First, this will not lead to the warnings when you load the file to FLUENT. Second, depending on the settings of your meshing tool, you will not have a bondary layer on an interior zone (normaly be default the boundary layer is only on fluid walls).
To reduce the time effort. Load the previous cas file in fluent, then go to File > Read > Mesh, choose your refined mesh file and then select the option which does not discard the current cas file. In this way you do not have to set cas again. Remember to use the same names for the boundaries and zones in the meshing tool.