[Christoph.Ha]

The think is, i also want to get the surface temperatures of the solid housing. So it would be necessary to make a simulation with fluid and solid part.

[MKuhn]

In my opinion you will get nearly the same results without solid mesh and wall thickness+shell conduction instead. Which is the thermal condition on your outer wall? (Heat flux, fixed temperature or convection?)

[Christoph.Ha]

Its a heat flux, but coupled with a heat generation rate inside an electrical componend which is coupled to the wall. In an later step i want to model this electircal componend also, therefore i think i need that wall physically?

[MKuhn]

You can also impose a heat load (Heat Generation Rate in w/m³) to a shell conduction layer. Please refer to here and here.

[AlexanderZ]

Originally Posted by Christoph.Ha

Hello,

i have some news. Today i tested an setup without the solid wall, so just the fluid domain. That converged very well and max. Velocitys are <10m/s (with an inlet Velocity of 5m/s). So i think there must be something wrong with the interface.
During initialization i get following info: "Info: Interface zones overlap for mesh interface contact_region.
This could adversely affect your solution."
After some research i found out, that the walls of both domains have some issus with the contact definition. But i´m not aware of how i could solve that issue, does anybody of you guys can tell me how to fix it?

Thanks in advance,
Christoph

EDIT: Mesh -> Contacts -> Contact Region shows Contact: 686 Faces, Target: 687 Faces. Scoping Method is Geometry Selection.

I think, for your case you do not need contacts.
Delete them before loading mesh into fluent. In case you are using ansys mesher go to mesh -> contacts -> delete contacts.

Than load mesh into fluent, define materials for solid and fluid parts.
use

mesh m-z s-i-b

This will create shadows between solids, in case you have more than one.

Best regards

[Fole]

If I were you:

1) Change to kwSST standard (no transition). Because y+=1 is a must in that model.
2) Check y+ and BL resolution. If after reducing speed your model converged, maybe it is the cause.
3) In my experience, inflation on complex geometries, I limit the transition ratio even more (limiting the height), and then adaptive mesh refinement during solution. ICEM CFD is another solution, I am on the way.

[Christoph.Ha]

Hello Guys,

i found the problem!
It was a problem with the interface between the fluid and the solid wall!
I solved it with a mapped (+coupled) interface between those domains. No it converges very well with k-e-model and energy equation!

Thank you all very much, i still learned a lot about troubleshooting with fluent divergence!

Best Regards,
Christoph

[MKuhn]

Hi Christoph,

thanks for your reply, fine that its works now

Moritz