Conjugate Heat Transfer (CHT)

Absolutely. For example, in turbine blade cooling design, the cooling air flowing through internal cooling passages and the high-temperature combustion gas passing over the external blade surface are thermally coupled through the blade metal. To accurately obtain the temperature distribution on the solid side, it's necessary to solve the fluid temperature field and solid heat conduction simultaneously, rather than assuming a heat transfer coefficient $h$ on the fluid side.

Of course. Any problem where solid heat conduction and fluid convective heat transfer are tightly coupled is a candidate for CHT: combinations of heat sinks and fan cooling, cold plate design for power semiconductor modules, heat dissipation design for LED packages, etc.

In the fluid domain, the Navier-Stokes equations and the energy equation are solved. In the solid domain, the heat conduction equation is solved. Then, continuity conditions for temperature and heat flux are imposed at the interface between these two domains.

The interface conditions can be written mathematically as follows.

Exactly. The steady-state heat conduction equation for the solid side is

where $\dot{q}_v$ is volumetric heat generation (like Joule heating). The energy equation on the fluid side includes the convection term. The essence of CHT is that these two are coupled through the interface conditions.

The above is fine for an ideal interface. For actual TIMs (Thermal Interface Materials) or bolted joint surfaces, contact thermal resistance needs to be added to the interface conditions. In Ansys Fluent or STAR-CCM+, this can be set as a thin wall or contact resistance.

There are two main types: monolithic and partitioned. Monolithic solves the solid and fluid simultaneously with a single solver. Ansys Fluent, STAR-CCM+, and OpenFOAM's chtMultiRegionFoam use this approach.

Partitioned runs separate solid and fluid solvers and exchanges interface data. For example, co-simulation between Ansys Mechanical and Fluent, or between Abaqus and STAR-CCM+, falls into this category. It's also a method used in FSI (Fluid-Structure Interaction).

Monolithic offers high interface consistency and faster convergence. Partitioned provides flexibility to combine existing solvers, but requires attention to interface interpolation accuracy and convergence stability.

It certainly can. The solid side can often be relatively coarse, but the fluid side needs to resolve the wall boundary layer. In Ansys Fluent, you choose to set the wall first layer $y^+$ to around 1 and not use wall functions (low-Re turbulence model), or use $y^+ \approx 30$ with wall functions.

Exactly. Especially if discussing local heat transfer coefficient or Nu number distribution, you should place a sufficient number of prism layers (inflation layer). In STAR-CCM+, you can specify total thickness from the wall and number of layers for automatic generation. In OpenFOAM, you set it in snappyHexMesh's addLayersControl.

Monitoring temperature and heat flux at the interface is crucial, not just residuals. You need to confirm that the average or maximum temperature at the interface stops fluctuating between iterations. In Fluent, a standard practice is to track the area-weighted average temperature of the interface using a surface monitor.

For monolithic, it's similar to regular CFD calculations. For partitioned co-simulation, set the number of sub-iterations per step to around 3–10 and confirm that interface value fluctuations become sufficiently small. Adjusting the relaxation factor (under-relaxation) is also key.

A typical procedure is as follows. (1) Define solid and fluid domains from CAD. (2) Generate mesh for the fluid domain, resolving the wall boundary layer with prism layers. (3) Generate mesh for the solid domain. (4) Connect the interface conformally (node-matched) or non-conformally. (5) Set material property values. (6) Set boundary and initial conditions and execute the calculation.