Simcenter FLOEFD Optimizing Precision: Mesh Considerations for heat sink simulation

Occasionally, we observe that the heat analysis results appear accurate in the fins, but anomalies or discontinuities arise in the flow results. The instinctive solution might be to refine the mesh, but the critical question pertains to the extent of refinement necessary.

Within the realm of FLOEFD, a valuable technology known as thin-channel mode comes into play. This feature allows us to assess the thermal performance of heat sinks or fins without resorting to an excessive mesh density, thereby optimizing computational efficiency.

Thin-channel mode becomes operational in scenarios characterized by a coarse mesh, specifically when there are precisely 7 or fewer cells across a slot (d) (Fig.1). Under this approach, the determination of shear stress and heat flux proximal to the wall relies on approximations derived from experimental data, diverging from the conventional CFD methodology. This strategic employment proves advantageous in instances where conventional approaches encounter challenges.

Figure1: “d” is the distance between two neighboring fins.

Counting cells to determine whether you've applied this technique is unnecessary. To check if you are utilizing Thin or Thick channel mode, conduct a surface plot analysis. Typically, Thin Channel Mode isn't included in the default list; you can access it by clicking "Add Parameter" at the list's bottom. Find it within the Boundary Layer parameters group (Fig. 2)

Figure 2. The customize parameter list.

The "Thin channel mode" parameter shows the activation state of the thin channels engineering model: "1" means that the surface on which this parameter is visualized is a wall of a channel in which the thin channel model is active, "0" means that a regular CFD solution is used in the fluid volume that is adjacent to the surface. 

Figure 3. Thin channel mode: (A) shows thin channel mode off and (B) shows thin channel model on.

For more precise flow behavior results, it's advisable to increase the number of nodes to a minimum of 10. This shift enhances the transition from an engineering model to Computational Fluid Dynamics (CFD), offering a more thorough insight into the system. If the primary simulation goal is to comprehend the dissipated heat quantity, maintaining a coarse mesh is preferable to economize on computational time. However, if the focus is on fan/blower optimization, flow analysis including pinpointing separation points, it's suggested to employ a finer mesh, with more than 10 cells between fins.

Notes:

Please note that there are at least 7 cells situated between the fins. It's important to consider that the fluid volumes of the partial cells adjacent to the solid/fluid interface (the fin wall) are also considered fluid cells. The estimation of the number of cells across the channel is based on the dimensions of the near-wall cells. Therefore, if the number of cells falls below 7 due to larger cells present in the middle of the channel, FLOEFD might count more than 7 cells. This occurs because FLOEFD divides the channel height by the size of the near-wall cells to determine the number of cells across the channel, disregarding the actual lower number of cells due to the presence of larger, unrefined cells in the middle.

The channel is not recognized as flat - for instance, if the fins are heavily tapered. In that case the thin channel model will not activate.