## 2 Materials and Methods
### Method of Solution  
The finite volume method (FVM) was used for calculations in this work by Ansys/Fluent implementation. Generally, the method discretizes the computational domain into a set of volumetric cells, that is, control volumes. The governing equations are solved within each control volume, and in a typical scenario the solution is obtained by solving a set of algebraic equations that involve the values of the physical quantities (e.g., pressure, velocity, density, etc.) at the center and/or boundaries of the control volume. The values of the physical quantities are then collected to obtain a solution at any point in the computational domain. The calculation procedure is iterative by design and convergence is controlled by the under-relaxation terms for each equation, which consequently control the advancement process in the solution from one iteration to the next. Additionally, the convergence also depends on the order of the discretization selected for each solved equation. The geometry of all cases presented was developed using the construction of a solid along a given forming path shaped in the form of an appropriate zigzag. A zigzag profile was inserted into a rectangular area measuring 80 \(\times\) 9 mm, making the number of sections change from a straight channel with 0 sections to 7, then to 10, and finally to 16 sections. The cooling channel was shaped from a rectangular profile with dimensions of 1 \(\times\) 0.5 mm. The size of the tetrahedral mesh cells was determined by the classical procedure based on a series of calculations with changing the base size of the cell. As soon as the mesh size decreased, no significant changes were observed in the obtained mass imbalance, taken as the difference between input and output; the base size of the mesh cells was considered sufficiently small to realistically express the running process. The figure below (Figure 3) presents the convergent profile of results against mesh size. As a size that guarantees the correct accuracy of the calculations with a reasonable calculation rate, 10\({}^{-4}\) m was selected. The flow problem was solved using a pressure-velocity coupling scheme (in which pressures and velocities are updated simultaneously). The gradients required for the calculations were defined by a least squares cell-based scheme. The pressure was discretized using second order and the momentum and energy using second order upwind scheme. The coupled approach presents several advantages over the noncoupled or segregated approach. It yields a robust and efficient single-phase implementation for steady-state flows, demonstrating superior performance compared to the segregated solution schemes. The pressure-based coupled algorithm offers an alternative to the density-based and pressure-based segregated algorithms with SIMPLE-type pressure-velocity coupling. In the case of  
Figure 3: Solution imbalance vs. size of the tetrahedral cell. An improved convergence with reducing mesh size can be observed. The blue dots indicate numerical values and the line show the trend of convergence. transient flows (which were not calculated here), employing the coupled algorithm becomes necessary when either the mesh quality is poor or large time steps are employed. The coupled algorithm simultaneously solves the momentum- and pressure-based continuity equations. Full implicit coupling is achieved through an implicit discretization of pressure gradient terms in the momentum equations and an implicit discretization of the face mass flux, incorporating Rhie-Chow pressure dissipation terms. The Rhie-Chow pressure dissipation terms involve the introduction of an extra term to the pressure equation that depends on the velocity field. This term, known as the pressure correction term, acts to dissipate pressure fluctuations that are not consistent with the velocity field, thereby improving the stability of the simulation.