*2.2. Geometrical Model*

The aim of the numerical calculations was to investigate the thermal-flow characteristics of pipes with internal micro-fins, with a very similar geometry as shown in Figure 1 for the industrial pipe "TECTUBE fin 12736CV50/65D". The only geometric parameter that was changed was the height of the micro-fin *H*. All other parameters, including the fin helix angle *α* = 30◦ and the helical tooth line angle *β* = 30◦, remained unchanged, as in the mentioned real pipe. Modifications of the tooth height *H* were made every 0.05 mm in the range of 0.05–0.40 mm, changing its size in relation to the height *H* = 0.25 mm, which the actual pipe has (see Figure 4). The relative roughness of the pipe, which is defined as the ratio of the height of unevenness on the surface of the pipe to its diameter *ε = H/d* changes with a change of the micro-fin height. In this case, the "unevenness" are micro-fins of a given height *H*. Table 2 lists all the fin heights tested, together with the corresponding relative roughness *ε*. The models of selected cases are shown in Figure 5.

**Figure 4.** Scheme of changes in the fin height tested in the simulation.

**Table 2.** Results of the calculations of relative roughness.


**Figure 5.** Different height of fins in the tube fragment model. (**a**) *H* = 0.05 mm, (**b**) *H* = 0.25 mm, (**c**) *H* = 0.40 mm.

## *2.3. Numerical Model*

As the computational domain, a part of the spiral extruded pipe geometry was used, with a width of three fins as in Figure 5 and a length corresponding to its single helix pitch through an angle of 360◦ (Figure 6). The use of the width of three fins was due to the more convenient procedure of generating a computational mesh, which allowed us to maintain its better geometrical quality (cells angles, aspect ratio, etc.) in the central part of the channel near its axis, than for the width of one fin, but also applicable in such geometry. The list of used boundary conditions is introduced in Table 3.

Generally, instead of a full, long pipe, a repeating and periodic fragment of it, representative of the entire channel and reflecting the same heat-flow phenomena, was used for the calculations. This approach to the problem is correct, and it is commonly used in the numerical analysis [25,26], as long as the resulting flow is fully developed, both hydraulically and thermally. It is known that under normal conditions, a fully developed flow can be obtained only on a pipe length equal to approximately 40–50 diameters from its inlet. In the

case of using a short repeating domain fragment, appropriate boundary conditions have to be applied to obtain such a flow structure. According to this, translational periodicity was used at the inlet and outlet of the domain, where the fluid flow was forced by a pressure gradient, corresponding to the range of numbers *Re* = 10,000–100,000. Due to the twist of the micro-fins by an angle of 30◦, there is also a component of the rotational velocity during the flow. Therefore, the rotational periodicity was used on the flank surfaces instead of the normal plane of symmetry. The concept of reducing the domain size, and thus also the number of computational mesh nodes, enables a significant reduction in computation time while maintaining high mesh quality and accuracy of results. This method of investigations has also been presented in [24,27,28].

**Figure 6.** Boundary conditions on the models.



The pipe segment forming the computational domain was "extended" to the length of a full revolution, as shown along with other boundary conditions in Figure 6. As previously mentioned, the boundary condition forcing the fluid flow was a pressure gradient.

The simulation was conducted in Ansys CFX 2020 R2. The numerical model consisted of two computational domains. In the flow domain, water is defined as the working fluid with an average temperature of 298 K. The solid-state domain was defined as copper, which is the pipe material in the experiment. Additionally, a negative volumetric heat source was set in the fluid domain to obtain a fully thermally developed flow and to calculate the correct temperature field. This solution made it possible to balance the thermal energy supplied to the domain wall as a heat flux of *q* = 10,000 W/m2.

The SST k-ω turbulence model is one of the most popular models used in many CFD (Computational Fluid Dynamics) applications. Its main attribute is the ability to solve the viscous sublayer by applying the k-ω model near the wall and the standard k-ε model in the turbulent core area. Switching between the two models is controlled by a special builtin blending function [29,30]. Correct use of the SST model requires several mesh nodes inside the turbulent sublayer to maintain the condition of dimensionless distance *y+* < 2 in the entire boundary layer of the computational domain [31]. In the results presented in this work, the maximum value of *y<sup>+</sup>* did not exceed the mentioned value in any of the geometries.

One of the criteria for the uniqueness of the numerical solution was to achieve the appropriate convergence for residues: momentum, energy, and turbulence. In all simulations, a convergence of 1 × <sup>10</sup>−<sup>4</sup> or maximal residuals and an order of magnitude lower (1 × <sup>10</sup>−5) for mean RMS (Root-Mean-Square) residuals were obtained. The second criterion for the uniqueness of the solution was the stabilization of flow-thermal parameters, such as velocity, pressure, and temperature, which were monitored both as mean values and in several selected points in the computational domain. The computation process was finished if the above parameters did not change for several consecutive iterations.

Before the actual simulations, checking calculations were performed for different mesh qualities. For further calculations, a structural (in solid) and hexagonal mesh of such density, at which its further densification gives results differing less than 1%, was selected. For all geometries, efforts were made to maintain a computational mesh of approximately the same average cell volume. In the area of the hydraulic boundary layer, the mesh was additionally compacted to obtain the appropriate *y+* value. After the test, it can be concluded that the mesh used and the test results are independent of its density, which is consistent with the recommendations in [32]. The obtained value of the GCI (Grid Convergence Method) parameters in relation to the average temperature is GCIfine = 1.8%, and in case of the wall heat flux, it is GCIfine = 0.001%.

In Figure 7, the mesh used for the numerical calculations for *H* = 0.25 mm is shown.

**Figure 7.** Mesh used in the numerical simulations for *H* = 0.25 mm: (**a**) full view of mesh; (**b**) mesh region between solid and fluid domain.
