# Asphal Heat Recovery Application for Sustainable Green Energy
## 5 Numerical Model  
In addition to experimental campaigns, a numerical study was conducted in Ansys Fluent with the experimental stand geometry. The numerical study was done in order to study in depth the phenomenon and to compare the results obtained from the two approaches. The results from the numerical study were post-processed using Tecplot software. The geometry of the numerical study that was made in the Design Modeler of Ansys Workbench and can be seen in Figure 5. It reproduces the geometry of the experimental approach, both in terms of shape and structure, as well as the dimensions and configuration of the pipeline route. The numerical case has the dimension of 2600 \(\times\) 2000 \(\times\) 500 mm, with the pipes incorporated at a depth of 40 mm from the surface. The calculation grid contained 9.7 million tetrahedral elements. The \"inflation\" option was used for generating boundary layers, resulting in five boundary layers at the level of the pipes with a smooth transition, depending on the size cell and the number of cells in the respective area. At the same time, in order to improve the quality of the elements, the high smoothing mesh option was used. Figure 6 shows the calculation grid in the areas of interest. From here, one can see how the grid was generated in terms of boundary layers, cell dimensions, and the transitions at the level of the tetrahedral elements. Figure 4: (**a**) Thermographic image of the area located (**a**) above the CSA and (**b**) between the CSA pipes. Figure 5: Numerical model geometry. The boundary condition data imposed on the numerical study were obtained from measurements performed on the experimental stand. The numerical calculation used RANS equations (Reynolds-averaged Navier-Stokes equations), while the calculation was performed in \"steady-state conditions\". A step-by-step approach was used to test and simulate the case gradually, initially using stationary conditions with heat transfer through conduction and subsequently, after checking the case, using solar radiation conditions. The gravitational force function was also activated (9.81 m/s\({}^{2}\)) in the numerical model. The turbulence model used to study the flow of the fluid through the pipes was k-\(\upomega\) SST. A \"pressure-based solver\" was used for calculating the pressure and velocity equations, using the \"Coupled\" algorithm for \"Pressure-Velocity Coupling\", with \"Least Squares Cell Based\", \"Second Order\", and \"Second Order Upwind\". The radiation model used was Surface to Surface (S2S), with the \"Solar Ray Tracing\" option activated, considering normal (ideal) weather conditions. The values of direct and diffuse solar radiation were obtained from the experimental measurements, imposing values of 725 W/m\({}^{2}\) (constant) for direct solar radiation and 125 W/m\({}^{2}\) (constant) for diffuse solar radiation. The thermal agent fluid used in the numerical model was water, similar to the experimental measurements. Regarding the simulation of heat transfer through the solid material, the numerical model used the general characteristics of an asphalt (density 2243 kg/m\({}^{3}\), specific heat 920 J/kg\(\cdot\)K, thermal conductivity 0.75 W/m\(\cdot\)K). The initialization of the case was \"Hybrid Initialization\", while the convergence on the numerical calculation was set to 10\({}^{-6}\). The thermal agent mass flow rate was 0.125 kg/s, similar to the one used in the measurements. The numerical model took into consideration the heat transfer through conduction (asphalt and pipes) and radiation (sun radiation). As a simplifying hypothesis regarding the air force convection, it was shown in previous studies that heat transferred through air force convection has a very small proportion in the total heat transfer [25; 26]. Of course, this transfer method is also subject to the context of the location (geographical area, surroundings, etc).