**5. Methodology and numerical modeling**

Due to the administrative and financial barriers to field measurements as well as the more thorough analytical parameters offered by numerical simulation, CFD Fluent was chosen for this project to model pedestrian level comfort levels and wind condition settings. The 3D stable RANS equations and the CFD package Fluent were used to do the CFD simulations. The realizable (k-) turbulence model offered the closure. This turbulence model was selected based on suggestions made by [57] and past validation investigations for wind conditions at the pedestrian level [11]. One of the most crucial factors in analyses of the building's exterior aerodynamics is the accurate modeling of the atmospheric boundary layer in CFD. The roughness coefficient is defined as 0 in the CFD since a lot of analytical software does flow analysis for materials with a low roughness coefficient. The roughness coefficient must to additionally be specified according to the area where the construction is situated. As it is an open zone surface, 0.2 m is the specified surface roughness [58].

The algorithm paired with the Pseudo Transient option and the pressure velocity matching are taken into account. Second order equations are used for viscous terms. Simulations were made for eight wind directions. The following minimum values were reached: for x, y, z velocity components: 10−7, (k –ε): 10−4, for continuity: 10−4. The first phase involves creating a flow volume all around the structures. The computational area is where this is located. The mesh structure is used to mesh this area while building the mathematical model. Afterward, boundary conditions are established. The equations are solved and the answer is obtained once these definitions have been formed. An example of the mesh structure used is given in **Figure 3**. 18 million polyhedral elements are used in the mesh structure created in the model. When the findings are compared to experimental values, the grid's quality has an impact on the precision. When the grid tuning was applied twice during the analysis, the grid became denser where it was required and the flow solution converging into the continuous flow regime. Depending on the average pressure changes on the pre-determined surfaces in the structures, it was applied automatically every 300 iterations.

**Figure 3.** *CFD 3D Model and Mesh Structure for the case study texture.*

In accordance with AIJ recommendations, four levels (2.25 m above ground, layer height: 0.5 m) are placed below the assessment height. The first phase involves creating a flow volume all around the structures. The computational area is where this is located. While building the mathematical model, this region is connected to the network structure. Afterward, boundary conditions are established. The equations are solved and the answer is obtained once these definitions have been formed. In all simulations, a denser network structure has been developed in regions where substantial pressure and velocity gradients are anticipated [59].

A portion of the continuous space surrounding the structure under consideration must first be discretized. The computational domain is the name given to this area of space. There was a limited volume created from the domain. The basic equations were drawn up for each volume of the computing domain. The equations are then resolved in the presence of a set of starting and boundary conditions. Every simulation that is run makes use of a mesh that is denser in areas where pressure or velocity gradients are expected to be high.

A solid model of the case study area was created with the information obtained from the 2-D architectural project and site plans of the buildings. Three dimensional model of the project is illustrated in **Figure 3**. The CFD model represents buildings set along with the real topography of their location. The design of buildings must account for wind loads, and these are affected by wind gradients. The respective gradient levels, usually assumed in the Building Codes, are 500 m for cities, 400 m for suburbs, and 300 m for flat open terrain.

The approaching wind was created from a power-law model to approximate the mean velocity profile:

$$U = U\_r + \left(\frac{Z - d}{Z\_r}\right)^a \tag{6}$$

Where U is mean wind speed, Zr is reference height, Ur is wind speed at reference height Zr, d is zero plane displacement, and is power-law exponent. For open country, suburban, and urban exposures, respectively, the exponent changes depending on the type of terrain; it is 0.14, 0.25, and 0.35 for each. The power-law equation is employed at the inlet condition to simulate a mean wind speed of 30.5 m/s at the building height according to an exponent, which is dependent on the surface roughness of the terrain surrounding the building model. On the basis of the actual wind characteristic, the input parameters for wind density and wind dynamic viscosity were developed (**Table 1**).

*Pedestrian Level Relationship between Building Forms and Streets Effects on the Condition… DOI: http://dx.doi.org/10.5772/intechopen.108735*


#### **Table 1.**

*Power law exponents for various descriptions of terrain.*

In all simulations, a denser network structure has been created in areas where velocity and pressure gradients are expected to be high. CFD-based numerical models are frequently used as a technique to study the airflow near structures in urban terrain. By giving both the real wind flow velocity and the distribution of turbulence throughout the whole research area, computational fluid dynamics (CFD) overcomes the issue of producing and modifying air flow conditions experienced in a wind tunnel. Surface roughness modeling in an atmospheric boundary layer is included in the case study field of wind modeling, which also accounts for local meteorological period average data and regional topography characteristics [60–62].

Mean wind velocity 5–10–15-20 m/s were used as inlet boundary conditions at eight directions. 20 m/s maximum wind velocity was used as inlet boundary conditions at eight directions. The suitable computational modeling, such as domain size, grid size, and grid discrepancy, is largely dependent on the accuracy of simulation results in order to account for the worst case situations. Since the AIJ (Architectural Institute of Japan) recommendations are one of the standards in the literature for the urban pedestrian wind environment, the CFD simulation modeling for the validation technique mentioned in this work complies with them. Based on a number of cross-comparisons between CFD, wind tunnel tests, and field measurements, AIJ recommendations were developed. In contrast, Cost recommendations, another well-liked guideline, is founded on a literature study [14]. The validation experiment's computation area measures 500 × 500 × 20 m. (WxLxH). 150,200 grid points are used to partition the domain. The Simple approach handled the problem of pressure velocity coupling. The viscosity terms of the governing equations were discretized using second-order methods. The iterations were terminated when the scaled residuals showed a very little further reduction with an increasing number of iterations.
