Enhancing the Dynamic Stability of Pylons via Their Drag and Lift Coefficients by Finite Volume Method

Abstract

This study aimed to estimate the drag and lift coefficients of the long-span bridge pylon using the finite volume method (FVM). The k-ω turbulence model was applied to analyze the behavior of wind flow around the pylon, yielding drag and lift coefficient values with an error of 0.98% compared to a previous tunnel experiment. Four recommended cross-sections were proposed to reduce drag and lift forces acting on the pylon, including concave, convex, crossing, and chamfering cross-sections. The finding indicated that drag and lift coefficient decreased for all cross-sections. Cutting edges of concave, convex, and chamfering cross-sections with a ratio ranging from 0.2 to 0.3 has the greatest impact on reducing drag coefficient, while the crossing cross-section with a cutting ratio ranging from 0.2 to 0.25 has the lowest drag coefficient. The maximum reduction in drag and lift coefficients were 23.69% and 13.14% for concave and chamfering cross-sections. Thus, cutting edges of cross-sections is an effective method to enhance the aerodynamic stability of the pylon. Additionally, we evaluated drag and lift coefficients for different wind direction angles. The angles of 0, 30, and 90 degrees resulted in the highest drag coefficient, while the angle of 0 degrees and the angle of 90 degrees resulted in the lowest and highest lift coefficient, respectively. This study not only provides recommendations for cross-sections that reduce forces acting on the pylon but also provides the intensity of this reduction through corresponding estimation equations. In conclusion, concave and chamfering cross-sections are the most effective in reducing drag and lift coefficients, or, in other words, increasing the aerodynamic stability of the pylon.

1. Introduction

Since the Tacoma Narrows Bridge collapsed due to high-intensity winds on 7 November 1940, the aerodynamics of long-span bridges has been a significant concern. Researchers have conducted a series of studies using various methods such as experimentation [1,2,3], computational modeling [4,5,6], and analytical techniques [7,8] to evaluate the impact of wind on the dynamic stability of long-span bridges. Wind-induced vibrations of the bridge can be categorized into three types: self-excited vibrations (such as galloping and flutter), vortex-induced vibrations, and buffeting [9]. Each type of vibration can cause different types of damage, leading to diverse research fields and the beginning of the era of wind-resistant design for long-span bridges.

The upper part of the bridge, including the bridge deck, handrail, pylon, and cable, is primarily affected by wind flow [10]. Many studies have investigated and improved the stability of bridges under different wind conditions using various methods. For example, some studies have investigated the effect of stationary vehicles on bridge decks through their aerodynamic coefficients [11], explored the competitive relationships between aerodynamic and fluttered stability for a super long cable-stayed bridge based on different types of bridge decks [12], examined the vortex-induced vibration caused by the handrail of the box-girder bridge [13], or identified the potential risk of wire mesh in bridge cables for bridge stability when ice falls [4], among others. While the harmful effect of wind flow on bridge parts is well recognized, methods for improving bridge stability are still limited or less concerned, except for the bridge deck. Although the vertical stabilizer plate is an effective method for improving the aerodynamic stability of the bridge deck [14], attaching a stabilizer plate is known to be a simple and dominant method. Therefore, it is necessary to investigate the effect of other methods for improving the aerodynamic stability of other bridge parts, such as the pylon, cable, or handrail.

This study aimed to investigate the stability of a bridge pylon by analyzing its drag ($C_d$) and lift ($C_l$) coefficients using the finite volume method (FVM) with commercial software support. Firstly, the $C_d$ of the free-standing pylon of the Cao Lanh bridge in Vietnam was examined using the Ansys CFX tool and compared to a previous tunnel experiment. Four recommended cross-sections, consisting of concave, convex, crossing, and chamfering shapes, were then created by cutting edges from the original rectangle section to investigate their effect on $C_d$ and $C_l$ under different wind directions. A series of comparisons have been created to discover the effect of incidence wind direction, cutting shapes (cut by a straight line or curve), and cutting ratio (the ratio of cutting width to the pylon width) on drag and lift coefficients. From that, we highlighted the most effective cross-section and its recommendation range, which can provide the best performance in reducing the aerodynamic coefficients.

This current investigation solely utilized simulation techniques; thus, the obtained results must be validated via experimentation. Moreover, this study only examined a limited number of basic cross-sections, and further exploration of more intricate shapes is necessary to achieve a more comprehensive understanding of how modifying cross-sections can improve the dynamic stability of pylons. Additionally, this study’s scope was restricted to H-type pylons, and other types of long-span bridge pylons should also be included for a more inclusive investigation. Furthermore, although this study focused on drag and lift coefficients, a complete understanding of the reduction of aerodynamic coefficients by cutting edges requires the examination of other coefficients, such as vortex and buffering. Lastly, for more precise results, the investigation of non-uniform winds should also be considered in future research.

However, this study did produce some valuable outcomes, including (i) demonstrating that the FVM method is an inexpensive approach for studying the aerodynamic stability of long-span bridge parts, particularly during the pre-feasibility study phase, (ii) highlighting that $C_d$ and $C_l$ values are specific to each angle of incidence and each pylon shape, (iii) confirming that cutting the corner of the cross-section can reduce drag and lift forces, regardless of the cutting geometry, (iv) identifying the concave and chamfering cross-sections as the most effective shapes for increasing the aerodynamic stability of pylons, and (v) determining that the optimal cutting range is between 0.2 and 0.3 for reducing drag and lift forces.

2. Material and Methodology

2.1. Finite Volume Method and Governing Equations

The FVM is the method for solving partial differential equations such as the Navier–Stokes equations in the form of algebraic equations [15]. In the finite volume method, volume integrals in a partial differential equation that contains a divergence term are evaluated as fluxes at the surfaces of each finite volume. The partial differential equation is often called the conservation law, which is represented by the following equation:

$$\frac{\partial u}{\partial t}+\nabla ·f\left(u\right)=0,$$

(1)

where $u$ and $f$ are a vector of states and the corresponding flux tensor, respectively. We take the volume integral over the total volume of the cell $v_i$, which gives the following:

$${\int }_{v_i}^{}\frac{\partial u}{\partial t}dv+{\int }_{v_i}^{}\nabla .f\left(u\right)dv=0.$$

(2)

By integrating the first part of Equation (2) and applying the divergence theorem, the general result equivalent is obtained as Equation (3).

$$\frac{d\overline{u_i}}{dt}+\frac{1}{v_i}{\oint }_{S_i}^{}f\left(u\right).n.dS=0,$$

(3)

where $S_i$ and $n$ are the total surface area of the cell and normal vector of the surface, respectively. The edge fluxes value can be reconstructed by interpolation or extrapolation of the cell averages.

In the fluid mechanic, the vector of state $u$ in Equation (1) is also the velocity vector of a small fluid particle. If the flow is incompressible, irrotational, and viscous, the velocity field can be described by the Navier–Stokes equation that is established from the conversation of momentum and conservation of mass.

$$\frac{\partial u}{\partial t}+\left(u.\nabla \right)u-\nu {\nabla }^{2}u=-\frac{1}{\rho }\nabla p+g,$$

(4)

where ν is viscosity, $\rho$ is the fluid density, $p$ is inertia pressure, and $g$ is acceleration gravity. As shown in Equation (4), the velocity $u$ of each fluid particle depends on the internal force term $-\frac{1}{\rho }\nabla p$ and the external force $g$. The velocity $u$ can be obtained by solving the Navier-Stoke equation, and the resultant velocity $u$ is a component in the drag and lift force, as shown in Equations (5) and (6) below:

$$F_d=\frac{1}{2}{C}_d\rho u^{2}A,$$

(5)

$$F_l=\frac{1}{2}{C}_l\rho u^{2}A,$$

(6)

where $F_d$ and $F_l$ are drag and lift forces, respectively; $\rho$ is the fluid density of particles around the object that has the velocity $u$; and $A$ is the reference area.

The fluid model is the most important concern when solving the computational fluid dynamics, and the $k-\omega$ is a common two-equation turbulence model, as shown in the turbulence kinetic energy Equation (12a) and specific dissipation rate Equation (12b). $i$ and $j$ are notation, $\rho$ is fluid density, $P$ is pressure in fluid and defined by Equation (13) with $\tau$ is shear stress component.

$$k=\frac{3}{2}{\left(UI\right)}^2$$

(7)

$$I=\frac{u^{\prime }}{U}$$

(8)

$$u^{\prime }=\sqrt{\frac{1}{3}\left(u_x^{’}{}^2+u_y^{’}{}^2+u_z^{’}{}^2\right)}=\sqrt{\frac{2}{3}k}$$

(9)

$$U=\sqrt{U_x^2+U_y^2+U_z^2}$$

(10)

$$\omega =C_{\mu }^{3/4}\frac{k^{1/2}}{l}$$

(11)

$$\frac{\partial \left(\rho k\right)}{\partial t}+\frac{\partial \left(\rho u_{j}k\right)}{\partial x_j}=\rho P-{\beta }^{*}\rho \omega k+\frac{\partial }{\partial x_j}\left[\left(\mu +{\sigma }_k\frac{\rho k}{\omega }\right)\frac{\partial k}{\partial x_j}\right]$$

(12a)

$$\frac{\partial \left(\rho \omega \right)}{\partial t}+\frac{\partial \left(\rho u_j\omega \right)}{\partial x_j}=\frac{\alpha \omega }{k}P-\beta \rho {\omega }^2+\frac{\partial }{\partial x_j}\left[\left(\mu +{\sigma }_{\omega }\frac{\rho k}{\omega }\right)\frac{\partial \omega }{\partial x_j}\right]+\frac{\rho {\sigma }_d}{\omega }\frac{\partial k}{\partial x_j}\frac{\partial \omega }{\partial x_i}$$

(12b)

$$P={\tau }_{ij}\frac{\partial u_i}{\partial x_j}$$

(13)

The velocity component estimated from Equation (12a,b), the mean velocity U and the root-mean-square velocity fluctuation are given as Equations (9) and (10), respectively. From that, the turbulence kinetic energy k and the specific rate of dissipation ω are determined by Equations (7) and (11). Where I is the level of turbulence and can be defined by Equation (8), $C_{\mu }$ is the turbulence constant which usually takes the value of 0.09, and $l$ is the turbulence length scale. In Equation (12), the closure coefficients and auxiliary relation can simply be as follows: $\alpha =\raisebox{1ex}{$5$}\!\left/ \!\raisebox{-1ex}{$9$}\right., \beta =\raisebox{1ex}{$3$}\!\left/ \!\raisebox{-1ex}{$40$}\right.$, ${\beta }^{*}=\raisebox{1ex}{$9$}\!\left/ \!\raisebox{-1ex}{$100$}\right.$, and ${\sigma }_k={\sigma }_{\omega }=\raisebox{1ex}{$1$}\!\left/ \!\raisebox{-1ex}{$2$}\right.$ [16].

The k − ω turbulence model is a commonly used method for simulating turbulent flows in engineering applications. It is a two-equation turbulence model that solves for turbulent kinetic energy and the specific rate of dissipation [16,17]. This model is relatively simple to implement in CFD codes and requires fewer input parameters than other turbulence models, which translates to less solving time and computing resources [18]. The k − ω turbulence model is effective in predicting complex flows with separated regions and flow reattachments, such as those found in aircraft wings, turbomachinery, and heat exchangers. It is also known for providing accurate predictions of the behavior of the boundary layer, which is critical in many engineering applications [19,20]. However, the k − ω model has some limitations, such as its inability to predict anisotropic turbulence and the associated swirl and secondary flows. It can also be sensitive to initial and boundary conditions and may require more computational resources than simpler turbulence models such as the k-epsilon model. The k − ω model may not be appropriate for all applications, such as those involving highly compressible flows or strong buoyancy effects [19,20]. Considering the interaction of the pylon surface and the air environment in this study, the k − ω turbulence model, due to its well-established performance in predicting the behavior of the boundary layer and requiring less solving time and computing resources, is a potential model for this study’s modeling.

2.2. Material

Because of a lack of information on air properties, we proposed applying the standard material property provided by ANSYS CFX database. The detailed information is shown in

Table 1. Standard air properties.

Parameter (Unit)/Material	Air
Density (kg·m−3)	1.225
$\mathrm{Specific} \mathrm{Heat} C_p$ (J·kg−1·K−1)	1006.43
Thermal Conductivity (W·m−1·K−1)	0.0242
Viscosity (kg·m−1·s−1)	1.7894 × 10−5
Molecular Weight (kg·kmol−1)	28.966
Standard State Enthalpy (J·kg−1·mol−1)	-
Standard State Entropy (J·kmol−1·K−1)	194,336
Reference Temperature (K)	298.15
L-J Charateristic Length (angstrom)	3.711
L-J Energy Parameter (K)	78.6
Thermal Accommodation Coefficient	0.9137
Momentum Accommodation Coefficient	0.9137
Critical Temperature (K)	132.3
Critical Pressure (Pa)	3,758,000
Critical Specific Volume (m3·kg−1)	0.002875
Acentric Factor	0.033

.

The air density of 1.225 kg/m³ was commonly used in previous research, as evidenced by its application in various studies. For example, this value was utilized to assess the impact of unsteady air density on the aerodynamic performance of a fixed-wing aircraft [21], as well as to explore the influence of flapping trajectories on dragonfly aerodynamics [22]. However, the air density is slightly different in other studies, such as the air density of 1.25 kg/m³ measured in a tunnel test of Cao Lanh bridge, Vietnam [23]. The difference is about 2%, and this error can be ignored for investigation.

2.3. Meshes

Mesh strategy (e.g., mesh type, size, and qualities) is one of essential modeling parameters in computational fluid dynamics. The higher the mesh quality, the greater the accuracy of solutions [24]. In this section, we describe, in turn, the meshing strategy and its effect on the obtained result.

Five mesh types (i.e., tetrahedron, hexahedron, prism/wedge, pyramid, and polyhedral) were provided for computational meshing [25]. Each mesh type has its advantages in simulation. As shown in Figure 1, tetrahedron and hexahedron are plaintiff configurations. A tetrahedron has only four triangular surfaces, while a hexahedron has six rectangular surfaces. Therefore, these two meshes are more straightforward than the wedge, pyramid, or polyhedron, which are more complicated mesh types. The wedge mesh type has a rectangular combined with three triangular surfaces, while the pyramid is similar to the wedge mesh type but increases the number of triangular surfaces, as shown in Figure 1c,d. The most complicated mesh type is the polyhedron, the number of surfaces and their shapes cannot be accurately determined, as it depends on the particular geometry. Because of the complicated geometry of prism/wedge, pyramid, and polyhedral, those mesh types were then rarely applied in the meshing procedure. In contrast, the simple mesh types (tetrahedral and hexahedron) were widely selected [26]. Tetrahedral can be more easily applied for automated meshing as well as improving the stress visualization or the contact pressure and contact shear stress predictions [27]. The hexahedron is often used for simulating some physics because this mesh type significantly increases both the time modeling and the solution accuracy. Reasons are that the hexahedron contains a smaller number of elements (in normal 5–6 tetrahedrons for a single hexahedron) or the hexahedron layer can be aligned along with geometric boundary features [28]. For all the reasons we mentioned above, the tetrahedron was selected for the current simulation of this study. As mentioned, the automated meshing method was compatible with the tetrahedron mesh type; hence, this method was also applied for observing the contact pressure and contact shear stress [27].

The mesh size is closely related to the accuracy of the model in the finite element analysis [29]. The better result requires a smaller mesh size or a higher mesh quality. The simple method for increasing the mesh quality is creating a fine mesh. However, this work increases the time processing and requires great computer resources. The suitable mesh size is defined when this mesh size is enough to obtain good results, but the time processing has to be the smallest or the lowest computer resources required. To reach those, we selected the mesh combination in this study, including the coarse mesh size located near the boundary and the finer mesh size distributed in the area around the objective. Six meshes combinations are evaluated, as shown in

Table 2. Mesh qualities.

No.	Mesh Combination	Number of Nodes	Number of Elements	Skewness Quality	Orthogonal Quality
C1	0.4 m + 0.2 m	4279	20,364	0.255	0.744
C2	0.2 m + 0.1 m	20,278	100,991	0.237	0.762
C3	0.1 m + 0.05 m	98,000	506,809	0.231	0.767
C4	0.1 m + 0.02 m	121,911	640,701	0.229	0.769
C5	0.05 m + 0.01 m	606,363	3,274,660	0.222	0.777
C6	0.03 m + 0.075 m	1,499,081	8,120,961	0.221	0.777

. Figure 2 shows the process of finding the suitable mesh size when we calculated the $C_d$ of each combination. The combination mesh size of 0.05 m and 0.01 m became the suitable mesh size because the value of $C_d$ is stable on decreasing mesh size. Therefore, we applied this mesh combination for all simulations in this study.

Mesh configuration for the combination mesh of C5 (0.05 m + 0.01 m) is presented in Figure 3. This mesh comprises 606,363 nodes and 3,274,660 elements, where finer mesh sizes are placed near the pylon and coarser mesh sizes near the boundaries. The transition between the two mesh sizes is determined based on a growth rate of 1.2. To assess the mesh quality, Ansys software calculates two indices, skewness and orthogonal, which measure the difference between the shape of the cell and the shape of an equilateral cell of equivalent volume, and the vector from the cell centroid to each of its faces, respectively [30]. The results indicate excellent and very good cell quality for skewness and orthogonal methods, respectively, as shown in Table 2.

2.4. Domain

The computational domain is determined by the environment surrounding the object of interest. In the case of studying the bridge pylon, the computational domain includes the area surrounding the pylon. However, in reality, the domain size can be extremely large, such as the actual size of the room where a tunnel test is conducted. Therefore, it is important to reduce the domain size, even though it is always larger than the dimensions of the object. A similar approach was used in previous research to investigate the sensitivity of important output metrics to varying domain sizes and determine an appropriate domain size [31]. In this study, we also employed a similar method to determine the domain length and width, as shown in Figure 4a,b, respectively.

To determine the appropriate domain length, we increased it from 5.0 m to 12.5 m in increments of 2.5 m and analyzed the resulting drag coefficient ($C_d$) as the key output. As seen in Figure 4a, a domain length larger than 7.5 m yields a similar $C_d$ value. Therefore, we selected 10.0 m as the domain length for our simulation model. Similarly, we investigated the domain width using 4 different cases and selected the appropriate value based on Figure 4b, which was 2.5 m. Figure 5 shows the chosen domain length and width of 10.0 m and 2.5 m, respectively, for this study simulation.

2.5. Boundary Conditions

The boundary conditions (BCs) for our problem are similar to those in computational fluid dynamics. Since we have a rectangular domain, we need to define six surfaces. Typically, the front and back surfaces are set as the inlet and outlet BCs, respectively. The other four surfaces can be either symmetry BCs [32] or no-slip wall BCs [33]. In this study, we applied similar BCs: inlet and outlet for the front and back surfaces, symmetry BC for the top surface, and no-slip wall BC for the bottom and two side surfaces. Additionally, the interface between the pylon and the air environment is also BC and is assigned as a no-slip wall. Figure 5 shows all the BCs used in this study.

At the inlet BC, we specify the turbulent flow, velocity magnitude, direction, air pressure, and temperature. The outlet BC is applied to the back surface and sets the air pressure equal to the inlet condition. The symmetry BC ensures that the environment on both sides of the boundary is identical. The no-slip wall BC specifies that the boundary is stationary, there is no shear stress during the analysis, and the fluid does not slip at the boundary [30].

3. Results and Discussion

3.1. Number of Iterations

In CFX simulation, iteration refers to the process of repeating a calculation to approach the desired results or target with higher accuracy. The nature of the ordinary differential equations (ODEs) is not significant in the computational method as it uses approximate analytical methods. To solve ODEs, implicit solver iterative methods are required, and the Newton–Raphson method is used to linearize the nonlinear terms in each iteration step. At each iteration, the Jacobian matrix is applied when solving a large number of ODEs [34]. Equation (14) below shows the nonlinear term in the following form:

$$y^{\left(1\right)}=f\left(t,y\right)$$

(14)

where $f\left(t,y\right)$ is nonlinear concerning the approximate dependent variable $y$. We use the Backward Euler method to solve the equations as Equation (15).

$$y_{n+1}-hf\left(t_{n+1},y_{n+1}\right)=y_n,$$

(15)

where $n$ is the number of steps, $y_n$ and $h$ are the approximate dependent variable at the time step n and (n+1), respectively, and $h$ is the step size. The Newton–Raphson method was applied to solve Equation (15) to obtain Equation (16).

$$\left(1-h\frac{df\left(t_{n+1},y_{n+1}\right)}{d{y}_{n+1}}\right)\mathsf{\Delta }{y}_{n+1,i+1}=-\left(y_{n+1,i}-hf\left(t_{n+1},y_{n+1,i}\right)-y_n\right),$$

(16)

where $i$ is the iteration number and depends on the user’s purpose. The higher given iteration number provides more accuracy of the target results. In this study, we investigated the number of iterations of 10, 30, 50, 100, and 200 iterations and focused on the target value of drag coefficient, as shown in Figure 6. $C_d$ remains at a value of 1.22 from the number of iterations is 100. Hence, we selected this number of iterations for investigation.

3.2. Validation

The validity of the simulation approach used in this study was assessed by comparing its results with the findings from a tunnel test of the Cao Lanh bridge in Vietnam conducted by the Department of Civil Engineering at Chonbuk National University in 2016 [23]. The real and lab-scale dimensions of the free-standing pylon are described in Figure 7, where all dimension is in millimeter. The test involved a 1:75 scale model of the free-standing pylon being tested in a large, enclosed room, with an incidence wind direction of 0 degrees resulting in an average drag coefficient of 1.22. The corresponding $C_d$ values obtained from the simulation using the SST and k − ω models were 1.223 and 1.208, respectively, with very small errors of 1.24% and 0.98%, which can be considered negligible. As a result, the modeling results were deemed to be highly accurate.

The high level of accuracy achieved through the FVM method, as mentioned previously with errors less than 1.00% (k − ω models), makes it a suitable pre-feasibility study method for structures where creating a lab-scale model or conducting experiments would be difficult or expensive. Furthermore, the FVM method can be used as an independent research method to compare and evaluate results, thereby increasing the overall reliability of the project.

3.3. Drag and Lift Coefficients of Four Typical Cross-Sections

To optimize the cross-section of the pylon, four different sections were proposed based on previous structural standards [35]. These sections include the concave, convex, crossing, and chamfering cross-sections, which are detailed in Figure 8, with R representing the cutting radius. To investigate the geometry of the pylon section, the cutting radius was varied by 0.25 m, 0.50 m, 0.75 m, and 1.00 m for each of the 4 recommended cross-sections, resulting in 16 types of cross-sections. For each cross-section, simulations were conducted for 7 incidence wind directions ranging from 0 to 90 degrees, with a 15-degree interval, resulting in a total of 112 simulation cases. The symmetry properties of each cross-section allowed for the investigation of all incidence wind directions blowing around the pylon with only seven incidence wind directions.

Figure 9 illustrates the variation of $C_d$ and $C_l$ for the concave cross-section. The circle contours represent the magnitude of $C_d$ and $C_l$, and the values around the larger circle denote the incidence wind direction. $C_d$ ranges from 0.85 to 1.20, while $C_l$ ranges from 0.20 to 0.70, as shown in Figure 9a,b, respectively. The projected cross-sectional area and resistance force vary slightly with the incidence wind direction, leading to a relatively stable value of $C_d$. However, the difference in pylon shape results in a significant difference in the magnitude of $C_l$. For instance, at an incidence wind direction of 0 degrees, the inclined windbreak surface reduces the resistance force in the vertical direction, thereby decreasing the lift force and $C_l$. In contrast, at an incidence wind direction of 90 degrees, the vertical windbreak surface increases the lift force and $C_l$. These properties are well depicted in Figure 9a,b. The maximum $C_d$ is attained at incidence wind directions of 0, 30, or 90 degrees, while the maximum and minimum $C_l$ are achieved at incidence wind directions of 90 and 0 degrees, respectively. Figure 9, Figure 10 and Figure 11 show similar properties of $C_d$ and $C_l$ for the convex, crossing, and chamfering cross-sections, respectively.

The concave, convex, crossing, and chamfering cross-sections exhibited similar properties in terms of their maximum and minimum $C_d$ and $C_l$ values, which were obtained at specific incidence wind directions. The maximum $C_d$ was obtained at the incidence wind direction of 0, 30, or 90 degrees, while the minimum value was at 15 degrees or 60 degrees. Similarly, the maximum and minimum $C_l$ values were observed at the incidence wind direction of 90 and 0 degrees, respectively, corresponding to the vertical surface and the inclined surface of the pylon shape. These properties were also observed in the convex, cross, and chamfering cross-sections, as shown in Figure 10, Figure 11 and Figure 12.

In Figure 13, velocity fields for 4 wind directions are presented for a chamfering cross-section with a radius of 250 mm. Negative velocity values indicate that the incidence wind is opposite to the positive direction of the coordinate axis. The velocity or pressure differences in the front, behind, above, and below the pylon mainly affect the values of $C_d$ and $C_l$. In the case of $C_l$, its value remains stable because there is no significant difference in velocity (Figure 13) or pressure (Figure 14) between the front and behind areas. However, when the wind direction is at 30 degrees, there are 2 large and significantly different areas of velocity or pressure, as shown in Figure 13b and Figure 14b. This results in the greatest value of $C_d$. Similarly, different wind zones (represented by different colors) in Figure 13c,d and Figure 14c,d lead to varying velocities or pressures above and below the pylon. Consequently, $C_l$ is greater for wind directions of 60 and 90 degrees.

Figure 13 displays the velocity fields for a chamfering cross-section with a radius of 250 mm for four wind directions. Negative velocity values indicate that the incoming wind opposes the positive direction of the coordinate axis. The values of $C_d$ and $C_l$ are mainly affected by the velocity or pressure differences in the front, behind, above, and below the pylon. $C_l$ remains consistent since there is no substantial difference in velocity (Figure 13) or pressure (Figure 14) between the front and back areas. However, for a wind direction of 30 degrees, Figure 13b and Figure 14b indicate 2 large and significantly different areas of velocity or pressure, resulting in the highest value of $C_d$. Additionally, Figure 13c,d and Figure 14c,d show different wind zones (represented by different colors) that cause varying velocities or pressures above and below the pylon. As a result, $C_l$ is highest for wind directions of 60 and 90 degrees.

Figure 13 and Figure 14 provide valuable information on the velocity and pressure patterns, allowing authors to identify the region with low values of both parameters. These figures indicate that the section located in the middle of the pylon has the lowest velocity and pressure if we take into account the overall incidence wind directions. As a result, this region experiences the lowest aerodynamic force and has a high safety factor if the decorative or monitoring equipment is installed in this area.

Figure 15 and Figure 16 illustrate the velocity and pressure distributions for a chamfering cross-section under an incident wind direction of 0 degrees, where the cutting radius ranges from 250 mm to 1000 mm. While velocity fields provide some insight into the magnitude of drag and lift, pressure fields offer a clearer understanding. The extensive range of pressure changes results in small variations in the rate of change, leading to a small $C_d$ and vice versa. Therefore, the chamfering cross-section with a cutting radius of 1000 mm has the smallest $C_d$, whereas the cross-section with 250 mm has the largest. This principle applies to the velocity and pressure fields of the four recommended cross-sections, as demonstrated in Figure 17 and Figure 18.

After investigating four cases, we have identified that the values of $C_d$ and $C_l$ are dependent on the incidence wind direction, which is attributed to the variation in the shape of the windbreak surface. Consequently, $C_d$ and $C_l$ of the pylon are not constant for each type but specific to each incidence wind direction and pylon shape.

3.4. Effect of Non-Dimensional Cutting Ratio on Drag and Lift Coefficients

The non-dimensional cutting ratio is determined by dividing the cutting radius R by the original width of the pylon. In the case of the Cao Lanh pylon with actual width of 3 m, the non-dimensional cutting ratio is 0.083, 0.167, 0.250, and 0.333, corresponding to the cutting radius of 250 m, 500 m, 750 m, and 1000 m, respectively.

In Figure 19a, a quadratic equation with a high coefficient of determination (0.9736) is used to estimate the relationship between the non-dimensional concave ratio of the concave cross-section and its $C_d$. The graph shows that the minimum $C_d$ can be achieved when the non-dimensional concave ratio ranges from 0.2 to 0.3, which is the lowest point on the graph. The corresponding decrease in $C_d$ is up to 23.69%, creating a cusp, as illustrated in Figure 19b. On the other hand, $C_l$ decreases as the non-dimensional concave ratio increases and remains greater than 0.2 (within the range investigated), as demonstrated in Figure 19c,d, with a decrease of up to 8.92% concerning the non-dimensional cutting ratio of 0.33. As previously stated, lower values of $C_d$ and $C_l$ lead to greater stability of the pylon or equipment in direct contact with the pylon, such as the suspension bridge cable. Consequently, the non-dimensional concave ratio of 0.2 to 0.3 is the recommended ratio for the concave cross-section in increasing the pylon stability in aerodynamics.

The investigation of $C_d$ and $C_l$ of convex, crossing, and chamfering cross-sections were described in Figure 20, Figure 21 and Figure 22, respectively. Similar properties to the concave cross-section occurred in the convex and chamfering cross-section. The recommended non-dimensional ratio was 0.2 to 0.3 for both cross-sections, as shown in Figure 20 and Figure 22, which was similar to the concave cross-section. In terms of the crossing cross-section, because of the complicated shape of the cross-section, the estimated equation of the lift coefficient was a cubic equation. The recommended range of the non-dimensional crossing ratio for $C_d$ was 0.10 to 0.25, while its range for $C_l$ was 0.33. Finally, by investigating of nondimensional ratio on four types of cross-sections (i.e., concave, convex, crossing, and chambering), we recommended four ranges of each cross-section that can be given the best performance in reducing $C_d$ and $C_l$ of the pylon, as summarized in

Table 3. Recommended non-dimensional cutting ratios.

Cross-Section	${\mathit{C}}_{\mathit{d}}$	${\mathit{C}}_{\mathit{l}}$
Concave	0.20–0.30 (23.69%)	0.33 (8.92%)
Convex	0.20–0.30 (20.19%)	0.33 (10.40%)
Crossing	0.10–0.25 (17.66%)	-
Chamfering	0.20–0.30 (17.34%)	0.33 (13.14%)

.

For the value of $C_d$, 3 cross-sections (i.e., concave, convex, and chamfering) have the same recommended range (from 0.20 to 0.30). The crossing cross-section has a more comprehensive corresponding range (from 0.10 to 0.25). All 4 types of cross-sections significantly affected reducing $C_d$, and the maximum reduction is up to 23.69% with respect to the concave cross-section. In the case of $C_l$, except for the crossing cross-section, which has an ambiguous effect, the remaining three cross-sections gave the same survey results. The larger the value of the non-dimensional cutting ratio, the greater the $C_l$ reduction. Because the investigation range of the non-dimensional cutting ratio is only from 0 to 0.33, the maximum effect of cutting is at 0.33, and the chamfering cross-section has the most effect in four cross-sections (up to 13.14%).

Overall, the investigation found that the choice of cross-section shape has a significant impact on the aerodynamic performance of pylons. The recommended non-dimensional cutting ratios for concave, convex, and chamfering cross-sections were found to be in the range of 0.20 to 0.30, while the crossing cross-section had a broader range of 0.10 to 0.25. By selecting cross-sections within these ranges, the maximum reduction in $C_d$ and $C_l$ can be achieved, providing higher stability for pylons or equipment directly attached to them. The reduction in $C_d$ can be up to 23.69%, while the reduction in $C_l$ can be up to 13.14%, depending on the cross-section shape and non-dimensional cutting ratio.

The four cross-sections are capable of effectively reducing aerodynamic coefficients by changing the interaction surface from a flat nose to a rounded nose, which is shown in Figure 23. A flat nose obstructs the flow by directly blocking it and creates the largest obstruction because it is perpendicular to the flow. This generates a high-pressure area in front of the interaction and a low-pressure area behind it, resulting in a slightly higher aerodynamic coefficient. However, if the flat nose is replaced with a rounded one, the coefficients can decrease significantly as the high-pressure area in front of the interaction reduces and the flow becomes smoother. Overall, cutting the corners of a traditional rectangular section, regardless of which of the four types is used, transforms the section from a flat nose to a rounded nose. This is a primary reason for the reduction of aerodynamic coefficients.

3.5. Comparison of Four Recommended Cross-Sections in Drag and Lift Coefficients

Comparing the performance of each cross-section is important to understand their effectiveness in reducing aerodynamic forces. It is also essential to consider the specific application and operating conditions of the pylon when selecting the optimal cross-section. For example, the recommended range for the non-dimensional cutting ratio varies between cross-sections, and a smaller cutting radius may be more suitable for some applications than others. Therefore, it is essential to consider the trade-off between the reduction of aerodynamic forces and other factors, such as structural integrity and manufacturing feasibility.

Within the scope of our investigation, our focus was on the effectiveness of reducing the aerodynamic coefficients through the implementation of cutting edges. Therefore, we emphasize the performance of each cross-section in terms of their ability to decrease the aerodynamic forces via their coefficients.

Figure 24 presents a comparison of the four recommended cross-sections based on their $C_d$ (Figure 24a), the decrease in $C_d$ (Figure 24b), $C_l$ (Figure 24c), and the decrease in $C_l$ (Figure 24d). All four recommended cross-sections show similar trends. The values of $C_d$ and $C_l$ change rapidly in the non-dimensional ratio range of 0 to 0.1. Specifically, $C_l$ decreases rapidly from 0 to 0.1 but then stabilizes from 0.1 to 0.3. Therefore, cutting the 4 corners of the pylon by at least 10% of the pylon width is the most effective method to reduce drag force or increase the aerodynamic stability of the pylon. On the other hand, $C_l$ increases rapidly from 0 to 0.1 but decreases from 0.1 to 0.3. If the cutting ratio is less than 10% of the pylon width, it has a reverse effect on aerodynamic stability. However, a cutting ratio larger than 0.1 has a positive effect on reducing lift force around the pylon.

Among the four recommended cross-sections (i.e., concave, convex, crossing, and chamfering), the concave cross-section has the best performance in reducing $C_d$, as shown in Figure 24a. On the other hand, the chamfering cross-section provides the largest reduction in lift force or $C_l$. Therefore, the concave and chamfering cross-sections are the most effective sections for increasing the aerodynamic stability of the pylon.

4. Conclusions

The FVM is applied to estimate $C_d$ and $C_l$ in four recommended cross-sections and a series of incidence wind directions. The important findings have contributed to supplement the lack of research on the long-span bridge pylon, which are as follows:

(i)

We have already shown an insignificant error in calculating the aerodynamic coefficients by the FVM method. Hence, this method is a low-cost method for investigating the dynamic stability of the long-span bridge, especially suitable for the pre-feasibility study step;

(ii)

$C_d$ and $C_l$ are characteristic for each incidence wind direction and depend on the shape of the pylon. By investigating four recommended cross-sections, the maximum of $C_d$ and $C_l$ often come from the incidence wind direction of 0 or 90 degrees, which are the front face or side face of the pylon;

(iii)

$C_d$ and $C_l$, i.e., the drag and lift forces of the pylon reduced by cutting at the cross-section corner regardless of the cutting geometry and reduced up to 23.69% and 13.19%, respectively;

(iv)

In four recommended cross-sections, the concave and chamfering cross-sections stand out as the most effective section for increasing the aerodynamic stability of the pylon;

(v)

The non-dimensional cutting range is from 0.2 to 0.3 and provides the best performance in reducing the drag and lift forces of the pylon. This range is a recommended standard for adjusting the pylon cross-section to increase its dynamic stability.

By reducing drag and lift forces acting on recommended pylons with different cross-sections via their coefficients, we enhance the dynamic stability of the pylon, thereby prolonging the service life and stable exploitation of the pylon.

Cutting at the corners in the cross-sectional geometry not only reduces the dynamic forces acting on the pylon but also saves building materials in the discarded portions. For long-span bridges with many large pylons, cutting these corners saves a significant amount of material. Moreover, this corner cutting also brings high aesthetic efficiency by making the pylon appear softer compared to the traditional rectangular cross-section. However, this also poses some challenges in practice, such as more detailed cross-sectional shapes requiring the technical requirements of curved cuts, longer construction times compared to simple rectangular cross-sections, and, therefore, increased construction costs. Additionally, this corner cutting may also cause difficulties in arranging cable anchorages because the flat surface area is reduced. Therefore, it is necessary to choose a suitable cross-sectional shape and cutting ratio to overcome the difficulties that this approach may bring.