Wind responses on twin box girder bridge deck using a fluid–structure interaction approach

Wind responses on a twin box girder bridge can be observed by a wind tunnel experiment or by having a full-scale setup if possible. Another possible approach is to go through a numerical approach, which is the CFD simulation of the atmospheric boundary layer surrounding the twin box girder bridge deck. A virtual wind tunnel CFD modelling simulation was carried out on the bridge deck using the Ansys Fluent FSI technique to find out the displacement of the bridge deck. The steady-state simulations were computed. The turbulence model was used to calculate the mean force coefficients as K-ω SST. It has been seen that steady simulation is needed to get the static aerodynamic coefficients right when modelling. Ansys ICEM CFD is used for meshing the bridge deck. In this study, the wind flow behaviour around the structure is analysed at different wind incident angles of − 10°, − 5°, 0°, 5°, and 10°. The pressure variations at different wind directions are mapped in the present work. Responses across and along the wind are also depicted. It was found that the drag coefficient was higher at low angles of attack, whereas the moment and the lift coefficients showed fewer values at large angles.


Introduction
The instability due to aerodynamics is an important issue for discussion in the design of bridges with long spans.In bridge engineering history, many failures happened due to a lack of knowledge about the behaviour of the structure under the dynamic load due to wind, especially in the collapse of the Tacoma Narrows (Attia et al., 2016).In the design of bridges, especially long-span bridges, the wind load is always considered the most important load.After the collapse of the Tacoma Narrows Bridge in 1941, the major concern of the bridge designer was the flutter assessment.The wind tunnel testing of the bridge deck was carried out to determine the flutter derivative.Using the fluid-structure interaction (FSI) in a CFD (computational fluid dynamics) modelling and simulation approach, the flutter derivative can also be estimated (Szabó & Györgyi, 2009).The CFD approach is widely used as a complementary approach to wind tunnel testing and an additional analytical tool to discern the effect of wind forces on the bridge structure (Khan & Roy, 2017).Computational fluid dynamics (CFD) is used to solve different fluid flow problems (Roy et al., 2018;Singh & Roy, 2019a, 2019b).
A number of researchers have distinctly shown that the CFD approach is a possible complementary approach to a wind tunnel or full-scale experimental study (Hosseini, 2019;Verma et al., 2015;Wu & Kareem, 2013).The majority of the wind and structure interaction problems were solved using a wind tunnel experiment and design codes.Previously, it was uncommon to use computational fluid dynamics (CFD) to understand the aerodynamic behaviour of the atmospheric boundary layer (ABL) (Mashnad & Jones, 2014;Roy et al., 2017).The CFD approach is used to predict fluid response, but to know the structural response, the FEA technique is used for any model.To know the structural behaviour of the model, finite element analysis is performed.The FEA technique was employed in the evaluation of the structural behaviour of bridge decks due to several loads, and it has also been observed in numerous studies (Lanzafame et al., 2016).However, the boundary conditions used for finite element analysis, i.e. loading, are still obtained from wind tunnel experimentation or CFD (Benra et al., 2011;Chen et al., 2015;Teixeira & Awruch, 2005).The fluid-structure interaction technique is used here, which combines these two approaches to fulfil the objective of the work.The FEA is used for the structural response of models such as displacements, forces, and stresses.
This paper uses the FSI approach to find out the structural response of the bridge deck section under wind conditions.In this work, ANSYS Fluent is used as the commercial software.The shape of the bridge deck is chosen by a design engineer based on past experiences and after a wind tunnel experiment, to understand how the aerodynamic behaviour is affected by the shape of the deck at different wind angles of attack for ease of deck shaping procedures on bridge decks (Ahamed et al., 2017).During a wind tunnel test, it was discovered that as the wind's angle of attack changed, dissimilar pressures were induced on the outside surfaces of the structure with the "+" shaped plan (Haque et al., 2016;Kaveh et al., 2022).In bridge aerodynamics, there are two ways to represent the mean wind load by using the structural coordinate, one of which is the wind coordinate, as shown in Fig. 1.
In Fig. 1, the wind coordinate system shows three different types of mean load.First is the drag force that acts along the wind direction and is defined as the integral of pressure on the bridge deck along the wind direction.The second is the lift force, which acts in the perpendicular direction, and the integral of the pressure, which operates in the perpendicular direction to the mean wind pressure.The third is the moment of torsion, which is the moment of the resultant force, and the distance taken from the centroid (Chakraborty et al., 2014).
A number of studies have been conducted on bridge aerodynamics, but all the studies have been performed on a 2-D model of a bridge deck.The reason behind this is an increase in computational cost and time.A lot of research has been done to predict the flow behaviour of wind around the boundaries of bridge deck geometry (Mannini et al., 2010).To reduce the computational time and cost, hybrid meshes are used, which are fine meshes near the wall and coarser meshes far from the wall (Mannini et al., 2010;Patruno, 2015;Xu et al., 2011).Very few researchers have worked on the 3-D bridge deck.In India, different Indian standards are used for evaluating wind loads.The Indian wind code is IS 875 (Part 3) (Raja, 2012).This Indian standard provides wind forces (static and dynamic) and the effect of wind forces.While designing the buildings and structures, these forces should be considered.For bridges, IRC-6 provides a clause for the calculation of wind loads on bridges (IS: 875 2015).IRC-6 has a different clause that provides information for calculating the transverse and horizontal forces on a bridge deck using different force coefficient values.

Research scope
The choice of the shape of the bridge deck is typically informed by the design engineer's previous experiences and wind tunnel experiments.However, there is limited research available regarding how different bridge deck shapes affect aerodynamic behaviour at various wind angles of attack.Thus, additional research is required to understand the impact of different bridge deck shapes on aerodynamic behaviour and to establish guidelines for selecting the most suitable deck shape for different wind conditions.The purpose of this study is to investigate the aerodynamic behaviour of bridge deck at different wind angles of attack.

Methodology
In FSI, two types of approaches are available, i.e. a oneway or two-way approach (Chen et al., 2015).The one-way approach is less complicated than the two-way approach.In this approach, a converged solution obtained from a fluid solver is used for the structural solver as a boundary condition.However, the two-way methodology solves both solid and fluid equations independently and iterates within each time step to obtain an implicit solution.The dependencies between the solid and fluid fields are implicitly converged within a time step (Xu et al., 2011).In the case of unsteady transient turbulence models, two-way FSI analysis is more suitable, while steady simulations utilise a one-way FSI approach (Teixeira & Awruch, 2005).The one-way is easier to implement as compared to the two-way FSI due to the variability of obtaining convergence and the potential of having numerical singularities during the simulation in the interface and fluid domains.The flowchart of the one-way FSI that is used in this study is shown in Fig. 2.

CFD simulation
The settings and criteria of the computational domain are presented in this section.The model creation, meshing, and setting of the mechanical and fluid solvers that were utilised to solve the problem are also discussed.

Geometry
The model of the Hanogi cable-stayed bridge used to study the FSI is shown in Fig. 3a.A small portion of the bridge deck is considered to avoid computational issues such as computational cost and computational time.The 22-m-long deck section is used here to study the wind parameters given in Fig. 3b.The assumptions are taken while modelling deck geometry.Sharp edges are modelled in place of rounded edges at the deck's corners to avoid complex meshing.In ANSYS, the design modeller software is used to create the geometry of the bridge.It has an excellent user interface and is easy to handle.Another CAD software is recommended for new design modeller users.Because the ANSYS workbench supports different kinds of CAD file formats, like the software solid work file format, it is supported in the ANSYS workbench.So, for smooth working, a well-known software may also be used.

Computational domain and its meshing
In this study, a computational domain (see Fig. 4a, b) was used and meshed to accurately mimic the ABL in wind tunnel geometry.The computational domain adheres to the finest practise recommendations by Franke et al. (Petit, 2007;Revuz et al., 2012).The dimension of the mesh is shown in Fig. 4a (Fransos & Bruno, 2010).The size of the minimum element is about 2.5 mm, and a growth rate of 1.1 was used here to scale the appropriate computational fluid domain.
To ensure that the CFD results are not affected by the grid, a grid-sensitivity analysis is performed using four different mesh types, namely, the finest, fine, medium, and coarse grids, and the results are incorporated.The medium mesh is found suitable for this study, which is shown in Fig. 4b, c.

Grid-independent test
It is very obvious that the CFD solution depends on the grids.So the solution from fluid dynamics can never be trusted if we do not have any experimental values to justify our solution.The solution of a coarse mesh and a fine mesh can never be the same.So by varying a mesh again and again, it does not impact your solution, so we stop at that point and choose a minimum mesh, and the result of that mesh is our final solution.In this study, a medium-size mesh is used because this mesh provides results that do not vary much with the variation in mesh sizes.Table 1 presents the details of the grid-independent test.

Boundary conditions
Boundary conditions are constraints that come in handy when trying to solve a boundary value problem.These boundary conditions are an essential part of a numerical model.These provide a well-defined path for the flow of fluid motion, resulting in a unique solution.There are different boundary conditions provided in any general Ansys  CFD such as inlet, outlet, wall, symmetry, and many others.
In this study, mixed boundary conditions are used.These boundary conditions are mentioned in Table 2.

Fluid solver setting
The finite volume approach is used by Fluent.In the finite volume method, the domain is divided into small volumes called "finite volumes."The finite volume is also called a  cell.Each cell stores the information in its centroid.It follows the concept of conservation.The governing equations of conservation should be satisfied in each cell.The governing equation is the Navier-Stokes equation (Mishra & Roy, 2007).It conserves mass, momentum, and energy.So the quality and size of the cell should be such that these equations are solved accurately and without error.Table 3 shows the solver settings used in fluent.

Mechanical solver setting
In the mechanical solver of ANSYS, the setup part is easy compared to the fluid solver.Here only the named selection of the geometry has to be specified, and if the named selection was given in the previous part, i.e. the geometry part, then there is no need to do it again.The next step is to assign pressure or another load to the structure.After that, provide the analysis set, which is an essential part of the whole setup.
Care should be taken while delivering the setup as per the requirements of the project.It helps to generate accurate and precise results for the given problem.

Material properties
The fluid solver that is used here is fluent.The material used is air.A static structural solver and static structural two materials are used to solve the structural part.For the deck and one for the steel reinforcement.The first material is concrete nonlinear, and the second is structural steel nonlinear.These materials can easily be found from the engineering data on the Ansys workbench.Table 4 represents the used fluid properties.In this study, two properties are used in the structural portion.The first is nonlinear structural steel, and the second is nonlinear concrete.In this study, the modified features are used as per requirements.Table 5 shows all the properties of the structural system.

Coupling setup
The last and most relevant part of the simulation is the coupling.The one-way coupling is used here.The one-way coupling has been discussed previously in Sect."Methodology".The guided user interface (GUI) of the one-way process is shown in Fig. 5.
GUI helps transfer the data of the fluid solver to the mechanical solver and import the pressure of the fluid flow on the structural system.

Results and discussions
In the present work, the deck of a bridge model was simulated through CFD at different wind angles.The current study's goal is to detect vortex generation, determine the variation in wind pressure distribution with changing wind angles, and calculate displacement due to this wind pressure.

Velocity streamlines
The flow variation is shown around the deck section.The streamlines at different angles of attack (AOA) are represented.All these figures are in the X-Y plane.It is observed that by changing the angle of attack, the wake region widens suddenly.The formation of vortices is distinctly visible in each figure.As the angle is increased, irrespective of whether it is positive or negative, the vortex shedding is also increased on the leeward side of the deck.von Karman street effect was observed.In fluid dynamics, a pattern of circular vortices is repeated by a phenomenon of vortex shedding called Karman vortex street (Xu, 2013), as shown in Fig. 6f, which is observed around bluff bodies.
In Fig. 6a, the streamline at 0° is shown with clear vortices formation.In Fig. 6b and d    direction of wind velocity is from − X to + X.In Fig. 6, the left side of the deck is the windward side, and the right side of the deck is the leeward side.The constant wind velocity of 39 m/s is taken as per Indian standard code (IS: 875 2015).In Fig. 6c and d streamlines are presented at 10° and − 10° respectively, and it was distinctly observed that the maximum velocity was reduced as the angle of attack increased or decreased.The separation was also seen on both the upper and lower surfaces.At the corners of the deck, a sudden increase in velocity was observed on both the upper and lower surfaces (Fig. 7).
For the increased depth of deck, it can be seen that the velocity streamlines at the corners reach 72 m/s, whereas the increased deck has a maximum velocity streamline of about 58 m/s and the standard deck has the least velocity streamlines of about 52 m/s.Both the top and bottom surfaces are separated.On both the top and lower surfaces of the deck, there is a rapid rise in velocity at the corners.

Pressure variations around the structure
The variation in pressure is shown in the following figures in the form of raster contours.The unit of pressure is Pa.The variation is again shown at different wind angles and remarkable changes are seen.These pressures are within the limits of the Indian Road Congress specification (IRC-6-2016) (IRC-21-2000) (Fig. 8).
It was distinctly observed that the maximum pressure was on the windward side.This is positive pressure.Negative pressure is also observed, which is also known as the lowpressure zone.At every wind angle, flow separation takes place and creates vortices on the downstream side.This is known as vortex shedding.
At both positive and negative angle of attack (AOA), lowpressure regions are created at the downstream side, which increase with an increase in angle from 0° to 10°.Low pressure creates a vacuum zone in the region and suction takes place.So movement is observed in vertical as well as in horizontal direction (Fig. 9).
The suction is increased drastically with the variation of the deck size.The standard deck considered has a maximum suction pressure of 1000 Pa, the deck with increased width is found to have a suction pressure of 1453 Pa, which is 40% higher than the standard size of bridge deck, and finally, the suction pressure for the deck with increased width is the highest at 3872 Pa, which is 3.8 times higher than the standard size of deck.The positive pressure observed is almost the same for all three decks, varying from 860 to 950 Pa.So, as it is found that the standard deck has the highest factor of safety and has positive and negative pressure within permissible limits according to IS 875, the static displacement of this deck is further found out using ANSYS Static Structural.

Variations of static wind force coefficients
The variation of drag coefficient, the variation of lift coefficient, and the variation of moment coefficient concerning the angle of attack of wind were studied.The wind force coefficients for the bridge deck section are plotted in Fig. 8.With these coefficients, the mean forces on the section of the bridge deck can be determined.The model used is the K-ω SST model (Fig. 10).
It is observed from these graphs that the wind force coefficients depend on the angle of attack of the wind.The coefficient of drag clearly showed a decreasing slope up until the angle reaches zero.Both models provide approximately the same wind force coefficients.The use of these coefficients is not only limited to the determination of mean wind load, but is also used to determine buffeting forces and galloping stability.These coefficients are also called aerodynamic coefficients.

FSI structural analysis
Using FSI analysis, total displacements were obtained at different wind angles.In the present study, maximum displacements of the deck due to wind pressure occurred on the windward side at a 0° wind angle (Fig. 11).The displacement plots and imported pressure are shown in Fig. 9b and a, respectively.
Further observation indicated that the lowest pressure was on the leeward side and the highest on the windward side.

Along-wind and across-wind response
The displacement is monitored in terms of along-and across-wind responses, as shown in Fig. 10a and b, respectively.It was detected from the figures that the displacements due to wind vibrations were very small in both directions.A comparison of response is shown in both directions by  (Xu, 2013) choosing suitable paths on the deck surface.All the dimensions are in metres (Fig. 12).
Due to wind pressure, only such types of displacements are seen.The value of displacement is higher on the windward side as compared to the leeward side.The displacement due to pressure load changes with time and within the limit as per the IRS code of practise for plain, reinforced, and prestressed concrete for general bridge construction in 2014.

Aerodynamic coefficients time history
The only way to determine the critical speed is to do an unsteady evaluation of the force coefficients.This is accomplished by gradually increasing the speed of the wind coming in via the entrance.When the aerodynamic coefficient amplitude starts growing at a certain velocity, the condition is said to have occurred.Therefore, the speed is referred to as the critical velocity (Fig. 13).
1.When the wind speed is 30 m/s, the amplitudes of the moment and lift coefficients begin to decrease as time passes.This indicates that the model's overall damping is positive.2. When the wind speed is 35 m/s, the amplitudes of the lift and moment coefficients are about the same.3. When the wind speed exceeds 40 m/s, the amplitudes of the moment and lift coefficients begin to grow with time.
As a result, the critical velocity for this bridge deck is between 38 and 40 m/s.The flow around the structure is observed closely.The structure is subjected to a different angle of attack, and the remarkable points of this work are as follows: • As the angle of incidence varies, vortices are generated on a very large scale.Due to the large generation of vortices, the vibrations in the structures also increase and cause damage to the structure, if the frequency of these vibrations is the same as the natural frequencies of the structures producing resonance.• At different positive angles of wind, the wake region becomes wider as compared to the 0° angle.This region is created due to flow separation, which is visible in this work.As a result of flow separation, reduced lift force and an increment in pressure drag are observed, due to which buffeting of structures can take place.• At every wind angle, flow separation takes place and creates vortices on the downstream side.This term is also called vortex shedding.At both positive and negative angles of attack, a low-pressure region forms on the downstream side, which increases as the angle increases from 0° to 10°.These low pressures create a vacuum zone, and the structure moves towards this low-pressure zone.It will create a movement in structure in both the vertical and horizontal directions.If the structure involves both vertical and rotational motion together, it will lead to instability called "flutter."

Fig. 1
Fig.1A representation of mean wind load in the wind and structural coordinate system(Xu, 2013)

Fig. 4 a
Fig.4a Size of the computational domain(Fransos & Bruno, 2010), b computational domain with deck model, and c computational domain with quality check , streamlines are shown at 5° and − 5° wind angles, respectively, with the same vortex formation but with different maximum wind velocities.The triad shown in the figure represents the X-Y plane.The

Fig. 5
Fig. 5 Graphical user ınterface of one-way coupling

Fig. 9
Fig. 9 Pressure variations on a standard deck, b deck with increased width and c with increased depth

Fig. 11 a
Fig. 11 a Imported pressure and b total displacements

Fig. 12 a
Fig. 12 a Along with wind response of deck section and b across-wind response of deck section

Table 3
Solver setup

Table 4
Fluid properties

Table 5
Structural properties of the member