1 Introduction

The flow over a cylindrical tube continues to be a formidable obstacle in the research area of fluid mechanics for many years. Determining the intricate chaotic dynamics of the wake flow continues to require exhaustive investigation. Problems associated with the heat and mass transfer due to cross-flow perpendicular to the axis of a stationary tube occur in many engineering applications. Both numerical calculations and experimental data have shown that the wake flow beneath a cylinder becomes unstable at Reynolds numbers (Re) greater than a certain value, leading to a periodic flow with distinct frequencies acknowledged as the Von Karman vortex street, which is well-known in the scientific community [1]. When laminar flow passes over the cylindrical tubes featuring a regular polygonal cross-section, it is typically separated at different pointed angles of the geometry of the cross-Sect. [2]. This separation results in the generation of a vortex system in the wake, which extends on both sides of the middle-symmetry plane.

Conversely, the physics of the flow in a cylindrical tube at the point of flow separation is determined by the characteristics of the upstream boundary layers. These layers are considerably more intricate than their comparatively uncomplicated appearance would indicate [1, 3,4,5]. A multitude of physical complexities arise as the Re changes from a laminar value of approximately 0.1 to a turbulent flow with a Re value of 1 M or greater [6,7,8,9]. At Reynolds numbers between 5 and 40, the steady laminar flow is assessed based on the development of two symmetric counter-rotating vortices behind the tube [10,11,12,13]. Depending on the presence of additional flow disturbances, oscillations and vortices emanating from the cylindrical surface occur beyond a critical value of Re. It has been observed that the wakes generated by two-dimensional cylinders become vulnerable to a primary instability mechanism at Re = 190 and Re = 260 [14,15,16,17,18]. This vulnerability results in the amplification of 3D disturbances and ultimately gives rise to the formation of powerful stream-wise oriented vortices. The evolution and shape of the wake vortices are significantly changed by these 3D disturbances. Consequently, the 2D simulations frequently prove inadequate in terms of accurate determination of properties like lift coefficient, drag coefficient, vortex velocity, lift fluctuation, and Strouhal Number (St) even at low Reynolds numbers. Steady-state simulations are generally used for the time-independent flows for fully developed flows. On the other hand, the steady-state simulations may fail to capture unsteady phenomena such as vortex shedding, flow separation, and transient effects. Therefore, the transient flow simulations are very important for such analyses.

Furthermore, the cylindrical tubes are the common component in the flow structure which is broadly used in modern industry primarily for turbo-kinematics [18]. The CFD and empirical data of flow resistance for both steady and transient conditions can be used to enhance the turbomachinery output which can be helpful in the optimization of turbomachinery performance [4]. In Industry, the various components of turbines, compressors, and pumps are connected with the various sizes of cylindrical tubes. These devices use very precise transformation of energy from one form into another by just moving or spinning objects. Aircraft propulsion, compression of gases, or electricity generation are the most common applications which are connected with the different types of tubes. The major feature of turbomachinery units is the interconnection between the liquid flow and the cylindrical tubes in which liquid passes [7]. This study is aimed to analyse the influence of laminar flow over the cylindrical tubes used in the turbomachinery.

Literature review revealed that various turbulence models, including the k-ε, k-ω, Large Eddy Simulation (LES), and Direct Numerical Simulation (DNS), exhibit a range of degrees of complexity and precision. The LES and DNS help provide more accurate results but at a higher computational cost than the RANS models. In this study, the numerical results in the form of wake flow structures, the drag coefficient, stagnation pressure, and wake beneath the cylinder are numerically investigated as the value of Re increases from 10 to 10,000. The accuracy of numerical models depends on the validation of numerical models. In this study, the model’s validation was done by comparing them with experimental data. Furthermore, both steady and transient conditions of flow are numerically studied. The lift and drag coefficients as well as plots to show the vortex shedding behind the cylinder are evaluated numerically. Utilizing a steady-state solver, the coefficient of drag and lift over a cylinder was determined at different Re values. So, the detailed study of parameters can help minimize the vortexes for the cylindrical components used for the fabrication of the turbomachinery parts.

2 Mathematical modelling

2.1 Governing equations

The Navier-Stokes equations which describe unsteady laminar incompressible flow, can be expressed succinctly in the following manner adopting non-orthogonal curvilinear coordinates, which are utilized in the numerical simulation:

2.1.1 Momentum equation

The continuity equation provides the following supplement to these three momentum equations:

$$\eqalign{& {{\partial (p{U_i})} \over {\partial t}} + {1 \over J}{\partial \over {\partial {x_j}}} \cr & \left[ {(p{U_i}{U_k}{\beta _i}^j) - {\mu \over J}\left( {{{\partial {U_i}} \over {\partial {x_m}}}{B_m}^j + {{\partial {U_k}} \over {\partial {x_m}}}{\beta _i}^m{\beta _k}^j + P{\beta _i}^j} \right)} \right] = S{U_i} \cr}$$
(1)

In the above equation, J denotes the Jacobian transformation between Cartesian and curvilinear coordinates, \({\beta _i}^j\)and \({\beta _i}^j\) are the pertinent metric coefficients associated with the geometrical transformation, P represents the pressure, and j, k, and m function as repeated summing indices in the direction of the grid. The calculated mean cartesian velocity in the ith direction is denoted as Ui.

2.1.2 Continuity equation

The finite volume analysis was performed to solve the mass flow in the governing equations. The current algorithm for flow solutions (RANS3D) is a two-step iterative predictor-corrector process that is comparable to Patankar’s SIMPLE algorithm [11]. The momentum equations were solved during the predictor phase to partially develop the velocity field in time for a pressure field that is estimated. The Poisson’s equation was used for pressure correction using the continuity equation followed by a corrector step. This provides the necessary corrections to the pressure and velocity fields. Additionally, the temporal derivatives are discretized utilizing a three-level entirely implicit scheme which provides accuracy to second-order derivatives. To guarantee the stability of the solution numerically, a deferred correction procedure [12] was implemented. In this procedure [12], a suitable weighting function was used to combine the desired scheme flux with upwind fluxes that permit a small amount of numerical diffusion. The flux balance equation was implicitly represented in the subsequent quasilinear form by employing 2nd order temporal and spatial discretisation methods in conjunction with the pertinent geometric factors:

$$\int {{{\partial \phi } \over {\partial t}}\Delta v + {A_P}{\phi _P}^{n + 1} = } \sum\nolimits_{nb} {{A_{nb}}{\phi _{nb}}^{n + 1} + SU}$$
(2)

In the given expression, AP = ƩAnb –SP, denotes the mutual effect of convection and diffusion from adjacent nodes at the cell faces (coefficient Anb), the components of the linearized source term (SU and SP), the volume of the cell (Δv), and the time step size (Δt). The time increment is denoted by the superscripts of ɸ. The comprehensive explanation of Eq. (3) concerning the cell face projection areas and flow variables can be found in another source [3,4,5].

In the form of Eq. (3), the Poisson equation was used for the pressure correction. In conjunction with the firmly implicit procedure provided by Stone [13], a segregated iterative method is utilized to sequentially solve the system of linear equations (Eq. 3) that corresponds to each transport equation. The normalized residue for each solved equation is reduced at each time step until it reaches an acceptable convergence threshold of 104.

2.2 Dimensionless number and coefficients

2.2.1 Strouhal number (St)

The St was employed to characterize a flow system that oscillated. The St is frequently expressed as [14]:

$$St = {{f \times D} \over U}$$
(3)

In this equation, the parameters are the characteristic diameter of the cylinder (D), the frequency of vortex scattering (f), and the fluid flow velocity (U).

2.2.2 Coefficient of drag (C d)

The Cd was adopted to calculate the drag that the cylindrical tube experiences against the moving fluid. The drag coefficient was computed utilizing the subsequent equation [15]:

$$St = {{2{F_d}} \over {p{u^2}A}}$$
(4)

In Eq. 4, the parameters are described as follows: ρ represents the mass density of the fluid, u signifies the object’s flow speed in relation to the fluid, Fd denotes the drag force, which is defined as the force component acting in the direction of the flow velocity, A signifies the reference area.

2.2.3 Lift coefficient

The lift coefficient (Cl) represents the amount of lift produced by flowing fluid [16]:

$${C_l} = {L \over {qS}} = {L \over {{\raise0.5ex\hbox{$\scriptstyle 1$}\kern-0.1em/\kern-0.15em\lower0.25ex\hbox{$\scriptstyle 2$}}p{u^2}S}} = {{2L} \over {p{u^2}S}}$$
(5)

In Eq. 5, the lift force (L), the pertinent surface area (S), and the fluid dynamic pressures (q) were used to calculate the value of Cl. Here, ρ represents the fluid density, and u represents the flow speed.

3 Numerical modelling and simulation parameter

The FLUENT module was initially opened in the ANSYS workbench by using the drag-and-drop method. The following stages were used to solve the problem.

3.1 Geometry and meshing

A plate with the dimensions 20 × 60 produced by placing a cylinder wall of 2 mm thickness at the distance is shown in Fig. 1. To solve the flow domain, the geometry was first meshed. Initially, the faces were named as inlet walls, outlet walls, symmetry walls, and cylinder walls. In the next step, the colours were blended. A baseline mesh was created in this study. The triangular method was selected in order to mesh the rectangular domain geometry. The size of the cell was taken as 0.1 m. The meshed domain is shown in Fig. 2(a). The number of divisions of the circle was increased for acquiring a 2D cylindrical shape and an adequate size of cylinder was chosen i.e. a total of 36 divisions were selected. With the help of the inflation layer, the design of a mesh was body-fitted. This indicates that a layer of mesh was generated whose geometry was identical to that of the originating cylinder. Because the flow surrounding the cylinder has a critical significance, this type of region is required in the form of inflated layers to ensure the accurate representation of fluid flow. After the inflation, the first layer was found to have a thickness of 5 mm and a total of six layers were generated, as seen in Fig. 2(b). The value of the growth ratio was calculated as 1.2.

Fig. 1
figure 1

Geometry of flow domain

Full size image
Fig. 2
figure 2

Meshed domain (a) before and (b, c) after inflation

Full size image

3.2 Flow domain

The flow domain was solved using FLUENT code which is configured using initial conditions, boundary conditions, and material. Computational domain size plays a crucial role in boundary effects, capturing flow features, and transience effects. The computational domain size is necessary to be large enough to capture all relevant flow features, including boundary layers, separation zones, and wake regions behind the cylindrical tube. For transient flow conditions, the computational domain size influences the propagation of transient flow characteristics. A larger domain size may be necessary to allow transient effects, such as vortices shedding behind the cylinder in order to propagate and dissipate without interacting with the domain boundaries prematurely. Both the steady and the unstable cases were simulated in the experiment conducted for flow around the cylinder. In both of these methods, the flow reached a point of convergence and the Strouhal number (St) was computed at different values of Re. Firstly, the quality of the mesh was checked on the mesh which was found superior. In the next step, the various conditions were set such as the solver, viscous model, beginning and boundary conditions, etc. For transient flow along a cylindrical tube, the inlet boundary conditions accurately represent the time-varying flow profile. Inlet velocity profiles, inlet turbulence intensity, and inlet turbulence length scale are crucial parameters to specify for transient simulations. Outlet boundary conditions are essential for allowing flow to exit the computational domain without reflections or disturbances. For transient simulations, the outlet boundary condition was chosen to prevent artificial wave reflections that can affect the accuracy of the results. Common outlet boundary conditions include pressure outlet, mass flow outlet, and outflow conditions, depending on the flow characteristics and desired modelling assumptions. Wall boundary conditions are crucial for capturing the interaction between the fluid flow and the solid surface of the cylindrical tube. In transient simulations, an accurate representation of wall boundary conditions is essential for capturing transient effects such as boundary layer development, flow separation, and vortex shedding. To solve the numerical model, the pressure-based solver was used that operates in a steady state (time) condition. The velocity formulation was selected as an absolute value. The viscous model was selected as laminar since the value of Re was very small. This model was proposed for the calculation of the drag force and pressure drop, flow regime transition, particle or bubble dispersion, and flow instabilities. The air was taken as a working fluid. The dynamic viscosity, density and viscosity of fluid as well as the velocity of flowing fluid were varied in order to control the value of Re. The Reynolds equation was employed to simulate the numerous values of Re by varying the velocity. A steady state solver was employed to determine the coefficient of drag and lift over a cylinder by first adjusting the Reynolds number to 10, 100, 1000, 10,000, and 100,000 respectively. The different values of Re were chosen as 10, 100, 1000, 10,000, and 100,000 at a velocity of 0.25, 2.5, 25, 250, and 2500 m/s. The vertex velocity was generated and the iterations were initialized. A total of 450 iterations were performed for each velocity. The drag coefficient, Strouhal number, and lift coefficient were calculated based on these parametric variations. The inlet conditions were taken as: area = 2 m2, density = 1 kg/m3, depth = 1 m, enthalphy = 0 J/kg, length = 2 m, Pressure = 0 Pa, temperature = 288.16, viscosity = 0.05 kg/ms, ratio of specific heats = 1.4, Y + for heat transfer coefficient = 300. The validation of the numerical model was done by comparing the numerical results of the coefficient of drag with the analytical results. The present numerical model showed a good agreement with the analytical results and had a deviation of ± 3.68%, as shown in Fig. 3.

Fig. 3
figure 3

Validation of numerical model

Full size image

4 Results and discussion

Numerical simulation was performed to calculate the coefficient of drag, coefficient of lift, and vortex shedding behind the cylindrical tube. The following results were evaluated using the numerical simulations:

Fig. 4
figure 4

Comparison of various parameters for steady state and transient condition (a, b) Strauhal number, (c, d) vortex velocity, (e, f) coefficient of drag, and (g, h) coefficient of drag

Full size image

4.1 Steady-state versus transient condition

Figure 4 illustrates the comparison between the steady state and transient condition for a cylinder. It was found that the solution is more detail-oriented than in steady state. Since it is time-dependent, the difference in time steps and the total time steps are mentioned to calculate for vertices’ steps, but the efficiency is not superior in the former case as observed by data comparisons.

The results of the Strauhal number for steady and transient conditions for Re = 100 are shown in Fig. 4(a, b). The value of the Strouhal number in the steady state was found very close to 0.08 whereas the Strouhal number in the transient state was found as 0.076. In case, the Strouhal number is significant (approximately 1), the viscosity of the fluid supersedes its flow, resulting in a cohesive oscillatory motion exhibited by the fluid “plug” [17,18,19,20,21,22]. Conversely, although the St is comparatively smaller, the oscillation is primarily characterised by a quasi-steady-state and high-velocity component [23,24,25,26,27,28]. At intermediate Strouhal numbers, oscillation is characterised by the swift generation and consequent dissipation of vortices. Such occurrences are frequent throughout the oscillation. Additionally, in the case of coefficients of drag, the steady state value was found as 1.33 whereas 1.38 in the case of transient state value (Fig. 4e, f). The pressure force oscillation analysis helps to minimize vibration-related issues, optimization of performance, and enhance operational efficiency. The lift coefficient was found as -0.08 in the steady condition and − 0.076 in the case of the transient state (Fig. 4g, h).

4.2 Effect of variation of Re

4.2.1 Vertex average of velocity magnitude

The vortex velocity was calculated for the inlet velocity condition of the V = 2.5 m/s, viscosity of 0.05 kg/m-s, and density of 1 kg/m3. The vortex velocity was calculated at different values of Re i.e. 10, 100, 1000, 10,000, and 100,000. It was found that the magnitude of the vortex velocity drops after certain iterations and becomes stable after a passage of time. Figure 5 shows the vertex average of velocity magnitude with respect to time at different Reynolds numbers. From Fig. 5(a), it can be found that the vortex velocity gradually drops as time increases. Afterwards, it becomes steady at Re = 10. However, at Re = 1000, vortex velocity drops suddenly and increases sharply after a small time interval (Fig. 5b). After this rise, the vortex velocity follows a wavy pattern at a steady state. In Fig. 5(c), the vortex velocity follows a wavy pattern and doesn’t become steady. This represents a wake pattern at a steady state condition. Figure 6 represents the vortex velocity in terms of Re. It can be perceived that as the Re increases there is a sudden increase in the value of vortex velocity. This phenomenon is previously observed by many investigators [28,29,30]. The flow characteristics over a cylindrical tube change with variations in the values of Re. The flow characteristics remain laminar at lower values of Re (typically Re < 2000) and are characterized by smooth, regular flow patterns with well-defined streamlines. The flow characteristics become turbulent as the value of Re increases (Re > 4000 for flow around cylinders). Turbulent flow is characterized by chaotic, unsteady motion with significant mixing and vortices. The Cd also varies with the Re which remains lower at lower Re value [31]. However, the drag coefficient increases with Re due to the development of larger separation zones and increased turbulence intensity. The boundary layer thickness for the laminar flow remains thin and relatively stable along the surface of the cylinder. In turbulent flow, the boundary layer becomes thicker and more turbulent which leads to increased mixing and higher skin friction. Vortex shedding is generated behind the cylinder in turbulent flow regimes. It was perceived that the frequency and strength of vortex shedding increase with Re. At certain Reynolds numbers, the shedding frequency may synchronize with the natural frequency of the system which may lead towards the vortex-induced vibrations. Also, the cavitation can be mitigated by the vortex-free design which also may help in preventing the bubble formation around cylindrical components.

Fig. 5
figure 5

Time-dependent vertex average of velocity magnitude at (a) Re = 10, (b) Re = 1000, and (c) Re = 100,000

Full size image
Fig. 6
figure 6

Vertex Average of velocity magnitude at different values of re

Full size image

4.2.2 Coefficient of drag

Figure 7 shows the variation in the drag coefficients (Cd) over time which was determined separately for various values of Re by the 2D flow models. At a lower value of Re (i.e. Re = 10), the value of Cd drops suddenly then it attains a steady condition, as shown in Fig. 7(a). Similar types of trend were observed in the case of Re = 1000 but the curve follows a waviness pattern (Fig. 7b). As shown in Fig. 7(c), a periodic but statistically stationary condition of the flow was attained after the first transients have subsided during the early time steps at Re = 100,000. The inconsistencies were previously explained by Mittal and Balachandar [32]. According to them, the inconsistencies arise because of the vortex structures of the flow extracting energy from the 2D shedding motion. As a result, the mean drag was reduced as the base pressure rose and the 2D Reynolds stresses decreased. Furthermore, the trend of the drag coefficient was also analysed for the increase in Reynolds number. Figure 8 represents that the value of Cd drops with the increase in the value of Re.

Fig. 7
figure 7

Coefficient of drag at (a) Re = 10, (b) Re = 1000, and (c) Re = 100,000

Full size image
Fig. 8
figure 8

Coefficient of drag at different values of Re

Full size image

4.2.3 Coefficient of lift

Figure 9 shows the coefficient of lift at different values of Re. It can be seen that there is a sharp increase in the value of Cl at the initial time step at Re = 10 (Fig. 9a). Afterward it drops and then rises again. After following this pattern, it gradually drops and becomes steady. In the case of Re = 1000, the value of Cl at the initial time step remained uneven then it started following a cyclic pattern (Fig. 9b). It was observed that the computation results approach a state of statistical stationary when Re = 1000. At a higher value of Re (i.e. Re = 10,000), it starts following the cyclic pattern after an initial drop. However, the cyclic pattern was observed uneven in this case.

Fig. 9
figure 9

Coefficient of lift at (a) Re = 10, (b) Re = 1000, and (c) Re = 100,000

Full size image

4.2.4 Contour

The pressure contours were collected after the completion of iterations using the post-processor tool. Figure 10 represents the pressure contours at Re = 10, 1000, and 100,000. The pressure contour plots for the pressure components over the Cartesian axes which typically depict the wakes beside the cylinder. The vortex velocity contour for cylindrical tubes at different values of Re is shown in Fig. 11. The phenomenon of alternative vortex shedding is vividly shown in the vorticity contours around the cylinder and wake region was formed as shown in Fig. 11. Nevertheless, while Re increases, the far wake still shows waviness outlines [33].

Fig. 10
figure 10

Pressure contours at (a) Re = 10, (b) Re = 1000, and (c) Re = 100,000

Full size image
Fig. 11
figure 11

Vortex velocity contours at (a) Re = 10, (b) Re = 1000, and (c) Re = 10,000

Full size image

5 Conclusions

In study was done to analyse the 2D flow across a circular cylindrical tube under various laminar as well as turbulent flow regimes. In this study, the implicit finite volume scheme was employed to compute incompressible flow with time precision using convective flux discretization schemes of the second order. From the numerical results, it can be concluded that the phenomenon of the von Karman vortex street was found significant except in the case Re = 10. As the Re increases, it was noticed that the effect of vortex shedding becomes more dominating. The pressure at the stagnation point rises as the Reynolds number rises, and more low pressure is generated toward the monitoring point (back side). While the velocity of fluid increases, the Cd decreases while the coefficient of lift increases.

The identification of transient phenomena in steady-state simulations can help the engineers or designers to understand the fluid flow dynamics in terms of vortex flow analysis, study of turbulences, calculation of Re, and lift/drag coefficients. This can further facilitate in improvement of system design, operation, and control for various turbomachinery components in cylindrical shape. Also, this can improve the efficiency, dependability, and optimization of interactive systems in design and manufacturing through enhanced understanding of flow dynamics, optimized component design, improved control strategies, and reduction of cavitation and vortex.