Formation Flight Computational Fluid Dynamics

     This is a post about computational fluid dynamics analysis of formation flight.

     The results from an analysis of three unmanned combat aerial vehicles (UCAVs) flying in a V-type formation are presented. The chosen UCAV configuration, shown in Figs. 1-2 and available for download here, is named SACCON (Stability And Control Configuration) UCAV. This configuration is used because of the availability of the geometric and aerodynamic data, used in the validation and verification of the numerical analysis. The SACCON UCAV is designed by NATO's (North Atlantic Treaty Organization) RTO (Research and Technology Group) under Applied Vehicle Task Group (AVT-161) to assess the performance of military aircrafts.

Fig. 1, SACCON UCAV

Fig. 2, Technical drawing for the SACCON UCAV

     The simulation is performed using commercially available computational fluid dynamics code.  The details about the solver and the discretization schemes are presented next. The simulation is performed using SIMPLE-R solver for pressure-velocity coupling. The diffusive terms of the Navier-Stokes equations are discretized using central differentiating scheme while the convective terms are discretized using the upwind scheme of second order. The κ-ε turbulence model with damping functions is implemented to model turbulence. The simulation predicts three-dimensional steady–state flow over UCAVs.

     The Reynolds and Mach number of flow are set at 1e6 and 0.15, respectively. The two trailing UCAVs are placed 3 wingspans behind the leading UCAV. The trailing UCAVs are a wingspan apart. The V-type configuration is chosen because it is the most common observation in birds (author's observation). The V-type formation is shown in Fig. 3. All three UCAVs are at 5° angle-of-attack.

Fig. 3, The V-type formation (top view)

     The boundaries of the computational domain are located at a distance equivalent to 10 times the distance between the nose of the leading UCAV and the tail of the trailing UCAV. The mesh is made of 821,315 cells. Mesh controls are used to refine the mesh in the areas of interest i.e. on the surfaces of the UCAVs and in the wake of all three UCAVs. A cartesian mesh with immersed boundary method is used for the present study. The computational domain with mesh is shown in Fig. 4 while a closeup of the mesh is shown in Fig. 5.

Fig. 4, The computational domain and mesh

Fig. 5, Closeup of mesh, notice the refined wakes of the UCAVs

     For validation and verification, the lift and drag forces from the present study are compared with studies [1-2]. The results are in close agreement with [1,2] As a result of flying in a formation, an improvement in the lift-to-drag ratio of 10.05% is noted. The lift-to-drag ratio of the trailing UCAVs is at 11.825 in comparison with a lift-to-drag ratio of a single UCAV, i.e. 10.745. The lift coefficient is increased by 7.43% while the drag coefficient decreased by 2.174%. The reason(s) to why the efficiency increases will be looked upon later, if ever the author has the time and will power ☺.

     The results from post processing of the simulations are presented in Figs. 6-7. The pressure iso-surfaces colored by velocity magnitude are shown in Fig. 6. While the velocity iso-surfaces colored by pressure magnitude are shown in Fig. 7.

Fig. 6, Flight direction towards the reader

Fig. 7, Flight direction away from the reader

     Thank you very much for reading. If you would like to collaborate on research projects, please reach out.

[1] https://doi.org/10.2514/1.C031386

[2] https://doi.org/10.1155/2017/4217217

Hypersonic Flow over a Two Dimensional Heated Cylinder

     This post is about the simulation of hypersonic flow over a heated circular cylinder, in two dimensions.

     Equation 1 is used as a relationship between Mach and the Reynold number.

M= Re*μ*√(R*T) ÷ d*P*√γ     (1)

     w.r.t. equation 1, the parameters represent the following quantities.

     M     Freestream Mach number at 17.6
     Re    Reynolds number at 376,000
     μ     Dynamic viscosity at 1.329045e^-5 Ns.m^-2
     R     Specific gas constant at 286.9 J.(kg.K)^-1
     T     Freestream temperature 200 K
     d     Cylinder diameter at 5.6730225e^-4 m
     P     Freestream pressure at 101325 Pa
     γ     Specific heat ratio at 1.4
     Tw  Wall temperature of cylinder at 500 K
     Pr    Prandtl number at 0.736

     The boundary conditions were taken from [1]. A comparison with [1] is shown in Fig. 1. Inside Fig. 1, the red dotted line with circles represents the data from [1]. The black solid line represents the data from the present simulation. Within Fig. 1, 0° represents the stagnation point. The velocity, pressure, Mach number and temperature contours are shown in Fig. 2.

Fig. 1 A comparison with previous research [1].

Fig. 2, Top Row, L-R: Velocity and pressure contours. Bottom Row, L-R: Mach number and temperature contours.

The computational mesh and the computational domain with boundary conditions visible are shown in Fig. 3-4, respectively. The computational domain had a size of 20D x 20D. The mesh had 836,580 total cells and 944 cells were located at the solid fluid boundary. Several local mesh controls were employed to capture the shockwave properly.

Fig. 3, The computational mesh.

Fig. 4, The computational domain.

     The solution method is Finite Volume method. SIMPLE-R is the solver employed. Implicit central difference scheme for diffusion terms, second-order Upwind scheme for convective terms and first-order implicit for temporal terms are used. The mesh created uses the Cartesian mesh with Immersed Boundary method.

     Reference:

     [1] https://arc.aiaa.org/doi/10.2514/6.2004-2371 

     Thank you for reading. If you would like to collaborate on research projects, please reach out. I am looking for a PhD position, any guidance would be appreciated.

Automotive Computational Fluid Dynamics (CFD) Analysis

     This post is about the numerical analysis of an Ahmed body. It was a new experience because of the area between the car's floor and the road which is different from most of the numerical analysis performed in open channel aeronautics and turbo-machinery.

     The numerical analysis was performed using the commercial software, SolidWorks Flow Simulation. The software employs κ − ε turbulence model with damping functions, SIMPLE-R (modified), as the numerical algorithm and second-order upwind and central approximations as the spatial discretization schemes for the convective fluxes and diffusive terms. The time derivatives are approximated with an implicit first-order Euler scheme. Flow simulation solves the Navier–Stokes equations, which are formulations of mass, momentum, and energy conservation laws for fluid flows. To predict turbulent flows, the Favre-averaged Navier–Stokes equations are used.

     The software generates Cartesian mesh using immersed boundary method. The mesh had a cell size of 0.035 m in the far field regions within the computational domain. A fine mesh was need between the road the the car's floor to make sure the interaction of the car's floor with the road was captured accurately. Therefore the mesh between the car's floor and the road was refined to have a cell size of 0.00875 m. Another mesh control was applied around the body to refine the mesh with a cells size of 0.0175 m to capture the trailing vortices. The resulting mesh had 209,580 total cells, among those cells, 31,783 cells were at the solid fluid boundary. The computational domain size was ~1L x 1.12L x 3L where L being the vehicle's length. The computational domain along with the computational mesh is shown in Fig. 1.

Fig. 1 Mesh, computational domain and the boundary conditions.

     The red arrows within the Fig. 1 represents the inlet boundary condition of ambient (free-stream) velocity and the blue arrows represent the outlet boundary condition of the ambient pressure. The green arrows represents the co-ordinates axes direction.

     The results from the numerical analysis were compared with [1-3]. The results are within 10% of the experimental results. The velocity (superimposed by the velocity streamlines) and pressure profiles around the car body at various free-stream velocities is shown in Fig. 2.

Fig. 3 Velocity and pressure plots. From the top, Row 1, L-R; ambient velocity of 30 and 40 m/s. Row 2, L-R; ambient velocity of 60 and 80 m/s. Row 3, ambient velocity of 105 m/s.

     It was a good experience learning about automotive CFD after spending a long time in aeronautic/turbo-machinery CFD. Thank you for reading. Please share my work. If you would like to collaborate on a project please reach out.

[1] F.J.Bello-Millán, T.Mäkelä, L.Parras, C.delPino, C.Ferrera, "Experimental study on Ahmed's body drag coefficient for different yaw angles", Journal of Wind Engineering and Industrial Aerodynamics, Volume 157, October 2016, Pages 140-144.

[2] Guilmineau E., Deng G.B., Queutey P., Visonneau M. (2018) Assessment of Hybrid LES Formulations for Flow Simulation Around the Ahmed Body. In: Deville M. et al. (eds) Turbulence and Interactions. TI 2015. Notes on Numerical Fluid Mechanics and Multidisciplinary Design, vol 135. Springer, Cham.

[3] A. Thacker, S.Aubrun, A.Leroy, P.Devinant, "Effects of suppressing the 3D separation on the rear slant on the flow structures around an Ahmed body", Journal of Wind Engineering and Industrial Aerodynamics, Volumes 107–108, August–September 2012, Pages 237-243.

Vertical Axis Wind Turbine Computational Fluid Dynamics Analysis

     This post is be about the validation and verification of the computational fluid dynamics analysis of a three blade vertical axis wind turbine. The turbine had a diameter of 2 m with each blade being 1 m tall. The blades had an NACA-0018 airfoil cross section.

     The computational fluid dynamics analysis employed the κ-ε turbulence model with damping functions as the turbulence model, SIMPLE-R as the numerical algorithm. The spatial discretization schemes for the convective fluxes and diffusive terms used are the second order upwind and central approximations, respectively. An implicit first-order Euler scheme is employed to approximate the time derivatives.

     The Cartesian computational mesh with immersed boundary method had a total of 769,357 cells. Among those 769,357 cells, 166,188 cells were around the turbine blades. Mesh controls were employed to refine the mesh near the turbine blades. A time step of 3e^-3 was employed. The computational domain inlet was 1.5 D away from the turbine and the outlet was 3D away. The computational domain walls on the sides were 1D x 1.5D, where D represents the turbine diameter. The mesh and the computational domain are shown in Fig. 1. The vertical teal arrow represents the force of gravity, the curved teal arrow represents the direction of turbine rotation. The dark blue arrow represents the direction of free stream velocity.

Fig. 1, Mesh and computational domain.

     The simulations ran at a tip-speed ratio of 1.87 at a wind speed of 4.03 m.s^-1. The velocity distribution around the turbine after 4 revolutions is shown in Fig. 2. Validation of the numerical analysis was carried out using [1]. The results of power produced by the turbine were with in 4% of the experimental results [1]. An animation of the numerical analysis is also shown.

Fig. 1, Flow field around the turbine.

     Thank you for reading. If you would like to contribute to the research, both financially and scientifically, please feel free to reach out.





[1] Yi-Xin Peng, You-Lin Xu, Sheng Zhan and Kei-Man Shum, High-solidity straight-bladed vertical axis wind turbine: Aerodynamic force measurements, Journal of Wind Engineering and Industrial Aerodynamics, January 2019.