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.

Flying Wing Design using Computational Fluid Dynamics (Verification and Validation)

     This post is about a transient simulation of the ONERA M-6 flying-wing aircraft with a cross-section of ONERA D airfoil, as shown in Fig. 1.

Fig. 1, The simulated geometry. 

     The mesh had 2,474,614 cells in total with 300,892 cells on the wing surface, as shown in Fig. 2. The computational domain is shown in Fig. 4. The computational domain walls are at a distance equal to ten times the wingspan.

Fig. 2, The computational mesh.

Fig. 3, The computational domain.

     The simulated conditions are taken from [1-4] i.e. a freestream Mach number of 0.8395 at 101,325 Pa and 293.2 K. The angle of attack is 3.06°.

     The lift force from the present numerical simulation is at 19,551.65 N as compared to the lift force of 20,438.53 N as determined by [1-4]. The numerically determined drag force from present simulation is 1,370.88 N as compared to 1,313.24 N, as determined by [1-4].

     The results of lift and drag force from the present simulation are within 4.35% and 4.2% of the results calculated by NASA [4] and [1-3]. Streamlines and pressure surface plot around the aircraft surface are shown in Fig. 4.

Fig. 4, Results.

References

[1] Le Moigne, "A Discrete Navier-Stokes Adjoint Method for Aerodynamic Optimization of Blended Wing-Body, Configurations", PhD thesis, Cranfield University, United Kingdom, 2002.

[2] J. Lee, C. S. Kim, C. Kim, O. H. Rho, and K. D. Lee, "Parallelized Design Optimization for Transonic Wings using Aerodynamic Sensitivity Analysis", AIAA Paper 2002-0264, 2002.

[3] E. J. Neilsen and W. K. Anderson, "Recent Improvements in Aerodynamic Design Optimization on Unstructured Meshes", AIAA Paper 2001-0596, 2001.

[4] 3D ONERA M6 Wing Validation, https://turbmodels.larc.nasa.gov/onerawingnumerics_val_sa.html.

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

Computational Fluid Dynamics Analysis of a Drone

     This post is about the computational fluid dynamics analysis of a small drone. The drone features a blended body-wing design with various cross sections at different span-wise locations. The drone has a wing-span and length of 6 ft. and 4.92 ft., respectively. The root (center) portion of the drone is relatively thicker and symmetrical in cross section for increased mechanical strength while the the mid-section and wing tips are thinner and utilize more cambered aero-foils. This is purely a concept design and as of now, no physical model of this drone exists.

     The numerical simulations for the present study were carried out using SolidWorks Flow Simulation Premium© code. The code employs κ-ε model with Two-Scales Wall Functions approach as the turbulence model. The numerical algorithm implemented is the SIMPLE-R, modified. The second-order upwind discretization scheme is used to approximate the convective fluxes while the diffusive terms are approximated using the central differencing scheme. The time derivatives are approximated with an implicit first order Euler scheme. The SolidWorks Flow Simulation© solves the Navier-Stokes equations, equations 1-3, which are formulations of mass, momentum and energy conservation laws for fluid flows. Turbulent flows are predicted using the Favre-averaged Navier-Stokes equations.

     The mesh independence test was carried out starting with 348,679 fluid cells. The mesh density was then increased up to 2,360,514 cells. The results of mesh independence study are mentioned below.

                          Mesh Name             Cells            Lift [N]         Drag [N]      Lift/Drag

                          M1                          348,679       382.41 -48.14      7.95

                          M2                          1,032,665    466.08      -48.73      9.57

                          M3                          1,559,516    473.48 -47.89      9.89

                          M4                          1,990,010    486.38 -48.08      10.12

                          M5                          2,360,514    491.07 -48.32      10.16

     It can be seen that as the mesh density increased, the difference in the critical parameters between two successive meshes also reduced. The mesh independence test was stopped as the difference between all of the critical parameters was less than one percent for the meshes M4 and M5.

     The pressure and velocity plots at various span-wise locations are shown in Fig. 1-2. It can be clearly seen that there is a negligible change in the velocity and pressure distributions around the drone between meshes M4 and M5. It can also be seen that as the mesh becomes finer, the resolution of both the pressure and velocity plots also increases.

Fig. 1, Velocity contours of various meshes.

Fig. 2, Pressure contours of various meshes.

     Aero-acoustics around the drone were also examined, as shown Fig. 3.

Fig. 3, Sound level contours of various meshes.

     A zoomed in view of the computational mesh is shown in Fig. 4. The refined mesh at the drone walls as a result of the mesh controls employed is clearly visible. The hump near the root of the drone is also visible, it was added in order to prevent the span-wise flow.

Fig. 4, Mesh level M4.

     The boundary conditions and the computational domain are shown in Fig. 5. The large red arrows represents inlet velocity boundary condition and the large blue arrows represents the atmospheric pressure outlet boundary condition. The red squares represents real wall boundary condition (slip) applied to the computational domain walls so that the boundary layer from the walls does not effect the flow around the drone.

An animation of an aileron roll can be seen here.

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

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.