NUMERICAL INVESTIGATION OF FLOW AROUND SPIT FIRE Mk VIII AIRCRAFT
Casestudy No: FTLCFD001
Keywords: CFD, Aerodynamics, Spitfire, MRF
Introduction
Accurate and cost-effective Computational Fluid Dynamics (CFD) methods, coupled with easy access to computational resources and numerical modeling tools, play a vital role in optimizing fighter aircraft. This benchmark study focuses on assessing flow patterns and pressure distributions around the legendary SPITFIRE Mk VIII in low subsonic, incompressible flow conditions.
The SPITFIRE, designed by Reginald Mitchell and produced by Supermarine Aviation Works, is an iconic British fighter aircraft renowned for its pivotal role in World War II. Its sleek, streamlined design, featuring elliptical wings, contributed to its exceptional maneuverability and high-speed performance.
Figure1: SPIT FIRE Mk VIII Fighter Aircraft [1]
Computational Domain
For benchmarking, a computational domain of 55m × 55m × 180m was used. The domain dimensions were chosen to ensure adequate flow development, extending 10L upstream, 10L downstream, 5L to the sides, and 10L above the ground surface.
The geometry used in this study is the Spitfire Mk VIII, with the CAD model freely available on Grab CAD [2]. The key parameters of the Spitfire Mk VIII are:
Aircraft Length: 9.54 m
Wing Surface Area: 22.5 m²
Figure 1. The modelled computational domain with spit fire
The whole computational domain is divided into two components (volumes) – a region formed by the plane body and the bounding box, and the cylinder around the propeller. The rotating zone is highlighted in blue color.
Mesh
An unstructured poly hexacore mesh was generated in Fluent Mesher. The generated mesh consisted of approximately 23 Million cells with first layer thickness of 1mm and 10 layers of boundary layer mesh. The figure shows the meshed domain.
Figure 2 : The computational mesh of the Spitfire body and the front view of the propeller blade includes mesh refinement, highlighting the boundary layers.
Numerical Model
The 3D steady-state, incompressible, single-phase analysis was performed using ANSYS Fluent. The rotating propeller was initially simulated using the Multiple Reference Frame (MRF) method as a frozen rotor, followed by the sliding mesh approach for improved accuracy.
For the numerical setup, second-order discretization schemes were applied to the continuity and momentum equations. A convergence criterion of 1 × 10⁻⁶ was set for continuity, momentum, and turbulence equations. The k-ω SST model with a wall function approach was used to obtain the initial steady-state solution. Subsequently, a high-fidelity Detached Eddy Simulation (DES) was conducted, using the steady-state results for initialization.
| Property | Value |
|---|---|
Density,  (kg/m3) | 1.22 |
| Dynamic viscosity, (kg/ms) | 1.8 x 10-5 |
Table 1: Fluid Properties
| Surface | Boundary Condition |
|---|---|
| Inlet | Velocity Inlet: 90 [m/s] |
| Angle of Attack | 8 degrees |
| Outlet | Gauge pressure outlet: 0 [Pa] |
| Spitfire Body | No Slip Wall |
| Ground Wall | Symmetry |
| Side Wall | Symmetry |
Table 2: Boundary conditions details
Results
The results in Table 3 include the visualization drag and Lift coefficients. The axial force was kept as a monitor for convergence in the steady state simulations. Velocity streamlines distribution is shown in the spanwise direction vortex pattern and flow recirculation zones are clearly shown Figure 4.
| Force Coefficients | CFD Simulation |
|---|---|
| Drag coefficient (Cd ) | 0.044 |
| Lift coefficient (Cl) | 0.432 |
Table 3 : Force coefficients from numerical simulation
Figure 4: Velocity streamline distribution in flow direction
Figure 5: Q-criterion showing the turbulent structures of the tip flow: DES
Figure 6: Rendered view of Q-criterion showing the turbulent structures of the tip flow: DES
Figure 5 illustrates the turbulent structures from propeller and wing tip flow using iso-surfaces of the Q-criterion, coloured by flow velocity for DES simulations. These surfaces highlight vortices within the flow. Large-scale structures emanating from the blade tips and further move downstream of the flow.
Conclusion
- CFD simulation of flow over the Spitfire Mk VIII was performed . The Multiple Reference Frame (MRF) method was initially used for steady-state analysis, followed by Sliding Mesh and Detached Eddy Simulation (DES) for transient flow analysis.
- The Lift and Drag Coefficients were computed .
- Velocity field streamlines were analyzed, revealing wingtip vortices in both the spanwise direction and perpendicular to the flow.
- The DES approach provided insights into unsteady flow characteristics, enhancing the accuracy of the aerodynamic analysis.
References
- “A CFD evaluation of three prominent World War II fighter aircraft”, D Lednicer – The Aeronautical Journal, 1995.
- Geometry data – https://grabcad.com/library/supermarine-spitfire-mk-viii.
Contact us
If you are interested in consultancy services, please write to us with your requirements. We will get back to you and arrange for an online Teams/Zoom meeting to discuss further. Either fill out the form below or email us at consult@flowthermolab.com. Please note that we are offering consultancy services only for industries (B2B) and not for individuals or students.