Computation of flow past aerospace vehicles

S. K. Chakrabartty*, K. Dhanalakshmi and J. S. Mathur

Computational and Theoretical Fluid Dynamics Division, National Aerospace Laboratories, Bangalore 560 017, India

This paper describes the simulation of compressible flow past complex aerospace geometries, using Computational Fluid Dynamics (CFD). The computations have been done using a cell vertex-based finite volume scheme and structured multi-block grids. Results are described for the viscous flow past a cropped delta wing, where the flow simulation is able to explain some of the complex fluid flow pheno-
mena. Results are also shown for inviscid flow past multi-body launch vehicle configurations and an aircraft configuration. These simulations of the flow past realistic aerospace configurations show that CFD can now play an important role in the design and development of such vehicles.

IN the design and development of aerospace vehicles, it is essential to have an accurate estimate of aerodynamic data. The aerodynamic loads at different flight conditions are needed for the structural design of the vehicle, while the total aerodynamic forces and moments determine the overall performance. Earlier, this data could be obtained only by experimental methods, but now it is possible to simulate the flow past realistic aerospace configurations using Computational Fluid Dynamics (CFD). Besides, CFD can also be used for fundamental studies which lead to a better understanding of complex fluid flow phenomena. Recent developments in high speed digital computers, numerical algorithms and computer graphics enable such simulations to be performed in a reasonable amount of time. Thus, CFD can now play a major role in the design process and also help in improving our knowledge of fluid mechanics and the understanding of science. In two-dimensions, for example, capturing the shock-induced separation and re-attachment on an airfoil surface at transonic speeds, and the appearance of double shock waves on transonic super-critical airfoils at off-design conditions, are among the difficult cases used to test the accuracy of the numerical methodology. Another important fluid mechanical phenomenon is the three-dimensional boundary layer separation on the surface of the body and the corresponding re-attachment. A highly accurate solution of the Reynolds Averaged Navier–Stokes (RANS) equations, with a proper turbulence model, is necessary to simulate this flow. Earlier, the studies of such phenomena were limited to experimental flow visualization, but

*For correspondence. (e-mail:

it is now also possible to use CFD for such studies. Three-dimensional separated flows are further complicated by transitional turbulent boundary layers and shock waves, along with their mutual interactions. The accurate prediction of transition is generally not possible, and the transition point usually must be specified based on experimental data. It is more common for CFD computations to simulate either fully laminar or fully turbulent flows.

Using their experience in the computation of transonic flows, the authors have developed a three-dimensional Euler code, JUEL3D1, and the corresponding RANS code, JUMBO3D2. These codes use a vertex-based finite volume space discretization with five-stage Runge–Kutta time integration. These codes have been tested and validated systematically starting from two-dimensional flow past airfoils to simple three-dimensional flows like subsonic and transonic flow past wings. Complexities with respect to three-dimensional geometry and also with respect to flow structure were gradually introduced and carefully studied. These studies included the study of grid consistency and the effect of other parameters involved in the flow algorithm. The present paper summarizes some of the results obtained by these codes for three different three-dimensional geometries of practical interest.


The unsteady RANS equations, along with an appropriate turbulence model, constitute an accepted set of equations governing the motion of a viscous compressible fluid. These equations can be written in integral form as




where V is a control volume with surface S and normal represents the vector of conserved variables, FE represents the Euler fluxes and FV represents the viscous fluxes. The addition of the perfect gas law makes this a closed set of equations.

For many practical applications, the viscous effects are confined to very small regions of the flow domain, and an inviscid simulation of the flow can provide the required aerodynamic data with considerably lower computing costs. The Euler equations for an inviscid compressible fluid are derived by neglecting the viscous fluxes in the Navier–Stokes (N–S) equations.

The finite volume method is suitable for the solution of either the Euler or the N–S equations for the flow past any complex geometry. In this method, a certain region around the geometry is identified as the computational domain, which is then divided into a number of small volumes or grid cells. This is called the computational grid and various grid generation techniques exist to accomplish this discretization of the domain. For a complex shape, the generation of the grid is itself a
major task which often requires more time and effort than the flow analysis. The more commonly used grids are the structured grids. Any structured grid generation technique essentially maps the given physical domain to a cube in computational space. This is not always possible, or desirable, for a closed complex body in a simply connected physical domain. To overcome this problem, the multi-block approach is used in which the entire domain is divided into a number of blocks. The topology of the overall grid is determined by the arrangement of the blocks and a simple grid is generated in each block. The use of structured multi-block grids makes it possible to generate good quality grids for extremely complex geometries. The finite volume method can be either of the cell centred type or the cell vertex type, depending on whether the flow variables are stored at the centres or the vertices of the grid cells. Both the JUEL3D and JUMBO3D codes use the cell vertex finite volume scheme.

Two-dimensional cell vertex schemes for the Euler equations, proposed by Ni3 and Hall4, were extended to solve the N–S equations by Chakrabartty5,6. The main advantages of cell vertex schemes over cell-centred

1296a.gif (15202 bytes)

1296b.jpg (42823 bytes)

schemes are: (1) the accuracy in the computation of derivatives, particularly for stretched and skewed grids, and (2) direct computation of the pressure on the wall. A novel vertex-based scheme, proposed by Chakrabartty7, gives second-order accurate first derivatives and at least first-order accurate second derivatives even for stretched and skewed grids. This scheme takes almost the same numerical effort to solve the full RANS equations as for the thin layer Navier–Stokes (TLNS) equations. The scheme has been used to study the effect of different turbulence models on the shock-induced separation in transonic flow8. It has also been used to study the off-design behaviour of the Korn airfoil9 in viscous transonic flow, where a highly accurate scheme is required to predict the presence of double shock waves on the surface of the airfoil. The method is thus well established for two-dimensional flows and has been successfully extended to three dimensions.

1297a.gif (27235 bytes) 

Flow past a cropped delta wing

The N–S code, JUMBO3D, has been used to study the vortex flow over a 65 cropped delta wing with round leading edge10, at a free-stream Mach number of 0.85 and Reynolds number of 2.38   106. Figure 1 shows a schematic of the flow features for a delta wing at high angle of attack. Leeward vortices, formed by the rolling up of the shear layer in a spiral fashion, occur in counter-rotating pairs about opposite leading edges. The primary separation originates close to the apex and inboard of the leeward side of the wing, and gradually moves closer to the leading edge further downstream. Due to the low pressure induced by these vortices on the wing surface, the flow experiences an adverse pressure gradient in the cross-flow direction towards the leading edge. This causes the secondary separation depending on the condition of the boundary layer, and also formation of a cross-flow shock depending on the free-stream conditions. Due to the property of turbulent flow to delay boundary-layer separation, the secondary vortex in a laminar flow lies inboard of its position in a turbulent flow. Interaction with the cross-flow shock causes the boundary layer separation to reduce to a small separated bubble sitting at the foot of the shock, which re-attaches inboard of the leading edge. Depending on the position of re-attachment, a tertiary vortex may appear in the same orientation as the primary vortex. Further downstream of the flow, when the secondary vortex meets the terminating shock, it reduces further and gradually gets
dissipated. A highly accurate solution of the RANS equations, with a proper turbulence model, is necessary to simulate this flow.

1297b.jpg (15865 bytes) 

1298.gif (39645 bytes) 


The algebraic turbulence model of Baldwin and Lomax11, modified by Degani and Schiff12 for vertical flows, has been used in the computations with a grid containing about 647,000 grid points. Only the half wing has been considered, assuming a symmetry plane along the root chord, and computed results obtained at 10 , 20 and 30 angles of attack have been studied in detail to explain and understand the physical phenomena discussed earlier. Figure 2 shows the static pressure contours on the surface of the wing, on the symmetry plane and on a cross-flow plane just downstream of the trailing edge, while Figure 3 shows the particle traces superimposed on pressure distribution at different planes for the flow at 30 angle of attack. This is the flow condition where vortex breakdown occurs. In Figure 2 it can be seen that double shock waves appear and extend up to 20% of the semi-span. The leading edge separation vortex breaks down due to the interaction of strong terminating and cross-flow shock waves. Secondary and tertiary vortices appear and diffuse downstream. As shown in Figure 3, vortex breakdown initiates at around 50% of the root chord and a bubble-type vortex core forms and extends beyond the trailing edge. No experimental data is available for this flow condition. How-

1299.gif (30569 bytes)

ever, experimental data is available for the flow at 10 angle of attack13, and Figure 4 compares the computed coefficient of pressure with experimental values for this case.

The conclusions made from the complete analysis of the three cases computed earlier10 are reproduced below for completeness.

  1. The primary separation starts inboard and close
    to the apex. Along the flow direction, the starting point moves gradually towards the leading edge.
  2. The starting point of the secondary separation moves upstream as the angle of attack increases.
  3. At the end of the secondary separation, there exists always a node–saddle pair on the surface skin-friction lines and another singular point appears in the field.
  4. The leading edge rolled up vortex above the wing surface remains stable as long as the vortex feeding continues from the leading edge.
  5. This vortex feeding to the primary vortex core may cease either due to the geometric discontinuity at the leading edge or due to the interaction of terminating and cross-flow shocks with the vortex system.
  6. As the feeding vortex ceases, the flow near the surface tends to turn towards the leading edge and tries to exit from the wing surface through the tip, the primary vortex core remains above the surface and becomes unstable, leading to vortex breakdown.
  7. Between the primary attachment and secondary separation lines, a cross-flow shock starts from the surface, separates the two vortex regions, and causes small binary core-like structures in the primary vortex.
  8. The existence of a cross-flow shock attracts the primary vortex and obstructs the growth of the secondary vortex.
  9. The secondary vortex diffuses due to the interaction of cross-flow and terminating shocks, and ceases to exist further downstream.


Flow past a launch vehicle

We now consider the computation of flows past launch vehicle configurations14. A typical launch vehicle consists of a number of strap-on boosters attached to a core vehicle. The configuration thus consists of multiple bodies separated by extremely small gaps, and it is quite difficult to accurately model this geometry and simulate the flow past it. N–S computations are able to simulate the detailed features of complex flow fields, but are expensive in terms of computer resources. If such details are not required and only the overall aerodynamic forces and loads are needed, Euler computations can provide the required data at a substantially lower cost.

The first difficulty is, of course, in the generation of a computational grid. For these computations, a relatively simple grid stacking methodology has been used. This consists of generating two-dimensional grids at a number of cross-sections and then stacking these to form the three-dimensional grid. This technique results in extremely fast grid generation, but cannot be used with most geometries of interest, where a more complex grid topology is needed for an accurate simulation of the flow.

The JUEL3D code has been used to compute the flow past two launch vehicles, one with two strap-on boosters and the other with four strap-on boosters. In both cases, flow over half the vehicle has been computed using a

1300a.gif (12150 bytes)

1300b.jpg (44196 bytes)

243,000 grid points. For the four strap-on launch vehicle, two different kinds of grids were tried, a single block grid containing about 580,000 grid points, and a two-block grid containing about 151,000 grid points in the inner block and about 424,000 grid points in the outer block.

Computations have been done for various free-stream conditions. For the two strap-on launch vehicle, the free-stream Mach number was 2.09, at an incidence of 0 and 4 . For the four strap-on launch vehicle, the three free-stream Mach numbers were 0.8, 1.75 and 3.0, each at an incidence of 0 and 5 . Figure 5 shows the computed surface pressure distribution for the flow with a free-stream Mach number of 1.75 at zero incidence, and the major flow features like compression and expansion waves can be clearly seen. Experimental data15 are available for this flow condition, and are compared with the computed values in Figures 6 and 7, where grid 1 refers to the single-block grid and grid 2 refers to the two-block grid. Figure 6 shows the computed coefficient of pressure along the length of the core vehicle at four different angular positions. Figure 7 shows the coefficient of pressure at three different angular positions on booster S4. These angular positions are identified on the sketch of the cross-section of the launch vehicle.

Overall, these computations have shown that for supersonic flows the computed surface pressure distributions agree quite well with experimental data. For subsonic flows, it has been seen that the agreement is not good, and the simulation of viscous flow appears to be essential for such flows.

Flow past an aircraft

The SARAS is a 9–14 seater light transport aircraft being designed and developed by the National Aerospace Laboratories (NAL), Bangalore. For the generation of aerodynamic data for this aircraft, the Euler code, JUEL3D, has been used to compute the inviscid flow past the SARAS wing-fuselage16. A simple grid generation procedure, like the one used for the launch vehicles, is not suitable for such a complex geometry. A thirty-block grid has been generated for this configuration using the multi-block grid generation code, JUMGRID17, which can be used for any arbitrary, geometrically complex body. This grid contains a total of 896,700 grid points. Figure 8 shows a view of the grid on the surface of the aircraft, and Figure 9 shows the computed surface Mach number distribution for a typical flow situation with a free-stream Mach number of 0.5, at zero incidence. The accuracy of these computations can be seen in Figure 10 where the computed values of the coefficient of lift for the different angles of incidence are compared with experimental data18.

As the complexity of the aircraft geometry is increased, the effort required in the grid generation and flow simulation also increases substantially. The complete SARAS aircraft configuration contains, in addition to the wing and fuselage, a tail and an engine nacelle connected to the fuselage by a stub wing. As a first step in modelling the complete geometry, the stub wing has been added to the basic wing fuselage. This has caused an increase in the number of blocks from thirty to sixty-four. This sixty-four-block grid, containing about 1,005,000 grid points, has been generated using a grid generation package, GRIDGEN, recently acquired by NAL, from M/s Pointwise Inc., USA. Figure 11 shows a view of this grid on the surface of the aircraft. A comparison with Figure 8 shows that the large increase in the number of blocks is due to the higher position of the stub wing on the fuselage as compared to the position of the main wing. Figure 12 shows the computed surface Mach number distribution for a free-stream Mach number of 0.5 at zero incidence. All these computations are for half the configuration, using a symmetry condition on the plane of symmetry.

These results show that the Euler code can be used to obtain a reasonably accurate estimate of the aerodynamic loads acting on SARAS at different flight conditions.


The results presented in this paper have shown that CFD is now able to simulate the flow past realistic configurations and can thus play a major role in the design and development of aerospace vehicles. In the near future, CFD will be able to simulate more complex geometries and thus become an even more valuable design tool. It is now also possible to use CFD for extremely accurate computations in order to study complex fluid pheno-
mena in detail.


  1. Chakrabartty, S. K., Dhanalakshmi, K. and Mathur, J. S., Acta Mech., 1996, 115, 161–177.
  2. Chakrabartty, S. K., Dhanalakshmi, K. and Mathur, J. S., Acta Mech., 1996, 119, 181–197.
  3. Ni, R. H., AIAA J., 1982, 20, 1565–1571.
  4. Hall, M. G., in Numerical Methods for Fluid Dynamics (eds Morton, K. W. and Baines, M. J.), Oxford, 1986, vol II, pp. 303–345.
  5. Chakrabartty, S. K., AIAA J., 1989, 27, 843–844.
  6. Chakrabartty, S. K., AIAA J., 1990, 28, 1829–1831.
  7. Chakrabartty, S. K., Acta Mech., 1990, 84, 139–153.
  8. Chakrabartty, S. K. and Dhanalakshmi, K., AIAA J., 1995, 33, 1979–1981.
  9. Chakrabartty, S. K. and Dhanalakshmi, K., Acta Mech., 1996, 118, 235–239.
  10. Chakrabartty, S. K., Dhanalakshmi, K. and Mathur, J. S., Acta Mech., 1998, 131, 69–87.
  11. Baldwin, B. S. and Lomax, H., AIAA Paper 78–257, AIAA
    16th Aerospace Sciences Meeting, Huntsville, Alabama, 16–18 January 1978.
  12. Degani, D. and Schiff, L. B., J. Comp. Phys., 1986, 66, 173–196.
  13. Hartmann, K., Proc. Int. Vortex Flow Experiments on Euler Code Validation, FFA TN, Aeronautical Research Institute of Sweden, Stockholm, 1986, pp. 63–88.
  14. Chakrabartty, S. K., Dhanalakshmi, K. and Mathur, J. S., Proceedings of the 3rd Asian CFD Conference, Bangalore, 7–11 December 1998, vol. 2, pp. 1–6.
  15. Vikram Sarabhai Space Centre, Thiruvananthapuram, private commun.
  16. Chakrabartty, S. K., Dhanalakshmi, K. and Mathur, J. S., Proceedings of the 3rd Asian CFD Conference, Bangalore, 7–11 December 1998, vol 2, pp. 126–131.
  17. Chakrabartty, S. K., Dhanalakshmi, K. and Mathur, J. S., Proceedings of the 3rd Asian CFD Conference, Bangalore, 7–11 December 1998, vol. 2, pp. 62–67.
  18. Centre for Civil Aircraft Design & Development, National Aerospace Laboratories, Bangalore, private commun.


ACKNOWLEDGEMENTS.  We acknowledge the Vikram Sarabhai Space Centre, Thiruvananthapuram, for sponsoring work on the launch vehicles, and the encouragement and support provided by the Centre for Civil Aircraft Design & Development, NAL, Bangalore for work on the SARAS aircraft.