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 vertexbased finite
volume scheme and structured multiblock 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 multibody 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
twodimensions, for example, capturing the shockinduced separation and reattachment on
an airfoil surface at transonic speeds, and the appearance of double shock waves on
transonic supercritical airfoils at offdesign conditions, are among the difficult cases
used to test the accuracy of the numerical methodology. Another important fluid mechanical
phenomenon is the threedimensional boundary layer separation on the surface of the body
and the corresponding reattachment. 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. (email:
drskc@ctfd.cmmacs.ernet.in)
it is now also possible to use CFD for such studies.
Threedimensional 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 threedimensional Euler code, JUEL3D^{1},
and the corresponding RANS code, JUMBO3D^{2}. These codes use a vertexbased
finite volume space discretization with fivestage Runge–Kutta time integration.
These codes have been tested and validated systematically starting from twodimensional
flow past airfoils to simple threedimensional flows like subsonic and transonic flow past
wings. Complexities with respect to threedimensional 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 threedimensional geometries of practical interest.
Methodology
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
(1)
where V is a control volume with surface S
and normal represents the vector of conserved variables, F_{E}
represents the Euler fluxes and F_{V} 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 multiblock 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 multiblock 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.
Twodimensional cell vertex schemes for the Euler
equations, proposed by Ni^{3} and Hall^{4}, were extended to solve the
N–S equations by Chakrabartty^{5,6}. The main advantages of cell vertex
schemes over cellcentred
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 vertexbased scheme, proposed by
Chakrabartty^{7}, gives secondorder accurate first derivatives and at least
firstorder 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 shockinduced separation in transonic flow^{8}.
It has also been used to study the offdesign behaviour of the Korn airfoil^{9} 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 twodimensional flows and has been successfully extended to three dimensions.
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 edge^{10}, at a
freestream Mach number of 0.85 and Reynolds number of 2.38 ´ 10^{6}.
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 counterrotating 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 crossflow
direction towards the leading edge. This causes the secondary separation depending on the
condition of the boundary layer, and also formation of a crossflow shock depending on the
freestream conditions. Due to the property of turbulent flow to delay boundarylayer
separation, the secondary vortex in a laminar flow lies inboard of its position in a
turbulent flow. Interaction with the crossflow shock causes the boundary layer separation
to reduce to a small separated bubble sitting at the foot of the shock, which reattaches
inboard of the leading edge. Depending on the position of reattachment, 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.
The algebraic turbulence model of Baldwin and Lomax^{11},
modified by Degani and Schiff^{12} 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 crossflow 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 semispan. The leading edge separation
vortex breaks down due to the interaction of strong terminating and crossflow 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 bubbletype vortex
core forms and extends beyond the trailing edge. No experimental data is available for
this flow condition. How
ever, experimental data is
available for the flow at 10° angle of attack^{13}, 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 earlier^{10} are reproduced below for completeness.
 The primary separation starts inboard and close
to the apex. Along the flow direction, the starting point moves gradually towards the
leading edge.
 The starting point of the secondary separation moves upstream as the
angle of attack increases.
 At the end of the secondary separation, there exists always a
node–saddle pair on the surface skinfriction lines and another singular point
appears in the field.
 The leading edge rolled up vortex above the wing surface remains
stable as long as the vortex feeding continues from the leading edge.
 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 crossflow shocks with the vortex system.
 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.
 Between the primary attachment and secondary separation lines, a
crossflow shock starts from the surface, separates the two vortex regions, and causes
small binary corelike structures in the primary vortex.
 The existence of a crossflow shock attracts the primary vortex and
obstructs the growth of the secondary vortex.
 The secondary vortex diffuses due to the interaction of crossflow
and terminating shocks, and ceases to exist further downstream.
Flow past a launch vehicle
We now consider the computation of flows past launch
vehicle configurations^{14}. A typical launch vehicle consists of a number of
strapon 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 twodimensional grids at a
number of crosssections and then stacking these to form the threedimensional 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 strapon boosters and the other with four strapon
boosters. In both cases, flow over half the vehicle has been computed using a
243,000 grid points. For
the four strapon launch vehicle, two different kinds of grids were tried, a single block
grid containing about 580,000 grid points, and a twoblock 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 freestream
conditions. For the two strapon launch vehicle, the freestream Mach number was 2.09, at
an incidence of 0° and 4° . For the four strapon launch vehicle, the three freestream
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 freestream Mach number of
1.75 at zero incidence, and the major flow features like compression and expansion waves
can be clearly seen. Experimental data^{15} are available for this flow condition,
and are compared with the computed values in Figures 6 and 7, where grid 1 refers to the
singleblock grid and grid 2 refers to the twoblock 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 crosssection
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
wingfuselage^{16}. A simple grid generation procedure, like the one used for the
launch vehicles, is not suitable for such a complex geometry. A thirtyblock grid has been
generated for this configuration using the multiblock grid generation code, JUMGRID^{17},
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 freestream 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 data^{18}.
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 sixtyfour. This sixtyfourblock 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
freestream 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.
Conclusions
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.
 Chakrabartty, S. K., Dhanalakshmi, K. and Mathur, J. S., Acta Mech.,
1996, 115, 161–177.
 Chakrabartty, S. K., Dhanalakshmi, K. and Mathur, J. S., Acta Mech.,
1996, 119, 181–197.
 Ni, R. H., AIAA J., 1982, 20, 1565–1571.
 Hall, M. G., in Numerical Methods for Fluid Dynamics (eds
Morton, K. W. and Baines, M. J.), Oxford, 1986, vol II, pp. 303–345.
 Chakrabartty, S. K., AIAA J., 1989, 27, 843–844.
 Chakrabartty, S. K., AIAA J., 1990, 28, 1829–1831.
 Chakrabartty, S. K., Acta Mech., 1990, 84,
139–153.
 Chakrabartty, S. K. and Dhanalakshmi, K., AIAA J., 1995, 33,
1979–1981.
 Chakrabartty, S. K. and Dhanalakshmi, K., Acta Mech., 1996, 118,
235–239.
 Chakrabartty, S. K., Dhanalakshmi, K. and Mathur, J. S., Acta Mech.,
1998, 131, 69–87.
 Baldwin, B. S. and Lomax, H., AIAA Paper 78–257, AIAA
16th Aerospace Sciences Meeting, Huntsville, Alabama, 16–18 January 1978.
 Degani, D. and Schiff, L. B., J. Comp. Phys., 1986, 66,
173–196.
 Hartmann, K., Proc. Int. Vortex Flow Experiments on Euler Code
Validation, FFA TN, Aeronautical Research Institute of Sweden, Stockholm, 1986, pp.
63–88.
 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.
 Vikram Sarabhai Space Centre, Thiruvananthapuram, private commun.
 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.
 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.
 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.
