VKI_RVAD_2005_Application_of_a_Lattice_Boltzmann_Code

VKI Lecture Series on Road Vehicle Aerodynamics 2005 „Application of a Lattice-Boltzmann Code in Automobile and Motorcycle Aerodynamics“
- 1 –
APPLICATION OF A LATTICE-BOLTZMANN CODE
IN AUTOMOBILE AND MOTORCYCLE AERODYNAMICS
Lecture Series on “Road Vehicle Aerodynamics”
Von Karman Institute, Brussels, Belgium, May 30 – June 3, 2005
Dr.-Ing. Norbert Grün
BMW Group, Germany
1. Introduction
The request for shortening development cycles in the automotive industry enforces the
employment of simulation methods, especially in the early phase where no hardware is
available yet for physical testing. Analyzing concepts by simulation in the initial phase can
avoid errors whose correction will be cost and time intensive in later stages of the
development process. But also during serial development, simulation tools provide a deeper
understanding of the physics and thus may reduce the number of physical models to be tested
for instance in the wind tunnel in case of aerodynamics (Fig. 1, Ref. [1]).
Serial Development Phase
Styling
Process
Simultaneous Usage of Experimental & Virtual Tools
CFD-Model
Prototypes
100%
Windtunnel Model
Proportion-
Studies
A
C
D
F
C
C
F
A
B
C
D
E
F
Styling-
Freeze
Styling–Competition
A
C
D
F
C
C
F
A
B
C
D
E
F
Aero-
dynamic
Analysis
40%
Windtunnel Model
Concept Phase Serial Development Phase
Styling
Process
Simultaneous Usage of Experimental & Virtual Tools
CFD-Model
Prototypes
100%
Windtunnel Model
Proportion-
Studies
A
C
D
F
C
C
F
A
B
C
D
E
F
Styling-
Freeze
Styling–Competition
A
C
D
F
C
C
F
A
B
C
D
E
F
Aero-
dynamic
Analysis
40%
Windtunnel Model
Concept Phase
Fig.1: CFD in the aerodynamic development process [1]
At the BMW group wind tunnel and CFD are not considered as competing tools, rather they
are utilized in a complementary fashion.
To be accepted as a valuable tool in an industrial environment a CFD code ideally has to
• be accurate (∆CX <±0.005, ∆CZ <±0.010), at least for trend predictions
• require a minimum of geometry input preparation
• be able to handle complex geometries (underhood & underbody details)
• deliver results in a reasonable timeframe (over night)
• be easy to use (by wind tunnel engineers, i.e. non-numerics specialists)

- 2 –
Around 1997 BMW started to validate a Lattice-Boltzmann code (PowerFLOW by EXA
Corp.) for aerodynamics [2]. To date the tool has reached a level of maturity which enables its
productive use in external aerodynamics. In close cooperation with the code developers we
are working to extend the applicabilty to thermal management investigations, where currently
still a traditional tool (STAR-CD) is employed.
2. Basics of Lattice-Boltzmann Methods
This chapter only intends to convey the basic ideas of Lattice-Boltzmann methods. Details
can be found in [3]-[6].
2.1 Mesoscopic Approach
The macroscopic behaviour of fluids that we observe and which is governed by the Navier-
Stokes equations is the consequence of molecular motion, described by kinetic theory.
Although molecular dynamics is simpler and more general than the macroscopic approach,
the numerical simulation of flows at a microscopic level is still prohibitive for practical
problems.
The idea of Lattice methods is to construct a simplified microscopic description at a
mesoscopic level between kinetic theory and Navier-Stokes equations that still contains the
essentials to produce the correct macroscopic appearance (Fig. 2).
Fig.2: Mesoscopic approach to the simulation of fluid motion
2.2 Kinetic Theory
The interaction of molecules composing a fluid is described by kinetic theory. Unlike the
Navier-Stokes equations where macroscopic variables like density, velocity and temperature
are used, the fundamental quantity in kinetic theory is a velocity distribution function
Eq. (1) ( )tcxff ,,=
which gives the number of particles per unit volume at time t in the phase space x and
c (location and particle speed). Macroscopic quantities are obtained by integration (Eq.2-4).

- 3 –
Eq. (2) Density
Eq. (3) Momentum = cdctcxftxutx ),,(),(),(ρ
Eq. (4) Energy −= cductcxftxTtx 2
)(),,(),(),(ρ
This velocity distribution function is governed by the Boltzmann equation describing the rate
of change due to non-equilibrium which is represented by the collision term on the right-hand
side
Eq. (5) ),,(),,(),,(),,( tcxCtcxfctcxf
t
tcxf
dt
d
=∇⋅+
∂
∂
=
Realistic fluid behaviour is obtained only if the collision term satisfies the necessary
conservation laws
Eq. (6) Mass = 0)( cdcC
Eq. (7) Momentum = 0)( cdcCc
Eq. (8) Energy ( ) = 0)(
2
2
1 cdcCc
It should be noted that the Navier-Stokes equations can be derived from kinetic theory by the
so-called Chapman-Enskog expansion.
2.3 Concept of Lattice Methods
Lattice methods are the numerical implementation of kinetic theory. The continous velocity
distribution function is replaced by a discrete set of particle states, i.e. velocities in terms of
direction and magnitude.
Eq. (9) Vtxiftxintcxf ∆≡→ ),(),(),,( where },...,1;{ miicc =∈
This means that the actual state of the fluid is described by the number ni of particles
populating the i-th state in each cell at each time step. The choice of the number m of possible
particle states is a tradeoff between accuracy/noise in the solution and memory
consumption/computational effort.
During one elementary timestep particles will move to one of the neighbouring cells
according to their current speed. In each cell the total population of particles will be
redistributed among the available states by a collision operator Ci of the Lattice-Boltzmann
equation.
= cdtcxftx ),,(),(ρ

- 4 –
Eq. (10) ),(),(),( txiCtxintticxin +=∆++
The properties of the collision operator determine wether a lattice system produces a
physically meaningful flow field. In particular, it has to be ensured that the conservation laws
(Eq. 6) are satisfied by the numerical model.
Since the molecular viscosity depends on the mean free path between collisions MFPλ and the
speed of sound a (determined by temperature T)
Eq. (11) RTa MFPMFP κλλν ⋅=⋅=
it can be calculated in Lattice methods once the particle distributions are known. A result of
the Chapman-Enskog expansion is the relation between viscosity ν, temperature T and a
collision frequency ω
Eq. (12)
2
11
−=
ω
ν
T
Viscosity is reduced by increasing the collision frequency, i.e by reducing the time between
collisions and hence the mean free path. For a positive viscosity it is necessary that ω<2 but
inviscid flow can not be simulated by setting ω=2 because this would cause stability
problems in the collision algorithm which requires a finite remainder of viscosity.
The above relation is used to set the molecular viscosity in the collision operator as a
relaxation parameter ω when driving the particle distribution to an equilibrium representing
the status of maximum entropy. The latter is calculated from the instantaneous macroscopic
quantities.
Eq. (13)
( ) i
n
eq
i
n
eq
i
n
i
ntx
i
n
tx
i
n
i
Ctx
i
ntt
i
cx
i
n
⋅−+⋅=
−−=
+=∆++
ωω
ω
1
),(
),(),(),(
The basic concept of a lattice model will be explained for a simple 2D model (Fig.3)
If we choose a lattice composed of cubic cells (any other shape would also be conceivable),
four directions are possible along which particles can travel. How far they may move per time
step depends on their speed. In this example we allow 0, 1 and 2 cells/timestep, resulting in 4
directions x 3 speeds = 12 states. Since it is not necessary to store directions for rest particles
with 0 speed we actually have 9 states, i.e. 9 integer arrays can hold the description of the
flow field in each cell per time step. The maximum number of particles which can populate
each state depends on the number of bits allocated for the state vectors and hence determines
the memory consumption (and computational effort) of the code.

- 5 –
1
Possible
Directions
2
3
4
1
Possible
Directions
2
3
4
Particle with
speed 1 in
direction 4
Particle with
speed 1 in
direction 4
Particle with
speed 2 in
direction 3
Particle with
speed 2 in
direction 3
Particle with speed 0
Particle with speed 0
Fig.3: A simple 2D lattice model
Macroscopic quantities of interest are obtained by statistical evaluations of the states, i.e. the
integrations (Eq. 2-4) are replaced by summations
Eq. (14) Density =
j
j txntx ),(),(ρ
Eq. (15) Momentum ⋅=
j
jj txnctxutx ),(),(),(ρ
Eq. (16) Energy ⋅⋅=
j
jjj txnccmtxE ),()(),( 2
1
It should be noted that higher order moments like the stress tensor can also be evaluated
statistically without the need to calculate local derivatives of macroscopic quantities.
Individual particle speeds can be much higher than what we observe as the macroscopic fluid
velocity. If the same number of particles is moving in each of the directions of the lattice
model, the fluid velocity vanishes. As an example, the average speed of oxygen molecules at
20°C in a fluid at rest is approximately 1000 m/s.
2.4 Fluid-Fluid Interaction
In the course of a transient simulation the dynamics in the fluid consists of the two steps Move
and Collide. First particles move to neighbouring cells according to their current state (Eq.12).
This leads to collisions which are resolved by redistributing the total number of particles in
each cell to the available states. For a 2-state model this process is sketched in Fig. 4.

- 6 –
Time t
Time t+1
n1
n2
n‘2
n‘1
Fig.4: Move & Collide Process (with two states)
This collision process only produces physically correct fluid behaviour if the collision
(redistribution) respects the conservation laws (Eq.6-8). In case of mass conservation this
requirement is very obvious because it means that the total number of particles after collision
must must be the same as before
Eq. (17) 21
'
2
'
1 nnnn +=+
If the state vectors ni are integer quantities conservation will be guaranteed without any
round-off errors.
The repetition of this Move-Collide process according to the update equation (Eq. 9,12) forms
an inherently transient solver. It does not solve a partial differential equation like in traditional
CFD codes but rather simulates the evolution of particle distributions in time. This algorithm
is very well suited for parallel processing and – in the presence of a finite viscosity – stable,
i.e. computationally robust.
2.5 Fluid-Surface Interaction
Usually the computational domain contains solid walls so that there will be particles
impinging on these surfaces. The interaction between wall and fluid is modeled by surface
elements (surfels) which gather and scatter particles while altering their momentum. Two
extreme situations are possible, specular reflection (Fig. 5-left) and bounce-back reflection
(Fig.5-right).
Fig.5: Gathering and scattering of particles on solid walls
Bounce Back ReflectionSpecular Reflection
Vin
Vout
Vtin
Vnin
Vtout
Vnout
Vin Vout
Bounce Back ReflectionBounce Back ReflectionSpecular Reflection
Vin
Vout
Vtin
Vnin
Vtout
Vnout
Vin Vout

- 7 –
During a specular reflection the normal component of a particle’s velocity is inverted while
the tangential component remains unchanged. A momentum balance before and after collision
shows that only a normal force is exchanged between fluid and surface, i.e. this type of
reflection represents a frictionless wall (slip condition).
The bounce-back reflection inverts both the normal and the tangential velocity component of
impinging particles and hence results also in a tangential force between fluid and surface.
This is the no-slip condition where the fluid velocity is zero at the wall. This wall boundary
condition can only be applied if the local resolution is sufficient to capture the velocity
gradients in the boundary layer near the wall. The wall model used for high Reynolds number
flows with extreme gradients in turbulent boundary layer profiles will be explained in the next
chapter.
2.6 Turbulence Modeling
The nondimensional key figure describing the character of a fluid is the Reynolds number as
the ratio between inertial and viscous forces
Eq. (18)
For high Reynolds numbers the flow becomes turbulent, i.e. velocity fluctuations are
superimposing the average motion.
It is known that turbulence spans a large range of scales in space and time. On the lower end
we have the Kolmogorov scale lK where turbulent kinetic energy is dissipated to heat while
the upper end goes to what is usually denoted as unsteady flow (Fig. 6).
Fig.6: Scales of turbulent motion
Even with todays computer resources we can not afford a mesh density in turbulent flows that
would be sufficient to resolve the entire range of scales for practical problems.
Space Time
TurbulentScales
Kl ν/2
Kl
L UL /
4/3
Re/ ≈KlL ( ) ( ) 2/12
Re/// ≈νKlUL
Unsteady Flow
Dissipation
ν
LU ⋅
=Re

- 8 –
However, since the small scales can have a large effect on large scale phenomena, several
approaches have been developed to model turbulence instead of directly computing its impact
on the flow field (Fig. 7). A comprehensive survey of turbulence modeling is compiled in [7].
Fig.7: Approaches to turbulence modeling
The most general method is Direct Numerical Simulation (DNS) where nothing is modeled,
instead one relies on sufficient resolution in space and time. Due to the enourmous resources
required this approach is still far away from being applied to real-world engineering problems
at high Reynolds numbers but it is successfully used to simulate laminar flows at low
Reynolds numbers, i.e. without turbulent phenomena.
A first step to turbulence modeling is Large Eddy Simulation (LES), where a filter width –
usually but not necessarily the grid size – is introduced. Turbulent structures below the filter
width are modeled by a Sub-Grid-Scale model while everything above is computed using
modifed (filtered) transient Navier-Stokes equations. In the automotive industry this model is
hardly ever used routinely in a productive environment because the requirements on computer
resources are still too high.
The model used in PowerFLOW is called Very Large Eddy Simulation (VLES). It divides the
world into universal eddies which are captured by a two-equation model and coherent
structures which are computed by the transient Lattice-Boltzmann algorithm. Details are
described in [8]-[10].
The most popular approach is called Reynolds-Averaged-Navier-Stokes (RANS) where the
velocity is split into a time averaged value and a fluctuation portion. Inserting this into the
Navier-Stokes equations leads to additional unknowns which have the form of shear stresses
and actually increase the effective viscosity. In order to close the equations system again a
vast multitude of turbulence models has been developed. The fundamental difference to the
previously mentioned approaches is the fact that this method is usually used in conjunction
with steady-state flows only.
DNS = Direct Simulation
All scales of motion in space and time are computed
RANS = Reynolds Averaging
All scales of motion are described by statistical methods (time averaged)
LES = Large Eddy Simulation
Alle Skalen werden berechnetmodeled computed via modified unsteady Navier-Stokes equations
Filter Width (Grid Size)
VLES = Very Large Eddy Simulation
modeled computed unsteady
Coherent anisotropic eddiesUniversal eddies

- 9 –
At high Reynolds numbers the extreme velocity gradients in the immediate vicinity of a wall
can not be resolved. However, they determine the wall shear stress and are therefore crucial
for correct results. When setting up a case it has to be decided in which mode the simulation
should be conducted. For low Reynolds numbers (and sufficient resolution) the choice is DNS
where neither in the fluid nor at the wall a model is employed.
For turbulent flows the boundary layer near solid walls is modeled. Under the assumptions
• Two-dimensional flow (no cross flow in the boundary layer)
• Equilibrium condition (no streamwise pressure gradient along the wall)
a universal nondimensional velocity profile – the logarithmic law of the wall - can be derived
from the Navier-Stokes equations.
Eq. (19)
where velocity and distance from the wall have been non-dimensionalized as
Eq. (20)
Using the velocity in the first cell above the wall and the local wall distance allows the
calculation of the wall shear stress which is then used to alter the momentum of scattered
particles (Fig.5). According to the assumptions above this law of the wall is strictly valid only
for flat plate flow. For a reasonable prediction of pressure induced free surface separation an
extension has been added where the nondimensionless wall distance is scaled as a function of
local pressure gradient.
Eq. (21)
∂
∂
+=→ ++++
x
p
fAAyUyU 1with)/()(
The function f has been adjusted such that in the presence of a pressure gradient the scaling
leads to a realistic separation behaviour.
Transition from laminar to turbulent flow can currently not be simulated yet.
0.54.0)ln(
1
:505
:5
≈≈+=≤≤
=≤
+++
+++
BandwithByuyfor
yuyfor
κ
κ
ρ
τ
ν
τ
τ
τ
w
uwith
u
yy
u
u
u === ++

- 10 –
3. Simulation Process
With the Lattice-Boltzmann method the individual steps to a result are essentially the same as
for traditional (RANS) CFD codes (Fig.8).
Fig.8: Simulation process
The fundamental difference here is the discretization which is fully automatic as part of the
simulation and leads to a significant shortening of the total turnaround, especially for complex
models with high level of detail.
3.1 Geometry Preparation
There are two sources of geometry input, either virtual models from a CAD/CAS-system
(CATIA/ALIAS)) or hardware clay models which are laser-scanned and processed with
PolyWORKS. In both cases geometry preparation means to create the surface facetizations of
any number of solids which compose the entire configuration (Fig.9).
This facetization only represents the geometry, it does not define the resolution for the
simulation. A cube for instance would be completely described by two triangles on each face,
regardless at which resolution it will be simulated. Components may be arranged in an
arbitrary fashion and even intersect each other without the need to create a single mesh over
all wetted surfaces as in RANS codes. Typical facet counts are several hundred thousand to
some million triangles for detailed automobiles or motorcycles.
CAD/CAS Model
CATIA/ALIAS
CAD/CAS Model
CATIA/ALIAS
Clay Model
POLYWORKS
Clay Model
POLYWORKS
Simulation Model
(Surface Facetization)
ANSA, POLYWORKS, PowerWRAP, ...
1-5 Days
Simulation Model
(Surface Facetization)
ANSA, POLYWORKS, PowerWRAP, ...
1-5 Days
Simulation
PowerFLOW
1 Day
Simulation
PowerFLOW
1 Day
Postprocessing
PowerVIZ
Postprocessing
PowerVIZ
ResultResult
Shape Modification
of CAD/CAS Data
Shape Modification
of CAD/CAS Data
Morphing of the
Surface Mesh
(PowerCLAY)
Morphing of the
Surface Mesh
(PowerCLAY)
Turnaround
2-6 Days
Turnaround
2-6 Days

- 11 –
Fig.9: Geometry input (solids represented by surface facetizations)
3.2 Automatic Discretization
The lattice applied in PowerFLOW is a rectangular cartesian mesh with cubic cells (Fig.10).
For an economic use of cells it is possible to have regions of variable resolution in the
flowfield. Cell size always varies by a factor of 2 from one level to the next. These resolution
regions are defined by simple geometries or created as offsets to selected parts of the surface.
Fig.10: Lattice of cubic cells

- 12 –
During the automatic discretization all intersections between lattice planes and geometry
facets are calculated. This breaks up the triangles into arbitrary but still planar surface
elements (surfels) which accomplish the fluid-surface interaction by gathering and scattering
particles. That means that solids are represented as smooth as they are defined by the
facetization and not simply by blocking cells. The 2D sketch of this process in Fig.11 looks
quite trivial but is actually very complex for detailed 3D configurations.
Voxels
(Fluid Cells)
Solid Body
Facets
(Geometry)
Surfels
(Surface Elements)
Voxels
(Fluid Cells)
Solid Body
Facets
(Geometry)
Surfels
(Surface Elements)
Fig.11: Automatic discretization
3.3 Transient Simulation
Simulations are always run in transient mode by iterating the update equation (Eq.13). The
physical time ∆t per timestep is fixed by the cell size ∆x [m/cells] and the mapping of a
macroscopic reference velocity V∞ [m/s] to its equivalent in the lattice world VL
[cells/timestep].
Eq. (22) [ ]mestepseconds/ti
V
V
xt L
∞
⋅∆=∆
Replacing the lattice velocity by the speed of sound aL (depending on temperature only) and
the Mach number Ma∞ strictly does not leave room for the user to control the timestep once
test conditions and setup have been fixed.
Eq. (23) [ ]mestepseconds/ti
V
x
Maat L
∞
∞
∆
⋅⋅=∆
Since the ratio of seconds per timestep determines the computational effort to simulate a
certain physical time interval, it is desirable to make this as large as possible.

- 13 –
PowerFLOW is a compressible code but limited to a Mach number range of up to Ma≈ 0.4
due to details of the particle model. If we assume that compressibility effects are weak in this
range a speedup can be achieved by optionally running at an artificially elevated Mach
number. For example, at V∞ = 50m/s and T∞ = 20°C the Mach number is Ma∞ ≈ 0.15 and with
a cell size of ∆x=2mm results in a timestep of ∆t ≈ 5.
10-6
sec/timestep so that we need 200000
timesteps to cover one second of physical time. If we simulate at Ma∞ ≈ 0.3 instead the run
time for the same physical time is cut in half. This would only neglect the difference in
compressibility between the two Mach numbers, not dropping it completely.
A simulation runs similar to a wind tunnel experiment. Starting from initial conditions the
flow field is updated from timestep to timestep. There is no explicit convergence criterion like
in steady-state RANS codes. Instead the user sets the physical time or number of timesteps to
run and/or monitors the transient behaviour of certain criteria to decide when to stop. In
external aerodynamics these are typically the integral force coefficients and for internal flows
pressure losses or mass flow rates.
An example for the time history of drag and lift coefficients is shown in Fig.12. When starting
from scratch the initial condition is usually free stream velocity everywhere and therefore far
away from a physical state around the car. After an initial transient the flow field will
eventually fluctuate more or less around an average, depending on the particular problem. A
significant time saving can be achieved if the solution for a similar case is already available
for seeding initial conditions, for instance when conducting detail optimization or variant
studies.
Fig.12: Time history of drag and lift coefficients
After the simulation has been terminated the time-dependent results are available for post-
processing their transient behaviour, for instance with open convertibles or evaluating surface
pressure fluctuations to identify aeroacoustic noise sources. For reporting integral forces or
pressure loads on surface parts like windows or hoods it is possible to generate averaged
results over selected time intervals (Fig.12).

- 14 –
4. Validation Examples
For internal validation purposes BMW uses amongst others the previous 5series limousine
and touring variants equipped with pressure probes and an open convertible, all in 40% scale
as well as a full scale motorcycle model.
A comparison of drag and axle lift forces for the 5series limousine is shown in Fig.13. The
perfect agreement of CX is a coincidence here because of course there would also be a certain
variation across different wind tunnels or test conditions but usually the error in drag is well
below 10 counts. Remarkable is the good correlation between measured and computed axle
lift forces. Since the top projection of a car is roughly four times larger than the frontal area,
this component is also four times more sensitive to errors in the pressure distribution.
Fig.13 : Comparison of drag and lift (BMW 5series limousine)
A good correlation of integral values can be the result of compensating errors. Therefore it is
vital to also check flow field details. The centerline pressure distribution of the 5series touring
is compared in Fig.14.
!"# $
!"# $
Fig.14 : Comparison of the centerline pressure distribution (BMW 5series touring)

- 15 –
Discrepancies are visible on the bottom between the wheels and on the rear window.
However, this is an example that only looking at details can also be misleading. Although the
calculated pressure on the rear glass and the front underbody is lower, the integrated drag is
5% smaller and the front lift 45 counts higher than in experiment.
A very vivid way of visualizing the flow field topology in the wind tunnel are oil flow
pictures which are compared with computed wall streamlines in Fig.15.
A-Pillar C-Pillar
Fig.15 : Comparison of wall streamlines and oil flow pictures
A typical property of the Lattice-Boltzmann code is visible on the sideglass. The A-pillar
vortex tends to be predicted too strong – in contrast to RANS methods where higher
numerical diffusion mostly leads to a faster decay of vortices. The agreement looks better for
the reattachment line inboard of the C-pillar and even a focus point on its foot is produced
like in experiment.
The velocity distribution in the wake reflects what is happening to the flow when it passes the
vehicle. Fig.16 compares hot wire anemometry data with simulation results in a plane 400mm
behind the car.

- 16 –
Experiment Simulation
Fig.16 : Comparison of the velocity magnitude in the wake
It is known that it takes a
certain velocity for drag and
lift to become independent of
the Reynolds number. In
Fig.17 it is shown that this
effect is correctly captured in
simulation, both when
running the full scale
geometry and the 40% scale
model at a 2.5 times higher
velocity to obtain the same
Reynolds number.
Fig.17 : Comparison of drag coefficient Reynolds dependency
The Reynolds effect study above also demonstrates the possible spreading between different
wind tunnels
An advantage of CFD vs. experiment is the availability of all flow field details for in-depth
analysis. If geometry modifications yield unexpected results it is very difficult if not
impossible to identify the reasons in the wind tunnel. Figs. 18 and 19 demonstrate how CFD
can help to gain insight.
The vehicle is cut into slices whose drag and lift contributions are integrated individually (red
bars). A drag and lift development along the free stream direction is obtained by summing up
the slices (blue curve). This diagram makes obvious where drag and lift are generated or
reduced. Conducting this analysis also in vertical direction enables the aerodynamicist to
clearly identify critical regions. Even more value can be realized by generating the difference
of this data between two variants.
Note the good agreement of lift balance which is important in particular for motorsports.

- 17 –
0,0 0,1 0,3 0,4 0,5 0,6 0,7 0,9 1,0
0,0
!
%%
Fig.18 : Analysis of drag generation
0,0 0,1 0,3 0,4 0,5 0,6 0,7 0,9 1,0
0,0
"
" !
Fig.19 : Analysis of lift generation

- 18 –
After a thorough validation [11] the code is now also used for motorcycle aerodynamics.
Fig.20 shows a good correlation of the drag area CX*A for three different windshields, both in
terms of absolute values and ranking.
0,300
0,320
0,340
0,360
0,380
0,400
0,420
0,440
Serie LT Sport
Cx*A
Windkanal
(Aschheim)
PowerFLOW
&
'
&(
&
'
&(
Fig.20 : Comparison of motorcycle drag areas
On a motorcycle the rider is part of the aerodynamics and immediately exposed to the flow.
Beyond the prediction of drag and lift a correct flow field is crucial for the assessment of the
rider’s comfort. The comparison of the velocity distribution in a horizontal plane shows that
the trajectory of the shear layer which separates from the windshield is correctly predicted
relative to the rider.
) #!) #!
Fig.21 : Comparison of velocity magnitude in a horizontal plane

- 19 –
5. Various Applications
Apart from calculating drag and axle lift coefficients CFD is used to gain qualitative insight to
flow field details which are hardly or not at all accessible by experiment.
Isosurfaces of total total pressure are used to identify regions where losses are generated. In
Fig.22 the isosurface for Cpt=(pt-p∞)/q∞=0 is depicted, illustrating where the energy loss is
equal to the dynamic free stream pressure. Postprocessing tools allow to sweep dynamically
through any range of values. Generating an isosurface for VX=0 visualizes regions of reverse
flow. As time dependent animation this allows the assessment of passenger comfort in open
convertibles or on motorcycles (Fig.23).
Fig.22 : Isosurface of total pressure (Cpt=0) Fig.23 : Isosurface of reverse flow (VX=0)
Once the surface pressure distribution is available it can be used to generate area loads for
structural analysis. The FEM model (or parts thereof) is mapped onto the CFD model and the
pressure including an optional backside value is applied. A file in NASTRAN or ABAQUS
format is exported ready as input for the FEM tool.
CFD Model
FEM Model
Area Loads on the FEM Model
Fig.24 : Mapping of area loads to FEM models
In a similar way heat transfer coefficients may be transferred to ABAQUS models. When heat

- 20 –
transfer is switched on, the coefficients are part of the solution while in isothermal
simulations they are obtained by an extended Reynolds analogy which also takes into account
information from turbulence modeling. An example for brake cooling is shown in Fig.25.
Fig.25 : Mapping of heat transfer coefficients to ABAQUS models (brake cooling)
More and more detailed underbodies and the flow through the engine compartment are
already included in the early phase of external aerodynamic development in order not to miss
their influence on the outer flow field. Cooling package components are modeled as porous
media applying Darcy’s law for the pressure loss [12]. For fans the most recent version offers
a rotating frame of reference model as an alternative to a simple momentum source.
Fig.26 : Underhood cooling air flow
For isothermal flows the cooling air mass flow rate is now predicted with around 5% error
which is in the range of experimental uncertainty. Development work still needs to be done
for simulations including heat transfer through radiators or involving hot surfaces.

- 21 –
0
20
40
60
80
100
120
140
10 100 1000 10000
Hz
dB(A)
Experiment
PowerFLOW
0
20
40
60
80
100
120
140
10 100 1000 10000
Hz
dB(A)
Experiment
PowerFLOW
Due to the small timesteps of the transient
simulation it is possible to record pressure
fluctuations at the surface and in the flow
field at high sampling rates. Applying Fast-
Fourier-Transformation (FFT) these signals
can be converted to sound pressure levels
(SPL) vs. frequency to identify the
generation of aerodynamic noise [13-14].
Since the noise is very different wether the
monitor point is lying in- or outside of a
shear layer, this application imposes
extreme requirements on the accuracy of
the flow field topology. Only recently a
validation of this capability on and around
the helmet of a motorcycle driver
has been started at the BMW group [15].
Fig.27 : Sound pressure level on a motorcycle [15]
Reasonable to good results are seen up to frequencies of 1000Hz. For better results at higher
frequencies probably more resolution would be needed. Validation in this field will be
continued.
6. Conclusion
To date the employment of a Lattice-Boltzmann code at the BMW group has reached a level
of maturity which allows its productive use in the aerodynamic development process of
passenger cars, motorcycles and in motorsports. Accuracy levels are in the order of 5% for
integral forces and cooling air mass flow rates. In particular the ability to simply compose
complex configurations of solids and the ease-of-use enable the non-numeric aerodynamicist
to use it as a complementary tool to the wind tunnel. Work is under way to complete the
capabilities for thermal management simulations and the validation of aeroacoustic
predictions has just started.
References
[1] H. Kerschbaum, N. Grün, P. Hoff, H. Winkelmann,
“On Various Aspects of Testing Methods in Vehicle Aerodynamics”
JSAE Paper 20045445, 2004
[2] W. Bartelheimer,
“Validation and Application of CFD to Vehicle Aerodynamics”
JSAE Paper 20015332, 2001
[3] C. Teixera,
“Continuum Limit of Lattice Gas Fluid Dynamics”
Ph.D Thesis, MIT, Boston, September 1992

- 22 –
[4] H. Chen,
“Volumetric Formulation of the Lattice-Boltzmann Method for Fluid Dynamics: Basic
Concepts”
Physical Review E, Volume 58, Number 3, September 1998
[5] Bernaschi, S. Succi, Y.H. Qian, H. Chen,
“Effective Volumetric Lattice Boltzmann Scheme”
Physical Review E, Vol 63, 056705, 2001
[6] H. Chen, S. Kandasamy, S. Orzag,
“Extended-Boltzmann Kinetic Equation for Turbulent Flows”
Science Magazine, 2003
[7] J.P.A.J van Beeck, C. Benocci (Editors),
“Introduction to the Modeling of Turbulence”
VKI Lecture Series, March 13-17, 2000
[8] M. Pervaiz, C. Teixeira
“Two Equation Turbulence Modeling with Lattice-Boltzmann Method”
ASME Proceedings, Boston, MA, August 1999
[9] V. Yakhot, H. Chen, I. Staroselsky
“New Approach to Modelling Strongly Non-Eqlibrium, Time-Dependent Turbulent
Flows”,
EXA Corporation, 2003
[10] H. Chen, S. Orzag, I. Staroselsky,
“Expanded Analogy Between Boltzmann Kinetic Theory of Fluids and Turbulence”
Journal of Fluid Mechanics, 2004
[11] C. Kleiner, N. Grün,
“CFD Simulation in Motorcycle Aerodynamics at the BMW Group”
HdT Conference on Motorcycle Aerodynamics, 2003, Munich, Germany
[12] D. Freed,
“Lattice-Boltzmann Method for Macroscopic Porous Media Modeling”
Int. Journal of Modern Physics C, Vol. 9,Nr. 8 (1998), pp 1491-1503
[13] K. Uchida, K. Okumura,
“Aerodynamic Noise Simulation Based on Lattice-Boltzmann Method”
SAE Paper 1999-01-1127, 1997
[14] B.D. Duncan, R. Sengupta, S. Mallick, R. Shock,
“Numerical Simulation and Spectral Analysis of Pressure Fluctuations in Vehicle
Aerodynamic Noise Generation”
SAE Paper 2002-01-0597, 2002
[15] U. Niedermüller,
“Validierung eines CFD-Tools für den Einsatz in der Aeroakustikentwicklung
von Motorrädern”
Diploma Thesis, Technical University of Munich, 2005
[16] P.J. Stewart,
“Interactive Tools for Digital CAE Shape Optimization of Class A Surface: A Bridge
between Styling and Engineering”
SAE Paper 2005-01-1902, 2005

VKI_RVAD_2005_Application_of_a_Lattice_Boltzmann_Code

Recommended

Recommended

More Related Content

What's hot

What's hot (16)

Viewers also liked

Viewers also liked (7)

Similar to VKI_RVAD_2005_Application_of_a_Lattice_Boltzmann_Code

Similar to VKI_RVAD_2005_Application_of_a_Lattice_Boltzmann_Code (20)

VKI_RVAD_2005_Application_of_a_Lattice_Boltzmann_Code