Computational Fluid Dynamics

1. KIRAN VOONNA
CSM SOFTWARE Pvt. Ltd
Bangalore
Concepts of CFD

2. • CAE with CFD is entering into a new phase
– Growing emphasis on product development, optimisation
– Wider range of applications, many involving multiple phenomena
• Industrial CFD codes already have many of required attributes
– Quick turnaround, via fast meshing, solvers and computers
– Links with design optimisation procedures
– Simultaneous flow, heat/mass transfer capability
• Improvements and extensions needed in key areas
– Overall requirement for better accuracy
– Quantify and reduce errors due to physics modelling and numerics
– Provide wider multiphysics capability, both within and outside fluids
engineering
Need of CFD

3. CFD is used to analyse problems involving fluid flow and its
associated phenomena:
• Heat Transfer
• Mass Transfer
• Chemical Reaction
• Combustion
• Multiphase Flow
Definition

4. • What is CFD
CFD is the analysis of systems involving fluid
flow, heat transfer and associated phenomena
such as chemical reactions by means of
computer based simulation.
What is CFD ?

5. CFD is not used solely for pure fluid flow problems. It can be used to
model thermodynamic effects and chemical reactions that occur
within a moving fluid.
The thermodynamic effects include heat transfer within the fluid, plus
heat transfer to and from a solid surface. Conjugate heat transfer
problems can be analyzed, in which the temperature distribution
within a solid is calculated alongside that within an adjacent fluid. As
well as heat transfer by convection and conduction, radiative heat
transfer can also be modeled.
CFD techniques are used to model the transport of chemical species
within a moving fluid. Reactions involving these chemical species
can be represented. A common example is the complex interaction
of fluid dynamics, heat transfer and mass transfer that occurs in
combustion processes.

6. Aerospace
• Cooling of gas turbine blades
• Ram air induction systems
• Flow in turbine duct cavities
• Gas turbine and rocket combustors
• Cabin ventilation and fire simulation
• Hazard analysis
Automotive
• External aerodynamics
• Underhood air flow
• Engine coolant system
• Induction system
• Catalytic converter
• Engine combustion
• Passenger comfort
Building and Environment
• Heating and air conditioning
• Clean room design
• Wind loading
• Fire hazard analysis
• Plume and effluent dispersion
• Marine technology
• Shipbuilding
• Mining
Chemical Process
• Stirred mixing vessels
• Spray dryers
• Packed bed reactors
• Jet-stirred reactor
• Furnace combustion
• Cryogenic fluid storage and flow
Industrial Applications of CFD

7. Mechanical
• Centrifugal pumps
• Heat exchangers
• Recuperators
• Steam turbine blade loading
• Flow meters
• Valves and ducting
• Home appliances
Also in
• Oil exploration and refining
• Nuclear power generation
• Coal/gas/hydro power generation
• Food processing
• Pharmaceuticals
• Physiological flow
• Electronics cooling
• Materials processing
Contd…

8. Substantial reduction of lead times and costs of new design
1.Ability to study studies where controlled experiments are difficult or
impossible to perform (e.g. very large systems, cooling of a turbine Blades)
2. Ability to study systems under hazardous conditions at and beyond their
performance limits (e.g. Fire simulation, Pipe break in Reactor etc)
3. Unlimited level of details of results, (Quantitative as well as qualitative
results)
Advantages of CFD over experiments

10. • Steady State and Transient
• Laminar and Turbulent
• Newtonian and Non-Newtonian
• Incompressible and Compressible
• Distributed Resistance (Porous Media)
• Multiple Stream
• Heat Transfer (Convection, Conduction and Radiation)
• Mass Transfer
• Chemical Reaction (including Combustion)
• Buoyancy
• Rotation
• Dispersed Multi-Phase Flows
• Free Surface flows (including Cavitation)
Types of Analysis by using CFD

11. Governing Equation (for Time dependent, 3D flow and Heat transfer of a
compressible Newtonian fluid)
The conservative form
  0




U
div
t


Mass
   
   
    S
S
S
Mz
My
Mx
w
grad
div
z
wU
div
t
w
v
grad
div
y
vU
div
t
v
u
grad
div
x
uU
div
t
u







































)
(
)
(
)
( X momentum
Y momentum
Z momentum
    Si
T
grad
k
div
divU
p
iU
div
t
i










 )
(
Internal energy
)
,
(
)
,
(
T
i
i
T
p
p




Eqn. Of State
SM Momentum Source
 Dissipation function

12. Rate of increase of
 of fluid element +
Net rate of flow
of  out of fluid
element
= Rate of increase of
 due to diffusion + Rate of increase of  due to
Sources
Transport equation of property 
Rate of increase of
 of fluid element +
Net rate of
decrease of  due
to convection
across the
boundaries
= Rate of increase of
 due to diffusion
across the
boundaries
+ Net Rate of creation of 
For the fluid in the control Volume,
 

 





A V
A
V
S
dA
grad
dA
U
dV
t 



Unsteady Convection Diffusion Generation

13. It is not generally possible to obtain analytical solutions to
the equations that govern the phenomena modeled
using CFD. Consequently, numerical techniques are
used. In essence, all the methods comprise two stages.
 The first stage involves approximating the full equations (usually non-linear
partial differential equations) to algebraic expressions that give the values of
the dependent variables (velocity, pressure,temperature, etc.) at a finite
number of locations within the solution domain. This process is referred to
as discretisation of the equations.
 The second stage involves obtaining solutions to the algebraic expressions
using a suitable computational algorithm.
 The different classes of CFD method employ different techniques to
discretise the governing equations.

14. Most of the transport phenomena analyzed using CFD are governed by
non-linear partial differential equations.
There are four types of numerical method used to obtain solutions to
these equations:
 Finite Difference
 Finite Volume
 Finite Element
 Spectral Methods
OBTAINING SOLUTIONS

15. Now a days most of the commercial CFD
codes are developed on the basis of
Finite Volume Method
WHICH METHOD?

16. The four discretisation methods have their own weaknesses and
strengths. The strengths of the finitevolume method are:
 Implementation into computer codes is straightforward
 Can easily be applied to arbitrarily shaped solution domains
 Algorithms are highly developed
 Discretisation error decreases with number of nodes used
 Emphasis is on balance of fluxes over control volumes
 Conservation is ensured because of continuity of fluxes

17. Steps involved in numerical analysation are:
 Formal integration of GDE of fluid flow over all (finite) control volumes of the
solution domain.
 Discretization involves the substitution of a variety of FD type approximation
for the terms in the integrated equation representing flow process such as
convection, diffusion and sources. This converts the integral equation into a
system of alzebraic equation.
 Solution of the alzebraic equations solved by using iterative methods to
compute different dependent variables.
WHAT IS FINITE VOLUME METHOD

18. The fluxes passing through the cell faces are calculated.
The fluxes passing through a cell face are calculated from relationships based on
geometric factors and dependent variable values at the cell centre and
neighbouring cell centers.
These flux relationships are approximations to the exact relationships that would
be derived from the governing equations.
In addition to the fluxes entering and leaving the cell, expressions representing
any sources or sinks in the cell need to be derived.
Finite Volume Method

19. The flux of a dependent variable leaving one cell is equated to the flux entering the
neighbour cell.
The value of the dependent variable at the cell centre is calculated by balancing all
the fluxes entering and leaving the cell against the sources and sinks in the cell.
Finite Volume Method

20. Flow Models

21. Coordinate Systems
x
y
z
x
y
z
x
y
z
(r,,z)
z
r

(r,,)
r


(x,y,z)
Cartesian Cylindrical Spherical
General Curvilinear Coordinates
General orthogonal
Coordinates

22. Eularian vs Lagrangian Framework

23. Flow Models
Typical model flows are:
Laminar steady flows, relatively straight forward; eg. boundary layers.
Turbulent flows, more complex and may require some form of averaging of the
kinetic energy spectrum; eg. aircraft wing flow.

24. CFD Physics Domain

25. Transport Equation
Direct Numerical Simulation (DNS),
Large Eddy Simulation (LES),
Time-dependent Reynolds Averaged Navier Stokes
equations (TRANS),
Reynolds Averaged Navier Stokes equations (RANS).

26. Transport Equation: Connections

27. Physical Behavior: Classification
Equilibrium problem Marching problem
 steady state temperature distributions
 potential flow
 steady viscous flow
 steady inviscid flow M < 1 PHYSICS
MATHS
 transient viscous flow
 transient heat conduction
 transient viscous flow
 thin shear layers (S/T)
 steady boundary layer
 transient inviscid flow
 steady inviscid flow M > 1
 wave equation
Boundary Value Problem Initial-Boundary-Value Problem
Elliptic Parabolic/Hyperbolic
0
)
( 


 
k )
( 







k
t
)
(
2
2
2








c
t
Nonlinear equations of fluid flow can change
type locally depending on the local values of
the equation.

28. Auxx + 2Buxy + Cuyy + Dux + Euy + F = 0
B2-4AC > 0 Wave Equation
B2-4AC < 0 Elliptic Equation
B2-4AC = 0  Parabolic Equation
Classification of 2nd order PD Eqn:

29. Physical Behavior: Cause, Effect & Interpretation

30. Physical Behavior: Hyperbolic

31. Physical Behavior: Parabolic
• Only one characteristic
direction
• Marching type solution

32. No limited regions of influence
Boundary Conditions
Physical Behavior: Elliptic

33. Initial Conditions
• Initial conditions (ICS,
steady/unsteady flows)
– ICs should not affect final results and only
affect convergence path, i.e. number of
iterations (steady) or time steps (unsteady)
need to reach converged solutions
– More reasonable guess can speed up the
convergence
– For complicated unsteady flow problems,
CFD codes are usually run in the steady
mode for a few iterations for getting a better
initial conditions

34. Boundary Conditions
 No-slip or slip-free on walls, periodic
 inlet (velocity inlet, mass flow rate, constant pressure, etc.)
 outlet (constant pressure, velocity convective, numerical beach*, zero-
gradient)
 and non-reflecting (for compressible flows, such as acoustics), etc.
No-slip walls: u=0,v=0
v=0, dp/dr=0,du/dr=0
Inlet ,u=c,v=0 Outlet, p=c
Periodic boundary condition
in spanwise direction of an
airfoil
o
r
x
Axisymmetric
*adding dissipative terms to the free-surface boundary

35. Boundary Conditions
Under-specification of boundary conditions leads to failure to obtain a solution.
Over-specification leads to unphysical solution near the boundary where
conditions have been applied.
• To define a problem that results in a unique solution, you must specify
information on the dependent (flow) variables at the domain boundaries.
– Specifying fluxes of mass, momentum, energy, etc. into domain.
• Defining boundary conditions involves:
– identifying the location of the boundaries (e.g., inlets, walls, symmetry)
– supplying information at the boundaries
• The data required at a boundary depends upon the boundary condition type
and the physical models employed.
• You must be aware of the information that is required of the boundary
condition and locate the boundaries where the information on the flow
variables are known or can be reasonably approximated.

36. • 1. INLET: Complete specification of the distribution of all variables except
PRESSURE.
• 2. Specification of PRESSURE at one location inside flow domain.
• 3. OUTLET: F=0, in the flow direction.
• 4. Specification of all variables or their normal gradient, except
PRESSURE and DENSITY, at solid walls.
Under-specification of boundary conditions leads to failure to obtain a solution.
Over-specification leads to unphysical solution near the boundary where
conditions have been applied.
Boundary Conditions

37. Turbulence Modeling

38. Turbulence Models

39. Turbulence, Boundary Layers etc.

40. Turbulence, Boundary Layers etc.
Transmits the effects of viscosity into the
interior of the flow (and hence the boundary-
layer concept breaks down)
Usually results in a massive increase in
pressure (or form) drag.

41. Transition
Transition from laminar to turbulent
 Amplification of initially small disturbances
 3D distortion of T-S waves
 Development of areas with concentrated rotational structures
 Formation of intense small scale motions
 Growth and merging of these areas of small scale motions into fully
turbulent flows
Transition is strongly affected by
 Pressure gradients
 Disturbance levels
 Wall roughness
 Heat transfer

42. Turbulence, Boundary Layers etc.: The effect
( )
Reynolds Stresses
Viscous Stresses
• A 3-D, time-dependent, eddying motion with many scales, causing continuous mixing
of fluid elements and often superposed on a drastically simpler mean flow;
• A solution of the Navier-Stokes equations;
• The natural state at high Re; most engineering flows are fully turbulent;
• An efficient mixer ... of momentum, energy and constituents;
• A major source of energy loss
• But not necessarily a bad thing to happen!!!
The force (per unit area)
exerted by the upper fluid
on the lower OR the rate of
transport of momentum (per
unit area) from upper fluid
to lower.
Basically turbulence can
actually be beneficial in delaying separation
and reducing pressure drag.

43. Turbulent Flow
• Six main approaches to predict
turbulent flow-
DNS
LES
RANS
PDF
DES
DSM
Data from DNS could be used to estimate measurement errors in
experiments.

44. Turbulent Flow
• Six main approaches to predict
turbulent flow-
DNS
LES
RANS
PDF
DES
DSM
A sub-grid-scale model is employed to account for the dissipation
of energy at the smallest scales and any backscatter of energy from
the large to small scale.

45. Turbulent Flow
• Six main approaches to predict
turbulent flow-
DNS
LES
RANS
PDF
DES
DSM
Single-point correlation
Multi-point or two-point correlation

46. Turbulent Flow
• Six main approaches to predict
turbulent flow-
DNS
LES
RANS
PDF
DES
DSM
The mean velocity and Reynolds stress are the first and second
moments of the Eularian PDF of velocity.

47. Turbulent Flow
• Six main approaches to predict
turbulent flow-
DNS
LES
RANS
PDF
DES
DSM
A hybrid method that uses URANS and LES.

48. Turbulent Flow
• Six main approaches to predict
turbulent flow-
DNS
LES
RANS
PDF
DES
DSM
These models involve the solution of transport equations for each
of the independent Reynolds stress components.

49. Star-CD Implementation
EVM
DSM
LES
DES
Zero Equation
model
Constant turbulent viscosity
User defined turbulent viscosity
k-l
Spalart - Allmaras
Linear WF
One Equation
model
Linear
WF
Two Equation
model
Linear
Standard
RNG
Chen
Non-linear
Quadratic / Cubic
WF/LRe/2LR
/
HW/NWF
Linear
Non-linear
Quadratic
k-e
WF/2LR/NW
F
WF/LRe/
HW
Spezial
e
Suga Non-linear
Quadratic/Cubic
WF/2LR/NW
F
WF/LRe/NW
F
k-w Standard
SST
Linear
V2F
WF/LRe/NW
F/
HW
Linear LRe

50. Star-CD Implementation
EVM
DSM
LES
DES
RSM
Six Equation model WF
Linear
Gibson-Launder
Speziale-Sarkar-
Gatski
LRe Damping
WF
Zero Equation
model
One Equation
model
Smagorinsky
k-l
One Equation
model
Spalart - Allmaras
k-e
k-w SST
Two Equation
model

51. RANS
Fluctuation
Time averaged component
Now if we write continuity equation
RANS
( )
Reynolds Stresses
Viscous Stresses
Total 10 variables: 3 u,v,w; pressure; 6 Reynolds stress terms

52. k-e model (linear and non-linear)
 Applicable to fully turbulent, incompressible or compressible flow
 Buoyancy effects, up to some extent
Eddy Viscosity Model: k-e
RNG k-e model
 No explicit account of compressibility / buoyancy effects
 STAR-CD models these effects
 Corresponding terms could be omitted
Chen’s k-e model
 Turbulent energy transfer mechanism responds more effectively to the mean
strain rate
 STAR-CD models compressibility / buoyancy effects
 Corresponding terms could be omitted

53. Eddy Viscosity Model: k-e
BOUNDARY CONDITIONS
INLET: k and e
OUTLET or SYMMETRY: Zero gradient extrapolation
FREE STREAM: both are zero
SOLID WALLS: depends on the treatment
ADVANTAGES
Simple/st, Excellent Performance, Well established, widely validated
DISADVANTAGES
Poor performance in – flow over curved boundary layers, swirling flow, rotating
flows, fully developed flow in non-circular ducts and some unconfined flows.

54. V2F model
 Based on RSM and DNS data
 Designed to handle wall effects and to accommodate non-local effects
 Two additional turbulence quantities are solved
- wall normal turbulence intensity
- a redistribution term in the wall normal turbulence intensity expression
 Valid throughout the domain, automatically modeling the region close to wall
 Wall distance is not required
 Damping function or wall function are not needed
Eddy Viscosity Model: V2F & k-w
k-w model
Solves a transport equation for the “turbulence frequency” or, more
correctly, the dissipation rate per unit turbulent kinetic energy
 Performs well in 2-D boundary layers with adverse or favorable pressure
gradients and in recirculating flows
 Suffers from increased sensitivity to freestream boundary conditions in free
shear flows

55. Eddy Viscosity Model: k-w SST
k-w SST model
 Blends the best aspects of both k-e and k-w
 The k-w model is applied in the inner region of the boundary layer (near the
wall) whilst the k-e model is used in the outer region and in free shear flows
 Blending functions are used to switch between the turbulence models and to
calculate turbulent viscosity
 Performs well in a variety of flows including adverse pressure-gradient
boundary layers and transonic flows

56. Eddy Viscosity Model: Two Layer Model
RANS turbulence models can be to make two-layer or zonal schemes
Typically a two-equation or higher-order model is used in the bulk of the
flow while the near-wall region is treated with a simpler, usually algebraic
or one-equation, low-Reynolds-number model.

57. Eddy Viscosity Model: In general
Good Things-
 Easy to implement
 Give reasonable prediction to attached boundary layers.
Bad Things –
 Reynolds shear stresses predicted by linear EVM are isotropic
 DNS shows these are anisotropic
 Correct prediction of normal stress anisotropy is vital in predicting secondary
flow in non-circular ducts.
 Linear EVM models overpredict the turbulent kinetic energy near the stagnation
point in impinging flow  far higher heat transfer rates than occur experimentally
 Linear EVM model predicts a linear variation in swirl velocity with radius in a
fully-developed swirling shear flow in a pipe
 The asymmetric velocity profile that is observed in a fully-developed curved
channel flow cannot be predicted with a linear EVM without curvature corrections

58. NLEVM
A compromise between the simple low-cost linear EVMs and the more accurate
but expensive DSMs
Reynolds stress is calculated from an algebraic expression which includes linear,
quadratic and sometimes higher-order combinations of strain-rate and vorticity
One simple approach-
Introduce higher-order combinations of strain rate and vorticity into the eddy-
viscosity model and then tune the constants for a wide range of flows.
 Quadratic combinations of strain rate and vorticity are necessary to account for
Reynolds stress anisotropy
 Swirl and curvature effects are only accounted for by cubic terms
 Speziale’s quadratic model ensures that turbulent kinetic energy is always
positive
NLEVMs are unable to account accurately for history effects
(since convection and diffusion of the individual Reynolds stress
components are not modeled directly)

59. Differential Stress Model
aka Second Moment Closures or Stress-Transport Model or Reynolds Stress
Model
These models involve the solution of transport equations for each of the
independent Reynolds stress components. The transport equations for the
Reynolds stress are of the following form:
Calculated in exact
form and does not
require any modeling
Redistributes energy
among the normal
stresses whilst usually
acting as a sink for the
shear stresses.
Since it has zero trace,
it does not appear in
the turbulent kinetic
energy equation used
in simpler two-
equation models
Improved modeling of flow curvature and Reynolds
stress anisotropy
 Able to account for the history of the Reynolds stresses,
which is important in rapidly developing flows

60. Differential Stress Model
ADVANTAGES
 Improved modeling of flow curvature and Reynolds stress anisotropy
 Able to account for the history of the Reynolds stresses, which is important in rapidly
developing flows
 Offer the greatest sophistication of current one-point closures
 Very accurate for many simple and complex flows such as jets, asymmetric channel,
non-circular duct flows, and curved flows
DISADVANTAGES
 Very expensive to use, as it requires the solution in 3-D of 11 transport equations
rather than the 6 used by two-equation models
 Complex to implement and computations can sometimes suffer from numerical
instability
 Poor performance in axisymmetric jets and unconfined recirculating flows due to e-
equation modeling
 Not widely validated
BOUNDARY CONDITIONS
INLET: Rij and e
OUTLET or SYMMETRY: Zero gradient extrapolation
FREE STREAM: both are zero
SOLID WALLS: wall functions

61. LES
The current implementation in STAR-CD is limited to incompressible
isothermal flows
A transient analysis setting is also required, although the problem being
modeled may in reality be a steady-state one.
Smagorinsky Model
 The simplest and most commonly used eddy-viscosity SGS model.
 It has been derived from a local equilibrium assumption
 equating production and dissipation of sub-grid turbulence kinetic
energy
Sub-grid k model
 The one-equation sub-grid k SGS model abandons the assumption of the
local equilibrium
 A filter width is defined that separates the resolved scales from sub-grid
scales
 The filter width is related to the mesh size

62. LES: Tips & Hints
The recommended discretisation practices are as follows:
• Temporal discretisation should preferably be of the Crank-Nicholson type.
 The time step for the calculation should be selected so that the
maximum Courant number is of the order of 0.5
• The convection differencing scheme for the momentum equation should
ideally be CD, MARS or Blended Differencing with a high blending factor
(greater than 0.9)
Caution is required when of linearising the source and sink terms
The SGS model influences the resolved scales through the energy sink (sub-grid
viscosity)
 It is thus essential to ensure that no other (numerical) energy sinks are
present

63. DES
 A promising approach that combines the advantages of RANS in boundary
layers and LES elsewhere
 This approach relies on modified turbulence models that can operate either
as a standard RANS model in boundary layers or as a sub-grid-scale (SGS)
eddy viscosity model in detached or separated flow regions
 Compared to other unsteady approaches like URANS, the resolved
turbulence depends on mesh density (similar to LES)
Spalart-Allmaras Model (one equation model)
k-w SST Model (two equation model)
k-e model (two equation model)

64. DES: Implementation
Since it can operate in two modes, careful handling of the convective fluxes is
required
 In the first reported DES simulations, high-order upwind schemes were
used
 Then hybrid (upwind-central) schemes where introduced to eliminate
numerical viscosity caused by upwinding in the LES regions of DES
 The present implementation in STAR-CD relies on a hybrid scheme
based on MARS and CD schemes:
Euler fluxes for DES
Central approximation of Euler fluxes
upwind approximation of Euler fluxes,
Empirical blending function
1: DES operates in RANS mode
0: DES operates in LES mode

65. DES: How to setup

66. DES: How to setup

67. Near Wall Phenomena

68. Near Wall Phenomena

69. Near Wall Phenomena

70. Near Wall Phenomena

71. Y+: Limits of Various Regions

72. Y+: Limits of Various Regions
Log Law
u+=y+
First cell here
for wall
functions
“Universal" velocity distribution for a smooth wall

73. Wall Functions vs Low-Re Models
Two main approaches to the treatment of the near-wall region
 Low-Reynolds-number approach
 Wall-function approach
Outer edge
of log layer
The lower limit of nodes
required for accurate CFD
simulations is around ten.
In the low-Re approach, the model
incorporate damping functions that
account for the increasing influence of
molecular viscosity and the preferential
damping of wall-normal fluctuating
velocity components as the wall is
approached.
A very fine grid has to be employed in
order to track the rapid changes in the
turbulence parameters near the wall,
with typically 10 nodes within y+ = 10
and the near-wall node below y+ = 1.
Offers the greater accuracy of the two
methods. However, the highly
elongated cells in the near-wall region
slow numerical convergence, CPU
costs are high and computer storage
requirements are large.

74. Wall Functions vs Low-Re Models

75. Wall Functions vs Low-Re Models
A wall function computes properties in the log layer (15< y+ < 100) of an attached
turbulent boundary layer at a wall-
 Can remove the grid points in the log layer  this reduces the overall number of
grid points
 Also removes the smallest grid cells that inhibit iterative convergence.
 Applicable in very simple near-wall flows
 Can lead to major errors in complex, non-equilibrium flows
To link the fluxes through the wall face of the
boundary cell to variable values at the central node
To modify the calculation of the source terms in
the turbulence transport equations
So that the non-linear variations in the flow
properties through the turbulent boundary
layer could be captured

76. Wall Functions
Standard wall functions
 Variations in velocity etc. are predominantly normal to the wall  one-dimensional
behavior
 Effects of pressure gradients and body forces are negligibly small  uniform shear
stress
 Shear stress and velocity vectors are aligned and unidirectional throughout the layer
 A balance exists between turbulence energy production and dissipation.
 There is a linear variation of turbulence length scale
 To capture non-equilibrium turbulence, k-transport eqn is solved in an approximate way
Non-equilibrium wall functions
 Effect of pressure gradient is taken into account
 Implemented in k-transport eqn through the modification of its production term at the
first node
 Available only with k-e model (linear & non-linear)

77. Wall Functions
Hybrid wall functions
 Applies only to Low –Re models
 No need to have a small near-wall y+
 Y+ independency is achieved using
 either an asymptotyic expression valid for 0.1 < y+ < 100 or
 by blending low-Re & high-Re expressions for shear stress, th. energy
and chemical species wall fluxes
 Blending factor
 for viscous sub-layer  0
 for log sub-layer  1

78. Wall Functions
LES wall functions
“Quasi-DNS” is quite expensive  uses fine grid in all 3 directions in near-
wall region
Requires fine mesh (comparatively coarser) in near-wall region  y+ = 1.0
A two step process in STAR-CD
 wall fiction velocity is calculated by inverting a third order
Spalding law
 relevant fluxes for momentum, th. energy and chemical species
are computed

79. Hints & Tips
 For turbulence models using a wall function approach, or when there is
shock to be captured, use non-linear turbulence models or the Menter SST
k-ω model to predict the shock location, the pressure recovery behind the
shocks and velocities in zones with flow separation
 For an accurate prediction of the pressures on the lifting surfaces (and so
the lift coefficient), use the k-ω turbulence model
 It is not possible to tell which turbulence model is to be used for an
accurate prediction of boundary layer profile and wake
External Aerodynamics

80. Hints & Tips
 The stagnation point flow on a turbo-machine blade is often incorrectly predicted
by standard k-ε or k-ω turbulence models due to an overproduction of turbulent
kinetic energy.
 Higher-order discretisation is recommended on momentum, since the k-ε equations
are dominated by their (velocity-based) source terms.
 Lower-order (even UD) is adequate for the k-ε equation convection terms.
Ultimately, the k-ε equations are used only to approximate the turbulence viscosity
(whose existence is itself based on hypothesis), so it is reasonable to choose the
most stable approach to these equations
 Both low-Reynolds number and non-linear models are slightly less stable than the
linear high Reynolds number models. They may require slightly tighter under-
relaxation on momentum and turbulence.
Turbo-machinery

81. Changing the Turbulence Model
This facility allows you to run
a turbulent flow case by
restarting from a simulation
done for the same case but
with a different turbulence
model.
The table below illustrates the
combinations allowed and the
conversion formula adopted
when STAR encounters a
different turbulence model in
the solution file to the one
currently in use

82. – Rotating & Moving Mesh

83. Categories
1. Some moving problems can be solved in a steady state manner. The
simplest examples are such as a car in a wind tunnel where movement of
the wheels and floor can be modelled by prescribed motion at the
boundaries. More complex treatments involve the application of body
forces (centrifugal and corriolis) to be applied to part, or all, of the domain
with application to cases such as rotating machinery.
2. For cases where the domain changes shape during the course of the
calculation, such as internal combustion engines, it is necessary to use a
more complex treatment. This next degree of difficulty involves cases
where there is a one way coupling between the fluid and its boundaries.
That is to say that the behaviour of the fluid is dictated by the motion of the
boundaries, but the fluid has no influence on the motion of the boundaries.
In simple terms this means that the motion of the boundaries is known in
advance and so, whatever method is used, the mesh position as a function
of time can be calculated in advance. There are many cases where this
assumption is not fully valid: for IC engine flows the pressure in the
cylinder is enough to cause slight compression of the con-rod, but for all
intents and purposes it is sufficient.

84. Categories
Categories
3. The most complex set of moving mesh problems involves
coupling between the fluid and its boundaries: fluid-structure
interaction. For these cases the motion of the boundaries
cannot be calculated in advance, though some bounds can in
general be imposed. This type of problem requires the use of a
general mechanism to move the mesh in response to the
boundary motion.
Contd…

85. Geometry and Topology

86. STEADY
STATE
TRANSIENT Rotating and Moving Meshes
The rotating reference frame simulation
feature of STAR-CD enables the user to
model cases where the entire mesh is
rotating at a constant angular velocity about
a prescribed axis.
The same feature is extended to multiple
rotating frames of reference, in which
different angular velocities (and even
different rotating axes) are assigned to
different mesh blocks within the model.
Applications where this facility may be
used include:
 Turbomachinery
 Torque converters
 Mixing vessels
 Axial and centrifugal pumps
 Ducted fans
 Rotating Mesh
 Single rotating frame
 MRF
 Implicit
 Explicit
 Non-reflecting
 Moving meshes
 Cell-layer removal/deletion
 Sliding meshes
 Regular
 Arbitrary
 Conditional cell attachment/detachment
and change of fluid type
 Mesh region inclusion/exclusion

87. TRANSIENT
STEADY
STATE Rotating and Moving Meshes
Some practical applications of moving meshes
require a large variation in the solution
domain size. A typical example is flow in
piston engines. If the total number of cells in
the solution domain remains fixed, the cell
spacing may become too dense at some
stages of the solution and too sparse at
others. This is undesirable for the following
reasons:
 The time step required to obtain a
temporally accurate solution is dependent on
the mesh Courant number. Thus,
unnecessarily small time steps might be
necessary if smaller cells are generated
during the transient process, leading to
longer computational times.
 Numerical instability problems associated
with large aspect ratios may occur.
• Rotating Mesh
• Single rotating frame
• MRF
– Implicit
– Explicit
• Non-reflecting
• Moving meshes
• Cell-layer removal/deletion
• Sliding meshes
– Regular
– Arbitrary
• Conditional cell attachment/detachment
and change of fluid type
• Mesh region inclusion/exclusion

88. TRANSIENT
STEADY
STATE Rotating and Moving Meshes
In many practical applications of fluid
dynamics, fluid motion is caused or
regulated by the relative movement
between one part of a solid body and
another. This is usually accompanied
by a strong inherent unsteadiness in the
flow pattern. Examples of situations
where such flows occur are:
• Mixing vessels
• Turbomachinery
• Ducted fans
• Ship and aircraft propellers
• Reciprocating engines
• Train passing through a tunnel
• Rotating Mesh
• Single rotating frame
• MRF
– Implicit
– Explicit
• Non-reflecting
• Moving meshes
• Cell-layer removal/deletion
• Sliding meshes
– Regular
– Arbitrary
• Conditional cell attachment/detachment
and change of fluid type
• Mesh region inclusion/exclusion

89. TRANSIENT
STEADY
STATE Rotating and Moving Meshes
It is possible with STAR-CD to connect or
disconnect adjoining cells or groups thereof
dynamically, according to some user
condition. The latter might be, for example,
time-related or flow-related e.g. To model
leaf valves which pop open when the
pressure difference across them exceeds a
given value. This can be done on both static
and moving meshes.
A typical application of this feature might be
the simultaneous calculation of the flows
within the intake manifold and combustion
chamber of a reciprocating engine. When the
intake valve is open, the two regions are
treated as one in the fluids calculated. At
valve closure, they are disconnected and
each region is calculated separately, using
the multiple-stream facility described above.
• Rotating Mesh
• Single rotating frame
• MRF
– Implicit
– Explicit
• Non-reflecting
• Moving meshes
• Cell-layer removal/deletion
• Sliding meshes
– Regular
– Arbitrary
• Conditional cell attachment/detachment
and change of fluid type
• Mesh region inclusion/exclusion

90. TRANSIENT
STEADY
STATE Rotating and Moving Meshes
In some practical applications, the solution
in certain parts of the mesh is of no further
interest after a given time. For example, the
flow through the intake port in an engine
simulation is important while the intake
valve is open. Once the intake valve closes,
there is no further reason to compute the
intake port flow unless a second cycle is to
be simulated (and probably not even then).
Continuing the solution in the port has the
following disadvantages:
Stability — Solution time step may still be
governed by the cell sizes in the valve region. A
larger number of corrector stages may be
necessary to reduce the residuals in this isolated
region.
Boundary conditions — Reasonable boundary
conditions must be provided. Pressure boundary
conditions, for example, may cause divergence in
the port if the volume is too small.
Resources—CPU time spent computing the
solution in this region is wasted.
• Rotating Mesh
• Single rotating frame
• MRF
– Implicit
– Explicit
• Non-reflecting
• Moving meshes
• Cell-layer removal/deletion
• Sliding meshes
– Regular
– Arbitrary
• Conditional cell attachment/detachment
and change of fluid type
• Mesh region inclusion/exclusion

91. Difference Schemes

92. Discretization Techniques Route Map

93. Difference Schemes

94. Truncation Errors: Dissipation & Diffusion
Pure Convection Equation

95. Difference Schemes

96. Unbounded Schemes
 Each of the above can be blended with UD
 The blending factor can be fixed throughout the domain or
can be specified locally using a user subroutine.
 Blending helps to reduce unboundedness.
NOTE
Difference Schemes

97. Filtered Schemes
Bounded Schemes
 Local flow conditions are used to specify a locally varying blending factor.
 The principle is to use just enough upwinding locally to ensure boundedness,
where needed, and to use CD everywhere else.
NOTE
Difference Schemes

98. Normalised Variable Diagram

99. Normalised Variable Diagram
This relationship allows the differencing scheme to be represented as a
unique line on a graph known as a Normalised Variable Diagram.

100. Normalised Variable Diagram
NVD allows one to judge whether a scheme is
bounded —
 A bounded scheme will lie within the
shaded region above, and follow UD outside
this region
 A scheme which passes through the point
(0.5,0.75) will be at least second-order, while
a scheme which passes through this point with
a gradient of 0.75 (as does QUICK) will be
third-order.
Conclusion —
 UD: only possible bounded linear scheme
 Blending of UD with a higher-order linear
scheme will reduce the order of the scheme
without ensuring boundedness.
 The closer a scheme is to UD (the less
“compressive” it is) the more stable it will be
Knowing the representation of a scheme on the NVD does not help one
to judge its usefulness beyond establishing its order and boundedness.

101. Reconstruction

102. CASE Study - I
Description –
Convection of a scalar by a velocity field
not aligned with the mesh
Goal –
 We seek a solution which is bounded
[0,1] and minimises numerical diffusion
 The solution should also be easy to
obtain, i.e. the scheme should be stable
and robust.

103. CASE Study - I

104. CASE Study - I

105. CASE Study - I

106. CASE Study - I
• Higher-order schemes diffuse less than UD
• The effect of increased compression (GAMMA0.3 compared to 0.5;
MARS1.0 compared to 0.0) is to sharpen the resolution of the discontinuity
(but at the expense of stability – MARS1.0 being the hardest to converge)
• The unbounded schemes (CD, LUD, QUICK) all violate the bounds, this
effect being reduced by blending in some UD, but otherwise capture the
discontinuity quite sharply

107. CASE Study - II
Description:
Compressible flow over an RAE2822 airfoil.
It displays supersonic expansion and shock compression
To judge the capability of the two candidate density schemes (CD and
MARS) for shock capture
Setup:
C-mesh of about 12000 hex cells
Low Reynolds k-e number turbulence model
M = 0.731, a = 2.51, Re = 6.5E06

108. CASE Study - II

109. CASE Study - II

110. CASE Study - II
Conclusion:
For shock capture one must
balance the requirements of
stability and boundedness
(MARS on density) with
sharpness of resolution (CD
on density).
The latter leads to over-shoots
and under-shoots, but these
are usually of less interest
than resolution.

111. Hints & Tips
1. Higher-order spatial discretisation is recommended on momentum
2. Higher-order schemes are more expensive per iteration, so a lower-order
initial calculation may be desirable to:
- evolve an approximate and representative field quickly before restarting
with the higher-order scheme.
- quantify the benefit of the increased order of spatial discretisation.
3. Higher-order discretisation is recommended on momentum, since the k-ε
equations are dominated by their (velocity-based) source terms.
4. It is important that the velocity gradients are modelled accurately and are
bounded
5. Lower-order (even UD) is adequate for the k-ε equation convection terms.
Ultimately, the k-ε equations are used only to approximate the turbulence
viscosity (whose existence is itself based on hypothesis), so it is reasonable
to choose the most stable approach to these equations

112. Hints & Tips
6. Both low-Reynolds number and non-linear models are slightly less stable than the
linear high Reynolds number models. They may require slightly tighter under-
relaxation on momentum and turbulence.
7. The convergence characteristics of higher-order schemes are enhanced by
slight under-relaxation (e.g. for MARS use 0.5 on momentum and
turbulence, 0.15 on pressure).
8. For compressible flows, aim to use CD on density eventually, in order to
capture shocks as sharply as possible.
9. SFCD, GAMMA and QUICK are not recommended on all-tet meshes.
10.The extra computation involved in non-linear schemes can provide a further
mechanism for round-off error to influence the solution. Where round-off is
suspected as contributing to switching or non-convergence of a run with a
non-linear scheme, running in double precision will minimise its influence.

113. Hints & Tips
Hints & Tips
11.As seen in the scalar diffusion example, discretisation practices depend on the
mesh – the user can make sensible choices to make the task easier for the
discretisation scheme. A hex mesh placed at 45 degrees to the flow can produce as
much numerical diffusion as a tet mesh.
12.The order of accuracy of a scheme is formally derived from a Taylor series
expansion to calculate cell-face values on a regular mesh. Severe mesh variations
(mesh expansion or kinks) reduce the order by one (at least).