SlideShare uma empresa Scribd logo
1 de 11
Baixar para ler offline
Master thesis report on
VORTEX SHEDDING AND AERODYNAMIC DRAG ON TRUNCATED
TRAILING EDGE AIRFOIL
Conducted during
February - June 2015
Submitted by:
Koushik Bangalore Gangadharacharya
Master of Science in Aerospace Engineering
Royal Institute of Technology, Stockholm, Sweden
Under the supervision of
Hans Mårtensson&Lars Ellbrant
GKN Aerospace, Trollhättan, Sweden
Examiner:
Prof. Arthur Rizzi
Aeronautical and Vehicle Engineering Dept.
Royal Institute of Technology, Stockholm, Sweden.
1 Copyright © 2015 by GKN Aerospace Sweden
Master thesis report
February – June 2015
VORTEX SHEDDING AND AERODYNAMIC DRAG ON TRUNCATED TRAILING
EDGE AIRFOIL
Koushik Bangalore Gangadharacharya
Royal Institute of Technology
SE-100 44 Stockholm, Sweden
E-mail: kobg@kth.se
ABSTRACT
The thesis work content is to evaluate the use of more
advanced turbulence models available in the ANSYS CFX
software for aerodynamic calculations. In particular for flows
over airfoils with thick trailing edges, the turbulence modeling
is challenging to traditional methods, as both thin boundary
layers as well as an unsteady wake needs to be well
represented. This is done by using the standard SST and then
performing unsteady computations using the more advanced
unsteady SAS-SST model to get the relevant CFD results. By
comparing to tests performed at GKN and results from
literature the improvement could be assessed in terms of
modeling quality and computational cost. The results presented
give a good contribution to how the modeling of unsteady
wakes can be improved and used for design purposes.
KEY WORDS
Computational fluid dynamics (CFD), unsteady
aerodynamics, turbulence modeling, Reynolds number (Re),
Strouhal number (St), coefficient of pressure.
NOMENCLATURE (SI UNITS)
Cp Coefficient of pressure
Cpb Coefficient of pressure at airfoil base
c Chord length of the airfoil
D Base height of the airfoil
f Frequency of vortex shedding
k Von Karman length scale
LES Large Eddy Simulation
RANS Reynolds Averaged Navier Stokes
Re Reynolds number
SAS Scale Adaptive Simulation
SST Shear Stress Transport
St Strouhal number
S Strain rate
TET Truncated tailing edge
u,U Velocity
URANS Unsteady Reynolds Averaged Navier Stokes
Δp pin- pout
φ Loss coefficient
ρ Density
µa Viscosity of air at 25º C
µw Viscosity of water at 20º C
p1 Static pressure
1. INTRODUCTION
The modern day numerical CFD prediction tool is
validated with experiment results for vortex shedding and drag
prediction for the flow over truncated trailing edge (TET)
airfoil (so-called flatback or thick trailing edge airfoil). As
discussed in [1], RANS numerical simulation and experimental
data of TET airfoil demonstrates significant improvement in
subsonic lift characteristics compared to non-TET airfoil
including higher maximum lift coefficients and less loss of lift
due to premature boundary layer transition. TET airfoil also
serves as viable configuration of airfoil, connecting the
structural and manufacturing requirements for rotary turbine
blades with acceptable aerodynamic performance. However,
TET airfoils exhibit higher drag levels due to the low pressure
region in the wake of thick tailing edge. The adverse pressure
gradient allows vortices to form immediately after the trailing
edge as shown in Figure 1.
Figure 1. Vortex shedding at the blunt trailing
edge [2].
2 Copyright © 2015 by GKN Aerospace Sweden
Previous study of the drag on the TET airfoil by using
RANS and LES numerical simulation suggests that 2D
numerical simulations over-predicts the drag by nearly 100%.
However, same trend is not shown in case of 3D simulations
[3].
In this paper, flow over the blunt trailing edge airfoil
NACA 64-621-TET as shown in Figure 2 is simulated using
SST and SAS SST turbulence models on ANSYS CFX solver
as a test case. The Cp distribution is determined, in particular
the base pressure coefficient Cpb is estimated for effectively 2D
and 3D cases of NACA airfoil. The 2D simulation results are
then validated with effectively 2D wind tunnel experimental
values conducted at Ohio State University, Ohio [4].
Figure 2. Dimensions of NACA 64-621 TET airfoil [4].
Using the results of NACA 64-621-TET airfoil the order of
magnitude of error is determined. Further, same turbulence
models are used to simulate the flow over GKN TET airfoil and
the results are again validated with water tunnel experiment
conducted at GKN Aerospace, Sweden. By doing so, validation
is made whether unsteady SAS SST turbulence model can
predict the drag and capture the wake vortices as a measure of
Strouhal number (St) for the flow over TET airfoil to assess the
efficiency and accuracy of the model.
2. METHODOLOGY
2.1 NUMERICAL METHODS
The SST is a standard two-equation eddy viscosity
turbulence model in CFD. It is expected to accurately predict
the onset and the amount of flow separation under adverse
pressure gradient. The flow separation at the flat face of the
TET airfoil can be essentially related to the Cpb value as the
adverse pressure gradient occurs at the base of the airfoil. SST
model is a combination of k-ω and k-ε turbulence models such
that the k-ω is used in the inner region of the boundary layer
and switches to k-ε in the free shear flow [5]. SST turbulence
model gives the steady state results for the flow.
The SAS SST (or just SAS) is a hybrid model used to solve
an unstable flow conditions considered in this paper. SAS is
based on the introduction of Von Karman length-scale into the
turbulence scale equation. In SAS model, unstable vortices in
the wake of the airfoil are resolved based on Lνk shown in
Equation 1 and Figure 3, which is governed by Von Karman
length-scale, strain rate and square of velocity gradient tensor.
Whereas in LES model, wake vortices are resolved based on
grid size as shown in Figure 3. Therefore, SAS is expected have
less grid influence compared to LES. At the same time, SAS
model provides standard RANS capabilities in stable flow
regions. These capabilities of SAS can be well utilized when
the mesh resolution and the time-step is optimum for the
considered flow conditions.
U
S
kL k 2

 (1)
Figure 3. Resolved vortex comparison in SAS with
LES [6].
2.2 PREDICTION METHODS
The drag due to pressure loss Δp for the flow over TET
airfoil in a confined space as shown in Figure 4 is estimated by
Equation 2 and hence the loss coefficient φ can be defined as
shown in Equation 4.
Figure 4. Flow domain.
crossApD  (2)
qACD baseD  (3)
cross
base
D
A
A
C
q
p


 (4)
An important flow parameter in analysis of blunt airfoil
profile is Cp and Cpb as defined in Equation 5 and 6. Due to
flow in a confined space, average pressure reduces at section-1
shown in Figure 5. Pressure drop is expected because of
reduced flow area at section-1 due to presence of airfoil. Hence
Cpb1 is defined in Equation 7.
3 Copyright © 2015 by GKN Aerospace Sweden
inin
in
p
PP
PP
C



0
(5)
inin
inbase
pb
PP
PP
C



0
(6)
10
1
1
PP
PP
C
in
base
pb


 (7)
Figure 5. Flow domain with section-1.
2.3 MESH
2.3.1 NACA 64-621 TEST CASE
Typical structured grid for TET airfoil is created using
ICEM CFD as shown in Figure 5. It has a uniform rectangular
grid in the wake, allowing the wake vortices to resolve.
Figure 6. Structured grid for NACA 64-621.
As mentioned before, 2D wind tunnel experiment results
for NACA 64-621 TET airfoil is compared to CFD simulation
in 2D and 3D as a test case. Relation between the Cpb for the
free-flow and blockage is estimated by simulating the flow
domain as shown in Figure 7 and 8.
Figure 7. Free-flow case grid for NACA 64-621.
The boundary walls in free-flow case are very far from
the airfoil and are not expected to influence the flow. Whereas
in blockage case, it is expected to have boundary wall influence
from top and bottom walls as a result of which higher pressure
drop is expected in the wake for blockage case compared to
free-flow case. The blockage here is 10% of the flow area.
Figure 8. Blockage case grid for NACA 64-621.
The grid is effectively made 2D by having 2 cells in the
transverse direction of the flow and the 3D grid is created by
having node density in transverse direction same as that on the
base height D of the airfoil. The domain size for 3D case in
transverse direction is 3 times the base height D of the airfoil as
shown in Figure 9. The free-flow grid has coarse and fine
variant to study the mesh influence on the flow as shown in
Figure 10 and 11.
4 Copyright © 2015 by GKN Aerospace Sweden
Figure 9. 3D grid for NACA 64-621.
Figure 10. Coarse grid for NACA 64-621.
The fine mesh has thrice as many nodes as coarse mesh on
base height. As steady state simulation does not require higher
mesh resolution, coarse grid is used to simulate the steady state
SST turbulence model.
Figure 11. Fine grid for NACA 64-621.
2.3.2 GKN TET AIRFOIL
The simulation conditions for GKN TET airfoil are same
as that of water tunnel experiment. Hence the fluid domain size
in the simulation is same as water tunnel. A typical grid for
TET airfoil is as shown in Figure 12.
Figure 12. Typical grid for symmetric GKN TET airfoil.
To study the influence of mesh, the water tunnel simulation
is run with coarse and fine mesh as shown in Figure 13 and 14.
Figure 13. Coarse grid for GKN TET.
Figure 14. Fine grid for GKN TET.
2.4 SIMULATION
All the simulations are run on ANSYS CFX 15 solver.
Initial prediction of Cpb is done using SST steady state
turbulence model and the order of error when compared to the
experimental value is estimated. Further, Cp and Cpb predictions
5 Copyright © 2015 by GKN Aerospace Sweden
are done using SAS SST unstable turbulence model and
validated with experimental results.
The boundary conditions for both 2D and 3D NACA test
case are shown in Table 1. NACA test case simulations are run
using air at 25º C for free-flow and blockage grid.
Table 1. Boundary condition for NACA test case.
Boundary wall Boundary condition
Airfoil No-slip wall
Side walls Translational Periodicity
Top and Bottom walls No-slip wall
Inlet 16 m/s
Re 1 000 000
The boundary conditions for GKN TET airfoil simulation
are shown in Table 2. Simulation boundary conditions and
domain dimensions are similar to water tunnel with water as the
fluid model and no-slip walls surfaces as shown in Figure 15.
The yellow marks on airfoil surface are the monitor points
placed exactly on the same position as the pressure probes in
the experimental setup.
Table 2. Boundary condition for GKN TET airfoil.
Boundary wall Boundary condition
Airfoil No-slip wall
Side walls No-slip wall
Top and Bottom walls No-slip wall
Re 750 000
Figure 15. Simulation setup for GKN TET.
SAS SST unstable simulations are run until the flow
parameters in the airfoil wake are having a sustained periodic
variation (or oscillating constantly with time). To get a good
estimate of flow parameters, simulations are run for about 20
vortex shedding cycles. The expected value of shedding
frequency f is determined by assuming St = 0.2 and the base
height D of NACA test case and GKN TET airfoil in
Equation 8.
u
Df
St

 (8)
Time average values of Cp and Cpb for SAS SST unstable
simulations are compared to experimental results.
2.5 TIME AVERAGE
In case of unsteady wake flow Cp and Cpb values in the
wake are periodically varying. Therefore the time average value
of Cp and Cpb are used for analysis and validation. The time
average value fave for time varying function f(t) taken over a
time period of T is given by Equation 9.
dttf
T
fave  )(
1
(9)
3. DESCRIPTION OF EXPERIMENT
The experimental data for GKN TET airfoil are obtained
from water tunnel at GKN Aerospace Sweden. The
experimental rig with GKN TET airfoil, wake vortices and
pressure probes on the airfoil surface is shown in Figure 16.
Figure 16. Experimental setup of GKN TET airfoil.
Pressure probes on the upper surface and the base reads the
pressure distribution on the airfoil surface and base
respectively. The experimental Strouhal number and flow speed
is determined by splitting the video into several frames and
following the water bubbles and vortex pattern [7]. The
experimental Cpb and St is found to be -0.47 and 0.25
respectively.
4. RESULTS AND DISCUSSION
Both 2D and 3D simulations have shown interesting
results. The following section will present the simulation results
with relevant discussions.
4.1 NACA 64-621 TEST CASE
4.1.1 SST 2D STEADY SIMULATION
The velocity contours for 2D SST Steady simulation are
shown in Figure 17, 18 and 19 for coarse, fine and boxed mesh
respectively.
6 Copyright © 2015 by GKN Aerospace Sweden
Figure 17. Velocity contour for NACA 64-621 2D
SST steady simulation with coarse mesh.
Figure 18. Velocity contour for NACA 64-621 2D
SST steady simulation with fine mesh.
Figure 19. Velocity contour for NACA 64-621 2D
SST steady simulation with boxed mesh.
It can be seen from the Figure 17 and 18 that the velocity
contours for coarse and fine looks alike. However, the velocity
contours for boxed mesh shows the boundary wall influence on
the flow. The boundary walls are sufficiently far in case of
coarse and fine mesh. Hence it can be called free-flow
condition or essentially blockage free.
As mentioned in earlier section, the flow in the boxed
mesh has 10% blockage. Therefore the flow experiences drop
in the pressure and increase in velocity as it flows over the
airfoil. The blockage and the pressure drop is schematically
represented in Figure 20.
Figure 20. Effect of 10% blockage in boxed mesh.
The Cp distribution along the axis of the NACA 64-621
airfoil is shown in Figure 21. It can be clearly seen that the
pressure drops and recovers along the flow with higher pressure
drop in case of boxed mesh compared to coarse and fine mesh.
Figure 21. Cp distribution for NACA 64-621 2D SST
steady simulation.
Table 3. Cpb value for coarse, fine and boxed mesh.
Mesh type Cpb
Coarse mesh -0.0389
Fine mesh -0.0349
Boxed mesh -0.1824
The Cpb value for the 2D SST steady simulation for NACA
64-621 airfoil is shown in Table 3. It can be seen that the
difference between Cpb value coarse and fine mesh is negligible
compared to the order of magnitude of experimental Cpb value
[4] which is -0.21. Therefore, coarse mesh is sufficient to
investigate the problem.
Using the Cpb values of experiment and free-flow
simulation, the Cpb value for boxed mesh can be theoretically
predicted using equation 10 (notations can be related to Figure
5 for better understanding) [8]. As the Cpb in case of boxed
mesh is expected to be lesser than the free-flow case, first term
7 Copyright © 2015 by GKN Aerospace Sweden
in equation 10 represents the Cpb loss due to the blockage and
the second term represents the Cpb loss factor obtained from the
experiment [4].
2
1
(exp)
2
1
)( 1 





















in
pb
in
boxpb
u
u
C
u
u
C (10)
The theoretical prediction value of Cpb for boxed mesh case
using equation 10 is -0.25 which is less than the Cpb value for
boxed simulation which is -0.18. It’s seen that the simulation
predicts higher base pressure and hence under-predicts drag.
Since the difference between the Cpb value for experiment
and simulation for free-flow case is ∆Cpb= 0.17, we see that the
2D SST steady simulation under-predicts the base pressure and
hence the drag for both free-flow and boxed mesh.
4.1.2 SAS 2D UNSTEADY SIMULATION
As we saw in the previous section, SST steady simulation
largely under-predict the drag. Therefore, NACA 64-621
profile is simulated using SAS unsteady turbulence model with
the same 2D coarse and fine free-flow mesh.
Typical velocity contour for SAS 2D unsteady simulation
is shown in Figure 22 and 23. The instantaneous wake vortex
street is seen in Figure 22 and the time averaged velocity
contour is seen in Figure 23.
Figure 22. Velocity contour for SAS 2D NACA case.
Figure 23. Time average velocity contour for SAS 2D
NACA case.
It is clearly evident from the figure that SAS model is able
to resolve the vortex for the given time-step and Reynolds
number. The Cpb value for coarse and fine mesh in case of SAS
simulation is shown in Table 4 and the Strouhal number is 0.24
for both mesh.
Table 3. Cpb value for coarse and fine mesh using SAS.
Mesh type Cpb
Coarse mesh -0.4605
Fine mesh -0.5639
The Cpb in case of SAS unsteady is lower than SST steady
simulation. However that wake of the SST is longer than SAS
as shown in Figure 24. Therefore, with a lower value of Cpb,
SAS over-predicts the drag due to wake vortices.
SAS Simulation SST Simulation
Figure 24. Wake comparison of time average
velocity contour.
The 2D SAS simulation over-predicts drag because the
wake vortices are confined to 2D and hence are not allowed to
breakdown in space. It can also be seen that the Cpb for fine
mesh is lower compared to coarse mesh. This is because the
vortices are more resolved and hence sheds much faster as it is
confined in 2D space.
From the SST steady and SAS unsteady simulations, we
get a upper and lower limit for the Cpb prediction as shown in
Table 4 and gives a roadmap to use the SAS model in the best
possible way to predict the Cpb within the acceptable range.
Table 4. Cpb limit for free-flow mesh.
Simulation type Cpb
SST steady simulation -0.0389
Experimental -0.21
SAS unsteady simulation -0.4605
8 Copyright © 2015 by GKN Aerospace Sweden
4.1.2A MESH SENSITIVITY STUDY
The vortices breakdown soon after shedding 6-7 vortices as
seen in Figure 22 and might have an effect on Cpb. This was
verified by having much finer mesh in the wake as shown in
Figure 25 and the found no influence on Cpb, confirming that
the vortex breakdown point on the coarse free-flow mesh is
sufficiently far from the airfoil base. Therefore, the coarse free-
flow mesh does a fairly good prediction.
Figure 25. Finer mesh in the wake.
4.1.3 SAS 3D UNSTEADY SIMULATION
After estimating the upper and lower limit of Cpb, the
coarse and fine mesh (or free-flow case) is essentially made 3D
by increasing the width of the domain, that is, by having the
length and mesh density of the domain in transverse direction
to the flow equal to three times the base height of the airfoil, as
mentioned in earlier section. By having a 3D mesh, wake
vortices are expected to resolve in 3D space and hence
predicting better Cpb value.
A typical velocity contour for SAS 3D simulation is shown
in Figure 26. In case of 3D mesh, the velocity in transverse
direction is significantly high as shown in Figure 27. This
confirms that wake vortices are resolved in 3D space.
Figure 26. Velocity contour for SAS 3D NACA case.
Figure 27. Transverse velocity contour for SAS 3D.
The Cpb in this case is -0.28 which is closer to the
experimental value of -0.21. This infers that by allowing the
vortices to resolve in 3D space SAS turbulence model predicts
the Cpb better and closer to the experimental value. The 3D
vortices can be further visualized in Figure 28 showing the rear
view of the flow domain.
Figure 28. 3D vortices in SAS 3D NACA
simulation.
Although the Cpb value is getting closer to experimental
value by increasing the flow domain in transverse direction, the
variation of Cpb with simulation time shows a sub harmonic
frequencies as seen in Figure 29. However, this effect may
seem to occur due to mesh being coarse in the wake, it needs to
be investigated further.
9 Copyright © 2015 by GKN Aerospace Sweden
Figure 29. Sub-harmonic variation of Cpb for SAS 3D
4.2 GKN TET AIRFOIL
Unsteady simulation of GKN TET airfoil with mesh
dimensions same as water tunnel test rig described in earlier
section and using SAS turbulence model gives a typical wake
vortices shown in Figure 29. It can also be seen from Figure 30
that the vortices are three dimensional and the transverse
velocity is same as the domain inlet velocity.
Figure 29. Velocity contour for GKN TET airfoil.
Figure 30. Transverse velocity contour for GKN TET
airfoil.
Further investigation of GKN TET SAS simulation shows
a bow pattern in the wake when visualizing the vertical velocity
component as shown in Figure 31. The bow patter may be due
to the interaction of vortices with the end wall of the flow
domain. As mentioned earlier, the walls of the mesh is made of
no slip walls to replicate the same flow condition as in water
tunnel experiment. Therefore that end walls of the domain may
cause the near wall vortices to slow down compared to the
vortices in the middle section and hence causing the bow patter.
However, it could be studied further for better understanding of
the phenomenon.
Figure 31. Bow pattern seen in vertical velocity
component.
GKN TET airfoil was also analyzed using a coarse and fine
mesh. The SST steady simulation of course mesh gives Cpb of
-0.25 whereas SAS unsteady simulation gives -0.37, both of
which are far from the experimental value of -0.47. However
SAS simulation of fine mesh gives -0.46 which effectively is
same as the experimental Cpb.
4.2.1 VALIDATION DATA
The CFD simulation and analysis of GKN TET airfoil are
validated with the experiment results. Since the objective is to
asses the Cp and Cpb prediction capability of SST and SAS
turbulence models, the Cp and Cpb distribution along the airfoil
for simulation is compared with the experimental values as
shown in Figure 32. It can be seen that SAS simulation curve
matches well with SST simulation curve till the mid-point of
airfoil and later follows the experimental curve. Although there
is a slight difference in the SAS and experimental Cp
distribution, it is well in the acceptable range in an engineering
sense. Whereas SST simulation is way too far from the
experimental results near the trailing edge and hence it under-
predicts the drag.
10 Copyright © 2015 by GKN Aerospace Sweden
Figure 32. Cp distribution for CFD and Experiment.
Comparing the Cp distribution across the base of the airfoil
as shown in Figure 33, which is nothing but Cpb. It can be seen
that SAS curve is symmetric as expected and matches quite
well with the experimental curve only in the left half. This is
because the experimental curve is asymmetric which is
unexpected and unexplained at the moment. Effective the right
half of the experimental curve should have the same value as
the left as seen in case of SAS curve. It is not the case maybe
due to error in the experimental setup or pressure reading
probe. SST model under-predicts the drag and hence not
suitable for predicting the flow parameter in the presence of
wake vortices.
Figure 33. Cpb distribution across the base for CFD
and Experiment.
5. CONCLUSIONS
The GKN TET airfoil considered in the project was
analyzed by using SST and SAS turbulence model, and NACA
64-621 as the test case with fairly good mesh resolution. CFD
prediction for various wake mesh resolution was studied and
found that SST model under-predicts the drag on the airfoil and
the SAS model does a good prediction within the acceptable
error. The time-steps of 300 per cycle of vortex shedding
allows vortices to resolve well for the given Re. The value of
St. is 0.24 which matches well with the experiment value.
The total simulation time to get a considerable vortex
shedding cycles using SAS turbulence model for GKN TET
airfoil is about a week. Therefore, it can be concluded that the
modern day CFD SAS model does a good job in predicting Cp
in a flow involving wake vortices due to blunt trailing edge
with a simulation time of 1 week. Although SAS may seem
expensive in terms of computer capacity, one week is fairly
acceptable time frame for an engineering project involving
CFD analysis of TET airfoils.
6. SCOPE FOR FUTURE WORK
The simulations in this project are run using fairly
acceptable mesh resolution and time-step. Although the mesh
resolution and time-step seem to give a good prediction using
SAS model, further studies could be made by having a different
mesh resolution and topology with optimized time-steps.
The end wall effect seen in Figure 31 should be
investigated further to get better understanding of wake vortices
resolved by SAS model.
ACKNOWLEDGMENTS
I would like to thank my thesis supervisors Hans
Martensson and Lars Ellbrant at GKN for their kind support
during the project. I would also like to thank Arthur Rizzi who
is my thesis examiner at KTH for his time and support.
REFERENCES
[1] Van Dam, C. P., 2010, “Thick Airfoil with Blunt Trailing
Edge for Wind Turbine Blades”, ASME Turbo Expo 2010,
Paper GT2010-23786.
[2] Van Dam, C. P., 2009, “Blade Aerodynamics – Passive
and Active Load Control for Wind Turbine Blades”, Dept.
of Mechanical Engineering, University of California,
Davis, Lecture.
[3] Stone, Christopher, Barone M.,Lynch C. E., Marilyn J.,
Smith, 2009, “A Computational Study of the
Aerodynamics and Aeroacoustics of a Flatback Airfoil
Using Hybrid RANS-LES”, Proc. of 47th AIAA
Aerospace Sciences Meeting Including The New Horizons
Forum and Aerospace Exposition, Orlando, Florida. 273rd
ed. AIAA, 2009. Print.
[4] Law, S.P.,Gregorek G.M., 1987, “Wind Tunnel Evaluation
of a Truncated NACA 64-621 Airfoil for Wind Turbine
Applications”, DOE/NASA/0330-2 NASA CR-180803.
[5] Menter, F. R. (August 1994), "Two-Equation Eddy-
Viscosity Turbulence Models for Engineering
Applications", AIAA Journal 32 (8): 1598–1605,
Bibcode:1994AIAAJ.32.1598M
[6] Egorov Y., Menter F., “Development and application of
SST-SAS turbulence model in the DESIDER project”,
ANSYS Germany, ppt.
[7] Johansson U., “Water tunnel test of truncated airfoil”,
VOLS: 10209642, GKN Aerospace Sweden.
[8] Martensson H., VOLS: 10205671, GKN Aerospace
Sweden.
-1.40
-1.20
-1.00
-0.80
-0.60
-0.40
-0.20
0.00
0.00 0.50 1.00 1.50
X/C
EXP CFD SST CFD SAS
-0.60
-0.50
-0.40
-0.30
-0.20
-0.10
0.00
-150 -100 -50 0 50 100 150
ACROSS THE AIRFOIL BASE
EXP CFD SST CFD SAS

Mais conteúdo relacionado

Mais procurados

Morphological model of the river rhine branches from the concept to the opera...
Morphological model of the river rhine branches from the concept to the opera...Morphological model of the river rhine branches from the concept to the opera...
Morphological model of the river rhine branches from the concept to the opera...Deltares
 
Computational Fluid Dynamics for Aerodynamics
Computational Fluid Dynamics for AerodynamicsComputational Fluid Dynamics for Aerodynamics
Computational Fluid Dynamics for AerodynamicsIRJET Journal
 
Studies on impact of inlet viscosity ratio, decay rate & length scales in a c...
Studies on impact of inlet viscosity ratio, decay rate & length scales in a c...Studies on impact of inlet viscosity ratio, decay rate & length scales in a c...
Studies on impact of inlet viscosity ratio, decay rate & length scales in a c...QuEST Global
 
Computation of Hydrodynamic Characteristics of Ships using CFD
Computation of Hydrodynamic Characteristics of Ships using CFDComputation of Hydrodynamic Characteristics of Ships using CFD
Computation of Hydrodynamic Characteristics of Ships using CFDNabila Naz
 
Final-presentation-KTH-RedQual
Final-presentation-KTH-RedQualFinal-presentation-KTH-RedQual
Final-presentation-KTH-RedQualDejan Koren
 
An introduction to abaqus cfd
An introduction to abaqus cfdAn introduction to abaqus cfd
An introduction to abaqus cfdAhmadreza Aminian
 
CFD and Artificial Neural Networks Analysis of Plane Sudden Expansion Flows
CFD and Artificial Neural Networks Analysis of Plane Sudden Expansion FlowsCFD and Artificial Neural Networks Analysis of Plane Sudden Expansion Flows
CFD and Artificial Neural Networks Analysis of Plane Sudden Expansion FlowsCSCJournals
 
15 june 7 structural_modeling_2016_distribution_klymshyn
15 june 7 structural_modeling_2016_distribution_klymshyn15 june 7 structural_modeling_2016_distribution_klymshyn
15 june 7 structural_modeling_2016_distribution_klymshynleann_mays
 
Design of pipe network
Design of pipe networkDesign of pipe network
Design of pipe networkManoj Mota
 
LES Analysis on Confined Swirling Flow in a Gas Turbine Swirl Burner
LES Analysis  on Confined Swirling Flow in a Gas Turbine Swirl BurnerLES Analysis  on Confined Swirling Flow in a Gas Turbine Swirl Burner
LES Analysis on Confined Swirling Flow in a Gas Turbine Swirl BurnerROSHAN SAH
 
Question and answers webinar hydrodynamic modeling on the northwest european ...
Question and answers webinar hydrodynamic modeling on the northwest european ...Question and answers webinar hydrodynamic modeling on the northwest european ...
Question and answers webinar hydrodynamic modeling on the northwest european ...Deltares
 
Reservoir connectivity analysis_with_streamline_sim_nov_2010_v2
Reservoir connectivity analysis_with_streamline_sim_nov_2010_v2Reservoir connectivity analysis_with_streamline_sim_nov_2010_v2
Reservoir connectivity analysis_with_streamline_sim_nov_2010_v2Arif Khan
 
Computational Fluid Dynamics (CFD)
Computational Fluid Dynamics (CFD)Computational Fluid Dynamics (CFD)
Computational Fluid Dynamics (CFD)Taani Saxena
 

Mais procurados (19)

Hydrostatics and stability
Hydrostatics and stabilityHydrostatics and stability
Hydrostatics and stability
 
Morphological model of the river rhine branches from the concept to the opera...
Morphological model of the river rhine branches from the concept to the opera...Morphological model of the river rhine branches from the concept to the opera...
Morphological model of the river rhine branches from the concept to the opera...
 
ADNOC_Simulation_Challenges
ADNOC_Simulation_ChallengesADNOC_Simulation_Challenges
ADNOC_Simulation_Challenges
 
Computational Fluid Dynamics for Aerodynamics
Computational Fluid Dynamics for AerodynamicsComputational Fluid Dynamics for Aerodynamics
Computational Fluid Dynamics for Aerodynamics
 
dighe (3)
dighe (3)dighe (3)
dighe (3)
 
Studies on impact of inlet viscosity ratio, decay rate & length scales in a c...
Studies on impact of inlet viscosity ratio, decay rate & length scales in a c...Studies on impact of inlet viscosity ratio, decay rate & length scales in a c...
Studies on impact of inlet viscosity ratio, decay rate & length scales in a c...
 
Computation of Hydrodynamic Characteristics of Ships using CFD
Computation of Hydrodynamic Characteristics of Ships using CFDComputation of Hydrodynamic Characteristics of Ships using CFD
Computation of Hydrodynamic Characteristics of Ships using CFD
 
Example_Aerodynamics
Example_AerodynamicsExample_Aerodynamics
Example_Aerodynamics
 
The naca airfoil series
The naca airfoil seriesThe naca airfoil series
The naca airfoil series
 
Final-presentation-KTH-RedQual
Final-presentation-KTH-RedQualFinal-presentation-KTH-RedQual
Final-presentation-KTH-RedQual
 
An introduction to abaqus cfd
An introduction to abaqus cfdAn introduction to abaqus cfd
An introduction to abaqus cfd
 
CFD and Artificial Neural Networks Analysis of Plane Sudden Expansion Flows
CFD and Artificial Neural Networks Analysis of Plane Sudden Expansion FlowsCFD and Artificial Neural Networks Analysis of Plane Sudden Expansion Flows
CFD and Artificial Neural Networks Analysis of Plane Sudden Expansion Flows
 
15 june 7 structural_modeling_2016_distribution_klymshyn
15 june 7 structural_modeling_2016_distribution_klymshyn15 june 7 structural_modeling_2016_distribution_klymshyn
15 june 7 structural_modeling_2016_distribution_klymshyn
 
Design of pipe network
Design of pipe networkDesign of pipe network
Design of pipe network
 
LES Analysis on Confined Swirling Flow in a Gas Turbine Swirl Burner
LES Analysis  on Confined Swirling Flow in a Gas Turbine Swirl BurnerLES Analysis  on Confined Swirling Flow in a Gas Turbine Swirl Burner
LES Analysis on Confined Swirling Flow in a Gas Turbine Swirl Burner
 
Question and answers webinar hydrodynamic modeling on the northwest european ...
Question and answers webinar hydrodynamic modeling on the northwest european ...Question and answers webinar hydrodynamic modeling on the northwest european ...
Question and answers webinar hydrodynamic modeling on the northwest european ...
 
Reservoir connectivity analysis_with_streamline_sim_nov_2010_v2
Reservoir connectivity analysis_with_streamline_sim_nov_2010_v2Reservoir connectivity analysis_with_streamline_sim_nov_2010_v2
Reservoir connectivity analysis_with_streamline_sim_nov_2010_v2
 
E121 gt2014 26029
E121 gt2014 26029E121 gt2014 26029
E121 gt2014 26029
 
Computational Fluid Dynamics (CFD)
Computational Fluid Dynamics (CFD)Computational Fluid Dynamics (CFD)
Computational Fluid Dynamics (CFD)
 

Destaque

uma cv - Copy
uma cv - Copyuma cv - Copy
uma cv - CopyUman Arif
 
Price List Grand Kamala Lagoon, Emerald north
Price List Grand Kamala Lagoon, Emerald northPrice List Grand Kamala Lagoon, Emerald north
Price List Grand Kamala Lagoon, Emerald northHermanto Piliang
 
Integrated Delivery System (IDS) and the Future of the Health Care
Integrated Delivery System (IDS) and the Future of the Health Care     Integrated Delivery System (IDS) and the Future of the Health Care
Integrated Delivery System (IDS) and the Future of the Health Care Tunisia Ismalia Evans. Al-Salahuddin
 

Destaque (19)

uma cv - Copy
uma cv - Copyuma cv - Copy
uma cv - Copy
 
Coral reefs pwp
Coral reefs pwpCoral reefs pwp
Coral reefs pwp
 
CV JS new
CV JS newCV JS new
CV JS new
 
Katherine Santiago resume
Katherine Santiago resumeKatherine Santiago resume
Katherine Santiago resume
 
CFD analysis of an Airfoil
CFD analysis of an AirfoilCFD analysis of an Airfoil
CFD analysis of an Airfoil
 
THINK HOLISTIC CUISINE CATERING MENU
THINK HOLISTIC CUISINE CATERING MENU THINK HOLISTIC CUISINE CATERING MENU
THINK HOLISTIC CUISINE CATERING MENU
 
The role_of_stakeholder_trust
 The role_of_stakeholder_trust The role_of_stakeholder_trust
The role_of_stakeholder_trust
 
ORGANIZATIONAL CHANGE
ORGANIZATIONAL CHANGEORGANIZATIONAL CHANGE
ORGANIZATIONAL CHANGE
 
Price List Grand Kamala Lagoon, Emerald north
Price List Grand Kamala Lagoon, Emerald northPrice List Grand Kamala Lagoon, Emerald north
Price List Grand Kamala Lagoon, Emerald north
 
Think holistic cuisine
Think holistic cuisineThink holistic cuisine
Think holistic cuisine
 
The Chakra Food Pyramid
The Chakra Food PyramidThe Chakra Food Pyramid
The Chakra Food Pyramid
 
Organizational staffing for contra costa county
Organizational staffing for contra costa countyOrganizational staffing for contra costa county
Organizational staffing for contra costa county
 
The Chakra Food Pyramid
The Chakra Food PyramidThe Chakra Food Pyramid
The Chakra Food Pyramid
 
A Examination and Discussion-Ayurveda
A Examination and Discussion-Ayurveda A Examination and Discussion-Ayurveda
A Examination and Discussion-Ayurveda
 
Linea del tiempo
Linea del tiempoLinea del tiempo
Linea del tiempo
 
THE ROLE OF STAKEHOLDER
THE ROLE OF STAKEHOLDERTHE ROLE OF STAKEHOLDER
THE ROLE OF STAKEHOLDER
 
Distribution of health care
Distribution of health careDistribution of health care
Distribution of health care
 
Integrated Delivery System (IDS) and the Future of the Health Care
Integrated Delivery System (IDS) and the Future of the Health Care     Integrated Delivery System (IDS) and the Future of the Health Care
Integrated Delivery System (IDS) and the Future of the Health Care
 
The role_of_stakeholder_trust
 The role_of_stakeholder_trust The role_of_stakeholder_trust
The role_of_stakeholder_trust
 

Semelhante a Master_Thesis_Koushik

Determination of shock losses and pressure losses in ug mine openings (1)
Determination of shock losses and pressure losses in ug mine openings (1)Determination of shock losses and pressure losses in ug mine openings (1)
Determination of shock losses and pressure losses in ug mine openings (1)Safdar Ali
 
Performance Analysis of savonius hydro turbine using CFD simulation
Performance Analysis of savonius hydro turbine using CFD simulationPerformance Analysis of savonius hydro turbine using CFD simulation
Performance Analysis of savonius hydro turbine using CFD simulationIRJET Journal
 
Airfoil Design for Mars Aircraft Using Modified PARSEC Geometry Representation
Airfoil Design for Mars Aircraft Using Modified PARSEC Geometry RepresentationAirfoil Design for Mars Aircraft Using Modified PARSEC Geometry Representation
Airfoil Design for Mars Aircraft Using Modified PARSEC Geometry RepresentationMasahiro Kanazaki
 
CFD Analysis for Computing Drag force on Various types of blades for Vertical...
CFD Analysis for Computing Drag force on Various types of blades for Vertical...CFD Analysis for Computing Drag force on Various types of blades for Vertical...
CFD Analysis for Computing Drag force on Various types of blades for Vertical...IRJET Journal
 
Atmospheric turbulent layer simulation for cfd unsteady inlet conditions
Atmospheric turbulent layer simulation for cfd unsteady inlet conditionsAtmospheric turbulent layer simulation for cfd unsteady inlet conditions
Atmospheric turbulent layer simulation for cfd unsteady inlet conditionsStephane Meteodyn
 
On The Form Factor Prediction Of A Displacement Type Vessel: JBC Case
On The Form Factor Prediction Of A Displacement Type Vessel: JBC CaseOn The Form Factor Prediction Of A Displacement Type Vessel: JBC Case
On The Form Factor Prediction Of A Displacement Type Vessel: JBC CaseIsmail Topal
 
Full paper jbc icame2016
Full paper jbc icame2016Full paper jbc icame2016
Full paper jbc icame2016Uğur Can
 
Numerical Investigation of Turbulent Flow over a Rotating Circular Cylinder u...
Numerical Investigation of Turbulent Flow over a Rotating Circular Cylinder u...Numerical Investigation of Turbulent Flow over a Rotating Circular Cylinder u...
Numerical Investigation of Turbulent Flow over a Rotating Circular Cylinder u...IJERA Editor
 
Aerodynamic and Acoustic Parameters of a Coandã Flow – a Numerical Investigation
Aerodynamic and Acoustic Parameters of a Coandã Flow – a Numerical InvestigationAerodynamic and Acoustic Parameters of a Coandã Flow – a Numerical Investigation
Aerodynamic and Acoustic Parameters of a Coandã Flow – a Numerical Investigationdrboon
 
Optimization of Closure Law of Guide Vanes for an Operational Hydropower Plan...
Optimization of Closure Law of Guide Vanes for an Operational Hydropower Plan...Optimization of Closure Law of Guide Vanes for an Operational Hydropower Plan...
Optimization of Closure Law of Guide Vanes for an Operational Hydropower Plan...Dr. Amarjeet Singh
 
Investigation of buffet control on transonic airfoil by tangential jet blowing
Investigation of buffet control on transonic airfoil by tangential jet blowingInvestigation of buffet control on transonic airfoil by tangential jet blowing
Investigation of buffet control on transonic airfoil by tangential jet blowingМурад Брутян
 
Study of different contraction design of wind tunnel for better performance b...
Study of different contraction design of wind tunnel for better performance b...Study of different contraction design of wind tunnel for better performance b...
Study of different contraction design of wind tunnel for better performance b...IRJET Journal
 
Analysis Of 3C-Sic Double Implanted MOSFET With Gaussian Profile Doping In Th...
Analysis Of 3C-Sic Double Implanted MOSFET With Gaussian Profile Doping In Th...Analysis Of 3C-Sic Double Implanted MOSFET With Gaussian Profile Doping In Th...
Analysis Of 3C-Sic Double Implanted MOSFET With Gaussian Profile Doping In Th...IJRES Journal
 
Effect of spikes integrated to airfoil at supersonic speed
Effect of spikes integrated to airfoil at supersonic speedEffect of spikes integrated to airfoil at supersonic speed
Effect of spikes integrated to airfoil at supersonic speedeSAT Journals
 

Semelhante a Master_Thesis_Koushik (20)

Wason_Mark
Wason_MarkWason_Mark
Wason_Mark
 
cfd naca0012
cfd naca0012cfd naca0012
cfd naca0012
 
Determination of shock losses and pressure losses in ug mine openings (1)
Determination of shock losses and pressure losses in ug mine openings (1)Determination of shock losses and pressure losses in ug mine openings (1)
Determination of shock losses and pressure losses in ug mine openings (1)
 
Performance Analysis of savonius hydro turbine using CFD simulation
Performance Analysis of savonius hydro turbine using CFD simulationPerformance Analysis of savonius hydro turbine using CFD simulation
Performance Analysis of savonius hydro turbine using CFD simulation
 
cfd ahmed body
cfd ahmed bodycfd ahmed body
cfd ahmed body
 
Airfoil Design for Mars Aircraft Using Modified PARSEC Geometry Representation
Airfoil Design for Mars Aircraft Using Modified PARSEC Geometry RepresentationAirfoil Design for Mars Aircraft Using Modified PARSEC Geometry Representation
Airfoil Design for Mars Aircraft Using Modified PARSEC Geometry Representation
 
ASSIGNMENT
ASSIGNMENTASSIGNMENT
ASSIGNMENT
 
CFD Analysis for Computing Drag force on Various types of blades for Vertical...
CFD Analysis for Computing Drag force on Various types of blades for Vertical...CFD Analysis for Computing Drag force on Various types of blades for Vertical...
CFD Analysis for Computing Drag force on Various types of blades for Vertical...
 
Atmospheric turbulent layer simulation for cfd unsteady inlet conditions
Atmospheric turbulent layer simulation for cfd unsteady inlet conditionsAtmospheric turbulent layer simulation for cfd unsteady inlet conditions
Atmospheric turbulent layer simulation for cfd unsteady inlet conditions
 
On The Form Factor Prediction Of A Displacement Type Vessel: JBC Case
On The Form Factor Prediction Of A Displacement Type Vessel: JBC CaseOn The Form Factor Prediction Of A Displacement Type Vessel: JBC Case
On The Form Factor Prediction Of A Displacement Type Vessel: JBC Case
 
Full paper jbc icame2016
Full paper jbc icame2016Full paper jbc icame2016
Full paper jbc icame2016
 
Numerical Investigation of Turbulent Flow over a Rotating Circular Cylinder u...
Numerical Investigation of Turbulent Flow over a Rotating Circular Cylinder u...Numerical Investigation of Turbulent Flow over a Rotating Circular Cylinder u...
Numerical Investigation of Turbulent Flow over a Rotating Circular Cylinder u...
 
83
8383
83
 
Aerodynamic and Acoustic Parameters of a Coandã Flow – a Numerical Investigation
Aerodynamic and Acoustic Parameters of a Coandã Flow – a Numerical InvestigationAerodynamic and Acoustic Parameters of a Coandã Flow – a Numerical Investigation
Aerodynamic and Acoustic Parameters of a Coandã Flow – a Numerical Investigation
 
Optimization of Closure Law of Guide Vanes for an Operational Hydropower Plan...
Optimization of Closure Law of Guide Vanes for an Operational Hydropower Plan...Optimization of Closure Law of Guide Vanes for an Operational Hydropower Plan...
Optimization of Closure Law of Guide Vanes for an Operational Hydropower Plan...
 
Investigation of buffet control on transonic airfoil by tangential jet blowing
Investigation of buffet control on transonic airfoil by tangential jet blowingInvestigation of buffet control on transonic airfoil by tangential jet blowing
Investigation of buffet control on transonic airfoil by tangential jet blowing
 
Simulation of the Design of an Exhaust Silencer Stack by CFD
Simulation of the Design of an Exhaust Silencer Stack by CFDSimulation of the Design of an Exhaust Silencer Stack by CFD
Simulation of the Design of an Exhaust Silencer Stack by CFD
 
Study of different contraction design of wind tunnel for better performance b...
Study of different contraction design of wind tunnel for better performance b...Study of different contraction design of wind tunnel for better performance b...
Study of different contraction design of wind tunnel for better performance b...
 
Analysis Of 3C-Sic Double Implanted MOSFET With Gaussian Profile Doping In Th...
Analysis Of 3C-Sic Double Implanted MOSFET With Gaussian Profile Doping In Th...Analysis Of 3C-Sic Double Implanted MOSFET With Gaussian Profile Doping In Th...
Analysis Of 3C-Sic Double Implanted MOSFET With Gaussian Profile Doping In Th...
 
Effect of spikes integrated to airfoil at supersonic speed
Effect of spikes integrated to airfoil at supersonic speedEffect of spikes integrated to airfoil at supersonic speed
Effect of spikes integrated to airfoil at supersonic speed
 

Master_Thesis_Koushik

  • 1. Master thesis report on VORTEX SHEDDING AND AERODYNAMIC DRAG ON TRUNCATED TRAILING EDGE AIRFOIL Conducted during February - June 2015 Submitted by: Koushik Bangalore Gangadharacharya Master of Science in Aerospace Engineering Royal Institute of Technology, Stockholm, Sweden Under the supervision of Hans Mårtensson&Lars Ellbrant GKN Aerospace, Trollhättan, Sweden Examiner: Prof. Arthur Rizzi Aeronautical and Vehicle Engineering Dept. Royal Institute of Technology, Stockholm, Sweden.
  • 2. 1 Copyright © 2015 by GKN Aerospace Sweden Master thesis report February – June 2015 VORTEX SHEDDING AND AERODYNAMIC DRAG ON TRUNCATED TRAILING EDGE AIRFOIL Koushik Bangalore Gangadharacharya Royal Institute of Technology SE-100 44 Stockholm, Sweden E-mail: kobg@kth.se ABSTRACT The thesis work content is to evaluate the use of more advanced turbulence models available in the ANSYS CFX software for aerodynamic calculations. In particular for flows over airfoils with thick trailing edges, the turbulence modeling is challenging to traditional methods, as both thin boundary layers as well as an unsteady wake needs to be well represented. This is done by using the standard SST and then performing unsteady computations using the more advanced unsteady SAS-SST model to get the relevant CFD results. By comparing to tests performed at GKN and results from literature the improvement could be assessed in terms of modeling quality and computational cost. The results presented give a good contribution to how the modeling of unsteady wakes can be improved and used for design purposes. KEY WORDS Computational fluid dynamics (CFD), unsteady aerodynamics, turbulence modeling, Reynolds number (Re), Strouhal number (St), coefficient of pressure. NOMENCLATURE (SI UNITS) Cp Coefficient of pressure Cpb Coefficient of pressure at airfoil base c Chord length of the airfoil D Base height of the airfoil f Frequency of vortex shedding k Von Karman length scale LES Large Eddy Simulation RANS Reynolds Averaged Navier Stokes Re Reynolds number SAS Scale Adaptive Simulation SST Shear Stress Transport St Strouhal number S Strain rate TET Truncated tailing edge u,U Velocity URANS Unsteady Reynolds Averaged Navier Stokes Δp pin- pout φ Loss coefficient ρ Density µa Viscosity of air at 25º C µw Viscosity of water at 20º C p1 Static pressure 1. INTRODUCTION The modern day numerical CFD prediction tool is validated with experiment results for vortex shedding and drag prediction for the flow over truncated trailing edge (TET) airfoil (so-called flatback or thick trailing edge airfoil). As discussed in [1], RANS numerical simulation and experimental data of TET airfoil demonstrates significant improvement in subsonic lift characteristics compared to non-TET airfoil including higher maximum lift coefficients and less loss of lift due to premature boundary layer transition. TET airfoil also serves as viable configuration of airfoil, connecting the structural and manufacturing requirements for rotary turbine blades with acceptable aerodynamic performance. However, TET airfoils exhibit higher drag levels due to the low pressure region in the wake of thick tailing edge. The adverse pressure gradient allows vortices to form immediately after the trailing edge as shown in Figure 1. Figure 1. Vortex shedding at the blunt trailing edge [2].
  • 3. 2 Copyright © 2015 by GKN Aerospace Sweden Previous study of the drag on the TET airfoil by using RANS and LES numerical simulation suggests that 2D numerical simulations over-predicts the drag by nearly 100%. However, same trend is not shown in case of 3D simulations [3]. In this paper, flow over the blunt trailing edge airfoil NACA 64-621-TET as shown in Figure 2 is simulated using SST and SAS SST turbulence models on ANSYS CFX solver as a test case. The Cp distribution is determined, in particular the base pressure coefficient Cpb is estimated for effectively 2D and 3D cases of NACA airfoil. The 2D simulation results are then validated with effectively 2D wind tunnel experimental values conducted at Ohio State University, Ohio [4]. Figure 2. Dimensions of NACA 64-621 TET airfoil [4]. Using the results of NACA 64-621-TET airfoil the order of magnitude of error is determined. Further, same turbulence models are used to simulate the flow over GKN TET airfoil and the results are again validated with water tunnel experiment conducted at GKN Aerospace, Sweden. By doing so, validation is made whether unsteady SAS SST turbulence model can predict the drag and capture the wake vortices as a measure of Strouhal number (St) for the flow over TET airfoil to assess the efficiency and accuracy of the model. 2. METHODOLOGY 2.1 NUMERICAL METHODS The SST is a standard two-equation eddy viscosity turbulence model in CFD. It is expected to accurately predict the onset and the amount of flow separation under adverse pressure gradient. The flow separation at the flat face of the TET airfoil can be essentially related to the Cpb value as the adverse pressure gradient occurs at the base of the airfoil. SST model is a combination of k-ω and k-ε turbulence models such that the k-ω is used in the inner region of the boundary layer and switches to k-ε in the free shear flow [5]. SST turbulence model gives the steady state results for the flow. The SAS SST (or just SAS) is a hybrid model used to solve an unstable flow conditions considered in this paper. SAS is based on the introduction of Von Karman length-scale into the turbulence scale equation. In SAS model, unstable vortices in the wake of the airfoil are resolved based on Lνk shown in Equation 1 and Figure 3, which is governed by Von Karman length-scale, strain rate and square of velocity gradient tensor. Whereas in LES model, wake vortices are resolved based on grid size as shown in Figure 3. Therefore, SAS is expected have less grid influence compared to LES. At the same time, SAS model provides standard RANS capabilities in stable flow regions. These capabilities of SAS can be well utilized when the mesh resolution and the time-step is optimum for the considered flow conditions. U S kL k 2   (1) Figure 3. Resolved vortex comparison in SAS with LES [6]. 2.2 PREDICTION METHODS The drag due to pressure loss Δp for the flow over TET airfoil in a confined space as shown in Figure 4 is estimated by Equation 2 and hence the loss coefficient φ can be defined as shown in Equation 4. Figure 4. Flow domain. crossApD  (2) qACD baseD  (3) cross base D A A C q p    (4) An important flow parameter in analysis of blunt airfoil profile is Cp and Cpb as defined in Equation 5 and 6. Due to flow in a confined space, average pressure reduces at section-1 shown in Figure 5. Pressure drop is expected because of reduced flow area at section-1 due to presence of airfoil. Hence Cpb1 is defined in Equation 7.
  • 4. 3 Copyright © 2015 by GKN Aerospace Sweden inin in p PP PP C    0 (5) inin inbase pb PP PP C    0 (6) 10 1 1 PP PP C in base pb    (7) Figure 5. Flow domain with section-1. 2.3 MESH 2.3.1 NACA 64-621 TEST CASE Typical structured grid for TET airfoil is created using ICEM CFD as shown in Figure 5. It has a uniform rectangular grid in the wake, allowing the wake vortices to resolve. Figure 6. Structured grid for NACA 64-621. As mentioned before, 2D wind tunnel experiment results for NACA 64-621 TET airfoil is compared to CFD simulation in 2D and 3D as a test case. Relation between the Cpb for the free-flow and blockage is estimated by simulating the flow domain as shown in Figure 7 and 8. Figure 7. Free-flow case grid for NACA 64-621. The boundary walls in free-flow case are very far from the airfoil and are not expected to influence the flow. Whereas in blockage case, it is expected to have boundary wall influence from top and bottom walls as a result of which higher pressure drop is expected in the wake for blockage case compared to free-flow case. The blockage here is 10% of the flow area. Figure 8. Blockage case grid for NACA 64-621. The grid is effectively made 2D by having 2 cells in the transverse direction of the flow and the 3D grid is created by having node density in transverse direction same as that on the base height D of the airfoil. The domain size for 3D case in transverse direction is 3 times the base height D of the airfoil as shown in Figure 9. The free-flow grid has coarse and fine variant to study the mesh influence on the flow as shown in Figure 10 and 11.
  • 5. 4 Copyright © 2015 by GKN Aerospace Sweden Figure 9. 3D grid for NACA 64-621. Figure 10. Coarse grid for NACA 64-621. The fine mesh has thrice as many nodes as coarse mesh on base height. As steady state simulation does not require higher mesh resolution, coarse grid is used to simulate the steady state SST turbulence model. Figure 11. Fine grid for NACA 64-621. 2.3.2 GKN TET AIRFOIL The simulation conditions for GKN TET airfoil are same as that of water tunnel experiment. Hence the fluid domain size in the simulation is same as water tunnel. A typical grid for TET airfoil is as shown in Figure 12. Figure 12. Typical grid for symmetric GKN TET airfoil. To study the influence of mesh, the water tunnel simulation is run with coarse and fine mesh as shown in Figure 13 and 14. Figure 13. Coarse grid for GKN TET. Figure 14. Fine grid for GKN TET. 2.4 SIMULATION All the simulations are run on ANSYS CFX 15 solver. Initial prediction of Cpb is done using SST steady state turbulence model and the order of error when compared to the experimental value is estimated. Further, Cp and Cpb predictions
  • 6. 5 Copyright © 2015 by GKN Aerospace Sweden are done using SAS SST unstable turbulence model and validated with experimental results. The boundary conditions for both 2D and 3D NACA test case are shown in Table 1. NACA test case simulations are run using air at 25º C for free-flow and blockage grid. Table 1. Boundary condition for NACA test case. Boundary wall Boundary condition Airfoil No-slip wall Side walls Translational Periodicity Top and Bottom walls No-slip wall Inlet 16 m/s Re 1 000 000 The boundary conditions for GKN TET airfoil simulation are shown in Table 2. Simulation boundary conditions and domain dimensions are similar to water tunnel with water as the fluid model and no-slip walls surfaces as shown in Figure 15. The yellow marks on airfoil surface are the monitor points placed exactly on the same position as the pressure probes in the experimental setup. Table 2. Boundary condition for GKN TET airfoil. Boundary wall Boundary condition Airfoil No-slip wall Side walls No-slip wall Top and Bottom walls No-slip wall Re 750 000 Figure 15. Simulation setup for GKN TET. SAS SST unstable simulations are run until the flow parameters in the airfoil wake are having a sustained periodic variation (or oscillating constantly with time). To get a good estimate of flow parameters, simulations are run for about 20 vortex shedding cycles. The expected value of shedding frequency f is determined by assuming St = 0.2 and the base height D of NACA test case and GKN TET airfoil in Equation 8. u Df St   (8) Time average values of Cp and Cpb for SAS SST unstable simulations are compared to experimental results. 2.5 TIME AVERAGE In case of unsteady wake flow Cp and Cpb values in the wake are periodically varying. Therefore the time average value of Cp and Cpb are used for analysis and validation. The time average value fave for time varying function f(t) taken over a time period of T is given by Equation 9. dttf T fave  )( 1 (9) 3. DESCRIPTION OF EXPERIMENT The experimental data for GKN TET airfoil are obtained from water tunnel at GKN Aerospace Sweden. The experimental rig with GKN TET airfoil, wake vortices and pressure probes on the airfoil surface is shown in Figure 16. Figure 16. Experimental setup of GKN TET airfoil. Pressure probes on the upper surface and the base reads the pressure distribution on the airfoil surface and base respectively. The experimental Strouhal number and flow speed is determined by splitting the video into several frames and following the water bubbles and vortex pattern [7]. The experimental Cpb and St is found to be -0.47 and 0.25 respectively. 4. RESULTS AND DISCUSSION Both 2D and 3D simulations have shown interesting results. The following section will present the simulation results with relevant discussions. 4.1 NACA 64-621 TEST CASE 4.1.1 SST 2D STEADY SIMULATION The velocity contours for 2D SST Steady simulation are shown in Figure 17, 18 and 19 for coarse, fine and boxed mesh respectively.
  • 7. 6 Copyright © 2015 by GKN Aerospace Sweden Figure 17. Velocity contour for NACA 64-621 2D SST steady simulation with coarse mesh. Figure 18. Velocity contour for NACA 64-621 2D SST steady simulation with fine mesh. Figure 19. Velocity contour for NACA 64-621 2D SST steady simulation with boxed mesh. It can be seen from the Figure 17 and 18 that the velocity contours for coarse and fine looks alike. However, the velocity contours for boxed mesh shows the boundary wall influence on the flow. The boundary walls are sufficiently far in case of coarse and fine mesh. Hence it can be called free-flow condition or essentially blockage free. As mentioned in earlier section, the flow in the boxed mesh has 10% blockage. Therefore the flow experiences drop in the pressure and increase in velocity as it flows over the airfoil. The blockage and the pressure drop is schematically represented in Figure 20. Figure 20. Effect of 10% blockage in boxed mesh. The Cp distribution along the axis of the NACA 64-621 airfoil is shown in Figure 21. It can be clearly seen that the pressure drops and recovers along the flow with higher pressure drop in case of boxed mesh compared to coarse and fine mesh. Figure 21. Cp distribution for NACA 64-621 2D SST steady simulation. Table 3. Cpb value for coarse, fine and boxed mesh. Mesh type Cpb Coarse mesh -0.0389 Fine mesh -0.0349 Boxed mesh -0.1824 The Cpb value for the 2D SST steady simulation for NACA 64-621 airfoil is shown in Table 3. It can be seen that the difference between Cpb value coarse and fine mesh is negligible compared to the order of magnitude of experimental Cpb value [4] which is -0.21. Therefore, coarse mesh is sufficient to investigate the problem. Using the Cpb values of experiment and free-flow simulation, the Cpb value for boxed mesh can be theoretically predicted using equation 10 (notations can be related to Figure 5 for better understanding) [8]. As the Cpb in case of boxed mesh is expected to be lesser than the free-flow case, first term
  • 8. 7 Copyright © 2015 by GKN Aerospace Sweden in equation 10 represents the Cpb loss due to the blockage and the second term represents the Cpb loss factor obtained from the experiment [4]. 2 1 (exp) 2 1 )( 1                       in pb in boxpb u u C u u C (10) The theoretical prediction value of Cpb for boxed mesh case using equation 10 is -0.25 which is less than the Cpb value for boxed simulation which is -0.18. It’s seen that the simulation predicts higher base pressure and hence under-predicts drag. Since the difference between the Cpb value for experiment and simulation for free-flow case is ∆Cpb= 0.17, we see that the 2D SST steady simulation under-predicts the base pressure and hence the drag for both free-flow and boxed mesh. 4.1.2 SAS 2D UNSTEADY SIMULATION As we saw in the previous section, SST steady simulation largely under-predict the drag. Therefore, NACA 64-621 profile is simulated using SAS unsteady turbulence model with the same 2D coarse and fine free-flow mesh. Typical velocity contour for SAS 2D unsteady simulation is shown in Figure 22 and 23. The instantaneous wake vortex street is seen in Figure 22 and the time averaged velocity contour is seen in Figure 23. Figure 22. Velocity contour for SAS 2D NACA case. Figure 23. Time average velocity contour for SAS 2D NACA case. It is clearly evident from the figure that SAS model is able to resolve the vortex for the given time-step and Reynolds number. The Cpb value for coarse and fine mesh in case of SAS simulation is shown in Table 4 and the Strouhal number is 0.24 for both mesh. Table 3. Cpb value for coarse and fine mesh using SAS. Mesh type Cpb Coarse mesh -0.4605 Fine mesh -0.5639 The Cpb in case of SAS unsteady is lower than SST steady simulation. However that wake of the SST is longer than SAS as shown in Figure 24. Therefore, with a lower value of Cpb, SAS over-predicts the drag due to wake vortices. SAS Simulation SST Simulation Figure 24. Wake comparison of time average velocity contour. The 2D SAS simulation over-predicts drag because the wake vortices are confined to 2D and hence are not allowed to breakdown in space. It can also be seen that the Cpb for fine mesh is lower compared to coarse mesh. This is because the vortices are more resolved and hence sheds much faster as it is confined in 2D space. From the SST steady and SAS unsteady simulations, we get a upper and lower limit for the Cpb prediction as shown in Table 4 and gives a roadmap to use the SAS model in the best possible way to predict the Cpb within the acceptable range. Table 4. Cpb limit for free-flow mesh. Simulation type Cpb SST steady simulation -0.0389 Experimental -0.21 SAS unsteady simulation -0.4605
  • 9. 8 Copyright © 2015 by GKN Aerospace Sweden 4.1.2A MESH SENSITIVITY STUDY The vortices breakdown soon after shedding 6-7 vortices as seen in Figure 22 and might have an effect on Cpb. This was verified by having much finer mesh in the wake as shown in Figure 25 and the found no influence on Cpb, confirming that the vortex breakdown point on the coarse free-flow mesh is sufficiently far from the airfoil base. Therefore, the coarse free- flow mesh does a fairly good prediction. Figure 25. Finer mesh in the wake. 4.1.3 SAS 3D UNSTEADY SIMULATION After estimating the upper and lower limit of Cpb, the coarse and fine mesh (or free-flow case) is essentially made 3D by increasing the width of the domain, that is, by having the length and mesh density of the domain in transverse direction to the flow equal to three times the base height of the airfoil, as mentioned in earlier section. By having a 3D mesh, wake vortices are expected to resolve in 3D space and hence predicting better Cpb value. A typical velocity contour for SAS 3D simulation is shown in Figure 26. In case of 3D mesh, the velocity in transverse direction is significantly high as shown in Figure 27. This confirms that wake vortices are resolved in 3D space. Figure 26. Velocity contour for SAS 3D NACA case. Figure 27. Transverse velocity contour for SAS 3D. The Cpb in this case is -0.28 which is closer to the experimental value of -0.21. This infers that by allowing the vortices to resolve in 3D space SAS turbulence model predicts the Cpb better and closer to the experimental value. The 3D vortices can be further visualized in Figure 28 showing the rear view of the flow domain. Figure 28. 3D vortices in SAS 3D NACA simulation. Although the Cpb value is getting closer to experimental value by increasing the flow domain in transverse direction, the variation of Cpb with simulation time shows a sub harmonic frequencies as seen in Figure 29. However, this effect may seem to occur due to mesh being coarse in the wake, it needs to be investigated further.
  • 10. 9 Copyright © 2015 by GKN Aerospace Sweden Figure 29. Sub-harmonic variation of Cpb for SAS 3D 4.2 GKN TET AIRFOIL Unsteady simulation of GKN TET airfoil with mesh dimensions same as water tunnel test rig described in earlier section and using SAS turbulence model gives a typical wake vortices shown in Figure 29. It can also be seen from Figure 30 that the vortices are three dimensional and the transverse velocity is same as the domain inlet velocity. Figure 29. Velocity contour for GKN TET airfoil. Figure 30. Transverse velocity contour for GKN TET airfoil. Further investigation of GKN TET SAS simulation shows a bow pattern in the wake when visualizing the vertical velocity component as shown in Figure 31. The bow patter may be due to the interaction of vortices with the end wall of the flow domain. As mentioned earlier, the walls of the mesh is made of no slip walls to replicate the same flow condition as in water tunnel experiment. Therefore that end walls of the domain may cause the near wall vortices to slow down compared to the vortices in the middle section and hence causing the bow patter. However, it could be studied further for better understanding of the phenomenon. Figure 31. Bow pattern seen in vertical velocity component. GKN TET airfoil was also analyzed using a coarse and fine mesh. The SST steady simulation of course mesh gives Cpb of -0.25 whereas SAS unsteady simulation gives -0.37, both of which are far from the experimental value of -0.47. However SAS simulation of fine mesh gives -0.46 which effectively is same as the experimental Cpb. 4.2.1 VALIDATION DATA The CFD simulation and analysis of GKN TET airfoil are validated with the experiment results. Since the objective is to asses the Cp and Cpb prediction capability of SST and SAS turbulence models, the Cp and Cpb distribution along the airfoil for simulation is compared with the experimental values as shown in Figure 32. It can be seen that SAS simulation curve matches well with SST simulation curve till the mid-point of airfoil and later follows the experimental curve. Although there is a slight difference in the SAS and experimental Cp distribution, it is well in the acceptable range in an engineering sense. Whereas SST simulation is way too far from the experimental results near the trailing edge and hence it under- predicts the drag.
  • 11. 10 Copyright © 2015 by GKN Aerospace Sweden Figure 32. Cp distribution for CFD and Experiment. Comparing the Cp distribution across the base of the airfoil as shown in Figure 33, which is nothing but Cpb. It can be seen that SAS curve is symmetric as expected and matches quite well with the experimental curve only in the left half. This is because the experimental curve is asymmetric which is unexpected and unexplained at the moment. Effective the right half of the experimental curve should have the same value as the left as seen in case of SAS curve. It is not the case maybe due to error in the experimental setup or pressure reading probe. SST model under-predicts the drag and hence not suitable for predicting the flow parameter in the presence of wake vortices. Figure 33. Cpb distribution across the base for CFD and Experiment. 5. CONCLUSIONS The GKN TET airfoil considered in the project was analyzed by using SST and SAS turbulence model, and NACA 64-621 as the test case with fairly good mesh resolution. CFD prediction for various wake mesh resolution was studied and found that SST model under-predicts the drag on the airfoil and the SAS model does a good prediction within the acceptable error. The time-steps of 300 per cycle of vortex shedding allows vortices to resolve well for the given Re. The value of St. is 0.24 which matches well with the experiment value. The total simulation time to get a considerable vortex shedding cycles using SAS turbulence model for GKN TET airfoil is about a week. Therefore, it can be concluded that the modern day CFD SAS model does a good job in predicting Cp in a flow involving wake vortices due to blunt trailing edge with a simulation time of 1 week. Although SAS may seem expensive in terms of computer capacity, one week is fairly acceptable time frame for an engineering project involving CFD analysis of TET airfoils. 6. SCOPE FOR FUTURE WORK The simulations in this project are run using fairly acceptable mesh resolution and time-step. Although the mesh resolution and time-step seem to give a good prediction using SAS model, further studies could be made by having a different mesh resolution and topology with optimized time-steps. The end wall effect seen in Figure 31 should be investigated further to get better understanding of wake vortices resolved by SAS model. ACKNOWLEDGMENTS I would like to thank my thesis supervisors Hans Martensson and Lars Ellbrant at GKN for their kind support during the project. I would also like to thank Arthur Rizzi who is my thesis examiner at KTH for his time and support. REFERENCES [1] Van Dam, C. P., 2010, “Thick Airfoil with Blunt Trailing Edge for Wind Turbine Blades”, ASME Turbo Expo 2010, Paper GT2010-23786. [2] Van Dam, C. P., 2009, “Blade Aerodynamics – Passive and Active Load Control for Wind Turbine Blades”, Dept. of Mechanical Engineering, University of California, Davis, Lecture. [3] Stone, Christopher, Barone M.,Lynch C. E., Marilyn J., Smith, 2009, “A Computational Study of the Aerodynamics and Aeroacoustics of a Flatback Airfoil Using Hybrid RANS-LES”, Proc. of 47th AIAA Aerospace Sciences Meeting Including The New Horizons Forum and Aerospace Exposition, Orlando, Florida. 273rd ed. AIAA, 2009. Print. [4] Law, S.P.,Gregorek G.M., 1987, “Wind Tunnel Evaluation of a Truncated NACA 64-621 Airfoil for Wind Turbine Applications”, DOE/NASA/0330-2 NASA CR-180803. [5] Menter, F. R. (August 1994), "Two-Equation Eddy- Viscosity Turbulence Models for Engineering Applications", AIAA Journal 32 (8): 1598–1605, Bibcode:1994AIAAJ.32.1598M [6] Egorov Y., Menter F., “Development and application of SST-SAS turbulence model in the DESIDER project”, ANSYS Germany, ppt. [7] Johansson U., “Water tunnel test of truncated airfoil”, VOLS: 10209642, GKN Aerospace Sweden. [8] Martensson H., VOLS: 10205671, GKN Aerospace Sweden. -1.40 -1.20 -1.00 -0.80 -0.60 -0.40 -0.20 0.00 0.00 0.50 1.00 1.50 X/C EXP CFD SST CFD SAS -0.60 -0.50 -0.40 -0.30 -0.20 -0.10 0.00 -150 -100 -50 0 50 100 150 ACROSS THE AIRFOIL BASE EXP CFD SST CFD SAS