1. NEW YORK CITY COLLEGE, MECHANICAL ENGINEERING
Atmospheric Turbulence
for ME G200 - Applied Fluid Mechanics with Dr. Goushcha
Johnaton McAdam
12/21/16

2. 1
Contents
1. Introduction...........................................................................................................................................2
A. Problem Statement............................................................................................................................2
B. Objective...........................................................................................................................................2
C. Atmospheric Turbulence...................................................................................................................2
D. Governing Equations ........................................................................................................................3
2. Geometry...............................................................................................................................................4
A. Geometry Sketch (mm).....................................................................................................................4
B. Geometry Description.......................................................................................................................5
3. Mesh......................................................................................................................................................6
A. Meshed Geometry.............................................................................................................................6
B. Meshing Parameters......................................................................................................................7
4. Boundary Conditions ............................................................................................................................8
A. Annotated Geometry.........................................................................................................................8
B. Boundary Conditions Explained.......................................................................................................9
5. Setup ...................................................................................................................................................10
A. Model..............................................................................................................................................10
B. Solver Setup....................................................................................................................................10
C. Resulting Residuals Plot .................................................................................................................11
6. Results.................................................................................................................................................11
A. Velocity Profiles .............................................................................................................................11
B. Turbulence Intensity .......................................................................................................................12
C. Total Pressure..................................................................................................................................13
7. Discussion...........................................................................................................................................13
A. What Does the Results mean?.........................................................................................................13
B. What conclusions can be made? .....................................................................................................14
8. Acknowledgements.............................................................................................................................15
9. Conclusion ..........................................................................................................................................15
10. References.......................................................................................................................................15
11. Appendix.........................................................................................................................................16

3. 2
1. Introduction
A. Problem Statement
The Problem that will be addressed in this research is the simulation of atmospheric
turbulence using the Ansys-Fluent computational fluids dynamics software. The governing
equation will include the naiver stokes equations and the two equation model, k-epsilon to give
the turbulent properties.
B. Objective
The purpose of this research paper is to generate a computer simulation of atmospheric
turbulence in a wind tunnel to study its effects. The methodology that will be used to tackle this
problem will include the use of three main components, turbulent fins, roughness element and a
barrier. The goal is to create the boundary layer as seen below and to validate the results; the
data computed will be compared to those found in literature.
C. Atmospheric Turbulence
In many engineering and physics research the study of the turbulent spectrum and its
influence of the atmospheric are important for many applications such as wind turbine, air craft
design and even weather phenomenon. The term Atmospheric turbulence is used to describe the
dynamic irregular motion of winds that varies in velocities and directions, this occurrence causes
the water vapor, smoke and as well as the energies to become distributed horizontally and
vertically in 3D. The boundary layers created at the lowest part of the atmospheric are created
from the effects of earth surface roughness, temperature and other turbulent movements.
Scientist has always wanted to replicate this phenomenon to study its effect on aerodynamic
bodies such as rockets because it has been argue that the upper atmosphere wind conditions is a
contributing factor to rocket crashes or to simply harvest this natural energy with the use of wind
turbines.
Figure 1:
Atmospheric
Turbulent Boundary
Layer illustration

4. 3
D. Governing Equations
Continuity
1.
𝜕𝑈𝑖
𝜕𝑥 𝑖
= 0
Momentum
2. 𝜌 (
𝜕𝑈𝑖
𝜕𝑡
+
𝜕(𝑈𝑖 𝑈 𝑗)
𝜕𝑥 𝑗
) = −
𝜕𝑃 𝑖
𝜕𝑥 𝑖
+ 𝜇 (
𝜕2 𝑈𝑖
𝜕𝑥 𝑗
2) + 𝜌𝑔𝑖
Reynolds-averaged Naiver–Stokes equations
Let: 𝑈𝑖
′̅̅̅̅ = 0 𝑈𝑖
′′̅̅̅̅ ≠ 0 = 𝑈𝑖
′ 2̅̅̅̅̅ 𝑈𝑖=𝑈̅𝑖 + 𝑈𝑖
′
𝑈̅𝑖
̅ = 𝑈̅𝑖
Plug in appropriates values
𝜕(𝑈̅𝑖 + 𝑈𝑖
′
)
𝜕𝑥𝑖
= 0
𝜌 (
𝜕(𝑈̅𝑖 + 𝑈𝑖
′
)
𝜕𝑡
+
𝜕(𝑈̅𝑖 + 𝑈𝑖
′
)(𝑈̅𝑗 + 𝑈𝑗
′
)
𝜕𝑥𝑗
) = −
𝜕(𝑃̅𝑖 + 𝑃𝑖
′
)
𝜕𝑥𝑖
+ 𝜇 (
𝜕2(𝑈̅𝑖 + 𝑈𝑖
′
)
𝜕𝑥𝑗
2 ) + 𝜌𝑔𝑖
Take the Average of both equations
𝜕(𝑈̅𝑖 + 𝑈𝑖
′̅̅̅̅̅̅̅̅̅̅)
𝜕𝑥𝑖
= 0
3.
𝜕(𝑈̅𝑖)
𝜕𝑥 𝑖
= 0
𝜌 (
𝜕(𝑈̅𝑖 + 𝑈𝑖
′)
𝜕𝑡
+
𝜕(𝑈̅𝑖 + 𝑈𝑖
′)(𝑈̅𝑗 + 𝑈𝑗
′)
𝜕𝑥𝑗
̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅̅
) = −
𝜕(𝑃̅𝑖 + 𝑃𝑖
′̅̅̅̅̅̅̅̅̅)
𝜕𝑥𝑖
+ 𝜇 (
𝜕2
(𝑈̅𝑖 + 𝑈𝑖
′̅̅̅̅̅̅̅̅̅̅)
𝜕𝑥𝑗
2 ) + 𝜌𝑔𝑖
4. 𝜌 (
𝜕(𝑈̅ 𝑖)
𝜕𝑡
+
𝜕(𝑈̅ 𝑖 𝑈̅ 𝑗)
𝜕𝑥 𝑗
) = −
𝜕(𝑃̅ 𝑖)
𝜕𝑥 𝑖
+ 𝜇 (
𝜕2(𝑈̅ 𝑖)
𝜕𝑥 𝑗
2 ) − 𝜌
𝜕(𝑈𝑖
′ 𝑈𝑗
′̅̅̅̅̅̅̅)
𝜕𝑥 𝑗
+ 𝜌𝑔𝑖
Κ − 𝜖 𝑀𝑜𝑑𝑒𝑙
5.
𝐷 𝑘
𝐷𝑡
=
𝜕
𝜕𝑥 𝑖
(
𝜇 𝑒𝑓𝑓
𝜎 𝑘
𝜕 𝑘
𝜕𝑥 𝑖
) + [𝜇 𝑇 (
𝜕(𝑈̅𝑖)
𝜕𝑥 𝑗
+
𝜕(𝑈̅ 𝑗)
𝜕𝑥 𝑖
) −
2
3
𝜌 𝛿𝑖𝑗𝑘]
𝜕(𝑈̅ 𝑗)
𝜕𝑥 𝑖
− 𝐶 𝐷
𝜌𝜅3/2
𝑙 𝑚
6.
𝐷ϵ
𝐷𝑡
=
𝜕
𝜕𝑥 𝑖
(
𝜇 𝑒𝑓𝑓
𝜎ϵ
𝜕ϵ
𝜕𝑥 𝑖
) + 𝐶1 [𝜇 𝑇 (
𝜕(𝑈̅𝑖)
𝜕𝑥 𝑗
+
𝜕(𝑈̅ 𝑗)
𝜕𝑥 𝑖
) −
2
3
𝜌 𝛿𝑖𝑗𝑘]
𝜕(𝑈̅ 𝑗)
𝜕𝑥 𝑖
− 𝐶2
𝜌ϵ2
𝜅

5. 4
2. Geometry
A. Geometry Sketch (mm).
Figure 2: Fluid and Solid Domains
Figure 3: Solid Domain Dimensions

6. 5
B. Geometry Description
The geometry was drawn from various atmospheric boundary experiments, which composed
of three main components; the vortex generators, barrier wall and roughness elements. The
dimensions of the roughness element were chosen arbitrary thus three different types of the
structure were created each having a unique measurement. The elliptical vortex generators were
implemented from the Counihan design with is use in various wind tunnel experiments as seen in
figure 5. Lastly the barrier wall or trip wire was created from looking at different types of
experiment setups then comparing their ratio of the wall height to the fins. Each one of the
components serve an important purpose this simulation, the barrier wall will create the vorticity
by creating regions of low pressure, the fins will create vortex that will later create the turbulence
layer in the atmosphere and the roughness element will create the turbulent boundary layer. Due
to the limitations of the student version of Fluent I was unable to increase the complexity of my
roughness geometry or the number of fins I originally intended to have.
Figure 4: Experimental Geometry Representation
Figure 5: Experimental Geometry Setup

7. 6
3. Mesh
A. Meshed Geometry
Figure 6: Meshing Domain
Figure 7: Refine Meshing Region

8. 7
B. Meshing Parameters
Type Triangle Meshes Advanced
Settings Number of CPU for Parallel
Meshing
Program Controlled
Physics Preferences CFD Straight Side Element
Solver Preference Fluent Number of Retries 0
Relevance 0 Rigid Body Behavior Dimensionally
Reduced
Export Format Standard Mesh Morphing Disabled
Shape Checking CFD Triangle Surface Mesher Program Controlled
Target Skewness Program Controlled Topology Checking No
Element Midside Nodes Dropped Pinch Tolerance 2.938e-003m
Sizing Generate Pinch on Refresh No
Size Function Proximity and Curvature
Relevance Center Fine
Initial Size Seed Active Assembly
Smoothing Medium
Transition Slow
Span Angle Center Fine
Curvature Normal Angle 18
Num Cell Across Gap 3
Proximity Size Function Face and Edges
Min Size 3.2643e-003 m
Proximity Min Size 3.2643e-003 m
Max Face Size 0.326430 m
Max Tet Size 0.652870 m
Growth Rate 1.64
Automatic Mesh Based
Defeaturing
On
Defeature Size 1.6322e-003 m
Minimum Edge Length 1e-002 m
Inflation
Use Automatic Inflation None
Inflation Option Smooth Transition
Transition Ratio 0.272
Maximum Layers 5
Growth Rate 1.2
Inflation Algorithm Pre
View Advanced Options No
Assembly Meshing
Method None
Statistics
Nodes 97797
Elements 494796
Mesh Metric None

9. 8
4. Boundary Conditions
A. Annotated Geometry
Annotated
Geometry
Description Boundary
Conditions
Illustration
Inlet This is the location
where the fluid will
be prescribed.
Velocity Inlet
Walls Area Surrounding
the fluid domain.
No Slip Wall
Turbulent
Geometry
The main
components of this
experiment that will
create the
atmospheric
boundary layer.
No Slip Wall
Floor Area that that will
act as the earth
surface for the
simulation.
No Slip Wall
Outlet The region where the
fluid will leave the
control volume.
Pressure Outlet

10. 9
B. Boundary Conditions Explained
i) Inlet Velocity Profile
The inlet velocity profile will have a prescribe velocity behavior that is similar to the
power law use to determine wind velocity at different height. The reference velocity will be 5
m/s, the reference height will be 6m and the power index will be 1.7. The reason for the use of
this udf is due to the nature of the turbulent features dissipating very rapidly due to a uniform
flow, thus it was very difficult to conceive the atmospheric boundary layer. The fluid that was
used in this setup is air which is found in the fluent database. The turbulence model specification
model will include the turbulence intensity and viscosity ratio, the turbulence intensity will be set
to 10% and the viscosity ratio will be its default value of 16.
7. 𝑢 = 𝑢 𝑟
𝑧
𝑧 𝑟
𝛼
ii) Walls and Floor
The walls in this simulation are all stationary and will be subjected to the no slip
condition with a default roughness of 0m and a roughness coefficient of 0.5.
iii) Turbulent Geometry
The turbulent geometry will have the same conditions as the wall however the roughness
parameters will be different. From research the wall roughness is estimated to be 0.327 from
Pattanapol et al and the roughness height will be 0.6m.
Model Parameter Default FLUENT Pattanapol et al.
Roughness Height z (m) 30*z (m)
Roughness Constant 0.5 0.327
iv) Outlet
The outlet is treated as a pressure outlet with a gage pressure of 0 pascals, the backflow
direction specification method will be normal to the boundary. The turbulence features that will
be referenced are the backflow turbulence intensity of 5% and the backflow turbulent viscosity
ratio of 10.

11. 10
5. Setup
A. Model
The type of solver that will be used for this simulation is the pressure-based, absolute
velocity formulation, transient time scheme and gravity will be neglected. The modeling
equations that will be use for the analysis are the standard k-epsilon equations with standard wall
treatment and modified imperial constants. The modified k-epsilon constants were derived by
Alinot and Mason (2002) which was used in wind farm data. No dynamic meshes were used in
this simulation.
Κ − 𝜖 Constant 𝐶𝜀1 𝐶𝜀2 𝐶𝜇 𝜎𝑘 𝜎𝜀
Standard 1.44 1.92 0.09 1.0 1.3
Alinot-Masson 1.176 1.92 0.03329 1.0 1.3
B. Solver Setup
Solution Controls
Pressure Density Body Forces Momentum Turbulent
Kinetic Energy
Turbulent
Dissipation Rate
Turbulent
Viscosity
0.3 1 1 0.7 0.8 0.8 1
Pressure-Velocity
Coupling
Spatial Discretization Transient
Scheme Skewness
Correction
Gradient Pressure Momentum Turbulent
Kinetic
Energy
Turbulent
Dissipation
Rate
Transient
Formulation
SIMPLEC 0 Least
Square Cell
Based
PRESTO! Second
Order
Upwind
Second Order
Upwind
Second
Order
Upwind
Second Order
Implicit
Iterations
Time Stepping
Method
Time Step
Size (s)
Number of
Time Steps
Max Iterations/Time
Step
Solution
Time
Fixed .001 6000 250 6 hours

12. 11
C. Resulting Residuals Plot
Figure 8: Scaled Residual Plot, after a few hours the residuals becomes stable and converges
6. Results
A. Velocity Profile
The velocity profile that was generated from this simulation is comparable to the results
found in other researches. The study that was done in this setup is composed of walls all around
the fluid domain, as predicted the velocity has a sharp increase near the surface and as the height
increase so does the velocity but slowly. The fluid is very chaotic at the floor which is created
by the barrier, fins and roughness element therefore; those geometry has achieved their purpose.
Figure 9: Velocity Contour

13. 12
Figure 10: Mean Velocity Profile
B. Turbulence Intensity
Below is a contour of the turbulence intensity and as expected there is a large
concentration of turbulence activity where the fins and roughness grid are located. Due to this
chaotic behavior of the air molecules it can be expected for sudden increase in the velocities of
that region. The fins and roughness elements are generating wakes downstream of the flow as
can be seen in the image below.
Figure 11: Contour Plot of Turbulence Intensity %

14. 13
C. Total Pressure
The pressure readings shows fluctuating pressure values throughout the calculation
region, as expected the region with the lowest pressure have the highest velocity which can be
proven from Bernoulli’s principle. The pressure is not uniform throughout the region which
shows that there are variations in the velocities and areas of vorticity.
Figure12: Pressure Contour
7. Discussion
A. What Does the Results mean?
The results that were obtained from this experiment showed that this simulation was able to
successful generate the effects of atmospheric turbulence. The proof can be shown using the
turbulence intensity, velocity and pressure contour plots, the regions where there is high
velocities also has high turbulence and low pressure. Based on the velocity graph the success of
this simulation can be proven with other works of literature such as the graph below, which the
same behavior as the velocity profile has computed from the simulation. Both graphs describe a
sudden increase of the velocity near the surface and as the height increase the velocity becomes
stable achieving a quasi-constant state. The turbulence intensity plot also supports the evidence
that this simulation has achieve its goal, in theory there should be high turbulence near the
geometrical shapes because that is their purpose. The turbulence intensity graph which is found
from a wind experiment matches the data of the contour plot provided from the simulation, both
have the highest concentration of turbulence at the surface and as the height increase it becomes
less. Lastly, the final evidence that supports the simulation achieving its goal is the pressure
contour which describes behavior of the velocity due to the inverse relation between pressure and
velocity; areas of low pressure will create high velocities.

15. 14
B. What conclusions can be made?
The simulation of atmospheric turbulence is a very tedious procedure, because of the
different parameters that taken into consideration to achieve the desired results. The first part of
the problem includes designing the appropriate turbulence shapes such as the fins, barrier wall
and roughness elements. This will define how the flow separates, vorticity formation and the
concentration of turbulence. The second part of the problem is controlling the velocity inlet,
because of the nature of software creating very low drag on the surfaces a prescribed velocity
will be required to simulate the expected results. The final step of the problem is choosing the
correct viscous model and not all equations are created equally, some may have their advantages
depending on their application choosing the correct model will produce accurate and applicable
results. The nature of the fluid that was used is incompressible and one way to check if the
solution is valid is to simply plot the density and if it is constant then the conditions has been
satisfy.
Figure 14: Density Contour Plot
Figure 13: Results Obtain from Literature Reference 3

16. 15
8. Acknowledgements
I would like to thank the various scientist and engineers who made their research available so
that many young aspiring students may learn and implement our ideas to that field of research. I
would also like to thank my Professor Dr. Goushcha for providing guidance for me when I
needed it the most.
9. Conclusion
In conclusion, the simulation of atmospheric turbulence can be a tedious process, however
the results acquire from the analysis can be used to study different atmospheric phenomenon. I
have better understanding of how computation fluid dynamics can be used to study the
aerodynamics around a body. The results I was able to obtain from this simulation were able to
be comparable to the ones found in literature; therefore I was able to successfully simulate the
atmospheric turbulence boundary layer. For my future scope of research, I hope to use the
knowledge I gain from working on this research topic in order to create technologies such as a
cheap and efficient wind harvesting device designed by my creativity.
10.References
[1] Alan Russell, (2009). Computational Fluid Dynamics Modeling of Atmospheric Flow
Applied To Wind Energy Research. Boise State University
[2] Sanket A Unhale, (2004), Application and Analysis of RANS based Turbulence model for
Bluff Body Aerodynamics. Texas Tech University.
[3] Adrián Roberto Wittwer, Guilherme Sausen Welter and Acir M. Loredo-Souza (2013). ,
Wind Tunnel Designs and Their Diverse Engineering Applications, Dr. Noor Ahmed (Ed.),
Intech, DOI: 10.5772/54088. Available from: http://www..com/books/wind-tunnel-designs-and-
their-diverse-engineering-applications/statistical-analysis-of-wind-tunnel-and-atmospheric-
boundary-layer-turbulent-flows

17. 16
11.Appendix
Nomenclature
𝑈̅𝑖 − 𝑚𝑒𝑎𝑛 𝑣𝑒𝑙𝑜𝑐𝑖𝑡𝑦 (𝑚 𝑠⁄ )
𝑈𝑖
′
− 𝑓𝑙𝑢𝑥𝑎𝑡𝑖𝑛𝑔 𝑣𝑒𝑙𝑜𝑐𝑖𝑡𝑦 (𝑚 𝑠⁄ )
𝜌 − 𝑑𝑒𝑛𝑠𝑖𝑡𝑦 (Kg/L)
𝑃𝑖 − 𝑝𝑟𝑒𝑠𝑠𝑢𝑟𝑒 (𝑃𝑎)
𝜇 − 𝑣𝑖𝑠𝑐𝑜𝑖𝑠𝑡𝑦 (𝑃𝑎 − 𝑠)
𝑢 𝑟 − 𝑟𝑒𝑓𝑒𝑟𝑒𝑛𝑐𝑒 𝑣𝑒𝑙𝑜𝑐𝑖𝑡𝑦 (𝑚 𝑠⁄ )
𝑧 𝑟 − 𝑟𝑒𝑓𝑒𝑟𝑒𝑛𝑐𝑒 ℎ𝑒𝑖𝑔ℎ𝑡 (𝑚)
𝑧 − ℎ𝑒𝑖𝑔ℎ𝑡 (m)
𝛼 − 𝑝𝑜𝑤𝑒𝑟 𝑖𝑛𝑑𝑒𝑥
𝐶𝜀1 𝐶𝜀2 𝐶𝜇 𝜎𝑘 𝜎𝜀 − 𝑘 𝑒𝑝𝑖𝑙𝑠𝑜𝑛 𝑐𝑜𝑛𝑠𝑡𝑎𝑛𝑡𝑠
𝑔𝑖 − 𝑔𝑟𝑎𝑣𝑖𝑡𝑦 (𝑁)
Κ − 𝑡𝑢𝑟𝑏𝑢𝑙𝑒𝑛𝑡 𝑘𝑖𝑛𝑒𝑡𝑖𝑐 𝑒𝑛𝑒𝑟𝑔𝑦 (𝑚2
/𝑠2
)
𝜖 − 𝑑𝑖𝑠𝑠𝑝𝑎𝑡𝑖𝑜𝑛 𝑟𝑎𝑡𝑒 (𝑚2
/𝑠^3)
Table of Figures
Figure 1: Atmospheric Turbulent Boundary Layer illustration -------------------------------------------------------- 2
Figure 2: Fluid and Solid Domains-------------------------------------------------------------------------------------------- 4
Figure 3: Solid Domain Dimensions------------------------------------------------------------------------------------------ 4
Figure 4: Experimental Geometry Representation----------------------------------------------------------------------- 5
Figure 5: Experimental Geometry Setup------------------------------------------------------------------------------------ 5
Figure 6: Meshing Domain ----------------------------------------------------------------------------------------------------- 6
Figure 7: Refine Meshing Region --------------------------------------------------------------------------------------------- 6
Figure 8: Velocity Contour ----------------------------------------------------------------------------------------------------11
Figure 9: Mean Velocity Profile ----------------------------------------------------------------------------------------------12
Figure 10: Contour Plot of Turbulence Intensity %----------------------------------------------------------------------12
Figure11: Pressure Contour---------------------------------------------------------------------------------------------------13
Figure 12: Results Obtain from Literature Reference 3 ----------------------------------------------------------------14
Figure 13: Density Contour Plot----------------------------------------------------------------------------------------------14

18. 17
UDF
#include "udf.h"
/* Constant Ur - wind velocity at ref height */
/* Constant Yr - reference height */
#define Ur 5.0
#define Yr 6.0
DEFINE_PROFILE(x_velocity, t, i)
{
real x[ND_ND];
real y;
face_t f;
begin_f_loop(f,t) /*loops over all faces in thread passed in Define Profile*/
{
F_CENTROID(x,f,t);
y = x[1];
F_PROFILE(f,t,i) = Ur*pow((y/Yr),(1./7.));
}
end_f_loop(f,t)
}
*this UDF was borrowed from the master thesis of reference [1]
Matlab Code
clc
clear all
filename = 'C:UsersJohnDesktop2016 Fall MEG200 - McAdamvelocity.csv';
delimiter = ',';
startRow = 5;
formatSpec = '%f%f%[^nr]';
fileID = fopen(filename,'r');
textscan(fileID, '%[^nr]', startRow-1, 'WhiteSpace', '', 'ReturnOnError',
false);
dataArray = textscan(fileID, formatSpec, 'Delimiter', delimiter,
'ReturnOnError', false);
fclose(fileID);
Vm = dataArray{:, 1};
Ym = dataArray{:, 2};
clearvars filename delimiter startRow formatSpec fileID dataArray ans;
hold on
plot(Vm,Ym)
ylabel('Displacement(m)')
xlabel('Velocity(m/s)')
title('Atmospheric Velocity')

19. 18
Technical Sketches

20. 19