Diploma Thesis of Jagannath Nandi

CZECH TECHNICAL UNIVERSITY, PRAGUE
FACULTY OF MECHANICAL ENGINEERING
DEPARTMENT OF PROCESS ENGINEERING
CFD simulation of impinging jet
DIPLOMA THESIS
2016 JAGANNATH NANDI

Declaration
I confirm that the diploma (Master’s) work was executed by my independent efforts,
under leading of my thesis supervisor. I stated all sources of the documents and
literature.
In Prague……………….. Name and Surname
………………………………

Acknowledgments
┼ I dedicate this study to my family and special friends for my source of inspiration
and strength.
I would like to thank Ing. Karel Petera, PhD for his extended supports, advice and
guidance.

Annotation sheet
Name: Jagannath
Surname: Nandi
Title Czech:
Title English: CFD Simulation of impinging jet
Scope of work: Number of pages: 65
Number of figures: 30
Number of tables: 5
Number of appendices:
Academic year: 2014-2016
Language: English
Department: Process Engineering
Specialization: Process Engineering
Supervisor: Ing. Karel Petera, PhD
Reviewer:
Tutor:
Submitter: Czech Technical University Prague, Faculty of Mechanical Engineering,
Department of Process Engineering
Annotation- Czech:

Annotation- English: Make a literature research of the given problem. Create a flow
and heat transfer model in ANSYS CFD. Make a grid/mesh independence study with
the created model. Compare the simulation results with experimental data. Make a
comparison of the analysis results for constant and developed inlet velocity profiles,
3-D vs. 2-D geometry, several Reynolds numbers and distances of the jet from the
impinged plate along with experimental data. Summarize the methodology used in the
thesis and propose possible improvements of the solution procedure.
Keywords CFD simulation, Impinging jet, Heat transfer, Nusselt number, Reynolds number
Utilization:

CONTENTS
ABSTRACT…………………………………………………………………………..7
NOMECLATURE…………………………………………………………………….8
1. INTRODUCTION……………………………………………………………10
2. LITERATURE RESEARCH ……………………………………………….11
2.1 Study of methods of experiment …………………………………...14
2.2 Experimental data ……………………………………………………..17
2.3 Graph or Figures……………………………………………………….18
3. Computational Fluid Dynamics…………………………………………..19
3.1 Ansys Fluent…………………………………………………………….19
3.2 Flow and Heat Transfer geometry…………………………..............20
3.3 Mesh generation & quality…………………………………………….23
3.4 Run Analysis and estimated models………………………………..30
4. 3D & 2D approaches comparison with experimental data…………..33
5. Background of grid convergence study………………………………...35
5.1 Theory of Grid convergence Index (GCI)…………………………...35
5.2 GIC analysis with simulated data…………………………………...36
5.3 Comparison with experimental data ……………………………….42
6. Theory of Wall Function …………………………………………………...43
6.1 Graphs from simulated results ……………………………………....46

7. CFD Simulation ……………………………………………………………….46
7.1 Model ……………………………………………………………………….50
7.2 Developed and Constant velocity profile comparison……………..54
7.3 Comparison of models with experiment at different Re & z/d…….56
8. Conclusion……………………………………………………………………...61
8.1 References……………………………………………………………….....63
8.2 List of Tables…………………………………………………………….....64
8.3 List of Figures……………………………………………………………....64

Abstract
This works aims at CFD simulation of flow and heat transfer of impinging jet through
circular nozzle which impacts the flat plate at certain distance. Simulation for various
distances of the nozzle to impinging plate and Reynolds number were performed.
Boundary conditions with constant and developed profile at the nozzle inlet were
compared. In this analysis of heat transfer, the Nusselt number dependency in on
dimensionless radius r/D was evaluated. Different turbulence models are available in
ANSYS Fluent (k epsilon, k omega SST, etc).These were compared with
experimental data from literature. From this perspective proper turbulence model can
be evaluated for different Reynolds number and different nozzle to impinged plate
distances (at different z/D ratio).
Keywords: CFD simulation, Impinging jet, Heat transfer, Nusselt number, Reynolds
number

NOMENCLATURE
Equivalent diameter [m]De
Hydraulic diameter [m]DH
u Air velocity at computational domain [m/s]
h Heat transfer coefficient [W/ (m2 K)]
k Thermal conductivity of solid [W/ (m K)]
L Length [m]
Fluid velocity [m/s)]V
Volumetric flow rate [m3/s]Q
Number of elementN
A Area [m2]
Nusselt number [-]
P
Nu
Perimeter [m]
Shear velocity [m/s] defined by wall shear stressUτW
τW Wall share stress [N/m2]
Prandtl number [-]
Air density [Kg/m3]
Pr
ρ
Reynolds number [-]Re
Specific heat [J/ (kg-K)]cp

Dimensionless distance from wall [-]
Coefficient of Thermal Conductivity of fluid [W/m K]
Z Distance from nozzle to impinged plate [m]
r Radius of impinged plate [m]
D Nozzle diameter [m]
α Thermal diffusivity [m2/s]
ρ Density [kg/m3]
µ Dynamic viscosity [Pas]
ν Kinematic viscosity [m2/s]
Average velocity [m/s]
T Temperature [K]
Dimensionless velocity [-]u+
y+
λ

1. Introduction: In modern arena jet impingement heat transfer and its
application is highly impacted on manufacturing, material processing and
electronic cooling, significantly. Impinging jets have received considerable
attention due to their inherent characteristics of high rates of heat transfer be-
sides having simple geometry. Such impinging flow devices allow for short flow
paths and relatively high rates of cooling from comparatively small surface
area. Various industrial processes involving high heat transfer rates apply
impinging jets. Few industrial processes which employ impinging jets are
drying of food products, textiles, films and papers; processing of some metals
and glass, cooling of gas turbine blades and outer wall of the combustion
chamber, cooling of electronic equipments, etc. Heat transfer rates in case of
impinging jets are affected by various parameters like Reynolds number, jet-to-
plate spacing, and radial distance from stagnation point. Here graph for
Nusselt number vs. distance from center of impinging plate to wall is very
important to get idea about heat transfer form nozzle to impinging jet and the
area or point of maximum heat Transfer. The below equation denotes relation
between Nusselt number and heat transfer coefficient.
Nu = (h De)/ λ [1]
This analysis report is about heat transfer by impinging jet by circular nozzle to
plate where nozzle diameter of D= 20mm (has been considered) and different
distances from nozzle to impinging plate (ratio of distance of nozzle to
impinging plate and diameter of nozzle), Z/D: 2 and Z/D: 6 at Reynolds
Number of 23000 and 73000 which is in turbulence zone. For geometry we
choose 3D and 2D both approaches and made comparison of Nusselt graph
(Nu vs. r/D) with experimental values and estimated models through ANSYS
simulation .Accordingly, we choose closest one, analysis of different model like
k- ε, k- ω standard and k- ω SST intermittency with constant and developed
profile for Reynolds number 23000 & 73000 of Z/D 2 & Z/D 6. We also made

grid independence study to select proper mesh element by calculation of
percentage of error for three different Mesh elements from same geometry.
Now as per selected number of mesh elements, we did simulations by different
model at different Reynolds number at Z/D 2 & 6 and achieved different Nu vs.
r/D graphs. Next we made comparison with experimental data to achieve right
prediction of model which is closer to experimental data at respective
condition.
2. LITERATURE RESEARCH
In order to compare with practical data of experiment of impinging jet we have
studied different literatures and their experimental approaches of impinging jet
effect on flat impinged plate, effect of heat transfer at different location of plate
for Reynolds number 23000 & 73000 at Z/D 2 and Reynolds Number 23000&
73000 at Z/D 6.
From the literature we have also observed comparisons of different models
along with experimental data and their approaches for correct estimated
model, experimental methods, and correction of measurements in different
cross sections of nozzle, different Reynolds number and different distance of
nozzle from impinging plate.
We performed our simulation of predicted model of Reynolds Number 23000,
Reynolds Number73000 with Z/D 2 & Z/D 6 taking reference of literatures of
Baughn & Shimizu(1989), Behnia (1997) ,Katti (2008). But other researchers
like Lytle and Webb(1995), Geo et al (2003),Lee et. al,(2004) , and their
experimental data for Nu number Vs r/D graph has been shown below that
reference we took from Gulati (2009), which will given an idea about similarity
as well as bit diversity of different experimental approaches at Reynolds
Number 23000 and Z/D 6

Table 1: Experimental data of Lytle and Webb (1995)
r/D Nu
0.45331 173.4461
0.912363 153.2968
1.426815 143.5986
1.831528 122.7475
2.345375 107.4783
2.806016 101.9531
3.321072 97.82609
3.726768 86.02801
4.214163 77.02357
4.701936 71.50106
Table 2: Experimental data of Geo et al(2003)
r/D Nu
0.455939 147.8557
0.965517 139.5543
1.340996 125.6238
1.850575 109.6193
2.306513 100.6069
2.789272 95.10126
3.218391 88.8846
3.727969 85.48515
4.157088 82.76989

Table 3: Experimental data of Lee et al (2004)
r/D Nu
0.457692 123.2591
0.915385 116.9916
1.4 94.70752
1.857692 81.47632
2.342308 73.81616
2.773077 70.33426
3.284615 64.06685
3.769231 59.88858
4.2 53.62117
4.684615 46.65738
5.196154 38.99721
5.653846 33.42618
Graph 1: Comparison Experimental graph for Table Number 1, 2 & 3 at
Reynolds Number 23000 at Z/D 6 , Reference from Gulati (2009)

2.1 Study of methods of experiment
We have chosen below research journals for our study and necessary action to
make comparison of experimental methods, approaches, and data along with
our simulated results. Baugh & Shimizu(1989) , Behnia 1997 and Katti(2008)
are significant for our comparison. We choose those journals as reference
model of experimental method for comparison along with our simulated model
Tabular form for an overview of mentioned literatures as selected for
comparison study according to our calculated conditions:
Table 4: Selection of literature as per condition
Sl No
Experimental
Literature
Condition
1
Baughn &
Shimizu(1989) Z/D 2, Re 23000
2
Baughn &
Shimizu(1989) Z/D 6, Re 23000
3
Baughn &
Shimizu(1989) Z/D 6, Re 73000
4 Benia (1997) Z/D 2, Re 73000
5
Katti (2008) ,
Baughn &
Shimizu(1989)
Z/D 2, Re 23000 for
Sec 5.2

We are describing experimental method of Baughn & Shimizu (1989)
Experimental Technique and apparatus: In this experimental
technique source of uniform heat flux has been developed by electrically
heating a very thin gold coating on plastic substrate. The surface
temperature distribution has been measured using liquid crystal. An
isotherm on the surface represent a color of constant heat transfer
coefficient and line of particular color( a light green was used most of
the data here) .The liquid crystal used here has narrow range of
approximately 1 °C over which the whole color spectrum occurs.
Temperature resolution of the green color was better than 0.1°C .The
position of the green line shifted by changing the electrical heating of the
gold coating and thus surface heat flux. This arranges a complete
mapping of heat transfer coefficient over the entire surface.
The apparatus were consisted essentially a bower, a long pipe for
development of flow to test section. The upstream developed length
provides fully developed flow at jet exit. The turbulence level at the
centre of the jet at the exit was measured with a hot wire, having
Reynolds number 23000.The test section has thin (0.64 centimeter
thick) plexiglass plate on front of which plastic sheet containing gold
coating and on the back of which there was Styrofoam for insulation.
The liquid crystal was air brushed on the surface of the gold coating. A
Mylar board surrounded the plexiglass to ensure a flat smooth surface.
The data reduction was straightforward and consisted of computing the
surface heat flux from gold coating voltage, current (determined from
shunt register) and the area. A radiation correction, using measured
emissivity of 0.5, was made to determine the convective component of
surface heat flux. The radiation correction usually less than 5
percentage .Conduction loss is less than 1 percentage due to low
thermal conductivity of plastic substrate which has been neglected.
Using ambient temperature and liquid crystal temperature, heat transfer
coefficient and corresponding Nusselt Number which is based on jet
diameter were calculated.

Uncertainty analysis of Nusselt Number was calculated by Kline and
Mcclintock method. Estimated uncertainty of Nusselt Number was 2.4
percentage, Reynolds Number was 2.3 percentage, r/D and z/D was 1
percentage.
Figure 1: Experimental set up of Baughn & Shimizu (1989)

2.2 Experimental data
Result of Experiment Baughn & Shimizu (1989)
At condition of Reynolds Number 23000 and z/D 2, experimental data and
accordingly graph as follow:
Table 5: Experimental data of Baughn & Shimizu (1989)
r/D Nu
0.000751 138.8252
0.271609 137.3573
0.623516 134.6696
0.757326 127.8469
0.908441 118.1011
1.112316 102.7523
1.300439 96.17177
1.607851 96.16428
1.799472 102.7355
1.963256 106.6284
2.16217 106.6236
2.351071 102.9657
2.701488 94.67632
3.150391 82.73129
3.536781 73.71042
3.788519 68.34612
3.995632 65.17489
4.292578 59.80949
4.508992 57.61225
5.203182 50.04519
5.653834 44.67605
6.430369 40.76029
8.724457 31.4494

2.3Graph or Figures
Graph 2: Experimental graph of Baughn & Shimizu (1989), Reynolds Number
23000 at Z/D: 2

3. Computational Fluid Dynamics
Computational fluid dynamics, usually abbreviated as CFD, is a branch of fluid
mechanics that uses numerical analysis and algorithms to solve and analyze
problems that involve fluid flows. Computers are used to perform the calculations
required to simulate the interaction of liquids and gases with surfaces defined
by boundary conditions. With high-speed computers, better solutions can be
achieved. The fundamental basis of almost all CFD problems are the Navier–Stokes
equations, which define many single-phase (gas or liquid, but not both) fluid flows.
Our thesis all simulation on turbulent flows simulation are based on RANS model
(Reynolds Average Navier - Stokes)
3.1ANSYS Fluent
ANSYS FLUENT software contains the broad physical modeling capabilities needed
to model flow, turbulence, heat transfer, and reactions for industrial applications
ranging from air flow over an aircraft wing to combustion in a furnace, from bubble
columns to oil platforms, from blood flow to semiconductor manufacturing, and from
clean room design to wastewater treatment plants. Special models that give the
software the ability to model in-cylinder combustion, aero acoustics, turbo machinery,
and multiphase systems have served to broaden its reach. Our application is heat
transfer by impinging jet at impinging plate at turbulent fluid flow at different distance
.Our intention is also to observe velocity profile from impact section to stagnation
point of wall. For that very reason we ran our simulation by models like k epsilon, k
omega standard, K omega SST, K omega SST intermittency for our simulation and
comparison with experimental data.

3.2Flow and Heat Transfer geometry
Geometry was created in ANSYS Design Modeler, based on the idea of
creation of the fluid volume of nozzle inlet. On the basis of above concept , we
created two types of geometry for impinging jet in Fluent, One geometry has
been created in 3 Dimensional and another one in 2Dimensional axial
symmetric aspect. The named sections are inlet, inlet wall, side outlet, top
outlet and flat impinged plate/wall. We also considered distance between
nozzle and impinged plate and which varies by z/D 2 and z/D 6. So we have
changed geometry accordingly.
Here nozzle diameter has been considered as 20 mm. Nozzle has circular
cross section. For the purpose of boundary condition specification, we created
named sections; Inlet, Inlet wall/nozzle wall, Side outlet, Top outlet, impinged
wall and side wall.
Figure 2: Sketch showing named sections of geometry

Figure 4: 2D Geometry (axisymmetric)

3.3Mesh generation & quality
Concept of Mesh in CFD:
The partial differential equations that govern fluid flow and heat transfer are not
usually amenable to analytical solutions, except for very simple cases. Therefore, in
order to analyze fluid flows, flow domains are split into smaller sub domains (made up
of geometric primitives like hexahedra and tetrahedral in 3D and quadrilaterals and
triangles in 2D). The governing equations are then discretized and solved inside each
of these sub domains. Typically, one of three methods is used to solve the
approximate version of the system of equations: finite volumes, finite elements, or
finite differences. Care must be taken to ensure proper continuity of solution across
the common interfaces between two sub domains, so that the approximate solutions
inside various portions can be put together to give a complete picture of fluid flow in
the entire domain. The sub domains are often called elements or cells, and the
collection of all elements or cells is called a mesh or grid. The origin of the term mesh
(or grid) goes back to early days of CFD when most analyses were 2D in nature. For
2D analyses, a domain split into elements resembles a wire mesh, hence the name.
Figure 5: Figure of geometric primitives for mesh

We created mesh for our simulation by below methods:
For 3D geometry we used ANSYS Meshing and its Multizone, sweep method, Edge sizing,
Face sizing, Inflation, and body sizing method to create mesh ( see the following figure 6)
Figure 6: Figure of mesh of 3D geometry

For 2D geometry, face sizing and inflation setting along with Automatic method in ANSYS
Meshing were used to create the mesh.
Figure 7: Figure of mesh of 2D geometry(axisymmetric)

Mesh Quality:
Quality of mesh is checked by following parameters to obtain proper mesh quality.
This module can be found in ANSYS under mesh statistics, which is also called mesh
metrics.
Main Parameters which have been defined mesh qualities are as follow:
a) Orthogonal Quality: In order to check orthogonal quality, we must know the
value. The value towards 0 means it is bad orthogonal value on the other hand
value close to 1 is good value.
Figure 8: Mesh matrix orthogonal quality (Ref: ANSYS study materials)
b) Skewness : Theoretical approaches of skewness is as follow
Skewness = (Optimal cell size – Cell size) / (Optimal Cell size)
For value 0 in skewness is perfect and value 1 or close to it is worst.
Figure 9: Mesh matrix Skewness (Ref: ANSYS study materials)

c) Aspect Ratio: For 2D geometry it is ratio between length and height, for 3D it is
ratio of circumcised to inscribed. Sometimes we accept larger aspect ratio
when there is no strong transverse gradient.
Mesh metrics graphs for 3D geometry
Figure 10 .a: Element quality of 3D mesh
Figure 10 .b: Graph of Element quality of 3D mesh
Figure 11 .a: Aspect Ratio of 3D mesh
Figure 11 .b: Graph of Aspect Ratio of 3D mesh

Figure 12 .a: Skewness of 3D mesh
Figure 12 .b: Graph of Skewness of 3D mesh
Figure 13 .a: Orthogonal quality of 3D mesh
Figure 13 .b: Graph of Orthogonal quality of 3D mesh

Mesh metrics graphs for 2D geometry
Figure 14 .a: Element quality of 2D mesh
Figure 14 .b: Graph of Element quality of 2D mesh
Figure 15 .a: Aspect Ratio of 2D mesh
Figure 15 .b: Graph of Aspect Ratio of 2D mesh
Figure 16 .a: Skewness of 2D mesh
Figure 16 .b: Graph of Skewness of 2D mesh

Figure 17 .a: Orthogonal quality of 2D mesh
Figure 17 .b: Graph of Orthogonal quality of 2D mesh
3.3Run Analysis and estimated models
In order to run analysis or simulation in CFD, there are some steps which are very
important before run calculation.
a) Model: In Fluent solution first we have to select model whichgives a good
prediction. In this work, we focus on RANS model like k epsilon, K omega SST
etc. Then we have to define the type of condition. For our case we need to see
heat transfer by hot air jet in turbulence at impinged wall, so we switch energy
equation on, other models like radiation, discrete phase, were set to off.
b) Material: We have to define type of material like solid, fluid and then specific
property of material like density, coefficient of heat, thermal conductivity and
viscosity. Fluent has huge data base for material properties. In our case we
used air at standard condition with constant thermo-physical properties.

c) Cell zone condition: As per mesh generation, it consists of larger number of
cells or finite volume. Each cell bounded by number of faces and this faces are
grouped in zone. In 2D case the cell zone is surface body .
d) Boundary condition: This parameter plays very vital role in analysis. It is very
much important to define proper boundary condition by specific data. For our
problem we had to define, velocity of air at nozzle. So here velocity is boundary
condition. In order to define it properly we must think of air flow at higher
Reynolds number through nozzle pipe and then hit at impinging plate, then we
must consider developed velocity profile through pipe as an input parameter
instead of constant velocity. This will be very close to practical approach. Now
developed velocity profile through pipe is my boundary condition to define. We
accordingly made separate analysis of flow through straight pipe at Reynolds
number 73000 and Reynolds number 23000 and we used it as boundary
condition.
e) Reference values: In this section we have to define necessary values like
density, temperature, viscosity ,specific heat etc which are important in
evaluation of derived quantities (Nusselt number for example)
f) Solution Method: Our simulation is pressure based so we choose solver
accordingly. In section of scheme couple based has been used in order to
obtain faster convergence. We choose second order upwind for momentum
and energy as well as pressure to get better accuracy.
g) Initialization: Before starting any iteration we should initialize the solution .Idea
behind a value at assigned for every cell in mesh for every solution variable to
make initial guess. A realistic initial guess make acceleration in convergence.
We used hybrid initialization which is common in use.

h) Run calculation: We choose number of iteration minimum 1000 and some
cases 10000 to get converged solution. In calculation it shows the graph of
residuals and number of iterations. Residuals basically measure imbalance of
current numerical solution. We can say the calculation has been converged
when residuals decreases by three order of magnitude.
In our simulations we tried to get the continuity residuals was below 10 (-5). See
the below figure 18, as example of one of our simulation where continuity
residuals dropped below 10 (-5).Parameters are 2D geometry model k omega
SST intermittency, developed velocity profile, of Reynolds Number 23000, Z/D
2
Figure 18: Sample Residuals Graph from one of simulation
The above figure shows that solution is in convergence both by nature and value.

4. 3D & 2D approaches comparison with experimental data
The above approaches showed us clear view to select appropriate type of geometry
for future calculation on different Reynolds number and different distances.
We choose condition of Reynolds number 23000 and z/D = 2.Initially we created 3D
geometry and run calculation to get convergence .Next we made four line on
impinged wall(each line 90° apart to other and meet each other at origin) and plot
graph Nusselt number vs r/D along four lines. We observed that all graphs are close
to each other so we selected closer graph and compare the same with 2D
approaches. Results are as follow:
Graph 3: Graph of 3D geometry Nusselt number Vs r/D
The above Graph 3 shows all four are almost similar which is on four lines on
impinged wall. We choose line 2 for next comparison with 2 D geometry along with
experimental data.
Now we will choose one of the geometry for future calculation based on below 2D &
3D graph along with experimental data Baughn (1989) at condition Reynolds number
23000, Z/D =2. Simulation model is k epsilon.

Graph 4: Graph of comparison between 3D & 2D geometry
From the above Graph 4 we can see the difference of 3D & 2D case specially at the
centre point (zero point), in 3D case number of element is very high ( number of
elements 218274 in 3D) compared to 2D and this causes also high computational
time. So we choose 2D approach for future calculations.

5. Background of grid convergence study
This is very important aspect of any numerical solution and its accuracy. It directly
depends on the size of mesh cells that is we need to use larger number of cells to get
a more accurate solution. Because the necessary computational time increases with
the increasing number of cells, we want to use only such number of cells which give
us reasonable accuracy within some chosen interval (distance) from a correct
solution, 1% for example. Unfortunately, we do not know the correct solution in
advance, so we have to make an extrapolation of results based on different mesh
sizes, and then we can make an estimation of the accuracy of individual solutions and
choose proper mesh size which will give us reasonable accuracy. Percentage of error
we can consider 1.5% with respect to extrapolated value.
5.1Theory of Grid convergence Index (GCI)
The dependence of solution to the number of elements can be described by the
equation
[2]
N, here represents the number of elements, and D is equal to two for the 2 - D case,
and equal to three for 3 - D. Number of mesh elements power to − 1/D represents a
value that is proportional to the size of mesh element, such as a two-dimensional
case 10x10 grid will result in 0.1, for mesh 100x100 it will be 0.01. In the above
equation, we have three unknown parameters, Φext, a & p, which can be obtained by
solving the system of three equations for the three different sizes of networks.
[3]
[4]
[5]

The parameter p here is the order of accuracy solutions aim is to be the greatest.
Φext parameter here is the extrapolated value of the exact solution for an infinite
number of elements. This value can then be used to assess the accuracy solutions for
each network size
[6]
[7]
[8]
Here, r21 is the ratio of the size of the elements for each size of the network. It is
recommended to select the compared network size so that the ratio is greater than
1.3, this means that for the 2-D case, the ratio of the number of elements should be
approximately 1.32^2 = 1.7, and for a 3- D it will 1.33^3 = 2.2
5.2 GCI analysis with simulated data
In order to make that analysis in our case, we consider 2D geometry of Reynolds
number 23000 at Z/D 2 where we observed from comparison study that k omega SST
intermittency model shows close nature to experimental data compare to other
models.
The below graph is prove of above statement, though we can observe some jump of
Nusselt number at 0 point. We made an approach in section 8 (e) to avoid that
confusion

Graph 5: Graph of comparison between simulated models
As per above realization we choose 2D geometry Reynolds Number 23000 and Z/D 2
for the next step calculation of GCI. We made GCI analysis by adopting calculation
steps as per section 5.1. We made the whole calculation in MATLAB. Here in our
case, N = Number of element that we choose three type of different mesh elements,
and Φ = Nusselt number for respective to the number of elements. We also made
three approaches to see the required percentage of error with respect to extrapolated
value. The motto is to find number of element which is close to accurate. In order to
do that we choose three sizes of mesh elements for 2D geometry Reynolds Number
23000 and Z/D 2.Here our simulated model is k omega SST intermittency. Now we
ran analysis and obtained Nusselt number vs. r/D three graph for each three
elements. (element name:0 having number of element 9883, element name1 having
number of element 27793 & element name 2 having number of element 79646). Next
we took three approaches to compare list percentage of error of three elements at
three different r/D values.
Approach number 1: We choose a point where r/D value is 0 and took Nusselt
number of each three element and made calculation. We obtained comparison result
for percentage of error is 1.8639 of point 2 with respect to point1. The below Graph
(Graph 7) obtained from MATLAB calculation .In that Graph X axis is Number of

elements and Y axis is Nusselt number. Three points represent three number of
elements and corresponding Nusselt number and another line represented
extrapolated value. We can observe from Graph 7 the closeness of the points from
extrapolated value.
MATLAB calculated values for Approach 1:
Phi21ext = 111.6889; e32a =1.4122; CGI32 =0.2609;e21a =10.5289;e21ext =1.4692;
CGI21 =1.8639; (for detail abbreviation and understanding of calculation, please
follow MATLAB script, shown in page number: 42 &43)
Graph 6: Graph for GCI analysis approach 1
However, the above Graph6 does not shows the decreasing tendency of evaluted
variable, the probable cause of interpolation by Fluent solver at the axis.Fluent is cell
center solver ,hence interpolation has to be used to get values at boundary of cells.

Approach number 2: Same methodology of previous approach .Here point choose
for Nusselt number at r/D 0.5. We observed from calculation that percentage of error
of point 2 with respect to point 1 is 1.7123 [%] which is better value than approach 1.
In the Graph 7 we can see the reflection of calculated result.
MATLAB calculated values for Approach 2:
Phi21ext =126.1480; e32a =2.3236; CGI32 =3.2430; e21a =1.2572; e21ext =1.3888;
CGI21 =1.7123 (for detail abbreviation and understanding of calculation, please follow
MATLAB script, shown in page number: 42 &43)
Approach number 3: Same methodology of previous approach .Here point choose
for Nusselt number at r/D 2.5. We observed from calculation percentage of error of
point 2 with respect to point 1 is 0.6399 [%]. In the Graph 9 we can see the reflection
of calculated result.

Matlab Calculated Values for Approach 3:
Phi21ext = 101.9523; e32a =0.8845; CGI32 =1.2336; e21a = 0.4703; e21ext =0.5093;
CGI21 =0.6399 (for detail abbreviation and understanding of calculation, please follow
MATLAB script, shown in page Number: 42 &43)
The accuracy of midsized mesh with number of elements 27793 was represented by
CGI32=3.24% at r/D = 0.5, and CGI32=1.16% at r/D= 2.5. This was considered as
sufficient and this mesh (element name 1) was used in consequent solutions.

MATLAB script:
N = [ 9883 27793 79646 ];
%%Phi = [ 99.591 100.085 101.433 ]; % r/D 2.5 ... wrong values - an
interpolation should be used
%Phi = [ 99.8517 98.4612 110.048 ]; % r/D = 0
%Phi = [ 132.5172 129.508 127.9 ] % r/D = 0.5
Phi = [ 100.063 100.956 101.433 ]; % r/D = 2.5
[N, i] = sort(N,'descend'); % reverse order of elements
Phi = Phi(i);
N
Phi
figure(1);
plot(N,Phi,'r*', N,Phi,'b');
grid on;
D = 2;
r21 = (N(1)/N(2))^(1/D)
r32 = (N(2)/N(3))^(1/D)
if ( r21 < 1.3 || r32 < 1.3 )
disp('refinement factors r21 and r32 should be greater than 1.3');
end
eps32 = Phi(3)-Phi(2)
eps21 = Phi(2)-Phi(1)
R = eps21/eps32
s = sign(eps32/eps21)
fq = @(p) log((r21.^p-s)./(r32.^p-s));
fp = @(p) p - 1/log(r21)*abs(log(abs(eps32/eps21))+fq(p));
%p = fzero(fp,1)
p = fsolve(fp,1)
Phi21ext = (r21^p*Phi(1)-Phi(2))/(r21^p-1)
%Phi32ext = (r32^p*Phi2-Phi3)/(r32^p-1)
e32a = abs((Phi(2)-Phi(3))/Phi(2))*100
CGI32 = 1.25*e32a/(r32^p-1)
e21a = abs((Phi(1)-Phi(2))/Phi(1))*100
e21ext = abs((Phi21ext-Phi(1))/Phi21ext)*100
CGI21 = 1.25*e21a/(r21^p-1)
Phi_ext = Phi21ext
abs((Phi(3)-Phi_ext)/Phi_ext)*100 % percentage difference from extrapolated
solution
abs((Phi(2)-Phi_ext)/Phi_ext)*100
abs((Phi(1)-Phi_ext)/Phi_ext)*100
%break;

%fun = @(x,N) x(1)+x(2)*N.^(-x(3)/D);
figure(2);
plot(N,Phi,'r*',N,Phi,'b');
hold on;
n = linspace(0.9*N(3),1.1*N(1),30);
plot(n,Phi_ext*ones(1,length(n)),'r');
%plot(n,fun(b,n),'b',n,fun(b,n),'b*');
%%text(80000,16.225,'Phi ext');
hold off;
grid on;
5.3 Comparison with experimental data
Now see the Graph 9 where we took simulated result of same model for element
name1, element name 0 and element name 2 made comparison with experimental
data to observe closest nature of number of elements to experimental data.
Graph 9: Graph of different element numbers and comparison with
experimental data
From above Graph 9 it’s clear that k omega SST intermittency developed model is
close to experimental data.

6. Theory of Wall Function & Boundary wall.
Theory of wall function is about approximation of the velocity profile near wall. In order
to define the same, we must know about concept of boundary layer.
Boundary wall: In physics and fluid mechanics, a boundary layer is the layer
of fluid in the immediate vicinity of a bounding surface where the effects of viscosity
are significant. The laminar boundary is a very smooth flow, while the turbulent
boundary layer contains swirls or eddies. The laminar flow creates less skin friction
drag than the turbulent flow, but is less stable. Boundary layer flow over a surface
begins as a smooth laminar flow. As the flow continues back from impact zone the
laminar boundary layer increases in thickness. At some distance back from the impact
zone, the smooth laminar flow breaks down and transitions to a turbulent flow. From a
drag standpoint, it is advisable to have the transition from laminar to turbulent flow,
the boundary layer inevitably thickens and becomes less stable as the flow develops
along the body, and eventually becomes turbulent, the process known as boundary
layer transition.
Wall functions are used to approximate the velocity profile near walls. These functions
describe the velocity with respect to the distance from the wall, most recently in a
form with dimensionless velocity u+ versus dimensionless distance y+. Their
definitions are the following
[9]
[10]
Here, uτ is "shear" velocity defined by the wall shear stress τw as
[11]

For smaller distances from the wall, the relation between the velocity and distance is
defined as linear
For larger distances, the logarithmic relation is used
[12]
Figure 19.Figure of boundary layer profile
Figure 20.Figure of logarithmic graph of u+ vs. y+

Figure 21 .Figure of Turbulent Boundary layer
Wall modeling strategies: Near wall region the solution gradient is very high, but
accurate calculation near wall is the success of simulation model. We have two
choices to achieve the same.
a) Using wall function: This wall function provides dimension less boundary profile
which allow long layer of mesh near to wall. For the first layer of the long layers
near wall, whose value y+ must be the range of 30< y+ < 300. This wall
function approach can be used when we focus on the middle domain instead of
evaluating a force on wall, for example.
b) Resolving viscous sub layer: In this approach in first grid cell y+ =1 and prism
layer mesh with growth rate not higher than 1.2 must be used. This approach
highly recommended for k omega SST model. We used this approach for our
work.

6.1 Graphs from simulated results
During simulation with higher element number we check Y+ must be around 1 by
following Graph to make it confirm that number of layer near wall is accurate as per
our prediction.
Below graph 10 for value of y+ Vs position and we observed for three different
numbers of elements (Element name 0, 1 & 2) and result was satisfactory. All are
within value of 0.6 and they have been merged with each other (as per below graph).
Thickness of first layer 0.01 mm which has been used for simulation and simulated
model k omega SST intermittency
Graph 10: Graph of y plus
7. CFD Simulation
The majority of engineering flows are turbulent flow, in order to simulate such a flow
we need CFD simulation by some turbulence model. Near boundary wall we have to
select specific model with certain boundary condition to define proper turbulence
model.
Some basic terms (quantities) used in the definition of turbulence flow

a) Reynolds Number (Re): The Reynolds number is defined as the ratio of
inertial forces to viscous forces and consequently quantifies the relative
importance of these two types of forces for given flow conditions. Reynolds
numbers frequently arise when performing scaling of fluid dynamics problems,
and as such can be used to determine dynamic similitude between two
different cases of fluid flow. They are also used to characterize different flow
regimes within a similar fluid, such as laminar or turbulent flow:
 Laminar flow occurs at low Reynolds numbers, where viscous forces are
dominant, and is characterized by smooth, constant fluid motion;
 Turbulent flow occurs at high Reynolds numbers and is dominated by inertial
forces, which tend to produce chaotic eddies, vortices and other flow instabilities.
In practice, matching the Reynolds number is not on its own sufficient to guarantee
similitude. Fluid flow is generally chaotic and very small changes to shape and
surface roughness can result in very different flows. Reynolds numbers are a very
important guide and are widely used.
Flow in parallel Plate:
[13]
Flow in pipe:
[14]
For Square, rectangular, annular duct:
[15]

Figure 22 .Figure of Moody Diagram (Reference internet)
The above Moody diagram clearly shows the laminar, transition, and turbulent flow
regimes as Reynolds number increases. The nature of pipe flow is strongly
dependent on whether the flow is laminar or turbulent.

b) Nusselt Number(Nu) : In heat transfer at a boundary (surface) within a fluid,
the Nusselt number (Nu) is the ratio of convective to conductive heat transfer
across (normal to) the boundary. Named after Wilhelm Nusselt, it is
a dimensionless number. The conductive component is measured under the
same conditions as the heat convection but with a (hypothetically) stagnant (or
motionless) fluid. A Nusselt number close to one, namely convection and
conduction of similar magnitude, is characteristic of "slug flow" or laminar
flow. A larger Nusselt number corresponds to more active convection,
with turbulent flow typically in the 100–1000 range .The convection and
conduction heat flows are parallel to each other and to the surface normal of
the boundary surface, and are all perpendicular to the mean fluid flow in the
simple case. Please follow equation Number [1] for numerical representation of
Nusselt Number.
For Turbulent regime in a pipe Nusselt number is defined as follow
Nu = 0.023 x (Re) 0.8 x (Pr) 0.33 [16]
c) The Prandtl number (Pr) : It is a dimensionless number, named after the
German physicist Ludwig Prandtl, defined as the ratio of momentum
diffusivity to thermal diffusivity. That is, the Prandtl number is given as:
[17]
d) Navier–Stokes equations: This equation describes the motion of viscous
fluid substances. These balance equations arise from applying Newton's
second law to fluid motion, together with the assumption that the stress in the
fluid is the sum of a diffusing viscous term (proportional to the gradient of
velocity) and pressure term. This is generally follow the concept of
Accumulation = input – output + source
This is significant application in dynamic flow analysis and in its computational
approaches.

7.1Model
In computational for simulation of fluid flow, there are three types of approaches.
a) RANS (Reynolds Average Navier-stoke Simulation): This is mostly used
approach in industrial flow, where simulations are performed on based of time
average Navier –stokes equations. The basic tool required for the derivation of
the RANS equations from the instantaneous Navier–Stokes equations is
the Reynolds decomposition. Reynolds decomposition refers to separation of
the flow variable (like velocity ) into the mean (time-averaged) component ( )
and the fluctuating component ( ). Because the mean operator is a Reynolds
operator, it has a set of properties. One of these properties is that the mean of
the fluctuating quantity being equal to zero. Please follow figure 23.
[18], where ,
Figure 23.Figure of instantaneous velocity (Ref: ANSYS study materials)
Instantaneous velocity = Time average velocity + Fluctuation velocity
Figure24. Sample Figure of RANS (Ref: ANSYS study materials)
b) LES (Larger Eddie Simulation) : This is a mathematical model
for turbulence used in computational fluid dynamics. The simulation of turbulent
flows by numerically solving the Navier–Stokes equations requires resolving an
ample range of time- and length-scales. The main idea behind LES is to

reduce this computational cost by reducing the range of time- and length-
scales that are being solved for via a low-pass filtering of the Navier–Stokes
equations. Such a low-pass filtering, which can be viewed as a time- and
spatial-averaging, effectively removes small-scale information from the
numerical solution. This information is not irrelevant and needs further
modeling, a task which is an active area of research for problems in which
small-scales can play an important role, problems such as near-wall flows,
reacting flows, and multiphase flows.
Figure25. Sample Figure of LES (Ref: ANSYS study materials)
C) DNS (Direct Numerical Simulation) : A direct numerical simulation (DNS) is
a simulation in computational fluid dynamics in which the Navier–Stokes
equations are numerically solved without any turbulence model. This means that the
whole range of spatial and temporal scales of the turbulence must be resolved. All the
spatial scales of the turbulence must be resolved in the computational mesh, from the
smallest dissipative scales, up to the integral scale, associated with the motions
containing most of the kinetic energy. Application of this model where full unsteady
Navier–Stokes equations. Usage is not in regular industrial flow.
Figure26. Sample Figure of DNS (Ref: ANSYS study materials)

RANS Turbulence model usage
In RANS model, substituting the velocity decomposed in to mean and fluctuation
velocities in to Navier stokes equation. A new term arrived which is Reynolds stress
tensor .It is modeled by some turbulence model like k epsilon, standard k omega,
realizable k epsilon, RNG k epsilon, SST k omega etc.
In general realizable k epsilon or k omega are used for standard cases.
SST k omega is used where highly accurate resolution of boundary layer is critical,
such as application involving flow separations or finely resolved heat transfer profiles
are required.
Standard k epsilon model is used, only when we are in need for crude estimation of
turbulence mode.
For our calculation we have used Realizable k epsilon, k omega SST, k omega SST
Intermittency Transient model.
A brief description of the above models has been mentioned in next page.
Realizable k epsilon: Realizable k−ɛ, an improvement over the standard k−ɛ model.
It is a relatively recent development and differs from the standard k−ɛ model in two
ways. The realizable k−ɛ model contains a new formulation for the turbulent viscosity
and a new transport equation for the dissipation rate, ɛ, which is derived from an
exact equation for the transport of the mean-square vortices fluctuation. The term
"realizable" means that the model satisfies certain mathematical constraints on the
Reynolds stresses, consistent with the physics of turbulent flows. Neither the standard
k-ɛ model nor the RNG k-ɛ model is realizable (Re-Normalisation Group -RNG). It
introduces a Variable Cμ instead of constant. An immediate benefit of the realizable k-
ɛ model is that it provides improved predictions for the spreading rate of both planar
and round jets. It also exhibits superior performance for flows involving rotation,
boundary layers under strong adverse pressure gradients, separation, and
recirculation. In virtually every measure of comparison, Realizable k-ɛ demonstrates a
superior ability to capture the mean flow of the complex structures.
Standard k omega: In computational fluid dynamics, the k–omega (k–ω) turbulence
model is a common two-equation turbulence model, that is used as a closure for

the Reynolds-averaged Navier–Stokes equations (RANS equations). The model
attempts to predict turbulence by two partial differential equations for two
variables, k and ω, with the first variable being the turbulence kinetic energy (k) while
the second (ω) is the specific rate of dissipation (of the turbulence kinetic
energy k into internal thermal energy).
k omega SST : The SST k-ω turbulence model is a two-equation eddy-
viscosity model which has become very popular. The shear stress transport (SST)
formulation combines the better of two worlds. The use of a k-ω formulation in the
inner parts of the boundary layer makes the model directly usable all the way down to
the wall through the viscous sub-layer, hence the SST k-ω model can be used as
a Low-Re turbulence model without any extra damping functions. The SST
formulation also switches to a k-ε behavior in the free-stream and thereby avoids the
common k-ω problem that the model is too sensitive to the inlet free-stream
turbulence properties. Authors who use the SST k-ω model often merit it for its good
behavior in adverse pressure gradients and separating flow. The SST k-ω model
does produce a bit too large turbulence levels in regions with large normal strain, like
stagnation regions and regions with strong acceleration. This tendency is much less
pronounced than with a normal k-ε model though.
k omega SST Intermittency Transient model :
The turbulence model solves another term which is intermittency along with
turbulence kinetic energy (k) and specific dissipation ( omega ) in equations. It
belongs the category model which can predict laminar to turbulence transition and
helps to increase prediction in various cases.

7.2Developed and Constant velocity profile comparison:
In order to achieve appropriate estimate model while comparison with
experimental results, we performed comparison study between two approaches
one is constant velocity profile and another developed velocity profile.
Constant Velocity profile is the hypothesis which describes that at inlet with certain
constant velocity air passes through burner tube. In this approach we do not
consider development of any profile while passing through burner tube.
On the other hand in Developed Velocity profile we assume condition fluid (air)
flowing through a pipe and simulated that results for different Reynolds and
incorporated the simulated to velocity profile of main geometry. Then we run the
whole calculation on that developed velocity profile.
As per observation, we have come to conclusion that Developed velocity profile is
more accurate with respect to constant velocity profile while comparing with
experimental results. We can say that this Developed velocity profile is close
estimation to practical situation. We considered Developed velocity profile in all
simulated results.
Graph 11 where we observed above comparison study and result.
Graph 11: Comparison between developed & constant velocity profile

We would also like to illustrate the above approach by comparison below figure of
velocity profile; we can easily distinguish the difference from below
Figure 27.Constant velocity profile (Z/D 2, Re 23000. Element 1)
Figure 28. Developed velocity profile (Z/D 2, Re 23000,Element 1)

7.3Comparison of models with experiment at different Re & Z/D & Results
In our thesis of simulation of fluent model and comparison study of experimental data,
we choose below condition
i) Creation of different Geometry in ANSYS Fluent in 3D & 2D approaches,
comparison with experimental data for selection suitable approach.
Details already described in section 4
.
ii) After consideration 2D geometry, run analysis to different, model k-epsilon,
k- omega standard, k – omega SST intermittency developed velocity profile
along with Experimental data for Reynolds number 23000 and Z/D :2
.Comparison results of graph Nu Vs r/D ,
Details already described in section 5.2
iii) Comparison study for Z/D : 2 and Reynolds Number 73000, estimated
model k omega SST intermittency developed & constant velocity profile
along with experimental data .Objective to find suitable estimated model:
For the above condition, we made little bit change in geometry as Reynolds Number
was too high, please follow figure 29 & 30 where it has been reflected that for case
Re 73000, length of impinged plate has been increased in double compare to Re
23000.The reason behind this change is only taking consideration of high inlet
velocity and proper boundary wall phenomena while prediction of suitable model.

Figure29. Figure for 2D geometry Re 23000, Z/D 2
Figure30. Figure for 2D geometry Re 73000, Z/D

Graph 12: Graph for comparison of simulated model and experimental data
From the above graph 12 we can see the difference between constant and developed
profile along with experimental data. Here we can see in developed velocity profile ,
jump of Nusselt number at 0 point is less compare to graph 5,due to change of
computational domain( as per figure 30)

iv) In this condition of Z/D: 6 and Reynolds Number 23000 to execute a
comparison study of different estimated model along with experimental
data.
Please follow below Graph 13, here we have also incorporated two experimental data
and we can get an idea of range of experimental data along with simulated results.
Graph 13: Graph for comparison of simulated model at Re 23000, Z/D 6
From the above graph we can say developed velocity profile trends to accuracy in
view of the range of experimental data (Baughn (1989) & Lytle & Webb (1995))

v) The last condition of Z/D: 6 and Reynolds Number 73000 to execute a
comparison study of different estimated model along with experimental
data.
Please follow below Graph 14, for the comparison study where it has been observed
that simulated results are bit away from experimental data, our observation has been
mentioned in conclusion( Section 8 (f) ).
Graph 14: Graph for comparison of simulated model at Re 73000, Z/D 6

8. Conclusion:
In view of our above approaches while pursuing simulation in ANSYS Fluent of
impinging jet, we can conclude point wise as follow:
a) Sec 2: Literature research: Here we did comparison different experimental data
from different experimental methods of impinging jet over plate and we
observed range of experimental data which is relatively large space (follow
Graph: 1). From that perspective we have accepted and taking into
consideration of that spread range while comparison with simulated model. As
we observed some simulated results may be not accurate with experimental
data, but they are closer and nature of graph almost in same manner. We
accepted that simulation results as best prediction.
b) Section 4: 2D & 3D approaches and comparison with experimental data: In this
section we have observed 2D axisymmetric model is much better (follow
Graph4) Moreover, 3D geometry has huge number of element which causes
huge computational cost, in order to avoid the same; we chose 2D approaches
for future calculations.
c) Section 5: Grid convergence index (GCI) : In this section we made comparison
study/ analysis for three different number of element and selected the mid-
sized mesh with number of elements 27793, which has been represented by
GCI index =3.24% . We used inflation layers near impinged wall, so that value
of y+ is close to1 and no wall functions have been used.
d) Section: 7.2: We observed difference between inlet constant and developed
velocity profile (follow Graph 11) and we can come to in conclusion that
developed velocity profile is better prediction or description real world boundary
condition. Therefore, we made simulation of flow in pipe to get developed
velocity profile and imported to inlet at impinging jet.

e) In section 7.3 (iii), we noticed that smaller computation domain caused an
unrealistic jump of Nusselt number at the centre while for larger domain we can
get better result. For example if we compare graph 5 and graph 12 , where
both of the case Z/D is 2 , but for graph 5 Reynolds number 23000 and in case
of graph 12 Reynolds number is 73000.So we made change in geometry by
increasing impinging wall length ( please follow figure (28 & 29) and we
observed substantial reduction of Nusselt number jump at central point ( follow
Graph 5 & 12).
f) Lastly in section 7.3, simulation of various Reynolds numbers and distance of
jet from impinged wall were performed. Several turbulence models were
compared and the best result obtained with k omega intermittency turbulence
model which was only model, predicted two peaks in Nusselt number
dependency. The best agreements with experimental data were observed for
smaller Reynolds number and smaller distances z/D. For larger Reynolds
number and larger distance, the agreement with experimental data was not
good with any of tested turbulence model. It may be possible to get closer
result for larger Reynolds number and larger distance by prediction with LES &
DNS model.

8.1References
N. Gao, H. Sun, D. Ewing(2003), Heat transfer to impinging round jets with triangular
tabs, International Journal of heat Mass Transfer 46 2557–2569
D. Lytle, B.W.Webb(1994), Air jet impingement heat transfer at low nozzle plate
Spacing’s, International Journal of heat and mass transfer 37 1687–1697.
D.H. Lee, J. Song, C.J. Myeong, (2004) The effect of nozzle diameter on impinging jet
heat transfer and fluid flow, Journal of heat transfer 126 554–557.
J.W. Baughn and S. Shimizu (1989), Heat transfer measurements from a surface
with uniform heat flux and an Impinging jet, J. of Heat Transfer 111(4) 1096- 1098.
M.Behnia. S. Parneix. P.Durbin.(1997),Accurate predictions of jet impingement Heat
transfer. HTD-VOL 343 National Heat Transfer conference.5,
Book No.H0190, 111-118
Katti, S.V.Prabhu (2008)/ International Journal of Heat Transfer 51 4480-4495
Gulati, Katti, S.V. Prabhu (2008)∗ Influence of the shape of the nozzle on local
heat transfer distribution between smooth flat surface and impinging air jet.
International Journal of Thermal Sciences 48 602-617.
ANSYS study material, https://moodle.fs.cvut.cz/course/view.php?id=102

8.2List of Tables
Table 1: Experimental data of Lytle and Webb (1995) …………………………. 12
Table 2: Experimental data of Geo et al(2003) ………………………………….. 12
Table 3: Experimental data of Lee et al (2004) ………………………………….. 13
Table 4: Selection of literature as per condition …………………………………. 14
Table 5: Experimental data of Baughn (1989) …………………………………….17
8.3List of Figures
Figure 1: Experimental set up of Baughn 1989& Shimizu (1989)……………….16
Figure 2: Sketch showing named sections of geometry ………………………….20
Figure 3: 3D Geometry ………………………………………………………………21
Figure 4: 2D Geometry (axisymmetric) …………………………………………….22
Figure 5: Figure of geometric primitives for mesh………………………………….23
Figure 6: Figure of mesh of 3D geometry…………………………………………...24
Figure 7: Figure of mesh of 2D geometry(axisymmetric)………………………….25
Figure 8: Mesh matrix orthogonal quality…………………………………………...26
Figure 9: Mesh matrix Skewness…………………………………………………….26
Figure 10 .a: Element quality of 3D mesh…………………………………………...27
Figure 10 .b: Graph of Element quality of 3D mesh………………………………...27
Figure 11 .a: Aspect Ratio of 3D mesh………………………………………………27
Figure 11 .b: Graph of Aspect Ratio of 3D mesh……………………………………27
Figure 12 .a: Skewness of 3D mesh………………………………………………….28
Figure 12 .b: Graph of Skewness of 3D mesh………………………………………28
Figure 13 .a: Orthogonal quality of 3D mesh………………………………………...28
Figure 13 .b: Graph of Orthogonal quality of 3D mesh……………………………..28
Figure 14 .a: Element quality of 2D mesh……………………………………………29

Figure 14 .b: Graph of Element quality of 2D mesh…………………………………..29
Figure 15 .a: Aspect Ratio of 2Dmesh………………………………………………….29
Figure 15 .b: Graph of Aspect Ratio of 2D mesh……………………………………...29
Figure 16 .a: Skewness of 2D mesh……………………………………………………29
Figure 16 .b: Graph of Skewness of 2D mesh………………………………………..29
Figure 17 .a: Orthogonal quality of 2D mesh…………………………………………..30
Figure 17 .b: Graph of Orthogonal quality of 2D mesh………………………………..30
Figure 18: Sample Residuals Graph from one of simulation…………………………32
Figure 19.Figure of boundary layer profile……………………………………………...44
Figure 20.Figure of logarithmic graph of u+ vs. y+ ……………………………………44
Figure 21 .Figure of Turbulent Boundary layer ………………………………………..45
Figure 22 .Figure of Moody Diagram……………………………………………………48
Figure 23.Figure of instantaneous velocity…………………………………………….50
Figure24. Sample Figure of RANS ……………………………………………………..50
Figure25. Sample Figure of LES ………………………………………………………..51
Figure26. Sample Figure of DNS ……………………………………………………….51
Figure 27.Constant velocity profile (Z/D 2, Re 23000. Element 1) ………………….55
Figure 28. Developed velocity profile (Z/D 2, Re 23000, Element 1)………………..55
Figure29. Figure for 2D geometry Re 23000, Z/D 2 …………………………………..57
Figure30. Figure for 2D geometry Re 73000, Z/D 2 …………………………………..57

Diploma Thesis of Jagannath Nandi

Recommended

Recommended

More Related Content

Similar to Diploma Thesis of Jagannath Nandi

Similar to Diploma Thesis of Jagannath Nandi (20)

Diploma Thesis of Jagannath Nandi