Analysis of Flow in a Convering-Diverging Nozzle

Alber Douglawi Analysis of a Converging-Diverging Nozzle AERO 406
1
Analysis of a Converging-Diverging Nozzle
(Final Project Report – setup and results)
ALBER DOUGLAWI, Cal Poly ID 008603136
Department of Aerospace Engineering
California Polytechnic State University
San Luis Obispo, CA 93407
Nomenclature
d Normal Distance to the Nearest Wall (m)
Cb1 Spalart-Allmaras Model Constant
L Characteristic Length (m)
P Turbulence Production
Re Reynolds Number
U Flow Velocity (m/s)
Z Compressibility Factor
𝜈 Viscosity (Pa*s)
μ Dynamic Viscosity (N*s/m2
)
ρ density (kg/m3
)
Ω Vorticity (1/s)
1 Introduction
The purpose of this project was to model the flow of air
in a converging-diverging nozzle. The intent was to
study the flow properties such as Mach number,
pressure, and temperature. Creating a mesh that would
adequately capture flow features such as oblique or
normal shocks was also a priority during these
simulations. Various meshes and models were utilized
in Star CCM+ to model the supersonic flow. This type
of simulation is used in industry to aid in testing,
analysis, and the design process. Computational Fluid
Dynamics (CFD) simulations can save on lead time and
cost of design iterations and can also be used to study
systems where controlled experiments are difficult or
impossible to perform [1].
1.1 Project Description
The original proposal for this project contained several
consecutive stages, each with more complex aspects.
The goals outlined in the original proposal began with
analysing flow properties for flow in a converging-
diverging nozzle. Once this is complete, the following
steps included studying flow features such as shocks and
expansion waves. The flow features in the nozzle have
been modelled and grid convergence has been
demonstrated. Further analysis was also conducted
including a number of simulations to compare the results
from inviscid cases to those of two different turbulence
models.
The nozzle for this simulation was modelled based on an
area function given in a NASA CFD verification nozzle
[2]. This part was created using the integrated CAD
package in Star CCM+ because that facilitates possible
modifications to dimensions without having to import
the part once again. The nozzle was revolved to 90° and
two symmetry planes were designated at the beginning
and end planes of the revolve. The nozzle can be seen in
Figure 1. While the NASA resource provided the area
function, the specified boundary conditions included
100°R flow which proved to be problematic when
entered into the simulation. This was most likely due to
the nozzle containing two phase flow at that
temperature. As a result different boundary conditions
were chosen.
Figure 1. Geometry of the NASA CFD verification
nozzle. The flow moves from left to right and the
planes of interest are labelled.
The nozzle geometry parameters are given in Table 1
and the area function can be found in reference 2.
Stagnation
Inlet
Symmetry planes
Pressure
Outlet

2
Table 1. Geometric dimensions of interest for the
nozzle.
Parameter Value
Length 254 mm
Inlet Diameter 45.4 mm
Throat Diameter 20.0 mm
Outlet Diameter 55.8 mm
It was quickly determined that setting physical boundary
condition values that are compatible with one another
greatly affects the rate of convergence. For this reason,
a MATLAB script was created such that when given the
initial conditions for one boundary, the remaining
properties are calculated using isentropic relations.
Table 2 shows an example set of boundary conditions.
Table 2. Sample boundary conditions.
Pressure
(kPa)
Temperature
(K)
Velocity
(m/s)
Stag. Inlet 4238 700 N/A
Pres. Outlet 101 243 N/A
Initial Cond. 4033 695 100
A stagnation inlet and pressure outlet were chosen as the
boundary types because parameters for nozzles are
typically given as chamber stagnation conditions and a
back pressure specification. The values of pressure and
temperature were set such that the flow would be choked
at the nozzle throat to ensure supersonic flow.
The general approach was to address the problem in
stages. This meant that the initial simulation was a
simple case and more complex aspects were added as the
residual errors settled. This gave the effect of having an
initial condition that is close to the solution. This
approach was implemented after a number of
simulations that initialized including turbulence failed to
converge.
Simplifying assumptions were made including that the
air was an ideal gas and that the flow was inviscid for
the first simulation. The compressibility factor, Z, was
found to be 1.01 which supports the ideal gas
assumption [3]. The Reynolds number, Re, was
calculated using the following equation,
𝑅𝑒 =
𝜌𝑈𝐿
𝜇
(1)
where 𝜌 is the density of the flow, U is the velocity, 𝜇 is
the dynamic viscosity, and L is a characteristic length
which in this case is the nozzle diameter. The Reynolds
number at the nozzle exit was found to be 4.5*105
. A
high Reynolds number suggests that the viscous effects
in the boundary layer are negligible [6]. This is because
Reynold’s number is a ratio of inertial to viscous forces
and a high value means that viscous forces are
dominated by inertial forces. After the residual errors
converged for an inviscid solution, the part was
remeshed with a prism layer and the Spalart-Almaras
turbulence model was included. This method of starting
the simulation in a simplified state and stepping through
stages of increasing complexity proved to be effective.
An example of this can be seen in Figure 9 in the
Appendix. This figure shows the steps in which the
simulation was brought to converge including turbulent
parameters.
A study modelling the Space Shuttle Main Engine
(SSME) was used as a resource to guide the approach in
this project. In this study a structured mesh was utilized
in a 2-D axisymmetric case. Isentropic relations were
used to determine the boundary conditions based on the
known chamber pressure and temperature [1]. CEA
(Chemical Element Analysis) was used to determine the
equilibrium composition of the combustion products [1].
Due to the flow having a high Reynold’s number, the
flow was expected to be turbulent [1]. The turbulence
model chosen in this simulation was the Baldwin-
Lomax model. This is an algebraic zero equation model
well suited for high speed flows with attached boundary
layers [7]. This is because the viscosity in this model is
calculated using the distribution of vorticity, meaning
that far away from the nozzle wall the viscosity is
negligible [1]. This model is used in the aerospace
propulsion industry and would be helpful for this
simulation but is not available in Star CCM+. A similar
method to the one used in this study was implemented
calculate the initial conditions in an attempt to model the
flow in the SSME in this project. This is discussed
further in section 2.
2 Numerical Model
The software used was CD Adapco’s Star CCM+. This
software was chosen over ANSYS due to the fact that
Cal Poly’s license to use ANSYS includes a cell count
limit. The simulations were run on a personal windows
desktop using an AMD Phenom II 6-core processor and
laptop using an Intel i7-4500U quadcore processor in
parallel. The run times ranged from 2-10 hours
depending on complexity and the number of cells.
3-D simulations were run for a converging-diverging
nozzle that was modelled after a NASA CFD
verification nozzle with air assumed to be an ideal gas.
For a solution including turbulence, the approach was to
begin with inviscid flow to achieve a baseline before
including turbulence. The turbulence models used were
the Spalart-Almaras and the K-𝜔 SST models. A more
detailed discussion of these turbulence models is located
in Section 2.2.
Initially it was intended that the numerical results be
compared to experimental data. However, it was
difficult to find sufficient information to recreate a
nozzle geometry and have data available for that nozzle.
An attempt was made to model the SSME based on a

3
CFD study for that nozzle [1]. For that case the flow
would consist of combustion products from hydrogen
and oxygen. NASA CEA was used to determine the
chamber pressure, chamber temperature, and the mole
fractions of the products before those values were
entered into Star CCM+. The settings were then changed
to a non-reacting flow. After multiple attempts a
recurring error concerning mass fractions prevented this
case from running. The method used to ensure proper
convergence for these simulations was to vary the grid
size and rerun the simulation to compare the results.
These findings are presented in section 2.2.
2.1 Grid Description and Refinement
A polyhedral mesh was chosen for this assignment. This
mesh offered an ability to better conform to the shape of
the nozzle than other mesher choices. The base size used
was 0.001m and the meshers ultimately included the
polyhedral, surface wrapper, surface remesher, and
prism layer meshers. Initially, one volumetric control
was used to refine the mesh downstream of the nozzle
throat. The size in this volume was set to be 25% of the
base size. This was not an efficient use of cells as it
covered the entire second half of the nozzle and resulted
in a large number of cells, but it was used to locate the
flow features of interest. Prior to this, the residual errors
were not converging and it was suspected that it due to
flow features such as shocks were beginning to form and
the mesh was not sufficiently fine in those regions. By
refining the mesh downstream of the throat, it was
ensured that the shock formation is captured. Figure 2
shows this mesh with the volumetric control.
After running this mesh, the shocks developing in the
diverging section were located. The next step was to
refine the mesh only around these flow features. Figure
3 shows an oblique shock forming past the throat of the
nozzle and the shock reflecting at the intersection of the
symmetry planes. To see a larger figure of this plot with
the Mach color legend, see Figure 11 in the Appendix.
Figure 3. Visualization of the shock location using a
contour of the Mach number.
Another feature resembling flow separation can be seen
forming immediately before the nozzle outlet. Figure 4
shows the mesh refined around these flow features.
These volumetric controls were created as cones to make
efficient use of cells and still follow along the
formations of the shocks. The number of cells was cut
from over 2.5 million to 1.06 million. Table 3 shows the
settings used for the meshers. Note that size parameters
are given as percentages of the base size.
Figure 2. Mesh with block volumetric control set to 25% of
base size. This volumetric control engulfs the entire diverging
section of the nozzle.
Figure 4. Various views of mesh refinement results
with volumetric controls. Volumetric controls are in
place along the first shock and its reflection as well as
the second shock forming just before the outlet.

4
Table 3. Mesher settings used in this simulation.
Setting Value
Base Size 0.001m
Number of prism layers 7
Prism layer stretching ratio 2
Prism layer thickness 40%
Surface growth rate 1.3
Optimization cycles 3
Quality Threshold 0.8
The base size was set to 0.001m because it was fitting
for a 0.254m long nozzle. The prism layer was created
to capture the boundary layer effects. The values for
number of prism layers, stretching ratio and prism layer
thickness were varied to obtain a smooth transition from
the prism layer to the polyhedral cells with the last cell
in the prism layer having a similar volume to that of the
polyhedral cells. Figure 5 shows this gradual transition
along with the boundary layer representation.
(a)
(b)
Figure 5. a) Close-up view of the transition from the
prism layer to the polyhedral mesh. b) Velocity vector
representation of the boundary layer.
The surface growth rate was set for similar reasons. As
stated earlier, a number of volumetric controls were used
to refine the mesh in areas of interest. The surface
growth rate was set to prevent sudden shifts in cell sizes
near the volumetric controls. The optimization cycles
and mesh quality threshold were set to 3 and 0.8,
respectively. While this increased the mesh generation
time significantly, it was found to increase the resulting
cell quality. Figure 14 in the Appendix shows a
histogram plot of cell quality for one of the simulations.
It can also be seen from Figure 5a that the boundary
layer was successfully captured.
2.2 Discussion of Results
For the purposes of comparing solutions for grid
independence and the effects of turbulence model
selection, four simulations were run for an inviscid case,
five were run using the Spalart-Allmaras model, and
four were run using K-𝜔 SST. For each of the inviscid
cases, the base size was changed and the simulation
reinitialized and run. The first viscous case was the
original simulation that allowed capture of the flow
features. This simulation was run initially as inviscid
and refined with volumetric controls twice before the
Spalart-Allmaras turbulence model was enabled. After
enabling the turbulence model and allowing the
residuals to settle, the base size was changed and the
simulation was resumed. The same process was repeated
for the K-𝜔 SST model. The residuals plot for the
Spalart-Allmaras cases is shown in Appendix Figure 9
and the residuals for the K-𝜔 SST cases are shown in
Appendix Figure 10. In total, nine solutions were
obtained for viscous cases. Thrust was chosen as the
value for comparison across all cases because this
application is dependent on thrust. This also facilitates
the comparison because it is one value to be compared
rather than a contour plot. Table 4 in the Appendix
shows the resulting thrust for each case along with the
number of cells. These values were plotted in Figure 6
for comparison.
Figure 6. Plot of thrust versus number of cells to
demonstrate grid independence.
The largest percent difference in the calculated thrust for
the inviscid cases was 0.1%. These cases were run in
completely independent solutions starting from zero
iterations unlike the turbulent cases which were
sequential. Figure 11 in the Appendix shows a sample
residuals plot for an inviscid case. It can be seen for the
viscous cases that the residuals for continuity, energy,
and momentum consistently dropped with each mesh
refinement starting from the order of magnitude of 10-5
and decreasing to a minimum on the order of 10-8
. The
largest percent difference for the thrust values from the
viscous cases was 0.02%. The percent difference
between the average of the viscous and inviscid cases
was 0.4%. This was expected because viscous effects are
dominated by inertial forces for flows with a high

5
Reynold’s number such as this. The contour plots for the
inviscid and viscous cases were nearly identical with the
exception of the boundary layer and two other regions
that are discussed further in this report.
Another topic worth noting is that the viscous cases had
reversed flow on a number of faces on the outlet plane.
The number of faces with reversed flow ranged between
400 and 900 for the different cases of varying mesh size.
This issue was not present in the inviscid cases. This was
most likely due to what appears to be flow separation
just before the outlet of the nozzle. Figure 7 illustrates
this flow feature.
Figure 7. Close-up view of the separated flow just
before the outlet of the nozzle.
To investigate whether or not this issue is mesh related,
the mesh size was modified using volumetric controls.
The size in this region was set to be one quarter of the
base size and the simulation was rerun, yet the feature
remained. By creating a velocity vector scene, it was
found that the flow separated and that there was
recirculation immediately before the outlet of the
nozzle. This explains the reversed flow along the outer
rim of the nozzle outlet. Flow separation occurs when
the boundary layer travels a sufficient distance along an
adverse pressure gradient that the speed of the boundary
layer relative to the surface falls to near zero. This seems
to be in agreement with the results shown here. The
pressure contours show a highly adverse pressure
gradient just before the outlet and the velocity vector
scene shows the recirculation.
Running multiple cases also allowed for the comparison
of two turbulence models. The first turbulence model
used was the Spalart-Allmaras model. This model has
proven to be more numerically well behaved and
consistent in a variety of cases [5]. This is a one equation
model that is suited for flows with a thin boundary layer
and is better suited for supersonic flow than the K-𝜖 or
K-𝜔 models [7]. The Spalart-Allmaras model was
beneficial to use in this simulation for its stability and
also because the flow is mainly along one axis and the
exhaust plume is not included. One drawback of the
Spalart-Allmaras model is that it requires a calculation
to the nearest wall for every field point which is
computationally expensive [7]. For a comparison an
attempt was made to use the K-𝜖 model. This failed a
number of attempts including some with a considerably
smaller base size. The residuals would diverge until a
floating point exception stopped the simulation. This is
most likely due to the weakness of this model near the
wall and in separated regions. The K-𝜖 model assumes
that the turbulent viscosity is isotropic which introduces
error in regions with highly adverse pressure gradients
or separated flow [7]. This likely explains why the K-𝜖
model failed to converge as there was a region of
separated flow just prior to the outlet of the nozzle.
Another option was the K-𝜔 model which works well
for separated flows. The downside of this model is that
it is highly dependent on the ratio of the turbulent kinetic
energy to dissipation rate in the free stream. This led to
the use of the K-𝜔 SST (Shear Stress Transport) model.
The K-𝜔 SST is a combination of the K-𝜖 and K-𝜔
models that uses a blending function that is dependent
on the normal distance to the wall, y [7]. The blending
function places emphasis on the K-𝜖 model when far
from the wall and on the K-𝜔 model when near the wall.
This utilizes the performance of the K-𝜖 model in the far
field and the numerical stability of the K-𝜔 model near
the wall. The K-𝜔 SST model converged to stable
residuals.
Using the K-𝜔 SST model it was found that the
separation point occurs further upstream than the
simulation using the Spalart-Allmaras model. The K-𝜔
SST simulation had the separation point occur at 5.1mm
upstream of the outlet and the Spalart-Allmaras
simulation had the separation point at 2.5mm upstream
of the outlet. The region with significant vorticity behind
the separation point extended further into the flow for
the K-𝜔 SST simulation. To investigate the cause of this
difference further, the turbulence production term for
the Spalart-Allmaras model is displayed below,
𝑃 = 𝐶 𝑏1 𝑣 (Ω + (
𝑣
𝑘2 𝑑2
) 𝑓𝑣2) (2)
where P is the turbulence production, Cb1 is a constant,
𝑣 is the turbulence variable that has the dimensions of
viscosity, Ω is the magnitude of vorticity, d is the
distance to the wall, and fv2 is a function of a turbulent
viscosity ratio [7]. The turbulence production term for
K-𝜔 SST can be written as,
𝑃𝑘 = 𝑣𝑡 𝑆𝑖𝑗Ω𝑖𝑗 (3)
where Sij is the strain rate and Ω𝑖𝑗 is the vorticity [7]. It
can be seen from comparing equations 2 and 3 that the
production term for Spalart-Allmaras will decrease as
distance to the wall increases. This may explain why the
turbulent effects seen in the simulation using the K-𝜔
SST model extended further into the flow. The Spalart-
Allmaras model is also known to overdamp the flow in
the core of a vortex which causes the damp out
prematurely [7].
Nozzle
Outlet

6
Another interesting flow feature occurred near the
intersection of the symmetry planes. The oblique shocks
developed after the nozzle throat were expected to meet
at the nozzle centreline and reflect off of one another to
form diamond shapes. Prior to the oblique shocks
meeting, a feature resembling a normal shock developed
in between. This feature is called a Mach stem and is
shown in Figure 13 in the Appendix to allow for more
detailed visualization. Figure 8 shows experimental
results with a Mach stem in which shocks were
generated in a supersonic flow using wedges. Similar
flow features to those found in the numerical simulation
can be observed. This feature has been observed in
nozzles previously but is perhaps more important for
applications that involve initiating explosives using a
wave front [8].
Figure 8. Experimental results for supersonic flow
showing a Mach stem formation. [9]
According to Ivanov, a triple point forms from which an
oblique shock, the Mach stem, and a slip surface all
emanate [9]. This can be seen clearly in the experimental
results above. In addition, the slip surfaces emanating
from the triple points essentially form the shape of a
converging-diverging nozzle [9]. The flow velocity
behind the stem is nearly zero and begins to accelerate
through the converging portion of the slip surfaces until
it becomes choked once again and becomes supersonic.
All of these features can be seen in the numerical
simulation results presented in Figure 13 in the
Appendix. The lower limit of the scale has been set to
Mach 1 in order to easily distinguish between the
subsonic and supersonic regions.
The region behind the Mach stem has a flow velocity
that is nearly equal to zero. This region was identified as
a possible location that would display significant
difference in the results when using various turbulence
models. Figure 15 in the Appendix shows a comparison
of this region between the Spalart-Allmaras and K-𝜔
SST turbulence model cases. When an inviscid flow
case was inspected for the same location, it was found
that the results were nearly identical to that of the
Spalart-Allmaras case. This is expected because the
Spalart-Allmaras model is designed for supersonic
flows and includes a dependency on the distance to the
wall. Under this model when the distance to the wall is
large, turbulence is negligible. The Mach stem occurs at
the intersection of the symmetry planes and hence the
distance to the wall from this location is maximized. The
Spalart-Allmaras model resulted in higher pressure in
the region behind the Mach stem than the K-𝜔 SST
model. Figure 15 in the Appendix allows for a
comparison of these two cases. The scale was set to
match for both simulations and also set to a range that
would allow us to distinguish between contours easily.
Using the Spalart-Allmaras model resulted in a pressure
behind the Mach stem that is about 22% higher than the
K-𝜔 SST result for the same location. The K-𝜔 SST
model uses a correction when solving in areas with
rotational flows that is similar to the Spalart-Allmaras
model [7]. This correction has a much smaller effect on
the K-𝜔 SST model because it uses strain rather than
vorticity to calculate the turbulence production term as
seen in equations 2 and 3 above. The result is that the K-
𝜔 SST model may have obtained a lower pressure at this
location. Experimental results have shown that this
model tends to underpredict pressure in regions with
highly adverse pressure gradients and rotational flow
[7].
The choice of turbulence model was found to have no
significant effect on shock thickness or flow properties
such as pressure and temperature in the free stream with
the exception of the differences discussed above.
3 Conclusion
The results of these simulations accomplished the initial
goals of modelling flow features of interest in a
converging-diverging nozzle. Using an overexpanded
nozzle allowed the flow features of interest to form.
Results were obtained for values such as thrust,
pressure, Mach number, and other flow properties for
each simulation. One valuable lesson learned is the idea
of simplifying the simulation to obtain a stable solution
before adding in more complex models. This allows the
solver to initialize closer to the new desired solution.
Utilizing this method is what allowed the simulations in
this project to include a turbulence model and still
converge. Running the simulation as inviscid and
allowing the residuals to settle before including a
turbulence model proved to be effective.
Utilizing advanced initialization methods also proved to
be useful. One issue with this simulation was that the
inlet pressure was significantly different from the
pressure set throughout the medium under the physics
initial conditions node. The properties set here are the
initial conditions in all cells. When the simulation was
run, there was a very large pressure gradient near the
inlet that would result in supersonic flow at an incorrect
location. Using a linear Courant ramp was an effective
means of overcoming this issue. Another possibility
Oblique
Shocks
Mach Stem
Triple Point
Slip Surfaces

7
would be to use field functions to define the initial
conditions with respect to position downstream from the
inlet. This could be used to set the pressure and
temperature along the nozzle using isentropic relations.
Setting these initial conditions would allow the solver to
begin closer to the desired solution which provides more
numerical stability and a faster settling time.
A number of inviscid and viscous flow cases were run
to show grid independence and the solutions were well
in agreement. It can be concluded that the mesh is
capturing the appropriate flow features because further
refinements yield the same results. The inviscid and
viscous results for flow properties were closely
matched. This supports the hypothesis that the viscous
effects can be neglected. The Spalart-Allmaras and the
K-𝜔 SST models were also compared across a number
of cases. It was found that the turbulence model has no
discernible effect on the thrust results as discussed in
section 2. The choice of turbulence model did have an
effect on the flow separation point just before the outlet
of the nozzle. It was found that the flow separation using
the K-𝜔 SST model occurred earlier in the flow and the
region with significant vorticity extended further into
the flow. The shock location and thickness were not
affected. Using the K-𝜖 turbulence model proved to be
difficult. This turbulence residual errors using this
model model did not converge after numerous attempts
with various grid sizes. This was attributed to a region
with flow separation which the K-𝜖 model is known to
have difficulties with.
This analysis resulted in a deeper understanding of the
software and various methods of approaching the same
problem. Another product of this product is the
experience gained with using some of the advanced
tools for initializing the solution and also gained
experience with post processing.

8
Appendix:
Figure 9. Residuals plot for the viscous flow simulation using Spalart-Allmaras. The simulation was started as inviscid flow and refined before turbulence was included.
The mesh was then refined to obtain results to show grid convergence.
grid independence.

9
Figure 10. Residual errors plot for the cases using the K-𝝎 SST turbulence model. These cases were run after the Spalart-Allmaras cases seen in Figure 9. The Sdr residual can be
seen spiking between 11,000 and 11,400 iterations. This was a mesh size related issue that was solved in the following simulations.

10
Figure 11. Example residual plot for an inviscid case. This is the residual plot for case 4 in Table 4.
Figure 12. Mach number contour plot. This shows an oblique shock forming after the nozzle throat.

11
Figure 13. Mach contour showing the oblique shocks and Mach stem. The lower limit of the scale is set to 1.0 to aid
in distinguishing between the subsonic and supersonic regions.
Figure 14. Example cell quality histogram plot for case 9 in Table 4.
Detailed View
“CDV Nozzle” Slip Surfaces
Triple Point

12
Figure 15. Pressure contour plot comparison for Spalart-Allmaras and K-Omega SST turbulence models. The scale on
both contours was set to match and detailed views are presented.
Table 4. Thrust results for various grid sizes for viscous and inviscid flow cases
Case Turbulence Number of Cells Thrust (N)
1 Inviscid 273,128 1680.06
2 Inviscid 585,239 1681.39
3 Inviscid 657,041 1681.56
4 Inviscid 875,911 1681.84
5 Spalart-Allmaras 721,459 1673.88
6 Spalart-Allmaras 929,053 1673.83
7 Spalart-Allmaras 1,142,834 1673.82
10 K-Omega SST 1,162,506 1674.79
11 K-Omega SST 1,217,300 1674.77
12 K-Omega SST 1,445,052 1674.95
13 K-Omega SST 1,535,860 1674.95
Detailed Region
Spalart-Allmaras
K-𝝎 SST

13
References
[1] Chan, John S., and Jon A. Freeman. "Thrust Chamber Performance Using Navier-Stokes Solution." National
Aeronautics and Space Administration Marshall Space Flight Center (1984)
[2] "Converging-Diverging Verification (CDV) Nozzle." Converging-Diverging Verification (CDV) Nozzle. N.p., n.d.
Web. 09 Nov. 2015. <http://www.grc.nasa.gov/WWW/wind/valid/cdv/cdv.html>.
[3] Michael J. Moran, Howard N. Shapiro, Daisie D. Boettner, Margaret B. Bailey. Fundamentals of Engineering
Thermodynamics. 7th
edition, Wiley, 2011. Print.
[4] Allmaras, Steven R., Forrester T. Johnson, and Philippe R. Spalart. "Modifications and Clarifications for the
Implementation of the Spalart-Allmaras Turbulence Model." Seventh International Conference on Computational
Fluid Dynamics (2012)
[5] Cummings, Russell M., Scott A. Morton, William H. Mason, and David R. McDaniel. Applied Computational
Aerodynamics: A Modern Engineering Approach. Print.
[6] Shariatzadeh, Omid, Afshin Abrishamakar, and Aliakbar Joneidi Jafari. "Computational Modeling of a Typical
Supersonic Converging-Diverging Nozzle and Validation by Real Measured Data."
[7] Nichols, R. H. "Turbulence Models and Their Application to Complex Flows." University of Alabama at Birmingham
(n.d.): n. pag. <http://people.nas.nasa.gov/~pulliam/Turbulence/Turbulence_Guide_v4.01.pdf>.
[8] Ruban, Anatoly, and Mat Hunt. "The Shape of a Mach Stem." Society for Experimental Mechanics (2008): n. pag.
Web. <http://sem-proceedings.com/08s/sem.org-SEM-XI-Int-Cong-s070p01-The-Shape-Mach-Stem.pdf>.
[9] Ivanov, Mikhail S. "Transition Between Regular and Mach Reflections of Shock Waves: New Numerical and
Experimental Results."European Congress on Computational Methods in Applied Sciences and
Engineering (2000): n. pag. Web. <http://congress.cimne.com/eccomas/eccomas2000/pdf/611.pdf>.

Analysis of Flow in a Convering-Diverging Nozzle

Recommended

Recommended

More Related Content

What's hot

What's hot (18)

Similar to Analysis of Flow in a Convering-Diverging Nozzle

Similar to Analysis of Flow in a Convering-Diverging Nozzle (20)

Analysis of Flow in a Convering-Diverging Nozzle