The part is axisymmetrically modeled in solidworks(2D) before importing to ansys workbench where the boundary zones are identified and appropriate mesh settings is applied. The model is then imported in Fluent for analysis . Significant setting changes are Density based solver , Enhanced Eddy viscosity model with near wall treatment , solution steering , FMG initialization etc.

1. 1
CHAPTER -4
METHODOLOGY
4.1 GENERIC STEPS TO SOLVING PROBLEM IN FLUENT
Like solving any problem analytically, you need to define (1) your solution
domain, (2) the physical model, (3) boundary conditions and (4) the physical
properties. You then solve the problem and present the results. In numerical
methods, the main difference is an extra step called mesh generation. This is the
step that divides the complex model into small elements that become solvable in
an otherwise too complex situation. Below describes the processes in terminology
slightly more attune to the software. Build Geometry Construct a two or three
dimensional representation of the object to be modeled and tested using the work
plane coordinates system within ANSYS. Define Material Properties Now that
the part exists, define a library of the necessary materials that compose the object
(or project) being modeled. This includes thermal and mechanical properties.
Generate Mesh At this point ANSYS understands the makeup of the part. Now
define how the Modeled system should be broken down into finite pieces. Define
Boundary Conditions Once the system is fully designed, the last task is to burden
the system with constraints, such as physical loadings or boundary conditions.
Obtain Solution This is actually a step, because ANSYS needs to understand
within what state (steady state, transient… etc.) the problem must be solved.
Present the Results
After the solution is obtained, there are many ways to present ANSYS‟
results, choose from many options such as tables, graphs, and contour plots.
The solver used in this model is FLUENT, a commercial popular CFD
solver from ANSYS Inc. Solidworks of DS is also used to model the geometry as
per the study and its conversion into a neutral format.

2. 2
4.1.1 Domain
Every CFD simulation requires a domain where it is discretized and apply
the governing equations. The domain thus encompass the CAD geometry,
boundary conditions, control volumes and governing equations. In this project we
have designed a nozzle based on the data garnered from the journal we mostly
have referred. The CAD drawing of the model from Solidworks is shown below
The dimensions of the model is as follows
Table 4.1Nozzle dimensions
The model is drawn axisymmetric ally so only half of the dimensions shown is
taken to model the nozzle
Figure 4.1Cad drawing of a nozzle with a divergence angle of 11.3deg

3. 3
This CAD model, in order to do the analysis, has to be converted into a
geometrically neutral format called step (*.stp) before importing the model into
the simulation environment. Below is how the CAD part looks after it is imported
into Ansys.
Figure 4.2 Axisymmetric model of the nozzle in Ansys design modeler.
In the later phase of the project the divergence angle of the nozzle is changed to
13 and 15 degrees.
Figure 4.3 Model with 13 degrees divergence angle

4. 4
Figure 4.4 Model with 15 degrees divergence angle
The 11.3 degree divergence angle model is initially taken into the meshing
environment where mesh will controlled both locally and globally.
In any CFD analysis the mesh quality is so important and a critical factor
that affects the overall accuracy of the model. In this study we have taken utmost
care to make sure all the elements used in the model is of high quality nature.
These are achieved by the careful manipulation of the mesh settings available in
the Ansys Meshing tool; ICEM CFD. The meshed model is shown underneath.
Figure 4.5 11.3 degree nozzle after meshing

5. 5
The mesh chosen is high quality HEX mesh with very little or no skew.
This mesh has a global as well as local settings. The global settings affect the size
and nature of the mesh in a global sense where as local settings help us affect or
influence the mesh in a local sense.
Figure 4.6 Mesh settings with local and global controls
As explained above the shape the mesh is assigned to be very important when
considering the solution accuracy and the solver stability. Hence there are two
metrics to quantify or asses the condition of the mesh. They are (a) Orthogonal
quality and (b) Skewness. Both metrics vary between 0 and 1. Orthogonal quality
has to be maximum and Skewness has to be minimum.
The pick of mesh elements is so crucial that any distorted from ideal shapes if
selected may lead to difficult in solving and less accurate results. The mesh
element used in this model is of high quality one i.e. hex mesh in 2D.

6. 6
Figure 4.7Mesh Skewness
From the above figure it’s obvious that there are 5880 elements and the cell
centers of these elements are taken into account for finding out the pressure and
velocity fields. The average orthogonal quality is 0.982 and the average skewness
value is 0.083. These values when seen as ideal have a values of 1 and 0
respectively.
In order to complete the definition of domain we still need the boundary
conditions. Boundary conditions are applied over the edges or boundaries in this
case as shown below. Ansys needs proper identification of the boundaries or
edges in the way of Named Selections.
Figure 4.8 Mesh Orthogonal quality

7. 7
Figure 4.9. Naming or Identification of boundary zones
The boundary conditions taken for this analysis are tabulated as follows
Figure 4.10 Boundary condition illustration
Table 4.2Boundary conditions
Boundary Type Value
Inlet Pressure 100atm
Inlet Temperature 3300K
Outlet Pressure 1.68atm
Material chosen for this analysis is Air (ideal gas), Properties are shown below
Table 4.3 Material properties
Cp=1880J/kgK
Thermal
conductivity=.0142W/mK
Viscosity=8.983e-5 PaS

8. 8
CHAPTER -5
SOLVER SETTINGS
The solver selected to solve this problem is a density based solver. The
dependence of time is turned off in the solver settings. Hence we do a steady state
analysis. Compressible flows with Mach number greater than 3 are usually dealt
with the density based solver. Mach number is presumed to be higher since the
inlet and outlet pressure ranges are so enormous. The application of these nozzle
pressures find place in rocket propulsion activities.
5.1 SOLVER AND SOLUTION SETTINGS
Table 5.1 Solver and Solution settings
`General Solver type- Density based
2D space : Axisymmetric
Models Energy equation: On
Viscous model: Standard k-epsilon,
realizable , enhanced wall treatment
Solution controls Courant number=5(Changes with 10
intervals)
Solution initialization Full Multi Grid(FMG)
Run Calculation Solution steering method is adopted
Iterations 5000
Since the axisymmetric model is checked, all the conservation equations will be
solved in a cylindrical coordinate system.
To include the effects of temperature in the governing equations, energy equation
is turned on
The turbulent eddy viscosity model used is standard k epsilon model, where k
stands for turbulence kinetic energy and epsilon for the turbulent KE dissipation
rate. Local mesh settings have been invoked to additionally smear high aspect
ratio mesh cells on the geometry to capture the boundary layer turbulence

9. 9
phenomenon. That will only be calculated if the enhanced wall treatment is turned
on. The only condition that exists for calculation of the wall effects is the height
of the first cell adjacent to the wall should be very small. But too much small
mesh cells near the boundary layer leads to convergence difficulties.
Figure 5.1 High quality mesh cells with inflation layers
5.2 RESIDUALS
Since the mathematical model (Governing equations+Boundary
conditions) is discretely solved over the domain, two kinds of errors constitute,
they are (1) Discretization error and (2) linearization error. The discretization
error occurs when the domain is divided into a finite number of control volumes
whereby only the cell center values are calculated. The continuous values are then
computed after getting the pressure and velocity field values at the cell centers.
This is done through advanced interpolation methods on the cells and their
immediate neighbors. The distant the neighbors are the inaccurate the interpolated
values become. Thus discretization errors are brought down by refining the mesh.
But the value never becomes zero.
Second error that is inevitable in the CFD simulation or other numerical
method is the linearization error. Since the variables are nonlinear to find the root
or the unknown function is bit hard. Thus these nonlinear equations are linearized
using guess values and iterate them until the actual function is computed as a
range between two values. This iteration can’t be run eternally. By stopping the

10. 10
chain of events requires inputting another value called the Residual or the
tolerance limit. If the differences in values of two successive iterations fall below
this residual value the loop ceases. Setting the residual is also challenging. In
some cases if the residuals are input to be of very small order, difficulty in
convergence occurs. Thus it has to be input by trial and error.
5.3 CONVERGENCE CRITERION
Table 5.2Convergence criterion
RESIDUAL ABSOLUTE CRITERIA
Continuity 1e-8
X velocity 1e-8
Y velocity 1e-8
Energy 1e-8
K 1e-8
Epsilon 1e-8
Figure 5.2 Convergence Curve after the iterations
Turning on the FMG initialization, one of the advanced initialization
techniques available within the solver, the number of iterations taken to reach
convergence has dramatically been reduced.

11. 11
CHAPTER -6
RESULTS AND DISCUSSION
Following are the results obtained after the iterations
For the nozzle with the divergence angle 11.3 degrees
Figure 6.1 Pressure contours
Figure 6.2 Temperature Contours

12. 12
Figure 6.3 Velocity Contours
Table 6.1Velocity comparison
Section Ax/A* Velocity (m/s)
Theoretical CFD
Convergent 1.5 169.72 163.17
Convergent 1.2 482.91 478.139
Throat 1 1030.46 1022.64
Divergent 1.2 1335.28 2072.32
Divergent 4 2051.23 2081.47
Outlet 7.142 2387.52 2353.49
Table 6.2 Pressure Comparison
Section Ax/A* Pressure(atm)
Theoretical CFD
Convergent 1.5 87.33 96.68
Convergent 1.2 79.89 88.49
Throat 1 50.96 58.915
Divergent 1.2 32.08 32.87

13. 13
Divergent 4 10.98 7.63
Outlet 7.142 1.68 1.34
Table 6.3 Temperature Comparison
Section Ax/A* Temperature (K)
Theoretical CFD
Convergent 1.5 3240.08 3290.36
Convergent 1.2 3194.12 3223.75
Throat 1 2972.98 3012.7
Divergent 1.2 2760.50 2746.02
Divergent 4 2137.56 2154.2
Outlet 7.142 1774.90 1800.5
Figure 6.4 Mach number variation along the axis

14. 14
6.1 DIVERGENCE ANGLE WHEN VARIED
Initial CFD analysis had been conducted with the nozzle angle pegged at
11.3 degrees. This value has been changed to 13 and 15 degrees and the effects
are evaluated. The expected trend would be as the throat area drops the velocity
rises and as a result the pressure and the temperature drops.
DIVERGENCE ANGLE OF 13 DEGREES
Figure 6.5 Pressure contour at 13 deg divergence angle
Figure 6.6 Temperature contour at 13 deg divergence angle

15. 15
Figure 6.7 Velocity contour at 13 deg divergence angle
Figure 6.8 Mach number variation at 13 deg divergence angle

16. 16
DIVERGENCE ANGLE OF 15 DEGREES
Figure 6.9 Pressure contour at 15 deg divergence angle
Figure 6.10 Temperature contour at 15 deg divergence angle
Figure 6.11 Velocity contour at 15 deg divergence angle

17. 17
Figure 6.12 Mach number variation at 15 deg divergence angle
Table 6.4 Maximum and Minimum Parameter changes for 13 deg diverging angle
Temperature(K) Pressure(Pa) Velocity(m/s)
Min Max Min Max Min Max
1636 3285 1.6e4 1e7 137 2478

18. 18
Table 6.5 Maximum and Minimum Parameter changes for 15 deg diverging
angle
Temperature(K) Pressure(Pa) Velocity(m/s)
Min Max Min Max Min Max
981 3279 -6e4 1e7 148.9 2680

19. 19
CHAPTER -7
CONCLUSION
Following are the conclusion drawn from the analysis.
(1) CFD considers the factors like boundary layer effects, shock waves,
radial velocity component and so on, which leads to some variance from
theoretical results.
(2) The variation in the results of theoretical calculations and CFD are quite
insignificant.
(3) It thus establishes the fact that one-dimensional simplified nozzle
analysis is sufficient to predict the nozzle performance.
From the study conducted to assess the variation of divergence angle to the
pressure, velocity and temperature
It has been conclusively clear that as the divergence angle increases there’s a
sudden rise in velocity and thus decrease in temperature and pressure.