78_Compressible Flow in a Nozzle

In this post, although I haven't dealt with it during my graduate studies, I aim to study fluid dynamics, which seemed interesing and I wanted to learn more about. Instead of focusing on the theoretical aspects, I plan to concentrate on using commercial software for simulations, specifically using Ansys Fluent for the simulations.

 

I'm lacking in many areas and need to learn more, so I plan to follow the guides provided by the Innovation Courses from Ansys and post about it. (https://courses.ansys.com)

 

Toady, I intend to cover the topic of compressible flow in a nozzle. The problem is as follows.

 

 

The circular corss-scetional area $A$ of this nozzle changes according to the formula $A = 0.1 + {x^2}, - 0.5 < x < 0.5$ as a function of the axial distance $x$. Here, the unit of $A$ is square meter, and $x$ is in meters. The stagnation pressure ${p_0}$ at the inlet is 101,325Pa, and the stagnation temperature ${t_0}$ is 300K. The static pressure at the exit is 3,738.9Pa.

 

The analytical goal is to calculate the Mach number, pressure, and temperature distribution within the nozzle and compare it with the results from a given one-dimensional nozzle flow. Due to the high Reynolds number associated with such high-speed flows, the viscous effects will be confined to a small area near the walls. Therefore, it should be modeled as an inviscid flow.

 

First, run the Workbench and import Fluid Flow (Fluent) into the Project Schematic.

 

 

In the properties of Geometry, change the Analysis Type to 2D and click on New SpaceClaim Geometry. Change the unit of length to meters and set the Minor grid spacing to 0.1m.

In the Sketch's XY plane, select Equation and set the Curve Type to Custom, the limits of $t$ to -0.5 to 0.5, and the Change Scale to 1000. Afterward, modify $y$ to ${\text{Sqrt}}\left( {\left( {[t]*[t] + 0.1} \right)/3.1416} \right)$ to generate the following curve.

 

 

Then, connect both ends of the curve down to the x-axis to create a closed shape and save it.

 

In the Project Schematic, right-click on Mesh to enter Edit, then select Face Meshing. Set the Element Size to 0.025m and generate the mesh.

 

 

In the Setup under Mesh, check the Double Prescision option and change to Parallel, setting the Number of Processes to 2. In the Solver, set the Type to Desity-Based and 2D Space to Axisymmetric. In the Model, turn Energy On, and set the Viscous model to Inviscid. The reason for setting it to Inviscid is because the Reynolds number is high enough to neglect viscosity.

 

In Materials, change the Fluid Properties to ideal-gas. In Boundary Conditions, set the Gauge Pressure of the Pressure Outlet to 3738.9, the Gauge Total Pressure of the pressure_inlet to 101325, and the SUpersonic/Initial Gauge Pressure to 99348. Finally, set the operating pressure of the pressure_inlet to 0.

 

 

In the Solution settings, set the Gradient and FLow methods to Least Squares Cell Based and Second Order Upwind, respectively. Configure the initialization to start from the inlet and proceed with the calculation to obtain the following results.

 

 

Using the Graphics in the Results, visualizing the Mach number will yield the following representation.

 

 

Additionally, representing the total pressure will yield the following.

 

 

In the XY Plot, representing the Static Pressure applied to the axis and nozzle_wall will yield the following.

 

 

At the inlet, it is the highest and can be seen to decrease sharply as it passes through the interior.

 

 

On the other hand, the Mach number can be observed to increase sharply as it passes through the interior.