OpenFOAM-version-7/C3/Flow-in-a-Convergent-Divergent-Nozzle/English

Title of the script: Flow in a Convergent-Divergent Nozzle

Author: Ashley Melvin, Biraj Khadka

Keywords: OpenFOAM, ParaView, CFD, computational fluid dynamics, blockMesh, axi-symmetry, wedge geometry, spline, compressible flow, inviscid, convergent-divergent nozzle, rhoCentralFoam, shock, FOSSEE, spoken tutorial, video tutorial.

Visual Cue	Narration
Slide: Opening Slide	Welcome to the spoken tutorial on Flow in a Convergent-Divergent Nozzle.
Slide: Learning Objectives	In this tutorial, we will learn to: Create an axi-symmetric geometry using blockMesh Create spline curved edge using blockMesh, and Set up and run a case of compressible flow
Slide: System Specifications	To record this tutorial, I am using, Ubuntu Linux OS version 22.04 OpenFOAM version 9 ParaView version 5.6.3, and gedit Text editor
Slide: Prerequisites https://spoken-tutorial.org	As a prerequisite: You should have basic knowledge of compressible flows and gas dynamics. You should be familiar with setting up a case and creating a mesh in OpenFOAM. If not, please go through the prerequisite OpenFOAM tutorials on this website.
Slide: Code Files	The files used in this tutorial are available in the Code Files link on the tutorial page Please download and extract them Make a copy and then use them while practising.
Slide: Convergent-Divergent Nozzle	We will be solving flow through a convergent-divergent nozzle. Note that: at the inlet, total pressure is specified, and at the outlet, static pressure is specified.
Slide: Convergent-Divergent Nozzle	The geometry is a converging-diverging duct.
Slide: Convergent-Divergent Nozzle	Variation of the cross-sectional area is given by this cosine function along the length.
Press CTRL + ALT + T keys.	Open the terminal by pressing Ctrl, Alt and T keys together.
[Terminal] Type: cd $FOAM_RUN	At the prompt type this command and press Enter to go into the run directory.
[Terminal] Type: cp -r ~/Downloads/Nozzle .	We have downloaded and extracted the case folder. Let’s now copy it into the run directory.
[Terminal] Type: cd Nozzle	Let’s move into the case folder using the cd command.
[Terminal] Type: gedit system/blockMeshDict	Let’s open the blockMeshDict file in a text editor.
Slide: Axi-symmetric Geometry	Axi-symmetric geometry can be created in OpenFOAM using the wedge patch type. The geometry is a wedge of a small angle, usually less than 5o. It has 1 cell normal to the planes of symmetry.
Slide: Axi-symmetric Geometry	A typical wedge geometry is shown in the figure.
Slide: Axi-symmetric Geometry	The wedge geometry used for the convergent-divergent nozzle is shown in the figure.
Slide: Vertices	The geometry has 6 vertices. The vertices of the geometry are numbered as shown.
Slide: Vertex Coordinates	Let us consider the inlet plane.
Slide: Vertex Coordinates-Inlet	The inlet is along the y-z-plane at x = 0. Vertex 0 is at the origin. The cross-sectional area at the inlet is 2.5 m2. The radius at the inlet is therefore, 0.892 m. The y and z coordinates of vertex 1 are as indicated in the diagram. Similarly, the coordinates of vertex 2 are evaluated.
Slide: Vertex Coordinates-Outlet	The outlet is along the yz-plane at x = 10 and its cross-sectional area is 2.5 m2. The vertices of the outlet plane are indicated in the diagram.
[gedit - blockMeshDict] Highlight: Vertices List Link	The 6 vertices are entered in the ascending order of their vertex numbers as shown.
[gedit - blockMeshDict] Highlight: 0 3 5 2 Link	Let’s define the block. We first enter the vertices of the lower xy-plane. In this case, that would be the lower plane, when viewed along the negative z direction.
[gedit - blockMeshDict] Highlight: 0 3 4 1 Link	Similarly, the vertices of the front plane are ordered as shown.
[gedit - blockMeshDict] Highlight: 100 20 Link	The axis of the nozzle is along the x direction. There are 100 cells along the x direction and 20 cells along the y direction.
[gedit - blockMeshDict] Highlight: 1 Link	The z direction is normal to the plane of symmetry, also known as the azimuthal direction. There is only 1 cell along the z axis.
[gedit - blockMeshDict] Highlight: edges Link	We have curved edges that define the nozzle. We need to specify these edges.
Slide: Spline	Spline curves can be created in blockMesh using the keyword spline. It requires: The 2 vertices that edge connects, and The interpolation points through which edge passes
Slide: Front Edge	Let’s look at the front edge of the nozzle. Front edge connects the vertices 1 and 4.
[gedit - blockMeshDict] Highlight: spline 1 4 Link	We have used the keyword spline to indicate that a spline curve connects the vertices 1 and 4.
Slide: Interpolation Points	Let us calculate the interpolation points for the front edge: Let us calculate the coordinates of a point on the edge at x = 1. From the cosine relation, at x = 1, the cross-sectional area is 2.357 m2. The radius of the nozzle is therefore 0.866 m. We follow the same procedure as calculating the vertex coordinates earlier. The y and z coordinates are found to be 0.865 and 0.0378.
[gedit - blockMeshDict] Highlight: spline 2 5 Link	Using the same procedure, we define the spline edge connecting vertices 2 and 5.
Slide: Boundary	The boundaries of the geometry are: inlet and outlet nozzle back, and front
[gedit - blockMeshDict] Highlight: Boundaries List Link	We define the 5 boundaries as shown.
[gedit - blockMeshDict] Highlight: wedge >> wedge Link	Note that the back and front faces are of the type wedge. This indicates that the front and back faces are axi-symmetric wedge planes.
[gedit - blockMeshDict] Close the window	Close the blockMeshDict file.
[Terminal] Type: gedit 0/p	Let’s view the initial and boundary values of pressure.
[gedit - p] Highlight: internalField uniform 10000 Link	The domain is initialized with 10,000 Pa.
[gedit - p] Highlight: type totalPressure Link	At the inlet, we have the total pressure condition.
[gedit - p] Highlight: gamma 1.4 Link	Since the flow is compressible, we need to specify the ratio of specific heats. We consider the fluid to be air in this simulation. The ratio of specific heats, gamma, of air is 1.4.
[gedit - p] Highlight: p0 uniform 10000 Link	The total pressure at the inlet is set to 10,000 Pa.
[gedit - p] Highlight: value uniform 10000 Link	For the type totalPressure, value is just a placeholder for the first time-step.
[gedit - p] Highlight: back and front BC Link	The back and front faces are the axi-symmetric wedge planes. Therefore, the wedge boundary condition is used.
[gedit - p] Close the window	Close the p file.
Slide: Boundary Conditions	Let’s now look at the boundary values of temperature and velocity. They are tabulated as shown.
Slide: Boundary Conditions Highlight: slip Link	Note that slip condition is imposed at the nozzle wall as the flow is inviscid.
Slide: Thermophysical Properties	The molecular weight of air is 29 g/mol. The specific heat at constant pressure (cp) is 1005 J/kg-K. Since we don’t consider any phase change, the heat of fusion (Hf) can be taken as 0.
Slide: Transport Properties	Since the flow is inviscid, viscosity and thermal conductivity effects are ignored. Viscosity (μ) can be taken as 0, and The Prandtl number (Pr) can be taken as 1. You may assign any other non-zero value for the Prandtl number.
[Terminal] Type: gedit constant/thermophysicalProperties	Now, let’s view the thermophysicalProperties file.
[gedit - thermophysicalProperties] Highlight: Properties values Link	The thermophysical properties are entered as shown.
[gedit - thermophysicalProperties] Close the window	Close the thermophysicalProperties file.
[Terminal] Type: gedit system/controlDict	Let’s open the controlDict file.
[gedit - controlDict] Highlight: adjustTimeStep yes Link	We have enabled the adjustTimeStep. It calculates time step after every iteration based on the specified maximum Courant number.
[gedit - controlDict] Highlight: maxCo 0.9 Link	The maximum Courant number is set as 0.9.
[gedit - controlDict] Highlight: maxDeltaT 1 Link	The maximum time step is set as 1.
[gedit - controlDict] Highlight: writeControl adjustableRunTime Link	Since the time step is not constant, the write control is also made adjustable.
[gedit - controlDict] Highlight: deltaT 1e-6 Link	The first time step is 1 micro second. Value is chosen such that the Courant number is less than 0.9 for the first time step.
[gedit - controlDict] Close the window	Close the controlDict file.
[Terminal] Type: blockMesh	Let’s mesh the geometry using the blockMesh command.
Slide: rhoCentralFoam	We will be using the rhoCentralFoam solver in this simulation. It is: A density-based compressible flow solver Based on central-upwind schemes of Kurganov and Tadmor
[Terminal] Type: rhoCentralFoam	Let’s start the simulation using the following command.
Cursor in the terminal.	The simulation may take some time to complete.
[Terminal] Highlight: End	The simulation is now complete.
[Terminal] Type: paraFoam	Let’s view the simulated results in ParaView. Type paraFoam at the prompt.
[ParaView] Properties Tab Click on Apply	Click on the Apply button to view the geometry.
[ParaView] Active Variable Controls Click on vtkBlockColors >> Click on p	Let’s view the pressure contours for the simulation. Click on the vtkBlockColors dropdown in the Active Variable Controls and select p. Click on the p option with a point icon and not the box icon, in the dropdown.
[ParaView] VCR Controls Click on Last Frame	Let’s view the contours at the end of the simulation. Click on the Last Frame button in the VCR Controls. You can now see the steady-state pressure contour.
[ParaView] Active Variable Controls Click on Rescale to Data Range	Click on Rescale to Data Range
[ParaView] Layout Window Point to Shock	Notice the sudden jump in pressure in the diverging section of the nozzle. This jump indicates the presence of normal shock in the nozzle.
[ParaView] Close ParaView	Close the ParaView window.
Only Narration	With this we have come to the end of the tutorial. Let’s summarize.
Slide: Summary	In this tutorial, we have learnt to: Create an axi-symmetric geometry using blockMesh Create spline curved edge using blockMesh, and Set up and run a case of compressible flow
Slide: Assignment	As an assignment: Change the outlet pressure to 8900 Pa. Keep all the other parameters the same and run the simulation. View the steady-state pressure contour in ParaView
Slide: About the Spoken Tutorial Project	The video at the following link summarises the Spoken Tutorial project. Please download and watch it.
Slide: Spoken Tutorial Workshops	We conduct workshops using Spoken Tutorials and give certificates. Please contact us.
Slide: Spoken Tutorial Forum	Please post your timed queries in this forum.
Slide: FOSSEE Forum	Do you have any general/technical questions? Please visit the forum given in the link.
Slide: FOSSEE Case Study Project	The FOSSEE team coordinates solving feasible CFD problems of reasonable complexity using OpenFOAM. We give honorarium and certificates to those who do this. For more details, please visit these sites.
Slide: Acknowledgements	The Spoken Tutorial Project was established by the Ministry of Education, Govt. of India.
Only Narration	This tutorial is contributed by Ashutosh P. Shridhar, Binayak Lohani, Biraj Khadka and Payel Mukherjee from IIT Bombay. Thanks for joining.

Contributors and Content Editors

Biraj, Madhurig