Difference between revisions of "OpenFOAM-version-7/C3/Flow-in-a-Convergent-Divergent-Nozzle/English"

From Script | Spoken-Tutorial
Jump to: navigation, search
 
Line 154: Line 154:
 
The '''y''' and '''z coordinates''' of '''vertex 1''' are as indicated in the diagram.
 
The '''y''' and '''z coordinates''' of '''vertex 1''' are as indicated in the diagram.
  
−
Similarly, the coordinates of '''vertex 2''' are evaluated.
+
The coordinates of '''vertex 2''' are evaluated.
 
|-
 
|-
 
||'''Slide:'''
 
||'''Slide:'''
Line 209: Line 209:
  
 
'''Spline'''
 
'''Spline'''
−
||
+
|| '''Spline''' curves can be created in '''blockMesh''' using the keyword '''spline'''.
−
'''Spline''' curves can be created in '''blockMesh''' using the keyword '''spline'''.
+
  
 
It requires:
 
It requires:
  
−
The '''2 vertices''' that '''edge''' connects, and
+
* The '''2 vertices''' that '''edge''' connects, and
  
−
The '''interpolation points''' through which '''edge''' passes
+
* The '''interpolation points''' through which '''edge''' passes
 
|-
 
|-
 
|| Slide:  
 
|| Slide:  
Line 229: Line 228:
 
'''spline 1 4''' [https://imgur.com/3eURiww <span class="underline">Link</span>]
 
'''spline 1 4''' [https://imgur.com/3eURiww <span class="underline">Link</span>]
 
|| We have used the keyword '''spline''' to indicate that a '''spline''' curve connects the '''vertices 1''' and '''4'''.
 
|| We have used the keyword '''spline''' to indicate that a '''spline''' curve connects the '''vertices 1''' and '''4'''.
 +
 
|-
 
|-
 
|| Slide:
 
|| Slide:
Line 237: Line 237:
 
Let us calculate the coordinates of a point on the '''edge''' at '''x = 1'''.
 
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 m<sup>2</sup>'''.
+
From the '''cosine''' relation, at '''x = 1''', the cross-sectional area is 2.357 '''m<sup>2</sup>'''.
  
 
The radius of the '''nozzle''' is therefore '''0.866 m'''.
 
The radius of the '''nozzle''' is therefore '''0.866 m'''.
Line 385: Line 385:
 
|| We have enabled the '''adjustTimeStep'''.
 
|| We have enabled the '''adjustTimeStep'''.
  
−
It calculates '''time step''' after every iteration based on the specified '''maximum Courant number'''.
+
It calculates '''time step''' after every iteration based on the specific '''maximum Courant number'''.
 
|-
 
|-
 
||[gedit - '''controlDict'''] Highlight:
 
||[gedit - '''controlDict'''] Highlight:
Line 392: Line 392:
  
 
|| The '''maximum Courant number''' is set as '''0.9'''.
 
|| The '''maximum Courant number''' is set as '''0.9'''.
 +
 +
The time step is calculated after every iteration ensuring that the '''Courant number''' is 0.9.
 
|-
 
|-
 
|| [gedit - '''controlDict'''] Highlight:
 
|| [gedit - '''controlDict'''] Highlight:
Line 455: Line 457:
 
|| Let’s view the '''pressure contours''' for the simulation.
 
|| 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 '''vtkBlockColors''' drop down 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.
+
Click on the '''p''' option with a '''point icon''' and not the '''box icon''', in the drop down.
 
|-
 
|-
 
|| [ParaView] '''VCR Controls'''
 
|| [ParaView] '''VCR Controls'''
Line 546: Line 548:
 
|-
 
|-
 
|| Only Narration
 
|| Only Narration
−
|| This tutorial is contributed by Ashutosh P. Shridhar, Binayak Lohani, Biraj Khadka and Payel Mukherjee from IIT Bombay. Thanks for joining.
+
|| This tutorial is contributed by Ashutosh P. Shridhar, Binayak Lohani, Biraj Khadka and Payel Mukherjee from IIT Bombay.  
 +
 
 +
Thanks for joining.
 
|}
 
|}

Latest revision as of 21:59, 27 September 2024

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.

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 specific maximum Courant number.

[gedit - controlDict] Highlight:

maxCo 0.9 Link

The maximum Courant number is set as 0.9.

The time step is calculated after every iteration ensuring that the Courant number is 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 drop down in the Active Variable Controls and select p.

Click on the p option with a point icon and not the box icon, in the drop down.

[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

Retrieved from "https://script.spoken-tutorial.org/index.php?title=OpenFOAM-version-7/C3/Flow-in-a-Convergent-Divergent-Nozzle/English&oldid=56686"