Script | Spoken-Tutorial - User contributions [en]

OpenFOAM-version-7/C2/Setting-up-a-Test-Case-in-OpenFOAM/English

2020-09-17T06:03:48Z

Ashleymelvin:

'''Title of the script''': Setting-up a test case in OpenFOAM

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM, ParaView, lid driven cavity, pre-processing, blockMesh, controlDict, post-processing, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Setting up a test case in OpenFOAM'''.
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn to:
* Set up a '''case''' in '''OpenFOAM'''
* Access the '''case files''' using '''terminal'''
* '''Pre-process''' a '''case'''
* '''Run''' a '''case''', and
* '''Post-process''' a '''case'''
|-
|| Slide: System Specifications
|| This tutorial is recorded using,
* '''Ubuntu Linux''' OS version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0, and
* '''gedit Text editor'''

You may use any other '''text editor''' of your choice.
|-
|| Slide: Prerequisites

|| As a prerequisite:
* You should be familiar with basic '''Linux commands'''.
* If not, please go through the prerequisite '''Linux '''tutorials on this website.
|-
|| Slide: Lid Driven Cavity
|| In this tutorial, we will learn to set up the '''lid driven cavity case'''.

'''Lid driven cavity''' is one of the most widely used '''2D test cases''' for the validation of a '''CFD '''code.
|-
|| Slide: Diagram
|| This is the diagram of '''Lid Driven Cavity Flow'''.

It consists of 3 fixed walls and a moving top wall.
|-
|| Highlight '''Terminal''' on the machine
|| Open a '''terminal''' by pressing the '''Ctrl, Alt '''and''' T''' keys together.
|-
|| Only Narration
|| Here onwards please remember to press the '''Enter''' key after typing each '''command'''.
|-
|| [Terminal] Type:
'''mkdir -p $FOAM_RUN'''
|| Now, let’s create a '''RUN directory'''.

To do so, type the '''command''' as shown.
|-
|| [Terminal] Highlight

'''FOAM_RUN'''
|| '''Tutorial cases''' will later be copied into the '''RUN directory'''.
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| Go to the '''RUN directory''' using the '''cd command'''.

Now our present working directory is the '''RUN directory'''.
|-
|| Only Narration
|| '''OpenFOAM''' installation comes with a set of '''test cases'''.

The '''tutorials directory''' contains these '''test cases'''.

The '''Lid driven cavity case''' already exists inside the '''tutorials directory'''.
|-
|| [Terminal] Type:

'''cp -r $FOAM_TUTORIALS/incompressible/icoFoam/cavity/cavity .'''
|| We’ll now copy the '''Lid driven cavity case''' from the '''tutorials directory''' into the '''RUN directory'''.

To do so, type the following '''command'''.
|-
|| Slide: blockMesh
||
* The '''mesh generator''' for '''OpenFOAM''' is a utility called '''blockMesh'''.
* The '''input dictionary''' for '''blockMesh''' utility is '''blockMeshDict'''.
|-
|| [Terminal] Type:

'''gedit cavity/system/blockMeshDict'''
|| The '''blockMeshDict''' file is located in the '''system''' folder.

Open the '''blockMeshDict''' file in a '''text editor'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight

vertices, blocks, edges and boundary
|| Now let’s look at the contents of the file.

The '''blockMeshDict''' contains details of the geometry like vertices, blocks, edges and boundaries.
|-
|| [gedit - '''blockMeshDict'''] Close the window
|| Close the '''blockMeshDict''' file.
|-
|| [Terminal] Type:

'''cd cavity/0'''
|| The '''0''' folder contains the '''initial''' and '''boundary conditions''' for the '''simulation'''.

Type the following '''command''' to move into the '''0''' folder inside the '''cavity case directory'''.
|-
|| [Terminal] Type:

'''ls'''
|| Type '''ls''' and press '''Enter''' to view the files in the '''0''' folder.
|-
|| [Terminal] Highlight

'''p''' and '''U'''
|| The '''0''' folder contains the '''kinematic pressure file p''' and the '''velocity file U'''.
|-
|| [Terminal] Type:

'''gedit p'''
|| Open the '''kinematic pressure file p''' in a '''text editor'''.
|-
|| Only Narration
|| The '''p''' file contains the '''initial''' and '''boundary conditions''' of '''kinematic pressure'''.
|-
|| [gedit - '''p'''] Highlight

'''dimensions [0 2 -2 0 0 0 0] '''
|| The '''dimensions''' of '''kinematic pressure''' is meter squared per second squared.
|-
|| [gedit - '''p'''] Highlight

'''internalField '''
|| The '''internalField''' defines the values in the interior of the domain.
|-
|| [gedit - '''p'''] Highlight

'''uniform 0'''
|| The initial field is set as '''0 kinematic pressure'''.

This field is '''uniform''' across the domain.
|-
|| [gedit - '''p'''] Highlight

Both the '''zeroGradient'''
|| You can see that all walls are imposed with a '''zero gradient pressure boundary condition'''.
|-
|| [gedit - '''p'''] Close the window
|| Let us close the '''p''' file.
|-
|| [Terminal] Type:

'''gedit U'''
|| Now open the '''velocity file U''' in a '''text editor'''.
|-
|| Only Narration
|| The '''U file''' contains the '''initial''' and '''boundary conditions''' of '''velocity'''.
|-
|| [gedit - '''U'''] Highlight

'''uniform (1 0 0);'''
|| You can see that the moving wall is imposed with a '''velocity''' of '''1 m/s''' in the x direction.
|-
|| [gedit - '''U'''] Highlight

'''noSlip '''
|| Also notice that the '''no-slip condition''' is imposed on the three fixed walls.
|-
|| [gedit - '''U'''] Close the window
|| Now let us close the '''U''' file.
|-
|| [Terminal] Type:

'''cd ..'''
|| We’ll go back to the '''cavity''' folder.

Type '''cd (space)(dot)(dot)'''
|-
|| [Terminal] Type:

'''gedit constant/transportProperties'''
|| Next, we will view the '''transport properties file '''which is in the '''constant '''folder.
|-
|| [gedit - '''transportProperties'''] Highlight

'''nu '''
|| The '''transportProperties''' file contains the details of '''kinematic viscosity'''.
|-
|| [gedit - '''transportProperties''']

Highlight '''[0 2 -1 0 0 0 0] '''
|| The dimensions of '''kinematic viscosity''' is meter squared per second.
|-
|| Slide: Kinematic Viscosity
||
The '''kinematic viscosity''' is defined by:
'''''nu'' equals magnitude of ''U'' times ''d'' by ''Re'''''

where
*'''velocity''' is '''1 m per second'''
*characteristic length is '''0.1 meters'''

The '''Reynolds number (Re)''' for the '''flow''' is taken as '''10'''.

The '''kinematic viscosity''' is therefore '''0.01 meter squared per second'''
|-
|| Narration Only
|| Now let me switch back to '''transportProperties''' file.
|-
|| [gedit - '''transportProperties''']

Highlight '''0.01'''
|| The value of '''kinematic viscosity''' is indicated in the '''transportProperties''' file.
|-
|| [gedit - '''transportProperties'''] Close the window
|| Close the '''transportProperties''' file.
|-
|| [Terminal] Type:

'''cd system'''
|| To move into the '''system''' folder, type the following '''command'''.
|-
|| [Terminal] Type:

'''ls'''
|| Type '''ls''' to view the contents of the '''system''' folder.
|-
|| [Terminal] Highlight

'''blockMeshDict controlDict fvSchemes fvSolution'''
|| The '''system''' folder contains the following files:

'''blockMeshDict, controlDict, fvSchemes''' and '''fvSolution'''.
|-
|| [Terminal] Highlight

'''fvSchemes'''
|| The '''fvSchemes dictionary''' contains the '''finite volume discretisation schemes'''.
|-
|| [Terminal] Highlight

'''fvSolution'''
|| The '''fvSolution dictionary''' contains the '''linear equation solvers''' and '''tolerances'''.

It contains other '''algorithm controls''' as well.
|-
|| [Terminal] Highlight

'''controlDict'''
|| The '''controlDict dictionary''' contains the '''simulation control parameters'''.

The '''dictionary''' input includes the '''control''' of '''time''' and '''reading''' and '''writing''' of the '''solution data'''.
|-
|| [Terminal] Type:

'''gedit controlDict'''
|| Let’s open the '''controlDict''' file in a '''text editor'''.
|-
|| [Terminal] Highlight

'''startFrom '''and '''startTime'''
|| The '''start '''and''' stop times''' and the '''time step''' for the '''run''' must be set.
|-
|| [gedit - '''controlDict'''] Highlight

'''startTime''' '''0;'''
|| The '''start time''' is set at '''0''' seconds.
|-
|| [gedit - '''controlDict'''] Highlight

'''stopAt''' '''endTime;'''
|| The time at which the '''simulation''' stops, is specified using the '''keyword stopAt'''.

Here, '''stopAt''' is specified using the keyword '''endTime'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''endTime''' '''0.5;'''
|| The '''endTime''' is set at '''0.5 seconds'''.

This means that '''simulation''' stops after '''0.5 seconds'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''deltaT 0.005;'''
|| The value of the '''keyword deltaT''' defines the '''time step''' for the '''simulation'''.

The '''time step''' for the current '''simulation''' is set as '''0.005 seconds'''.

'''Temporal accuracy''' and '''numerical stability''' is essential while running the '''simulation'''.

To achieve this, a''' Courant number''' of less than 1 is required.

Keeping this in mind, the '''time step''' is set to '''0.005 seconds'''.

Please refer to the '''additional reading material''' on this tutorial page for details.

It mentions the steps used to calculate the '''time-step'''.
|-
|-
|-
|| [gedit - '''controlDict'''] Highlight

'''application''' '''icoFoam'''<nowiki>;</nowiki>
|| '''icoFoam''' is the '''OpenFOAM solver''' used to '''simulate''' the '''lid driven cavity flow'''.
|-
|| [gedit - '''controlDict'''] Close the window
|| Close the '''controlDict''' file.
|-
|| [Terminal] Type:

'''cd ..'''
|| Go back to the '''cavity''' folder using '''cd command'''.
|-
|| [Terminal] Type:

'''blockMesh''' >> '''Enter'''
|| Type the '''command blockMesh''' and press '''Enter''' to '''mesh''' the geometry.

The '''command''' takes input from the '''blockMeshDict dictionary''' and creates the geometry and '''meshes''' it.
|-
|| [Terminal] Highlight '''End'''
|| The '''meshing''' is now complete.
|-
|| [Terminal] Type:

'''icoFoam'''
|| The '''lid driven cavity flow''' is an '''incompressible flow'''.

It is solved using the''' OpenFOAM solver icoFoam.'''

To start the '''simulation''', type '''icoFoam''' in the '''terminal.'''
|-
|| [Terminal] Highlight '''End'''
|| The iterations are now complete.
|-
|| [Terminal] Type:

'''paraFoam'''
|| Let us view the '''simulated''' results in '''ParaView'''.

So, type '''paraFoam''' in the '''terminal.'''
|-
|| [ParaView] '''Properties''' Tab

Click on '''Apply'''
|| In the '''ParaView''' window, go to the '''Properties''' tab on the left.

Then click on the green coloured '''Apply '''button.
|-
|| [ParaView]

Click on '''vtkBlockColors''' >> Click on '''U'''
|| Go to the '''Active Variable Controls '''at the top.

Click on the '''vtkBlockColors''' dropdown and select '''U'''.

Ensure that you click on the '''U''' option with a '''point icon''' and not the '''box icon''', in the dropdown.

The '''box icon''' would display '''contours''' without any grading.
|-
|| [ParaView]

Velocity Contours in the Layout
|| The '''velocity contour''' at the start of the '''simulation''' is now displayed in the''' layout'''.
|-
|| [ParaView]

Go to '''VCR Controls''' and click on the '''Play''' Button
|| Let us see how the '''velocity contours''' develop through the '''simulation'''.

To do so, go to the '''VCR Controls''' and click on the '''Play''' button.
|-
|| [ParaView]

Final Velocity Contours in the Layout
|| The '''velocity contour''' at the end of the '''simulation''' is now displayed in the''' layout'''.
|-
|| [ParaView] Close the Window
|| Close the '''ParaView''' window.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

|-
|| Slide: Summary
|| To summarise, in this tutorial we have learnt to:
* Set up a''' case''' in '''OpenFOAM'''
* Access the '''case files''' using '''terminal'''
* '''Pre-process''' a '''case'''
* '''Run''' a '''case''', and
* '''Post-process''' a '''case'''
|-
|| 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 this 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley Melvin.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Overiew-of-OpenFOAM-7/English

2020-09-08T21:07:35Z

Ashleymelvin:

'''Title of the script''': Overview of OpenFOAM

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM version 7, ParaView, CFD, computational fluid dynamics, blockMesh, snappyHexMesh, solver, FOSSEE, spoken tutorial, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Overview of OpenFOAM'''.
|-
|| Slide: Learning Objective

|| In this tutorial, we will learn about:

* '''OpenFOAM''' and its capabilities
* Basic '''OpenFOAM''' utilities, and
* The content available in various tutorials in this series

|-
|| Slide: Prerequisites

|| To work with '''OpenFOAM''' you should have basic knowledge of''' computational fluid dynamics'''.
|-
|| Slide: System Specifications

|| Throughout this series, we will be using:

* '''Ubuntu Linux''' OS version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0, and
* '''gedit Text editor'''

However, you may use any other '''text editor''' of your choice.
|-
|| Slide: About OpenFOAM®

|| '''OpenFOAM®''' stands for
* '''Open source Field Operation And Manipulation'''
* It is licensed under '''GNU General Public Licence '''by '''OpenCFD Ltd'''.

Henceforth, in this series, whenever '''OpenFOAM''' is mentioned it indicates '''OpenFOAM®'''.
|-
|| Slide: About OpenFOAM
||
* '''OpenFOAM''' is an '''Open source Computational Fluid Dynamics''' software.
* It is a '''CFD toolbox''' written in '''C++'''.
* It has an '''Object Oriented Programming''' interface.
* '''OpenFOAM''' is available for '''Linux''', '''Mac''' and '''Windows''' operating systems.

|-
|| Slide: OpenFOAM Capabilities
||
* '''OpenFOAM''' is a '''Finite Volume '''based''' CFD''' software.
* It uses both
** '''Structured''', and
** '''Unstructured '''grid

|-
|| Slide: Mesh Generation
||
* '''OpenFOAM''' has an '''in-built mesh''' '''generation tool''' called '''blockMesh'''.
* It is used for '''structured meshing''' of simple geometries.
* '''OpenFOAM''' also has an advanced '''meshing tool''' called '''snappyHexMesh'''.

|-
|| Slide: Mesh Conversion
|| '''OpenFOAM''' allows importing '''mesh''' from other '''packages''' like:

* '''ANSYS''',
* '''Fluent''',
* '''CFX''',
* '''Gmsh''',
* '''STAR-CD''' etc.

Imported '''mesh''' can be converted to the format '''OpenFOAM''' uses.

For example, a '''fluent mesh''' is converted using the '''fluentMeshToFoam''' utility.
|-
|| Slide: Solvers
|| Using '''OpenFOAM''' one can solve problems in:
* '''Incompressible flows'''
* '''Compressible flows'''
* '''Multiphase flows'''
* '''Heat transfer'''
* '''Combustion systems'''
* '''Molecular dynamics'''
* '''Magnetohydrodynamic flows'''

and many other domains.
|-
|| Slide: ParaView
||
* Visualizing the simulated results comes under the '''post-processing''' stage.
* '''ParaView''' is the most commonly used software for '''post-processing OpenFOAM''' results.

|-
|| Only Narration
|| Now, let’s briefly go through various tutorials available in this series.
|-
|| Glimpse of Installing OpenFOAM in Ubuntu

(01: 50 - 01:55)
|| We first have the tutorial on installing '''OpenFOAM''' and '''ParaView''' in '''Ubuntu Linux OS'''.
|-
|| Glimpse of Setting-up a Test Case in OpenFOAM

(04:20 - 04:25) >> (10:06 - 10:11)
|| After this, we’ll see how to set up and view the files of an '''OpenFOAM case'''.

We’ll also see how to '''run''' the '''case''' and visualise the results in '''ParaView'''.
|-
|| Glimpse of Creating a 2D channel geometry in OpenFOAM

(05:40 - 05:45) >> (10:25 - 10:30)
|| In the next tutorial, we’ll see how to create a geometry and '''mesh''' using the '''blockMesh''' utility.

We’ll also see how to view the '''mesh''' in '''ParaView'''.
|-
|| Glimpse of Multi-block Meshing of 2D Geometry in OpenFOAM

(03:17 - 03:22) >> (09:31 - 09:36)
|| This is followed by the tutorial on creating a geometry with multiple '''blocks'''.

We’ll see how to '''mesh''' each '''block''' separately and '''refine cells''' locally.
|-
|| Glimpse of Creating 3D pipe geometry and mesh in OpenFOAM

(02:05 - 02:10) >> (06:14 - 06:19)
|| Next, we’ll see how to create a '''mesh''' for a cylindrical pipe.

We’ll see how '''curved edges''' are defined using the '''blockMesh''' utility.
|-
|| Glimpse of Simulating Hagen-Poiseuille flow through a Pipe

(07:20 - 07:25) >> (12:04 - 12:09)
|| Then, we’ll simulate the '''flow''' through a pipe.

We’ll also compare the results from '''simulation''' with the analytical solution.
|-
|| Glimpse of Basic Post-processing using ParaView

(04:23 - 04:26) >> (07:00 - 07:05)
|| The results from the '''pipe flow simulation''' are viewed in detail in '''ParaView''' in this tutorial.

We’ll also see how to '''plot''' the results in '''ParaView'''.
|-
|| Glimpse of Simulation of Turbulent Flow in a 2D Channel in OpenFOAM

(07:00 - 07:05)
|| In the next tutorial, we’ll learn how to use a '''turbulence model''' in a '''simulation'''.
|-
|| Glimpse of Turbulence Modelling in OpenFOAM

(12:00 - 12:05)
|| We will then compare the results from a '''simulation''' using three different '''turbulence models'''.
|-
|| Glimpse of Grid Resolution and Convergence in OpenFOAM

(07:53 - 07:58)
|| We also have a tutorial detailing the steps to establish '''grid independence'''.
|-
|| OpenFOAM version 7 Spoken Tutorial Page
|| Later on, there will be more tutorials in this series.

Please check the '''Spoken Tutorial website''' regularly for the latest topics.
|-
|| Only Narration
|| With this we have come to the end of this tutorial.

Let’s summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt about:
* '''OpenFOAM''' and its capabilities
* Basic '''OpenFOAM''' utilities, and
* The content available in various tutorials in this series

|-
|| 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

||
* Do you have questions in THIS Spoken Tutorial?
* Please visit this site.
* Choose the minute and second where you have the question
* Explain your question briefly
* Someone from our team will answer them
* You will have to register on this website to ask questions.

|-
|| Slide: Forum to answer questions
||
* Do you have any general/technical questions?
* Please visit the forum given in this link.

|-
|| Slide: Textbook Companion
||
* 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: Acknowledgment
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley Melvin.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Overiew-of-OpenFOAM-7/English

2020-09-08T20:32:32Z

Ashleymelvin:

'''Title of the script''': Overview of OpenFOAM

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM version 7, ParaView, CFD, computational fluid dynamics, blockMesh, snappyHexMesh, solver, FOSSEE, spoken tutorial, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Overview of OpenFOAM'''.
|-
|| Slide: Learning Objective

|| In this tutorial, we will learn about:

* '''OpenFOAM''' and its capabilities
* Basic '''OpenFOAM''' utilities, and
* The content available in various tutorials in this series

|-
|| Slide: Prerequisites

|| To work with '''OpenFOAM''' you should have basic knowledge of''' computational fluid dynamics'''.
|-
|| Slide: System Specifications

|| Throughout this series, we will be using:

* '''Ubuntu Linux''' OS version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0, and
* '''gedit Text editor'''

However, you may use any other '''text editor''' of your choice.
|-
|| Slide: About OpenFOAM®

|| '''OpenFOAM®''' stands for
* '''Open source Field Operation And Manipulation'''
* It is licensed under '''GNU General Public Licence '''by '''OpenCFD Ltd'''.

Henceforth, in this series, whenever '''OpenFOAM''' is mentioned it indicates '''OpenFOAM®'''.
|-
|| Slide: About OpenFOAM
||
* '''OpenFOAM''' is an '''Open source Computational Fluid Dynamics''' software.
* It is a '''CFD toolbox''' written in '''C++'''.
* It has an '''Object Oriented Programming''' interface.
* '''OpenFOAM''' is available for '''Linux''', '''Mac''' and '''Windows''' operating systems.

|-
|| Slide: OpenFOAM Capabilities
||
* '''OpenFOAM''' is a '''Finite Volume '''based''' CFD''' software.
* It uses both
** '''Structured''', and
** '''Unstructured '''grid

|-
|| Slide: Mesh Generation
||
* '''OpenFOAM''' has an '''in-built mesh''' '''generation tool''' called '''blockMesh'''.
* It is used for '''structured meshing''' of simple geometries.
* '''OpenFOAM''' also has an advanced '''meshing tool''' called '''snappyHexMesh'''.

|-
|| Slide: Mesh Conversion
|| '''OpenFOAM''' allows importing '''mesh''' from other '''packages''' like:

* '''ANSYS''',
* '''Fluent''',
* '''CFX''',
* '''Gmsh''',
* '''STAR-CD''' etc.

Imported '''mesh''' can be converted to the format '''OpenFOAM''' uses.

For example, a '''fluent mesh''' is converted using the '''fluentMeshToFoam''' utility.
|-
|| Slide: Solvers
|| Using '''OpenFOAM''' one can solve problems in:
* '''Incompressible flows'''
* '''Compressible flows'''
* '''Multiphase flows'''
* '''Heat transfer'''
* '''Combustion systems'''
* '''Molecular dynamics'''
* '''Magnetohydrodynamic flows'''

and many other domains.
|-
|| Slide: ParaView
||
* Visualizing the simulated results comes under the '''post-processing''' stage.
* '''ParaView''' is the most commonly used software for '''post-processing OpenFOAM''' results.

|-
|| Only Narration
|| Now, let’s briefly go through various tutorials available in this series.
|-
|| Glimpse of Installing OpenFOAM in Ubuntu

(01: 50 - 01:55)
|| We first have the tutorial on installing '''OpenFOAM''' and '''ParaView''' in '''Ubuntu Linux OS'''.
|-
|| Glimpse of Setting-up a Test Case in OpenFOAM

(04:20 - 04:25) >> (10:06 - 10:11)
|| After this, we’ll see how to set up and view the files of an '''OpenFOAM case'''.

We’ll also see how to '''run''' the '''case''' and visualise the results in '''ParaView'''.
|-
|| Glimpse of Creating a 2D channel geometry in OpenFOAM

(05:40 - 05:45) >> (10:25 - 10:30)
|| In the next tutorial, we’ll see how to create a geometry and '''mesh''' using the '''blockMesh''' utility.

We’ll also see how to view the '''mesh''' in '''ParaView'''.
|-
|| Glimpse of Multi-block Meshing of 2D Geometry in OpenFOAM

(03:17 - 03:22) >> (09:31 - 09:36)
|| This is followed by the tutorial on creating a geometry with multiple '''blocks'''.

We’ll see how to '''mesh''' each '''block''' separately and '''refine cells''' locally.
|-
|| Glimpse of Creating 3D pipe geometry and mesh in OpenFOAM

(02:05 - 02:10) >> (06:14 - 06:19)
|| Next, we’ll see how to create a '''mesh''' for a cylindrical pipe.

We’ll see how '''curved edges''' are defined using the '''blockMesh''' utility.
|-
|| Glimpse of Simulating Hagen-Poiseuille flow through a Pipe

(07:20 - 07:25) >> (12:04 - 12:09)
|| Then, we’ll simulate the '''flow''' through a pipe.

We’ll also compare the results from '''simulation''' with the analytical solution.
|-
|| Glimpse of Basic Post-processing using ParaView

(04:23 - 04:26) >> (07:00 - 07:05)
|| The results from the '''pipe flow simulation''' are viewed in detail in '''ParaView''' in this tutorial.

We’ll also see how to '''plot''' the results in '''ParaView'''.
|-
|| Glimpse of Simulation of Turbulent Flow in a 2D Channel in OpenFOAM

(07:00 - 07:05)
|| In the next tutorial, we’ll learn how to use a '''turbulence model''' in a '''simulation'''.
|-
|| Glimpse of Turbulence Modelling in OpenFOAM

(12:00 - 12:05)
|| We will then compare the results from a '''simulation''' using three different '''turbulence models'''.
|-
|| Glimpse of Grid Resolution and Convergence in OpenFOAM

(07:53 - 07:58)
|| We also have a tutorial detailing the steps to establish '''grid independence'''.
|-
|| Only Narration
|| Later on, there will be more tutorials in this series.

Please check the '''Spoken Tutorial website''' regularly for the latest topics.
|-
|| OpenFOAM version 7 Spoken Tutorial Page
|| With this we have come to the end of this tutorial.

Let’s summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt about:
* '''OpenFOAM''' and its capabilities
* Basic '''OpenFOAM''' utilities, and
* The content available in various tutorials in this series

|-
|| 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

||
* Do you have questions in THIS Spoken Tutorial?
* Please visit this site.
* Choose the minute and second where you have the question
* Explain your question briefly
* Someone from our team will answer them
* You will have to register on this website to ask questions.

|-
|| Slide: Forum to answer questions
||
* Do you have any general/technical questions?
* Please visit the forum given in this link.

|-
|| Slide: Textbook Companion
||
* 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: Acknowledgment
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley Melvin.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Overiew-of-OpenFOAM-7/English

2020-09-08T20:29:57Z

Ashleymelvin:

'''Title of the script''': Overview of OpenFOAM

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM version 7, ParaView, CFD, computational fluid dynamics, blockMesh, snappyHexMesh, solver, FOSSEE, spoken tutorial, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Overview of OpenFOAM'''.
|-
|| Slide: Learning Objective

|| In this tutorial, we will learn about:

* '''OpenFOAM''' and its capabilities
* Basic '''OpenFOAM''' utilities, and
* The content available in various tutorials in this series

|-
|| Slide: Prerequisites

|| To work with '''OpenFOAM''' you should have basic knowledge of''' computational fluid dynamics'''.
|-
|| Slide: System Specifications

|| Throughout this series, we will be using:

* '''Ubuntu Linux''' OS version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0, and
* '''gedit Text editor'''

However, you may use any other '''text editor''' of your choice.
|-
|| Slide: About OpenFOAM®

|| '''OpenFOAM®''' stands for * '''Open source Field Operation And Manipulation'''
* It is licensed under '''GNU General Public Licence '''by '''OpenCFD Ltd'''.

Henceforth, in this series, whenever '''OpenFOAM''' is mentioned it indicates '''OpenFOAM®'''.
|-
|| Slide: About OpenFOAM
||
* '''OpenFOAM''' is an '''Open source Computational Fluid Dynamics''' software.
* It is a '''CFD toolbox''' written in '''C++'''.
* It has an '''Object Oriented Programming''' interface.
* '''OpenFOAM''' is available for '''Linux''', '''Mac''' and '''Windows''' operating systems.

|-
|| Slide: OpenFOAM Capabilities
||
* '''OpenFOAM''' is a '''Finite Volume '''based''' CFD''' software.
* It uses both
** <div style="margin-left:2.54cm;margin-right:0cm;">'''Structured''', and
** <div style="margin-left:2.54cm;margin-right:0cm;">'''Unstructured '''grid

|-
|| Slide: Mesh Generation
||
* '''OpenFOAM''' has an '''in-built mesh''' '''generation tool''' called '''blockMesh'''.
* It is used for '''structured meshing''' of simple geometries.
* '''OpenFOAM''' also has an advanced '''meshing tool''' called '''snappyHexMesh'''.

|-
|| Slide: Mesh Conversion
|| '''OpenFOAM''' allows importing '''mesh''' from other '''packages''' like:

* '''ANSYS''',
* '''Fluent''',
* '''CFX''',
* '''Gmsh''',
* '''STAR-CD''' etc.

Imported '''mesh''' can be converted to the format '''OpenFOAM''' uses.

For example, a '''fluent mesh''' is converted using the '''fluentMeshToFoam''' utility.
|-
|| Slide: Solvers
|| Using '''OpenFOAM''' one can solve problems in:
* '''Incompressible flows'''
* '''Compressible flows'''
* '''Multiphase flows'''
* '''Heat transfer'''
* '''Combustion systems'''
* '''Molecular dynamics'''
* '''Magnetohydrodynamic flows'''

and many other domains.
|-
|| Slide: ParaView
||
* Visualizing the simulated results comes under the '''post-processing''' stage.
* '''ParaView''' is the most commonly used software for '''post-processing OpenFOAM''' results.

|-
|| Only Narration
|| Now, let’s briefly go through various tutorials available in this series.
|-
|| Glimpse of Installing OpenFOAM in Ubuntu

(01: 50 - 01:55)
|| We first have the tutorial on installing '''OpenFOAM''' and '''ParaView''' in '''Ubuntu Linux OS'''.
|-
|| Glimpse of Setting-up a Test Case in OpenFOAM

(04:20 - 04:25) >> (10:06 - 10:11)
|| After this, we’ll see how to set up and view the files of an '''OpenFOAM case'''.

We’ll also see how to '''run''' the '''case''' and visualise the results in '''ParaView'''.
|-
|| Glimpse of Creating a 2D channel geometry in OpenFOAM

(05:40 - 05:45) >> (10:25 - 10:30)
|| In the next tutorial, we’ll see how to create a geometry and '''mesh''' using the '''blockMesh''' utility.

We’ll also see how to view the '''mesh''' in '''ParaView'''.
|-
|| Glimpse of Multi-block Meshing of 2D Geometry in OpenFOAM

(03:17 - 03:22) >> (09:31 - 09:36)
|| This is followed by the tutorial on creating a geometry with multiple '''blocks'''.

We’ll see how to '''mesh''' each '''block''' separately and '''refine cells''' locally.
|-
|| Glimpse of Creating 3D pipe geometry and mesh in OpenFOAM

(02:05 - 02:10) >> (06:14 - 06:19)
|| Next, we’ll see how to create a '''mesh''' for a cylindrical pipe.

We’ll see how '''curved edges''' are defined using the '''blockMesh''' utility.
|-
|| Glimpse of Simulating Hagen-Poiseuille flow through a Pipe

(07:20 - 07:25) >> (12:04 - 12:09)
|| Then, we’ll simulate the '''flow''' through a pipe.

We’ll also compare the results from '''simulation''' with the analytical solution.
|-
|| Glimpse of Basic Post-processing using ParaView

(04:23 - 04:26) >> (07:00 - 07:05)
|| The results from the '''pipe flow simulation''' are viewed in detail in '''ParaView''' in this tutorial.

We’ll also see how to '''plot''' the results in '''ParaView'''.
|-
|| Glimpse of Simulation of Turbulent Flow in a 2D Channel in OpenFOAM

(07:00 - 07:05)
|| In the next tutorial, we’ll learn how to use a '''turbulence model''' in a '''simulation'''.
|-
|| Glimpse of Turbulence Modelling in OpenFOAM

(12:00 - 12:05)
|| We will then compare the results from a '''simulation''' using three different '''turbulence models'''.
|-
|| Glimpse of Grid Resolution and Convergence in OpenFOAM

(07:53 - 07:58)
|| We also have a tutorial detailing the steps to establish '''grid independence'''.
|-
|| Only Narration
|| Later on, there will be more tutorials in this series.

Please check the '''Spoken Tutorial website''' regularly for the latest topics.
|-
|| OpenFOAM version 7 Spoken Tutorial Page
|| With this we have come to the end of this tutorial.

Let’s summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt about:
* '''OpenFOAM''' and its capabilities
* Basic '''OpenFOAM''' utilities, and
* The content available in various tutorials in this series

|-
|| 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

||
* Do you have questions in THIS Spoken Tutorial?
* Please visit this site.
* Choose the minute and second where you have the question
* Explain your question briefly
* Someone from our team will answer them
* You will have to register on this website to ask questions.

|-
|| Slide: Forum to answer questions
||
* Do you have any general/technical questions?
* Please visit the forum given in this link.

|-
|| Slide: Textbook Companion
||
* 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: Acknowledgment
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley Melvin.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Overiew-of-OpenFOAM-7/English

2020-09-08T20:14:54Z

Ashleymelvin: Created page with "'''Title of the script''': Overview of OpenFOAM '''Author''': Ashley Melvin '''Keywords''': OpenFOAM version 7, ParaView, CFD, computational fluid dynamics, blockMesh, snapp..."

'''Title of the script''': Overview of OpenFOAM

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM version 7, ParaView, CFD, computational fluid dynamics, blockMesh, snappyHexMesh, solver, FOSSEE, spoken tutorial, video tutorial

{|
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Overview of OpenFOAM'''.
|-
|| Slide: Learning Objective

|| In this tutorial, we will learn about:

* '''OpenFOAM''' and its capabilities
* Basic '''OpenFOAM''' utilities, and
* The content available in various tutorials in this series

|-
|| Slide: Prerequisites

|| To work with '''OpenFOAM''' you should have basic knowledge of''' computational fluid dynamics'''.
|-
|| Slide: System Specifications

|| Throughout this series, we will be using:

* '''Ubuntu Linux''' OS version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0, and
* '''gedit Text editor'''

However, you may use any other '''text editor''' of your choice.
|-
|| Slide: About OpenFOAM®

|| '''OpenFOAM®''' stands for * '''Open source Field Operation And Manipulation'''
* It is licensed under '''GNU General Public Licence '''by '''OpenCFD Ltd'''.

Henceforth, in this series, whenever '''OpenFOAM''' is mentioned it indicates '''OpenFOAM®'''.
|-
|| Slide: About OpenFOAM
||
* '''OpenFOAM''' is an '''Open source Computational Fluid Dynamics''' software.
* It is a '''CFD toolbox''' written in '''C++'''.
* It has an '''Object Oriented Programming''' interface.
* '''OpenFOAM''' is available for '''Linux''', '''Mac''' and '''Windows''' operating systems.

|-
|| Slide: OpenFOAM Capabilities
||
* '''OpenFOAM''' is a '''Finite Volume '''based''' CFD''' software.
* It uses both
** <div style="margin-left:2.54cm;margin-right:0cm;">'''Structured''', and
** <div style="margin-left:2.54cm;margin-right:0cm;">'''Unstructured '''grid

|-
|| Slide: Mesh Generation
||
* '''OpenFOAM''' has an '''in-built mesh''' '''generation tool''' called '''blockMesh'''.
* It is used for '''structured meshing''' of simple geometries.
* '''OpenFOAM''' also has an advanced '''meshing tool''' called '''snappyHexMesh'''.

|-
|| Slide: Mesh Conversion
|| '''OpenFOAM''' allows importing '''mesh''' from other '''packages''' like:

* '''ANSYS''',
* '''Fluent''',
* '''CFX''',
* '''Gmsh''',
* '''STAR-CD''' etc.

Imported '''mesh''' can be converted to the format '''OpenFOAM''' uses.

For example, a '''fluent mesh''' is converted using the '''fluentMeshToFoam''' utility.
|-
|| Slide: Solvers
|| Using '''OpenFOAM''' one can solve problems in:
* '''Incompressible flows'''
* '''Compressible flows'''
* '''Multiphase flows'''
* '''Heat transfer'''
* '''Combustion systems'''
* '''Molecular dynamics'''
* '''Magnetohydrodynamic flows'''

and many other domains.
|-
|| Slide: ParaView
||
* Visualizing the simulated results comes under the '''post-processing''' stage.
* '''ParaView''' is the most commonly used software for '''post-processing OpenFOAM''' results.

|-
|| Only Narration
|| Now, let’s briefly go through various tutorials available in this series.
|-
|| Glimpse of Installing OpenFOAM in Ubuntu

(01: 50 - 01:55)
|| We first have the tutorial on installing '''OpenFOAM''' and '''ParaView''' in '''Ubuntu Linux OS'''.
|-
|| Glimpse of Setting-up a Test Case in OpenFOAM

(04:20 - 04:25) >> (10:06 - 10:11)
|| After this, we’ll see how to set up and view the files of an '''OpenFOAM case'''.

We’ll also see how to '''run''' the '''case''' and visualise the results in '''ParaView'''.
|-
|| Glimpse of Creating a 2D channel geometry in OpenFOAM

(05:40 - 05:45) >> (10:25 - 10:30)
|| In the next tutorial, we’ll see how to create a geometry and '''mesh''' using the '''blockMesh''' utility.

We’ll also see how to view the '''mesh''' in '''ParaView'''.
|-
|| Glimpse of Multi-block Meshing of 2D Geometry in OpenFOAM

(03:17 - 03:22) >> (09:31 - 09:36)
|| This is followed by the tutorial on creating a geometry with multiple '''blocks'''.

We’ll see how to '''mesh''' each '''block''' separately and '''refine cells''' locally.
|-
|| Glimpse of Creating 3D pipe geometry and mesh in OpenFOAM

(02:05 - 02:10) >> (06:14 - 06:19)
|| Next, we’ll see how to create a '''mesh''' for a cylindrical pipe.

We’ll see how '''curved edges''' are defined using the '''blockMesh''' utility.
|-
|| Glimpse of Simulating Hagen-Poiseuille flow through a Pipe

(07:20 - 07:25) >> (12:04 - 12:09)
|| Then, we’ll simulate the '''flow''' through a pipe.

We’ll also compare the results from '''simulation''' with the analytical solution.
|-
|| Glimpse of Basic Post-processing using ParaView

(04:23 - 04:26) >> (07:00 - 07:05)
|| The results from the '''pipe flow simulation''' are viewed in detail in '''ParaView''' in this tutorial.

We’ll also see how to '''plot''' the results in '''ParaView'''.
|-
|| Glimpse of Simulation of Turbulent Flow in a 2D Channel in OpenFOAM

(07:00 - 07:05)
|| In the next tutorial, we’ll learn how to use a '''turbulence model''' in a '''simulation'''.
|-
|| Glimpse of Turbulence Modelling in OpenFOAM

(12:00 - 12:05)
|| We will then compare the results from a '''simulation''' using three different '''turbulence models'''.
|-
|| Glimpse of Grid Resolution and Convergence in OpenFOAM

(07:53 - 07:58)
|| We also have a tutorial detailing the steps to establish '''grid independence'''.
|-
|| Only Narration
|| Later on, there will be more tutorials in this series.

Please check the '''Spoken Tutorial website''' regularly for the latest topics.
|-
|| OpenFOAM version 7 Spoken Tutorial Page
|| With this we have come to the end of this tutorial.

Let’s summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt about:
* '''OpenFOAM''' and its capabilities
* Basic '''OpenFOAM''' utilities, and
* The content available in various tutorials in this series

|-
|| 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

||
* Do you have questions in THIS Spoken Tutorial?
* Please visit this site.
* Choose the minute and second where you have the question
* Explain your question briefly
* Someone from our team will answer them
* You will have to register on this website to ask questions.

|-
|| Slide: Forum to answer questions
||
* Do you have any general/technical questions?
* Please visit the forum given in this link.

|-
|| Slide: Textbook Companion
||
* 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: Acknowledgment
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley Melvin.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM version 7

2020-09-05T09:52:32Z

Ashleymelvin:

'''OpenFOAM®''' (Open Source Field Operation and Manipulation) is an open source CFD software package developed by the OpenFOAM team at ESI and distributed by the OpenFOAM Foundation. OpenFOAM is a CFD toolbox, written in C++ and these C++ libraries are used to create executables, known as applications. The OpenFOAM distribution contains numerous solvers and utilities covering a wide range of CFD problems.

In this tutorial series, all the three stages in a CFD simulation, namely pre-processing, running, and post-processing, are focused in-depth. The first two stages are demonstrated in this series using version 7 of OpenFOAM, while ParaView 5.6.0 is used for post-processing. In addition to software training, this tutorial series also strives to demonstrate the basic CFD concepts for better understanding of various OpenFOAM solvers and utilities.

Being an open source software, OpenFOAM can be useful to technical institutes who cannot afford expensive licenses of commercial CFD software. The students and teachers trying to learn OpenFOAM through this series are expected to have some basic knowledge of CFD and Linux commands.

The '''Spoken Tutorial''' for '''OpenFOAM version 7''' has being contributed by Divyesh Variya, Padmini Priyadarshini, Ashley Melvin and Swetha Sridhar from '''FOSSEE Project, IIT''' Bombay with domain reviews done by Prof. Janani S Murallidharan of Dept. of Mechanical Engineering, IIT Bombay.

This series would be useful for Undergraduate and postgraduate students as well as faculty in the departments of Aerospace, Mechanical, Chemical and Civil Engineering.

__TOC__

==Basic Level==
#Overview of OpenFOAM
#*About OpenFOAM
#*OpenFOAM Capabilities
#*Mesh Generation in OpenFOAM
#*Mesh Conversion in OpenFOAM
#*OpenFOAM Solvers
#*Post-processing
#*Spoken Tutorials available on OpenFOAM
#*Timed discussion forum of Spoken Tutorials
#*Discussion forum of FOSSEE
#*OpenFOAM Case Study Project
#Installing OpenFOAM in Ubuntu
#*Public key for package signature verification
#*Add OpenFOAM to package list
#*Install OpenFOAM
#*Install ParaView
#*Accessing .bashrc file
#*User configuration to access OpenFOAM from terminal
#*Verify OpenFOAM installation
#*Verify ParaView Installation
#Setting-up a Test Case in OpenFOAM:
#*Create Run directory
#*Copy a case from Tutorial directory to Run directory
#*Overview of blockMeshDict
#*Overview of 0 folder
#*Contents of p and U files
#*Overview of transportProperties file
#*Parameters in controlDict file
#*blockMesh command
#*icoFoam solver
#*paraFoam command
#*View contour plots in ParaView
#Creating 2D Channel Geometry and Mesh in OpenFOAM:
#*2D channel flow problem description
#*Geometry of the channel
#*Boundaries of the channel
#*Dimensions of coordinates in blockMeshDict
#*Vertex numbering and coordinates
#*Defining a block
#*Meshing parameters
#*Labelling boundaries
#*Ordering the vertices of a face
#*Viewing mesh in ParaView
#Multi-block Meshing of a 2D Geometry in OpenFOAM:
#*Two-block geometry
#*Defining the vertices
#*Defining multiple blocks
#*Meshing parameters of each block
#*Cell Expansion Ratio
#*Labelling boundaries
#*Defining cyclic patches
#*Order of vertices of faces
#*neighbourPatch for cyclic boundaries
#*Viewing refined mesh in ParaView
#Creating 3D Pipe Geometry and Mesh in OpenFOAM:
#*Create a 3D Geometry using blockMeshDict
#*Create a Multi-block geometry and Mesh
#*Mesh a 3D geometry
#*Create arcs in blockMeshDict
#*Label the boundary patches
#*Check Mesh domain
#*Check Skewness
#*Check Aspect Ratio
#*Check number of cells
#*Check cell types
#*View the 3D geometry and mesh in ParaView
#Simulating Hagen Poiseuille flow through a pipe in OpenFOAM:
#*Set up the boundary conditions
#*Set up the initial conditions
#*Set up the physical properties
#*Set up the solve control parameter
#*Set up the write control parameter
#*Hagen Poiseuille Flow
#*3D flow in Pipe
#*Laminar flow
#*Viscous & Newtonian flow
#*Run the simulation
#Basic Post Processing using ParaView:
#*Flow through pipe
#*Hagen Poiseuille flow
#*Streamline visualization
#*Glyph visualization
#*Clip the Mesh
#*View internal flow field
#*Plot graph in paraview
#*Analytical and OpenFOAM result comparison
#*Export the field data to .csv file
#*Plot a graph in LibreOffice Suite Calc
#*Save a screenshot of a view
#Simulation of a 2D Turbulent Flow in a Channel using OpenFOAM:
#*2D channel flow problem description
#*Introduction to k-epsilon turbulence model
#*Calculation of yp for a given yplus
#*Boundary conditions for kappa
#*Boundary conditions for epsilon
#*Boundary conditions for kinematic eddy viscosity
#*Setting up k file
#*Setting up epsilon file
#*Setting up nut file
#*Running the simulation using simpleFoam
#*Outlet velocity profile
#Turbulence Modelling in OpenFOAM:
#*Create channel geometry with two blocks
#*Set up the blockMeshDict dictionary for a given YPlus value
#*Calculate expansion ratio
#*Implement k-epsilon turbulence model
#*Implement k-omega turbulence model
#*Implement k-omega SST turbulence model
#*Implement wall functions
#*Calculate kappa, epsilon and omega
#*Compare turbulence models
#*Run the simulation
#Grid Resolution and Convergence in OpenFOAM:
#*Lid-driven Cavity Flow Problem Statement
#*Meshing parameters of Coarse mesh
#*Time-step for Coarse mesh
#*Simulation using icoFoam
#*Probe Location Filter
#*Pressure at the centre of the domain
#*Refining a Mesh
#*Time-step for Refined mesh
#*Tabulated Pressure at the centre
#*Grid Independence Study

OpenFOAM version 7

2020-09-05T09:37:14Z

Ashleymelvin:

'''OpenFOAM®''' (Open Source Field Operation and Manipulation) is an open source CFD software package developed by the OpenFOAM team at ESI and distributed by the OpenFOAM Foundation. OpenFOAM is a CFD toolbox, written in C++ and these C++ libraries are used to create executables, known as applications. The OpenFOAM distribution contains numerous solvers and utilities covering a wide range of CFD problems.

In this tutorial series, all the three stages in a CFD simulation, namely pre-processing, running, and post-processing, are focused in-depth. The first two stages are demonstrated in this series using version 7 of OpenFOAM, while ParaView 5.6.0 is used for post-processing. In addition to software training, this tutorial series also strives to demonstrate the basic CFD concepts for better understanding of various OpenFOAM solvers and utilities.

Being an open source software, OpenFOAM can be useful to technical institutes who cannot afford expensive licenses of commercial CFD software. The students and teachers trying to learn OpenFOAM through this series are expected to have some basic knowledge of CFD and Linux commands.

The '''Spoken Tutorial''' for '''OpenFOAM version 7''' has being contributed by Divyesh Variya, Padmini Priyadarshini, Ashley Melvin and Swetha Sridhar from '''FOSSEE Project, IIT''' Bombay with domain reviews done by Prof. Janani S Murallidharan of Dept. of Mechanical Engineering, IIT Bombay.

This series would be useful for Undergraduate and postgraduate students as well as faculty in the departments of Aerospace, Mechanical, Chemical and Civil Engineering.

__TOC__

==Basic Level==
#Installing OpenFOAM in Ubuntu
#*Public key for package signature verification
#*Add OpenFOAM to package list
#*Install OpenFOAM
#*Install ParaView
#*Accessing .bashrc file
#*User configuration to access OpenFOAM from terminal
#*Verify OpenFOAM installation
#*Verify ParaView Installation
#Setting-up a Test Case in OpenFOAM:
#*Create Run directory
#*Copy a case from Tutorial directory to Run directory
#*Overview of blockMeshDict
#*Overview of 0 folder
#*Contents of p and U files
#*Overview of transportProperties file
#*Parameters in controlDict file
#*blockMesh command
#*icoFoam solver
#*paraFoam command
#*View contour plots in ParaView
#Creating 2D Channel Geometry and Mesh in OpenFOAM:
#*2D channel flow problem description
#*Geometry of the channel
#*Boundaries of the channel
#*Dimensions of coordinates in blockMeshDict
#*Vertex numbering and coordinates
#*Defining a block
#*Meshing parameters
#*Labelling boundaries
#*Ordering the vertices of a face
#*Viewing mesh in ParaView
#Multi-block Meshing of a 2D Geometry in OpenFOAM:
#*Two-block geometry
#*Defining the vertices
#*Defining multiple blocks
#*Meshing parameters of each block
#*Cell Expansion Ratio
#*Labelling boundaries
#*Defining cyclic patches
#*Order of vertices of faces
#*neighbourPatch for cyclic boundaries
#*Viewing refined mesh in ParaView
#Creating 3D Pipe Geometry and Mesh in OpenFOAM:
#*Create a 3D Geometry using blockMeshDict
#*Create a Multi-block geometry and Mesh
#*Mesh a 3D geometry
#*Create arcs in blockMeshDict
#*Label the boundary patches
#*Check Mesh domain
#*Check Skewness
#*Check Aspect Ratio
#*Check number of cells
#*Check cell types
#*View the 3D geometry and mesh in ParaView
#Simulating Hagen Poiseuille flow through a pipe in OpenFOAM:
#*Set up the boundary conditions
#*Set up the initial conditions
#*Set up the physical properties
#*Set up the solve control parameter
#*Set up the write control parameter
#*Hagen Poiseuille Flow
#*3D flow in Pipe
#*Laminar flow
#*Viscous & Newtonian flow
#*Run the simulation
#Basic Post Processing using ParaView:
#*Flow through pipe
#*Hagen Poiseuille flow
#*Streamline visualization
#*Glyph visualization
#*Clip the Mesh
#*View internal flow field
#*Plot graph in paraview
#*Analytical and OpenFOAM result comparison
#*Export the field data to .csv file
#*Plot a graph in LibreOffice Suite Calc
#*Save a screenshot of a view
#Simulation of a 2D Turbulent Flow in a Channel using OpenFOAM:
#*2D channel flow problem description
#*Introduction to k-epsilon turbulence model
#*Calculation of yp for a given yplus
#*Boundary conditions for kappa
#*Boundary conditions for epsilon
#*Boundary conditions for kinematic eddy viscosity
#*Setting up k file
#*Setting up epsilon file
#*Setting up nut file
#*Running the simulation using simpleFoam
#*Outlet velocity profile
#Turbulence Modelling in OpenFOAM:
#*Create channel geometry with two blocks
#*Set up the blockMeshDict dictionary for a given YPlus value
#*Calculate expansion ratio
#*Implement k-epsilon turbulence model
#*Implement k-omega turbulence model
#*Implement k-omega SST turbulence model
#*Implement wall functions
#*Calculate kappa, epsilon and omega
#*Compare turbulence models
#*Run the simulation
#Grid Resolution and Convergence in OpenFOAM:
#*Lid-driven Cavity Flow Problem Statement
#*Meshing parameters of Coarse mesh
#*Time-step for Coarse mesh
#*Simulation using icoFoam
#*Probe Location Filter
#*Pressure at the centre of the domain
#*Refining a Mesh
#*Time-step for Refined mesh
#*Tabulated Pressure at the centre
#*Grid Independence Study

OpenFOAM version 7

2020-09-05T09:35:34Z

Ashleymelvin:

'''OpenFOAM®''' (Open Source Field Operation and Manipulation) is an open source CFD software package developed by the OpenFOAM team at ESI and distributed by the OpenFOAM Foundation. OpenFOAM is a CFD toolbox, written in C++ and these C++ libraries are used to create executables, known as applications. The OpenFOAM distribution contains numerous solvers and utilities covering a wide range of CFD problems.

In this tutorial series, all the three stages in a CFD simulation, namely pre-processing, running, and post-processing, are focused in-depth. The first two stages are demonstrated in this series using version 7 of OpenFOAM, while ParaView 5.6.0 is used for post-processing. In addition to software training, this tutorial series also strives to demonstrate the basic CFD concepts for better understanding of various OpenFOAM solvers and utilities.

Being an open source software, OpenFOAM can be useful to technical institutes who cannot afford expensive licenses of commercial CFD software. The students and teachers trying to learn OpenFOAM through this series are expected to have some basic knowledge of CFD and Linux commands.

The '''Spoken Tutorial''' effort for OpenFOAM version 7 has being contributed by Divyesh Variya, Padmini Priyadarshini, Ashley Melvin and Swetha Sridhar from '''FOSSEE Project, IIT''' Bombay with domain reviews done by Prof. Janani S Murallidharan of Dept. of Mechanical Engineering, IIT Bombay.

This series would be useful for Undergraduate and postgraduate students as well as faculty in the departments of Aerospace, Mechanical, Chemical and Civil Engineering.

__TOC__

==Basic Level==
#Installing OpenFOAM in Ubuntu
#*Public key for package signature verification
#*Add OpenFOAM to package list
#*Install OpenFOAM
#*Install ParaView
#*Accessing .bashrc file
#*User configuration to access OpenFOAM from terminal
#*Verify OpenFOAM installation
#*Verify ParaView Installation
#Setting-up a Test Case in OpenFOAM:
#*Create Run directory
#*Copy a case from Tutorial directory to Run directory
#*Overview of blockMeshDict
#*Overview of 0 folder
#*Contents of p and U files
#*Overview of transportProperties file
#*Parameters in controlDict file
#*blockMesh command
#*icoFoam solver
#*paraFoam command
#*View contour plots in ParaView
#Creating 2D Channel Geometry and Mesh in OpenFOAM:
#*2D channel flow problem description
#*Geometry of the channel
#*Boundaries of the channel
#*Dimensions of coordinates in blockMeshDict
#*Vertex numbering and coordinates
#*Defining a block
#*Meshing parameters
#*Labelling boundaries
#*Ordering the vertices of a face
#*Viewing mesh in ParaView
#Multi-block Meshing of a 2D Geometry in OpenFOAM:
#*Two-block geometry
#*Defining the vertices
#*Defining multiple blocks
#*Meshing parameters of each block
#*Cell Expansion Ratio
#*Labelling boundaries
#*Defining cyclic patches
#*Order of vertices of faces
#*neighbourPatch for cyclic boundaries
#*Viewing refined mesh in ParaView
#Creating 3D Pipe Geometry and Mesh in OpenFOAM:
#*Create a 3D Geometry using blockMeshDict
#*Create a Multi-block geometry and Mesh
#*Mesh a 3D geometry
#*Create arcs in blockMeshDict
#*Label the boundary patches
#*Check Mesh domain
#*Check Skewness
#*Check Aspect Ratio
#*Check number of cells
#*Check cell types
#*View the 3D geometry and mesh in ParaView
#Simulating Hagen Poiseuille flow through a pipe in OpenFOAM:
#*Set up the boundary conditions
#*Set up the initial conditions
#*Set up the physical properties
#*Set up the solve control parameter
#*Set up the write control parameter
#*Hagen Poiseuille Flow
#*3D flow in Pipe
#*Laminar flow
#*Viscous & Newtonian flow
#*Run the simulation
#Basic Post Processing using ParaView:
#*Flow through pipe
#*Hagen Poiseuille flow
#*Streamline visualization
#*Glyph visualization
#*Clip the Mesh
#*View internal flow field
#*Plot graph in paraview
#*Analytical and OpenFOAM result comparison
#*Export the field data to .csv file
#*Plot a graph in LibreOffice Suite Calc
#*Save a screenshot of a view
#Simulation of a 2D Turbulent Flow in a Channel using OpenFOAM:
#*2D channel flow problem description
#*Introduction to k-epsilon turbulence model
#*Calculation of yp for a given yplus
#*Boundary conditions for kappa
#*Boundary conditions for epsilon
#*Boundary conditions for kinematic eddy viscosity
#*Setting up k file
#*Setting up epsilon file
#*Setting up nut file
#*Running the simulation using simpleFoam
#*Outlet velocity profile
#Turbulence Modelling in OpenFOAM:
#*Create channel geometry with two blocks
#*Set up the blockMeshDict dictionary for a given YPlus value
#*Calculate expansion ratio
#*Implement k-epsilon turbulence model
#*Implement k-omega turbulence model
#*Implement k-omega SST turbulence model
#*Implement wall functions
#*Calculate kappa, epsilon and omega
#*Compare turbulence models
#*Run the simulation
#Grid Resolution and Convergence in OpenFOAM:
#*Lid-driven Cavity Flow Problem Statement
#*Meshing parameters of Coarse mesh
#*Time-step for Coarse mesh
#*Simulation using icoFoam
#*Probe Location Filter
#*Pressure at the centre of the domain
#*Refining a Mesh
#*Time-step for Refined mesh
#*Tabulated Pressure at the centre
#*Grid Independence Study

OpenFOAM version 7

2020-09-05T09:33:01Z

Ashleymelvin:

'''OpenFOAM®''' (Open Source Field Operation and Manipulation) is an open source CFD software package developed by the OpenFOAM team at ESI and distributed by the OpenFOAM Foundation. OpenFOAM is a CFD toolbox, written in C++ and these C++ libraries are used to create executables, known as applications. The OpenFOAM distribution contains numerous solvers and utilities covering a wide range of CFD problems.

In this tutorial series, all the three stages in a CFD simulation, namely pre-processing, running, and post-processing, are focused in-depth. The first two stages are demonstrated in this series using version 7 of OpenFOAM, while ParaView 5.6.0 is used for post-processing. In addition to software training, this tutorial series also strives to demonstrate the basic CFD concepts for better understanding of various OpenFOAM solvers and utilities.

Being an open source software, OpenFOAM can be useful to technical institutes who cannot afford expensive licenses of commercial CFD software. The students and teachers trying to learn OpenFOAM through this series are expected to have some basic knowledge of CFD and Linux commands.

The '''Spoken Tutorial''' effort for OpenFOAM version 7 has being contributed by Divyesh Variya, Padmini Priyadarshini, Ashley Melvin and Swetha Sridhar from '''FOSSEE Project, IIT''' Bombay with domain reviews done by Prof. Janani S Murallidharan of Dept. of Mechanical Engineering, IIT Bombay.

This series would be useful for Undergraduate and postgraduate students as well as faculty in the departments of Aerospace, Mechanical, Chemical and Civil Engineering.

__TOC__

==Basic Level==
#Installing OpenFOAM in Ubuntu
#*Public key for package signature verification
#*Add OpenFOAM to package list
#*Install OpenFOAM
#*Install ParaView
#*Accessing .bashrc file
#*User configuration to access OpenFOAM from terminal
#*Verify OpenFOAM installation
#*Verify ParaView Installation
#Setting-up a Test Case in OpenFOAM:
#*Create Run directory
#*Copy a case from Tutorial directory to Run directory
#*Overview of blockMeshDict
#*Overview of 0 folder
#*Contents of p and U files
#*Overview of transportProperties file
#*Parameters in controlDict file
#*blockMesh command
#*icoFoam solver
#*paraFoam command
#*View contour plots in ParaView
#Creating 2D Channel Geometry and Mesh in OpenFOAM:
#*2D channel flow problem description
#*Geometry of the channel
#*Boundaries of the channel
#*Dimensions of coordinates in blockMeshDict
#*Vertex numbering and coordinates
#*Defining a block
#*Meshing parameters
#*Labelling boundaries
#*Ordering the vertices of a face
#*Viewing mesh in ParaView
#Multi-block Meshing of a 2D Geometry in OpenFOAM:
#*Two-block geometry
#*Defining the vertices
#*Defining multiple blocks
#*Meshing parameters of each block
#*Cell Expansion Ratio
#*Labelling boundaries
#*Defining cyclic patches
#*Order of vertices of faces
#*neighbourPatch for cyclic boundaries
#*Viewing refined mesh in ParaView
#Creating 3D Pipe Geometry and Mesh in OpenFOAM:
#*Create a 3D Geometry using blockMeshDict
#*Create a Multi-block geometry and Mesh
#*Mesh a 3D geometry
#*Create arcs in blockMeshDict
#*Label the boundary patches
#*Check Mesh domain
#*Check Skewness
#*Check Aspect Ratio
#*Check number of cells
#*Check cell types
#*View the 3D geometry and mesh in ParaView
#Simulating Hagen Poiseuille flow through a pipe in OpenFOAM:
#*Set up the boundary conditions
#*Set up the initial conditions
#*Set up the physical properties
#*Set up the solve control parameter
#*Set up the write control parameter
#*Hagen Poiseuille Flow
#*3D flow in Pipe
#*Laminar flow
#*Viscous & Newtonian flow
#*Run the simulation
#Basic Post Processing using ParaView:
#*Flow through pipe
#*Hagen Poiseuille flow
#*Streamline visualization
#*Glyph visualization
#*Clip the Mesh
#*View internal flow field
#*Plot graph in paraview
#*Analytical and OpenFOAM result comparison
#*Export the field data to .csv file
#*Plot a graph in LibreOffice Suite Calc
#*Save a screenshot of a view
#Turbulence Modelling in OpenFOAM:
#*Create channel geometry with two blocks
#*Set up the blockMeshDict dictionary for a given YPlus value
#*Calculate expansion ratio
#*Implement k-epsilon turbulence model
#*Implement k-omega turbulence model
#*Implement k-omega SST turbulence model
#*Implement wall functions
#*Calculate kappa, epsilon and omega
#*Compare turbulence models
#*Run the simulation
#Grid Resolution and Convergence in OpenFOAM:
#*Lid-driven Cavity Flow Problem Statement
#*Meshing parameters of Coarse mesh
#*Time-step for Coarse mesh
#*Simulation using icoFoam
#*Probe Location Filter
#*Pressure at the centre of the domain
#*Refining a Mesh
#*Time-step for Refined mesh
#*Tabulated Pressure at the centre
#*Grid Independence Study

OpenFOAM version 7

2020-09-05T09:30:54Z

Ashleymelvin: Created page with "'''OpenFOAM®''' (Open Source Field Operation and Manipulation) is an open source CFD software package developed by the OpenFOAM team at ESI and distributed by the OpenFOAM Fo..."

'''OpenFOAM®''' (Open Source Field Operation and Manipulation) is an open source CFD software package developed by the OpenFOAM team at ESI and distributed by the OpenFOAM Foundation. OpenFOAM is a CFD toolbox, written in C++ and these C++ libraries are used to create executables, known as applications. The OpenFOAM distribution contains numerous solvers and utilities covering a wide range of CFD problems.

In this tutorial series, all the three stages in a CFD simulation, namely pre-processing, running, and post-processing, are focused in-depth. The first two stages are demonstrated in this series using version 7 of OpenFOAM, while ParaView 5.6.0 is used for post-processing. In addition to software training, this tutorial series also strives to demonstrate the basic CFD concepts for better understanding of various OpenFOAM solvers and utilities.

Being an open source software, OpenFOAM can be useful to technical institutes who cannot afford expensive licenses of commercial CFD software. The students and teachers trying to learn OpenFOAM through this series are expected to have some basic knowledge of CFD and Linux commands.

The '''Spoken Tutorial''' effort for OpenFOAM version 7 has being contributed by Divyesh Variya, Padmini Priyadarshini, Ashley Melvin and Swetha Sridhar from '''FOSSEE Project, IIT''' Bombay with domain reviews done by Prof. Janani S Murallidharan of Dept. of Mechanical Engineering, IIT Bombay.

This series would be useful for Undergraduate and postgraduate students as well as faculty in the departments of Aerospace, Mechanical, Chemical and Civil Engineering.

__TOC__

==Basic Level==
#Installing OpenFOAM in Ubuntu
#*Public key for package signature verification
#*Add OpenFOAM to package list
#*Install OpenFOAM
#*Install ParaView
#*Accessing .bashrc file
#*User configuration to access OpenFOAM from terminal
#*Verify OpenFOAM installation
#*Verify ParaView Installation
#Setting-up a Test Case in OpenFOAM:
#*Create Run directory
#*Copy a case from Tutorial directory to Run directory
#*Overview of blockMeshDict
#*Overview of 0 folder
#*Contents of p and U files
#*Overview of transportProperties file
#*Parameters in controlDict file
#*blockMesh command
#*icoFoam solver
#*paraFoam command
#*View contour plots in ParaView

#Creating 2D Channel Geometry and Mesh in OpenFOAM:
#*2D channel flow problem description
#*Geometry of the channel
#*Boundaries of the channel
#*Dimensions of coordinates in blockMeshDict
#*Vertex numbering and coordinates
#*Defining a block
#*Meshing parameters
#*Labelling boundaries
#*Ordering the vertices of a face
#*Viewing mesh in ParaView
#Multi-block Meshing of a 2D Geometry in OpenFOAM:
#*Two-block geometry
#*Defining the vertices
#*Defining multiple blocks
#*Meshing parameters of each block
#*Cell Expansion Ratio
#*Labelling boundaries
#*Defining cyclic patches
#*Order of vertices of faces
#*neighbourPatch for cyclic boundaries
#*Viewing refined mesh in ParaView
#Creating 3D Pipe Geometry and Mesh in OpenFOAM:
#*Create a 3D Geometry using blockMeshDict
#*Create a Multi-block geometry and Mesh
#*Mesh a 3D geometry
#*Create arcs in blockMeshDict
#*Label the boundary patches
#*Check Mesh domain
#*Check Skewness
#*Check Aspect Ratio
#*Check number of cells
#*Check cell types
#*View the 3D geometry and mesh in ParaView
#Simulating Hagen Poiseuille flow through a pipe in OpenFOAM:
#*Set up the boundary conditions
#*Set up the initial conditions
#*Set up the physical properties
#*Set up the solve control parameter
#*Set up the write control parameter
#*Hagen Poiseuille Flow
#*3D flow in Pipe
#*Laminar flow
#*Viscous & Newtonian flow
#*Run the simulation
#Basic Post Processing using ParaView:
#*Flow through pipe
#*Hagen Poiseuille flow
#*Streamline visualization
#*Glyph visualization
#*Clip the Mesh
#*View internal flow field
#*Plot graph in paraview
#*Analytical and OpenFOAM result comparison
#*Export the field data to .csv file
#*Plot a graph in LibreOffice Suite Calc
#*Save a screenshot of a view
#Turbulence Modelling in OpenFOAM:
#*Create channel geometry with two blocks
#*Set up the blockMeshDict dictionary for a given YPlus value
#*Calculate expansion ratio
#*Implement k-epsilon turbulence model
#*Implement k-omega turbulence model
#*Implement k-omega SST turbulence model
#*Implement wall functions
#*Calculate kappa, epsilon and omega
#*Compare turbulence models
#*Run the simulation
#Grid Resolution and Convergence in OpenFOAM:
#*Lid-driven Cavity Flow Problem Statement
#*Meshing parameters of Coarse mesh
#*Time-step for Coarse mesh
#*Simulation using icoFoam
#*Probe Location Filter
#*Pressure at the centre of the domain
#*Refining a Mesh
#*Time-step for Refined mesh
#*Tabulated Pressure at the centre
#*Grid Independence Study

OpenFOAM-version-7/C2/Simulation-a-2D-Turbulent-Flow-in-a-Channel-using-OpenFOAM/English

2020-09-01T07:03:39Z

Ashleymelvin:

'''Title of the script:''' Simulation of a Turbulent Flow in a 2D Channel using OpenFOAM

'''Author:''' Padmini Priyadarshini

'''Keywords:''' OpenFOAM, Turbulence, k-epsilon, yplus, expansion ratio, blockMesh, wall function, channel flow, simpleFoam, ParaView, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Simulation of Turbulent Flow in a 2D Channel using OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn how to:
* Implement '''k-epsilon model'''
* Set up '''turbulence''' '''parameters'''
* '''Run '''the '''simulation'''
|-
|| Slide: System Specifications
|| To record this tutorial, I am using,
* '''Linux Mint OS''' version 18.3
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0
* '''gedit Text Editor'''

However, you may use any other '''text editor''' of your choice.

The steps explained in this tutorial are identical in '''Ubuntu Linux OS'''.
|-
|| Slide: Prerequisites
* If not, please go through the prerequisite '''OpenFOAM '''tutorial on https://spoken-tutorial.org
|| As a prerequisite:
* You should have basic knowledge of '''turbulent flows''' and '''fluid dynamics'''.
* You should also be familiar with '''simulating''' a '''flow''' through a '''pipe''' in '''OpenFOAM'''.
* If not, please go through the prerequisite '''OpenFOAM''' tutorial on this website
|-
|| Slide: Code Files
||
* The files used in this tutorial are available in the '''Code''' '''Files''' link on this tutorial page
* Please download and extract them
* Make a copy and then use them while practising
|-
|| Slide: Solver detail
|| We will use the '''simpleFoam solver''' to '''simulate''' this problem.

'''simpleFoam''' is a '''steady-state solver''' for '''incompressible''', '''turbulent flow'''.
|-
|| Slide: Problem statement
|| The diagram shows a''' 2D channel '''of length '''65 m '''and width '''1 m'''.

The '''kinematic viscosity''' is '''1e-05 m2/s (1e to the power of minus 5 metre squared per second).'''

The '''Inlet velocity '''is '''20 metres per second. '''

'''Outlet pressure '''is set to '''0 atmosphere.'''
|-
|| Slide: Flow Properties
|| '''Reynolds number''' is '''2 million'''.

And the '''flow''' is '''turbulent.'''
|-
|| Slide: K-Epsilon turbulence model
|| '''K-epsilon '''is a widely used '''RAS''' '''turbulence model.'''

It is a '''two-equation model'''.

It solves:
* The '''turbulent kinetic energy''' '''transport equation''', and
* The '''turbulent dissipation rate transport''' '''equation'''
|-
|| Only Narration
|| Let us set up the '''case.'''
|-
|| Only Narration
|| Download the '''kepsilon '''folder provided in the '''Code file''' and extract it.
|-
|| CTRL + ALT + T
|| Open the '''terminal''' by pressing '''Ctrl''', '''Alt''' & '''T''' keys.
|-
|| [Terminal]

Only Narration
|| From now onwards please remember to press the '''Enter''' key after typing each '''command '''in the''' Terminal.'''
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| Let us''' '''open the '''RUN directory'''.

To do so, type the following '''command.'''
|-
|| [Terminal] Type:

'''cp -r ~/Downloads/kepsilon .'''
|| And copy the downloaded file into the '''RUN directory'''.

To do so, type the following '''command.'''
|-
|| Only Narration
|| I have downloaded the file into my '''Downloads directory.'''

Please change the '''path''' as per your machine.
|-
|| [Terminal] Type:

'''cd kepsilon'''
|| With this '''command''', we will navigate to the '''kepsilon directory'''.
|-
|| Slide: Y plus
|| '''YPlus '''is the '''dimensionless wall distance.'''

For '''wall function''' '''approach,''' '''yplus''' value should be between '''30 '''and '''300.'''
|-
|| Slide: Wall distance, yp
|| Let “'''yp'''” be the distance between the '''wall''' and the nearest '''cell centre.'''

For our '''case, yp''' is '''0.00155''' for a '''yplus''' value of '''100.'''

For '''channel flow, '''the''' skin friction coefficient, Cf''' is given by this formula.
|-
|| Only Narration
|| The '''Additional Reading Material''' has more details on the''' wall function approach'''.

It mentions the steps used to calculate '''yp'''.
|-
|| [Terminal] Type:

'''ls system'''
|| Type the following''' command''' to view the content of the '''system directory'''.
|-
|| [Terminal] Highlight:

'''blockMeshDict'''
|| This '''directory''' contains the '''blockMeshDict''' file.
|-
|| Only Narration
|| I have already set up the '''blockMesh''' file for a '''2D multi-block channel '''with this''' yp value'''.
|-
|| Only Narration
|| Let us take a look at the''' initial''' and '''boundary conditions''' of the '''flow variables.'''
|-
|| Slide: Inlet Boundary Condition - k
|| Let us take a look at the '''inlet boundary condition '''for '''kappa.'''

We will use '''turbulentIntensityKineticEnergyInlet'''

This calculates''' kappa '''using the user-specified '''turbulence intensity'''.

For our '''case, turbulent intensity''' is '''0.0261 '''and '''Turbulent kinetic energy''' is '''0.41 m2/s2''' (metre squared per second squared)
|-
|| Slide: Inlet Boundary Condition - epsilon

|| Let us take a look at the '''inlet boundary condition '''for '''epsilon.'''

We will use '''turbulentMixingLengthDissipationRateInlet '''

This calculates '''epsilon''' using '''kappa '''and user-specified '''mixingLength'''.

'''mixingLength '''refers to the''' turbulent length scale.'''

'''Kappa''' value is automatically put in by the '''solver'''.

Here, the''' turbulent length scale''' is '''0.07 m'''.

And, the value of the '''turbulent dissipation rate''' is '''0.61 m2/s3''' (metre squared per seconds cubed)
|-
|| Slide: Wall Boundary Condition
|| Next, let us take a look at the '''wall boundary conditions '''to be used.

* '''turbulent kinetic energy '''is set to '''kqRWallFunction '''
* '''turbulent dissipation '''is set to '''epsilonWallFunction'''
|-
|| Slide: Outlet Boundary Condition
|| This slide shows the '''outlet boundary condition.'''

'''zeroGradient boundary condition''' is imposed at the '''outlet '''for both '''parameters'''.
|-
|| Slide: Kinematic eddy viscosity, nut
|| '''Kinematic eddy viscosity''' is a dependent '''variable'''.

Hence, its value is calculated by the''' solver'''.

At the '''wall, nutWallFunction''' is used.
|-
|| Only Narration
|| The '''Additional Reading Material''' has more details on the '''boundary conditions'''.

Please refer to it.

Let us take a look at the '''boundary''' and '''initial conditions''' for '''turbulent kinetic energy'''.
|-
|| [Terminal] Type:

'''gedit 0/k'''
|| Open the '''k''' file in a '''text editor.'''
|-
|| [gedit -'''k'''] Highlight:

'''internalField uniform 0.41;'''
|| The''' internalField''' is initialised as '''0.41'''
|-
|| [gedit -'''k'''] Highlight:''' '''

'''type turbulentIntensityKineticEnergyInlet'''
|| The''' inlet boundary type''' is set to '''turbulentIntensityKineticEnergyInlet'''
|-
|| [gedit -'''k'''] Highlight:''' '''

'''intensity 0.0261;'''
|| The '''keyword intensity '''represents the '''turbulent intensity''', and is set to '''0.0261'''
|-
|| [gedit -'''k'''] Highlight:

'''value $internalField;'''
|| We have passed the '''internalField''' value to the '''patch field''' value.
|-
|| [gedit -'''k'''] Highlight:

'''zeroGradient;'''
|| '''outlet''' is set to '''zeroGradient.'''
|-
|| [gedit -'''k'''] Highlight:

'''kqRWallFunction'''
|| The '''patch type''' for both walls are set to '''kqRWallFunction'''.
|-
|| [gedit -'''k'''] Highlight:

'''value $internalField; '''
|| The''' internalField''' value is passed to the '''patch field '''value.
|-
|| [gedit -'''k'''] Highlight:

'''type empty;'''
|| The '''frontAndBack patch '''is set as '''empty.'''
|-
|| [gedit - '''k'''] Close Text Editor
|| Close the '''k''' file.
|-
|| Only Narration
|| Let’s take a look at the '''epsilon''' file.
|-
|| [Terminal] Type:

'''gedit 0/epsilon'''
|| Open the '''epsilon''' file in a '''text editor.'''
|-
|| [gedit -'''epsilon'''] Highlight:

'''0.61'''
|| The '''internalField '''value is initialized to '''0.61'''
|-
|| [gedit -'''epsilon'''] Highlight:

'''turbulentMixingLengthDissipationRateInlet'''
|| The '''inlet type''' is defined as '''turbulentMixingLengthDissipationRateInlet'''
|-
|| [gedit -'''epsilon'''] Highlight:

'''0.07'''
|| The field''' mixingLength''' is set to '''0.07'''
|-
|| [gedit -'''epsilon'''] Highlight:

'''$internalField'''
|| The '''internalField''' value is passed to the '''patch field '''value.
|-
|| [gedit -'''epsilon'''] Highlight:

'''zeroGradient'''
|| The '''outlet patch''' is defined as '''zeroGradient.'''
|-
|| [gedit -'''epsilon'''] Highlight:

'''epsilonWallFunction'''
|| The '''wall patch type '''is set to '''epsilonWallFunction.'''
|-
|| [gedit - e'''psilon'''] Close Text Editor
|| Close the '''epsilon''' file.
|-
|| [Terminal] Type:

'''gedit 0/nut'''
|| Now, let’s open the '''nut '''file in a '''text editor.'''
|-
|| [gedit -'''nut'''] Highlight:

'''calculated'''
|| The '''inlet''' and '''outlet patches''' are set to '''calculated.'''
|-
|| [gedit -'''nut'''] Highlight:

'''type nutkWallFunction;'''
|| The '''wall patch type '''is set as '''nutkWallFunction'''.
|-
|| [gedit - '''nut'''] Close Text Editor
|| Close the '''nut''' file.
|-
|| [Terminal] Type:

'''gedit 0/U'''
|| Next, open the '''velocity '''file in a '''text editor.'''
|-
|| [gedit -'''U'''] Highlight:

'''(20 0 0)'''
|| The '''inlet patch''' is given a fixed value of '''20 '''along the axis.
|-
|| [gedit -'''U'''] Highlight:

'''zeroGradient'''
|| The '''outlet patch''' is set to '''zeroGradient.'''
|-
|| [gedit -'''U]''' Close Text Editor
|| Close the '''U''' file.
|-
|| Only Narration
|| The '''case '''is ready to be '''run. '''
|-
|| [Terminal] Type:

'''blockMesh'''
|| Type '''blockMesh''' to '''mesh''' the geometry.
|-
|| [Terminal] Type:

'''simpleFoam'''
|| Type '''simpleFoam''' in the '''terminal.'''
|-
|| Only Narration
|| The '''simulation''' will take some time depending on your computer’s '''hardware'''.
|-
|| [Terminal] Highlight:

'''End'''
|| The word '''End''' indicates that the '''simulation''' has finished successfully.
|-
|| Slide: Outlet Velocity Profile
|| The slide shows the '''velocity profile''' at the '''channel exit.'''
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

Let us summarize.
|-
|| Slide: Summary
|| In this tutorial, we learnt to,
* Implement '''k-epsilon turbulence model'''
* Set up the''' initial '''and '''boundary conditions''' for''' turbulence parameters'''
* '''Run''' the '''simulation'''
|-
|| Slide: Assignment
|| As an assignment:
* Change the '''inlet boundary condition''' for '''kappa '''and''' epsilon''' to''' fixedValue'''
* Repeat the '''simulation''' for a '''velocity '''value of '''40 m/s''', change '''kappa '''and '''epsilon''' accordingly
|-
|| 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Padmini.

And this is Swetha from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Simulation-a-2D-Turbulent-Flow-in-a-Channel-using-OpenFOAM/English

2020-07-27T11:38:38Z

Ashleymelvin:

'''Title of the script:''' Simulation of a Turbulent Flow in a 2D Channel using OpenFOAM

'''Author:''' Padmini Priyadarshini

'''Keywords:''' OpenFOAM, Turbulence, k-epsilon, yplus, expansion ratio, blockMesh, wall function, channel flow, simpleFoam, ParaView, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Simulation of Turbulent Flow in a 2D Channel using OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn how to:
* Implement '''k-epsilon model'''
* Set up '''turbulence''' '''parameters'''
* '''Run '''the '''simulation'''
|-
|| Slide: System Specifications
|| To record this tutorial, I am using,
* '''Linux Mint OS''' version 18.3
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0
* '''gedit Text Editor'''

However, you may use any other '''text editor''' of your choice.

The steps explained in this tutorial are identical in '''Ubuntu Linux OS'''.
|-
|| Slide: Prerequisites
* If not, please go through the prerequisite '''OpenFOAM '''tutorial on https://spoken-tutorial.org
|| As a prerequisite:
* You should have basic knowledge of '''turbulent flows''' and '''fluid dynamics'''.
* You should also be familiar with '''simulating a flow through a pipe''' in '''OpenFOAM'''.
* If not, please go through the prerequisite '''OpenFOAM''' tutorial on this website
|-
|| Slide: Code Files
||
* The files used in this tutorial are available in the '''Code''' '''Files''' link on this tutorial page
* Please download and extract them
* Make a copy and then use them while practising
|-
|| Slide: Solver detail
|| We will use the '''simpleFoam solver''' to '''simulate''' this problem.

'''simpleFoam''' is a '''steady-state solver''' for '''incompressible''', '''turbulent flow'''.
|-
|| Slide: Problem statement
|| The diagram shows a''' 2D channel '''of '''length''' '''65 m '''and '''width 1 m'''.

The '''kinematic viscosity''' is '''1e-05 m2/s.'''

The '''Inlet velocity '''is '''20 m/s. '''

'''Outlet pressure '''is set to '''0 atmosphere.'''
|-
|| Slide: Flow Properties
|| '''Reynolds number''' is '''2 million'''.

And the '''flow''' is '''turbulent.'''
|-
|| Slide: K-Epsilon turbulence model
|| '''K-epsilon '''is a widely used '''RAS''' '''turbulence model.'''

It is a '''two-equation model'''.

It solves:
* The '''turbulent kinetic energy''' '''transport equation''', and
* The '''turbulent dissipation rate transport''' '''equation'''
|-
|| Only Narration
|| Let us set up the '''case.'''
|-
|| Only Narration
|| Download the '''kepsilon '''folder provided in the '''Code file''' and extract it.
|-
|| CTRL + ALT + T
|| Open the '''terminal''' by pressing '''Ctrl''', '''Alt''' & '''T''' keys.
|-
|| [Terminal]

Only Narration
|| From now onwards please remember to press the '''Enter''' key after typing each '''command '''in the''' Terminal.'''
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| Let us''' '''open the '''Run directory'''.

To do so, type the following '''command.'''
|-
|| [Terminal] Type:

'''cp -r ~/Downloads/kepsilon .'''
|| And copy the downloaded file into the run directory.

To do so, type the following '''command.'''
|-
|| Only Narration
|| I have downloaded the file into my '''Downloads directory.'''

Please change the '''path''' as per your machine.
|-
|| [Terminal] Type:

'''cd kepsilon'''
|| With this command, we will navigate to the '''kepsilon''' directory.
|-
|| Slide: Y plus
|| '''YPlus '''is the '''dimensionless wall distance.'''

For '''wall function''' '''approach,''' '''yplus''' value should be between '''30 '''and '''300.'''
|-
|| Slide: Wall distance, yp
|| Let “'''yp'''” be the distance between the '''wall''' and the nearest '''cell centre.'''

For our '''case''', '''yp''' is '''0.00155''' for a '''yplus''' value of '''100.'''

For '''channel flow, '''the''' skin friction coefficient, Cf''' is given by this formula.
|-
|| Only Narration
|| The '''Additional Reading Material''' has more details on the''' wall function approach'''.

It mentions the steps used to calculate '''yp'''.
|-
|| [Terminal] Type:

'''ls system'''
|| Type''' '''the following''' command''' to view the content of the '''system''' directory.
|-
|| [Terminal] Highlight:

'''blockMeshDict'''
|| This directory contains the '''blockMeshDict''' file.
|-
|| Only Narration
|| I have already set up the '''blockMesh''' file for a '''2D multi-block channel '''with this''' yp value'''.
|-
|| Only Narration
|| Let us take a look at the''' initial''' and '''boundary conditions''' of the '''flow variables.'''
|-
|| Slide: Inlet Boundary Condition - k
|| Let us take a look at the '''inlet boundary condition '''for '''kappa.'''

We will use '''turbulentIntensityKineticEnergyInlet'''

This calculates''' kappa '''using the user-specified '''turbulence intensity'''.

For our '''case, turbulent intensity''' is '''0.0261 '''and '''Turbulent kinetic energy''' is '''0.41 m2/s2'''
|-
|| Slide: Inlet Boundary Condition - epsilon

|| Let us take a look at the '''inlet boundary condition '''for '''epsilon.'''

We will use '''turbulentMixingLengthDissipationRateInlet '''

This calculates '''epsilon''' using '''kappa '''and

user-specified '''mixingLength'''.

'''mixingLength '''refers to the''' turbulent length scale.'''

'''Kappa''' value is automatically put in by the '''solver'''.

Here''', '''the''' turbulent length scale''' is '''0.07 m'''.

And, the value of the '''turbulent dissipation rate''' is '''0.61 m2/s3'''
|-
|| Slide: Wall Boundary Condition
|| Next, let us take a look at the wall '''boundary conditions '''to be''' '''used.

* '''turbulent kinetic energy '''is set to '''kqRWallFunction '''
* '''turbulent dissipation '''is set to '''epsilonWallFunction'''
|-
|| Slide: Outlet Boundary Condition
|| This slide shows the '''outlet boundary condition.'''

'''zeroGradient boundary condition''' is imposed at the '''outlet '''for both parameters.
|-
|| Slide: Kinematic eddy viscosity, nut
|| '''Kinematic eddy viscosity''' is a dependent '''variable'''.

Hence, its value is calculated by the''' solver'''.

At the '''wall, nutWallFunction''' is used.
|-
|| Only Narration
|| The '''Additional Reading Material''' has more details on the boundary conditions.

Please refer to it.

Let us take a look at the '''boundary''' and '''initial conditions''' for '''turbulent kinetic energy'''.
|-
|| [Terminal] Type:

'''gedit 0/k'''
|| Open the '''k''' file in a '''text editor.'''
|-
|| [gedit -'''k'''] Highlight:

'''internalField uniform 0.41;'''
|| The''' internalField''' is initialised as '''0.41'''
|-
|| [gedit -'''k'''] Highlight:''' '''

'''type turbulentIntensityKineticEnergyInlet'''
|| The''' inlet boundary type''' is set to '''turbulentIntensityKineticEnergyInlet'''
|-
|| [gedit -'''k'''] Highlight:''' '''

'''intensity 0.0261;'''
|| The keyword''' intensity '''represents the '''turbulent intensity''', and is set to '''0.0261'''
|-
|| [gedit -'''k'''] Highlight:''' '''

'''value $internalField;'''
|| We have passed the '''internalField''' value to the '''patch field''' value.
|-
|| [gedit -'''k'''] Highlight:

'''zeroGradient;'''
|| '''outlet''' is set to '''zeroGradient.'''
|-
|| [gedit -'''k'''] Highlight:

'''kqRWallFunction'''
|| The '''patch''' type for both walls are set to '''kqRWallFunction'''.
|-
|| [gedit -'''k'''] Highlight:

'''value $internalField; '''
|| The''' internalField''' value is passed to the '''patch field '''value'''.'''
|-
|| [gedit -'''k'''] Highlight:''' '''

'''type empty;'''
|| The '''frontAndBack patch '''is set as '''empty.'''
|-
|| [gedit - '''k'''] Close Text Editor
|| Close the '''k''' file.
|-
|| Only Narration
|| Let’s take a look at the '''epsilon''' file.
|-
|| [Terminal] Type:

'''gedit 0/epsilon'''
|| Open the '''epsilon''' file in a '''text editor.'''
|-
|| [gedit -'''epsilon'''] Highlight:

'''0.61'''
|| The '''internalField '''value is initialized to '''0.61'''
|-
|| [gedit -'''epsilon'''] Highlight:

'''turbulentMixingLengthDissipationRateInlet'''
|| The '''inlet''' type is defined as '''turbulentMixingLengthDissipationRateInlet'''
|-
|| [gedit -'''epsilon'''] Highlight:

'''0.07'''
|| The field''' mixingLength''' is set to '''0.07'''
|-
|| [gedit -'''epsilon'''] Highlight:

'''$internalField'''
|| The '''internalField''' value is passed to the '''patch field '''value'''.'''
|-
|| [gedit -'''epsilon'''] Highlight:

'''zeroGradient'''
|| The '''outlet patch''' is defined as '''zeroGradient.'''
|-
|| [gedit -'''epsilon'''] Highlight:

'''epsilonWallFunction'''
|| The '''wall patch type '''is set to '''epsilonWallFunction.'''
|-
|| [gedit - e'''psilon'''] Close Text Editor
|| Close the '''epsilon''' file.
|-
|| [Terminal] Type:

'''gedit 0/nut'''
|| Now, let’s open the '''nut '''file in a '''text editor.'''
|-
|| [gedit -'''nut'''] Highlight:

'''calculated'''
|| The '''inlet''' and '''outlet patches''' are set to '''calculated.'''
|-
|| [gedit -'''nut'''] Highlight:

'''type nutkWallFunction;'''
|| The '''wall patch type '''is set as '''nutkWallFunction'''.
|-
|| [gedit - '''nut'''] Close Text Editor
|| Close the '''nut''' file.
|-
|| [Terminal] Type:

'''gedit 0/U'''
|| Next, open the '''velocity '''file in a '''text editor.'''
|-
|| [gedit -'''U'''] Highlight:''' '''

'''(20 0 0)'''
|| The '''inlet patch''' is given a fixed value of '''20 '''along the axis.
|-
|| [gedit -'''U'''] Highlight:''' '''

'''zeroGradient'''
|| The '''outlet patch''' is set to '''zeroGradient.'''
|-
|| [gedit -'''U]''' Close Text Editor
|| Close the '''U''' file.
|-
|| Only Narration
|| The '''case '''is ready to be '''run. '''
|-
|| [Terminal] Type:

'''blockMesh'''
|| Type '''blockMesh''' to '''mesh''' the '''geometry'''.
|-
|| [Terminal] Type:

'''simpleFoam'''
|| Type '''simpleFoam''' in the '''terminal.'''
|-
|| Only Narration
|| The '''simulation''' will take some time depending on your computer’s '''hardware'''.
|-
|| [Terminal] Highlight:''' '''

'''End'''
|| The word '''End''' indicates that the '''simulatio'''n has finished successfully.
|-
|| Slide: Outlet Velocity Profile
|| The slide shows the '''velocity profile''' at the '''channel exit.'''
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

Let us summarize.
|-
|| Slide: Summary
|| In this tutorial, we learnt to,
* Implement '''k-epsilon turbulence model'''
* Set up the''' initial '''and '''boundary conditions''' for''' turbulence parameters'''
* '''Run''' the '''simulation'''
|-
|| Slide: Assignment
|| As an assignment:
* Change the '''inlet boundary condition''' for '''kappa '''and''' epsilon''' to''' fixedValue'''
* Repeat the '''simulation''' for a '''velocity '''value of '''40 m/s''', change '''kappa '''and '''epsilon''' accordingly
|-
|| 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Padmini.

And this is Swetha from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Multi-block-Meshing-of-a-2D-Geometry-in-OpenFOAM/English

2020-07-23T11:48:27Z

Ashleymelvin:

'''Title of the script''': Multi-block Meshing of 2D Geometry in OpenFOAM

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM, ParaView, blockMesh, meshing, multiple blocks, graded mesh, mesh refinement, inflation layer, pre-processing, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Multi-block Meshing of 2D Geometry in OpenFOAM'''.
|-
|| Slide: Learning Objectives
|| In this tutorial, we will learn to:
* Create a '''geometry''' with multiple '''blocks''' using '''blockMeshDict'''
* Vary '''meshing parameters''' for each '''block'''
* Label the '''boundary patches''', and''' '''
* View the '''mesh''' in '''ParaView'''
|-
|| Slide: System Specifications
|| To record this tutorial, I am using,
* '''Ubuntu Linux''' OS version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0, and
* '''gedit Text editor'''

You may use any other '''text editor''' of your choice.
|-
|| Slide: Prerequisites
* If not, please go through the prerequisite '''OpenFOAM '''tutorial on https://spoken-tutorial.org
|| As a prerequisite:
* You should be familiar with the creation of a basic '''geometry '''using the '''blockMesh''' utility.
* If not, please go through the prerequisite '''OpenFOAM '''tutorial on this website.
|-
|| Slide: Code Files
||
* The files used in this tutorial are available in the '''Code''' '''Files''' link on this tutorial page
* Please download and extract them, and
* Make a copy and then use them while practising
|-
|| Slide: Geometry
|| This is the '''geometry''' we will be creating and '''meshing '''later on.
|-
|| Slide: Faces
||
* The left and right faces are the '''inlet''' and '''outlet''' respectively.
* The top and bottom faces are the two '''walls'''.
* The front and back faces are empty faces.

The faces are empty as we are creating a '''geometry''' for a '''2D simulation'''.
|-
|| CTRL + ALT + T
|| Now, open the '''terminal''' by pressing '''Ctrl''', '''Alt''' & '''T''' keys.
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| At the '''prompt''', type the following '''command''' to go to the '''run directory'''.
|-
|| Only Narration
|| Here onwards, please remember to press the '''Enter''' key after typing each '''command''' in the '''terminal'''.
|-
|| [Terminal] Type:

'''cp -r $FOAM_TUTORIALS/incompressible/pimpleFoam/LES/channel395 .'''
|| Now, let us copy the '''case''' from the '''tutorials directory''' into the '''run directory'''.

Type the following '''command''' to do so.
|-
|| [Terminal] Type:

'''rm -r channel395/0'''
|| We will only be creating and '''meshing''' the '''geometry'''.

So, we do not need the '''boundary conditions''' folder.

Type the following '''command''' to delete the '''boundary conditions''' folder.
|-
|| [Terminal] Type:

'''gedit channel395/system/blockMeshDict'''
|| Now open the '''blockMeshDict''' file in a '''text editor'''.

I am opening it in the '''gedit text editor.'''
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''Selection in the Text Editor >> Delete'''
|| Select the contents of the file from '''vertices''' to the end of the document as shown.

Then delete the selected section as we will be entering the '''input parameters'''.
|-
|| [gedit - '''multiBlock''']
|| Next open the '''multiBlock.txt''' file that you have downloaded in the '''text editor'''.
|-
|| [gedit - '''multiBlock'''] Highlight:

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''blockMeshDict''']

'''Paste'''
|| Paste the copied content into the '''blockMeshDict '''file as shown.
|-
|| Ctrl + S
|| And save the file.
|-
|| Slide: Blocks
|| The '''geometry''' is divided into 2 '''blocks''' as shown in the figure.
|-
|| Slide: Vertices
|| There are 12 '''vertices''' and they are numbered as shown.

Note that the '''vertex''' numbering starts from 0.
|-
|| Only Narration
|| Let me switch back to the '''blockMeshDict '''file.
|-
|| Only Narration
|| Let us enter the '''coordinates''' of '''vertices''' in ascending order of their '''vertex''' numbers.

The '''vertices''' are defined using the list '''vertices'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

vertices list
|| The '''coordinates''' of the 12 '''vertices''' are entered as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''blocks '''
|| Now, let us see how the '''blocks''' for this '''geometry''' are defined.
|-
|| Slide: Blocks
|| The '''geometry''' is divided into 2 '''blocks'''.

This division enables us to '''mesh''' the top and bottom sections of the '''geometry''' differently.

The '''blocks''' are numbered as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

Block 1 definition''' '''
|| '''Block 1''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''hex'''
|| We use '''hexahedral blocks''' for '''meshing'''.
|-
|| Only Narration
|| We will enter the '''vertices''' that define '''block 1'''.

We first enter the '''vertices''' of the lower xy-plane.
|-
|| Slide: Block 1
|| To define '''block 1''',
* We first enter the '''vertices''' of the '''back face''' and then that of the '''front face'''
* When viewed along the '''negative z-direction''', the '''vertices''' should be ordered '''counterclockwise'''
* Following this convention, the '''vertices''' of the back face are 0, 1, 3 and 2
* The corresponding order of the front face is 6, 7, 9 and 8
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''0 1 3 2 6 7 9 8'''
|| The '''vertices''' of '''block 1''' are therefore entered in the order as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''40 25 1'''
|| The number of '''cells''' in each '''direction''' is defined as shown.

There is only 1 '''cell''' in the '''z direction''' as this is a '''mesh''' for '''2D simulation''' in '''xy-plane'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''simpleGrading'''
|| We use '''simpleGrading''' as the cells have uniform expansion in all directions.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''1 10 1'''
|| The ratio of width of the '''end cell''' to that of the '''start cell''' in a '''direction''' is its '''expansion ratio'''.

The '''expansion ratio''' in each '''direction''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''1 '''in x direction
|| This means that all '''cells''' have uniform width along '''x''' '''direction'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''1 '''in z direction
|| The same is the case for '''z direction'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''10 '''in y direction
|| However, along the '''y direction''', the '''end cell''' is 10 times as wide as the '''start cell'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

Block 2 definition
|| '''Block 2''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''0.1 '''in y direction
|| The '''expansion ratio''' in '''y direction''' is the only '''parameter''' different in '''block 2''' from that of '''1.'''

Along '''y direction''', the '''end cell''' is now only 0.1 times as wide as the '''start cell'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

edges list
|| Since all the edges of the '''channel geometry''' are straight lines, we leave the '''edges''' field empty.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''boundary'''
|| Let us label the '''boundary patches '''now.
|-
|| Slide: Boundary
|| The bottom and top face is as shown in the figure.

We shall name them '''wallBottom''' and '''wallTop''' respectively.
|-
|| Only Narration
|| Each face resembles the characteristics of a '''solid wall'''.

Hence, the face is of the '''type wall'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''wallBottom '''and '''wallTop '''definitions
|| The two faces are defined as shown.
|-
|| Only Narration
|| We need to impose '''cyclic boundary conditions''' on the '''inlet''' and '''outlet''' faces of '''block 1'''.
|-
|| Slide: Cyclic Patch
||
* The '''face''' '''type''' for a '''cyclic patch''' is defined using the keyword''' cyclic.'''
* The pair of '''faces''' are linked to each other through the keyword''' neighbourPatch.'''
|-
|| Slide: Boundary
|| The '''inlet''' and '''outlet''' faces of '''block 1''' are named '''in1''' and '''out1''' respectively.

The same for '''block 2''' are named '''in2''' and '''out2''' respectively.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''in1 '''definition
|| The '''inlet''' face of '''block 1''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''cyclic'''
|| The '''boundary face type''' is '''cyclic'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''neighbourPatch out1'''
|| The '''outlet''' face is linked to the '''inlet''' face using the keyword''' neighbourPatch'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''((0 6 8 2))'''
|| The '''vertices''' of the '''inlet''' face are ordered in '''clockwise direction''' when viewed from inside of '''block 1'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''out1''' definition
|| The '''outlet''' face of '''block 1''' is defined as shown here.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''in2''' and '''out2''' definitions
|| The '''inlet''' and '''outlet''' faces of '''block 2''' are defined as shown here.
|-
|| Slide: Boundary
||
* The back and front faces of '''block 1''' are named '''sides1_half0''' and '''sides1_half1''' respectively.
* The back and front faces of '''block 2''' are named '''sides2_half0''' and '''sides2_half1''' respectively.
|-
|| Only Narration
|| We are creating a '''geometry''' for a '''2D simulation''' in the '''xy-plane'''.

Therefore, the faces normal to '''z-direction''' are kept empty.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''sides1_half0''' definition
|| The back face of '''block 1''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''empty'''
|| Note that we have kept the face''' empty'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''sides1_half1''', '''sides2_half0''' and '''sides2_half1''' definition
|| Similarly, we define the other 3 faces.
|-
|| Only Narration
|| We have now finished labelling all the '''boundary patches'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

mergePatchPairs list
|| Since we do not have any '''patches''' to merge, we leave the '''mergePatchPairs''' field empty.
|-
|| [gedit - '''blockMeshDict''']

Click on Save >> Close Text Editor
|| We have now entered all the necessary '''fields'''.

Save and close the file.
|-
|| [Terminal]''' '''Type:

'''cd channel395'''
|| Come to the '''terminal''', and type '''cd (space) channel395'''.
|-
|| [Terminal] Type:

'''blockMesh '''>>''' Enter'''
|| To '''mesh''' the '''geometry''', type '''blockMesh''' and press '''Enter'''.
|-
|| [Terminal] Highlight:

'''End'''
|| The '''meshing''' is now complete.
|-
|| [Terminal] Type:

'''paraFoam'''
|| To view the '''mesh''' in '''ParaView''', type '''paraFoam'''.
|-
|| [ParaView] '''Properties''' Tab

Click on '''Apply'''
|| Click on '''Apply''' in the '''Properties''' tab.
|-
|| [ParaView] '''Active Variable Controls'''

Click on '''Surface''' >> Click on '''Surface with Edges'''
|| Click on '''Surface''' available in the '''Active Variable Controls''' and change it to '''Surface with Edges'''.

We can now see the '''mesh''' structure in the '''xy-plane'''.

Notice the '''mesh refinement''' near the top and bottom faces of the '''geometry'''.
|-
|| [ParaView] Close the Window
|| And now, close the '''ParaView''' window.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

To summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt to:
* Create a '''geometry''' with multiple '''blocks''' using '''blockMeshDict'''
* Vary '''meshing parameters''' for each '''block'''
* Label the '''boundary patches''', and
* View the '''mesh''' in '''ParaView'''
|-
|| Slide: Assignment
|| As an assignment:
* Create a '''geometry''' having dimensions '''5 m''', '''4 m''' and '''3 m''' along '''x''', '''y''' and '''z axis'''
* Divide the '''geometry''' into 2 equal''' blocks '''along the''' x axis'''
* Mesh the '''geometry''' such that it has '''25''', '''20''' and '''1 cell''' along '''x''', '''y''' and '''z axis''' for each '''block'''
* Set expansion ratio as '''10''', '''1''' and '''1''' along the '''x''', '''y''' and '''z axis '''for both the '''blocks''', and
* View the '''mesh''' 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 this 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley Melvin.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Setting-up-a-Test-Case-in-OpenFOAM/English

2020-07-23T11:46:09Z

Ashleymelvin:

'''Title of the script''': Setting-up a test case in OpenFOAM

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM, ParaView, lid driven cavity, pre-processing, blockMesh, controlDict, post-processing, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Setting up a test case in OpenFOAM'''.
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn to:
* Set up a '''case''' in '''OpenFOAM'''
* Access the '''case files''' using '''terminal'''
* '''Pre-process''' a '''case'''
* '''Run''' a '''case''', and
* '''Post-process''' a '''case'''
|-
|| Slide: System Specifications
|| This tutorial is recorded using,
* '''Ubuntu Linux''' OS version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0, and
* '''gedit Text editor'''

You may use any other '''text editor''' of your choice.
|-
|| Slide: Prerequisites

|| As a prerequisite:
* You should be familiar with basic '''Linux commands'''.
* If not, please go through the prerequisite '''Linux '''tutorials on this website.
|-
|| Slide: Lid Driven Cavity
|| In this tutorial, we will learn to set up the '''lid driven cavity case'''.

'''Lid driven cavity''' is one of the most widely used '''2D test cases''' for the validation of a '''CFD '''code.
|-
|| Slide: Diagram
|| This is the diagram of '''Lid Driven Cavity Flow'''.

It consists of 3 fixed walls and a moving top wall.
|-
|| Highlight '''Terminal''' on the machine
|| Open a '''terminal''' by pressing the '''Ctrl, Alt '''and''' T''' keys together.
|-
|| Only Narration
|| Here onwards please remember to press the '''Enter''' key after typing each '''command'''.
|-
|| [Terminal] Type:
'''mkdir -p $FOAM_RUN'''
|| Now, let’s create a '''RUN directory'''.

To do so, type the '''command''' as shown.
|-
|| [Terminal] Highlight

'''FOAM_RUN'''
|| '''Tutorial cases''' will later be copied into the '''RUN directory'''.
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| Go to the '''RUN directory''' using the '''cd command'''.

Now our present working directory is the '''RUN directory'''.
|-
|| Only Narration
|| '''OpenFOAM''' installation comes with a set of '''test cases'''.

The '''tutorials directory''' contains these '''test cases'''.

The '''Lid driven cavity case''' already exists inside the '''tutorials directory'''.
|-
|| [Terminal] Type:

'''cp -r $FOAM_TUTORIALS/incompressible/icoFoam/cavity/cavity .'''
|| We’ll now copy the '''Lid driven cavity case''' from the '''tutorials directory''' into the '''RUN directory'''.

To do so, type the following '''command'''.
|-
|| Slide: blockMesh
||
* The '''mesh generator''' for '''OpenFOAM''' is a utility called '''blockMesh'''.
* The '''input dictionary''' for '''blockMesh''' utility is '''blockMeshDict'''.
|-
|| [Terminal] Type:

'''gedit cavity/system/blockMeshDict'''
|| The '''blockMeshDict''' file is located in the '''system''' folder.

Open the '''blockMeshDict''' file in a '''text editor'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight

vertices, blocks, edges and boundary
|| Now let’s look at the contents of the file.

The '''blockMeshDict''' contains details of the geometry like vertices, blocks, edges and boundaries.
|-
|| [gedit - '''blockMeshDict'''] Close the window
|| Close the '''blockMeshDict''' file.
|-
|| [Terminal] Type:

'''cd cavity/0'''
|| The '''0''' folder contains the '''initial''' and '''boundary conditions''' for the '''simulation'''.

Type the following '''command''' to move into the '''0''' folder inside the '''cavity case directory'''.
|-
|| [Terminal] Type:

'''ls'''
|| Type '''ls''' and press '''Enter''' to view the files in the '''0''' folder.
|-
|| [Terminal] Highlight

'''p''' and '''U'''
|| The '''0''' folder contains the '''kinematic pressure file p''' and the '''velocity file U'''.
|-
|| [Terminal] Type:

'''gedit p'''
|| Open the '''kinematic pressure file p''' in a '''text editor'''.
|-
|| Only Narration
|| The '''p''' file contains the '''initial''' and '''boundary conditions''' of '''kinematic pressure'''.
|-
|| [gedit - '''p'''] Highlight

'''dimensions [0 2 -2 0 0 0 0] '''
|| The '''dimensions''' of '''kinematic pressure''' is meter squared per second squared.
|-
|| [gedit - '''p'''] Highlight

'''internalField '''
|| The '''internalField''' defines the values in the interior of the domain.
|-
|| [gedit - '''p'''] Highlight

'''uniform 0'''
|| The initial field is set as '''0 kinematic pressure'''.

This field is '''uniform''' across the domain.
|-
|| [gedit - '''p'''] Highlight

Both the '''zeroGradient'''
|| You can see that all walls are imposed with a '''zero gradient pressure boundary condition'''.
|-
|| [gedit - '''p'''] Close the window
|| Let us close the '''p''' file.
|-
|| [Terminal] Type:

'''gedit U'''
|| Now open the '''velocity file U''' in a '''text editor'''.
|-
|| Only Narration
|| The '''U file''' contains the '''initial''' and '''boundary conditions''' of '''velocity'''.
|-
|| [gedit - '''U'''] Highlight

'''uniform (1 0 0);'''
|| You can see that the moving wall is imposed with a '''velocity''' of '''1 m/s''' in the x direction.
|-
|| [gedit - '''U'''] Highlight

'''noSlip '''
|| Also notice that the '''no-slip condition''' is imposed on the three fixed walls.
|-
|| [gedit - '''U'''] Close the window
|| Now let us close the '''U''' file.
|-
|| [Terminal] Type:

'''cd ..'''
|| We’ll go back to the '''cavity''' folder.

Type '''cd (space)(dot)(dot)'''
|-
|| [Terminal] Type:

'''gedit constant/transportProperties'''
|| Next, we will view the '''transport properties file '''which is in the '''constant '''folder.
|-
|| [gedit - '''transportProperties'''] Highlight

'''nu '''
|| The '''transportProperties''' file contains the details of '''kinematic viscosity'''.
|-
|| [gedit - '''transportProperties''']

Highlight '''[0 2 -1 0 0 0 0] '''
|| The dimensions of '''kinematic viscosity''' is meter squared per second.
|-
|| Slide: Kinematic Viscosity
||
The '''kinematic viscosity''' is defined by:
'''''nu'' equals magnitude of ''U'' times ''d'' by ''Re'''''

where
*'''velocity''' is '''1 m per second'''
*characteristic length is '''0.1 meters'''

The '''Reynolds number (Re)''' for the '''flow''' is taken as '''10'''.

The '''kinematic viscosity''' is therefore '''0.01 meter squared per second'''
|-
|| Narration Only
|| Now let me switch back to '''transportProperties''' file.
|-
|| [gedit - '''transportProperties''']

Highlight '''0.01'''
|| The value of '''kinematic viscosity''' is indicated in the '''transportProperties''' file.
|-
|| [gedit - '''transportProperties'''] Close the window
|| Close the '''transportProperties''' file.
|-
|| [Terminal] Type:

'''cd system'''
|| To move into the '''system''' folder, type the following '''command'''.
|-
|| [Terminal] Type:

'''ls'''
|| Type '''ls''' to view the contents of the '''system''' folder.
|-
|| [Terminal] Highlight

'''blockMeshDict controlDict fvSchemes fvSolution'''
|| The '''system''' folder contains the following files:

'''blockMeshDict, controlDict, fvSchemes''' and '''fvSolution'''.
|-
|| [Terminal] Highlight

'''fvSchemes'''
|| The '''fvSchemes dictionary''' contains the '''finite volume discretisation schemes'''.
|-
|| [Terminal] Highlight

'''fvSolution'''
|| The '''fvSolution dictionary''' contains the '''linear equation solvers''' and '''tolerances'''.

It contains other '''algorithm controls''' as well.
|-
|| [Terminal] Highlight

'''controlDict'''
|| The '''controlDict dictionary''' contains the '''simulation control parameters'''.

The '''dictionary''' input includes the '''control''' of '''time''' and '''reading''' and '''writing''' of the '''solution data'''.
|-
|| [Terminal] Type:

'''gedit controlDict'''
|| Let’s open the '''controlDict''' file in a '''text editor'''.
|-
|| [Terminal] Highlight

'''startFrom '''and '''startTime'''
|| The '''start '''and''' stop times''' and the '''time step''' for the '''run''' must be set.
|-
|| [gedit - '''controlDict'''] Highlight

'''startTime''' '''0;'''
|| The '''start time''' is set at '''0''' seconds.
|-
|| [gedit - '''controlDict'''] Highlight

'''stopAt''' '''endTime;'''
|| The time at which the '''simulation''' stops, is specified using the '''keyword stopAt'''.

Here, '''stopAt''' is specified using the keyword '''endTime'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''endTime''' '''0.5;'''
|| The '''endTime''' is set at '''0.5 seconds'''.

This means that '''simulation''' stops after '''0.5 seconds'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''deltaT 0.005;'''
|| The value of the '''keyword deltaT''' defines the '''time step''' for the '''simulation'''.

The '''time step''' for the current '''simulation''' is set as '''0.005 seconds'''.

'''Temporal accuracy''' and '''numerical stability''' is essential while running the '''simulation'''.

To achieve this, a''' Courant number''' of less than 1 is required.

Keeping this in mind, the '''time step''' is set to '''0.005 seconds'''.
|-
|-
|-
|| [gedit - '''controlDict'''] Highlight

'''application''' '''icoFoam'''<nowiki>;</nowiki>
|| '''icoFoam''' is the '''OpenFOAM solver''' used to '''simulate''' the '''lid driven cavity flow'''.
|-
|| [gedit - '''controlDict'''] Close the window
|| Close the '''controlDict''' file.
|-
|| [Terminal] Type:

'''cd ..'''
|| Go back to the '''cavity''' folder using '''cd command'''.
|-
|| [Terminal] Type:

'''blockMesh''' >> '''Enter'''
|| Type the '''command blockMesh''' and press '''Enter''' to '''mesh''' the geometry.

The '''command''' takes input from the '''blockMeshDict dictionary''' and creates the geometry and '''meshes''' it.
|-
|| [Terminal] Highlight '''End'''
|| The '''meshing''' is now complete.
|-
|| [Terminal] Type:

'''icoFoam'''
|| The '''lid driven cavity flow''' is an '''incompressible flow'''.

It is solved using the''' OpenFOAM solver icoFoam.'''

To start the '''simulation''', type '''icoFoam''' in the '''terminal.'''
|-
|| [Terminal] Highlight '''End'''
|| The iterations are now complete.
|-
|| [Terminal] Type:

'''paraFoam'''
|| Let us view the '''simulated''' results in '''ParaView'''.

So, type '''paraFoam''' in the '''terminal.'''
|-
|| [ParaView] '''Properties''' Tab

Click on '''Apply'''
|| In the '''ParaView''' window, go to the '''Properties''' tab on the left.

Then click on the green coloured '''Apply '''button.
|-
|| [ParaView]

Click on '''vtkBlockColors''' >> Click on '''U'''
|| Go to the '''Active Variable Controls '''at the top.

Click on the '''vtkBlockColors''' dropdown and select '''U'''.

Ensure that you click on the '''U''' option with a '''point icon''' and not the '''box icon''', in the dropdown.

The '''box icon''' would display '''contours''' without any grading.
|-
|| [ParaView]

Velocity Contours in the Layout
|| The '''velocity contour''' at the start of the '''simulation''' is now displayed in the''' layout'''.
|-
|| [ParaView]

Go to '''VCR Controls''' and click on the '''Play''' Button
|| Let us see how the '''velocity contours''' develop through the '''simulation'''.

To do so, go to the '''VCR Controls''' and click on the '''Play''' button.
|-
|| [ParaView]

Final Velocity Contours in the Layout
|| The '''velocity contour''' at the end of the '''simulation''' is now displayed in the''' layout'''.
|-
|| [ParaView] Close the Window
|| Close the '''ParaView''' window.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

|-
|| Slide: Summary
|| To summarise, in this tutorial we have learnt to:
* Set up a''' case''' in '''OpenFOAM'''
* Access the '''case files''' using '''terminal'''
* '''Pre-process''' a '''case'''
* '''Run''' a '''case''', and
* '''Post-process''' a '''case'''
|-
|| 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 this 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley Melvin.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Grid-Resolution-and-Convergence-in-OpenFOAM/English

2020-07-22T10:45:33Z

Ashleymelvin: Created page with "'''Title of the script''': Grid Resolution and Convergence in OpenFOAM '''Author''': Ashley Melvin '''Keywords''': OpenFOAM, ParaView, blockMesh, meshing, mesh refinement, c..."

'''Title of the script''': Grid Resolution and Convergence in OpenFOAM

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM, ParaView, blockMesh, meshing, mesh refinement, coarse mesh, medium mesh, fine mesh, grid independence study, Courant number, lid-driven cavity, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Grid Resolution and Convergence in OpenFOAM'''.
|-
|| Slide: Learning Objectives
|| In this tutorial, we will learn to:
* '''Refine''' a '''mesh''' using '''blockMeshDict'''
* Change the '''time step''' to achieve '''numerical stability''', and
* Perform a '''grid independence''' '''study'''
|-
|| Slide: System Specifications
|| To record this tutorial, I am using,
* '''Ubuntu Linux''' OS version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0, and
* '''gedit Text editor'''

However, you may use any other '''text editor''' of your choice.
|-
|| Slide: Prerequisites
|| As a prerequisite:
* You should be familiar with '''setting up a case''' and '''creating a mesh''' in '''OpenFOAM'''.
* You should also be familiar with '''basic post-processing''' using '''ParaView'''.
* If not, please go through the prerequisite '''OpenFOAM '''tutorials on this website.
|-
|| Slide: Lid Driven Cavity
|| We will use the '''lid driven cavity case''' in this tutorial.

This is the diagram of '''Lid Driven Cavity Flow'''.
|-
|| CTRL + ALT + T
|| Open the '''terminal''' by pressing '''Ctrl''', '''Alt''' & '''T''' keys.
|-
| | Only Narration
| | Here onwards please remember to press the '''Enter''' key after typing each '''command'''.
|-
|| [Terminal]

Type: '''cd $FOAM_RUN'''
|| Type the following '''command''' to move into the '''run directory'''.
|-
|| [Terminal] Type:

'''cp -r $FOAM_TUTORIALS/incompressible/icoFoam/cavity/cavity .'''
|| Let us copy the '''Lid driven cavity case''' from the '''tutorial directory''' into the '''run directory'''.

Type the following '''command''' to do so.
|-
|| [Terminal]

Type: '''cd cavity'''
|| Now let us go into the '''lid driven cavity case''' folder using the '''cd command'''.
|-
|| [Terminal]

Type: '''gedit system/blockMeshDict'''
|| Let’s open the '''blockMeshDict''' file in a '''text editor'''.
|-
|| [gedit - '''blockMeshDict''']

Highlight '''(20 20 1)'''
|| This is a '''2 dimensional mesh''' having '''20 cells''' along both '''x''' and '''y directions'''.
|-
|| [gedit - '''blockMeshDict''']

Close Text Editor
|| Close the '''blockMeshDict''' file.
|-
|| [Terminal]

Type: '''gedit system/controlDict'''
|| Now, let’s open the '''controlDict''' file in a '''text editor'''.
|-
|| [gedit - '''controlDict'''] Highlight:

'''deltaT'''
|| The '''time step''' for the '''simulation''' is specified using the '''keyword deltaT'''.

When '''running''' the '''simulation, temporal accuracy''' and '''numerical stability''' needs to be achieved.

The '''Courant number''' is required to be less than '''1''' to achieve this.

Please refer to the '''Additional Reading Material''' on this tutorial page for details.

It mentions the steps used to calculate the '''time-step'''.
|-
|| [gedit - '''controlDict''']

Highlight: '''0.005 '''
|| We have calculated the '''time step''' for this '''simulation''' to be '''0.005 s'''.

So, this will be the value of '''deltaT'''.
|-
|| [gedit - '''controlDict'''] Close Text Editor
|| Close the '''controlDict''' file.
|-
|| [Terminal] Type:

'''blockMesh'''
|| Let us '''mesh''' the '''geometry''' now using the '''blockMesh command''' on the '''terminal.'''
|-
|| [Terminal] Type:

'''icoFoam'''
|| We will be using the '''icoFoam solver''' to '''simulate''' the '''case'''.

Type the following '''command''' on the '''terminal''' to start the '''simulation'''.
|-
|| [Terminal] Highlight:

'''End'''
|| The iterations are now complete.
|-
|| [Terminal] Type:

'''paraFoam'''
|| Let us view the '''simulated''' results in '''ParaView''' using the '''paraFoam command'''.
|-
|| [ParaView] '''Properties''' Tab

Click on '''Apply'''
|| Click on the '''Apply''' button in the '''Properties''' tab to view the '''geometry'''.
|-
|| [ParaView] '''Active Variable Controls'''

Click on '''vtkBlockColors''' >> Click on '''p'''
|| Next, let’s view the '''pressure contours''' for the '''simulation'''.

Click on the '''vtkBlockColors''' dropdown in the '''Active Variable Controls''' and select '''p'''.
|-
|| [ParaView] '''VCR Controls'''

Click on '''Last Frame'''
|| Now, let us view the '''contours''' at the end of the '''simulation'''.

Click on the '''Last Frame''' button in the '''VCR Controls'''.
|-
|| [ParaView] '''Data Analysis'''

Click on '''Probe Location'''
|| Next, let’s see the values of '''pressure''' and '''velocity''' at the centre of the '''domain'''.

To do so, click on the '''Probe Location''' button in the '''Data Analysis''' section.
|-
|| Slide: Probe Location
||
* '''Probe Location filter''' shows the details of the points within an arbitrary '''sphere'''.
* By default, this '''sphere''' is centered at the '''center '''of the''' domain''' and has '''0''' radius.
* Changing these parameters will change the '''probe location''' or the '''range''' of the '''probe'''.
|-
|| [ParaView] Properties Tab

Click on '''Apply'''
|| We need the values at the '''centre '''of the''' domain'''.

Therefore, we stick with the default '''Sphere Parameters''' in the '''Properties''' Tab.

Click on the '''Apply''' button.
|-
|| [ParaView] '''SpreadSheetView'''
|| We can now see the velocity and pressure values in the '''SpreadSheetView'''.

Note down the value of '''pressure''' as we will be using this later.
|-
|| [ParaView] Close the Window
|| Then close the '''ParaView''' window.
|-
|| Only Narration
|| Now, let us increase the '''number of cells''' in the '''x''' and '''y direction''' to '''40 cells'''.
|-
|| Slide: Mesh Refinement
||
* This process of dividing the existing cells is called '''mesh refinement'''.
* '''Mesh refinement''' changes a '''coarse mesh''' into a '''finer mesh'''.
|-
|| [Terminal] Type:

'''gedit system/blockMeshDict'''
|| Let us open the '''blockMeshDict''' file in a '''text editor'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''40 40'''
|| Change the '''number of cells''' in '''x''' and '''y direction''' as shown.
|-
|| [gedit - '''blockMeshDict''']

Save >> Close the window
|| Save and close the file.
|-
|| Only Narration
|| Since we have changed the number of cells, we need to update the '''time step'''.

This is to ensure that the '''Courant number''' is less than '''1'''.
|-
|| [Terminal] Type:

'''gedit system/controlDict'''
|| Let’s open the '''controlDict''' file in a '''text editor'''.
|-
|| [gedit - '''controlDict''']

Highlight: '''0.0025'''
|| For the refined '''mesh''', the calculated '''time-step''' is '''0.0025 s'''.

Update '''deltaT''' as shown.
|-
|| [gedit - '''controlDict''']

Save >> Close the window
|| Save and close the file.
|-
|| [Terminal]

Type: '''blockMesh'''
|| Since we have changed the '''meshing parameters''', we need to '''mesh''' the '''geometry''' again.

On the '''terminal''', type the '''command''' as shown.
|-
|| [Terminal] Type:

'''ls'''
|| Let us view the contents of the '''cavity''' folder.

Type '''ls''' in the '''terminal.'''
|-
|| [Terminal] Highlight:

'''0.1 0.2 0.3 0.4 0.5'''
|| We can see that the files from the '''previous run''' exist in the '''cavity''' folder.
|-
|| [Terminal] Type:

'''foamListTimes -rm'''
|| Let’s remove these files by typing this '''command'''.
|-
|| [Terminal] Type:

'''icoFoam'''
|| Let’s run the '''icoFoam solver'''.
|-
|| [Terminal] Type:

'''paraFoam'''
|| And view the results in '''ParaView '''by typing '''paraFoam.'''
|-
|| [ParaView]

Click '''Apply''' >> Click on '''vtkBlockColors''' >> Click on '''p '''>> Click on '''Last Frame '''>> Click on '''Probe Location '''>> Click '''Apply'''
|| Let us find the value of the '''pressure field''' at the '''centre '''of the''' domain''' at the '''final time step'''.

As explained earlier, we use the '''Last Frame''' option to move to the '''final time step'''.

And, we use the '''Probe Location filter''' to find the '''data''' at the '''centre of the domain'''.
|-
|| [ParaView] '''SpreadSheetView'''
|| We can see the value of the '''pressure field''' at the '''centre '''of the''' domain'''.
|-
|| [ParaView] Close the Window
|| Close the '''ParaView''' window.
|-
|| Only Narration
|| Similarly, we can find the pressure at the '''centre''' for more number of cells.

Note that the '''time step''' is changed for each '''run''' depending on the '''cell size'''.
|-
|| Slide: Pressure at the Centre
|| The following table shows the '''pressure values''' for various '''numbers of cells'''.
|-
|| Slide: Pressure at the Centre
|| This is the '''Pressure versus number of cells''' plot based on the '''data'''.

Let’s consider that values within the order of '''10-3''' are acceptable.

We can see that the pressure values at '''6400''' and '''25600 cells''' differ only by an order of '''10-4'''.

Any more '''refinement''' than '''6400 cells,''' will only give us results that differ by less than '''10-3'''.

Therefore, the results from a '''mesh''' having '''6400 cells''' or more, surely gives acceptable results.

In other words, the results become independent of the '''mesh,''' if it has more than '''6400 cells'''.

What we have just performed is called a '''grid independence study'''.
|-
|| Only Narration
|| The '''Additional Reading Material''' has more details on '''grid independence study'''.

Please refer to it.
|-
|| 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:
* '''Refine''' a '''mesh''' using '''blockMeshDict'''
* Change the '''time step''' to achieve '''numerical stability''', and
* Perform a '''grid independence''' '''study'''
|-
|| 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley Melvin.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Multi-block-Meshing-of-a-2D-Geometry-in-OpenFOAM/English

2020-07-22T09:31:25Z

Ashleymelvin:

'''Title of the script''': Multi-block Meshing of 2D Geometry in OpenFOAM

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM, ParaView, blockMesh, meshing, multiple blocks, graded mesh, mesh refinement, inflation layer, pre-processing, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Multi-block Meshing of 2D Geometry in OpenFOAM'''.
|-
|| Slide: Learning Objectives
|| In this tutorial, we will learn to:
* Create a '''geometry''' with multiple '''blocks''' using '''blockMeshDict'''
* Vary '''meshing parameters''' for each '''block'''
* Label the '''boundary patches''', and''' '''
* View the '''mesh''' in '''ParaView'''
|-
|| Slide: System Specifications
|| To record this tutorial, I am using,
* '''Ubuntu Linux''' OS version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0, and
* '''gedit Text editor'''

You may use any other '''text editor''' of your choice.
|-
|| Slide: Prerequisites
* If not, please go through the prerequisite '''OpenFOAM '''tutorial on https://spoken-tutorial.org
|| As a prerequisite:
* You should be familiar with the creation of a basic '''geometry '''using the '''blockMesh''' utility.
* If not, please go through the prerequisite '''OpenFOAM '''tutorial on this website.
|-
|| Slide: Code Files
||
* The files used in this tutorial are available in the '''Code''' '''Files''' link on this tutorial page
* Please download and extract them, and
* Make a copy and then use them while practising
|-
|| Slide: Geometry
|| This is the '''geometry''' we will be creating and '''meshing '''later on.
|-
|| Slide: Faces
||
* The left and right faces are the '''inlet''' and '''outlet''' respectively.
* The top and bottom faces are the two '''walls'''.
* The front and back faces are empty faces.

The faces are empty as we are creating a '''geometry''' for a '''2D simulation'''.
|-
|| CTRL + ALT + T
|| Now, open the '''terminal''' by pressing '''Ctrl''', '''Alt''' & '''T''' keys.
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| At the '''prompt''', type the following '''command''' to go to the '''run directory'''.
|-
|| Only Narration
|| Here onwards, please remember to press the '''Enter''' key after typing each '''command''' in the '''terminal'''.
|-
|| [Terminal] Type:

'''cp -r $FOAM_TUTORIALS/incompressible/pimpleFoam/LES/channel395 .'''
|| Now, let us copy the '''case''' from the '''tutorial directory''' into the '''run directory'''.

Type the following '''command''' to do so.
|-
|| [Terminal] Type:

'''rm -r channel395/0'''
|| We will only be creating and '''meshing''' the '''geometry'''.

So, we do not need the '''boundary conditions''' folder.

Type the following '''command''' to delete the '''boundary conditions''' folder.
|-
|| [Terminal] Type:

'''gedit channel395/system/blockMeshDict'''
|| Now open the '''blockMeshDict''' file in a '''text editor'''.

I am opening it in the '''gedit text editor.'''
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''Selection in the Text Editor >> Delete'''
|| Select the contents of the file from '''vertices''' to the end of the document as shown.

Then delete the selected section as we will be entering the '''input parameters'''.
|-
|| [gedit - '''multiBlock''']
|| Next open the '''multiBlock.txt''' file that you have downloaded in the '''text editor'''.
|-
|| [gedit - '''multiBlock'''] Highlight:

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''blockMeshDict''']

'''Paste'''
|| Paste the copied content into the '''blockMeshDict '''file as shown.
|-
|| Ctrl + S
|| And save the file.
|-
|| Slide: Blocks
|| The '''geometry''' is divided into 2 '''blocks''' as shown in the figure.
|-
|| Slide: Vertices
|| There are 12 '''vertices''' and they are numbered as shown.

Note that the '''vertex''' numbering starts from 0.
|-
|| Only Narration
|| Let me switch back to the '''blockMeshDict '''file.
|-
|| Only Narration
|| Let us enter the '''coordinates''' of '''vertices''' in ascending order of their '''vertex''' numbers.

The '''vertices''' are defined using the list '''vertices'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

vertices list
|| The '''coordinates''' of the 12 '''vertices''' are entered as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''blocks '''
|| Now, let us see how the '''blocks''' for this '''geometry''' are defined.
|-
|| Slide: Blocks
|| The '''geometry''' is divided into 2 '''blocks'''.

This division enables us to '''mesh''' the top and bottom sections of the '''geometry''' differently.

The '''blocks''' are numbered as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

Block 1 definition''' '''
|| '''Block 1''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''hex'''
|| We use '''hexahedral blocks''' for '''meshing'''.
|-
|| Only Narration
|| We will enter the '''vertices''' that define '''block 1'''.

We first enter the '''vertices''' of the lower xy-plane.
|-
|| Slide: Block 1
|| To define '''block 1''',
* We first enter the '''vertices''' of the '''back face''' and then that of the '''front face'''
* When viewed along the '''negative z-direction''', the '''vertices''' should be ordered '''counterclockwise'''
* Following this convention, the '''vertices''' of the back face are 0, 1, 3 and 2
* The corresponding order of the front face is 6, 7, 9 and 8
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''0 1 3 2 6 7 9 8'''
|| The '''vertices''' of '''block 1''' are therefore entered in the order as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''40 25 1'''
|| The number of '''cells''' in each '''direction''' is defined as shown.

There is only 1 '''cell''' in the '''z direction''' as this is a '''mesh''' for '''2D simulation''' in '''xy-plane'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''simpleGrading'''
|| We use '''simpleGrading''' as the cells have uniform expansion in all directions.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''1 10 1'''
|| The ratio of width of the '''end cell''' to that of the '''start cell''' in a '''direction''' is its '''expansion ratio'''.

The '''expansion ratio''' in each '''direction''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''1 '''in x direction
|| This means that all '''cells''' have uniform width along '''x''' '''direction'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''1 '''in z direction
|| The same is the case for '''z direction'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''10 '''in y direction
|| However, along the '''y direction''', the '''end cell''' is 10 times as wide as the '''start cell'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

Block 2 definition
|| '''Block 2''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''0.1 '''in y direction
|| The '''expansion ratio''' in '''y direction''' is the only '''parameter''' different in '''block 2''' from that of '''1.'''

Along '''y direction''', the '''end cell''' is now only 0.1 times as wide as the '''start cell'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

edges list
|| Since all the edges of the '''channel geometry''' are straight lines, we leave the '''edges''' field empty.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''boundary'''
|| Let us label the '''boundary patches '''now.
|-
|| Slide: Boundary
|| The bottom and top face is as shown in the figure.

We shall name them '''wallBottom''' and '''wallTop''' respectively.
|-
|| Only Narration
|| Each face resembles the characteristics of a '''solid wall'''.

Hence, the face is of the '''type wall'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''wallBottom '''and '''wallTop '''definitions
|| The two faces are defined as shown.
|-
|| Only Narration
|| We need to impose '''cyclic boundary conditions''' on the '''inlet''' and '''outlet''' faces of '''block 1'''.
|-
|| Slide: Cyclic Patch
||
* The '''face''' '''type''' for a '''cyclic patch''' is defined using the keyword''' cyclic.'''
* The pair of '''faces''' are linked to each other through the keyword''' neighbourPatch.'''
|-
|| Slide: Boundary
|| The '''inlet''' and '''outlet''' faces of '''block 1''' are named '''in1''' and '''out1''' respectively.

The same for '''block 2''' are named '''in2''' and '''out2''' respectively.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''in1 '''definition
|| The '''inlet''' face of '''block 1''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''cyclic'''
|| The '''boundary face type''' is '''cyclic'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''neighbourPatch out1'''
|| The '''outlet''' face is linked to the '''inlet''' face using the keyword''' neighbourPatch'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''((0 6 8 2))'''
|| The '''vertices''' of the '''inlet''' face are ordered in '''clockwise direction''' when viewed from inside of '''block 1'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''out1''' definition
|| The '''outlet''' face of '''block 1''' is defined as shown here.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''in2''' and '''out2''' definitions
|| The '''inlet''' and '''outlet''' faces of '''block 2''' are defined as shown here.
|-
|| Slide: Boundary
||
* The back and front faces of '''block 1''' are named '''sides1_half0''' and '''sides1_half1''' respectively.
* The back and front faces of '''block 2''' are named '''sides2_half0''' and '''sides2_half1''' respectively.
|-
|| Only Narration
|| We are creating a '''geometry''' for a '''2D simulation''' in the '''xy-plane'''.

Therefore, the faces normal to '''z-direction''' are kept empty.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''sides1_half0''' definition
|| The back face of '''block 1''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''empty'''
|| Note that we have kept the face''' empty'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''sides1_half1''', '''sides2_half0''' and '''sides2_half1''' definition
|| Similarly, we define the other 3 faces.
|-
|| Only Narration
|| We have now finished labelling all the '''boundary patches'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

mergePatchPairs list
|| Since we do not have any '''patches''' to merge, we leave the '''mergePatchPairs''' field empty.
|-
|| [gedit - '''blockMeshDict''']

Click on Save >> Close Text Editor
|| We have now entered all the necessary '''fields'''.

Save and close the file.
|-
|| [Terminal]''' '''Type:

'''cd channel395'''
|| Come to the '''terminal''', and type '''cd (space) channel395'''.
|-
|| [Terminal] Type:

'''blockMesh '''>>''' Enter'''
|| To '''mesh''' the '''geometry''', type '''blockMesh''' and press '''Enter'''.
|-
|| [Terminal] Highlight:

'''End'''
|| The '''meshing''' is now complete.
|-
|| [Terminal] Type:

'''paraFoam'''
|| To view the '''mesh''' in '''ParaView''', type '''paraFoam'''.
|-
|| [ParaView] '''Properties''' Tab

Click on '''Apply'''
|| Click on '''Apply''' in the '''Properties''' tab.
|-
|| [ParaView] '''Active Variable Controls'''

Click on '''Surface''' >> Click on '''Surface with Edges'''
|| Click on '''Surface''' available in the '''Active Variable Controls''' and change it to '''Surface with Edges'''.

We can now see the '''mesh''' structure in the '''xy-plane'''.

Notice the '''mesh refinement''' near the top and bottom faces of the '''geometry'''.
|-
|| [ParaView] Close the Window
|| And now, close the '''ParaView''' window.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

To summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt to:
* Create a '''geometry''' with multiple '''blocks''' using '''blockMeshDict'''
* Vary '''meshing parameters''' for each '''block'''
* Label the '''boundary patches''', and
* View the '''mesh''' in '''ParaView'''
|-
|| Slide: Assignment
|| As an assignment:
* Create a '''geometry''' having dimensions '''5 m''', '''4 m''' and '''3 m''' along '''x''', '''y''' and '''z axis'''
* Divide the '''geometry''' into 2 equal''' blocks '''along the''' x axis'''
* Mesh the '''geometry''' such that it has '''25''', '''20''' and '''1 cell''' along '''x''', '''y''' and '''z axis''' for each '''block'''
* Set expansion ratio as '''10''', '''1''' and '''1''' along the '''x''', '''y''' and '''z axis '''for both the '''blocks''', and
* View the '''mesh''' 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 this 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley Melvin.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Multi-block-Meshing-of-a-2D-Geometry-in-OpenFOAM/English

2020-07-21T15:27:22Z

Ashleymelvin: Created page with "'''Title of the script''': Multi-block Meshing of 2D Geometry in OpenFOAM '''Author''': Ashley Melvin '''Keywords''': OpenFOAM, ParaView, blockMesh, meshing, multiple blocks..."

'''Title of the script''': Multi-block Meshing of 2D Geometry in OpenFOAM

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM, ParaView, blockMesh, meshing, multiple blocks, graded mesh, mesh refinement, inflation layer, pre-processing, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Multi-block Meshing of 2D Geometry in OpenFOAM'''.
|-
|| Slide: Learning Objectives
|| In this tutorial, we will learn to:
* Create a '''geometry''' with multiple '''blocks''' using '''blockMeshDict'''
* Vary '''meshing parameters''' for each '''block'''
* Label the '''boundary patches''', and''' '''
* View the '''mesh''' in '''ParaView'''
|-
|| Slide: System Specifications
|| To record this tutorial, I am using,
* '''Ubuntu Linux''' OS version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0, and
* '''gedit Text editor'''

You may use any other '''text editor''' of your choice.
|-
|| Slide: Prerequisites
* If not, please go through the prerequisite '''OpenFOAM '''tutorial on https://spoken-tutorial.org
|| As a prerequisite:
* You should be familiar with the creation of a basic '''geometry '''using the '''blockMesh''' utility.
* If not, please go through the prerequisite '''OpenFOAM '''tutorial on this website.
|-
|| Slide: Code Files
||
* The files used in this tutorial are available in the '''Code''' '''Files''' link on this tutorial page
* Please download and extract them, and
* Make a copy and then use them while practising
|-
|| Slide: Geometry
|| This is the '''geometry''' we will be creating and '''meshing '''later on.
|-
|| Slide: Faces
||
* The left and right faces are the '''inlet''' and '''outlet''' respectively.
* The top and bottom faces are the two '''walls'''.
* The front and back faces are empty faces.

The faces are empty as we are creating a '''geometry''' for a '''2D simulation'''.
|-
|| CTRL + ALT + T
|| Now, open the '''terminal''' by pressing '''Ctrl''', '''Alt''' & '''T''' keys.
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| At the '''prompt''', type the following '''command''' to go to the '''run directory'''.
|-
|| Only Narration
|| Here onwards, please remember to press the '''Enter''' key after typing each '''command''' in the '''terminal'''.
|-
|| [Terminal] Type:

'''cp -r $FOAM_TUTORIALS/incompressible/pimpleFoam/LES/channel395 .'''
|| Now, let us copy the '''case''' from the '''tutorial directory''' into the '''run directory'''.

Type the following '''command''' to do so.
|-
|| [Terminal] Type:

'''rm -r channel395/0'''
|| We will only be creating and '''meshing''' the '''geometry'''.

So, we do not need the '''boundary conditions''' folder.

Type the following '''command''' to delete the '''boundary conditions''' folder.
|-
|| [Terminal] Type:

'''gedit channel395/system/blockMeshDict'''
|| Now open the '''blockMeshDict''' file in a '''text editor'''.

I am opening it in the '''gedit text editor.'''
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''Selection in the Text Editor >> Delete'''
|| Select the contents of the file from '''vertices''' to the end of the document as shown.

Then delete the selected section as we will be entering the '''input parameters'''.
|-
|| [gedit - '''multiBlock''']
|| Next open the '''multiBlock.txt''' file that you have downloaded in the '''text editor'''.
|-
|| [gedit - '''multiBlock'''] Highlight:

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''blockMeshDict''']

'''Paste'''
|| Paste the copied content into the '''blockMeshDict '''file as shown.
|-
|| Ctrl + S
|| And save the file.
|-
|| Slide: Blocks
|| The '''geometry''' is divided into 2 '''blocks''' as shown in the figure.
|-
|| Slide: Vertices
|| There are 12 '''vertices''' and they are numbered as shown.

Note that the '''vertex''' numbering starts from 0.
|-
|| Only Narration
|| Let me switch back to the '''blockMeshDict '''file.
|-
|| Only Narration
|| Let us enter the '''coordinates''' of '''vertices''' in ascending order of their '''vertex''' numbers.

The '''vertices''' are defined using the list '''vertices'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

vertices list
|| The '''coordinates''' of the 12 '''vertices''' are entered as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''blocks '''
|| Now, let us see how the '''blocks''' for this '''geometry''' are defined.
|-
|| Slide: Blocks
|| The '''geometry''' is divided into 2 '''blocks'''.

This division enables us to '''mesh''' the top and bottom sections of the '''geometry''' differently.

The '''blocks''' are numbered as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

Block 1 definition''' '''
|| '''Block 1''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''hex'''
|| We use '''hexahedral blocks''' for '''meshing'''.
|-
|| Only Narration
|| We will enter the '''vertices''' that define '''block 1'''.

We first enter the '''vertices''' of the lower xy-plane.
|-
|| Slide: Block 1
|| To define '''block 1''',
* We first enter the '''vertices''' of the '''back face''' and then that of the '''front face'''
* When viewed along the '''negative z-direction''', the '''vertices''' should be ordered '''counterclockwise'''
* Following this convention, the '''vertices''' of the back face are 0, 1, 3 and 2
* The corresponding order of the front face is 6, 7, 9 and 8
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''0 1 3 2 6 7 9 8'''
|| The '''vertices''' of '''block 1''' are therefore entered in the order as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''40 25 1'''
|| The number of '''cells''' in each '''direction''' is defined as shown.

There is only 1 '''cell''' in the '''z direction''' as this is a '''mesh''' for '''2D simulation''' in '''xy-plane'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''simpleGrading'''
|| We use '''simpleGrading''' as the cells have uniform expansion in all directions.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''1 10 1'''
|| The ratio of width of the '''end cell''' to that of the '''start cell''' in a '''direction''' is its '''expansion ratio'''.

The '''expansion ratio''' in each '''direction''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''1 '''in x direction
|| This means that all '''cells''' have uniform width along '''x''' '''direction'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''1 '''in z direction
|| The same is the case for '''z direction'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''10 '''in y direction
|| However, along the '''y direction''', the '''end cell''' is 10 times as wide as the '''start cell'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

Block 2 definition
|| '''Block 2''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''0.1 '''in y direction
|| The '''expansion ratio''' in '''y direction''' is the only '''parameter''' different in '''block 2''' from that of '''1.'''

Along '''y direction''', the '''end cell''' is now only 0.1 times as wide as the '''start cell'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

edges list
|| Since all the edges of the '''channel geometry''' are straight lines, we leave '''edges''' field empty.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''boundary'''
|| Let us label the '''boundary patches '''now.
|-
|| Slide: Boundary
|| The bottom and top face is as shown in the figure.

We shall name them '''wallBottom''' and '''wallTop''' respectively.
|-
|| Only Narration
|| Each face resembles the characteristics of a '''solid wall'''.

Hence, the face is of the '''type wall'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''wallBottom '''and '''wallTop '''definitions
|| The two faces are defined as shown.
|-
|| Only Narration
|| We need to impose '''cyclic boundary conditions''' on the '''inlet''' and '''outlet''' faces of '''block 1'''.
|-
|| Slide: Cyclic Patch
||
* The '''face''' '''type''' for a '''cyclic patch''' is defined using the keyword''' cyclic.'''
* The pair of '''faces''' are linked to each other through the keyword''' neighbourPatch.'''
|-
|| Slide: Boundary
|| The '''inlet''' and '''outlet''' faces of '''block 1''' are named '''in1''' and '''out1''' respectively.

The same for '''block 2''' are named '''in2''' and '''out2''' respectively.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''in1 '''definition
|| The '''inlet''' face of '''block 1''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''cyclic'''
|| The '''boundary face type''' is '''cyclic'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''neighbourPatch out1'''
|| The '''outlet''' face is linked to the '''inlet''' face using the keyword''' neighbourPatch'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''((0 6 8 2))'''
|| The '''vertices''' of the '''inlet''' face are ordered in '''clockwise direction''' when viewed from inside of '''block 1'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''out1''' definition
|| The '''outlet''' face of '''block 1''' is defined as shown here.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''in2''' and '''out2''' definitions
|| The '''inlet''' and '''outlet''' faces of '''block 2''' are defined as shown here.
|-
|| Slide: Boundary
||
* The back and front faces of '''block 1''' are named '''sides1_half0''' and '''sides1_half1''' respectively.
* The back and front faces of '''block 2''' are named '''sides2_half0''' and '''sides2_half1''' respectively.
|-
|| Only Narration
|| We are creating a '''geometry''' for a '''2D simulation''' in the '''xy-plane'''.

Therefore, the faces normal to '''z-direction''' are kept empty.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''sides1_half0''' definition
|| The back face of '''block 1''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''empty'''
|| Note that we have kept the face''' empty'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''sides1_half1''', '''sides2_half0''' and '''sides2_half1''' definition
|| Similarly, we define the other 3 faces.
|-
|| Only Narration
|| We have now finished labelling all the '''boundary patches'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

mergePatchPairs list
|| Since we do not have any '''patches''' to merge, we leave the '''mergePatchPairs''' field empty.
|-
|| [gedit - '''blockMeshDict''']

Click on Save >> Close Text Editor
|| We have now entered all the necessary '''fields'''.

Save and close the file.
|-
|| [Terminal]''' '''Type:

'''cd channel395'''
|| Come to the '''terminal''', and type '''cd (space) channel395'''.
|-
|| [Terminal] Type:

'''blockMesh '''>>''' Enter'''
|| To '''mesh''' the '''geometry''', type '''blockMesh''' and press '''Enter'''.
|-
|| [Terminal] Highlight:

'''End'''
|| The '''meshing''' is now complete.
|-
|| [Terminal] Type:

'''paraFoam'''
|| To view the '''mesh''' in '''ParaView''', type '''paraFoam'''.
|-
|| [ParaView] '''Properties''' Tab

Click on '''Apply'''
|| Click on '''Apply''' in the '''Properties''' tab.
|-
|| [ParaView] '''Active Variable Controls'''

Click on '''Surface''' >> Click on '''Surface with Edges'''
|| Click on '''Surface''' available in the '''Active Variable Controls''' and change it to '''Surface with Edges'''.

We can now see the '''mesh''' structure in the '''xy-plane'''.

Notice the '''mesh refinement''' near the top and bottom faces of the '''geometry'''.
|-
|| [ParaView] Close the Window
|| And now, close the '''ParaView''' window.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

To summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt to:
* Create a '''geometry''' with multiple '''blocks''' using '''blockMeshDict'''
* Vary '''meshing parameters''' for each '''block'''
* Label the '''boundary patches''', and
* View the '''mesh''' in '''ParaView'''
|-
|| Slide: Assignment
|| As an assignment:
* Create a '''geometry''' having dimensions '''5 m''', '''4 m''' and '''3 m''' along '''x''', '''y''' and '''z axis'''
* Divide the '''geometry''' into 2 equal''' blocks '''along the''' x axis'''
* Mesh the '''geometry''' such that it has '''25''', '''20''' and '''1 cell''' along '''x''', '''y''' and '''z axis''' for each '''block'''
* Set expansion ratio as '''10''', '''1''' and '''1''' along the '''x''', '''y''' and '''z axis '''for both the '''blocks''', and
* View the '''mesh''' 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 this 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley Melvin.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Creating-2D-Channel-Geometry-and-Mesh-in-OpenFOAM/English

2020-07-21T08:39:20Z

Ashleymelvin: Created page with "'''Title of the script''': Creating 2D Channel Geometry and Mesh in OpenFOAM '''Author''': Ashley Melvin '''Keywords''': OpenFOAM, ParaView, channel flow, blockMesh, meshing..."

'''Title of the script''': Creating 2D Channel Geometry and Mesh in OpenFOAM

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM, ParaView, channel flow, blockMesh, meshing, structured mesh, graded mesh, pre-processing, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Creating 2D Channel Geometry and Mesh in OpenFOAM'''.
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn to:
* Create a '''2D channel''' '''geometry''' using '''blockMeshDict'''
* '''Mesh''' a '''geometry'''
* Label the '''boundary patches''', and''' '''
* View the '''mesh''' in '''ParaView'''
|-
|| Slide: System Specifications
|| To record this tutorial, I am using,
* '''Ubuntu Linux''' OS version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0, and
* '''gedit Text Editor'''

You may use any other '''editor''' of your choice.
|-
|| Slide: Code Files
||
* The files used in this tutorial are available in the '''Code''' '''Files''' link on this tutorial page
* Please download and extract them
* Make a copy and then use them while practising
|-
|| Slide: 2D Channel Flow
|| The problem description of '''2D flow in a channel '''is as shown in the diagram.
|-
|| Slide: Channel Geometry
|| This is the '''geometry''' for''' 2D flow in a channel'''.
|-
|| Slide: Faces
|| The '''faces''' of the geometry are:
* '''Inlet''' and '''outlet'''
* Bottom and top walls
* Back face, and
* Front face
|-
|| CTRL + ALT + T
|| Open the '''terminal''' by pressing '''Ctrl''', '''Alt''' & '''T''' keys.
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| At the '''prompt''', type the following '''command''' to go to the '''run directory'''.
|-
|| Only Narration
|| Here onwards, please remember to press the '''Enter''' key after typing each '''command''' in the '''terminal'''.
|-
|| [Terminal] Type:

'''cp -r $FOAM_TUTORIALS/incompressible/pimpleFoam/LES/channel395 .'''
|| Let us now copy the '''case''' of '''flow in a channel''' from the '''tutorial directory''' into the '''run directory'''.

Type the following '''command''' to do so.
|-
|| [Terminal] Type:

'''rm -r channel395/0'''
|| We will only be creating and '''meshing''' the '''geometry'''.

Hence, we do not need the '''boundary conditions''' folder.

Type the following '''command''' to delete the '''boundary conditions''' folder.
|-
|| [Terminal] Type:

'''gedit channel395/system/blockMeshDict'''
|| The '''blockMeshDict''' file is located in the '''system''' folder.

Let us open it in any '''text editor'''.

I am doing it in '''gedit Text Editor'''.
|-
|| [gedit - '''blockMeshDict''']
|| We can now see the '''blockMeshDict''' file.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> Delete'''
|| Select the contents of the file from '''vertices''' to the end of the document, as shown.

We don’t need the selected content as we will be entering the '''input parameters'''.

Hence, '''delete''' the selected section.

The remaining content is common for all '''blockMeshDict''' files.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''convertToMeters 1'''
|| The unit of the coordinates entered in the '''blockMesh dictionary''' needs to be specified.

It is defined using the '''keyword convertToMeters.'''

The value '''1''' indicates that the values of all the '''coordinates''' are in meters.
|-
|| [gedit - '''channel''']
|| Open the '''channel.txt''' file, that you had downloaded, in a '''text editor'''.
|-
|| [gedit - '''channel'''] Highlight

'''Selection in the Text Editor >> Copy '''
|| Copy the entire content of the text file.
|-
|| [gedit - '''blockMeshDict''']
|| Let me switch back to the '''blockMeshDict''' file.
|-
|| [gedit - '''blockMeshDict''']

'''Paste'''
|| Paste the copied contents into the '''blockMeshDict '''file as shown.
|-
|| Slide: Vertices
|| The vertices of the '''channel geometry''' are numbered as indicated.

The vertex numbering starts from 0.
|-
|| [gedit - '''blockMeshDict'''] Highlight

Vertices List

|| The coordinates of the vertices are entered as shown.

Note that the vertices are entered in the ascending order of their vertex numbers.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''(0 0 0)'''
|| '''Vertex''' '''0''' is located at the '''origin'''.

Its coordinates are entered as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''(4 0 0) '''
|| The''' x, y '''and''' z '''coordinates''' '''of vertex''' 1 '''are '''4''', '''0''' and '''0''' respectively.

Its coordinates are entered as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''(0 2 0) '''and''' (4 2 0)'''
|| Similarly, the coordinates of vertex''' 2 '''and''' 3''' are entered as shown.
|-
|| Only Narration
|| The '''z '''coordinate of all the points on the front face is 2.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''(0 0 2) to (4 2 2)'''
|| The coordinates of front face vertices''' 4, 5, 6 '''and''' 7''' are entered as shown.
|-
|| Only Narration
|| For '''meshing''', '''OpenFOAM''' requires '''3-dimensional blocks''' to be defined.

The '''blocks''' are specified using the vertices that define them.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

Blocks List
|| We use a single '''block''' in our '''geometry'''.

The '''block''' is defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''hex'''
|| We use '''hexahedral blocks''' for '''meshing'''.
|-
|| Only Narration
|| The order in which the vertices are specified define the '''block'''.

We first enter the vertices of the lower xy-plane, in this case, the back face.

We start from the '''origin''' and enter the vertices of the face.

When viewed along the '''negative z-direction''', the vertices should be ordered counterclockwise.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''0 1 3 2 '''
|| The vertices of the back face are defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''4 5 7 6'''
|| The vertices of the front face are entered in the same order as that of the back face.
|-
|| Only Narration
|| Let us start defining the '''meshing parameters''' of the '''block'''.

We first define the number of '''cells''' in each direction of the '''block'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''40 25 1'''
|| The number of '''cells''' in each '''direction''' is defined as shown.

This indicates that there are 40 cells in '''x direction''' and 25 cells in '''y direction'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''1 '''
|| There is only one '''cell''' along '''z direction''' indicating that the '''simulation''' is '''2D''' in '''xy-plane'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''simpleGrading'''
|| Next, let us define how the '''mesh''' is '''graded'''.

We use '''simpleGrading''' as the cells have '''uniform expansion''' in all '''directions'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''1 1 1'''
|| Let us now define the '''expansion ratios''' in each '''direction'''.

'''Expansion ratio''' along a '''direction''' is the ratio of width of the '''end cell''' to that of the '''start cell''' in that '''direction'''.

Since the '''cell''' width is uniform in all '''directions''', the '''expansion ratio''' is '''1'''.
|-
|| Only Narration
|| Now, let us define the '''edges'''.

'''Edges''' are used to define '''arc''' or '''spline edges'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

Edges List
|| Since all the '''edges''' of '''channel geometry''' are straight lines, we leave it empty.
|-
|| Only Narration
|| Let us label the '''boundary patches'''.

The labels are used to impose '''boundary conditions''' on the respective faces.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''boundary'''
|| '''Boundary '''labels are defined using the '''boundary''' list.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''bottomWall'''
|| The bottom face of the '''geometry''' is named '''bottomWall'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''type'''
|| The '''patch type''' of the '''boundary''' is defined using the '''keyword type'''.

|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''wall'''
|| The bottom face resembles the characteristics of a '''solid wall'''.

Hence, the face is of the '''type wall'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''faces'''
|| Vertices define a face.

The vertices and their order for a face is defined using the '''keyword faces'''.
|-
|| Slide: Bottom Wall
|| Since the '''block '''face is a quadrilateral, it is defined by 4 vertices.

When viewed from inside the '''block''', the vertices of the face should be ordered clockwise.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''0 1 5 4'''
|| Keeping this in mind, the vertices of the bottom wall are ordered as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''topWall '''definition
|| Following the same convention, the top face is named '''topWall''' and is defined as shown.
|-
|| Only Narration
|| We are creating the '''geometry''' for a '''2D simulation''' in '''xy-plane'''.

We do not need to solve in the '''z-direction'''.

Hence, we keep the front and back faces empty.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''Back '''and''' front '''planes definitions
|| The back and front faces are defined as shown.
|-
|| Only Narration
|| The '''inlet''' and '''outlet''' faces need the application of '''boundary condition'''.

Since they do not contain any '''geometric''' or '''topological''' information, a '''generic''' label would suffice.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''patch'''
|| Such '''generic boundaries''' are labelled using the '''keyword patch'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''Inlet '''and''' outlet '''planes definitions
|| The '''inlet''' and '''outlet''' faces are defined as shown.
|-
|| Only Narration
|| We have finished labelling all the '''boundary patches'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''mergePatchPairs'''
|| Next, we merge faces using the '''mergePatchPairs '''field.

We merge faces when a '''patch '''face from one '''block''' is connected to a '''patch '''face of another '''block'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight:

'''mergePatchPairs '''List
|| Our '''geometry''' has only one '''block''' and there are no '''patches''' to merge.

Therefore, we leave the '''mergePatchPairs field''' empty.
|-
|| [gedit - '''blockMeshDict''']

Save >> Close the window
|| We have entered all the necessary '''fields'''.

Save and close the file.
|-
|| [Terminal] Type:

'''cd channel395'''
|| In the '''terminal''', type '''cd(space)channel395'''.
|-
|| [Terminal] Type:

'''blockMesh '''>>''' Enter'''
|| Let us '''mesh''' the '''geometry'''.

Type '''blockMesh''' and press '''Enter''' to do so.
|-
|| [Terminal] Highlight: '''End'''
|| The '''meshing''' is complete.
|-
|| [Terminal] Type:

'''paraFoam '''>>''' Enter'''
|| To view the '''mesh''' in '''ParaView''', type '''paraFoam''' and press '''Enter'''.
|-
|| [ParaView]

Click on '''Apply'''
|| Click on the green coloured '''Apply''' on the left side of your window in the '''Properties''' tab.
|-
|| [ParaView]

Click on '''Surface''' >> Click on '''Surface with Edges'''
|| Click on '''Surface''' available in the '''Representation Toolbar''' and change it to '''Surface with Edges'''.

You can now see the '''mesh''' structure of the '''front''' face.
|-
|| [ParaView] Close the window
|| Close the '''ParaView''' window.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

Let us summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt to:
* Create a '''2D channel geometry''' using '''blockMeshDict'''
* '''Mesh''' a '''geometry'''
* Label the '''boundary patches''', and
* View the '''mesh''' in '''ParaView'''
|-
|| Slide: Assignment
|| As an assignment:
* Create a '''geometry''' having dimensions '''5 m''', '''4 m''' and '''3 m''' along '''x''', '''y''' and '''z axis'''
* Mesh the '''geometry''' such that it has '''50''', '''40''' and '''1 cell''' along '''x''', '''y''' and '''z axis''', and
* View the '''mesh''' 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 this 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley Melvin.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Setting-up-a-Test-Case-in-OpenFOAM/English

2020-07-20T19:52:40Z

Ashleymelvin:

'''Title of the script''': Setting-up a test case in OpenFOAM

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM, ParaView, lid driven cavity, pre-processing, blockMesh, controlDict, post-processing, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Setting up a test case in OpenFOAM'''.
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn to:
* Set up a '''case''' in '''OpenFOAM'''
* Access the '''case files''' using '''terminal'''
* '''Pre-process''' a '''case'''
* '''Run''' a '''case''', and
* '''Post-process''' a '''case'''
|-
|| Slide: System Specifications
|| This tutorial is recorded using,
* '''Ubuntu Linux''' OS version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0, and
* '''gedit''' Text editor
You may use any other '''text editor''' of your choice.
|-
|| Slide: Prerequisites
* If not, please go through the prerequisite '''Linux '''tutorials on https://spoken-tutorial.org
|| As a prerequisite:
* You should be familiar with basic '''Linux commands'''.
* If not, please go through the prerequisite '''Linux '''tutorials on this website.
|-
|| Slide: Lid Driven Cavity
|| In this tutorial, we will learn to set up the '''lid driven cavity case'''.

'''Lid driven cavity''' is one of the most widely used '''2D test cases''' for the validation of a '''CFD '''code.
|-
|| Slide: Diagram
|| This is the diagram of '''Lid Driven Cavity Flow'''.

It consists of 3 fixed walls and a moving top wall.
|-
|| Highlight '''Terminal''' on the machine
|| Open a '''terminal''' by pressing the '''Ctrl, Alt '''and''' T''' keys together.
|-
|| Only Narration
|| Here onwards please remember to press the '''Enter''' key after typing each '''command'''.
|-
|| [Terminal] Type:
'''mkdir -p $FOAM_RUN'''
|| Now, let’s create a '''run directory'''.

To do so, type the '''command''' as shown.
|-
|| [Terminal] Highlight

'''FOAM_RUN'''
|| '''Tutorial cases''' will later be copied into the '''run directory'''.
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| Go to the '''run directory''' using the '''cd command'''.

Now our '''present working directory''' is the '''run directory'''.
|-
|| Only Narration
|| '''OpenFOAM''' installation comes with a set of '''test cases'''.

The '''tutorial directory''' contains these '''test cases'''.

The '''Lid driven cavity case''' already exists inside the '''tutorial directory'''.
|-
|| [Terminal] Type:

'''cp -r $FOAM_TUTORIALS/incompressible/icoFoam/cavity/cavity .'''
|| We’ll now copy the '''Lid driven cavity case''' from the '''tutorial directory''' into the '''run directory'''.

To do so, type the following '''command'''.
|-
|| Slide: blockMesh
||
* The '''mesh generator''' for '''OpenFOAM''' is a utility called '''blockMesh'''.
* The '''input dictionary''' for '''blockMesh''' utility is '''blockMeshDict'''.
|-
|| [Terminal] Type:

'''gedit cavity/system/blockMeshDict'''
|| The '''blockMeshDict''' file is located in the '''system''' folder.

Open the '''blockMeshDict''' file in a '''text editor'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight

vertices, blocks, edges and boundary
|| Now let’s look at the contents of the file.

The '''blockMeshDict''' contains details of the geometry like vertices, blocks, edges and boundaries.
|-
|| [gedit - '''blockMeshDict'''] Close the window
|| Close the '''blockMeshDict''' file.
|-
|| [Terminal] Type:

'''cd cavity/0'''
|| The '''0''' folder contains the initial and boundary conditions for the '''simulation'''.

Type the following '''command''' to move into the '''0''' folder inside the '''cavity case directory'''.
|-
|| [Terminal] Type:

'''ls'''
|| Type '''ls''' and press '''Enter''' to view the files in the '''0''' folder.
|-
|| [Terminal] Highlight

'''p''' and '''U'''
|| The '''0''' folder contains the '''kinematic pressure file p''' and the '''velocity file U'''.
|-
|| [Terminal] Type:

'''gedit p'''
|| Open the '''kinematic pressure file p''' in a '''text editor'''.
|-
|| Only Narration
|| The '''p''' file contains the '''initial''' and '''boundary''' conditions of '''kinematic''' pressure.
|-
|| [gedit - '''p'''] Highlight

'''dimensions [0 2 -2 0 0 0 0] '''
|| The '''dimensions''' of '''kinematic pressure''' is meter squared per second squared.
|-
|| [gedit - '''p'''] Highlight

'''internalField '''
|| The '''internalField''' defines the values in the interior of the domain.
|-
|| [gedit - '''p'''] Highlight

'''uniform 0'''
|| The initial field is set as '''0 kinematic pressure'''.

This field is '''uniform''' across the domain.
|-
|| [gedit - '''p'''] Highlight

Both the '''zeroGradient'''
|| You can see that all walls are imposed with a '''zero gradient''' pressure boundary condition.
|-
|| [gedit - '''p'''] Close the window
|| Let us close the '''p''' file.
|-
|| [Terminal] Type:

'''gedit U'''
|| Now open the '''velocity file U''' in a '''text editor'''.
|-
|| Only Narration
|| The '''U file''' contains the initial and boundary conditions of '''velocity'''.
|-
|| [gedit - '''U'''] Highlight

'''uniform (1 0 0);'''
|| You can see that the '''moving wall''' is imposed with a '''velocity''' of '''1 m/s''' in the x direction.
|-
|| [gedit - '''U'''] Highlight

'''noSlip '''
|| Also notice that the '''no-slip''' condition is imposed on the three '''fixed walls'''.
|-
|| [gedit - '''U'''] Close the window
|| Now let us close the '''U''' file.
|-
|| [Terminal] Type:

'''cd ..'''
|| We’ll go back to the '''cavity''' folder.

Type '''cd (space)(dot)(dot)'''
|-
|| [Terminal] Type:

'''gedit constant/transportProperties'''
|| Next, we will view the '''transport properties file '''which is in the '''constant '''folder.
|-
|| [gedit - '''transportProperties'''] Highlight

'''nu '''
|| The '''transportProperties''' file contains the details of '''kinematic''' '''viscosity'''.
|-
|| [gedit - '''transportProperties''']

Highlight '''[0 2 -1 0 0 0 0] '''
|| The dimensions of '''kinematic viscosity''' is meter squared per second.
|-
|| Slide: Kinematic Viscosity
||
* The '''kinematic viscosity''' is defined by:
𝜈 = |U|𝑑 / 𝑅𝑒
where '''velocity''' (|U|) = '''1 m/s'''
characteristic length (d) = '''0.1 m'''
* The '''Reynolds number (Re)''' for the '''flow''' is taken as '''10'''
* The '''kinematic viscosity (𝜈) '''is therefore '''0.01 m2/s'''
|-
|| Narration Only
|| Now let me switch back to '''transportProperties''' file.
|-
|| [gedit - '''transportProperties''']

Highlight '''0.01'''
|| The value of '''kinematic''' '''viscosity''' is indicated in the '''transportProperties''' file.
|-
|| [gedit - '''transportProperties'''] Close the window
|| Close the '''transportProperties''' file.
|-
|| [Terminal] Type:

'''cd system'''
|| To move into the '''system''' folder, type the following '''command'''.
|-
|| [Terminal] Type:

'''ls'''
|| Type '''ls''' to view the contents of the '''system''' folder.
|-
|| [Terminal] Highlight

'''blockMeshDict controlDict fvSchemes fvSolution'''
|| The '''system''' folder contains the following files:

'''blockMeshDict''', '''controlDict''', '''fvSchemes''' and '''fvSolution'''.
|-
|| [Terminal] Highlight

'''fvSchemes'''
|| The '''fvSchemes dictionary''' contains the '''finite''' '''volume''' '''discretisation''' '''schemes'''.
|-
|| [Terminal] Highlight

'''fvSolution'''
|| The '''fvSolution dictionary''' contains the '''linear''' '''equation''' '''solvers''' and '''tolerances'''.

It contains other '''algorithm controls''' as well.
|-
|| [Terminal] Highlight

'''controlDict'''
|| The '''controlDict dictionary''' contains the '''simulation''' '''control''' '''parameters'''.

The '''dictionary''' input includes the '''control''' '''of time''' and '''reading''' and '''writing''' of the '''solution''' '''data'''.
|-
|| [Terminal] Type:

'''gedit controlDict'''
|| Let’s now open the '''controlDict''' file in a '''text editor'''.
|-
|| [Terminal] Highlight

'''startFrom '''and '''startTime'''
|| The '''start '''and''' stop times''' and the '''time step''' for the '''run''' must be set.
|-
|| [gedit - '''controlDict'''] Highlight

'''startTime''' '''0;'''
|| The '''start time''' is set at '''0''' seconds.
|-
|| [gedit - '''controlDict'''] Highlight

'''stopAt''' '''endTime;'''
|| The time at which the '''simulation''' stops is specified using the '''keyword stopAt'''.

Here, '''stopAt''' is specified using the keyword '''endTime'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''endTime''' '''0.5;'''
|| The '''endTime''' is set at '''0.5''' seconds.

This means that '''simulation''' stops after '''0.5''' seconds.
|-
|| [gedit - '''controlDict'''] Highlight

'''deltaT 0.005;'''
|| The value of the '''keyword deltaT''' defines the '''time step''' for the '''simulation'''.

The '''time step''' for the current '''simulation''' is set as '''0.005''' seconds.

'''Temporal accuracy''' and '''numerical stability''' is essential while running the '''simulation'''.

To achieve this, a''' Courant number''' of less than 1 is required.

Keeping this in mind, the '''time step''' is set to '''0.005''' seconds.
|-
|-
|-
|| [gedit - '''controlDict'''] Highlight

'''application''' '''icoFoam'''<nowiki>;</nowiki>
|| '''icoFoam''' is the '''OpenFOAM solver''' used to '''simulate''' the '''lid driven cavity''' '''flow'''.
|-
|| [gedit - '''controlDict'''] Close the window
|| Close the '''controlDict''' file.
|-
|| [Terminal] Type:

'''cd ..'''
|| Go back to the '''cavity''' folder using '''cd command'''.
|-
|| [Terminal] Type:

'''blockMesh''' >> '''Enter'''
|| Type the '''command blockMesh''' and press '''Enter''' to '''mesh''' the '''geometry'''.

The '''command''' takes input from the '''blockMeshDict dictionary''' and creates the '''geometry''' and '''meshes''' it.
|-
|| [Terminal] Highlight '''End'''
|| The '''meshing''' is now complete.
|-
|| [Terminal] Type:

'''icoFoam'''
|| The '''lid driven cavity flow''' is an '''incompressible flow'''.

It is solved using the''' OpenFOAM solver icoFoam.'''

To start the '''simulation''', type '''icoFoam''' in the '''terminal.'''
|-
|| [Terminal] Highlight '''End'''
|| The iterations are now complete.
|-
|| [Terminal] Type:

'''paraFoam'''
|| Let us view the '''simulated''' results in '''ParaView'''.

So, type '''paraFoam''' in the '''terminal.'''
|-
|| [ParaView] '''Properties''' Tab

Click on '''Apply'''
|| In the '''ParaView''' window, go to the '''Properties''' tab on the left.

Then click on the green coloured '''Apply '''button'''.'''
|-
|| [ParaView]

Click on '''vtkBlockColors''' >> Click on '''U'''
|| Go to the '''Active Variable Controls '''at the top.

Click on the '''vtkBlockColors''' dropdown and select '''U'''.

Ensure that you click on the '''U''' option with a '''point icon''' and not the '''box icon''', in the dropdown.

The '''box icon''' would display '''contours''' without any grading.
|-
|| [ParaView]

Velocity Contours in the Layout
|| The '''velocity''' '''contour''' at the start of the '''simulation''' is now displayed in the''' layout'''.
|-
|| [ParaView]

Go to '''VCR Controls''' and click on the '''Play''' Button
|| Let us see how the '''velocity contours''' develop through the '''simulation'''.

To do so, go to the '''VCR Controls''' and click on the '''Play''' button.
|-
|| [ParaView]

Final Velocity Contours in the Layout
|| The '''velocity contour''' at the end of the '''simulation''' is now displayed in the''' layout'''.
|-
|| [ParaView] Close the Window
|| Close the '''ParaView''' window.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

To summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt to:
* Set up a''' case''' in '''OpenFOAM'''
* Access the '''case files''' using '''terminal'''
* '''Pre-process''' a '''case'''
* '''Run''' a '''case''', and
* '''Post-process''' a '''case'''
|-
|| 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 this 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley Melvin.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Installing-OpenFOAM-in-Ubuntu-Linux/English

2020-07-20T19:38:12Z

Ashleymelvin:

'''Title of the script''': Installing OpenFOAM in Ubuntu

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM, ParaView, Linux, Ubuntu 18.04, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Installing OpenFOAM in Ubuntu Linux OS'''.
|-
|| Slide: Learning Objective

|| In this tutorial, we will learn how to install:
* '''OpenFOAM''' version 7 and
* '''ParaView''' version 5.6.0
|-
|| Slide: System Specifications
|| This tutorial is recorded using:
* '''Ubuntu Linux''' OS version 18.04
* A working '''Internet''' connection and
* A '''text editor'''
|-
|| Only Narration
|| We will install '''OpenFOAM''' using the '''terminal'''.
|-
|| Highlight '''Terminal''' on the machine
|| Open a '''terminal''' by pressing '''Ctrl, Alt and T''' keys together.

Make sure that you are connected to the '''Internet'''.
|-
|| [Terminal]

sudo sh -c "wget -O - http://dl.openfoam.org/gpg.key | apt-key add -"
|| A public key needs to be added to the '''repository'''.

This key enables the '''repository''' to verify '''OpenFOAM package signatures.'''

To do this, in the '''Terminal''', carefully type the following '''command''' and press '''Enter'''.
|-
|| [Terminal]

Type the password >> Press Enter.
|| The machine will ask for the '''system password'''.

Type the '''password''' and press '''Enter'''.
|-
|| Only Narration
|| Let me clear the screen.
|-
|| [Terminal]

sudo add-apt-repository http://dl.openfoam.org/ubuntu
|| Now type the following '''command''' and press '''Enter'''.

This will enable '''apt''' to search for '''dl.openfoam.org''' in the list of '''software repositories'''.
|-
|| Only Narration
|| Here onwards, please remember to press the '''Enter''' key after typing each '''command'''.

Let me clear the screen.
|-
|| [Terminal]

sudo apt-get update
|| Now type the following '''command''' to update the '''apt package''' list.
|-
|| [Terminal]

sudo apt-get -y install openfoam7
|| The '''repository''' is updated.

Next let us install '''OpenFOAM '''version 7.

To do so, type the following '''command''' in the '''terminal'''.
|-
|| [Terminal]

Point to the installation process
|| The installation may take some time depending upon your internet speed.
|-
|| [Terminal]

Point to the installation complete message
|| The installation is done now.
|-
|| Only Narration
|| Let’s now configure the system to use the installed '''OpenFOAM package'''.

Let me clear the screen.
|-
|| [Terminal]

gedit ~/.bashrc
|| Open the '''.bashrc''' file located in the '''Home''' directory in a '''text editor'''.

To do so, type the following '''command'''.

I will be using the '''gedit text editor'''.

You may use any '''text editor''' of your choice.
|-
|| [Text Editor]

source /opt/openfoam7/etc/bashrc
|| Scroll down to the end of the document.

Add the following line of '''code''' as shown.

This will enable us to execute the '''OpenFOAM commands''' via '''terminal'''.
|-
|| [Text Editor]

Ctrl + S and close the window
|| Save and close the file.
|-
|| Highlight new Terminal on the machine
|| Since the changes to '''.bashrc''' file is yet to be registered, we need to open a new '''terminal'''.

To open a '''new terminal''', press '''Ctrl, Alt and T''' keys together.
|-
|| [Terminal]

simpleFoam -help
|| In the new '''terminal''', type the following '''command'''.
|-
|| [Terminal]

‘Usage’ message
|| A message with the list of options is displayed on the '''terminal'''.

This confirms that '''OpenFOAM 7''' is properly installed.
|-
|| Only Narration
|| Let me clear the screen.
|-
|| Only Narration
|| Let us now check the installation of '''ParaView'''.
|-
|| [Terminal]

paraview
|| Type '''paraview''' in the '''terminal'''.
|-
|| Highlight '''ParaView '''window
|| The '''ParaView''' interface opens in a new window.

Close the start-up screen.

This confirms that '''ParaView''' is properly installed.
|-
|| [ParaView]

Click on close
|| '''Close''' this window.
|-
|| Only Narration
|| The installation of '''OpenFOAM 7''' is now complete.

We can access '''OpenFOAM''' '''commands''' from the '''terminal '''now.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

Let’s summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt how to:
* Install '''OpenFOAM''' version 7
* Install '''ParaView''' version 5.6.0 and
* Verify the installation
|-
|| 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
||
* Do you have questions in THIS Spoken Tutorial?
* Please visit this site.
* Choose the minute and second where you have the question
* Explain your question briefly
* Someone from our team will answer them
* You will have to register on this website to ask questions.

|-
|| 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley.

And this is Padmini from IIT Bombay signing off.

Thanks for joining.
|-
|-
|}

OpenFOAM-version-7/C2/Setting-up-a-Test-Case-in-OpenFOAM/English

2020-07-20T15:18:35Z

Ashleymelvin: Created page with "'''Title of the script''': Setting-up a test case in OpenFOAM '''Author''': Ashley Melvin '''Keywords''': OpenFOAM, ParaView, lid driven cavity, pre-processing, blockMesh, c..."

'''Title of the script''': Setting-up a test case in OpenFOAM

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM, ParaView, lid driven cavity, pre-processing, blockMesh, controlDict, post-processing, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Setting up a test case in OpenFOAM'''.
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn to:
* Set up a '''case''' in '''OpenFOAM'''
* Access the '''case files''' using '''terminal'''
* '''Pre-process''' a '''case'''
* '''Run''' a '''case''', and
* '''Post-process''' a '''case'''
|-
|| Slide: System Specifications
|| This tutorial is recorded using,
* '''Ubuntu Linux''' OS version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0, and
* '''gedit''' Text editor
However, you may use any other '''text editor''' of your choice.
|-
|| Slide: Prerequisites
* If not, please go through the prerequisite '''Linux '''tutorials on https://spoken-tutorial.org
|| As a prerequisite:
* You should be familiar with basic '''Linux commands'''.
* If not, please go through the prerequisite '''Linux '''tutorials on this website.
|-
|| Slide: Lid Driven Cavity
|| In this tutorial, we will learn to set up the '''lid driven cavity case'''.

'''Lid driven cavity''' is one of the most widely used '''2D test cases''' for the validation of a '''CFD '''code.
|-
|| Slide: Diagram
|| This is the diagram of '''Lid Driven Cavity Flow'''.

It consists of 3 fixed walls and a moving top wall.
|-
|| Highlight '''Terminal''' on the machine
|| Open a '''terminal''' by pressing the '''Ctrl, Alt '''and''' T''' keys together.
|-
|| Only Narration
|| Here onwards please remember to press the '''Enter''' key after typing each '''command'''.
|-
|| [Terminal] Type:
'''mkdir -p $FOAM_RUN'''
|| Now, let’s create a '''run directory'''.

To do so, type the '''command''' as shown.
|-
|| [Terminal] Highlight

'''FOAM_RUN'''
|| '''Tutorial cases''' will later be copied into the '''run directory'''.
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| Go to the '''run directory''' using the '''cd command'''.

Now our '''present working directory''' is the '''run directory'''.
|-
|| Only Narration
|| '''OpenFOAM''' installation comes with a set of '''test cases'''.

The '''tutorial directory''' contains these '''test cases'''.

The '''Lid driven cavity case''' already exists inside the '''tutorial directory'''.
|-
|| [Terminal] Type:

'''cp -r $FOAM_TUTORIALS/incompressible/icoFoam/cavity/cavity .'''
|| We’ll now copy the '''Lid driven cavity case''' from the '''tutorial directory''' into the '''run directory'''.

To do so, type the following '''command'''.
|-
|| Slide: blockMesh
||
* The '''mesh generator''' for '''OpenFOAM''' is a utility called '''blockMesh'''.
* The '''input dictionary''' for '''blockMesh''' utility is '''blockMeshDict'''.
|-
|| [Terminal] Type:

'''gedit cavity/system/blockMeshDict'''
|| The '''blockMeshDict''' file is located in the '''system''' folder.

Open the '''blockMeshDict''' file in a '''text editor'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight

vertices, blocks, edges and boundary
|| Now let’s look at the contents of the file.

The '''blockMeshDict''' contains details of the geometry like vertices, blocks, edges and boundaries.
|-
|| [gedit - '''blockMeshDict'''] Close the window
|| Close the '''blockMeshDict''' file.
|-
|| [Terminal] Type:

'''cd cavity/0'''
|| The '''0''' folder contains the initial and boundary conditions for the '''simulation'''.

Type the following '''command''' to move into the '''0''' folder inside the '''cavity case directory'''.
|-
|| [Terminal] Type:

'''ls'''
|| Type '''ls''' and press '''Enter''' to view the files in the '''0''' folder.
|-
|| [Terminal] Highlight

'''p''' and '''U'''
|| The '''0''' folder contains the '''kinematic pressure file p''' and the '''velocity file U'''.
|-
|| [Terminal] Type:

'''gedit p'''
|| Open the '''kinematic pressure file p''' in a '''text editor'''.
|-
|| Only Narration
|| The '''p''' file contains the '''initial''' and '''boundary''' conditions of '''kinematic''' pressure.
|-
|| [gedit - '''p'''] Highlight

'''dimensions [0 2 -2 0 0 0 0] '''
|| The '''dimensions''' of '''kinematic pressure''' is meter squared per second squared.
|-
|| [gedit - '''p'''] Highlight

'''internalField '''
|| The '''internalField''' defines the values in the interior of the domain.
|-
|| [gedit - '''p'''] Highlight

'''uniform 0'''
|| The initial field is set as '''0 kinematic pressure'''.

This field is '''uniform''' across the domain.
|-
|| [gedit - '''p'''] Highlight

Both the '''zeroGradient'''
|| You can see that all walls are imposed with a '''zero gradient''' pressure boundary condition.
|-
|| [gedit - '''p'''] Close the window
|| Let us close the '''p''' file.
|-
|| [Terminal] Type:

'''gedit U'''
|| Now open the '''velocity file U''' in a '''text editor'''.
|-
|| Only Narration
|| The '''U file''' contains the initial and boundary conditions of '''velocity'''.
|-
|| [gedit - '''U'''] Highlight

'''uniform (1 0 0);'''
|| You can see that the '''moving wall''' is imposed with a '''velocity''' of '''1 m/s''' in the x direction.
|-
|| [gedit - '''U'''] Highlight

'''noSlip '''
|| Also notice that the '''no-slip''' condition is imposed on the three '''fixed walls'''.
|-
|| [gedit - '''U'''] Close the window
|| Now let us close the '''U''' file.
|-
|| [Terminal] Type:

'''cd ..'''
|| We’ll go back to the '''cavity''' folder.

Type '''cd (space)(dot)(dot)'''
|-
|| [Terminal] Type:

'''gedit constant/transportProperties'''
|| Next, we will view the '''transport properties file '''which is in the '''constant '''folder.
|-
|| [gedit - '''transportProperties'''] Highlight

'''nu '''
|| The '''transportProperties''' file contains the details of '''kinematic''' '''viscosity'''.
|-
|| [gedit - '''transportProperties''']

Highlight '''[0 2 -1 0 0 0 0] '''
|| The dimensions of '''kinematic viscosity''' is meter squared per second.
|-
|| Slide: Kinematic Viscosity
||
* The '''kinematic viscosity''' is defined by:
𝜈 = |U|𝑑 / 𝑅𝑒
where '''velocity''' (|U|) = '''1 m/s'''
characteristic length (d) = '''0.1 m'''
* The '''Reynolds number (Re)''' for the '''flow''' is taken as '''10'''
* The '''kinematic viscosity (𝜈) '''is therefore '''0.01 m2/s'''
|-
|| Narration Only
|| Let me switch back to '''transportProperties''' file.
|-
|| [gedit - '''transportProperties''']

Highlight '''0.01'''
|| The value of '''kinematic''' '''viscosity''' is indicated in the '''transportProperties''' file.
|-
|| [gedit - '''transportProperties'''] Close the window
|| Close the '''transportProperties''' file.
|-
|| [Terminal] Type:

'''cd system'''
|| To move into the '''system''' folder, type the following '''command'''.
|-
|| [Terminal] Type:

'''ls'''
|| Type '''ls''' to view the contents of the '''system''' folder.
|-
|| [Terminal] Highlight

'''blockMeshDict controlDict fvSchemes fvSolution'''
|| The '''system''' folder contains the following files:

'''blockMeshDict''', '''controlDict''', '''fvSchemes''' and '''fvSolution'''.
|-
|| [Terminal] Highlight

'''fvSchemes'''
|| The '''fvSchemes dictionary''' contains the '''finite''' '''volume''' '''discretisation''' '''schemes'''.
|-
|| [Terminal] Highlight

'''fvSolution'''
|| The '''fvSolution dictionary''' contains the '''linear''' '''equation''' '''solvers''' and '''tolerances'''.

It contains other '''algorithm controls''' as well.
|-
|| [Terminal] Highlight

'''controlDict'''
|| The '''controlDict dictionary''' contains the '''simulation''' '''control''' '''parameters'''.

The '''dictionary''' input includes the '''control''' '''of time''' and '''reading''' and '''writing''' of the '''solution''' '''data'''.
|-
|| [Terminal] Type:

'''gedit controlDict'''
|| Let’s now open the '''controlDict''' file in a '''text editor'''.
|-
|| [Terminal] Highlight

'''startFrom '''and '''startTime'''
|| The '''start '''and''' stop times''' and the '''time step''' for the '''run''' must be set.
|-
|| [gedit - '''controlDict'''] Highlight

'''startTime''' '''0;'''
|| The '''start time''' is set at '''0''' seconds.
|-
|| [gedit - '''controlDict'''] Highlight

'''stopAt''' '''endTime;'''
|| The time at which the '''simulation''' stops is specified using the '''keyword stopAt'''.

Here, '''stopAt''' is specified using the keyword '''endTime'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''endTime''' '''0.5;'''
|| The '''endTime''' is set at '''0.5''' seconds.

This means that '''simulation''' stops after '''0.5''' seconds.
|-
|| [gedit - '''controlDict'''] Highlight

'''deltaT 0.005;'''
|| The value of the '''keyword deltaT''' defines the '''time step''' for the '''simulation'''.

The '''time step''' for the current '''simulation''' is set as '''0.005''' seconds.

'''Temporal accuracy''' and '''numerical stability''' is essential while running the '''simulation'''.

To achieve this, a''' Courant number''' of less than 1 is required.

Keeping this in mind, the '''time step''' is set to '''0.005''' seconds.
|-
|-
|-
|| [gedit - '''controlDict'''] Highlight

'''application''' '''icoFoam'''<nowiki>;</nowiki>
|| '''icoFoam''' is the '''OpenFOAM solver''' used to '''simulate''' the '''lid driven cavity''' '''flow'''.
|-
|| [gedit - '''controlDict'''] Close the window
|| Close the '''controlDict''' file.
|-
|| [Terminal] Type:

'''cd ..'''
|| Go back to the '''cavity''' folder using '''cd command'''.
|-
|| [Terminal] Type:

'''blockMesh''' >> '''Enter'''
|| Type the '''command blockMesh''' and press '''Enter''' to '''mesh''' the '''geometry'''.

The '''command''' takes input from the '''blockMeshDict dictionary''' and creates the '''geometry''' and '''meshes''' it.
|-
|| [Terminal] Highlight '''End'''
|| The '''meshing''' is now complete.
|-
|| [Terminal] Type:

'''icoFoam'''
|| The '''lid driven cavity flow''' is an '''incompressible flow'''.

It is solved using the''' OpenFOAM solver icoFoam.'''

To start the '''simulation''', type '''icoFoam''' in the '''terminal.'''
|-
|| [Terminal] Highlight '''End'''
|| The iterations are now complete.
|-
|| [Terminal] Type:

'''paraFoam'''
|| Let us view the '''simulated''' results in '''ParaView'''.

So, type '''paraFoam''' in the '''terminal.'''
|-
|| [ParaView] '''Properties''' Tab

Click on '''Apply'''
|| In the '''ParaView''' window, go to the '''Properties''' tab on the left.

Then click on the green coloured '''Apply '''button'''.'''
|-
|| [ParaView]

Click on '''vtkBlockColors''' >> Click on '''U'''
|| Go to the '''Active Variable Controls '''at the top.

Click on the '''vtkBlockColors''' dropdown and select '''U'''.

Ensure that you click on the '''U''' option with a '''point icon''' and not the '''box icon''', in the dropdown.

The '''box icon''' would display '''contours''' without any grading.
|-
|| [ParaView]

Velocity Contours in the Layout
|| The '''velocity''' '''contour''' at the start of the '''simulation''' is now displayed in the''' layout'''.
|-
|| [ParaView]

Go to '''VCR Controls''' and click on the '''Play''' Button
|| Let us see how the '''velocity contours''' develop through the '''simulation'''.

To do so, go to the '''VCR Controls''' and click on the '''Play''' button.
|-
|| [ParaView]

Final Velocity Contours in the Layout
|| The '''velocity contour''' at the end of the '''simulation''' is now displayed in the''' layout'''.
|-
|| [ParaView] Close the Window
|| Close the '''ParaView''' window.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

To summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt to:
* Set up a''' case''' in '''OpenFOAM'''
* Access the '''case files''' using '''terminal'''
* '''Pre-process''' a '''case'''
* '''Run''' a '''case''', and
* '''Post-process''' a '''case'''
|-
|| 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 this 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley Melvin.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Installing-OpenFOAM-in-Ubuntu-Linux/English

2020-07-20T13:32:09Z

Ashleymelvin:

'''Title of the script''': Installing OpenFOAM in Ubuntu

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM, ParaView, Linux, Ubuntu 18.04, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Installing OpenFOAM in Ubuntu Linux OS'''.
|-
|| Slide: Learning Objective

|| In this tutorial, we will learn how to install:
* '''OpenFOAM''' version 7 and
* '''ParaView''' version 5.6.0
|-
|| Slide: System Specifications
|| This tutorial is recorded using:
* '''Ubuntu Linux''' OS version 18.04
* A working '''Internet''' connection and
* A '''text editor'''
|-
|| Only Narration
|| We will install '''OpenFOAM''' using the '''terminal'''.
|-
|| Highlight '''Terminal''' on the machine
|| Open a '''terminal''' by pressing '''Ctrl, Alt and T''' keys together.

Make sure that you are connected to the '''Internet'''.
|-
|| [Terminal]

sudo sh -c "wget -O - http://dl.openfoam.org/gpg.key | apt-key add -"
|| A public key needs to be added to the '''repository'''.

This key enables the '''repository''' to verify '''OpenFOAM package signatures.'''

To do this, in the '''Terminal''', carefully type the following '''command''' and press '''Enter'''.
|-
|| [Terminal]

Type the password >> Press Enter.
|| The machine will ask for the '''system password'''.

Type the '''password''' and press '''Enter'''.
|-
|| Only Narration
|| Let me clear the screen.
|-
|| [Terminal]

sudo add-apt-repository http://dl.openfoam.org/ubuntu
|| Now type the following '''command''' and press '''Enter'''.

This will enable '''apt''' to search for '''dl.openfoam.org''' in the list of '''software repositories'''.
|-
|| Only Narration
|| Here onwards, please remember to press the '''Enter''' key after typing each '''command'''.
|-
|| [Terminal]

sudo apt-get update
|| Now type the following '''command''' to update the '''apt package''' list.
|-
|| [Terminal]

sudo apt-get -y install openfoam7
|| The '''repository''' is updated.

Next let us install '''OpenFOAM '''version 7.

To do so, type the following '''command''' in the '''terminal'''.
|-
|| [Terminal]

Point to the installation process
|| The installation may take some time depending upon your internet speed.
|-
|| [Terminal]

Point to the installation complete message
|| The installation is done now.
|-
|| Only Narration
|| Let’s now configure the system to use the installed '''OpenFOAM package'''.

Let me clear the screen.
|-
|| [Terminal]

gedit ~/.bashrc
|| Open the '''.bashrc''' file located in the '''Home''' directory in a '''text editor'''.

To do so, type the following '''command'''.

I will be using the '''gedit text editor'''.

You may use any '''text editor''' of your choice.
|-
|| [Text Editor]

source /opt/openfoam7/etc/bashrc
|| Scroll down to the end of the document.

Add the following line of '''code''' as shown.

This will enable us to execute the '''OpenFOAM commands''' via '''terminal'''.
|-
|| [Text Editor]

Ctrl + S and close the window
|| Save and close the file.
|-
|| Highlight new Terminal on the machine
|| Since the changes to '''.bashrc''' file is yet to be registered, we need to open a new '''terminal'''.

To open a '''new terminal''', press '''Ctrl, Alt and T''' keys together.
|-
|| [Terminal]

simpleFoam -help
|| In the new '''terminal''', type the following '''command'''.
|-
|| [Terminal]

‘Usage’ message
|| A message with the list of options is displayed on the '''terminal'''.

This confirms that '''OpenFOAM 7''' is properly installed.
|-
|| Only Narration
|| Let me clear the screen.
|-
|| Only Narration
|| Let us now check the installation of '''ParaView'''.
|-
|| [Terminal]

paraview
|| Type '''paraview''' in the '''terminal'''.
|-
|| Highlight '''ParaView '''window
|| The '''ParaView''' interface opens in a new window.

Close the start-up screen.

This confirms that '''ParaView''' is properly installed.
|-
|| [ParaView]

Click on close
|| '''Close''' this window.
|-
|| Only Narration
|| The installation of '''OpenFOAM 7''' is now complete.

We can access '''OpenFOAM''' '''commands''' from the '''terminal '''now.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

Let’s summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt how to:
* Install '''OpenFOAM''' version 7
* Install '''ParaView''' version 5.6.0 and
* Verify the installation
|-
|| 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
||
* Do you have questions in THIS Spoken Tutorial?
* Please visit this site.
* Choose the minute and second where you have the question
* Explain your question briefly
* Someone from our team will answer them
* You will have to register on this website to ask questions.

|-
|| 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley.

And this is Padmini from IIT Bombay signing off.

Thanks for joining.
|-
|-
|}

OpenFOAM-version-7/C2/Installing-OpenFOAM-in-Ubuntu-Linux/English

2020-07-20T13:30:35Z

Ashleymelvin:

'''Title of the script''': Installing OpenFOAM in Ubuntu

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM, ParaView, Linux, Ubuntu 18.04, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Installing OpenFOAM in Ubuntu Linux OS'''.
|-
|| Slide: Learning Objective

|| In this tutorial, we will learn how to install:
* '''OpenFOAM''' version 7 and
* '''ParaView''' version 5.6.0
|-
|| Slide: System Specifications
|| This tutorial is recorded using:
* '''Ubuntu Linux''' OS version 18.04
* A working '''Internet''' connection and
* A '''text editor'''
|-
|| Only Narration
|| We will install '''OpenFOAM''' using the '''terminal'''.
|-
|| Highlight '''Terminal''' on the machine
|| Open a '''terminal''' by pressing '''Ctrl, Alt and T''' keys together.

Make sure that you are connected to the '''Internet'''.
|-
|| [Terminal]

sudo sh -c "wget -O - http://dl.openfoam.org/gpg.key | apt-key add -"
|| A public key needs to be added to the '''repository'''.

This key enables the '''repository''' to verify '''OpenFOAM package signatures.'''

To do this, in the '''Terminal''', carefully type the following '''command''' and press '''Enter'''.
|-
|| [Terminal]

Type the password >> Press Enter.
|| The machine will ask for the '''system password'''.

Type the '''password''' and press '''Enter'''.
|-
|| Only Narration
|| Let me clear the screen.
|-
|| [Terminal]

sudo add-apt-repository http://dl.openfoam.org/ubuntu
|| Now type the following '''command''' and press '''Enter'''.

This will enable '''apt''' to search for '''dl.openfoam.org''' in the list of '''software repositories'''.
|-
|| Only Narration
|| Here onwards, please remember to press the '''Enter''' key after typing each '''command'''.
|-
|| [Terminal]

sudo apt-get update
|| Now type the following '''command''' to update the '''apt package''' list.
|-
|| [Terminal]

sudo apt-get -y install openfoam7
|| The '''repository''' is updated.

Next let us install '''OpenFOAM '''version 7.

To do so, type the following '''command''' in the '''terminal'''.
|-
|| [Terminal]

Point to the installation process
|| The installation may take some time depending upon your internet speed.
|-
|| [Terminal]

Point to the installation complete message
|| The installation is done now.
|-
|| Only Narration
|| Let’s now configure the system to use the installed '''OpenFOAM package'''.

Let me clear the screen.
|-
|| [Terminal]

gedit ~/.bashrc
|| Open the '''.bashrc''' file located in the '''Home''' directory in a '''text editor'''.

To do so, type the following '''command'''.

I will be using the '''gedit text editor'''.

You may use any '''text editor''' of your choice.
|-
|| [Text Editor]

source /opt/openfoam7/etc/bashrc
|| Scroll down to the end of the document.

Add the following line of '''code''' as shown.

This will enable us to execute the '''OpenFOAM commands''' via '''terminal'''.
|-
|| [Text Editor]

Ctrl + S and close the window
|| Save and close the file.
|-
|| Highlight new Terminal on the machine
|| Since the changes to '''.bashrc''' file is yet to be registered, we need to open a new '''terminal'''.

To open a '''new terminal''', press '''Ctrl, Alt and T''' keys together.
|-
|| [Terminal]

simpleFoam -help
|| In the new '''terminal''', type the following '''command'''.
|-
|| [Terminal]

‘Usage’ message
|| A message with the list of options is displayed on the '''terminal'''.

This confirms that '''OpenFOAM 7''' is properly installed.
|-
|| Only Narration
|| Let me clear the screen.
|-
|| Only Narration
|| Let us now check the installation of '''ParaView'''.
|-
|| [Terminal]

paraview
|| Type '''paraview''' in the '''terminal'''.
|-
|| Highlight '''ParaView '''window
|| The '''ParaView''' interface opens in a new window.

Close the start-up screen.

This confirms that '''ParaView''' is properly installed.
|-
|| [ParaView]

Click on close
|| '''Close''' this window.
|-
|| Only narration
|| The installation of '''OpenFOAM 7''' is now complete.

We can access '''OpenFOAM''' '''commands''' from the '''terminal '''now.
|-
|| Only narration
|| With this we have come to the end of the tutorial.

Let’s summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt how to:
* Install '''OpenFOAM''' version 7
* Install '''ParaView''' version 5.6.0 and
* Verify the installation
|-
|| 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
||
* Do you have questions in THIS Spoken Tutorial?
* Please visit this site.
* Choose the minute and second where you have the question
* Explain your question briefly
* Someone from our team will answer them
* You will have to register on this website to ask questions.

|-
|| 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley.

And this is Padmini from IIT Bombay signing off.

Thanks for joining.
|-
|-
|}

OpenFOAM-version-7/C2/Installing-OpenFOAM-in-Ubuntu-Linux/English

2020-07-20T12:52:05Z

Ashleymelvin: Created page with "'''Title of the script''': Installing OpenFOAM in Ubuntu '''Author''': Ashley Melvin '''Keywords''': OpenFOAM, ParaView, Linux, Ubuntu 18.04, video tutorial {| border = "..."

'''Title of the script''': Installing OpenFOAM in Ubuntu

'''Author''': Ashley Melvin

'''Keywords''': OpenFOAM, ParaView, Linux, Ubuntu 18.04, video tutorial

{| border = "1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Installing OpenFOAM in Ubuntu Linux OS'''.
|-
|| Slide: Learning Objective

|| In this tutorial, we will learn how to install:
* '''OpenFOAM''' version 7 and
* '''ParaView''' version 5.6.0
|-
|| Slide: System Specifications
|| This tutorial is recorded using:
* '''Ubuntu Linux''' OS version 18.04
* A working '''Internet''' connection and
* A '''text editor'''
|-
|| Only Narration
|| We will install '''OpenFOAM''' using the '''terminal'''.
|-
|| Highlight '''Terminal''' on the machine
|| Open a '''terminal''' by pressing '''Ctrl, Alt and T''' keys together.

Make sure that you are connected to the '''Internet'''.
|-
|| [Terminal]

sudo sh -c "wget -O - http://dl.openfoam.org/gpg.key | apt-key add -"
|| A public key needs to be added to the '''repository'''.

This key enables the '''repository''' to verify '''OpenFOAM package signatures.'''

To do this, in the '''Terminal''', carefully type the following '''command''' and press '''Enter'''.
|-
|| [Terminal]

Type the password >> Press Enter.
|| The machine will ask for the '''system password'''.

Type the '''password''' and press '''Enter'''.
|-
|| Only Narration
|| Let me clear the screen.
|-
|| [Terminal]

sudo add-apt-repository http://dl.openfoam.org/ubuntu
|| Now type the following '''command''' and press '''Enter'''.

This will enable '''apt''' to search for '''dl.openfoam.org''' in the list of '''software repositories'''.
|-
|| Only Narration
|| Here onwards, please remember to press the '''Enter''' key after typing each '''command'''.
|-
|| [Terminal]

sudo apt-get update
|| Now type the following '''command''' to update the '''apt package''' list.
|-
|| [Terminal]

sudo apt-get -y install openfoam7
|| The '''repository''' is updated.

Next let us install '''OpenFOAM '''version 7.

To do so, type the following '''command''' in the '''terminal'''.
|-
|| [Terminal]

Point to the installation process
|| The installation may take some time depending upon your internet speed.
|-
|| [Terminal]

Point to the installation complete message
|| The installation is done now.
|-
|| Only Narration
|| Let’s now configure the system to use the installed '''OpenFOAM package'''.

Let me clear the screen.
|-
|| [Terminal]

gedit ~/.bashrc
|| Open the '''.bashrc''' file located in the '''Home''' directory in a '''text editor'''.

To do so, type the following '''command'''.

I will be using the '''gedit text editor'''.

You may use any '''text editor''' of your choice.
|-
|| [Text Editor]

source /opt/openfoam7/etc/bashrc
|| Scroll down to the end of the document.

Add the following line of '''code''' as shown.

This will enable us to execute the '''OpenFOAM commands''' via '''terminal'''.
|-
|| [Text Editor]

Ctrl + S and close the window
|| Save and close the file.
|-
|| Highlight new Terminal on the machine
|| Since the changes to '''.bashrc''' file is yet to be registered, we need to open a new '''terminal'''.

To open a '''new terminal''', press '''Ctrl, Alt and T''' keys together.
|-
|| [Terminal]

simpleFoam -help
|| In the new '''terminal''', type the following '''command'''.
|-
|| [Terminal]

‘Usage’ message
|| A message with the list of options is displayed on the '''terminal'''.

This confirms that '''OpenFOAM 7''' is properly installed.
|-
|| Only Narration
|| Let me clear the screen.
|-
|| Only Narration
|| Let us now check the installation of '''ParaView'''.
|-
|| [Terminal]

paraview
|| Type '''paraview''' in the '''terminal'''.
|-
|| Highlight '''ParaView '''window
|| The '''ParaView''' interface opens in a new window.

Close the start-up screen.

This confirms that '''ParaView''' is properly installed.
|-
|| [ParaView]

Click on close
|| '''Close''' this window.
|-
|| Only narration
|| The installation of '''OpenFOAM 7''' is now complete.

We can access '''OpenFOAM''' '''commands''' from the '''terminal '''now.
|-
|| Only narration
|| With this we have come to the end of the tutorial.

Let’s summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt how to:

* Install '''OpenFOAM''' version 7
* Install '''ParaView''' version 5.6.0 and
* Verify the installation
|-
|| 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
||
* Do you have questions in THIS Spoken Tutorial?
* Please visit this site.
* Choose the minute and second where you have the question
* Explain your question briefly
* Someone from our team will answer them
* You will have to register on this website to ask questions.

|-
|| 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: Spoken Tutorial
|| The Spoken Tutorial project is supported by MHRD, Govt. of India.

The script for this tutorial is contributed by Ashley.

And this is Padmini from IIT Bombay signing off.

Thanks for joining.
|-
|-
|}