Script | Spoken-Tutorial - User contributions [en]

OpenFOAM-version-7/C2/Turbulence-Modelling-in-OpenFOAM/English

2020-08-07T13:07:44Z

Divyesh7:

'''Title of the script:''' Turbulence Modelling in OpenFOAM

'''Author:''' Padmini Priyadarshini

'''Keywords:''' OpenFOAM, Turbulence, YPlus, K-Omega, K-OmegaSST, Paraview, Video-Tutorial

{| border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Turbulence Modelling in OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn how to,
* Set up the '''blockMeshDict''' dictionary for a given '''YPlus''' value
* Implement '''k-omega''' and '''k-omega SST''' '''turbulence models'''
* '''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
|| As a prerequisite:
* You should have basic knowledge of geometric progression
* You should be familiar with '''simulating''' a''' turbulent flow''' through a''' channel '''and
* You should also be familiar with '''Multi-block Meshing of 2D''' geometry
* 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 metres '''and width '''1 metre'''.

The '''kinematic viscosity''' is '''1e to the power of minus 5 metres per second.'''
The '''Inlet velocity '''is '''20 metres per second. '''
'''Outlet pressure '''is set to '''zero atmosphere.'''
|-
|| Slide: Flow Properties
|| '''Reynolds number''' is '''2 million'''.

The flow is '''turbulent.'''
|-
|| Only Narration
|| First, We will use''' k-epsilon turbulence model '''to '''simulate''' this '''case'''.

Let us set up the '''case.'''
|-
|| Only Narration
|| Download the '''kepsilon''' folder provided in the '''Code files''' link and extract it.
|-
|| 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''' in the '''terminal'''.
|-
|| [Terminal] Type: '''cd $FOAM_RUN '''
|| Open the '''Run directory '''by typing this '''command.'''
|-
|| [Terminal]
Type: '''cp -r ~/Downloads/kepsilon .'''
|| Copy the downloaded file into the '''Run directory'''.
To do that, type the following '''command.'''
|-
|| Only Narration
|| I have downloaded the file into the '''Downloads directory.'''

Please change the '''command''' according to the '''file path''' on your machine.
|-
|| [Terminal] Type: '''cd kepsilon'''
|| Navigate to the '''kepsilon directory.'''
|-
|| [Terminal] Type:
'''gedit system/blockMeshDict'''
|| Open the '''blockMeshDict '''file in a '''text editor.'''
|-
|| [gedit -blockMeshDict]
Highlight '''blocks'''
|| Scroll down to the '''keyword “blocks”.'''
|-
|| [gedit -'''blockMeshDict''']
Highlight '''hex .... (1 0.18 1);'''
|| The '''domain''' has two equal-sized '''blocks.'''
|-
|| [gedit -'''blockMeshDict''']
Highlight '''75''' '''30'''
|| For each '''block''', the '''cell''' number is set to '''75 '''in the '''x-direction''', and '''30''' in the '''y-direction.'''
|-
|| Slide: Wall distance, yp
|| Let “'''yp'''” be the distance between the '''wall''' and the nearest '''cell centre'''.

For our '''case, yp''' is '''0.0031''' for '''YPlus''' value of '''200'''.

For''' channel flow''', the '''skin friction coefficient, Cf,''' is given by this formula.
|-
|| Slide: Cell width
|| The width of the''' cell '''near the '''wall''' is '''0.0062.'''
|-
|| Slide: Expansion ratio
|| The '''expansion ratio''' is the ratio of the last '''cell''' width to the first '''cell''' width.
|-
|| Slide: Expansion ratio calculation
|| It is calculated using geometric progression formula.

Please refer to the '''Additional Reading Material''' for more details.
|-
|| Slide: Expansion ratio value
|| The '''expansion ratio''' in the '''+y direction''' is found to be
* '''5.57 '''for '''block 1,''' and
* '''0.18 '''for''' block 2'''
* for a '''block''' of width of '''0.5 m''' and '''cell''' number 30.

Please refer to the '''Additional Reading Material''' on this tutorial page for details.
|-
|| Only Narration
|| I have already put these values into the '''blockMeshDict''' file.
|-
|| [gedit -blockMeshDict]
Highlight''' simpleGrading'''
|| '''simpleGrading''' describes the uniform '''expansion ratio '''in '''x, y''', and''' z-directions.'''
|-
|| Only Narration
|| For our '''case''', the''' expansion ratio''' in the '''y-direction''' is
|-
|| [gedit -'''blockMeshDict''']
Highlight '''5.57'''
|| '''5.57 '''for '''block 1'''
|-
|| [gedit -'''blockMeshDict''']

Highlight''' 0.18'''
|| '''0.18''' for '''block 2'''
|-
|| [gedit - '''blockMeshDict'''] Close Text Editor
|| Close the '''blockMeshDict''' file.
|-
|| Only Narration
|| The '''case''' is now ready to be''' run. '''
|-
|| [Terminal] Type: '''blockMesh'''
|| On the '''terminal''', type '''blockMesh''' to '''mesh''' the geometry.
|-
|| [Terminal] Type:
'''simpleFoam'''
|| Then type '''simpleFoam''' in the '''terminal '''to '''run '''the '''simulation'''.
|-
|| Only Narration
|| The '''simulation '''will take some time depending on your computer’s '''hardware'''.
|-
|| [Terminal] Highlight''' End'''
|| The''' simulation''' is complete.
|-
|| Only Narration
|| Let's check the final value of '''YPlus.'''
|-
|| [Terminal] Type:
'''simpleFoam -postProcess -func "yPlus" -latestTime'''
|| Now type the following '''command''' on the '''terminal''' to get the '''YPlus '''value on the '''walls.'''
|-
|| [Terminal]
Highlight''' Patch to 214.786'''
|| We can see that the '''YPlus''' value stays below 300.
|-
|| [Terminal] Type: '''cd ..'''
|| Let us go back to the '''Run directory''' using the '''cd command'''.
|-
|| Only Narration
|| Let us '''simulate''' the same problem using the '''k-omega turbulence model''' now.
|-
|| Slide: K-Omega turbulence model
|| '''k-omega '''is a '''two-equation model'''.
It solves-
* The '''turbulent kinetic energy transport equation''', and
* The '''specific turbulent dissipation rate transport equation'''
|-
|| Slide: Inlet Boundary Condition - omega
|| Let's look at the '''boundary''' and '''initial conditions''' for '''omega.'''

We will use '''turbulentMixingLengthFrequencyInlet'''

It calculates '''omega''' using '''kappa''' and user-specified '''mixing length. '''

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

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

Here, the value of '''turbulent length scale''' is '''0.07 metres'''

The '''specific turbulent dissipation rate '''value is '''16.67 second inverse'''

Where''' empirical constant, cmu '''is equal to '''0.09'''
|-
|| Slide: Wall & Outlet Boundary Condition - omega
|| '''Wall boundary condition''' is set to '''omegaWallFunction.'''

'''zeroGradient boundary condition''' is imposed at the '''outlet. '''

Please refer to the '''Additional Reading Material''' on this tutorial page for details.
|-
|| Only Narration
|| Download the '''komega '''folder provided in the '''Code files''' link and extract it.
|-
|| [Terminal] Type:
'''cp -r ~/Downloads/komega .'''
|| Copy the downloaded file into '''Run directory.'''

To do that, type the following '''command''' in the '''terminal.'''
|-
|| [Terminal] Type:
'''cd komega'''
|| Navigate to the '''komega''' directory using the '''cd command.'''
|-
|| Only Narration
|| Let’s take a look at the '''specific turbulent dissipation rate '''file.
|-
|| [Terminal] Type: '''gedit 0/omega'''
|| Open the '''omega''' file in a '''text editor.'''
|-
|| [gedit -'''omega''']
Highlight '''internalField ... 16.67;'''
|| The '''internalField''' value is initialised as '''16.67'''
|-
|| [gedit -'''omega''']
Highlight''' type turbulentMixingLengthFrequencyInlet'''
|| The '''inlet boundary type''' is set to '''turbulentMixingLengthFrequencyInlet'''
|-
|| [gedit -'''omega''']
Highlight''' mixingLength 0.07;'''
|| The '''keyword mixingLength '''represents the '''Turbulent length scale''', and is set to '''0.07'''
|-
|| [gedit -'''omega''']
Highlight''' value $internalField;'''
|| We have passed the '''internalField''' value to the '''patch field '''value.
|-
|| [gedit -'''omega'''] Highlight '''zeroGradient'''
|| The '''outlet patch type''' is set to '''zeroGradient.'''
|-
|| [gedit -'''omega''']
Highlight '''omegaWallFunction'''
|| The '''wall patch type''' is set to '''omegaWallFunction.'''
|-
|| [gedit -'''omega'''] Close Text Editor
|| Close the '''omega''' file.
|-
|| [Terminal] Type:
'''gedit constant/turbulenceProperties'''
|| Open the '''turbulenceProperties''' file in a '''text editor.'''
|-
|| [gedit -'''turbulenceProperties''']
Highlight''' kOmega'''
|| '''kOmega '''is selected as the '''RASModel.'''

Note,''' O '''is capitalized here.
|-
|| [gedit -'''turbulenceProperties''']
Highlight''' on'''
|| Ensure the '''keyword turbulence''' is set to '''On'''.
|-
|| [gedit -'''turbulenceProperties''']
Close Text Editor
|| Close the '''turbulenceProperties '''file.
|-
|| Only Narration
|| The '''case''' is now ready to be '''run.'''
|-
|| [Terminal] Type: '''blockMesh'''
|| On the '''terminal''', type '''blockMesh '''to '''mesh '''the geometry.
|-
|| [Terminal] Type: '''simpleFoam'''
|| Now, type the following '''command''' to '''run''' the '''case.'''
|-
|| [Terminal] Highlight''' End'''
|| The''' simulation''' is over.
|-
|| [Terminal] Type: '''cd ..'''
|| Let us go back to the '''Run directory''' using the '''cd command.'''
|-
|| Only Narration
|| Now, let’s '''run''' the same '''case''' with the '''k-omegaSST turbulence model.'''
|-
|| Slide: K-omegaSST turbulence model
|| The''' K-omega SST turbulence model''' is a '''hybrid model'''.
In the '''near-wall '''region, '''K-omegaSST''' uses the '''K-omega turbulence model.'''

In the region away from the '''wall''', it switches to the '''K-epsilon turbulence model'''.

Please refer to the '''Additional Reading Material''' on this tutorial page for details.
|-
|| Only Narration
|| Download the '''komegasst '''folder provided in the '''Code files''' link and extract it.
|-
|| [Terminal] Type:
'''cp -r ~/Downloads/komegasst .'''
|| Copy the downloaded file into the '''Run directory.'''

To do that, type the following '''command '''in the '''terminal.'''
|-
|| [Terminal] Type: '''cd komegasst'''
|| Navigate to the '''komegasst directory''' using the '''cd command.'''
|-
|| Only Narration
|| '''komega''' and '''komegasst models''' use the same''' turbulence variables'''.

Hence, the files in the '''zero''' directory are the same.
|-
|| [Terminal] Type:
'''gedit constant/turbulenceProperties'''
|| Open the '''turbulence properties''' file in a '''text editor.'''
|-
|| [gedit -'''turbulenceProperties''']
Highlight '''kOmegaSST'''
|| '''RASModel field''' entry is set to '''kOmegaSST.'''

Note,''' O''' and''' SST''' are capitalized here.
|-
|| [gedit -'''turbulenceProperties''']
Close Text Editor
|| Close the '''turbulenceProperties''' file.
|-
|| [Terminal] Type:
'''gedit system/fvSchemes'''
|| Open '''fvSchemes dictionary''' in a '''text editor.'''
|-
|| Only Narration
|| Scroll down to the end of the document.
|-
|| [gedit -'''fvSchemes''']
Highlight '''wallDist ... ;}'''
|| '''wallDist sub-dictionary''' is included in the '''fvSchemes dictionary'''.
|-
|| Only Narration
|| This enables the calculation of the distance between the '''cell centre''' and the nearest '''wall.'''
|-
|| [gedit -'''fvSchemes'''] Close Text Editor
|| Close the '''fvSchemes''' file.
|-
|| Only Narration
|| The setup is now ready.
Let us '''run''' the '''simulation.'''
|-
|| [Terminal] Type: '''blockMesh'''
|| '''Mesh''' the geometry using the '''blockMesh command '''on the '''terminal.'''
|-
|| [Terminal] Type: '''simpleFoam'''
|| Type '''simpleFoam''' in the '''terminal.'''
|-
|| [Terminal] Highlight''' End'''
|| The '''simulation''' is finished successfully.
|-
|| Show slide
Exit velocity profile - comparison
|| The slide shows the''' exit velocity profile''' for all three '''turbulence models'''
|-
|| 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,
* Set up the '''blockMeshDict''' file for a given '''YPlus''' value
* Implement '''k-omega '''and''' k-omega SST turbulence models'''
* '''Run''' the '''simulation'''
|-
|| Slide: Assignment
|| As an assignment:
* Repeat the '''simulation''' for a '''YPlus''' value of '''250 '''using '''k-epsilon''' '''model'''
* Repeat the''' simulation '''for a '''velocity''' of '''40 metres per second''' using '''k-omega''' and '''k-omega SST model'''
|-
|| 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 Sridhar from IIT Bombay signing off.
Thanks for joining.
|-
|}

OpenFOAM-version-7/C2/Turbulence-Modelling-in-OpenFOAM/English

2020-07-25T12:42:14Z

Divyesh7:

'''Title of the script:''' Turbulence Modelling in OpenFOAM

'''Author:''' Padmini Priyadarshini

'''Keywords:''' OpenFOAM, Turbulence, YPlus, K-Omega, K-OmegaSST, Paraview, Video-Tutorial

{| border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Turbulence Modelling in OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn how to,
* Set up the '''blockMeshDict''' dictionary for a given '''YPlus''' value
* Implement '''k-omega''' and '''k-omega SST''' '''turbulence models'''
* '''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
|| As a prerequisite:
* You should have basic knowledge of '''geometric progression'''
* You should be familiar with '''simulating''' a''' turbulent flow''' through a''' channel '''and
* You should also be familiar with '''Multi-block Meshing of 2D Geometry'''
* 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'''.
The flow is '''turbulent.'''
|-
|| Only Narration
|| First, We will use''' k-epsilon turbulence model '''to '''simulate''' this '''case'''.
Let us set up the '''case.'''
|-
|| Only Narration
|| Download the '''kepsilon''' folder provided in the '''code files''' link and extract it.
|-
|| 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''' in the '''terminal'''.
|-
|| [Terminal] Type: '''cd $FOAM_RUN '''
|| Open the '''Run directory '''by typing this '''command.'''
|-
|| [Terminal]
Type: '''cp -r ~/Downloads/kepsilon .'''
|| Copy the downloaded file into the '''Run directory'''.
To do that, type the following '''command.'''
|-
|| Only Narration
|| I have downloaded the file into the '''Downloads directory.'''
Please change the '''command''' according to the '''file path''' on your machine.
|-
|| [Terminal] Type: '''cd kepsilon'''
|| Navigate to the '''kepsilon directory.'''
|-
|| [Terminal] Type:
'''gedit system/blockMeshDict'''
|| Open the '''blockMeshDict '''file in a '''text editor.'''
|-
|| [gedit -blockMeshDict]
Highlight '''blocks'''
|| Scroll down to the '''keyword “blocks”.'''
|-
|| [gedit -'''blockMeshDict''']
Highlight '''hex .... (1 0.18 1);'''
|| The '''domain''' has two equal-sized '''blocks.'''
|-
|| [gedit -'''blockMeshDict''']
Highlight '''75''' '''30'''
|| For each '''block''', the '''cell number''' is set to '''75 '''in the '''x-direction''', and '''30''' in the '''y-direction.'''
|-
|| Slide: Wall distance, yp
|| Let “'''yp'''” be the distance between the '''wall''' and the nearest '''cell centre'''.
For our '''case, yp''' is '''0.0031''' for '''YPlus''' value of '''200'''.
For''' channel flow''', the '''skin friction coefficient, Cf,''' is given by this formula.
|-
|| Slide: Cell width
|| The width of the''' cell '''near the '''wall''' is '''0.0062.'''
|-
|| Slide: Expansion ratio
|| The '''expansion ratio''' is the ratio of the last '''cell width''' to the first '''cell width.'''
|-
|| Slide: Expansion ratio calculation
|| It is calculated using '''geometric progression''' formula.
Please refer to the '''Additional Reading Material''' for more details.
|-
|| Slide: Expansion ratio value
|| The '''expansion ratio''' in the '''+y direction''' is found to be
* '''5.57 '''for '''block 1,''' and
* '''0.18 '''for''' block 2'''
for a '''block''' of width of '''0.5 m''' and '''cell number 30.'''
Please refer to the '''Additional Reading Material''' on this tutorial page for details.
|-
|| Only Narration
|| I have already put these values into the '''blockMeshDict''' file.
|-
|| [gedit -blockMeshDict]
Highlight''' simpleGrading'''
|| '''simpleGrading''' describes the uniform '''expansion ratio '''in '''x, y''', and''' z-directions.'''
|-
|| Only Narration
|| For our '''case''', the''' expansion ratio''' in the '''y-direction''' is
|-
|| [gedit -'''blockMeshDict''']
Highlight '''5.57'''
|| '''5.57 '''for '''block 1'''
|-
|| [gedit -'''blockMeshDict''']

Highlight''' 0.18'''
|| '''0.18''' for '''block 2'''
|-
|| [gedit - '''blockMeshDict'''] Close Text Editor
|| Close the '''blockMeshDict''' file.
|-
|| Only Narration
|| The '''case''' is now ready to be''' run. '''
|-
|| [Terminal] Type: '''blockMesh'''
|| On the '''terminal''', type '''blockMesh''' to '''mesh''' the '''geometry'''.
|-
|| [Terminal] Type:
'''simpleFoam'''
|| Then type '''simpleFoam''' in the '''terminal '''to '''run '''the '''simulation'''.
|-
|| Only Narration
|| The '''simulation '''will take some '''time''' depending on your computer’s '''hardware'''.
|-
|| [Terminal] Highlight''' End'''
|| The''' simulation''' is complete.
|-
|| Only Narration
|| Let's check the final value of '''YPlus.'''
|-
|| [Terminal] Type:
'''simpleFoam -postProcess -func "yPlus" -latestTime'''
|| Now type the following '''command''' on the '''terminal''' to get the '''YPlus '''value on the '''walls.'''
|-
|| [Terminal]
Highlight''' Patch to 213.433'''
|| We can see that the '''YPlus''' value stays below 300.
|-
|| [Terminal] Type: '''cd ..'''
|| Let us go back to the '''Run directory''' using the '''cd command'''.
|-
|| Only Narration
|| Let us '''simulate''' the same problem using the k-omega''' turbulence model '''now'''.'''
|-
|| Slide: K-Omega turbulence model
|| '''k-omega '''is a '''two-equation model'''.
It solves-
* The '''turbulent kinetic energy''' '''transport equation''', and
* The '''specific''' '''turbulent dissipation rate transport equation'''
|-
|| Slide: Inlet Boundary Condition - omega
|| Let's look at the '''boundary''' and '''initial conditions''' for '''omega.'''
We will use '''turbulentMixingLengthFrequencyInlet'''
It calculates '''omega''' using '''kappa '''and
user-specified '''mixing length. '''
'''Mixing length '''refers to the''' turbulent length scale.'''
'''Kappa''' value is automatically put in by the '''solver.'''
Here''', '''the value of''' turbulent length scale''' is '''0.07 m'''
The '''specific''' '''turbulent dissipation rate '''value is '''16.67 1/s'''
Where''' empirical constant, cmu '''is equal to '''0.09'''
|-
|| Slide: Wall & Outlet Boundary Condition - omega
|| '''Wall boundary condition''' is set to '''omegaWallFunction.'''
'''zeroGradient boundary condition''' is imposed at the '''outlet. '''
Please refer to the '''Additional Reading Material''' on this tutorial page for details.
|-
|| Only Narration
|| Download the '''komega '''folder provided in the '''Code files''' link and extract it.
|-
|| [Terminal] Type:
'''cp -r ~/Downloads/komega .'''
|| Copy the downloaded file into '''Run directory.'''
To do that, type the following '''command '''in the '''terminal.'''
|-
|| [Terminal] Type:
'''cd komega'''
|| Navigate to the '''komega''' directory using the '''cd command.'''
|-
|| Only Narration
|| Let’s take a look at the '''specific''' '''turbulent dissipation rate '''file.
|-
|| [Terminal] Type: '''gedit 0/omega'''
|| Open the '''omega''' file in a '''text editor.'''
|-
|| [gedit -'''omega''']
Highlight '''internalField ... 16.67;'''
|| The '''internalField''' value is initialised as '''16.67'''
|-
|| [gedit -'''omega''']
Highlight''' type turbulentMixingLengthFrequencyInlet'''
|| The '''inlet '''boundary '''type''' is set to '''turbulentMixingLengthFrequencyInlet'''
|-
|| [gedit -'''omega''']
Highlight''' mixingLength 0.07;'''
|| The '''keyword''' '''mixingLength '''represents the '''Turbulent length scale''', and is set to '''0.07'''
|-
|| [gedit -'''omega''']
Highlight''' value $internalField;'''
|| We have passed the '''internalField''' value to the '''patch field '''value.
|-
|| [gedit -'''omega'''] Highlight '''zeroGradient'''
|| The '''outlet patch type''' is set to '''zeroGradient.'''
|-
|| [gedit -'''omega''']
Highlight '''omegaWallFunction'''
|| The '''wall patch type''' is set to '''omegaWallFunction.'''
|-
|| [gedit -'''omega'''] Close Text Editor
|| Close the '''omega''' file.
|-
|| [Terminal] Type:
'''gedit constant/turbulenceProperties'''
|| Open the '''turbulenceProperties''' file in a '''text editor.'''
|-
|| [gedit -'''turbulenceProperties''']
Highlight''' kOmega'''
|| '''kOmega '''is selected as the '''RASModel.'''
Note,''' O '''is capitalized here.
|-
|| [gedit -'''turbulenceProperties''']
Highlight''' on'''
|| Ensure the '''keyword''' '''turbulence''' is set to '''On'''.
|-
|| [gedit -'''turbulenceProperties''']
Close Text Editor
|| Close the '''turbulenceProperties '''file.
|-
|| Only Narration
|| The '''case''' is now ready to be '''run.'''
|-
|| [Terminal] Type: '''blockMesh'''
|| On the '''terminal''', type '''blockMesh '''to '''mesh '''the '''geometry.'''
|-
|| [Terminal] Type: '''simpleFoam'''
|| Now, type the following '''command''' to '''run''' the '''case.'''
|-
|| [Terminal] Highlight''' End'''
|| The''' simulation''' is over.
|-
|| [Terminal] Type: '''cd ..'''
|| Let us go back to the '''Run directory''' using the '''cd command.'''
|-
|| Only Narration
|| Now, let’s '''run''' the same '''case''' with the '''k-omegaSST''' '''turbulence model.'''
|-
|| Slide: K-omegaSST turbulence model
|| The''' K-omega SST turbulence model''' is a '''hybrid '''model.
In the '''near-wall '''region, '''K-omegaSST''' uses the '''K-omega turbulence model.'''

In the region away from the '''wall''', it switches to the '''K-epsilon''' '''turbulence model'''.

Please refer to the '''Additional Reading Material''' on this tutorial page for details.
|-
|| Only Narration
|| Download the '''komegasst '''folder provided in the '''Code files''' link and extract it.
|-
|| [Terminal] Type:
'''cp -r ~/Downloads/komegasst .'''
|| Copy the downloaded file into the '''Run directory.'''
To do that, type the following '''command '''in the '''terminal.'''
|-
|| [Terminal] Type: '''cd komegasst'''
|| Navigate to the '''komegasst '''directory using the '''cd command.'''
|-
|| Only Narration
|| '''komega''' and '''komegasst models''' use the same''' turbulence variables'''.
Hence, the files in the '''0''' directory are the same.
|-
|| [Terminal] Type:
'''gedit constant/turbulenceProperties'''
|| Open the '''turbulence''' properties file in a '''text editor.'''
|-
|| [gedit -'''turbulenceProperties''']
Highlight '''kOmegaSST'''
|| '''RASModel field''' entry is set to '''kOmegaSST.'''
Note,''' O''' and''' SST''' are capitalized here.
|-
|| [gedit -'''turbulenceProperties''']
Close Text Editor
|| Close the '''turbulenceProperties''' file.
|-
|| [Terminal] Type:
'''gedit system/fvSchemes'''
|| Open '''fvSchemes dictionary''' in a '''text editor.'''
|-
|| Only Narration
|| Scroll down to the end of the document.
|-
|| [gedit -'''fvSchemes''']
Highlight '''wallDist ... ;}'''
|| '''wallDist sub-dictionary''' is included in the '''fvSchemes dictionary'''.
|-
|| Only Narration
|| This enables the calculation of the '''distance '''between the '''cell centre''' and the nearest '''wall.'''
|-
|| [gedit -'''fvSchemes'''] Close Text Editor
|| Close the '''fvSchemes''' file.
|-
|| Only Narration
|| The setup is now ready.
Let us '''run''' the '''simulation.'''
|-
|| [Terminal] Type: '''blockMesh'''
|| '''Mesh''' the '''geometry''' using the '''blockMesh command '''on the '''terminal.'''
|-
|| [Terminal] Type: '''simpleFoam'''
|| Type '''simpleFoam''' in the '''terminal.'''
|-
|| [Terminal] Highlight''' End'''
|| The '''simulation''' is finished successfully.
|-
|| Show slide
Exit velocity profile - comparison
|| The slide shows the''' exit velocity''' '''profile''' for all three '''turbulence models'''
|-
|| 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,
* Set up the '''blockMeshDict''' file for a given '''YPlus''' value
* Implement '''k-omega '''and''' k-omega SST turbulence models'''
* '''Run''' the '''simulation'''
|-
|| Slide: Assignment
|| As an assignment:
* Repeat the '''simulation''' for a '''YPlus''' value of '''250 '''using '''k-epsilon''' '''model'''
* Repeat the''' simulation '''for a '''velocity''' of '''40 m/s''' using '''k-omega''' and '''k-omega SST model'''
|-
|| 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 Sridhar from IIT Bombay signing off.
Thanks for joining.
|-
|}

OpenFOAM-version-7/C2/Turbulence-Modelling-in-OpenFOAM/English

2020-07-25T12:40:21Z

Divyesh7:

'''Title of the script:''' Turbulence Modelling in OpenFOAM

'''Author:''' Padmini Priyadarshini

'''Keywords:''' OpenFOAM, Turbulence, YPlus, K-Omega, K-OmegaSST, Paraview, Video-Tutorial

{| border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Turbulence Modelling in OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn how to,
* Set up the '''blockMeshDict''' dictionary for a given '''YPlus''' value
* Implement '''k-omega''' and '''k-omega SST''' '''turbulence models'''
* '''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
|| As a prerequisite:
* You should have basic knowledge of '''geometric progression'''
* You should be familiar with '''simulating''' a''' turbulent flow''' through a''' channel '''and
* You should also be familiar with '''Multi-block Meshing of 2D Geometry'''
* 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'''.
The flow is '''turbulent.'''
|-
|| Only Narration
|| First, We will use''' k-epsilon turbulence model '''to '''simulate''' this '''case'''.
Let us set up the '''case.'''
|-
|| Only Narration
|| Download the '''kepsilon''' folder provided in the '''code files''' link and extract it.
|-
|| 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''' in the '''terminal'''.
|-
|| [Terminal] Type: '''cd $FOAM_RUN '''
|| Open the '''Run directory '''by typing this '''command.'''
|-
|| [Terminal]
Type: '''cp -r ~/Downloads/kepsilon .'''
|| Copy the downloaded file into the '''Run directory'''.
To do that, type the following '''command.'''
|-
|| Only Narration
|| I have downloaded the file into the '''Downloads directory.'''
Please change the '''command''' according to the '''file path''' on your machine.
|-
|| [Terminal] Type: '''cd kepsilon'''
|| Navigate to the '''kepsilon directory.'''
|-
|| [Terminal] Type:
'''gedit system/blockMeshDict'''
|| Open the '''blockMeshDict '''file in a '''text editor.'''
|-
|| [gedit -blockMeshDict]
Highlight '''blocks'''
|| Scroll down to the '''keyword “blocks”.'''
|-
|| [gedit -'''blockMeshDict''']
Highlight '''hex .... (1 0.18 1);'''
|| The '''domain''' has two equal-sized '''blocks.'''
|-
|| [gedit -'''blockMeshDict''']
Highlight '''75''' '''30'''
|| For each '''block''', the '''cell number''' is set to '''75 '''in the '''x-direction''', and '''30''' in the '''y-direction.'''
|-
|| Slide: Wall distance, yp
|| Let “'''yp'''” be the distance between the '''wall''' and the nearest '''cell centre'''.
For our '''case, yp''' is '''0.0031''' for '''YPlus''' value of '''200'''.
For''' channel flow''', the '''skin friction coefficient, Cf,''' is given by this formula.
|-
|| Slide: Cell width
|| The width of the''' cell '''near the '''wall''' is '''0.0062.'''
|-
|| Slide: Expansion ratio
|| The '''expansion ratio''' is the ratio of the last '''cell width''' to the first '''cell width.'''
|-
|| Slide: Expansion ratio calculation
|| It is calculated using '''geometric progression''' formula.
Please refer to the '''Additional Reading Material''' for more details.
|-
|| Slide: Expansion ratio value
|| The '''expansion ratio''' in the '''+y direction''' is found to be
* '''5.57 '''for '''block 1,''' and
* '''0.18 '''for''' block 2'''
for a '''block''' of width of '''0.5 m''' and '''cell number 30.'''
Please refer to the '''Additional Reading Material''' on this tutorial page for details.
|-
|| Only Narration
|| I have already put these values into the '''blockMeshDict''' file.
|-
|| [gedit -blockMeshDict]
Highlight''' simpleGrading'''
|| '''simpleGrading''' describes the uniform '''expansion ratio '''in '''x, y''', and''' z-directions.'''
|-
|| Only Narration
|| For our '''case''', the''' expansion ratio''' in the '''y-direction''' is
|-
|| [gedit -'''blockMeshDict''']
Highlight '''5.57'''
|| '''5.57 '''for '''block 1'''
|-
|| [gedit -'''blockMeshDict''']

Highlight''' 0.18'''
|| '''0.18''' for '''block 2'''
|-
|| [gedit - '''blockMeshDict'''] Close Text Editor
|| Close the '''blockMeshDict''' file.
|-
|| Only Narration
|| The '''case''' is now ready to be''' run. '''
|-
|| [Terminal] Type: '''blockMesh'''
|| On the '''terminal''', type '''blockMesh''' to '''mesh''' the '''geometry'''.
|-
|| [Terminal] Type:
'''simpleFoam'''
|| Then type '''simpleFoam''' in the '''terminal '''to '''run '''the '''simulation'''.
|-
|| Only Narration
|| The '''simulation '''will take some '''time''' depending on your computer’s '''hardware'''.
|-
|| [Terminal] Highlight''' End'''
|| The''' simulation''' is complete.
|-
|| Only Narration
|| Let's check the final value of '''YPlus.'''
|-
|| [Terminal] Type:
'''simpleFoam -postProcess -func "yPlus" -latestTime'''
|| Now type the following '''command''' on the '''terminal''' to get the '''YPlus '''value on the '''walls.'''
|-
|| [Terminal]
Highlight''' Patch to 213.433'''
|| We can see that the '''YPlus''' value stays below 300.
|-
|| [Terminal] Type: '''cd ..'''
|| Let us go back to the '''Run directory''' using the '''cd command'''.
|-
|| Only Narration
|| Let us '''simulate''' the same problem using the k-omega''' turbulence model '''now'''.'''
|-
|| Slide: K-Omega turbulence model
|| '''k-omega '''is a '''two-equation model'''.
It solves-
* The '''turbulent kinetic energy''' '''transport equation''', and
* The '''specific''' '''turbulent dissipation rate transport equation'''
|-
|| Slide: Inlet Boundary Condition - omega
|| Let's look at the '''boundary''' and '''initial conditions''' for '''omega.'''
We will use '''turbulentMixingLengthFrequencyInlet'''
It calculates '''omega''' using '''kappa '''and
user-specified '''mixing length. '''
'''Mixing length '''refers to the''' turbulent length scale.'''
'''Kappa''' value is automatically put in by the '''solver.'''
Here''', '''the value of''' turbulent length scale''' is '''0.07 m'''
The '''specific''' '''turbulent dissipation rate '''value is '''16.67 1/s'''
Where''' empirical constant, cmu '''is equal to '''0.09'''
|-
|| Slide: Wall & Outlet Boundary Condition - omega
|| '''Wall boundary condition''' is set to '''omegaWallFunction.'''
'''zeroGradient boundary condition''' is imposed at the '''outlet. '''
Please refer to the '''Additional Reading Material''' on this tutorial page for details.
|-
|| Only Narration
|| Download the '''komega '''folder provided in the '''Code files''' link and extract it.
|-
|| [Terminal] Type:
'''cp -r ~/Downloads/komega .'''
|| Copy the downloaded file into '''Run directory.'''
To do that, type the following '''command '''in the '''terminal.'''
|-
|| [Terminal] Type:
'''cd komega'''
|| Navigate to the '''komega''' directory using the '''cd command.'''
|-
|| Only Narration
|| Let’s take a look at the '''specific''' '''turbulent dissipation rate '''file.
|-
|| [Terminal] Type: '''gedit 0/omega'''
|| Open the '''omega''' file in a '''text editor.'''
|-
|| [gedit -'''omega''']
Highlight '''internalField ... 16.67;'''
|| The '''internalField''' value is initialised as '''16.67'''
|-
|| [gedit -'''omega''']
Highlight''' type turbulentMixingLengthFrequencyInlet'''
|| The '''inlet '''boundary '''type''' is set to '''turbulentMixingLengthFrequencyInlet'''
|-
|| [gedit -'''omega''']
Highlight''' mixingLength 0.07;'''
|| The '''keyword''' '''mixingLength '''represents the '''Turbulent length scale''', and is set to '''0.07'''
|-
|| [gedit -'''omega''']
Highlight''' value $internalField;'''
|| We have passed the '''internalField''' value to the '''patch field '''value.
|-
|| [gedit -'''omega'''] Highlight '''zeroGradient'''
|| The '''outlet patch type''' is set to '''zeroGradient.'''
|-
|| [gedit -'''omega''']
Highlight '''omegaWallFunction'''
|| The '''wall patch type''' is set to '''omegaWallFunction.'''
|-
|| [gedit -'''omega'''] Close Text Editor
|| Close the '''omega''' file.
|-
|| [Terminal] Type:
'''gedit constant/turbulenceProperties'''
|| Open the '''turbulenceProperties''' file in a '''text editor.'''
|-
|| [gedit -'''turbulenceProperties''']
Highlight''' kOmega'''
|| '''kOmega '''is selected as the '''RASModel.'''
Note,''' O '''is capitalized here.
|-
|| [gedit -'''turbulenceProperties''']
Highlight''' on'''
|| Ensure the '''keyword''' '''turbulence''' is set to '''On'''.
|-
|| [gedit -'''turbulenceProperties''']
Close Text Editor
|| Close the '''turbulenceProperties '''file.
|-
|| Only Narration
|| The '''case''' is now ready to be '''run.'''
|-
|| [Terminal] Type: '''blockMesh'''
|| On the '''terminal''', type '''blockMesh '''to '''mesh '''the '''geometry.'''
|-
|| [Terminal] Type: '''simpleFoam'''
|| Now, type the following '''command''' to '''run''' the '''case.'''
|-
|| [Terminal] Highlight''' End'''
|| The''' simulation''' is over.
|-
|| [Terminal] Type: '''cd ..'''
|| Let us go back to the '''Run directory''' using the '''cd command.'''
|-
|| Only Narration
|| Now, let’s '''run''' the same '''case''' with the '''k-omegaSST''' '''turbulence model.'''
|-
|| Slide: K-omegaSST turbulence model
|| The''' K-omega SST turbulence model''' is a '''hybrid '''model.
In the '''near-wall '''region, '''K-omegaSST''' uses the '''K-omega turbulence model.'''

In the region away from the '''wall''', it switches to the '''K-epsilon''' '''turbulence model'''.

Please refer to the '''Additional Reading Material''' on this tutorial page for details.
|-
|| Only Narration
|| Download the '''komegasst '''folder provided in the '''Code files''' link and extract it.
|-
|| [Terminal] Type:
'''cp -r ~/Downloads/komegasst .'''
|| Copy the downloaded file into the '''Run directory.'''
To do that, type the following '''command '''in the '''terminal.'''
|-
|| [Terminal] Type: '''cd komegasst'''
|| Navigate to the '''komegasst '''directory using the '''cd command.'''
|-
|| Only Narration
|| '''komega''' and '''komegasst models''' use the same''' turbulence variables'''.
Hence, the files in the '''0''' directory are the same.
|-
|| [Terminal] Type:
'''gedit constant/turbulenceProperties'''
|| Open the '''turbulence''' properties file in a '''text editor.'''
|-
|| [gedit -'''turbulenceProperties''']
Highlight '''kOmegaSST'''
|| '''RASModel field''' entry is set to '''kOmegaSST.'''
Note,''' O''' and''' SST''' are capitalized here.
|-
|| [gedit -'''turbulenceProperties''']
Close Text Editor
|| Close the '''turbulenceProperties''' file.
|-
|| [Terminal] Type:
'''gedit system/fvSchemes'''
|| Open '''fvSchemes dictionary''' in a '''text editor.'''
|-
|| Only Narration
|| Scroll down to the end of the document.
|-
|| [gedit -'''fvSchemes''']
Highlight '''wallDist ... ;}'''
|| '''wallDist sub-dictionary''' is included in the '''fvSchemes dictionary'''.
|-
|| Only Narration
|| This enables the calculation of the '''distance '''between the '''cell centre''' and the nearest '''wall.'''
|-
|| [gedit -'''fvSchemes'''] Close Text Editor
|| Close the '''fvSchemes''' file.
|-
|| Only Narration
|| The setup is now ready.
Let us '''run''' the '''simulation.'''
|-
|| [Terminal] Type: '''blockMesh'''
|| '''Mesh''' the '''geometry''' using the '''blockMesh command '''on the '''terminal.'''
|-
|| [Terminal] Type: '''simpleFoam'''
|| Type '''simpleFoam''' in the '''terminal.'''
|-
|| [Terminal] Highlight''' End'''
|| The '''simulation''' is finished successfully.
|-
|| Show slide
Exit velocity profile - comparison
|| The slide shows the''' exit velocity''' '''profile''' for all three '''turbulence models'''
|-
|| 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,
* Set up the '''blockMeshDict''' file for a given '''YPlus''' value
* Implement '''k-omega '''and''' k-omega SST turbulence models'''
* '''Run''' the '''simulation'''
|-
|| Slide: Assignment
|| As an assignment:
* Repeat the '''simulation''' for a '''YPlus''' value of '''250 '''using '''k-epsilon''' '''model'''
* Repeat the''' simulation '''for a '''velocity''' of '''40 m/s''' using '''k-omega''' and '''k-omega SST model'''
|-
|| 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 Sridhar from IIT Bombay signing off.
Thanks for joining.
|-
|}

OpenFOAM-version-7/C2/Turbulence-Modelling-in-OpenFOAM/English

2020-07-25T07:35:16Z

Divyesh7: Created page with "'''Title of the script:''' Turbulence Modelling in OpenFOAM '''Author:''' Padmini Priyadarshini '''Keywords:''' OpenFOAM, Turbulence, YPlus, K-Omega, K-OmegaSST, Paraview, V..."

'''Title of the script:''' Turbulence Modelling in OpenFOAM

'''Author:''' Padmini Priyadarshini

'''Keywords:''' OpenFOAM, Turbulence, YPlus, K-Omega, K-OmegaSST, Paraview, Video-Tutorial

{| border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Turbulence Modelling in OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn how to,
* Set up the '''blockMeshDict''' dictionary for a given '''YPlus''' value
* Implement '''k-omega''' and '''k-omega SST''' '''turbulence models'''
* '''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
|| As a prerequisite:
* You should have basic knowledge of '''geometric progression'''
* You should be familiar with '''simulating''' a''' turbulent flow''' through a''' channel '''and
* You should also be familiar with '''Multi-block Meshing of 2D Geometry'''
* 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'''.
The flow is '''turbulent.'''
|-
|| Only Narration
|| First, We will use''' k-epsilon turbulence model '''to '''simulate''' this '''case'''.
Let us set up the '''case.'''
|-
|| Only Narration
|| Download the '''kepsilon''' folder provided in the '''code files''' link and extract it.
|-
|| 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''' in the '''terminal'''.
|-
|| [Terminal] Type: '''cd $FOAM_RUN '''
|| Open the '''Run directory '''by typing this '''command.'''
|-
|| [Terminal]
Type: '''cp -r ~/Downloads/kepsilon .'''
|| Copy the downloaded file into the '''Run directory'''.
To do that, type the following '''command.'''
|-
|| Only Narration
|| I have downloaded the file into the '''Downloads directory.'''
Please change the '''command''' according to the '''file path''' on your machine.
|-
|| [Terminal] Type: '''cd kepsilon'''
|| Navigate to the '''kepsilon directory.'''
|-
|| [Terminal] Type:
'''gedit system/blockMeshDict'''
|| Open the '''blockMeshDict '''file in a '''text editor.'''
|-
|| [gedit -blockMeshDict]
Highlight '''blocks'''
|| Scroll down to the '''keyword “blocks”.'''
|-
|| [gedit -'''blockMeshDict''']
Highlight '''hex .... (1 0.18 1);'''
|| The '''domain''' has two equal-sized '''blocks.'''
|-
|| [gedit -'''blockMeshDict''']
Highlight '''75''' '''30'''
|| For each '''block''', the '''cell number''' is set to '''75 '''in the '''x-direction''', and '''30''' in the '''y-direction.'''
|-
|| Slide: Wall distance, yp
|| Let “'''yp'''” be the distance between the '''wall''' and the nearest '''cell centre'''.
For our '''case, yp''' is '''0.0031''' for '''YPlus''' value of '''200'''.
For''' channel flow''', the '''skin friction coefficient, Cf,''' is given by this formula.
|-
|| Slide: Cell width
|| The width of the''' cell '''near the '''wall''' is '''0.0062.'''
|-
|| Slide: Expansion ratio
|| The '''expansion ratio''' is the ratio of the last '''cell width''' to the first '''cell width.'''
|-
|| Slide: Expansion ratio calculation
|| It is calculated using '''geometric progression''' formula.
Please refer to the '''Additional Reading Material''' for more details.
|-
|| Slide: Expansion ratio value
|| The '''expansion ratio''' in the '''+y direction''' is found to be
* '''5.57 '''for '''block 1,''' and
* '''0.18 '''for''' block 2'''
for a '''block''' of width of '''0.5 m''' and '''cell number 30.'''
Please refer to the '''Additional Reading Material''' on this tutorial page for details.
|-
|| Only Narration
|| I have already put these values into the '''blockMeshDict''' file.
|-
|| [gedit -blockMeshDict]
Highlight''' simpleGrading'''
|| '''simpleGrading''' describes the uniform '''expansion ratio '''in '''x, y''', and''' z-directions.'''
|-
|| Only Narration
|| For our '''case''', the''' expansion ratio''' in the '''y-direction''' is
|-
|| [gedit -'''blockMeshDict''']
Highlight '''5.57'''
|| '''5.57 '''for '''block 1'''
|-
|| [gedit -'''blockMeshDict''']

Highlight''' 0.18'''
|| '''0.18''' for '''block 2'''
|-
|| [gedit - '''blockMeshDict'''] Close Text Editor
|| Close the '''blockMeshDict''' file.
|-
|| Only Narration
|| The '''case''' is now ready to be''' run. '''
|-
|| [Terminal] Type: '''blockMesh'''
|| On the '''terminal''', type '''blockMesh''' to '''mesh''' the '''geometry'''.
|-
|| [Terminal] Type:
'''simpleFoam'''
|| Then type '''simpleFoam''' in the '''terminal '''to '''run '''the '''simulation'''.
|-
|| Only Narration
|| The '''simulation '''will take some '''time''' depending on your computer’s '''hardware'''.
|-
|| [Terminal] Highlight''' End'''
|| The''' simulation''' is complete.
|-
|| Only Narration
|| Let's check the final value of '''YPlus.'''
|-
|| [Terminal] Type:
'''simpleFoam -postProcess -func "yPlus" -latestTime'''
|| Now type the following '''command''' on the '''terminal''' to get the '''YPlus '''value on the '''walls.'''
|-
|| [Terminal]
Highlight''' Patch to 213.433'''
|| We can see that the '''YPlus''' value stays below 300.
|-
|| [Terminal] Type: '''cd ..'''
|| Let us go back to the '''Run directory''' using the '''cd command'''.
|-
|| Only Narration
|| Let us '''simulate''' the same problem using the k-omega''' turbulence model '''now'''.'''
|-
|| Slide: K-Omega turbulence model
|| '''k-omega '''is a '''two-equation model'''.
It solves-
* The '''turbulent kinetic energy''' '''transport equation''', and
* The '''specific''' '''turbulent dissipation rate transport equation'''
|-
|| Slide: Inlet Boundary Condition - omega
|| Let's look at the '''boundary''' and '''initial conditions''' for '''omega.'''
We will use '''turbulentMixingLengthFrequencyInlet'''
It calculates '''omega''' using '''kappa '''and
user-specified '''mixing length. '''
'''Mixing length '''refers to the''' turbulent length scale.'''
'''Kappa''' value is automatically put in by the '''solver.'''
Here''', '''the value of''' turbulent length scale''' is '''0.07 m'''
The '''specific''' '''turbulent dissipation rate '''value is '''16.67 1/s'''
Where''' empirical constant, cmu '''is equal to '''0.009'''
|-
|| Slide: Wall & Outlet Boundary Condition - omega
|| '''Wall boundary condition''' is set to '''omegaWallFunction.'''
'''zeroGradient boundary condition''' is imposed at the '''outlet. '''
Please refer to the '''Additional Reading Material''' on this tutorial page for details.
|-
|| Only Narration
|| Download the '''komega '''folder provided in the '''Code files''' link and extract it.
|-
|| [Terminal] Type:
'''cp -r ~/Downloads/komega .'''
|| Copy the downloaded file into '''Run directory.'''
To do that, type the following '''command '''in the '''terminal.'''
|-
|| [Terminal] Type:
'''cd komega'''
|| Navigate to the '''komega''' directory using the '''cd command.'''
|-
|| Only Narration
|| Let’s take a look at the '''specific''' '''turbulent dissipation rate '''file.
|-
|| [Terminal] Type: '''gedit 0/omega'''
|| Open the '''omega''' file in a '''text editor.'''
|-
|| [gedit -'''omega''']
Highlight '''internalField ... 16.67;'''
|| The '''internalField''' value is initialised as '''16.67'''
|-
|| [gedit -'''omega''']
Highlight''' type turbulentMixingLengthFrequencyInlet'''
|| The '''inlet '''boundary '''type''' is set to '''turbulentMixingLengthFrequencyInlet'''
|-
|| [gedit -'''omega''']
Highlight''' mixingLength 0.07;'''
|| The '''keyword''' '''mixingLength '''represents the '''Turbulent length scale''', and is set to '''0.07'''
|-
|| [gedit -'''omega''']
Highlight''' value $internalField;'''
|| We have passed the '''internalField''' value to the '''patch field '''value.
|-
|| [gedit -'''omega'''] Highlight '''zeroGradient'''
|| The '''outlet patch type''' is set to '''zeroGradient.'''
|-
|| [gedit -'''omega''']
Highlight '''omegaWallFunction'''
|| The '''wall patch type''' is set to '''omegaWallFunction.'''
|-
|| [gedit -'''omega'''] Close Text Editor
|| Close the '''omega''' file.
|-
|| [Terminal] Type:
'''gedit constant/turbulenceProperties'''
|| Open the '''turbulenceProperties''' file in a '''text editor.'''
|-
|| [gedit -'''turbulenceProperties''']
Highlight''' kOmega'''
|| '''kOmega '''is selected as the '''RASModel.'''
Note,''' O '''is capitalized here.
|-
|| [gedit -'''turbulenceProperties''']
Highlight''' on'''
|| Ensure the '''keyword''' '''turbulence''' is set to '''On'''.
|-
|| [gedit -'''turbulenceProperties''']
Close Text Editor
|| Close the '''turbulenceProperties '''file.
|-
|| Only Narration
|| The '''case''' is now ready to be '''run.'''
|-
|| [Terminal] Type: '''blockMesh'''
|| On the '''terminal''', type '''blockMesh '''to '''mesh '''the '''geometry.'''
|-
|| [Terminal] Type: '''simpleFoam'''
|| Now, type the following '''command''' to '''run''' the '''case.'''
|-
|| [Terminal] Highlight''' End'''
|| The''' simulation''' is over.
|-
|| [Terminal] Type: '''cd ..'''
|| Let us go back to the '''Run directory''' using the '''cd command.'''
|-
|| Only Narration
|| Now, let’s '''run''' the same '''case''' with the '''k-omegaSST''' '''turbulence model.'''
|-
|| Slide: K-omegaSST turbulence model
|| The''' K-omega SST turbulence model''' is a '''hybrid '''model.
In the '''near-wall '''region, '''K-omegaSST''' uses the '''K-omega turbulence model.'''

In the region away from the '''wall''', it switches to the '''K-epsilon''' '''turbulence model'''.

Please refer to the '''Additional Reading Material''' on this tutorial page for details.
|-
|| Only Narration
|| Download the '''komegasst '''folder provided in the '''Code files''' link and extract it.
|-
|| [Terminal] Type:
'''cp -r ~/Downloads/komegasst .'''
|| Copy the downloaded file into the '''Run directory.'''
To do that, type the following '''command '''in the '''terminal.'''
|-
|| [Terminal] Type: '''cd komegasst'''
|| Navigate to the '''komegasst '''directory using the '''cd command.'''
|-
|| Only Narration
|| '''komega''' and '''komegasst models''' use the same''' turbulence variables'''.
Hence, the files in the '''0''' directory are the same.
|-
|| [Terminal] Type:
'''gedit constant/turbulenceProperties'''
|| Open the '''turbulence''' properties file in a '''text editor.'''
|-
|| [gedit -'''turbulenceProperties''']
Highlight '''kOmegaSST'''
|| '''RASModel field''' entry is set to '''kOmegaSST.'''
Note,''' O''' and''' SST''' are capitalized here.
|-
|| [gedit -'''turbulenceProperties''']
Close Text Editor
|| Close the '''turbulenceProperties''' file.
|-
|| [Terminal] Type:
'''gedit system/fvSchemes'''
|| Open '''fvSchemes dictionary''' in a '''text editor.'''
|-
|| Only Narration
|| Scroll down to the end of the document.
|-
|| [gedit -'''fvSchemes''']
Highlight '''wallDist ... ;}'''
|| '''wallDist sub-dictionary''' is included in the '''fvSchemes dictionary'''.
|-
|| Only Narration
|| This enables the calculation of the '''distance '''between the '''cell centre''' and the nearest '''wall.'''
|-
|| [gedit -'''fvSchemes'''] Close Text Editor
|| Close the '''fvSchemes''' file.
|-
|| Only Narration
|| The setup is now ready.
Let us '''run''' the '''simulation.'''
|-
|| [Terminal] Type: '''blockMesh'''
|| '''Mesh''' the '''geometry''' using the '''blockMesh command '''on the '''terminal.'''
|-
|| [Terminal] Type: '''simpleFoam'''
|| Type '''simpleFoam''' in the '''terminal.'''
|-
|| [Terminal] Highlight''' End'''
|| The '''simulation''' is finished successfully.
|-
|| Show slide
Exit velocity profile - comparison
|| The slide shows the''' exit velocity''' '''profile''' for all three '''turbulence models'''
|-
|| 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,
* Set up the '''blockMeshDict''' file for a given '''YPlus''' value
* Implement '''k-omega '''and''' k-omega SST turbulence models'''
* '''Run''' the '''simulation'''
|-
|| Slide: Assignment
|| As an assignment:
* Repeat the '''simulation''' for a '''YPlus''' value of '''250 '''using '''k-epsilon''' '''model'''
* Repeat the''' simulation '''for a '''velocity''' of '''40 m/s''' using '''k-omega''' and '''k-omega SST model'''
|-
|| 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 Sridhar from IIT Bombay signing off.
Thanks for joining.
|-
|}

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

2020-07-23T07:12:04Z

Divyesh7: Created page with "'''Title of the script:''' Simulation of a Turbulent Flow in a 2D Channel using OpenFOAM '''Author:''' Padmini Priyadarshini '''Keywords:''' OpenFOAM, Turbulence, K-Epsilon,..."

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

'''Author:''' Padmini Priyadarshini

'''Keywords:''' OpenFOAM, Turbulence, K-Epsilon, 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.
|-
|| [Terminal] Type:

'''ls system'''
|| Type''' '''the following''' command''' 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 '''0.00261 '''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 i'''s 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
|| 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 .. 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 0.00261;'''
|| The '''keyword intensity '''represents the '''turbulent intensity''', and is set to '''0.00261'''
|-
|| [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/Basic-Post-Processing-using-ParaView/English

2020-07-23T04:55:35Z

Divyesh7:

'''Title of the script:''' Basic Post Processing using ParaView

'''Author:''' Divyesh Variya

'''Keywords:''' OpenFOAM, Hagen Poiseuille, Paraview, Clip, Streamline, Glyph, Plot-over-line, Parabolic profile, Video-Tutorial

{| Border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Basic Post Processing using ParaView.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn,
* Some basic '''visualization techniques''' in '''ParaView'''
* Export the''' field data '''to '''.csv''' file
* Plot a''' graph''' in '''LibreOffice Suite Calc '''and
* Save a screenshot of a '''view'''

|-
|| 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
* '''LibreOffice Suite''' 6.4

|-
|| Slide: Prerequisites* Please go through these two tutorials on https://spoken-tutorial.org

|| As a prerequisite learner should practise,
* On '''Simulating Hagen Poiseuille Flow through a Pipe''' from the '''OpenFOAM '''tutorials and
* Tutorial on '''Using Charts and Graphs''' from '''LibreOffice Suite Calc'''
* Please go through these two tutorials on this website.

|-
|| Press Ctrl + Alt + T keys
|| Open the '''terminal''' by pressing the '''Ctrl''', '''Alt''' and '''T''' keys together.
|-
|| Only Narration
|| From now onwards please remember to press the '''Enter''' key after typing each '''command.'''
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| At the '''prompt''', type the following '''command''' to go to the '''run directory'''.
|-
|| [Terminal] Type:

'''cd pipe'''
|| Navigate to the '''pipe case '''folder.

We have created this in the''' “Simulating Hagen Poiseuille Flow through Pipe” '''tutorial.
|-
|| [Terminal] Type: '''paraFoam'''
|| Type '''paraFoam''' in the '''terminal''' to open the '''case''' file in '''paraView'''.
|-
|| [ParaView]

'''Uncheck >> inlet and outlet'''
|| Go to the '''properties''' panel.

Scroll down and locate the '''mesh parts''' section.

Uncheck all '''patches''' other than '''internalMesh'''.
|-
|| [ParaView] '''Click on Apply'''
|| Click on the '''Apply''' button in the '''Properties '''panel.
|-
|| [ParaView]

'''Click on Solid Color >> Click on U'''
|| Click on '''Solid Color '''available in the '''Active Variable Controls.'''

From here, we can change the fields that we want to visualize.

Select the '''U''' field with the dot, not the one with the box.
|-
|| [ParaView]

'''Click on Last Frame'''
|| From '''VCR Controls''', we can change the''' time steps''' and '''run animation''' using the '''Play''' button.

Currently we are on 0 time, which is for the '''initial field'''.

To go to the last '''time step, '''click on the '''Last Frame''' button.
|-
|| Show Picture of ICONS
|| As you can see, some '''filter''' icons are shown here.
|-
|| [ParaView]

'''Click on Stream Tracer filter'''
|| To visualize '''streamline''', click on the '''Stream tracer''' icon from '''Common and Data Analysis Filters'''.
|-
|| [ParaView]

'''Change seed type to point source'''
|| From the '''Properties''' panel we can change the '''seed type.'''

The two '''seed types''' available are:
* '''High resolution line source''' and
* '''Point Source'''

'''High resolution Line Source''' gives '''streamlines''' passing through a '''line'''.

'''Point Source''' gives '''streamlines''' passing through a '''sphere'''.

We will select '''Point Source'''.
|-
|| [ParaView]

'''Set number of points to 1000 >>'''

'''Uncheck Show Sphere checkbox'''
|| Set the '''number of points''' to '''1000''' and '''uncheck''' the '''Show Sphere''' option to hide the sphere.
|-
|| [ParaView]

'''Click on Apply'''
|| Click on the '''Apply''' button in the '''Properties''' panel.

We can see 1000 '''streamlines''' passing through 1000 random points within the sphere.
|-
|| [ParaView]

'''Click on Delete button'''
|| This way we can visualize the '''streamline'''.

Now '''Delete''' the '''Stream Tracer filter''' by clicking on the '''Delete''' button on the '''Properties''' panel.
|-
|| [ParaView] '''Click on Glyph filter'''
|| Click on the '''Glyph''' icon from '''Common and Data Analysis Filters'''.
|-
|| [ParaView]

'''Change Orientation U'''
|| Change '''Orientation Array''' to '''U '''from''' '''the '''Properties''' panel.
|-
|| [ParaView] '''Scale array U'''
|| Change '''Scale array''' to '''U '''in''' '''the '''Properties''' panel.
|-
|| [ParaView] '''Click on Apply'''
|| Click on the '''Apply''' button in the '''Properties '''panel.
|-
|| [ParaView]

'''Hide pipe.OpenFOAM'''
|| Hide '''pipe.OpenFOAM''' from the '''pipeline browser '''by clicking on the eye icon.
|-
|| [ParaView]

'''Zoom in render layout with left mouse click and drag'''
|| We can see '''Arrows''' in the direction of the '''flow'''.
|-
|| [ParaView] '''Delete Glyph filter'''
|| '''Delete''' the '''Glyph filter '''from the '''Properties''' panel.
|-
|| [ParaView] '''Click on Clip filter'''
|| Click on the '''clip''' icon from '''Common and Data Analysis Filters''' to clip the '''mesh'''.
|-
|| [ParaView]

'''Uncheck Show plane and invert'''
|| Uncheck “'''Show Plane'''” and “'''invert'''” boxes from the '''Properties '''panel.
|-
|| [ParaView] '''Click on Apply'''
|| Click on the '''Apply''' button in the '''Properties '''panel.
|-
|| Only Narration
|| This way we can clip any '''mesh''' and visualize '''internal flow'''.
|-
|| [ParaView] '''Delete Clip filter'''
|| Delete the '''Clip''' filter from the '''Properties''' panel.
|-
|| [ParaView]

'''Click on Plot Over Line Filter'''
|| Click on the “'''Plot Over Line'''” filter from '''Common and Data Analysis Filters'''.
|-
|| [ParaView]

'''Click on Y Axis'''
|| Click on '''Y Axis''' on the '''Properties''' panel and click '''Apply'''.
|-
|| [ParaView]'''Highlight '''

'''Line Chart view window'''
|| A new '''line chart window''' opens automatically with '''P''' and '''U_Magnitude''' '''graphs'''.
|-
|| [ParaView]

'''Scroll properties panel and uncheck p from series parameter'''
|| In the '''Properties''' panel, scroll down and locate the '''series parameters''' section.

Uncheck '''P''' from that.
|-
|| [ParaView] '''Highlight '''

'''Line Chart view window'''
|| We will get a '''parabolic profile''' for '''velocity''' in the graph.
|-
|| [ParaView] '''Click on Line chart view window'''

'''Press CTRL+S'''
|| Click on the '''Line Chart View''' window

And press '''Ctrl+S''' keys to save data.
|-
|| [Save File:]

'''Select file type as .csv '''

'''give name - Y-Axis'''
|| Select '''Files of type''' as '''.csv''' and give the file name '''Y(hyphen)Axis.'''
|-
|| [Save File:]

'''Click >> OK'''
|| Click on '''OK'''.

Again click on '''OK''' with default settings.
|-
|| Only Narration
|| The data is saved in a '''.csv''' file.

We can open this file in '''LibreOffice Calc''' and compare with an analytical solution.
|-
|| [ParaView]

'''Click on File >> Save Screenshot...'''
|| Now go to the '''File''' menu in the menu bar and select '''Save Screenshot.'''
|-
|| [ParaView]

'''File name - velocity'''

'''File type - .png'''
|| Give a '''File Name''' and select''' file type'''.

Here I am saving the screenshot as '''velocity''' with the '''.png''' file type.
|-
|| [ParaView] '''Click >> OK'''
|| Click on the '''OK''' button.
|-
|| [ParaView]

'''Click >> OK'''
|| The '''Save Screenshot''' option window pops up.

We can change the '''size''', '''scaling''', '''coloring''' and other image options here.

With the default values in the settings, click on the '''OK''' button.
|-
|| Only Narration
|| '''Screenshot''' of '''Parabolic curve profile''' is saved in our '''case '''directory.
|-
|| [ParaView]

'''Click on Z Axis'''
|| Go to the '''Properties''' panel.

Click on '''Z Axis''' and then click on the '''Apply''' button.
|-
|| [ParaView]

'''Uncheck U_Magnitude and check p'''
|| Then go to the '''series parameter''' section in the '''Properties''' panel.

Uncheck '''U_Magnitude''' field and check '''p field.'''
|-
|| [ParaView]

'''Press CTRL+S'''

'''Select .csv file type'''

'''Give a name - Z-Axis'''

'''Press OK'''

'''Press OK'''
|| Save this data to''' Z-Axis.csv''' file as explained earlier.
|-
|| [ParaView] '''Close ParaView'''
|| Close the '''ParaView''' window.
|-
|| '''Open File explorer'''
|| Open the '''File explorer '''from the '''taskbar'''.
|-
|| [File explorer]

'''Open >> OpenFOAM'''
|| Open the '''OpenFOAM''' directory.

Here we can see the '''username '''directory of our computer.
|-
|| [File explorer]

'''Open >> “username directory”'''
|| Now open your current '''user '''directory.

In the '''user''' directory we can see the “'''run'''” directory.
|-
|| [File explorer]

'''Open >> run'''
|| Open the “'''run'''” directory.

Our saved work is available here in the '''pipe''' directory.
|-
|| [File explorer] '''Open >> pipe '''
|| Now open the '''pipe''' directory.
|-
|| '''Only Narration'''
|| Here we can see all files including '''screenshot image''' and '''.csv files''' that we have saved.
|-
|| [File explorer]

'''Right click on >> Z-Axis.csv'''
|| Right click on '''Z-Axis.csv''' file.
|-
|| [File explorer]

'''Click on >> Open With Other Application'''
|| From the list, click on the “'''Open With Other Application'''” option.
|-
|| [File explorer]

'''Click on >> View All Application'''
|| Now click on the “'''View All Application'''” button.
|-
|| [File explorer]

'''Double click on >> LibreOffice Calc'''
|| A list of all the '''applications''' available in your computer will appear.

From this list find “'''LibreOffice Calc'''” and double click on it.
|-
|| [File explorer]

'''Click on >> OK'''
|| A “'''Text Import'''” window will open on your screen.

At the bottom right corner click on the '''OK''' button.
|-
|| Highlight '''LibreOffice suite calc'''
|| Our file is now open in '''LibreOffice Calc.'''
|-
|| [LibreOffice suite calc]

'''Highlight cells'''
|| We have

'''velocity U:0''' at '''Point:0'''

'''Velocity U:1''' at '''Point:1 '''and

'''Velocity U:2''' at '''Point:2'''.
|-
|| [LibreOffice suite calc]

'''Highlight cells'''
|| We have '''kinematic pressure p''', '''vtkValidPointMask''' and '''arc_length''' also.
|-
|| [LibreOffice suite calc]

'''Highlight cells'''
|| Necessary data to plot the graph is '''U:2''', '''Point:2''' and '''p'''.
|-
|| [LibreOffice suite calc]

Show Graphs
|| For this demonstration I have created a graph on '''z-axis''' versus '''kinematic pressure'''.

And another graph for '''z-axis''' versus '''velocity'''.
|-
|| [LibreOffice suite calc]

Show Graphs
|| In the same way I have created a '''y-axis''' versus '''velocity''' graph with a '''y-axis.csv''' file.
|-
|| Only Narration
|| Here you can also compare '''analytical '''solutions with '''OpenFoam''' solutions.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

Let us summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt,
* Some basic '''visualization techniques''' in '''ParaView'''
* Export''' field data '''to''' .csv''' file
* Plot''' graph''' in '''LibreOffice suite calc '''and
* Save screenshot of a '''view'''

|-
|| Slide: Assignment
|| As an assignment:
* Simulate the '''Hagen Poiseuille flow''' for the '''pipe''' of '''0.5 cm''' diameter with
* '''Inlet''' '''velocity''' '''0.05 m/s''' and '''outlet pressure''' '''0 Pascal''' and,
* Plot graphs of '''velocity''' and '''pressure '''in''' ParaView '''and''' LibreOffice Calc'''.

|-
|| 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 on this website
|-
|| 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 Divyesh Variya.

And this is Swetha Sridhar from IIT Bombay signing off. Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Simulating-Hagen-Poiseuille-flow-through-a-pipe-in-OpenFOAM/English

2020-07-22T10:50:47Z

Divyesh7:

'''Title of the script:''' Simulating Hagen Poiseuille flow through a pipe in OpenFOAM

'''Author:''' Divyesh Variya

'''Keywords:''' OpenFOAM, Hagen Poiseuille, Pipe flow, icoFoam, controlDict, Video-Tutorial

{| Border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Simulating Hagen Poiseuille flow through a pipe in OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn to,

* Set up the '''boundary''' and '''initial''' '''conditions'''
* Set up the '''physical properties'''
* Set up the '''solve & write control parameter '''and
* Run the '''simulation'''

|-
|| 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 '''Hagen Poiseuille flow''' and basic '''Fluid Dynamics '''concepts
* You should also be familiar with creation of a '''3D pipe Geometry''' in '''OpenFOAM'''
* If you are 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: Problem Setup
|| In this diagram, a '''section view''' of a '''3D pipe''' is shown.

This describes the '''problem statement'''.

* The '''diameter''' of the '''pipe''' is 1 centimeter and its '''length''' is 30 centimeters.
* It has one '''inlet''', one '''outlet''' and a '''cylindrical''' '''wall'''.

* The fluid here is water''' '''and its '''kinematic viscosity''' is taken as '''1e-06'''.

* The '''Inlet velocity '''is '''0.025 m/s '''and''' the Outlet pressure '''is''' 0 Pascals '''as shown in the diagram.

|-
|| Slide: Geometry Check

Highlight '''250'''

Highlight''' laminar'''

Only Narration

Le = 0.06*Re*D

Highlight''' 0.15 m'''

|| Let us check whether our '''geometry''' is suitable or not.

* '''Reynolds number''' of the problem is '''250'''.

* Hence, the flow is '''laminar'''.

* For '''fully developed flow''', length of the '''geometry''' should be greater than the '''Entrance length'''.

* '''Entrance length''' can be calculated by this '''formula'''.

* The length we have taken is greater than the '''entrance length'''.
|-
|| Slide: Solver detail
||
* To simulate this problem, we will use the '''icoFoam''' solver.

* '''icoFoam''' is a''' transient solver''' for '''incompressible''', '''laminar flow''' of '''Newtonian fluids'''.

* This is the most '''suitable solver''' for '''Hagen Poiseuille flow.'''

|-
|| Slide : Pressure Boundary Condition
|| The''' Pressure boundary conditions''' used are,

* At '''inlet - zero gradient'''
* At '''outlet - fixed Pressure''' and
* At '''wall - zero gradient'''

|-
|| Slide: Velocity Boundary Condition
|| The''' Velocity boundary condition''' used are,

* At '''inlet - fixed value'''
* At '''outlet - zero Gradient''' and
* At '''wall - No Slip'''

|-
|| Only Narration
|| We will use the '''mesh''' that we have created in the tutorial “'''Creating 3D Pipe Geometry and Mesh in OpenFoam'''”.
|-
|| Press Ctrl + Alt + T keys
|| Open the '''terminal''' by pressing the '''Ctrl''', '''Alt''' and '''T''' keys together.
|-
|| [Terminal]

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

'''cd $FOAM_RUN'''
|| At the '''prompt''', type the following '''command''' to go to the '''run directory'''.

|-
|| [Terminal] Type:

'''cd pipe'''
|| Navigate to the '''pipe case folder'''.

|-
|| [Terminal] Type:

'''mv 0.Orig 0'''
|| Now, '''rename''' '''0.Orig''' folder to''' 0''' by typing this '''command'''.

|-
|| [Terminal] Type: '''gedit 0/p'''
|| Let us open the “'''p'''” file in a '''text editor'''.
|-
|| [gedit - '''p'''] Highlight

'''dimensions [0 2 -2 0 0 0 0];'''
|| Here we can see, the '''p''' file is in the form of '''pressure divided by density'''.

This means, it is '''kinematic pressure'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''internalField''' to the end of the file as shown here.
|-
|| [gedit - '''pressure''']
|| Open the file '''pressure.txt''', that you had downloaded in any '''text editor'''.
|-
|| [gedit - '''pressure'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''p''']
|| Now let me switch back to the “'''p”''' file.
|-
|| [gedit - '''p'''] '''Paste '''
|| Paste the copied contents into the “'''p” '''file as shown here.
|-
|| [gedit - '''p'''] Highlight

'''internalField'''
|| Right after '''dimensions''', we have to define the '''initial condition'''.

It could be '''uniform''', '''non-uniform''' or in the form of '''code'''.
|-
|| [gedit - '''p'''] Highlight

'''uniform 0;'''
|| In this case, we will use the '''initial condition''' as''' uniform 0'''.

This means that the '''kinematic pressure''' inside the entire '''domain''' is '''0'''.
|-
|| [gedit - '''p'''] Highlight

'''boundaryField'''
|| In the '''boundaryField''', we specify '''boundary conditions''' for all '''patches''' and '''walls'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| '''Boundary condition''' for '''inlet''' in '''pressure''' is defined as shown.
|-
|| [gedit - '''p'''] Highlight

'''type zeroGradient;'''
|| Type of the '''boundary condition''' is '''zeroGradient'''.

'''Zero Gradient boundary '''extrapolates the quantity to the '''patch''' from the nearest '''cell value'''.

So, the value at the '''patch''' will be the same as the '''cell value'''.

Note that '''z''' is small and '''G''' is capital.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> wall'''
|| '''Boundary condition''' for the '''wall''' is defined as the same as '''inlet'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> outlet'''
|| '''Boundary condition''' for '''outlet''' in '''pressure''' is defined as shown here.
|-
|| [gedit - '''p'''] Highlight

'''type fixedValue;'''

'''value 0;'''
|| The type of '''boundary condition''' is '''fixedValue'''.

'''Value''' given is '''zero'''.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''p '''file and close the '''text editor'''.
|-
|| [Terminal] Type:

'''gedit 0/U'''
|| Now, let us set the '''initial''' and '''boundary condition''' for '''velocity'''.

To do so, open the '''U''' file in a '''text editor'''.
|-
|| [gedit - '''U'''] Highlight

'''dimensions [0 1 -1 0 0 0 0];'''
|| '''Dimensions''' here are in '''meters per second'''.
|-
|| [gedit - '''U'''] Highlight

'''internalField uniform (0 0 0);'''
|| '''Velocity''' is a '''vector field''', so the '''internal initial field''' is set as '''uniform (0 0 0)'''.
|-
|| [gedit - '''U'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''boundaryField''' to the end of the file as shown here.
|-
|| [gedit - '''velocity''']
|| Open the '''velocity.txt '''file that you had downloaded in a '''text editor'''.
|-
|| [gedit - '''velocity'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''U'''] '''Paste '''
|| Paste the copied contents into the “'''U” '''file as shown.
|-
|| [gedit - '''U'''] Highlight

'''boundaryField'''
|| In the '''boundaryField''', we will specify '''boundary conditions''' for all '''patches''' and '''walls'''.
|-
|| [gedit - '''U'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| '''Boundary condition''' for '''inlet''' in '''velocity''' is defined as shown here.
|-
|| [gedit - '''U'''] Highlight

'''type fixedValue;'''

'''value uniform (0 0 0.025);'''
|| Type of the '''boundary condition''' is '''fixedValue'''.

Value of '''velocity''' is 0.025 m/s in the '''Z direction'''.
|-
|| [gedit - '''U'''] Highlight

'''type noSlip;'''
|| '''Boundary condition''' for the '''wall''' is defined as '''noSlip'''.

This means '''velocity''' at the '''wall '''is '''0'''.
|-
|| [gedit - '''U'''] Highlight

'''type zeroGradient;'''
|| '''Boundary condition''' for '''outlet''' is '''zeroGradient''', defined as shown here.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''U '''file and close the '''text editor.'''
|-
|| [Terminal] Type:

'''gedit constant/transportProperties'''
|| Open '''transport properties''' file from '''constant folder''' in the '''text editor'''.
|-
|| [gedit - '''transportProperties'''] Highlight

'''nu'''
|| All '''properties''' of '''fluid''' which remain '''constant''' during the '''simulation''' is to be specified in the '''constant folder'''.

Here, we will set the value of '''kinematic viscosity'''.
|-
|| [gedit - '''transportProperties'''] Highlight

'''[0 2 -1 0 0 0 0]'''
|| Dimensions of '''kinematic viscosity''' are specified here.
|-
|| [gedit - '''transportProperties''']

'''Change: 0.01 >> 1e-06'''
|| To set the value of '''nu,''' replace '''0.01''' to '''1e-06'''.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''transportProperties '''file and close the '''text editor.'''
|-
|| Only Narration
|| '''Solve & write control parameters''' can be modified in the '''controlDict''' file.

The '''controlDict '''file is located in the '''system folder'''.
|-
|| [Terminal] Type:

'''gedit system/controlDict'''
|| Open the '''controlDict''' file in a '''text editor'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''application''' to the end of the file as shown here.
|-
|| [gedit - '''control''']
|| Open the '''control.txt''' file that you had downloaded in a '''text editor'''.
|-
|| [gedit - '''control'''] Highlight

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

|| and paste the copied contents into the “'''controlDict” '''file as shown here.
|-
|| [gedit - '''controlDict'''] Highlight

'''application icoFoam;'''
|| First line of the '''controlDict''' file shows the name of the '''solver'''.

In our case it is '''icoFoam'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''startFrom startTime;'''

'''startTime 0;'''
|| The second and third lines are '''start simulation controls'''.

Our '''simulation''' will start from the value specified in '''start time'''.

Here our '''start time''' is set to '''0'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''stopAt endTime;'''

'''endTime 5;'''
|| The fourth and fifth lines are '''stop simulation controls'''.

'''Simulation''' will stop at the''' endTime''' of '''5 seconds'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''deltaT 1e-2;'''
|| Then the value of '''deltaT''' is given, which is '''1e-02'''.

So, it will '''simulate''' for '''5 seconds''' with in a '''1e-02 time step'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''writeInterval 100;'''
|| '''Write interval''' is 100. So it will print and save every 100 '''time-step value''' that '''OpenFOAM''' solves.

So we will get '''results''' written for 1, 2, 3, 4, and 5 seconds.
|-
|| [gedit - '''controlDict'''] Highlight

'''purgeWrite 2;'''
|| '''OpenFOAM''' gives the option to save only the last few '''time steps. '''

To enable that option, you can use the '''purgeWrite''' value.

By changing it to 2, we will get the 2 latest updated '''time-step''' results.

The old files will automatically be deleted.

At the end of the '''simulation''' we will get results of 4 & 5 seconds.

This option will save''' space''' on your computer.
|-
|| Only Narration
|| The rest of the options are for the format of writing''' data''' files in '''OpenFOAM'''.

We do not need to change them.

Therefore, we won’t be making any more changes to the '''controlDict''' file.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''controlDict '''file and close the '''text editor'''.
|-
|| Only Narration
|| We are done setting up the '''case'''.

and now we will '''run''' the '''simulation'''.
|-
|| [Terminal] Type: '''icoFoam'''
|| To do so, type '''icoFoam''' in the '''terminal''' and press '''Enter'''.
|-
|| Only Narration
|| It will take some time to '''simulate,''' based on your computer’s '''hardware'''.

For me it took around 4 minutes to '''simulate'''.
|-
|| [Terminal] Highlight

'''End'''
|| Once the '''simulation''' is finished, you will get this line at the end.
|-
|| Slide: Formula and Analytical Solution

Highlight '''2.4 Pa'''

Highlight '''0.05 m/s'''

||
* To calculate''' pressure '''at''' inlet,''' let us put the values of the '''U, L, D '''and '''Po''' in this '''formula'''.

* We will get an '''inlet pressure''' value of '''2.4 Pascals'''.

* '''Maximum velocity''' will be twice of average '''velocity''' as per '''analytical solution'''.
|-
|| Slide: Result Comparison
||
* From the '''simulation''' we get,
** '''Maximum velocity''' 0.05 m/s and
** '''inlet Pressure 2.8 Pascals.'''

* In '''CFD''', there are always some deviations in results of '''analytical''' and '''numerical''' '''solutions'''.

* We will discuss '''results''' in details later in this series.

|-
|| Only Narration
|| With this we have come to the end of this tutorial.

To summarize.
|-
|| Slide: Summary

|| In this tutorial, we have learnt to,

* Set up the '''boundary''' and '''initial''' '''conditions'''
* Set up the '''physical properties'''
* Set up the '''solve & write control parameter '''and
* Run the '''simulation'''
|-
|| 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 Divyesh Variya.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Basic-Post-Processing-using-ParaView/English

2020-07-21T15:14:31Z

Divyesh7:

'''Title of the script:''' Basic Post Processing using ParaView

'''Author:''' Divyesh Variya

'''Keywords:''' OpenFOAM, Hagen Poiseuille, Paraview, Clip, Streamline, Glyph, Plot-over-line, Parabolic profile, Video-Tutorial

{| Border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Basic Post Processing using ParaView.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn,
* Some basic '''visualization techniques''' in '''ParaView'''
* Export the''' field data '''to '''.csv''' file
* Plot a''' graph''' in '''LibreOffice Suite Calc '''and
* Save a screenshot of a '''view'''

|-
|| 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
* '''LibreOffice Suite''' 6.4

|-
|| Slide: Prerequisites* Please go through these two tutorials on https://spoken-tutorial.org

|| As a prerequisite learner should practise,
* On '''Simulating Hagen Poiseuille Flow through a Pipe''' from the '''OpenFOAM '''tutorials and
* Tutorial on '''Using Charts and Graphs''' from '''LibreOffice Suite Calc'''
* Please go through these two tutorials on this website.

|-
|| Press Ctrl + Alt + T keys
|| Open the '''terminal''' by pressing the '''Ctrl''', '''Alt''' and '''T''' keys together.
|-
|| Only Narration
|| From now onwards please remember to press the '''Enter''' key after typing each '''command.'''
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| At the '''prompt''', type the following '''command''' to go to the '''run directory'''.
|-
|| [Terminal] Type:

'''cd pipe'''
|| Navigate to the '''pipe case '''folder.

We have created this in the''' “Simulating Hagen Poiseuille Flow through Pipe” '''tutorial.
|-
|| [Terminal] Type: '''paraFoam'''
|| Type '''paraFoam''' in the '''terminal''' to open the '''case''' file in '''paraView'''.
|-
|| [ParaView]

'''Uncheck >> inlet and outlet'''
|| Go to the '''properties''' panel.

Scroll down and locate the '''mesh parts''' section.

Uncheck all '''patches''' other than '''internalMesh'''.
|-
|| [ParaView] '''Click on Apply'''
|| Click on the '''Apply''' button in the '''Properties '''panel.
|-
|| [ParaView]

'''Click on Solid Color >> Click on U'''
|| Click on '''Solid Color '''available in the '''Active Variable Controls.'''

From here, we can change the fields that we want to visualize.

Select the '''U''' field with the dot, not the one with the box.
|-
|| [ParaView]

'''Click on Last Frame'''
|| From '''VCR Controls''', we can change the''' time steps''' and '''run animation''' using the '''Play''' button.

Currently we are on 0 time, which is for the '''initial field'''.

To go to the last '''time step, '''click on the '''Last Frame''' button.
|-
|| Show Picture of ICONS
|| As you can see, some '''filter''' icons are shown here.
|-
|| [ParaView]

'''Click on Stream Tracer filter'''
|| To visualize '''streamline''', click on the '''Stream tracer''' icon from '''Common and Data Analysis Filters'''.
|-
|| [ParaView]

'''Change seed type to point source'''
|| From the '''Properties''' panel we can change the '''seed type.'''

The two '''seed types''' available are:
* '''High resolution line source''' and
* '''Point Source'''

'''High resolution Line Source''' gives '''streamlines''' passing through a '''line'''.

'''Point Source''' gives '''streamlines''' passing through a '''sphere'''.

We will select '''Point Source'''.
|-
|| [ParaView]

'''Set number of points to 1000 >>'''

'''Uncheck Show Sphere checkbox'''
|| Set the '''number of points''' to '''1000''' and '''uncheck''' the '''Show Sphere''' option to hide the sphere.
|-
|| [ParaView]

'''Click on Apply'''
|| Click on the '''Apply''' button in the '''Properties''' panel.

We can see 1000 '''streamlines''' passing through 1000 random points within the sphere.
|-
|| [ParaView]

'''Click on Delete button'''
|| This way we can visualize the '''streamline'''.

Now '''Delete''' the '''Stream Tracer filter''' by clicking on the '''Delete''' button on the '''Properties''' panel.
|-
|| [ParaView] '''Click on Glyph filter'''
|| Click on the '''Glyph''' icon from '''Common and Data Analysis Filters'''.
|-
|| [ParaView]

'''Change Orientation U'''
|| Change '''Orientation Array''' to '''U '''from''' '''the '''Properties''' panel.
|-
|| [ParaView] '''Scale array U'''
|| Change '''Scale array''' to '''U '''in''' '''the '''Properties''' panel.
|-
|| [ParaView] '''Click on Apply'''
|| Click on the '''Apply''' button in the '''Properties '''panel.
|-
|| [ParaView]

'''Hide pipe.OpenFOAM'''
|| Hide '''pipe.OpenFOAM''' from the '''pipeline browser '''by clicking on the eye icon.
|-
|| [ParaView]

'''Zoom in render layout with left mouse click and drag'''
|| We can see '''Arrows''' in the direction of the '''flow'''.
|-
|| [ParaView] '''Delete Glyph filter'''
|| '''Delete''' the '''Glyph filter '''from the '''Properties''' panel.
|-
|| [ParaView] '''Click on Clip filter'''
|| Click on the '''clip''' icon from '''Common and Data Analysis Filters''' to clip the '''mesh'''.
|-
|| [ParaView]

'''Uncheck Show plane and invert'''
|| Uncheck “'''Show Plane'''” and “'''invert'''” boxes from the '''Properties '''panel.
|-
|| [ParaView] '''Click on Apply'''
|| Click on the '''Apply''' button in the '''Properties '''panel.
|-
|| Only Narration
|| This way we can clip any '''mesh''' and visualize '''internal flow'''.
|-
|| [ParaView] '''Delete Clip filter'''
|| Delete the '''Clip''' filter from the '''Properties''' panel.
|-
|| [ParaView]

'''Click on Plot Over Line Filter'''
|| Click on the “'''Plot Over Line'''” filter from '''Common and Data Analysis Filters'''.
|-
|| [ParaView]

'''Click on Y Axis'''
|| Click on '''Y Axis''' on the '''Properties''' panel and click '''Apply'''.
|-
|| [ParaView]'''Highlight '''

'''Line Chart view window'''
|| A new '''line chart window''' opens automatically with '''P''' and '''U_Magnitude''' '''graphs'''.
|-
|| [ParaView]

'''Scroll properties panel and uncheck p from series parameter'''
|| In the '''Properties''' panel, scroll down and locate the '''series parameters''' section.

Uncheck '''P''' from that.
|-
|| [ParaView] '''Highlight '''

'''Line Chart view window'''
|| We will get a '''parabolic profile''' for '''velocity''' in the graph.
|-
|| [ParaView] '''Click on Line chart view window'''

'''Press CTRL+S'''
|| Click on the '''Line Chart View''' window

And press '''Ctrl+S''' keys to save data.
|-
|| [Save File:]

'''Select file type as .csv '''

'''give name - Y-Axis'''
|| Select '''Files of type''' as '''.csv''' and give the file name '''Y(hyphen)Axis.'''
|-
|| [Save File:]

'''Click >> OK'''
|| Click on '''OK'''.

Again click on '''OK''' with default settings.
|-
|| Only Narration
|| The data is saved in a '''.csv''' file.

We can open this file in '''LibreOffice Calc''' and compare with an analytical solution.
|-
|| [ParaView]

'''Click on File >> Save Screenshot...'''
|| Now go to the '''File''' menu in the menu bar and select '''Save Screenshot.'''
|-
|| [ParaView]

'''File name - velocity'''

'''File type - .png'''
|| Give a '''File Name''' and select''' file type'''.

Here I am saving the screenshot as '''velocity''' with the '''.png''' file type.
|-
|| [ParaView] '''Click >> OK'''
|| Click on the '''OK''' button.
|-
|| [ParaView]

'''Click >> OK'''
|| The '''Save Screenshot''' option window pops up.

We can change the '''size''', '''scaling''', '''coloring''' and other image options here.

With the default values in the settings, click on the '''OK''' button.
|-
|| Only Narration
|| '''Screenshot''' of '''Parabolic curve profile''' is saved in our '''case '''directory.
|-
|| [ParaView]

'''Click on Z Axis'''
|| Go to the '''Properties''' panel.

Click on '''Z Axis''' and then click on the '''Apply''' button.
|-
|| [ParaView]

'''Uncheck U_Magnitude and check p'''
|| Then go to the '''series parameter''' section in the '''Properties''' panel.

Uncheck '''U_Magnitude''' field and check '''p field.'''
|-
|| [ParaView]

'''Press CTRL+S'''

'''Select .csv file type'''

'''Give a name - Z-Axis'''

'''Press OK'''

'''Press OK'''
|| Save this data to''' Z-Axis.csv''' file as explained earlier.
|-
|| [ParaView] '''Close ParaView'''
|| Close the '''ParaView''' window.
|-
|| '''Open File explorer'''
|| Open the '''File explorer '''from the '''taskbar'''.
|-
|| [File explorer]

'''Open >> OpenFOAM'''
|| Open the '''OpenFOAM''' directory.

Here we can see the '''username '''directory of our computer.
|-
|| [File explorer]

'''Open >> “username directory”'''
|| Now open your current '''user '''directory.

In the '''user''' directory we can see the “'''run'''” directory.
|-
|| [File explorer]

'''Open >> run'''
|| Open the “'''run'''” directory.

Our saved work is available here in the '''pipe''' directory.
|-
|| [File explorer] '''Open >> pipe '''
|| Now open the '''pipe''' directory.
|-
|| '''Only Narration'''
|| Here we can see all files including '''screenshot image''' and '''.csv files''' that we have saved.
|-
|| [File explorer]

'''Right click on >> Z-Axis.csv'''
|| Right click on '''Z-Axis.csv''' file.
|-
|| [File explorer]

'''Click on >> Open With Other Application'''
|| From the list, click on the “'''Open With Other Application'''” option.
|-
|| [File explorer]

'''Click on >> View All Application'''
|| Now click on the “'''View All Application'''” button.
|-
|| [File explorer]

'''Double click on >> LibreOffice Calc'''
|| A list of all the '''applications''' available in your computer will appear.

From this list find “'''LibreOffice Calc'''” and double click on it.
|-
|| [File explorer]

'''Click on >> OK'''
|| A “'''Text Import'''” window will open on your screen.

At the bottom right corner click on the '''OK''' button.
|-
|| Highlight '''LibreOffice suite calc'''
|| Our file is now open in '''LibreOffice Calc.'''
|-
|| [LibreOffice suite calc]

'''Highlight cells'''
|| We have

'''velocity U:0''' at '''Point:0'''

'''Velocity U:1''' at '''Point:1 '''and

'''Velocity U:2''' at '''Point:2'''.
|-
|| [LibreOffice suite calc]

'''Highlight cells'''
|| We have '''kinematic pressure p''', '''vtkValidPointMask''' and '''arc_length''' also.
|-
|| [LibreOffice suite calc]

'''Highlight cells'''
|| Necessary data to plot the graph is '''U:2''', '''Point:2''' and '''p'''.
|-
|| [LibreOffice suite calc]

Show Graphs
|| For this demonstration I have created a graph on '''z-axis''' versus '''kinematic pressure'''.

And another graph for '''z-axis''' versus '''velocity'''.
|-
|| [LibreOffice suite calc]

Show Graphs
|| And the same way I have created a '''y-axis''' versus '''velocity''' graph with a '''y-axis.csv''' file.
|-
|| Only Narration
|| Here you can also compare '''analytical '''solutions with '''OpenFoam''' solutions.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

Let us summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt,
* Some basic '''visualization techniques''' in '''ParaView'''
* Export''' field data '''to''' .csv''' file
* Plot''' graph''' in '''LibreOffice suite calc '''and
* Save screenshot of a '''view'''

|-
|| Slide: Assignment
|| As an assignment:
* Simulate the '''Hagen Poiseuille flow''' for the '''pipe''' of '''0.5 cm''' diameter with
* '''Inlet''' '''velocity''' '''0.05 m/s''' and '''outlet pressure''' '''0 Pascal''' and,
* Plot graphs of '''velocity''' and '''pressure '''in''' ParaView '''and''' LibreOffice Calc'''.

|-
|| 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 on this website
|-
|| 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 Divyesh Variya.

And this is Swetha Sridhar from IIT Bombay signing off. Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Simulating-Hagen-Poiseuille-flow-through-a-pipe-in-OpenFOAM/English

2020-07-21T12:44:31Z

Divyesh7:

'''Title of the script:''' Simulating Hagen Poiseuille flow through a pipe in OpenFOAM

'''Author:''' Divyesh Variya

'''Keywords:''' OpenFOAM, Hagen Poiseuille, Pipe flow, icoFoam, controlDict, Video-Tutorial

{| Border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Simulating Hagen Poiseuille flow through a pipe in OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn to,

* Set up the '''boundary''' and '''initial''' '''conditions'''
* Set up the '''physical properties'''
* Set up the '''solve & write control parameter '''and
* Run the '''simulation'''

|-
|| 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 '''Hagen Poiseuille flow''' and basic '''Fluid Dynamics '''concepts
* You should also be familiar with creation of a '''3D pipe Geometry''' in '''OpenFOAM'''
* If you are 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: Problem Setup
|| In this diagram, a '''section view''' of a '''3D pipe''' is shown.

This describes the '''problem statement'''.

* The '''diameter''' of the '''pipe''' is 1 centimeter and its '''length''' is 30 centimeters.
* It has one '''inlet''', one '''outlet''' and a '''cylindrical''' '''wall'''.

* The fluid here is water''' '''and its '''kinematic viscosity''' is taken as '''1e-06'''.

* The '''Inlet velocity '''is '''0.025 m/s '''and''' Outlet pressure '''is''' 0 Pascals '''as shown in the diagram.

|-
|| Slide: Geometry Check

Highlight '''250'''

Highlight''' laminar'''

Only Narration

Le = 0.06*Re*D

Highlight''' 0.15 m'''

|| Let us check whether our '''geometry''' is suitable or not.

* '''Reynolds number''' of the problem is '''250'''.

* Hence, the flow is '''laminar'''.

* For '''fully developed flow''', length of the '''geometry''' should be greater than the '''Entrance length'''.

* '''Entrance length''' can be calculated by this '''formula'''.

* The length we have taken is greater than the '''entrance length'''.
|-
|| Slide: Solver detail
||
* To simulate this problem, we will use the '''icoFoam''' solver.

* '''icoFoam''' is a''' transient solver''' for '''incompressible''', '''laminar flow''' of '''Newtonian fluids'''.

* This is the most '''suitable solver''' for '''Hagen Poiseuille flow.'''

|-
|| Slide : Pressure Boundary Condition
|| The''' Pressure boundary conditions''' used are,

* At '''inlet - zero gradient'''
* At '''outlet - fixed Pressure'''
* At '''wall - zero gradient'''

|-
|| Slide: Velocity Boundary Condition
|| The''' Velocity boundary condition''' used are,

* At '''inlet - fixed value'''
* At '''outlet - zero Gradient''' and
* At '''wall - No Slip'''

|-
|| Only Narration
|| We will use the '''mesh''' that we have created in the tutorial “'''Creating 3D Pipe Geometry and Mesh in OpenFoam'''”.
|-
|| Press Ctrl + Alt + T keys
|| Open the '''terminal''' by pressing the '''Ctrl''', '''Alt''' and '''T''' keys together.
|-
|| [Terminal]

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

'''cd $FOAM_RUN'''
|| At the '''prompt''', type the following '''command''' to go to the '''run directory'''.

|-
|| [Terminal] Type:

'''cd pipe'''
|| Navigate to the '''pipe case folder'''.

|-
|| [Terminal] Type:

'''mv 0.Orig 0'''
|| Now, '''rename''' '''0.Orig''' folder to''' 0''' by typing this '''command'''.

|-
|| [Terminal] Type: '''gedit 0/p'''
|| Let’s open the “'''p'''” file in a '''text editor'''.
|-
|| [gedit - '''p'''] Highlight

'''dimensions [0 2 -2 0 0 0 0];'''
|| Here we can see, the '''p''' file is in the form of '''pressure divided by density'''.

This means, it is '''kinematic pressure'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''internalField''' to the end of the file as shown here.
|-
|| [gedit - '''pressure''']
|| Open the file '''pressure.txt''', that you had downloaded in any '''text editor'''.
|-
|| [gedit - '''pressure'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''p''']
|| Now let me switch back to the “'''p”''' file.
|-
|| [gedit - '''p'''] '''Paste '''
|| Paste the copied contents into the “'''p” '''file as shown here.
|-
|| [gedit - '''p'''] Highlight

'''internalField'''
|| Right after '''dimensions''', we have to define the '''initial condition'''.

It could be '''uniform''', '''non-uniform''' or in the form of '''code'''.
|-
|| [gedit - '''p'''] Highlight

'''uniform 0;'''
|| In this case, we will use the '''initial condition''' as''' uniform 0'''.

This means that the '''kinematic pressure''' inside the entire '''domain''' is '''0'''.
|-
|| [gedit - '''p'''] Highlight

'''boundaryField'''
|| In the '''boundaryField''', we specify '''boundary conditions''' for all '''patches''' and '''walls'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| '''Boundary condition''' for '''inlet''' in '''pressure''' is defined as shown.
|-
|| [gedit - '''p'''] Highlight

'''type zeroGradient;'''
|| Type of the '''boundary condition''' is '''zeroGradient'''.

'''Zero Gradient boundary '''extrapolates the quantity to the '''patch''' from the nearest '''cell value'''.

So, the value at the '''patch''' will be the same as the '''cell value'''.

Note that '''z''' is small and '''G''' is capital.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> wall'''
|| '''Boundary condition''' for the '''wall''' is defined as the same as '''inlet'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> outlet'''
|| '''Boundary condition''' for '''outlet''' in '''pressure''' is defined as shown here.
|-
|| [gedit - '''p'''] Highlight

'''type fixedValue;'''

'''value 0;'''
|| The type of '''boundary condition''' is '''fixedValue'''.

'''Value''' given is '''zero'''.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''p '''file and close the '''text editor'''.
|-
|| [Terminal] Type:

'''gedit 0/U'''
|| Now, let us set the '''initial''' and '''boundary condition''' for '''velocity'''.

To do so, open the '''U''' file in a '''text editor'''.
|-
|| [gedit - '''U'''] Highlight

'''dimensions [0 1 -1 0 0 0 0];'''
|| '''Dimensions''' here are in '''meters per second'''.
|-
|| [gedit - '''U'''] Highlight

'''internalField uniform (0 0 0);'''
|| '''Velocity''' is a '''vector field''', so the '''internal initial field''' is set as '''uniform (0 0 0)'''.
|-
|| [gedit - '''U'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''boundaryField''' to the end of the file as shown here.
|-
|| [gedit - '''velocity''']
|| Open the '''velocity.txt '''file that you had downloaded in a '''text editor'''.
|-
|| [gedit - '''velocity'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''U'''] '''Paste '''
|| Paste the copied contents into the “'''U” '''file as shown.
|-
|| [gedit - '''U'''] Highlight

'''boundaryField'''
|| In the '''boundaryField''', we will specify '''boundary conditions''' for all '''patches''' and '''walls'''.
|-
|| [gedit - '''U'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| '''Boundary condition''' for '''inlet''' in '''velocity''' is defined as shown here.
|-
|| [gedit - '''U'''] Highlight

'''type fixedValue;'''

'''value uniform (0 0 0.025);'''
|| Type of the '''boundary condition''' is '''fixedValue'''.

Value of '''velocity''' is 0.025 m/s in the '''Z direction'''.
|-
|| [gedit - '''U'''] Highlight

'''type noSlip;'''
|| '''Boundary condition''' for the '''wall''' is defined as '''noSlip'''.

This means '''velocity''' at the '''wall '''is '''0'''.
|-
|| [gedit - '''U'''] Highlight

'''type zeroGradient;'''
|| '''Boundary condition''' for '''outlet''' is '''zeroGradient''', defined as shown here.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''U '''file and close the '''text editor.'''
|-
|| [Terminal] Type:

'''gedit constant/transportProperties'''
|| Open '''transport properties''' file from '''constant folder''' in the '''text editor'''.
|-
|| [gedit - '''transportProperties'''] Highlight

'''nu'''
|| All '''properties''' of '''fluid''' which remain '''constant''' during the '''simulation''' is to be specified in the '''constant folder'''.

Here, we will set the value of '''kinematic viscosity'''.
|-
|| [gedit - '''transportProperties'''] Highlight

'''[0 2 -1 0 0 0 0]'''
|| Dimensions of '''kinematic viscosity''' are specified here.
|-
|| [gedit - '''transportProperties''']

'''Change: 0.01 >> 1e-06'''
|| To set the value of '''nu,''' replace '''0.01''' to '''1e-06'''.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''transportProperties '''file and close the '''text editor.'''
|-
|| Only Narration
|| '''Solve & write control parameters''' can be modified in the '''controlDict''' file.

The '''controlDict '''file is located in the '''system folder'''.
|-
|| [Terminal] Type:

'''gedit system/controlDict'''
|| Open the '''controlDict''' file in a '''text editor'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''application''' to the end of the file as shown here.
|-
|| [gedit - '''control''']
|| Open the '''control.txt''' file that you had downloaded in a '''text editor'''.
|-
|| [gedit - '''control'''] Highlight

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

|| and paste the copied contents into the “'''controlDict” '''file as shown here.
|-
|| [gedit - '''controlDict'''] Highlight

'''application icoFoam;'''
|| First line of the '''controlDict''' file shows the name of the '''solver'''.

In our case it is '''icoFoam'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''startFrom startTime;'''

'''startTime 0;'''
|| The second and third lines are '''start simulation controls'''.

Our '''simulation''' will start from the value specified in '''start time'''.

Here our '''start time''' is set to '''0'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''stopAt endTime;'''

'''endTime 5;'''
|| The fourth and fifth lines are '''stop simulation controls'''.

'''Simulation''' will stop at the''' endTime''' of '''5 seconds'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''deltaT 1e-2;'''
|| Then the value of '''deltaT''' is given, which is '''1e-02'''.

So, it will '''simulate''' for '''5 seconds''' with in a '''1e-02 time step'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''writeInterval 100;'''
|| '''Write interval''' is 100. So it will print and save every 100 '''time-step value''' that '''OpenFOAM''' solves.

So we will get '''results''' written for 1, 2, 3, 4, and 5 seconds.
|-
|| [gedit - '''controlDict'''] Highlight

'''purgeWrite 2;'''
|| '''OpenFOAM''' gives the option to save only the last few '''time steps. '''

To enable that option, you can use the '''purgeWrite''' value.

By changing it to 2, we will get the 2 latest updated '''time-step''' results.

The old files will automatically be deleted.

At the end of the '''simulation''' we will get results of 4 & 5 seconds.

This option will save''' space''' on your computer.
|-
|| Only Narration
|| The rest of the options are for the format of writing''' data''' files in '''OpenFOAM'''.

We do not need to change them.

Therefore, we won’t be making any more changes to the '''controlDict''' file.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''controlDict '''file and close the '''text editor'''.
|-
|| Only Narration
|| We are done setting up the '''case'''.

and now we will '''run''' the '''simulation'''.
|-
|| [Terminal] Type: '''icoFoam'''
|| To do so, type '''icoFoam''' in the '''terminal''' and press '''Enter'''.
|-
|| Only Narration
|| It will take some time to '''simulate,''' based on your computer’s '''hardware'''.

For me it took around 4 minutes to '''simulate'''.
|-
|| [Terminal] Highlight

'''End'''
|| Once the '''simulation''' is finished, you will get this line at the end.
|-
|| Slide: Formula and Analytical Solution

Highlight '''2.4 Pa'''

Highlight '''0.05 m/s'''

||
* To calculate''' pressure '''at''' inlet,''' let us put the values of the '''U, L, D '''and '''Po''' in this '''formula'''.

* We will get an '''inlet pressure''' value of '''2.4 Pascal'''.

* '''Maximum velocity''' will be twice of average '''velocity''' as per '''analytical solution'''.
|-
|| Slide: Result Comparison
||
* From the '''simulation''' we get,
** '''Maximum velocity''' 0.05 m/s and
** '''inlet Pressure 2.8 Pascals.'''

* In '''CFD''', there are always some deviations in results of '''analytical''' and '''numerical''' '''solutions'''.

* We will discuss '''results''' in details later in this series.

|-
|| 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 the '''boundary''' and '''initial''' '''conditions'''
* Set up the '''physical properties'''
* Set up the '''solve & write control parameter '''and
* Run the '''simulation'''
|-
|| 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 Divyesh Variya.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Simulating-Hagen-Poiseuille-flow-through-a-pipe-in-OpenFOAM/English

2020-07-21T12:16:58Z

Divyesh7:

'''Title of the script:''' Simulating Hagen Poiseuille flow through a pipe in OpenFOAM

'''Author:''' Divyesh Variya

'''Keywords:''' OpenFOAM, Hagen Poiseuille, Pipe flow, icoFoam, controlDict, Video-Tutorial

{| Border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Simulating Hagen Poiseuille flow through a pipe in OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn to,

* Set up the '''boundary''' and '''initial''' '''conditions'''
* Set up the '''physical properties'''
* Set up the '''solve & write control parameter '''and
* Run the '''simulation'''

|-
|| 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 '''Hagen Poiseuille flow''' and basic '''Fluid Dynamics '''concepts
* You should also be familiar with creation of a '''3D pipe Geometry''' in '''OpenFOAM'''
* If you are 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: Problem Setup
|| In this diagram, a '''section view''' of a '''3D pipe''' is shown.

This describes the '''problem statement'''.

* The '''diameter''' of the '''pipe''' is 1 centimeter and its '''length''' is 30 centimeters.
* It has one '''inlet''', one '''outlet''' and a '''cylindrical''' '''wall'''.

* The fluid here is water''' '''and its '''kinematic viscosity''' is taken as '''1e-06'''.

* The '''Inlet velocity '''is '''0.025 m/s '''and''' Outlet pressure '''is''' 0 Pascals '''as shown in the diagram.

|-
|| Slide: Geometry Check

Highlight '''250'''

Highlight''' laminar'''

Only Narration

Le = 0.06*Re*D

Highlight''' 0.15 m'''

|| Let us check whether our '''geometry''' is suitable or not.

* '''Reynolds number''' of the problem is '''250'''.

* Hence, the flow is '''laminar'''.

* For '''fully developed flow''', length of the '''geometry''' should be greater than the '''Entrance length'''.

* '''Entrance length''' can be calculated by this '''formula'''.

* The length we have taken is greater than the '''entrance length'''.
|-
|| Slide: Solver detail
||
* To simulate this problem, we will use the '''icoFoam''' solver.

* '''icoFoam''' is a''' transient solver''' for '''incompressible''', '''laminar flow''' of '''Newtonian fluids'''.

* This is the most '''suitable solver''' for '''Hagen Poiseuille flow.'''

|-
|| Slide : Pressure Boundary Condition
|| The''' Pressure boundary conditions''' used are,

* At '''inlet - zero gradient'''
* At '''outlet - fixed Pressure'''
* At '''wall - zero gradient'''

|-
|| Slide: Velocity Boundary Condition
|| The''' Velocity boundary condition''' used are,

* At '''inlet - fixed value'''
* At '''outlet - zero Gradient''' and
* At '''wall - No Slip'''

|-
|| Only Narration
|| We will use the '''mesh''' that we have created in the tutorial “'''Creating 3D Pipe Geometry and Mesh in OpenFoam'''”.
|-
|| Press Ctrl + Alt + T keys
|| Open the '''terminal''' by pressing the '''Ctrl''', '''Alt''' and '''T''' keys together.
|-
|| [Terminal]

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

'''cd $FOAM_RUN'''
|| At the '''prompt''', type the following '''command''' to go to the '''run directory'''.

|-
|| [Terminal] Type:

'''cd pipe'''
|| Navigate to the '''pipe case folder'''.

|-
|| [Terminal] Type:

'''mv 0.Orig 0'''
|| Now, '''rename''' '''0.Orig''' folder to''' 0''' by typing this '''command'''.

|-
|| [Terminal] Type: '''gedit 0/p'''
|| Let’s open the “'''p'''” file in a '''text editor'''.
|-
|| [gedit - '''p'''] Highlight

'''dimensions [0 2 -2 0 0 0 0];'''
|| Here we can see, the '''p''' file is in the form of '''pressure divided by density'''.

This means, it is '''kinematic pressure'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''internalField''' to the end of the file as shown here.
|-
|| [gedit - '''pressure''']
|| Open the file '''pressure.txt''', that you had downloaded in any '''text editor'''.
|-
|| [gedit - '''pressure'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''p''']
|| Now let me switch back to the “'''p”''' file.
|-
|| [gedit - '''p'''] '''Paste '''
|| Paste the copied contents into the “'''p” '''file as shown here.
|-
|| [gedit - '''p'''] Highlight

'''internalField'''
|| Right after '''dimensions''', we have to define the '''initial condition'''.

It could be '''uniform''', '''non-uniform''' or in the form of '''code'''.
|-
|| [gedit - '''p'''] Highlight

'''uniform 0;'''
|| In this case, we will use the '''initial condition''' as''' uniform 0'''.

This means that the '''kinematic pressure''' inside the entire '''domain''' is '''0'''.
|-
|| [gedit - '''p'''] Highlight

'''boundaryField'''
|| In the '''boundaryField''', we specify '''boundary conditions''' for all '''patches''' and '''walls'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| '''Boundary condition''' for '''inlet''' in '''pressure''' is defined as shown.
|-
|| [gedit - '''p'''] Highlight

'''type zeroGradient;'''
|| Type of the '''boundary condition''' is '''zeroGradient'''.

'''Zero Gradient boundary '''extrapolates the quantity to the '''patch''' from the nearest '''cell value'''.

So, the value at '''patch''' will be the same as the '''cell value'''.

Note that '''z''' is small and '''G''' is capital.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> wall'''
|| '''Boundary condition''' for the '''wall''' is defined as the same as '''inlet'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> outlet'''
|| '''Boundary condition''' for '''outlet''' in '''pressure''' is defined as shown here.
|-
|| [gedit - '''p'''] Highlight

'''type fixedValue;'''

'''value 0;'''
|| Type of '''boundary condition''' is '''fixedValue'''.

'''Value''' given is '''zero'''.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''p '''file and close the '''text editor'''.
|-
|| [Terminal] Type:

'''gedit 0/U'''
|| Now, let’s set the '''initial''' and '''boundary condition''' for '''velocity'''.

To do so, open the '''U''' file in a '''text editor'''.
|-
|| [gedit - '''U'''] Highlight

'''dimensions [0 1 -1 0 0 0 0];'''
|| '''Dimensions''' here are in '''meters per second'''.
|-
|| [gedit - '''U'''] Highlight

'''internalField uniform (0 0 0);'''
|| '''Velocity''' is a '''vector field''', so the '''internal initial field''' is set as '''uniform (0 0 0)'''.
|-
|| [gedit - '''U'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''boundaryField''' to the end of the file as shown here.
|-
|| [gedit - '''velocity''']
|| Open the '''velocity.txt '''file that you had downloaded in a '''text editor'''.
|-
|| [gedit - '''velocity'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''U'''] '''Paste '''
|| Paste the copied contents into the “'''U” '''file as shown.
|-
|| [gedit - '''U'''] Highlight

'''boundaryField'''
|| In the '''boundaryField''', we will specify '''boundary conditions''' for all '''patches''' and '''walls'''.
|-
|| [gedit - '''U'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| '''Boundary condition''' for '''inlet''' in '''velocity''' is defined as shown here.
|-
|| [gedit - '''U'''] Highlight

'''type fixedValue;'''

'''value uniform (0 0 0.025);'''
|| Type of the '''boundary condition''' is '''fixedValue'''.

Value of '''velocity''' is 0.025 m/s in the '''Z direction'''.
|-
|| [gedit - '''U'''] Highlight

'''type noSlip;'''
|| '''Boundary condition''' for the '''wall''' is defined as '''noSlip'''.

This means '''velocity''' at the '''wall '''is '''0'''.
|-
|| [gedit - '''U'''] Highlight

'''type zeroGradient;'''
|| '''Boundary condition''' for '''outlet''' is '''zeroGradient''', defined as shown here.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''U '''file and close the '''text editor.'''
|-
|| [Terminal] Type:

'''gedit constant/transportProperties'''
|| Open '''transport properties''' file from '''constant folder''' in the '''text editor'''.
|-
|| [gedit - '''transportProperties'''] Highlight

'''nu'''
|| All '''properties''' of '''fluid''' which remain '''constant''' during the '''simulation''' is to be specified in the '''constant folder'''.

Here, we will set the value of '''kinematic viscosity'''.
|-
|| [gedit - '''transportProperties'''] Highlight

'''[0 2 -1 0 0 0 0]'''
|| Dimensions of '''kinematic viscosity''' are specified here.
|-
|| [gedit - '''transportProperties''']

'''Change: 0.01 >> 1e-06'''
|| To set the value of '''nu,''' replace '''0.01''' to '''1e-06'''.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''transportProperties '''file and close the '''text editor.'''
|-
|| Only Narration
|| '''Solve & write control parameters''' can be modified in the '''controlDict''' file.

The '''controlDict '''file is located in the '''system folder'''.
|-
|| [Terminal] Type:

'''gedit system/controlDict'''
|| Open the '''controlDict''' file in a '''text editor'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''application''' to the end of the file as shown here.
|-
|| [gedit - '''control''']
|| Open the '''control.txt''' file that you had downloaded in a '''text editor'''.
|-
|| [gedit - '''control'''] Highlight

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

|| Paste the copied contents into the “'''controlDict” '''file as shown here.
|-
|| [gedit - '''controlDict'''] Highlight

'''application icoFoam;'''
|| First line of the '''controlDict''' file shows the name of the '''solver'''.

In our case it is '''icoFoam'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''startFrom startTime;'''

'''startTime 0;'''
|| The second and third lines are '''start simulation controls'''.

Our '''simulation''' will start from the value specified in '''start time'''.

Here our '''start time''' is set to '''0'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''stopAt endTime;'''

'''endTime 5;'''
|| The fourth and fifth lines are '''stop simulation controls'''.

'''Simulation''' will stop at the''' endTime''' of '''5 seconds'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''deltaT 1e-2;'''
|| Then the value of '''deltaT''' is given, which is '''1e-02'''.

So, it will '''simulate''' for '''5 seconds''' with a '''1e-02 time step'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''writeInterval 100;'''
|| '''Write interval''' is 100. So it will print and save every 100 '''time-step value''' that '''OpenFOAM''' solves.

So we will get '''results''' written for 1, 2, 3, 4, and 5 seconds.
|-
|| [gedit - '''controlDict'''] Highlight

'''purgeWrite 2;'''
|| '''OpenFOAM''' gives the option to save only the last few '''time steps. '''

To enable that option, you can use the '''purgeWrite''' value.

By changing it to 2, we will get the 2 latest updated '''time-step''' results.

The old files will automatically be deleted.

At the end of the '''simulation''' we will get results of 4 & 5 seconds.

This option will save''' space''' on your computer.
|-
|| Only Narration
|| Rest of the options are for the format of writing''' data''' files in '''OpenFOAM'''.

We do not need to change them.

Therefore, we won’t be making any more changes to the '''controlDict''' file.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''controlDict '''file and close the '''text editor'''.
|-
|| Only Narration
|| We are done setting up the '''case'''.

Now we will '''run''' the '''simulation'''.
|-
|| [Terminal] Type: '''icoFoam'''
|| To do so, type '''icoFoam''' in the '''terminal''' and press '''Enter'''.
|-
|| Only Narration
|| It will take some time to '''simulate,''' based on your computer’s '''hardware'''.

For me it took around 4 minutes to '''simulate'''.
|-
|| [Terminal] Highlight

'''End'''
|| Once the '''simulation''' is finished, you will get this line at the end.
|-
|| Slide: Formula and Analytical Solution

Highlight '''2.4 Pa'''

Highlight '''0.05 m/s'''

||
* To calculate''' pressure '''at''' inlet,''' let’s put the values of the '''U, L, D '''and '''Po''' in this '''formula'''.

* We will get an '''inlet pressure''' value of '''2.4 Pascal'''.

* '''Maximum velocity''' will be twice of average '''velocity''' as per '''analytical solution'''.
|-
|| Slide: Result Comparison
||
* From the '''simulation''' we get,
** '''Maximum velocity''' 0.05 m/s and
** '''inlet Pressure 2.8 Pascals.'''

* In '''CFD''', there are always some deviations in results of '''analytical''' and '''numerical''' '''solutions'''.

* We will discuss '''results''' in detail later in this series.

|-
|| 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 the '''boundary''' and '''initial''' '''conditions'''
* Set up the '''physical properties'''
* Set up the '''solve & write control parameter '''and
* Run the '''simulation'''
|-
|| 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 Divyesh Variya.

And this is Swetha Sridhar from IIT Bombay signing off.

Thanks for joining.
|-
|}

OpenFOAM-version-7/C2/Simulating-Hagen-Poiseuille-flow-through-a-pipe-in-OpenFOAM/English

2020-07-21T12:14:50Z

Divyesh7:

'''Title of the script:''' Simulating Hagen Poiseuille flow through a pipe in OpenFOAM

'''Author:''' Divyesh Variya

'''Keywords:''' OpenFOAM, Hagen Poiseuille, Pipe flow, icoFoam, controlDict, Video-Tutorial

{| Border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Simulating Hagen Poiseuille flow through a pipe in OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn to,

* Set up the '''boundary''' and '''initial''' '''conditions'''
* Set up the '''physical properties'''
* Set up the '''solve & write control parameter '''and
* Run the '''simulation'''

|-
|| 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 '''Hagen Poiseuille flow''' and basic '''Fluid Dynamics '''concepts
* You should also be familiar with creation of a '''3D pipe Geometry''' in '''OpenFOAM'''
* If you are 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: Problem Setup
|| In this diagram, a '''section view''' of a '''3D pipe''' is shown.

This describes the '''problem statement'''.

* The '''diameter''' of the '''pipe''' is 1 centimeter and its '''length''' is 30 centimeters.
* It has one '''inlet''', one '''outlet''' and a '''cylindrical''' '''wall'''.

* The fluid here is water''' '''and its '''kinematic viscosity''' is taken as '''1e-06'''.

* The '''Inlet velocity '''is '''0.025 m/s '''and''' Outlet pressure '''is''' 0 Pascals '''as shown in the diagram.

|-
|| Slide: Geometry Check

Highlight '''250'''

Highlight''' laminar'''

Only Narration

Le = 0.06*Re*D

Highlight''' 0.15 m'''

|| Let us check whether our '''geometry''' is suitable or not.

* '''Reynolds number''' of the problem is '''250'''.

* Hence, the flow is '''laminar'''.

* For '''fully developed flow''', length of the '''geometry''' should be greater than the '''Entrance length'''.

* '''Entrance length''' can be calculated by this '''formula'''.

* The length we have taken is greater than the '''entrance length'''.
|-
|| Slide: Solver detail
||
* To simulate this problem, we will use the '''icoFoam''' solver.

* '''icoFoam''' is a''' transient solver''' for '''incompressible''', '''laminar flow''' of '''Newtonian fluids'''.

* This is the most '''suitable solver''' for '''Hagen Poiseuille flow.'''

|-
|| Slide : Pressure Boundary Condition
|| The''' Pressure boundary conditions''' used are,

* At '''inlet - zero gradient'''
* At '''outlet - fixed Pressure'''
* At '''wall - zero gradient'''

|-
|| Slide: Velocity Boundary Condition
|| The''' Velocity boundary condition''' used are,

* At '''inlet - fixed value'''
* At '''outlet - zero Gradient''' and
* At '''wall - No Slip'''

|-
|| Only Narration
|| We will use the '''mesh''' that we have created in the tutorial “'''Creating 3D Pipe Geometry and Mesh in OpenFoam'''”.
|-
|| Press Ctrl + Alt + T keys
|| Open the '''terminal''' by pressing the '''Ctrl''', '''Alt''' and '''T''' keys together.
|-
|| [Terminal]

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

'''cd $FOAM_RUN'''
|| At the '''prompt''', type the following '''command''' to go to the '''run directory'''.

|-
|| [Terminal] Type:

'''cd pipe'''
|| Navigate to the '''pipe case folder'''.

|-
|| [Terminal] Type:

'''mv 0.Orig 0'''
|| Now, '''rename''' '''0.Orig''' folder to''' 0''' by typing this '''command'''.

|-
|| [Terminal] Type: '''gedit 0/p'''
|| Let’s open the “'''p'''” file in a '''text editor'''.
|-
|| [gedit - '''p'''] Highlight

'''dimensions [0 2 -2 0 0 0 0];'''
|| Here we can see, the '''p''' file is in the form of '''pressure divided by density'''.

This means, it is '''kinematic pressure'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''internalField''' to the end of the file as shown here.
|-
|| [gedit - '''pressure''']
|| Open the file '''pressure.txt''', that you had downloaded in any '''text editor'''.
|-
|| [gedit - '''pressure'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''p''']
|| Let me switch back to the “'''p”''' file.
|-
|| [gedit - '''p'''] '''Paste '''
|| Paste the copied contents into the “'''p” '''file as shown here.
|-
|| [gedit - '''p'''] Highlight

'''internalField'''
|| Right after '''dimensions''', we have to define the '''initial condition'''.

It could be '''uniform''', '''non-uniform''' or in the form of '''code'''.
|-
|| [gedit - '''p'''] Highlight

'''uniform 0;'''
|| In this case, we will use the '''initial condition''' as''' uniform 0'''.

This means that the '''kinematic pressure''' inside the entire '''domain''' is '''0'''.
|-
|| [gedit - '''p'''] Highlight

'''boundaryField'''
|| In the '''boundaryField''', we specify '''boundary conditions''' for all '''patches''' and '''walls'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| '''Boundary condition''' for '''inlet''' in '''pressure''' is defined as shown.
|-
|| [gedit - '''p'''] Highlight

'''type zeroGradient;'''
|| Type of the '''boundary condition''' is '''zeroGradient'''.

'''Zero Gradient boundary '''extrapolates the quantity to the '''patch''' from the nearest '''cell value'''.

So, the value at '''patch''' will be the same as the '''cell value'''.

Note that '''z''' is small and '''G''' is capital.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> wall'''
|| '''Boundary condition''' for the '''wall''' is defined as the same as '''inlet'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> outlet'''
|| '''Boundary condition''' for '''outlet''' in '''pressure''' is defined as shown here.
|-
|| [gedit - '''p'''] Highlight

'''type fixedValue;'''

'''value 0;'''
|| Type of '''boundary condition''' is '''fixedValue'''.

'''Value''' given is '''zero'''.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''p '''file and close the '''text editor'''.
|-
|| [Terminal] Type:

'''gedit 0/U'''
|| Now, let’s set the '''initial''' and '''boundary condition''' for '''velocity'''.

To do so, open the '''U''' file in a '''text editor'''.
|-
|| [gedit - '''U'''] Highlight

'''dimensions [0 1 -1 0 0 0 0];'''
|| '''Dimensions''' here are in '''meters per second'''.
|-
|| [gedit - '''U'''] Highlight

'''internalField uniform (0 0 0);'''
|| '''Velocity''' is a '''vector field''', so the '''internal initial field''' is set as '''uniform (0 0 0)'''.
|-
|| [gedit - '''U'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''boundaryField''' to the end of the file as shown here.
|-
|| [gedit - '''velocity''']
|| Open the '''velocity.txt '''file that you had downloaded in a '''text editor'''.
|-
|| [gedit - '''velocity'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''U'''] '''Paste '''
|| Paste the copied contents into the “'''U” '''file as shown.
|-
|| [gedit - '''U'''] Highlight

'''boundaryField'''
|| In the '''boundaryField''', we will specify '''boundary conditions''' for all '''patches''' and '''walls'''.
|-
|| [gedit - '''U'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| '''Boundary condition''' for '''inlet''' in '''velocity''' is defined as shown here.
|-
|| [gedit - '''U'''] Highlight

'''type fixedValue;'''

'''value uniform (0 0 0.025);'''
|| Type of the '''boundary condition''' is '''fixedValue'''.

Value of '''velocity''' is 0.025 m/s in the '''Z direction'''.
|-
|| [gedit - '''U'''] Highlight

'''type noSlip;'''
|| '''Boundary condition''' for the '''wall''' is defined as '''noSlip'''.

This means '''velocity''' at the '''wall '''is '''0'''.
|-
|| [gedit - '''U'''] Highlight

'''type zeroGradient;'''
|| '''Boundary condition''' for '''outlet''' is '''zeroGradient''', defined as shown here.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''U '''file and close the '''text editor.'''
|-
|| [Terminal] Type:

'''gedit constant/transportProperties'''
|| Open '''transport properties''' file from '''constant folder''' in the '''text editor'''.
|-
|| [gedit - '''transportProperties'''] Highlight

'''nu'''
|| All '''properties''' of '''fluid''' which remain '''constant''' during the '''simulation''' is to be specified in the '''constant folder'''.

Here, we will set the value of '''kinematic viscosity'''.
|-
|| [gedit - '''transportProperties'''] Highlight

'''[0 2 -1 0 0 0 0]'''
|| Dimensions of '''kinematic viscosity''' are specified here.
|-
|| [gedit - '''transportProperties''']

'''Change: 0.01 >> 1e-06'''
|| To set the value of '''nu,''' replace '''0.01''' to '''1e-06'''.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''transportProperties '''file and close the '''text editor.'''
|-
|| Only Narration
|| '''Solve & write control parameters''' can be modified in the '''controlDict''' file.

The '''controlDict '''file is located in the '''system folder'''.
|-
|| [Terminal] Type:

'''gedit system/controlDict'''
|| Open the '''controlDict''' file in a '''text editor'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''application''' to the end of the file as shown here.
|-
|| [gedit - '''control''']
|| Open the '''control.txt''' file that you had downloaded in a '''text editor'''.
|-
|| [gedit - '''control'''] Highlight

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

|| Paste the copied contents into the “'''controlDict” '''file as shown here.
|-
|| [gedit - '''controlDict'''] Highlight

'''application icoFoam;'''
|| First line of the '''controlDict''' file shows the name of the '''solver'''.

In our case it is '''icoFoam'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''startFrom startTime;'''

'''startTime 0;'''
|| The second and third lines are '''start simulation controls'''.

Our '''simulation''' will start from the value specified in '''start time'''.

Here our '''start time''' is set to '''0'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''stopAt endTime;'''

'''endTime 5;'''
|| The fourth and fifth lines are '''stop simulation controls'''.

'''Simulation''' will stop at the''' endTime''' of '''5 seconds'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''deltaT 1e-2;'''
|| Then the value of '''deltaT''' is given, which is '''1e-02'''.

So, it will '''simulate''' for '''5 seconds''' with a '''1e-02 time step'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''writeInterval 100;'''
|| '''Write interval''' is 100. So it will print and save every 100 '''time-step value''' that '''OpenFOAM''' solves.

So we will get '''results''' written for 1, 2, 3, 4, and 5 seconds.
|-
|| [gedit - '''controlDict'''] Highlight

'''purgeWrite 2;'''
|| '''OpenFOAM''' gives the option to save only the last few '''time steps. '''

To enable that option, you can use the '''purgeWrite''' value.

By changing it to 2, we will get the 2 latest updated '''time-step''' results.

The old files will automatically be deleted.

At the end of the '''simulation''' we will get results of 4 & 5 seconds.

This option will save''' space''' on your computer.
|-
|| Only Narration
|| Rest of the options are for the format of writing''' data''' files in '''OpenFOAM'''.

We do not need to change them.

Therefore, we won’t be making any more changes to the '''controlDict''' file.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''controlDict '''file and close the '''text editor'''.
|-
|| Only Narration
|| We are done setting up the '''case'''.

Now we will '''run''' the '''simulation'''.
|-
|| [Terminal] Type: '''icoFoam'''
|| To do so, type '''icoFoam''' in the '''terminal''' and press '''Enter'''.
|-
|| Only Narration
|| It will take some time to '''simulate,''' based on your computer’s '''hardware'''.

For me it took around 4 minutes to '''simulate'''.
|-
|| [Terminal] Highlight

'''End'''
|| Once the '''simulation''' is finished, you will get this line at the end.
|-
|| Slide: Formula and Analytical Solution

Highlight '''2.4 Pa'''

Highlight '''0.05 m/s'''

||
* To calculate''' pressure '''at''' inlet,''' let’s put the values of the '''U, L, D '''and '''Po''' in this '''formula'''.

* We will get an '''inlet pressure''' value of '''2.4 Pascal'''.

* '''Maximum velocity''' will be twice of average '''velocity''' as per '''analytical solution'''.
|-
|| Slide: Result Comparison
||
* From the '''simulation''' we get,
** '''Maximum velocity''' 0.05 m/s and
** '''inlet Pressure 2.8 Pascals.'''

* In '''CFD''', there are always some deviations in results of '''analytical''' and '''numerical''' '''solutions'''.

* We will discuss '''results''' in detail later in this series.

|-
|| 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 the '''boundary''' and '''initial''' '''conditions'''
* Set up the '''physical properties'''
* Set up the '''solve & write control parameter '''and
* Run the '''simulation'''
|-
|| 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 Divyesh Variya.

And this is Swetha Sridhar from IIT Bombay signing off.

Thanks for joining.
|-
|}

OpenFOAM-version-7/C2/Simulating-Hagen-Poiseuille-flow-through-a-pipe-in-OpenFOAM/English

2020-07-21T12:13:02Z

Divyesh7:

'''Title of the script:''' Simulating Hagen Poiseuille flow through a pipe in OpenFOAM

'''Author:''' Divyesh Variya

'''Keywords:''' OpenFOAM, Hagen Poiseuille, Pipe flow, icoFoam, controlDict, Video-Tutorial

{| Border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Simulating Hagen Poiseuille flow through a pipe in OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn to,

* Set up the '''boundary''' and '''initial''' '''conditions'''
* Set up the '''physical properties'''
* Set up the '''solve & write control parameter '''and
* Run the '''simulation'''

|-
|| 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 '''Hagen Poiseuille flow''' and basic '''Fluid Dynamics '''concepts
* You should also be familiar with creation of a '''3D pipe Geometry''' in '''OpenFOAM'''
* If you are 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: Problem Setup
|| In this diagram, a '''section view''' of a '''3D pipe''' is shown.

This describes the '''problem statement'''.

* The '''diameter''' of the '''pipe''' is 1 centimeter and its '''length''' is 30 centimeters.
* It has one '''inlet''', one '''outlet''' and a '''cylindrical''' '''wall'''.

* The fluid here is water''' '''and its '''kinematic viscosity''' is taken as '''1e-06'''.

* The '''Inlet velocity '''is '''0.025 m/s '''and''' Outlet pressure '''is''' 0 Pascals '''as shown in the diagram.

|-
|| Slide: Geometry Check

Highlight '''250'''

Highlight''' laminar'''

Only Narration

Le = 0.06*Re*D

Highlight''' 0.15 m'''

|| Let us check whether our '''geometry''' is suitable or not.

* '''Reynolds number''' of the problem is '''250'''.

* Hence, the flow is '''laminar'''.

* For '''fully developed flow''', length of the '''geometry''' should be greater than the '''Entrance length'''.

* '''Entrance length''' can be calculated by this '''formula'''.

* The length we have taken is greater than the '''entrance length'''.
|-
|| Slide: Solver detail
||
* To simulate this problem, we will use the '''icoFoam''' solver.

* '''icoFoam''' is a''' transient solver''' for '''incompressible''', '''laminar flow''' of '''Newtonian fluids'''.

* This is the most '''suitable solver''' for '''Hagen Poiseuille flow.'''

|-
|| Slide : Pressure Boundary Condition
|| The''' Pressure boundary conditions''' used are,

* At '''inlet - zero gradient'''
* At '''outlet - fixed Pressure'''
* At '''wall - zero gradient'''

|-
|| Slide: Velocity Boundary Condition
|| The''' Velocity boundary condition''' used are,

* At '''inlet - fixed value'''
* At '''outlet - zero Gradient'''
* At '''wall - No Slip'''

|-
|| Only Narration
|| We will use the '''mesh''' that we have created in the tutorial “'''Creating 3D Pipe Geometry and Mesh in OpenFoam'''”.
|-
|| Press Ctrl + Alt + T keys
|| Open the '''terminal''' by pressing the '''Ctrl''', '''Alt''' and '''T''' keys together.
|-
|| [Terminal]

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

'''cd $FOAM_RUN'''
|| At the '''prompt''', type the following '''command''' to go to the '''run directory'''.

|-
|| [Terminal] Type:

'''cd pipe'''
|| Navigate to the '''pipe case folder'''.

|-
|| [Terminal] Type:

'''mv 0.Orig 0'''
|| Now, '''rename''' '''0.Orig''' folder to''' 0''' by typing this '''command'''.

|-
|| [Terminal] Type: '''gedit 0/p'''
|| Let’s open the “'''p'''” file in a '''text editor'''.
|-
|| [gedit - '''p'''] Highlight

'''dimensions [0 2 -2 0 0 0 0];'''
|| Here we can see, the '''p''' file is in the form of '''pressure divided by density'''.

This means, it is '''kinematic pressure'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''internalField''' to the end of the file as shown here.
|-
|| [gedit - '''pressure''']
|| Open the file '''pressure.txt''', that you had downloaded in any '''text editor'''.
|-
|| [gedit - '''pressure'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''p''']
|| Let me switch back to the “'''p”''' file.
|-
|| [gedit - '''p'''] '''Paste '''
|| Paste the copied contents into the “'''p” '''file as shown here.
|-
|| [gedit - '''p'''] Highlight

'''internalField'''
|| Right after '''dimensions''', we have to define the '''initial condition'''.

It could be '''uniform''', '''non-uniform''' or in the form of '''code'''.
|-
|| [gedit - '''p'''] Highlight

'''uniform 0;'''
|| In this case, we will use the '''initial condition''' as''' uniform 0'''.

This means that the '''kinematic pressure''' inside the entire '''domain''' is '''0'''.
|-
|| [gedit - '''p'''] Highlight

'''boundaryField'''
|| In the '''boundaryField''', we specify '''boundary conditions''' for all '''patches''' and '''walls'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| '''Boundary condition''' for '''inlet''' in '''pressure''' is defined as shown.
|-
|| [gedit - '''p'''] Highlight

'''type zeroGradient;'''
|| Type of the '''boundary condition''' is '''zeroGradient'''.

'''Zero Gradient boundary '''extrapolates the quantity to the '''patch''' from the nearest '''cell value'''.

So, the value at '''patch''' will be the same as the '''cell value'''.

Note that '''z''' is small and '''G''' is capital.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> wall'''
|| '''Boundary condition''' for the '''wall''' is defined as the same as '''inlet'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> outlet'''
|| '''Boundary condition''' for '''outlet''' in '''pressure''' is defined as shown here.
|-
|| [gedit - '''p'''] Highlight

'''type fixedValue;'''

'''value 0;'''
|| Type of '''boundary condition''' is '''fixedValue'''.

'''Value''' given is '''zero'''.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''p '''file and close the '''text editor'''.
|-
|| [Terminal] Type:

'''gedit 0/U'''
|| Now, let’s set the '''initial''' and '''boundary condition''' for '''velocity'''.

To do so, open the '''U''' file in a '''text editor'''.
|-
|| [gedit - '''U'''] Highlight

'''dimensions [0 1 -1 0 0 0 0];'''
|| '''Dimensions''' here are in '''meters per second'''.
|-
|| [gedit - '''U'''] Highlight

'''internalField uniform (0 0 0);'''
|| '''Velocity''' is a '''vector field''', so the '''internal initial field''' is set as '''uniform (0 0 0)'''.
|-
|| [gedit - '''U'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''boundaryField''' to the end of the file as shown here.
|-
|| [gedit - '''velocity''']
|| Open the '''velocity.txt '''file that you had downloaded in a '''text editor'''.
|-
|| [gedit - '''velocity'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''U'''] '''Paste '''
|| Paste the copied contents into the “'''U” '''file as shown.
|-
|| [gedit - '''U'''] Highlight

'''boundaryField'''
|| In the '''boundaryField''', we will specify '''boundary conditions''' for all '''patches''' and '''walls'''.
|-
|| [gedit - '''U'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| '''Boundary condition''' for '''inlet''' in '''velocity''' is defined as shown here.
|-
|| [gedit - '''U'''] Highlight

'''type fixedValue;'''

'''value uniform (0 0 0.025);'''
|| Type of the '''boundary condition''' is '''fixedValue'''.

Value of '''velocity''' is 0.025 m/s in the '''Z direction'''.
|-
|| [gedit - '''U'''] Highlight

'''type noSlip;'''
|| '''Boundary condition''' for the '''wall''' is defined as '''noSlip'''.

This means '''velocity''' at the '''wall '''is '''0'''.
|-
|| [gedit - '''U'''] Highlight

'''type zeroGradient;'''
|| '''Boundary condition''' for '''outlet''' is '''zeroGradient''', defined as shown here.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''U '''file and close the '''text editor.'''
|-
|| [Terminal] Type:

'''gedit constant/transportProperties'''
|| Open '''transport properties''' file from '''constant folder''' in the '''text editor'''.
|-
|| [gedit - '''transportProperties'''] Highlight

'''nu'''
|| All '''properties''' of '''fluid''' which remain '''constant''' during the '''simulation''' is to be specified in the '''constant folder'''.

Here, we will set the value of '''kinematic viscosity'''.
|-
|| [gedit - '''transportProperties'''] Highlight

'''[0 2 -1 0 0 0 0]'''
|| Dimensions of '''kinematic viscosity''' are specified here.
|-
|| [gedit - '''transportProperties''']

'''Change: 0.01 >> 1e-06'''
|| To set the value of '''nu,''' replace '''0.01''' to '''1e-06'''.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''transportProperties '''file and close the '''text editor.'''
|-
|| Only Narration
|| '''Solve & write control parameters''' can be modified in the '''controlDict''' file.

The '''controlDict '''file is located in the '''system folder'''.
|-
|| [Terminal] Type:

'''gedit system/controlDict'''
|| Open the '''controlDict''' file in a '''text editor'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''application''' to the end of the file as shown here.
|-
|| [gedit - '''control''']
|| Open the '''control.txt''' file that you had downloaded in a '''text editor'''.
|-
|| [gedit - '''control'''] Highlight

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

|| Paste the copied contents into the “'''controlDict” '''file as shown here.
|-
|| [gedit - '''controlDict'''] Highlight

'''application icoFoam;'''
|| First line of the '''controlDict''' file shows the name of the '''solver'''.

In our case it is '''icoFoam'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''startFrom startTime;'''

'''startTime 0;'''
|| The second and third lines are '''start simulation controls'''.

Our '''simulation''' will start from the value specified in '''start time'''.

Here our '''start time''' is set to '''0'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''stopAt endTime;'''

'''endTime 5;'''
|| The fourth and fifth lines are '''stop simulation controls'''.

'''Simulation''' will stop at the''' endTime''' of '''5 seconds'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''deltaT 1e-2;'''
|| Then the value of '''deltaT''' is given, which is '''1e-02'''.

So, it will '''simulate''' for '''5 seconds''' with a '''1e-02 time step'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''writeInterval 100;'''
|| '''Write interval''' is 100. So it will print and save every 100 '''time-step value''' that '''OpenFOAM''' solves.

So we will get '''results''' written for 1, 2, 3, 4, and 5 seconds.
|-
|| [gedit - '''controlDict'''] Highlight

'''purgeWrite 2;'''
|| '''OpenFOAM''' gives the option to save only the last few '''time steps. '''

To enable that option, you can use the '''purgeWrite''' value.

By changing it to 2, we will get the 2 latest updated '''time-step''' results.

The old files will automatically be deleted.

At the end of the '''simulation''' we will get results of 4 & 5 seconds.

This option will save''' space''' on your computer.
|-
|| Only Narration
|| Rest of the options are for the format of writing''' data''' files in '''OpenFOAM'''.

We do not need to change them.

Therefore, we won’t be making any more changes to the '''controlDict''' file.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''controlDict '''file and close the '''text editor'''.
|-
|| Only Narration
|| We are done setting up the '''case'''.

Now we will '''run''' the '''simulation'''.
|-
|| [Terminal] Type: '''icoFoam'''
|| To do so, type '''icoFoam''' in the '''terminal''' and press '''Enter'''.
|-
|| Only Narration
|| It will take some time to '''simulate,''' based on your computer’s '''hardware'''.

For me it took around 4 minutes to '''simulate'''.
|-
|| [Terminal] Highlight

'''End'''
|| Once the '''simulation''' is finished, you will get this line at the end.
|-
|| Slide: Formula and Analytical Solution

Highlight '''2.4 Pa'''

Highlight '''0.05 m/s'''

||
* To calculate''' pressure '''at''' inlet,''' let’s put the values of the '''U, L, D '''and '''Po''' in this '''formula'''.

* We will get an '''inlet pressure''' value of '''2.4 Pascal'''.

* '''Maximum velocity''' will be twice of average '''velocity''' as per '''analytical solution'''.
|-
|| Slide: Result Comparison
||
* From the '''simulation''' we get,
** '''Maximum velocity''' 0.05 m/s and
** '''inlet Pressure 2.8 Pascals.'''

* In '''CFD''', there are always some deviations in results of '''analytical''' and '''numerical''' '''solutions'''.

* We will discuss '''results''' in detail later in this series.

|-
|| 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 the '''boundary''' and '''initial''' '''conditions'''
* Set up the '''physical properties'''
* Set up the '''solve & write control parameter '''and
* Run the '''simulation'''
|-
|| 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 Divyesh Variya.

And this is Swetha Sridhar from IIT Bombay signing off.

Thanks for joining.
|-
|}

OpenFOAM-version-7/C2/Simulating-Hagen-Poiseuille-flow-through-a-pipe-in-OpenFOAM/English

2020-07-21T12:10:13Z

Divyesh7:

'''Title of the script:''' Simulating Hagen Poiseuille flow through a pipe in OpenFOAM

'''Author:''' Divyesh Variya

'''Keywords:''' OpenFOAM, Hagen Poiseuille, Pipe flow, icoFoam, controlDict, Video-Tutorial

{| Border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Simulating Hagen Poiseuille flow through a pipe in OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn to,

* Set up the '''boundary''' and '''initial''' '''conditions'''
* Set up the '''physical properties'''
* Set up the '''solve & write control parameter '''and
* Run the '''simulation'''

|-
|| 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 '''Hagen Poiseuille flow''' and basic '''Fluid Dynamics '''concepts
* You should also be familiar with creation of a '''3D pipe Geometry''' in '''OpenFOAM'''
* If you are 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: Problem Setup
|| In this diagram, a '''section view''' of a '''3D pipe''' is shown.

This describes the '''problem statement'''.

* The '''diameter''' of the '''pipe''' is 1 centimeter and its '''length''' is 30 centimeters.
* It has one '''inlet''', one '''outlet''' and a '''cylindrical''' '''wall'''.

* The fluid here is water''' '''and its '''kinematic viscosity''' is taken as '''1e-06'''.

* The '''Inlet velocity '''is '''0.025 m/s '''and''' Outlet pressure '''is''' 0 Pascals '''as shown in the diagram.

|-
|| Slide: Geometry Check

Highlight '''250'''

Highlight''' laminar'''

Only Narration

Le = 0.06*Re*D

Highlight''' 0.15 m'''

|| Let us check whether our '''geometry''' is suitable or not.

* '''Reynolds number''' of the problem is '''250'''.

* Hence, the flow is '''laminar'''.

* For '''fully developed flow''', length of the '''geometry''' should be greater than the '''Entrance length'''.

* '''Entrance length''' can be calculated by this '''formula'''.

* The length we have taken is greater than the '''entrance length'''.
|-
|| Slide: Solver detail
|| * To simulate this problem, we will use the '''icoFoam''' solver.

* '''icoFoam''' is a''' transient solver''' for '''incompressible''', '''laminar flow''' of '''Newtonian fluids'''.

* This is the most '''suitable solver''' for '''Hagen Poiseuille flow.'''

|-
|| Slide : Pressure Boundary Condition
|| The''' Pressure boundary conditions''' used are,

* At '''inlet - zero gradient'''
* At '''outlet - fixed Pressure'''
* At '''wall - zero gradient'''

|-
|| Slide: Velocity Boundary Condition
|| The''' Velocity boundary condition''' used are,

* At '''inlet - fixed value'''
* At '''outlet - zero Gradient'''
* At '''wall - No Slip'''

|-
|| Only Narration
|| We will use the '''mesh''' that we have created in the tutorial “'''Creating 3D Pipe Geometry and Mesh in OpenFoam'''”.
|-
|| Press Ctrl + Alt + T keys
|| Open the '''terminal''' by pressing the '''Ctrl''', '''Alt''' and '''T''' keys together.
|-
|| [Terminal]

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

'''cd $FOAM_RUN'''
|| At the '''prompt''', type the following '''command''' to go to the '''run directory'''.

|-
|| [Terminal] Type:

'''cd pipe'''
|| Navigate to the '''pipe case folder'''.

|-
|| [Terminal] Type:

'''mv 0.Orig 0'''
|| Now, '''rename''' '''0.Orig''' folder to''' 0''' by typing this '''command'''.

|-
|| [Terminal] Type: '''gedit 0/p'''
|| Let’s open the “'''p'''” file in a '''text editor'''.
|-
|| [gedit - '''p'''] Highlight

'''dimensions [0 2 -2 0 0 0 0];'''
|| Here we can see, the '''p''' file is in the form of '''pressure divided by density'''.

This means, it is '''kinematic pressure'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''internalField''' to the end of the file as shown here.
|-
|| [gedit - '''pressure''']
|| Open the file '''pressure.txt''', that you had downloaded in any '''text editor'''.
|-
|| [gedit - '''pressure'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''p''']
|| Let me switch back to the “'''p”''' file.
|-
|| [gedit - '''p'''] '''Paste '''
|| Paste the copied contents into the “'''p” '''file as shown here.
|-
|| [gedit - '''p'''] Highlight

'''internalField'''
|| Right after '''dimensions''', we have to define the '''initial condition'''.

It could be '''uniform''', '''non-uniform''' or in the form of '''code'''.
|-
|| [gedit - '''p'''] Highlight

'''uniform 0;'''
|| In this case, we will use the '''initial condition''' as''' uniform 0'''.

This means that the '''kinematic pressure''' inside the entire '''domain''' is '''0'''.
|-
|| [gedit - '''p'''] Highlight

'''boundaryField'''
|| In the '''boundaryField''', we specify '''boundary conditions''' for all '''patches''' and '''walls'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| '''Boundary condition''' for '''inlet''' in '''pressure''' is defined as shown.
|-
|| [gedit - '''p'''] Highlight

'''type zeroGradient;'''
|| Type of the '''boundary condition''' is '''zeroGradient'''.

'''Zero Gradient boundary '''extrapolates the quantity to the '''patch''' from the nearest '''cell value'''.

So, the value at '''patch''' will be the same as the '''cell value'''.

Note that '''z''' is small and '''G''' is capital.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> wall'''
|| '''Boundary condition''' for the '''wall''' is defined as the same as '''inlet'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> outlet'''
|| '''Boundary condition''' for '''outlet''' in '''pressure''' is defined as shown here.
|-
|| [gedit - '''p'''] Highlight

'''type fixedValue;'''

'''value 0;'''
|| Type of '''boundary condition''' is '''fixedValue'''.

'''Value''' given is '''zero'''.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''p '''file and close the '''text editor'''.
|-
|| [Terminal] Type:

'''gedit 0/U'''
|| Now, let’s set the '''initial''' and '''boundary condition''' for '''velocity'''.

To do so, open the '''U''' file in a '''text editor'''.
|-
|| [gedit - '''U'''] Highlight

'''dimensions [0 1 -1 0 0 0 0];'''
|| '''Dimensions''' here are in '''meters per second'''.
|-
|| [gedit - '''U'''] Highlight

'''internalField uniform (0 0 0);'''
|| '''Velocity''' is a '''vector field''', so the '''internal initial field''' is set as '''uniform (0 0 0)'''.
|-
|| [gedit - '''U'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''boundaryField''' to the end of the file as shown here.
|-
|| [gedit - '''velocity''']
|| Open the '''velocity.txt '''file that you had downloaded in a '''text editor'''.
|-
|| [gedit - '''velocity'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''U'''] '''Paste '''
|| Paste the copied contents into the “'''U” '''file as shown.
|-
|| [gedit - '''U'''] Highlight

'''boundaryField'''
|| In the '''boundaryField''', we will specify '''boundary conditions''' for all '''patches''' and '''walls'''.
|-
|| [gedit - '''U'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| '''Boundary condition''' for '''inlet''' in '''velocity''' is defined as shown here.
|-
|| [gedit - '''U'''] Highlight

'''type fixedValue;'''

'''value uniform (0 0 0.025);'''
|| Type of the '''boundary condition''' is '''fixedValue'''.

Value of '''velocity''' is 0.025 m/s in the '''Z direction'''.
|-
|| [gedit - '''U'''] Highlight

'''type noSlip;'''
|| '''Boundary condition''' for the '''wall''' is defined as '''noSlip'''.

This means '''velocity''' at the '''wall '''is '''0'''.
|-
|| [gedit - '''U'''] Highlight

'''type zeroGradient;'''
|| '''Boundary condition''' for '''outlet''' is '''zeroGradient''', defined as shown here.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''U '''file and close the '''text editor.'''
|-
|| [Terminal] Type:

'''gedit constant/transportProperties'''
|| Open '''transport properties''' file from '''constant folder''' in the '''text editor'''.
|-
|| [gedit - '''transportProperties'''] Highlight

'''nu'''
|| All '''properties''' of '''fluid''' which remain '''constant''' during the '''simulation''' is to be specified in the '''constant folder'''.

Here, we will set the value of '''kinematic viscosity'''.
|-
|| [gedit - '''transportProperties'''] Highlight

'''[0 2 -1 0 0 0 0]'''
|| Dimensions of '''kinematic viscosity''' are specified here.
|-
|| [gedit - '''transportProperties''']

'''Change: 0.01 >> 1e-06'''
|| To set the value of '''nu,''' replace '''0.01''' to '''1e-06'''.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''transportProperties '''file and close the '''text editor.'''
|-
|| Only Narration
|| '''Solve & write control parameters''' can be modified in the '''controlDict''' file.

The '''controlDict '''file is located in the '''system folder'''.
|-
|| [Terminal] Type:

'''gedit system/controlDict'''
|| Open the '''controlDict''' file in a '''text editor'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''application''' to the end of the file as shown here.
|-
|| [gedit - '''control''']
|| Open the '''control.txt''' file that you had downloaded in a '''text editor'''.
|-
|| [gedit - '''control'''] Highlight

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

|| Paste the copied contents into the “'''controlDict” '''file as shown here.
|-
|| [gedit - '''controlDict'''] Highlight

'''application icoFoam;'''
|| First line of the '''controlDict''' file shows the name of the '''solver'''.

In our case it is '''icoFoam'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''startFrom startTime;'''

'''startTime 0;'''
|| The second and third lines are '''start simulation controls'''.

Our '''simulation''' will start from the value specified in '''start time'''.

Here our '''start time''' is set to '''0'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''stopAt endTime;'''

'''endTime 5;'''
|| The fourth and fifth lines are '''stop simulation controls'''.

'''Simulation''' will stop at the''' endTime''' of '''5 seconds'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''deltaT 1e-2;'''
|| Then the value of '''deltaT''' is given, which is '''1e-02'''.

So, it will '''simulate''' for '''5 seconds''' with a '''1e-02 time step'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''writeInterval 100;'''
|| '''Write interval''' is 100. So it will print and save every 100 '''time-step value''' that '''OpenFOAM''' solves.

So we will get '''results''' written for 1, 2, 3, 4, and 5 seconds.
|-
|| [gedit - '''controlDict'''] Highlight

'''purgeWrite 2;'''
|| '''OpenFOAM''' gives the option to save only the last few '''time steps. '''

To enable that option, you can use the '''purgeWrite''' value.

By changing it to 2, we will get the 2 latest updated '''time-step''' results.

The old files will automatically be deleted.

At the end of the '''simulation''' we will get results of 4 & 5 seconds.

This option will save''' space''' on your computer.
|-
|| Only Narration
|| Rest of the options are for the format of writing''' data''' files in '''OpenFOAM'''.

We do not need to change them.

Therefore, we won’t be making any more changes to the '''controlDict''' file.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''controlDict '''file and close the '''text editor'''.
|-
|| Only Narration
|| We are done setting up the '''case'''.

Now we will '''run''' the '''simulation'''.
|-
|| [Terminal] Type: '''icoFoam'''
|| To do so, type '''icoFoam''' in the '''terminal''' and press '''Enter'''.
|-
|| Only Narration
|| It will take some time to '''simulate,''' based on your computer’s '''hardware'''.

For me it took around 4 minutes to '''simulate'''.
|-
|| [Terminal] Highlight

'''End'''
|| Once the '''simulation''' is finished, you will get this line at the end.
|-
|| Slide: Formula and Analytical Solution

Highlight '''2.4 Pa'''

Highlight '''0.05 m/s'''

||
* To calculate''' pressure '''at''' inlet,''' let’s put the values of the '''U, L, D '''and '''Po''' in this '''formula'''.

* We will get an '''inlet pressure''' value of '''2.4 Pascal'''.

* '''Maximum velocity''' will be twice of average '''velocity''' as per '''analytical solution'''.
|-
|| Slide: Result Comparison
||
* From the '''simulation''' we get,
** '''Maximum velocity''' 0.05 m/s and
** '''inlet Pressure 2.8 Pascals.'''

* In '''CFD''', there are always some deviations in results of '''analytical''' and '''numerical''' '''solutions'''.

* We will discuss '''results''' in detail later in this series.

|-
|| 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 the '''boundary''' and '''initial''' '''conditions'''
* Set up the '''physical properties'''
* Set up the '''solve & write control parameter '''and
* Run the '''simulation'''
|-
|| 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 Divyesh Variya.

And this is Swetha Sridhar from IIT Bombay signing off.

Thanks for joining.
|-
|}

OpenFOAM-version-7/C2/Creating-3D-Pipe-Geometry-and-Mesh-in-OpenFOAM/English

2020-07-21T06:19:52Z

Divyesh7:

'''Title of the script:''' Creating 3D Pipe Geometry and Mesh in OpenFOAM

'''Author:''' Divyesh Variya

'''Keywords:''' OpenFOAM, 3D-Geometry, Pipe, Meshing, ParaView, Pre-Processing, Video-Tutorial, blockMesh

{| border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening slide
|| Welcome to this tutorial on '''Creating 3D Pipe Geometry and Mesh in OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn to:

* Create a '''3D Geometry''' using '''blockMeshDict'''
* '''Mesh''' a '''3D''' '''geometry'''
* Label the''' boundary patches'''
* Check the '''mesh results '''using''' checkMesh command''' and
* View the '''3D geometry''' and '''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: Prerequisites
* If not, please go through the prerequisite '''OpenFOAM '''tutorial on https://spoken-tutorial.org

|| As a prerequisite:
* You should be familiar with creation of a basic '''geometry''' using the '''blockMesh''' utility.
* If you are 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: Hagen Poiseuille flow through a pipe
||
* In this tutorial, we will learn to create the '''geometry''' for '''Hagen Poiseuille flow through a pipe'''.
* The problem description of '''Hagen Poiseuille flow through a pipe''' is shown in the diagram.

|-
|| Slide: Pipe Geometry
||
* This is the diagram of the '''geometry''' for '''Hagen Poiseuille flow through a pipe.'''
* The left and right faces are the '''inlet''' and '''outlet''' respectively.
* The cylindrical face of the '''geometry''' is a '''wall'''.
* The '''diameter''' of the pipe is 1 centimeter and its '''length''' is 30 centimeters.

|-
|| 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'''.
|-
|| [Terminal] Type:

'''cp -r $FOAM_TUTORIALS/incompressible/icoFoam/cavity/cavity pipe'''
|| Let us now copy the '''cavity case''' from the '''icoFoam''' '''tutorial directory''' to the '''run directory'''.

Type the following '''command''' to do so.
|-
|| [Terminal] Highlight: '''pipe'''
|| Note that the '''cavity case''' is copied to the '''pipe''' directory.
|-
|| [Terminal] Type:

'''mv pipe/0 pipe/0.Orig'''
|| In this tutorial we don’t need to define '''initial''' and '''boundary''' '''conditions''' in '''zero''' time.

Type this '''command''' to '''rename''' '''“0”''' folder to '''“0.Orig”'''
|-
|| [Terminal] Type:

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

Open this file in a '''text editor'''. I am doing it in the '''gedit text editor'''.
|-
|| [gedit - '''blockMeshDict''']
|| Now we can see the '''blockMeshDict''' file in the '''text editor.'''
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> Delete'''
|| '''Delete''' the lines from '''convertToMeters''' to the end of the file as shown here.

The remaining content is common for all '''blockMeshDict''' files.
|-
|| [gedit - '''pipe''']
|| Next, open the '''pipe.txt''' file that you had downloaded in the '''text editor'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.

|-
|| [gedit - '''blockMeshDict''']
|| Now switch back to the '''blockMeshDict''' file.
|-
|| [gedit - '''blockMeshDict''']

'''Paste '''
|| And paste the copied contents into the '''blockMeshDict '''file as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''0.01'''
|| Note that all the '''dimensions''' will be in '''centimeters'''.
|-
|| Slide: Vertices Detail
||
* '''Vertices''' are shown in the slide.
* Here we are going to use '''18''' '''vertices''' to define the '''geometry''' of a '''pipe'''.
* For example, '''two reference points''' 0 and 17 are on (0 0 0) and (0 0 30) respectively.

|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> vertices '''
|| All '''18''' '''points''' are defined in the '''vertices''' '''section''' in the '''blockMeshDict''' file as shown.
|-
|| Only Narration
|| Now let me switch back to the '''Slides'''.
|-
|| Slide: Block Detail
||
* Here we will use 5 '''hexahedral blocks''' to define the''' pipe geometry'''.
* As you can see, the '''center hexahedral block''' is separately shown in the '''figure''' on the right.
* To '''define''' this '''block''', we need to type the '''back plane’s vertices '''first.
* The '''vertices''' should be ordered''' anti-clockwise''' when viewed '''along the negative z-axis'''.
* The '''front plane’s vertices''' should also follow the same order.

|-
|| Slide: Block Detail

Highlight: '''hex (1 2 3 4 9 10 11 12) (8 8 80) simpleGrading (1 1 1)'''
|| An '''example''' is shown in the '''slide'''.

The same '''block''' can be defined correctly in more than one way.

|-
|| Slide: Block Detail

Highlight: '''(8 8 80)'''
|| To generate '''3D mesh''' we are using:

* '''8 cells''' in '''X direction''',
* '''8 cells '''in '''Y direction''' and
* '''80 cells''' in '''Z direction'''.

|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> blocks'''
|| Other '''4''' '''blocks''' are defined in the '''blockMeshDict''' file as shown.

|-
|| Slide: Geometry Arc Detail
|| For the '''curved geometry''', we need to define the '''edges'''.
|-
|| Slide: Geometry Arc Detail
||
* There are a total of '''16 arcs''' that we need to define.
* The '''arcs''' and the '''intermediate points''' are shown in the slide.
* Note that I have used the '''midpoint''' of the '''arc''' as the '''intermediate point'''.
* However, '''any other point''' through which the '''arc''' passes is acceptable.

|-
|| Slide: Geometry Arc Detail

Highlight: '''arc 5 6 (0 0.5 0)'''
|| For example, the''' edge''' from '''Point''' number '''5''' to '''6''' is passing through (0 0.5 0).
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> edges'''
|| All '''16''' '''arcs''' are defined in the '''edges''' '''section''' in the '''blockMeshDict''' file as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''arc 5 6 (0 0.5 0)'''
|| The '''curved edge''' connecting '''points 5''' and '''6''' is defined as shown.

|-
|| [gedit - '''blockMeshDict'''] Highlight

'''arc'''
|| The edge is an '''arc'''.

|-
|| [gedit - '''blockMeshDict'''] Highlight

'''5 6'''
|| Its two '''end''' '''points''' are 5 and 6.

|-
|| [gedit - '''blockMeshDict'''] Highlight

'''(0 0.5 0)'''
|| The '''coordinates''' of the '''point''' through which the '''arc''' passes through is 0, 0.5, 0

|-
|| Only Narration
|| Let’s label the '''boundary patches'''.

The '''boundary faces''' should be labelled appropriately.

The labels are used to impose '''boundary conditions''' on the respective faces.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| The '''inlet boundary''' is defined as shown.

|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >>'''
|| The''' inlet boundary''' has 5 faces.

These faces are defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> outlet and wall'''
|| The '''outlet '''and''' wall boundary''' is defined as shown.

|-
|| Only Narration
|| Note that all '''boundaries''' have more than one face.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> mergePatchPairs'''
|| We do not have any '''patches '''or''' internal faces''' to merge.

Therefore, we leave the '''mergePatchPairs''' field empty.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''blockMeshDict '''file and close the text editor.
|-
|| [Terminal] Type:

'''cd pipe'''
|| Now, go to the '''terminal''' and navigate to the '''pipe''' directory.
|-
|| [Terminal] Type:

'''blockMesh'''
|| Type '''blockMesh command''' and press '''Enter'''.

|-
|| [Terminal] Highlight

'''End'''
|| The '''meshing''' is now complete.

|-
|| [Terminal] Highlight

'''Patches section'''
|| As we can see in '''terminal results''', three patches are created.

|-
|| [Terminal] Type:

'''checkMesh'''
|| Now, let’s '''check''' '''mesh''' '''results''' and '''quality'''.

To do that type '''checkMesh''' in the '''terminal''' and press '''Enter'''.

Note that '''M '''in''' checkMesh''' is capital.
|-
|| Only Narration
|| We get the '''results''' printed of the '''mesh''' we created.
|-
|| [Terminal] Highlight

'''Max skewness = 0.6954 OK.'''

'''Non-orthogonality check OK.'''

'''Max aspect ratio = 30.3404 OK.'''

'''Overall domain bounding box '''
|| Here we can see:

* '''Skewness'''

* '''Orthogonality'''

* '''Aspect ratio'''

* '''Negative volume''' values if they are present

In our case, no negative volume is present.

* '''Bounding box '''coordinates and

|-
|| [Terminal] Highlight

'''Overall number of cells of each type:'''

'''hexahedra: 25600'''

'''prisms: 0'''

'''wedges: 0'''

'''pyramids: 0'''

'''tet wedges:0'''

'''tetrahedra:0'''

'''polyhedra: 0'''
||
* '''Number of cells''' with their '''types'''

|-
|| [Terminal] Type '''paraFoam'''

|| To view '''mesh''' in '''paraview''' type '''paraFoam''' and press '''Enter'''.
|-
|| [ParaView] Click

'''Apply'''
|| Click on '''Apply''' on the left side of your window in the '''Properties''' tab.

Now you can see '''pipe geometry''' in the''' Layout window'''.
|-
|| [ParaView] '''Rotate geometry'''
|| You can''' rotate''' geometry in the '''Layout''' '''window''' by pressing the left mouse button and dragging.
|-
|| [ParaView]

'''Click on Surface >> Click on Surface with Edges'''
|| Click on '''Surface''' available in the '''Active Variable Controls.'''

Then change it to '''Surface with Edges'''.
|-
|| [ParaView]

'''Click on vtkBlockColors >> SolidColor'''
|| Click on '''vtkBlockColors''' available in the '''Active Variable Controls.'''
and change it to '''SolidColor'''.

You can now see the '''mesh structure''' of '''pipe geometry''' that we created.
|-
|| [ParaView] '''Close ParaView'''
|| You can close the '''ParaView''' window.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

Let’s summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt to,

* Create a '''3D Geometry''' using '''blockMeshDict'''
* Mesh a '''3D''' '''geometry'''
* Label the''' boundary patches'''
* Check the '''mesh results '''using''' checkMesh command''' and
* View the '''3D geometry''' and '''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 Divyesh Variya.

And this is Swetha Sridhar from IIT Bombay signing off.

Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Basic-Post-Processing-using-ParaView/English

2020-07-21T06:09:29Z

Divyesh7: Created page with "'''Title of the script:''' Basic Post Processing using ParaView '''Author:''' Divyesh Variya '''Keywords:''' OpenFOAM, Hagen Poiseuille, Paraview, Clip, Streamline, Glyph, P..."

'''Title of the script:''' Basic Post Processing using ParaView

'''Author:''' Divyesh Variya

'''Keywords:''' OpenFOAM, Hagen Poiseuille, Paraview, Clip, Streamline, Glyph, Plot-over-line, Parabolic profile, Video-Tutorial

{| border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Hello and welcome to this tutorial on '''Basic Post Processing using ParaView.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn,
* Some basic '''visualization techniques''' in '''ParaView'''
* Export the''' field data '''to '''.csv''' file
* Plot a''' graph''' in '''LibreOffice Suite Calc'''
* Save a screenshot of a '''view'''

|-
|| Slide: System Specifications
|| To record this tutorial, I am using,
* '''Ubuntu Linux OS''' version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0
* '''LibreOffice Suite''' 6.4

|-
|| Slide: Prerequisites
* Please go through these two tutorials on https://spoken-tutorial.org

|| As a prerequisite learner should practise,
* On '''Simulating Hagen Poiseuille Flow through a Pipe''' from the '''OpenFOAM '''tutorials and
* Tutorial on '''Using Charts and Graphs''' from the '''LibreOffice Suite Calc''' tutorials
* Please go through these two tutorials on this website.

|-
|| Press Ctrl + Alt + T keys
|| Open the '''terminal''' by pressing the '''Ctrl''', '''Alt''' and '''T''' keys together.
|-
|| Only Narration
|| From now onwards please remember to press the '''Enter''' key after typing each '''command.'''
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''
|| At the '''prompt''', type the following '''command''' to go to the '''run directory'''.
|-
|| [Terminal] Type:

'''cd pipe'''
|| Navigate to the '''pipe case '''folder.

We have created this in the''' “Simulating Hagen Poiseuille Flow through Pipe” '''tutorial.
|-
|| [Terminal] Type: '''paraFoam'''
|| Type '''paraFoam''' in the '''terminal''' to open the '''case''' file in '''paraView'''.
|-
|| [ParaView]

'''Uncheck >> inlet and outlet'''
|| Go to the '''properties''' panel.

Scroll down and locate the '''mesh parts''' section.

Uncheck all '''patches''' other than '''internalMesh'''.
|-
|| [ParaView] '''Click on Apply'''
|| Click on the '''Apply''' button in the '''Properties '''panel.
|-
|| [ParaView]

'''Click on Solid Color >> Click on U'''
|| Click on '''Solid Color '''available in the '''Active Variable Controls.'''

From here, we can change the fields that we want to visualize.

Select the '''U''' field with the dot, not the one with the box.
|-
|| [ParaView]

'''Click on Last Frame'''
|| From '''VCR Controls''', we can change the''' time steps''' and '''run animation''' using the '''Play''' button.

Currently we are on 0 time, which is for the '''initial field'''.

To go to the last '''time step, '''click on the '''Last Frame''' button.
|-
|| Show Picture of ICONS
|| As you can see, some '''filter''' icons are shown here.
|-
|| [ParaView]

'''Click on Stream Tracer filter'''
|| To visualize '''streamline''', click on the '''Stream tracer''' icon from '''Common and Data Analysis Filters'''.
|-
|| [ParaView]

'''Change seed type to point source'''
|| From the '''Properties''' panel we can change the '''seed type.'''

The two '''seed types''' available are:
* '''High resolution line source''' and
* '''Point Source'''

'''High resolution Line Source''' gives '''streamlines''' passing through a '''line'''.

'''Point Source''' gives '''streamlines''' passing through a '''sphere'''.

We will select '''Point Source'''.
|-
|| [ParaView]

'''Set number of points to 1000 >>'''

'''Uncheck Show Sphere checkbox'''
|| Set the '''number of points''' to '''1000''' and '''uncheck''' the '''Show Sphere''' option to hide the sphere.
|-
|| [ParaView]

'''Click on Apply'''
|| Click on the '''Apply''' button in the '''Properties''' panel.

We can see 1000 '''streamlines''' passing through 1000 random points within the sphere.
|-
|| [ParaView]

'''Click on Delete button'''
|| This way we can visualize the '''streamline'''.

Now '''Delete''' the '''Stream Tracer filter''' by clicking on the '''Delete''' button on the '''Properties''' panel.
|-
|| [ParaView] '''Click on Glyph filter'''
|| Click on the '''Glyph''' icon from '''Common and Data Analysis Filters'''.
|-
|| [ParaView]

'''Change Orientation U'''
|| Change '''Orientation Array''' to '''U '''from''' '''the '''Properties''' panel.
|-
|| [ParaView] '''Scale array U'''
|| Change '''Scale array''' to '''U '''in''' '''the '''Properties''' panel.
|-
|| [ParaView] '''Click on Apply'''
|| Click on the '''Apply''' button in the '''Properties '''panel.
|-
|| [ParaView]

'''Hide pipe.OpenFOAM'''
|| Hide '''pipe.OpenFOAM''' from the '''pipeline browser '''by clicking on the eye icon.
|-
|| [ParaView]

'''Zoom in render layout with left mouse click and drag'''
|| We can see '''Arrows''' in the direction of the '''flow'''.
|-
|| [ParaView] '''Delete Glyph filter'''
|| '''Delete''' the '''Glyph filter '''from the '''Properties''' panel.
|-
|| [ParaView] '''Click on Clip filter'''
|| Click on the '''clip''' icon from '''Common and Data Analysis Filters''' to clip the '''mesh'''.
|-
|| [ParaView]

'''Uncheck Show plane and invert'''
|| Uncheck “'''Show Plane'''” and “'''invert'''” boxes from the '''Properties '''panel.
|-
|| [ParaView] '''Click on Apply'''
|| Click on the '''Apply''' button in the '''Properties '''panel.
|-
|| Only Narration
|| This way we can clip any '''mesh''' and visualize '''internal flow'''.
|-
|| [ParaView] '''Delete Clip filter'''
|| Delete the '''Clip''' filter from the '''Properties''' panel.
|-
|| [ParaView]

'''Click on Plot Over Line Filter'''
|| Click on the “'''Plot Over Line'''” filter from '''Common and Data Analysis Filters'''.
|-
|| [ParaView]

'''Click on Y Axis'''
|| Click on '''Y Axis''' on the '''Properties''' panel and click '''Apply'''.
|-
|| [ParaView]'''Highlight '''

'''Line Chart view window'''
|| A new '''line chart window''' opens automatically with '''P''' and '''U_Magnitude''' '''graphs'''.
|-
|| [ParaView]

'''Scroll properties panel and uncheck p from series parameter'''
|| In the '''Properties''' panel, scroll down and locate the '''series parameters''' section.

Uncheck '''P''' from that.
|-
|| [ParaView] '''Highlight '''

'''Line Chart view window'''
|| We will get a '''parabolic profile''' for the '''velocity''' in the graph.
|-
|| [ParaView] '''Click on Line chart view window'''

'''Press CTRL+S'''
|| Click on the '''Line Chart View''' window

And press '''Ctrl+S''' keys to save data.
|-
|| [Save File:]

'''Select file type as .csv '''

'''give name - Y-Axis'''
|| Select '''Files of type''' as '''.csv''' and give the file name '''Y(hyphen)Axis.'''
|-
|| [Save File:]

'''Click >> OK'''
|| Click on '''OK'''.

Again click on '''OK''' with default settings.
|-
|| Only Narration
|| The data is saved in a '''.csv''' file.

We can open this file in '''LibreOffice Calc''' and compare with an analytical solution.
|-
|| [ParaView]

'''Click on File >> Save Screenshot...'''
|| Now go to the '''File''' menu in the menu bar and select '''Save Screenshot.'''
|-
|| [ParaView]

'''File name - velocity'''

'''File type - .png'''
|| Give a '''File Name''' and select''' file type'''.

Here I am saving the screenshot as '''velocity''' with the '''.png''' file type.
|-
|| [ParaView] '''Click >> OK'''
|| Click on the '''OK''' button.
|-
|| [ParaView]

'''Click >> OK'''
|| The '''Save Screenshot''' option window pops up.

We can change the '''size''', '''scaling''', '''coloring''' and other image options here.

With the default values in the settings, click on the '''OK''' button.
|-
|| Only Narration
|| '''Screenshot''' of '''Parabolic curve profile''' is saved in our '''case '''directory.
|-
|| [ParaView]

'''Click on Z Axis'''
|| Go to the '''Properties''' panel.

Click on '''Z Axis''' and then click on the '''Apply''' button.
|-
|| [ParaView]

'''Uncheck U_Magnitude and check p'''
|| Then go to the '''series parameter''' section in the '''Properties''' panel.

Uncheck '''U_Magnitude''' field and check '''p field.'''
|-
|| [ParaView]

'''Press CTRL+S'''

'''Select .csv file type'''

'''Give a name - Z-Axis'''

'''Press OK'''

'''Press OK'''
|| Save this data to''' Z-Axis.csv''' file as explained earlier.
|-
|| [ParaView] '''Close ParaView'''
|| Close the '''ParaView''' window.
|-
|| '''Open File explorer'''
|| Open the '''File explorer '''from the '''taskbar'''.
|-
|| [File explorer]

'''Open >> OpenFOAM'''
|| Open the '''OpenFOAM''' directory.

Here we can see the '''username '''directory of our computer.
|-
|| [File explorer]

'''Open >> “username directory”'''
|| Now open your current '''user '''directory.

In the '''user''' directory we can see the “'''run'''” directory.
|-
|| [File explorer]

'''Open >> run'''
|| Open the “'''run'''” directory.

Our saved work is available here in the '''pipe''' directory.
|-
|| [File explorer] '''Open >> pipe '''
|| Now open the '''pipe''' directory.
|-
|| '''Only Narration'''
|| Here we can see all files including '''screenshot image''' and '''.csv files''' that we have saved.
|-
|| [File explorer]

'''Right click on >> Z-Axis.csv'''
|| Right click on '''Z-Axis.csv''' file.
|-
|| [File explorer]

'''Click on >> Open With Other Application'''
|| From the list, click on the “'''Open With Other Application'''” option.

|-
|| [File explorer]

'''Click on >> View All Application'''
|| Now click on the “'''View All Application'''” button.

|-
|| [File explorer]

'''Double click on >> LibreOffice Calc'''
|| A list of all the '''applications''' available in your computer will appear.

From this list find “'''LibreOffice Calc'''” and double click on it.
|-
|| [File explorer]

'''Click on >> OK'''
|| A “'''Text Import'''” window will open on your screen.

At the bottom right corner click on the '''OK''' button.
|-
|| Highlight '''LibreOffice suite calc'''
|| Our file is now open in '''LibreOffice Calc.'''
|-
|| [LibreOffice suite calc]

'''Highlight cells'''
|| We have

'''velocity U:0''' at '''Point:0'''

'''Velocity U:1''' at '''Point:1 '''and

'''Velocity U:2''' at '''Point:2'''.
|-
|| [LibreOffice suite calc]

'''Highlight cells'''
|| We have '''kinematic pressure p''', '''vtkValidPointMask''' and '''arc_length''' also.
|-
|| [LibreOffice suite calc]

'''Highlight cells'''
|| Necessary data to plot the graph is '''U:2''', '''Point:2''' and '''p'''.
|-
|| [LibreOffice suite calc]

Show Graphs
|| For this demonstration I have created a graph on '''z-axis''' versus '''kinematic pressure'''.

And another graph for '''z-axis''' versus '''velocity'''.
|-
|| [LibreOffice suite calc]

Show Graphs
|| In the same way I have created a '''y-axis''' versus '''velocity''' graph with a '''y-axis.csv''' file.
|-
|| Only Narration
|| Here you can also compare '''analytical '''solutions with '''OpenFoam''' solutions.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

Let’s summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt,
* Some basic '''visualization techniques''' in '''ParaView'''
* Export''' field data '''to''' .csv''' file
* Plot''' graph''' in '''LibreOffice suite calc'''
* Save screenshot of a '''view'''

|-
|| Slide: Assignment
|| As an assignment:
* Simulate the '''Hagen Poiseuille flow''' for the '''pipe''' of '''0.5 cm''' diameter with
* '''Inlet''' '''velocity''' '''0.05 m/s''' and '''outlet pressure''' '''0 Pascal''' and,
* Plot graphs of '''velocity''' and '''pressure '''in''' ParaView '''and''' LibreOffice Calc'''.

|-
|| 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
|| Pls post your timed queries on this website
|-
|| 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 Divyesh Variya.

And this is Swetha Sridhar from IIT Bombay signing off. Thank you for joining.
|-
|}

OpenFOAM-version-7/C2/Simulating-Hagen-Poiseuille-flow-through-a-pipe-in-OpenFOAM/English

2020-07-21T05:18:26Z

Divyesh7: Created page with "'''Title of the script:''' Simulating Hagen Poiseuille flow through a pipe in OpenFOAM '''Author:''' Divyesh Variya '''Keywords:''' OpenFOAM, Hagen Poiseuille, Pipe flow, ic..."

'''Title of the script:''' Simulating Hagen Poiseuille flow through a pipe in OpenFOAM

'''Author:''' Divyesh Variya

'''Keywords:''' OpenFOAM, Hagen Poiseuille, Pipe flow, icoFoam, controlDict, Video-Tutorial

{| Border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening Slide
|| Welcome to this tutorial on '''Simulating Hagen Poiseuille flow through a pipe in OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn to,

* Set up the '''boundary''' and '''initial''' '''conditions'''
* Set up the '''physical properties'''
* Set up the '''solve & write control parameter '''and
* Run the '''simulation'''

|-
|| Slide: System Specifications
|| To record this tutorial, I am using,

* '''Ubuntu Linux OS''' version 18.04
* '''OpenFOAM''' version 7
* '''ParaView''' version 5.6.0
* '''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 '''Hagen Poiseuille flow''' and basic '''Fluid Dynamics '''concepts
* You should also be familiar with creation of a '''3D pipe Geometry''' in '''OpenFOAM'''
* If you are 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: Problem Setup
|| In this diagram, a '''section view''' of a '''3D pipe''' is shown.

This describes the '''problem statement'''.

* The '''diameter''' of the '''pipe''' is 1 centimeter and its '''length''' is 30 centimeters.
* It has one '''inlet''', one '''outlet''' and a '''cylindrical''' '''wall'''.

* The fluid here is water''' '''and its '''kinematic viscosity''' is taken as '''1e-06'''.

* The '''Inlet velocity '''is '''0.025 m/s '''and''' Outlet pressure '''is''' 0 Pascals '''as shown in the diagram.

|-
|| Slide: Geometry Check

Highlight '''250'''

Highlight''' laminar'''

Only Narration

Le = 0.06*Re*D

Highlight''' 0.15 m'''

|| Let us check whether our '''geometry''' is suitable or not.

* '''Reynolds number''' of the problem is '''250'''.

* Hence, the flow is '''laminar'''.

* For '''fully developed flow''', length of the '''geometry''' should be greater than the '''Entrance length'''.

* '''Entrance length''' can be calculated by this '''formula'''.

* The length we have taken is greater than the '''entrance length'''.
|-
|| Slide: Solver detail
|| * To simulate this problem, we will use the '''icoFoam''' solver.

* '''icoFoam''' is a''' transient solver''' for '''incompressible''', '''laminar flow''' of '''Newtonian fluids'''.

* This is the most '''suitable solver''' for '''Hagen Poiseuille flow.'''

|-
|| Slide : Pressure Boundary Condition
|| The''' Pressure boundary conditions''' used are,

* At '''inlet - zero gradient'''
* At '''outlet - fixed Pressure'''
* At '''wall - zero gradient'''

|-
|| Slide: Velocity Boundary Condition
|| The''' Velocity boundary condition''' used are,

* At '''inlet - fixed value'''
* At '''outlet - zero Gradient'''
* At '''wall - No Slip'''

|-
|| Only Narration
|| We will use the '''mesh''' that we have created in the tutorial “'''Creating 3D Pipe Geometry and Mesh in OpenFoam'''”.
|-
|| Press Ctrl + Alt + T keys
|| Open the '''terminal''' by pressing the '''Ctrl''', '''Alt''' and '''T''' keys together.
|-
|| [Terminal]

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

'''cd $FOAM_RUN'''
|| At the '''prompt''', type the following '''command''' to go to the '''run directory'''.

|-
|| [Terminal] Type:

'''cd pipe'''
|| Navigate to the '''pipe case folder'''.

|-
|| [Terminal] Type:

'''mv 0.Orig 0'''
|| Now, '''rename''' '''0.Orig''' folder to''' 0''' by typing this '''command'''.

|-
|| [Terminal] Type: '''gedit 0/p'''
|| Let’s open the “'''p'''” file in a '''text editor'''.
|-
|| [gedit - '''p'''] Highlight

'''dimensions [0 2 -2 0 0 0 0];'''
|| Here we can see, the '''p''' file is in the form of '''pressure divided by density'''.

This means, it is '''kinematic pressure'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''internalField''' to the end of the file as shown here.
|-
|| [gedit - '''pressure''']
|| Open the file '''pressure.txt''', that you had downloaded in any '''text editor'''.
|-
|| [gedit - '''pressure'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''p''']
|| Let me switch back to the “'''p”''' file.
|-
|| [gedit - '''p'''] '''Paste '''
|| Paste the copied contents into the “'''p” '''file as shown here.
|-
|| [gedit - '''p'''] Highlight

'''internalField'''
|| Right after '''dimensions''', we have to define the '''initial condition'''.

It could be '''uniform''', '''non-uniform''' or in the form of '''code'''.
|-
|| [gedit - '''p'''] Highlight

'''uniform 0;'''
|| In this case, we will use the '''initial condition''' as''' uniform 0'''.

This means that the '''kinematic pressure''' inside the entire '''domain''' is '''0'''.
|-
|| [gedit - '''p'''] Highlight

'''boundaryField'''
|| In the '''boundaryField''', we specify '''boundary conditions''' for all '''patches''' and '''walls'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| '''Boundary condition''' for '''inlet''' in '''pressure''' is defined as shown.
|-
|| [gedit - '''p'''] Highlight

'''type zeroGradient;'''
|| Type of the '''boundary condition''' is '''zeroGradient'''.

'''Zero Gradient boundary '''extrapolates the quantity to the '''patch''' from the nearest '''cell value'''.

So, the value at '''patch''' will be the same as the '''cell value'''.

Note that '''z''' is small and '''G''' is capital.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> wall'''
|| '''Boundary condition''' for the '''wall''' is defined as the same as '''inlet'''.
|-
|| [gedit - '''p'''] Highlight

'''Selection in the Text Editor >> outlet'''
|| '''Boundary condition''' for '''outlet''' in '''pressure''' is defined as shown here.
|-
|| [gedit - '''p'''] Highlight

'''type fixedValue;'''

'''value 0;'''
|| Type of '''boundary condition''' is '''fixedValue'''.

'''Value''' given is '''zero'''.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''p '''file and close the '''text editor'''.
|-
|| [Terminal] Type:

'''gedit 0/U'''
|| Now, let’s set the '''initial''' and '''boundary condition''' for '''velocity'''.

To do so, open the '''U''' file in a '''text editor'''.
|-
|| [gedit - '''U'''] Highlight

'''dimensions [0 1 -1 0 0 0 0];'''
|| '''Dimensions''' here are in '''meters per second'''.
|-
|| [gedit - '''U'''] Highlight

'''internalField uniform (0 0 0);'''
|| '''Velocity''' is a '''vector field''', so the '''internal initial field''' is set as '''uniform (0 0 0)'''.
|-
|| [gedit - '''U'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''boundaryField''' to the end of the file as shown here.
|-
|| [gedit - '''velocity''']
|| Open the '''velocity.txt '''file that you had downloaded in a '''text editor'''.
|-
|| [gedit - '''velocity'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.
|-
|| [gedit - '''U'''] '''Paste '''
|| Paste the copied contents into the “'''U” '''file as shown.
|-
|| [gedit - '''U'''] Highlight

'''boundaryField'''
|| In the '''boundaryField''', we will specify '''boundary conditions''' for all '''patches''' and '''walls'''.
|-
|| [gedit - '''U'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| '''Boundary condition''' for '''inlet''' in '''velocity''' is defined as shown here.
|-
|| [gedit - '''U'''] Highlight

'''type fixedValue;'''

'''value uniform (0 0 0.025);'''
|| Type of the '''boundary condition''' is '''fixedValue'''.

Value of '''velocity''' is 0.025 m/s in the '''Z direction'''.
|-
|| [gedit - '''U'''] Highlight

'''type noSlip;'''
|| '''Boundary condition''' for the '''wall''' is defined as '''noSlip'''.

This means '''velocity''' at the '''wall '''is '''0'''.
|-
|| [gedit - '''U'''] Highlight

'''type zeroGradient;'''
|| '''Boundary condition''' for '''outlet''' is '''zeroGradient''', defined as shown here.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''U '''file and close the '''text editor.'''
|-
|| [Terminal] Type:

'''gedit constant/transportProperties'''
|| Open '''transport properties''' file from '''constant folder''' in the '''text editor'''.
|-
|| [gedit - '''transportProperties'''] Highlight

'''nu'''
|| All '''properties''' of '''fluid''' which remain '''constant''' during the '''simulation''' is to be specified in the '''constant folder'''.

Here, we will set the value of '''kinematic viscosity'''.
|-
|| [gedit - '''transportProperties'''] Highlight

'''[0 2 -1 0 0 0 0]'''
|| Dimensions of '''kinematic viscosity''' are specified here.
|-
|| [gedit - '''transportProperties''']

'''Change: 0.01 >> 1e-06'''
|| To set the value of '''nu,''' replace '''0.01''' to '''1e-06'''.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''transportProperties '''file and close the '''text editor.'''
|-
|| Only Narration
|| '''Solve & write control parameters''' can be modified in the '''controlDict''' file.

The '''controlDict '''file is located in the '''system folder'''.
|-
|| [Terminal] Type:

'''gedit system/controlDict'''
|| Open the '''controlDict''' file in a '''text editor'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''Selection in the Text Editor >> Delete '''
|| Delete the lines from '''application''' to the end of the file as shown here.
|-
|| [gedit - '''control''']
|| Open the '''control.txt''' file that you had downloaded in a '''text editor'''.
|-
|| [gedit - '''control'''] Highlight

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

|| Paste the copied contents into the “'''controlDict” '''file as shown here.
|-
|| [gedit - '''controlDict'''] Highlight

'''application icoFoam;'''
|| First line of the '''controlDict''' file shows the name of the '''solver'''.

In our case it is '''icoFoam'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''startFrom startTime;'''

'''startTime 0;'''
|| The second and third lines are '''start simulation controls'''.

Our '''simulation''' will start from the value specified in '''start time'''.

Here our '''start time''' is set to '''0'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''stopAt endTime;'''

'''endTime 5;'''
|| The fourth and fifth lines are '''stop simulation controls'''.

'''Simulation''' will stop at the''' endTime''' of '''5 seconds'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''deltaT 1e-2;'''
|| Then the value of '''deltaT''' is given, which is '''1e-02'''.

So, it will '''simulate''' for '''5 seconds''' with a '''1e-02 time step'''.
|-
|| [gedit - '''controlDict'''] Highlight

'''writeInterval 100;'''
|| '''Write interval''' is 100. So it will print and save every 100 '''time-step value''' that '''OpenFOAM''' solves.

So we will get '''results''' written for 1, 2, 3, 4, and 5 seconds.
|-
|| [gedit - '''controlDict'''] Highlight

'''purgeWrite 2;'''
|| '''OpenFOAM''' gives the option to save only the last few '''time steps. '''

To enable that option, you can use the '''purgeWrite''' value.

By changing it to 2, we will get the 2 latest updated '''time-step''' results.

The old files will automatically be deleted.

At the end of the '''simulation''' we will get results of 4 & 5 seconds.

This option will save''' space''' on your computer.
|-
|| Only Narration
|| Rest of the options are for the format of writing''' data''' files in '''OpenFOAM'''.

We do not need to change them.

Therefore, we won’t be making any more changes to the '''controlDict''' file.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''controlDict '''file and close the '''text editor'''.
|-
|| Only Narration
|| We are done setting up the '''case'''.

Now we will '''run''' the '''simulation'''.
|-
|| [Terminal] Type: '''icoFoam'''
|| To do so, type '''icoFoam''' in the '''terminal''' and press '''Enter'''.
|-
|| Only Narration
|| It will take some time to '''simulate,''' based on your computer’s '''hardware'''.

For me it took around 4 minutes to '''simulate'''.
|-
|| [Terminal] Highlight

'''End'''
|| Once the '''simulation''' is finished, you will get this line at the end.
|-
|| Slide: Formula and Analytical Solution

Highlight '''2.4 Pa'''

Highlight '''0.05 m/s'''

||
* To calculate''' pressure '''at''' inlet,''' let’s put the values of the '''U, L, D '''and '''Po''' in this '''formula'''.

* We will get an '''inlet pressure''' value of '''2.4 Pascal'''.

* '''Maximum velocity''' will be twice of average '''velocity''' as per '''analytical solution'''.
|-
|| Slide: Result Comparison
||
* From the '''simulation''' we get,
** '''Maximum velocity''' 0.05 m/s and
** '''inlet Pressure 2.8 Pascals.'''

* In '''CFD''', there are always some deviations in results of '''analytical''' and '''numerical''' '''solutions'''.

* We will discuss '''results''' in detail later in this series.

|-
|| 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 the '''boundary''' and '''initial''' '''conditions'''
* Set up the '''physical properties'''
* Set up the '''solve & write control parameter '''and
* Run the '''simulation'''
|-
|| 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 Divyesh Variya.

And this is Swetha Sridhar from IIT Bombay signing off.

Thanks for joining.
|-
|}

OpenFOAM-version-7/C2/Creating-3D-Pipe-Geometry-and-Mesh-in-OpenFOAM/English

2020-07-20T15:04:25Z

Divyesh7: Created page with "'''Title of the script:''' Creating 3D Pipe Geometry and Mesh in OpenFOAM '''Author:''' Divyesh Variya '''Keywords:''' OpenFOAM, 3D-Geometry, Pipe, Meshing, ParaView, Pre-Pr..."

'''Title of the script:''' Creating 3D Pipe Geometry and Mesh in OpenFOAM

'''Author:''' Divyesh Variya

'''Keywords:''' OpenFOAM, 3D-Geometry, Pipe, Meshing, ParaView, Pre-Processing, Video-Tutorial, blockMesh

{| border="1"
|-
|| '''Visual Cue'''
|| '''Narration'''
|-
|| Slide: Opening slide
|| Welcome to this tutorial on '''Creating 3D Pipe Geometry and Mesh in OpenFOAM.'''
|-
|| Slide: Learning Objective
|| In this tutorial, we will learn to:

* Create a '''3D Geometry''' using '''blockMeshDict'''
* '''Mesh''' a '''3D''' '''geometry'''
* Label the''' boundary patches'''
* Check the '''mesh results '''using''' checkMesh command'''
* View the '''3D geometry''' and '''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
* '''gedit''' Text editor

You may use any other 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 creation of a basic '''geometry''' using the '''blockMesh''' utility.
* If you are 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: Hagen Poiseuille flow through a pipe
||
* In this tutorial, we will learn to create the '''geometry''' for '''Hagen Poiseuille flow through a pipe'''.
* The problem description of '''Hagen Poiseuille flow through a pipe''' is shown in the diagram.

|-
|| Slide: Pipe Geometry
||
* This is the diagram of the '''geometry''' for '''Hagen Poiseuille flow through a pipe.'''
* The left and right faces are the '''inlet''' and '''outlet''' respectively.
* The cylindrical face of the '''geometry''' is a '''wall'''.
* The '''diameter''' of the pipe is 1 centimeter and its '''length''' is 30 centimeters.

|-
|| 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'''.
|-
|| [Terminal] Type:

'''cp -r $FOAM_TUTORIALS/incompressible/icoFoam/cavity/cavity pipe'''
|| Let’s now copy the '''cavity case''' from the '''icoFoam''' '''tutorial directory''' to the '''run directory'''.

Type the following '''command''' to do so.
|-
|| [Terminal] Highlight: '''pipe'''
|| Note that the '''cavity case''' is copied to the '''pipe''' directory.
|-
|| [Terminal] Type:

'''mv pipe/0 pipe/0.Orig'''
|| In this tutorial we don’t need to define '''initial''' and '''boundary''' '''conditions''' in '''zero''' time.

Type this '''command''' to '''rename''' '''“0”''' folder to '''“0.Orig”'''
|-
|| [Terminal] Type:

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

Open this file in a '''text editor'''. I am doing it in the '''gedit text editor'''.
|-
|| [gedit - '''blockMeshDict''']
|| Now we can see the '''blockMeshDict''' file in the '''text editor.'''
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> Delete'''
|| '''Delete''' the lines from '''convertToMeters''' to the end of the file as shown here.

The remaining content is common for all '''blockMeshDict''' files.
|-
|| [gedit - '''pipe''']
|| Next, open the '''pipe.txt''' file that you had downloaded in the '''text editor'''.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> Copy'''
|| Copy the entire content of the text file.

|-
|| [gedit - '''blockMeshDict''']
|| Now switch back to the '''blockMeshDict''' file.
|-
|| [gedit - '''blockMeshDict''']

'''Paste '''
|| And paste the copied contents into the '''blockMeshDict '''file as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''0.01'''
|| Note that all the '''dimensions''' will be in '''centimeters'''.
|-
|| Slide: Vertices Detail
||
* '''Vertices''' are shown in the slide.
* Here we are going to use '''18''' '''vertices''' to define the '''geometry''' of a '''pipe'''.
* For example, '''two reference points''' 0 and 17 are on (0 0 0) and (0 0 30) respectively.

|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> vertices '''
|| All '''18''' '''points''' are defined in the '''vertices''' '''section''' in the '''blockMeshDict''' file as shown.
|-
|| Only Narration
|| Now let me switch back to the '''Slides'''.
|-
|| Slide: Block Detail
||
* Here we will use 5 '''hexahedral blocks''' to define the''' pipe geometry'''.
* As you can see, the '''center hexahedral block''' is separately shown in the '''figure''' on the right.
* To '''define''' this '''block''', we need to type the '''back plane’s vertices '''first.
* The '''vertices''' should be ordered''' anti-clockwise''' when viewed '''along the negative z-axis'''.
* The '''front plane’s vertices''' should also follow the same order.

|-
|| Slide: Block Detail

Highlight: '''hex (1 2 3 4 9 10 11 12) (8 8 80) simpleGrading (1 1 1)'''
|| An '''example''' is shown in the '''slide'''.

The same '''block''' can be defined correctly in more than one way.

|-
|| Slide: Block Detail

Highlight: '''(8 8 80)'''
|| To generate '''3D mesh''' we are using:

* '''8 cells''' in '''X direction''',
* '''8 cells '''in '''Y direction''' and
* '''80 cells''' in '''Z direction'''.

|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> blocks'''
|| Other '''4''' '''blocks''' are defined in the '''blockMeshDict''' file as shown.

|-
|| Slide: Geometry Arc Detail
|| For the '''curved geometry''', we need to define the '''edges'''.
|-
|| Slide: Geometry Arc Detail
||
* There are a total of '''16 arcs''' that we need to define.
* The '''arcs''' and the '''intermediate points''' are shown in the slide.
* Note that I have used the '''midpoint''' of the '''arc''' as the '''intermediate point'''.
* However, '''any other point''' through which the '''arc''' passes is acceptable.

|-
|| Slide: Geometry Arc Detail

Highlight: '''arc 5 6 (0 0.5 0)'''
|| For example, the''' edge''' from '''Point''' number '''5''' to '''6''' is passing through (0 0.5 0).
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> edges'''
|| All '''16''' '''arcs''' are defined in the '''edges''' '''section''' in the '''blockMeshDict''' file as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''arc 5 6 (0 0.5 0)'''
|| The '''curved edge''' connecting '''points 5''' and '''6''' is defined as shown.

|-
|| [gedit - '''blockMeshDict'''] Highlight

'''arc'''
|| The edge is an '''arc'''.

|-
|| [gedit - '''blockMeshDict'''] Highlight

'''5 6'''
|| Its two '''end''' '''points''' are 5 and 6.

|-
|| [gedit - '''blockMeshDict'''] Highlight

'''(0 0.5 0)'''
|| The '''coordinates''' of the '''point''' through which the '''arc''' passes through is 0, 0.5, 0

|-
|| Only Narration
|| Let’s label the '''boundary patches'''.

The '''boundary faces''' should be labelled appropriately.

The labels are used to impose '''boundary conditions''' on the respective faces.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> inlet'''
|| The '''inlet boundary''' is defined as shown.

|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >>'''
|| The''' inlet boundary''' has 5 faces.

These faces are defined as shown.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> outlet and wall'''
|| The '''outlet '''and''' wall boundary''' is defined as shown.

|-
|| Only Narration
|| Note that all '''boundaries''' have more than one face.
|-
|| [gedit - '''blockMeshDict'''] Highlight

'''Selection in the Text Editor >> mergePatchPairs'''
|| We do not have any '''patches '''or''' internal faces''' to merge.

Therefore, we leave the '''mergePatchPairs''' field empty.
|-
|| CTRL+S >> Close Text Editor
|| Now, save the '''blockMeshDict '''file and close the text editor.
|-
|| [Terminal] Type:

'''cd pipe'''
|| Now, go to the '''terminal''' and navigate to the '''pipe''' directory.
|-
|| [Terminal] Type:

'''blockMesh'''
|| Type '''blockMesh command''' and press '''Enter'''.

|-
|| [Terminal] Highlight

'''End'''
|| The '''meshing''' is now complete.

|-
|| [Terminal] Highlight

'''Patches section'''
|| As we can see in '''terminal results''', three patches are created.

|-
|| [Terminal] Type:

'''checkMesh'''
|| Now, let’s '''check''' '''mesh''' '''results''' and '''quality'''.

To do that type '''checkMesh''' in the '''terminal''' and press '''Enter'''.

Note that '''M '''in''' checkMesh''' is capital.
|-
|| Only Narration
|| We get the '''results''' printed of the '''mesh''' we created.
|-
|| [Terminal] Highlight

'''Max skewness = 0.6954 OK.'''

'''Non-orthogonality check OK.'''

'''Max aspect ratio = 30.3404 OK.'''

'''Overall domain bounding box '''
|| Here we can see:

* '''Skewness'''

* '''Orthogonality'''

* '''Aspect ratio'''

* '''Negative volume''' values if they are present

In our case, no negative volume is present.

* '''Bounding box '''coordinates and

|-
|| [Terminal] Highlight

'''Overall number of cells of each type:'''

'''hexahedra: 25600'''

'''prisms: 0'''

'''wedges: 0'''

'''pyramids: 0'''

'''tet wedges:0'''

'''tetrahedra:0'''

'''polyhedra: 0'''
||
* '''Number of cells''' with their '''types'''

|-
|| [Terminal] Type '''paraFoam'''

|| To view '''mesh''' in '''paraview''' type '''paraFoam''' and press '''Enter'''.
|-
|| [ParaView] Click

'''Apply'''
|| Click on '''Apply''' on the left side of your window in the '''Properties''' tab.

Now you can see '''pipe geometry''' in the''' Layout window'''.
|-
|| [ParaView] '''Rotate geometry'''
|| You can''' rotate''' geometry in the '''Layout''' '''window''' by pressing the left mouse button and dragging.
|-
|| [ParaView]

'''Click on Surface >> Click on Surface with Edges'''
|| Click on '''Surface''' available in the '''Active Variable Controls.'''

Then change it to '''Surface with Edges'''.
|-
|| [ParaView]

'''Click on vtkBlockColors >> SolidColor'''
|| Click on '''vtkBlockColors''' available in the '''Active Variable Controls.'''
and change it to '''SolidColor'''.

You can now see the '''mesh structure''' of '''pipe geometry''' that we created.
|-
|| [ParaView] '''Close ParaView'''
|| You can close the '''ParaView''' window.
|-
|| Only Narration
|| With this we have come to the end of the tutorial.

Let’s summarize.
|-
|| Slide: Summary
|| In this tutorial, we have learnt to,

* Create a '''3D Geometry''' using '''blockMeshDict'''
* Mesh a '''3D''' '''geometry'''
* Label the''' boundary patches'''
* Check the '''mesh results '''using''' checkMesh command'''
* View the '''3D geometry''' and '''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 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 Divyesh Variya.

And this is Swetha Sridhar from IIT Bombay signing off.

Thanks for joining.
|-
|}