View source for OpenFOAM-version-7/C3/Simulating-Flow-using-Cyclic-Conditions/English

Title of the script: Simulating flow using cyclic conditions

Author: Divyesh Variya, Abhushan Regmi 

Keywords: OpenFOAM, Channel flow, Cyclic condition, Paraview, Video-Tutorial.

{| border =1
|- 
|| '''Visual Cue'''
|| '''Narration'''
|-
||Slide: '''Opening Slide'''
||Welcome to this tutorial on '''Simulating flow using cyclic conditions'''.
|- 
|| Slide: '''Learning Objectives'''
|| In this tutorial, we will learn to,

* Setup ''' mesh ''' for a '''cyclic flow'''
* Setup ''' boundary conditions ''' for a '''cyclic flow'''
* Add ''' momentum source'''
* '''Simulate''' the case using '''pimpleFoam solver'''.

|- 
|| '''Slide''': 

'''System Specifications'''
|| To record this tutorial, I am using,

* '''Ubuntu Linux''' OS version 22.04
* '''OpenFOAM''' version 9
* '''ParaView''' version 5.6.0 and
* '''gedit Text Editor'''

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

'''Prerequisites'''

* If not, please go through the prerequisite '''OpenFOAM '''tutorial on https://spoken-tutorial.org

||To practise, this tutorial learner should have knowledge of,

* Basic Linux commands, and
* Basic knowledge of '''OpenFOAM ''' software
* If not, please go through the prerequisite '''OpenFOAM '''tutorials on this website.

|-
||'''Slide''': 

'''Cyclic Conditions'''
||'''Cyclic condition''' is a special '''periodic boundary condition'''.

It is often used in '''CFD''' when we have repetitive geometry for larger '''domains'''. 

Here we consider that both the ends of the geometry are connected.

Mainly two types of repetitive conditions can be seen.

# '''Rotational''' and
# '''Transitional'''

|-
||'''Slide''': 

'''Cyclic Conditions'''
||'''Rotational cyclic condition''' is helpful in '''turbomachinery''' applications.

'''Transitional cyclic conditions '''are helpful in simulating''' long pipes.'''

'''Cyclic conditions '''can help to save the '''computational time''' and ''' resources'''.
|-
||'''Slide''': 

'''Problem Statement'''
||As you can see, we have a '''2D channel geometry''' on the screen. 

Dimensions are 2 '''meter'''s in height and 4 '''mete'''rs in length. 

'''Reynolds number''' will be '''100''', so the case will be '''laminar'''.

In this case we will simulate '''cyclic conditions'''.

And compare '''computational time''' with '''traditional inlet-outlet''' condition cases.
|-
||'''Slide''': 

'''Analytical Solution'''
||From the input data, we can analytically calculate:

'''Entrance length''',

'''Maximum velocity ''', and

'''Pressure gradient'''.
|-
||'''Slide''': 

'''Solver & Base Tutorial'''
||We know that when we install '''OpenFOAM ''' some ''' benchmark cases''' come as '''tutorials'''. 

For a '''cyclic condition''', we have '''channel395''' case in '''pimpleFoam/LES''' location.

'''pimpleFoam''' solver is a '''Transient ''' solver for:
* '''Incompressible fluid'''
* '''Turbulent flow''' on a '''moving mesh'''. 

But it can also be used for ''' laminar flow''' with '''static mesh'''.
|-
||'''Slide''': 

'''Source Term'''
||When we use '''cyclic conditions''', two ends of the geometry are  connected.

To keep the fluid flowing, adding a constant force in the domain is necessary. 

This '''force''' can be applied using '''source terms''' in '''OpenFOAM'''.

We can give the '''mean velocity source''' in the '''fvConstraints''' file.

'''Syntax''' of the '''code''' is given in the slide for reference.

We shall explain the code later.
|-
||Only Narration
||Let’s copy the '''base case''' from the '''pimpleFoam tutorial''' to our local directory '''FOAM_RUN'''.
|-
||CTRL + ALT + T
||Open the '''terminal '''by pressing '''Ctrl''',''' Alt ''' and ''' T''' keys.
|-
|| [Terminal] Type:

'''cd $FOAM_RUN'''

'''cp -r $FOAM_TUTORIALS/incompressible/pimpleFoam/LES/channel395 $FOAM_RUN'''
|| Type these '''commands '''to go to the '''run''' folder and then copy the '''base case'''.
|-
|| [Terminal] Type:

'''cd channel395'''
||Go to the '''channel395 '''directory.
|-
|| [Terminal] Type:

'''rm -r 0 0.orig/k 0.orig/nu*'''
||The '''tutorial case''' we used is made for '''LES '''simulations.

There are a few unnecessary files to simulate a '''laminar '''case.

Hence, type this command to delete those files.
|-
||Only Narration
||Let’s first look at the '''blockMeshDict '''file.

Then setup '''geometry''' and '''mesh '''for our '''problem statement'''.
|-
|| [Terminal] Type:

'''gedit system/blockMeshDict'''
||Type the following command to open the '''blockMeshDict''' file in the '''text editor'''.
|-
|| [gedit] Change:

Here you need to mention from which number the changes have to be made.(0 0 '''2''') => (0 0 '''0.2''')

(4 0 '''2''') => (4 0 '''0.2''')

(0 1 '''2''') => (0 1 '''0.2''')

(4 1 '''2''') => (4 1 '''0.2''') 

(0 2 '''2''') => (0 2 '''0.2''') 

(4 2 '''2''') => (4 2 '''0.2''')

(40 25 '''30''') => (40 25 '''1''') 

(40 25 '''30''') => (40 25 '''1''') 
||As we can see, the entire geometry is made of '''2 blocks''' and it is '''3D geometry'''.

To convert it into 2D, we can simply change '''z-coordinates '''with '''0.2'''.

Also, don’t forget to make the '''number of cells''' in the '''z-direction''' '''<nowiki>= 1</nowiki>'''.

|-
||Point to the expansion ratio.
||By default, some '''expansion ratio''' is used to '''refine''' the '''mesh '''near the '''wall'''.

We will keep it as it is.
|-
||Point to the Top and Bottom walls part in the text editor.
||Here, our main focus is the '''boundary '''section.

As we can see, '''top''' and '''bottom walls '''were taken as '''wall '''types.
|-
||Point to the cyclic patches in the file.
||The '''cyclic patches''' can be defined as shown on the screen.

The type of the '''cyclic patch''' can be given as “'''cyclic'''.”

An additional entry needs to be added to define the '''neighbor patch'''.
|-
||Click on Save and Click on Close.
||Save the file and close it.
|-
||Only Narration
||To define '''boundary conditions''', we can go to the '''0.orig''' folder and modify the fields file.
|-
|| [Terminal] Type:

'''gedit 0.orig/U'''
||Let’s open the velocity file first.
|-
|| [gedit] Change:

internalField uniform ('''0.1335''' 0 0); '''<nowiki>=></nowiki>''' internalField uniform ('''1''' 0 0); 

Click on Save and Click on Close.
||Set up '''1 m/s velocity''' in the '''internal field''' to initialize the simulation. 

The other boundary conditions will be '''cyclic'''. 

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

'''gedit 0.orig/p'''

Click on Close

||In the same way, we have initialized the field with '''0 kinematic pressure''' in the '''p''' file.

The boundary conditions for other''' '''patches will be '''cyclic''' similar to that of '''U'''

Close the file.
|-
|| [Terminal] Type:

'''cp -r 0.orig 0'''
||Type the following command to make a clone of the 0.orig file with 0 name.
|-
|| [Terminal] Type:

'''gedit constant/transportProperties'''
||Now, we can set up '''kinematic viscosity''' in the '''transportProperties '''file from the '''constant''' folder.
|-
|| [gedit] Change:

'''nu 2e-05 => 0.02'''

'''Ubar 0.1335 => 1 '''

Click on Save and Click on Close
||Also, set the '''Ubar''' value in the x-direction to 

'''1 m/s'''.

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

'''gedit constant/momentumTransport'''

simulationType''' LES; => '''simulationType''' laminar; '''

Click on Save and Click on Close.


||In the''' momentumTransport '''file, we need to specify '''laminar''' type flow.

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

'''gedit system/controlDict '''

endTime''' 1000 => 15'''

deltaT''' 0.2 => 0.1'''

writeInterval''' 200 => 10'''

Click on Save and Click on Close

|| In the '''controlDict '''file, let's set '''endTime '''equal''' to 15 seconds'''. 

Also, set '''deltaT '''equals '''0.1 '''and''' writeInterval 10'''.

Save and close the file.

|-
|| [Terminal]:

Only Narration
||Our case setup is almost ready. 

But here, we haven't specified any '''force''' to drive fluid in our system.

It is necessary to provide an '''external force''' in our system to keep''' fluid flowing'''.

To add a specific type of '''external force''', we can use the '''fvConstraints '''utility in '''OpenFOAM'''.
|-
|| [Terminal] Type:

'''gedit system/fvConstraints'''
||The '''fvConstraints '''file is located in a '''constant '''or '''system '''folder. 

Here, in this '''tutorial''', it is located under the '''system '''folder. 

Open it in a text editor using the following command.
|-
|| [gedit fvConstraints]:

Point to '''momentumForce'''
|| In this dictionary we are providing '''momentumSource '''as a '''Source'''
|-
|| [gedit fvConstraints]:

Point to''' type'''
||We are providing '''meanVelocityForce'''

This applies a force to maintain a user-specified '''volume-averaged mean velocity'''
|-
|| [gedit fvConstraints]:

Point to '''SelectionMode'''
||Here we are selecting all '''cells''' of the '''domain'''
|-
|| [gedit fvConstraints]:

Point to '''fields and Ubar'''
||We are providing this source term to the '''field''' '''velocity'''.

We will provide mean velocity of '''1m/s '''in the x-direction.

Also, we will get a '''parabolic velocity profile''' in the domain.
|-
|| [gedit] Change:

Ubar ('''0.1335 '''0 0); '''<nowiki>=> </nowiki>'''

Ubar ('''1''' 0 0); 

Click on Save and Click on Close.
||Change '''Ubar''' value from '''0.1335 '''to '''1'''.

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

'''blockMesh'''

'''pimpleFoam'''
||Let us run simulation commands.

First type '''blockMesh '''for '''meshing '''and then '''pimpleFoam '''to run the '''simulation'''.
|-
|| [Terminal] Type:

'''paraFoam'''
|| In just a few seconds, the simulation is finished.

Let us open our case in '''ParaView '''using the '''paraFoam '''command.
|-
|| [ParaView] '''Properties''' '''Tab'''

Click on '''Apply''' button
||Click on the '''apply '''button and see the '''velocity field'''.
|-
|| [ParaView] 

'''VCR Controls''' '''<nowiki>=></nowiki>''' Click on '''Last Frame '''



'''&&'''

'''Active Variable Controls => '''Click on''' vtkBlockColors ==> Click on''' a''' box icon'''



||On the top of the screen, click on the '''last frame''' as shown.

Click on''' vtkBlockColors '''on the top-left and from the drop down menu select''' U''' with '''box icon'''

|-
|| [ParaView]

Showing Velocity Contour

||As you can see, we have the same '''profile '''or '''velocity distribution '''all over the domain.
|-
|| [ParaView] 

'''Data Analysis =>''' Click on '''plot over line filter'''



||Now, let us check the '''velocity profile '''over '''radial distance'''.

Click on the''' plot over line''' icon located on top of the screen as shown.
|-
|| [ParaView] 

'''Properties''' '''Tab =>''' Click on '''y-axis'''

'''&&'''

'''Properties''' '''Tab =>''' Click on '''Apply '''
||Click on the y-axis and then click on the Apply''' button.'''

As we can see, it is parabolic.

The''' maximum velocity''' is '''1.5 m/s'''.
|-
||where is the analytic solution? 

Point to it, instead writing only Narration.Only Narration
||Now, let us compare our result with the '''analytical solution'''.
|- 
|| Slide: '''Result Comparison'''
|| From the comparison we can find the following.

'''Cyclic condition''' results exactly match the '''analytical solution''' and '''full-length channel case'''.

The ''' time consumed''' to simulate '''cyclic cases''' is less than the '''entire domain case'''.
|- 
|| '''Slide''': 

'''Summary'''
|| In this tutorial, we have learned to,

* Setup''' mesh '''for''' cyclic flow'''
* Setup''' boundary conditions ''' for '''cyclic flow'''
* Add ''' momentum source'''
* '''Simulate''' the case using '''pimpleFoam solver'''.
|-
||'''Slide''': 

'''Assignment'''
||As an assignment:

* Simulate two cases using the same geometry with velocity 0.002 m/s.
* One with the '''cyclic condition''' and,
* Second without '''cyclic condition'''
* Compare both results with '''analytical solution'''
* Note time difference to run both cases

|-
||'''Slide''': 

'''About the Spoken Tutorial Project'''
||The video at the following link summarizes 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 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 the Ministry of Education, Govt. of India.

This tutorial is contributed by Divyesh Varya, Aabhushan Regmi and Payel Mukherjee from IIT Bombay. Thank you for joining.
|-
|}