OpenFOAM/C2/2D-Laminar-Flow-in-a-channel/English-timed

One line is said twice @08:35

Time	Narration
00:01	Hello and welcome to the spoken tutorial on Simulating 2D Laminar Flow in a Channel using openfoam
00:09	In this tutorial I will show you 2D geometry of channel Meshing the Geometry Solving and Post Processing results in Paraview and Validation using analytic result
00:25	To record this tutorial I am using Linux Operating system Ubuntu 12.04 . OpenFOAM version 2.1.1 ParaView version 3.12.0
00:39	Note that OpenFOAM version 2.1.1 is supported on ubuntu version 12.04
00:45	Hence forth all the tutorials will be covered using OpenFOAM version 2.1.1 and ubuntu version 12.04
00:56	As a Pre-requisite for this tutorial You should know how to create geometry using OpenFOAM
01:03	If not, please refer to the relevant tutorials on our website
01:09	we simulate flow in a channel to determine flow development length along the downstream Channel flow problem description
01:19	The boundary names and the inlet conditions are shown in this figure
01:26	The flow develpoment length is given by the formula L= 0.05 * Re * D
01:32	Re which is the Reynolds number and D which is the channel height
01:37	Using the formula length of the channel comes out to be 5 meters and height is kept as 1 meter.
01:45	The Inlet velocity is 1 meters per second And we are solving this for a Reynolds number ( Re ) equal 100
01:53	This is a steady state problem .Therefore we are using a steady state incompressible solver for this case
02:01	This is the file structure of our case the folder should be created in the solver type that we choose I have already created a folder in simpleFoam folder of incompressible flow solvers
02:18	The folder is named as channelNow let me switch to the folder
02:25	Copy 0,Constant and System folders of any other case file in the simpleFoam directory
02:34	I have copied the file structure of the case of pitzDaily
02:38	Paste it inside the channel folder and make the necessary changes in the geometry,boundary faces and boundary condition
02:48	Now let me open the command terminal
02:51	To do this press Ctrl+Alt +t keys simultaneously on your keyboard
02:57	In the terminal Type run and press enter
03:01	now type cd space tutorials and press enter
03:08	now type cd space incompressible and press enter
03:15	type cd space simpleFoam and press enter
03:20	now type cd channel and press enter
03:28	now type ls and press enter
03:33	You will see three folders 0 , Constant and System
03:37	now type cd constant and press enter
03:48	now type ls and press enter
03:52	In this you will see files containing properties of fluid and a folder named polymesh
03:59	RASProperties contains Reynolds-averaged stress model
04:03	transportProperties contain the transport model and kinematic viscosity that is (nu) in this case is set at 0.001 m²/s.
04:17	Now in terminal type cd polyMesh and press enter.Now type ls and press enter
04:30	You will see the blockMeshDict file here
04:33	To open up the blockMeshDict file in the terminal type gedit blockMeshDict and press enterScroll down
04:48	The geomery is in meters so the convertTometers is set to 1 next we have defined the vertices of the channel
04:59	We have used a 100 X 100 mesh size here and cell spacing is kept as ( 1 1 1 )
05:07	Next we have setup the boundary conditions and their types which are inlet ,outlet,top and bottom
05:19	As this is a 2D Geometry front And Back are kept as empty
05:27	Also this being a simple geometry mergePatchPair and edges are to be kept empty.Close the blockMeshDict file
05:38	In the command terminal Type cd space ..(dot dot) and press enter
05:44	Again type cd space .. (dot dot) and press enter
05:49	Now in the terminal type cd space 0 (Zero) and press enterNow Type ls and press enter
05:58	This contains the intial boundary conditions and wall functions for the channel case
06:05	It should contain various files such as epsilon ,k, nut,nuTilda which are the wall functionsand p , R and capital U which the are initial conditions of the flow
06:20	Let me switch back to the slides
06:24	Calculate k which is the turbulent kinetic energy from the formula given in the slide
06:29	Where Ux, Uy and Uz are the velocity components in the x, y and z direction And U' ( dash ) = 0.05 times u actual
06:43	Calculate epsilon from the formula given Where epsilon is the rate of disspiation turbulent energy C mu is a constant and its value is 0.09
06:56	And l is the length of the channel Let me minimise this
07:02	Change only the boundary names in each of the above folder
07:07	Note that the values of nut, nuTilda and R are to kept default
07:13	Rest of the files should contain initial value for each of the boundary faces
07:21	Now in the terminal Type cd (space) ..(dot dot) and press enter
07:27	There are no change to be done in the system folder
07:31	Now We need to mesh the geometry To do this In the command terminal type blockMesh and press enter
07:40	Meshing is done.Now Let me switch back to the slide
07:45	The type of solver we are using here is SimpleFoamIt is a Steady-state solver for incompressible, turbulent flow
07:55	let me minimise this
07:56	In the command terminal type simpleFoam and Press enter
08:03	Iterations running will be seen in the command terminal
08:07	Iterations running may take some time
08:11	The iterations will stop once the solution is converged or it reaches its end time value
08:16	To view the results in paraview in the terminal
08:20	type paraFoam and press enter.This will open up the paraview window
08:28	On let hand side of the paraview window click Apply.The geometry can be seen here.
08:35	On top of active variable control menu change the drop down menu from solid color to capital U
08:50	You can see the initial state of velocity magnitude at inlet.. On top of the paraview window click on theplay button of the VCR control
09:00	you can see the final value of the velocity magnitude
09:07	Also' toggle on the color legend from the left hand side top of active variable control menu'Click APPLY again
09:16	Now go to displayScroll down You can see Rescale, click on it
09:24	We can see that once the flow has fully developed it attains a maximum uniform velocity at the centerNow let me switch back to the slides
09:36	The results obtained can be validated with the analytical solution for laminar flow in achannel which is u(max)=1.5 Uavg
09:46	Using openfoam we obatain a velocity of 1.48 meters per second which is a good match.This brings us to the end of the tutorial
09:57	In this tutorial we learnt The File structure of channel Obtained solution using steady state solver Viewed the geometry in paraview 'Validation' with analytic results
10:08	As an assignment Solve the problem for Reynold Number 1500 and validate it with the analytical result
10:17	Watch The video available at this URL http://spoken-tutorial.org/What_is_a_Spoken_Tutorial It summarizes the Spoken Tutorial project. If you do not have good bandwidth, you can download and watch it.
10:28	The Spoken Tutorial Project Team Conducts workshops using spoken tutorials Gives certificates to those who pass an online test For more details, please write to contact@spoken-tutorial.org
10:42	Spoken Tutorials are part of Talk to a Teacher project, It is supported by the National Mission on Education through ICT, MHRD, Government of India.
10:52	More information on the same is available at the following URL link http://spoken-tutorial.org/NMEICT-Intro
10:57	This is Rahul Joshi from IIT BOMBAY signing off.Thanks for joining

Contributors and Content Editors

DeepaVedartham, PoojaMoolya, Pratik kamble, Sandhya.np14