OpenFOAM/C3/Simulating-Hagen-Poiseuille-flow/English

Tutorial: To simulate Hagen-Poiseuille flow in OpenFOAM.

Script and Narration : Saurabh S. Sawant

Keywords: Video tutorial,CFD.

Visual Cue	Narration
Slide 1:	Hello and welcome to the spoken tutorial on simulating Hagen-Poiseuille flow in OpenFOAM
Slide 2 : Learning Objectives	In this tutorial we will see: To create and mesh 3D cylindrical pipe To simulate the Hagen-Poiseuille flow having fixed pressure ratio across boundaries and To visualize the velocity contour in ParaView
Slide 3: System Requirement	To record this tutorial, I am using Linux Operating system Ubuntu 12.04 OpenFOAM version 2.1.1 and ParaView version 3.12.0
Slide 4: System Requirement The tutorials were recorded using the versions specified in previous slide Subsequently the tutorials were edited to latest versions To install latest system requirements go to Installation Sheet
Slide 5: Prerequisites	To practice this tutorial learner should have the knowledge of Basic Fluid Dynamics and Hagen-Poiseuille flow
Slide 6: Hagen-Poiseuille Flow Diagram Read aloud the given points and show the contents in the diagram with the mouse pointer.	Here is, Hagen-Poiseuille Flow diagram. We can see the dimensions and boundaries of the pipe. Viscosity of the fluid used, that is, water is given. Pressure at the inlet is 20 Pascals and at the outlet it is 0 Pascals. As it is an incompressible flow, only the pressure difference is of importance.
Slide 7: Formulas and Analytical Solution Read aloud the given points	Formulas and Analytical Solution: For Hagen-Poiseuille flow, Pressure drop along the pipe is: (P1 minus P2) equals (32 mu Uaverage L) upon (D square) By substituting the values from the previous diagram, we get, Uaverage equals to 0.208 m/s Maximum Velocity is given as, Two times the average velocity, which would be, 0.416 m/s Reynolds Number for the flow is, Uaverage into D upon nu, that comes out to be, 2080 Hence, the flow is transient.
Slide 8: Solver	Type of solver used here is icoFOAM. It is a Transient Solver. It is used for incompressible, laminar flow of Newtonian fluid.
Slide 9: Pressure Boundary Conditions	Pressure Boundary Conditions used, At Inlet: fixedPressure At Outlet: fixedPressure At Walls: ZeroGradient
Slide 10: Velocity Boundary Conditions	Velocity Boundary Conditions used, At Inlet: pressureInletVelocity At Outlet: zeroGradient At Walls: fixedValue
Show 3dpipe folder. Show the 3dpipe folder	For executing this case, first let's create the case directory in the 'icoFoam' folder. And give it some name. I have named it as '3dpipe'.
Point the mouse pointer from lid driven folder to 3d pipe folder.	To know the location of this folder, go through the tutorial on lid driven cavity. Copy this '0' (zero), 'constant' and 'system' folders of lid driven cavity problem in the newly created folder.
Go inside the 3dpipe folder.	Let's go inside the '3dpipe' folder.
Hover the pointer over the folder inside the 3dpipe folder.	I have already copied the folders into my '3dpipe' folder and modified the files in it.
Go into the '0' folder and open P file and show it	Now, let's go into the '0' folder and open the 'P' file. This is the pressure boundary condition file.
Show the pressure boundary condition file and show the dimensions inside it.	Note that the dimensions are in (meter square) per (second square) (m2/s2).
Show the pressure value written	Hence the pressure value in Pascals is divided by the density, that is, 1000 Kg/m3 (Kg per meter cube), and written here.
Close the file	Let's close the file.
Open U file in the same folder and show.	File containing the velocity boundary condition is as seen. Let's open the file we can see the velocity boundary condition for inlet, outlet and fixed walls.
Close the file and come out of the '0' folder.	Let's close the file and come out of the '0' folder.
Switch back to the slides.	To see the blocking strategy, let me switch back to the slides.
Slide 11: Blocking Strategy Hover the pointer on the geometry and drag it towards the z direction.	To create a 3D geometry of a pipe I have made a 2D circular geometry and extruded the length in z direction.
Point out the numbering pattern.	Numbering pattern is as shown. We can also see the dimension of the mesh.
Minimize the slides	To see the blockMeshDict file, let's minimize the slides.
Go to folder 'constant' and then 'polyMesh' and open blockMeshDict file and show it.	Let's go into the folder 'constant', and then 'polyMesh'. Let's open theblockMeshDict ' file. We can see the vertices, blocks,edges and boundaries for inlet, outlet and fixed walls.
Close the file and come out of the folder 'polyMesh	Let's close the file and lets come out of the 'polyMesh' folder.
Open and show transportProperties file and point at the value viscosity value	We see the 'transportProperties'file. Lets open the file. Note the dynamic viscosity value, here is 1 into 10 raise to minus 6.
Close the file and come out of the 'constant' folder.	Let's close the file and come out of the folder constant.
Go into the system folder and open the controlDict file. Show it.	Let's go into the 'system' folder. Now, let's have a look at the 'controlDict' file.
Show time step value	The solution converges after 18 seconds therefore the final time step is kept 19. The time step has been set to 1 into 10 raise to minus 3.
Close the file and the Home folder.	Let's close the file. Let's close the 'Home' folder.
Press 'Control', 'Alt' and 'T' keys altogether.	Now to execute the case, we will first go inside the '3dpipe' folder through terminal. Let's open the terminal by pressing 'Control', 'Alt' and 'T' key altogether.
Type run and press Enter in the terminal.	Type run and press Enter.
Type cd (space) tutorials and press Enter.	Type cd (space) tutorials and press Enter.
Type cd (space) incompressible and press Enter	Type cd (space) incompressible and press Enter.
Type cd (space) icoFoam and press Enter	Type cd (space) icoFoam and press Enter.
Type cd (space) 3dpipe and press Enter	Type cd (space) 3dpipe and press Enter.
Type blockMesh and press Enter	Now to create the mesh, type blockMesh and press Enter. Meshing has been done.
After the meshing is done, type icoFoam to start the iterations	To start the iterations type icoFoam and press Enter . We see the iterations are running.
After the iterations are done, type paraFoam for postprocessing the results and press Enter.	Iterations has been done. After the iterations end, type paraFoam for postprocessing the results and press Enter. It will open the" ParaView". This is " ParaView".
Click on Apply.	Let's click on Apply on the left hand side of the Object inspector menu to see the geometry.
Rotate the geometry by pressing the button of the mouse and move it in the required direction.	Let's rotate the geometry for a better view.
Click on the active variable control menu and select U in the drop-down menu	Click on the active variable control menu and select U in the drop-down menu.
Click on play button	At the top, in VCR toolbar, click on Play button.
Go to Object Inspector menu, go to Display, click on Rescale data range	Go to Object Inspector menu, go to Display, click on Rescale to data range.
go to the toolbar named common, click on Clips and press Apply	To view the half section, go to the toolbar named common, click on Clips. Go to Object Inspector menu properties and press Apply. Let's zoom in.
Open the color legend	Let's open the color legend.
	We can see the maximum velocity is near to the actual maximum velocitythat is 0.40 meters per second.
Go to Filters> Data Analysis> Plot Over Lines	To view the graph go to Filters at the top, Data Analysis and press Plot Over Line.
Click on Y axis and press Apply	Press Y axis and press Apply.
Point towards the parabolic profile	We can see the parabolic profile for Hagen-Poiseuille flow.
Close the graph	Let's close the graph.
Close ParaView	Let's close ParaView.
Switch to the slides	And switch to the slides.
Slide 12: Summary	In this tutorial we have learnt: To create and mesh 3D pipe geometry To simulate Hagen-Poiseuille flow for a fixed pressure ratio across boundaries and To visualize the velocity results in Parafoam
Slide 13 : Assignment	As an assignment, Change the geometry parameters such as length and diameter Change the corresponding pressure ratio and Use the fluid of different viscosity
Slide 14: About Spoken tutorials	Watch the video available at the following link It summarises the Spoken Tutorial project If you do not have good bandwidth, you can download and watch it
Slide 15: About Spoken tutorials	The Spoken Tutorial Project Team Conducts workshops using spoken tutorials Gives certificates for those who pass an online test For more details, please write to contact at spoken hyphen tutorial dot org
Slide 16: Forum to answer questions Do you have questions on THIS Spoken Tutorial? Choose the minute and second where you have the question Explain your question briefly Someone from the FOSSEE team will answer them. Please visit http://forums.spoken-tutorial.org/
Slide 17: Forum to answer questions Questions not related to the Spoken Tutorial? Do you have general/technical questions on the Software? Please visit the FOSSEE forum http://forums.fossee.in/ Choose the Software and post your question
Slide 18: Lab Migration project We coordinate migration from commercial CFD software like ANSYS to OpenFOAM We conduct free Workshops and provide solutions to CFD Problem Statements in OpenFOAM For more details visit this site: http://cfd.fossee.in/
Slide 19: Case Study project We invite students to solve a feasible CFD problem statement of reasonable complexity using OpenFOAM We give honorarium and certificate to those who do this For more details visit this site: http://cfd.fossee.in/
Slide 20: Acknowledgement	Spoken Tutorial Project is a part of the Talk to a Teacher project It is supported by the National Mission on Education through ICT, MHRD, Government of India More information on this Mission is available at spoken hyphen tutorial dot org slash NMEICT hyphen Intro

Contributors and Content Editors

DeepaVedartham, Nancyvarkey, P12575, Sneha