# Difference between revisions of "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

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

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
Slide 10:

Velocity Boundary Conditions

Velocity Boundary Conditions used,
• At Inlet: pressureInletVelocity
• 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

• 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
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
• 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