Skill-Lync Launch Pad – Your Gateway to a Core Engineering Job by 2025! Only 1̶0̶0̶ +50 Seats Available.

04D 11H 21M 34S

Menu

Executive Programs

Workshops

Projects

Blogs

Careers

Placements

Student Reviews

For Business

More

Academic Training

Informative Articles

Find Jobs

We are Hiring!

All Courses

Choose a category

Mechanical

Electrical

Civil

Computer Science

Electronics

Offline Program

All Courses

All Courses

logo

CHOOSE A CATEGORY

Mechanical

Electrical

Civil

Computer Science

Electronics

Offline Program

Top Job Leading Courses

Automotive

CFD

FEA

Design

MBD

Med Tech

Courses by Software

Design

Solver

Automation

Vehicle Dynamics

CFD Solver

Preprocessor

Courses by Semester

First Year

Second Year

Third Year

Fourth Year

Courses by Domain

Automotive

CFD

Design

FEA

Tool-focused Courses

Design

Solver

Automation

Preprocessor

CFD Solver

Vehicle Dynamics

Machine learning

Machine Learning and AI

POPULAR COURSES

coursePost Graduate Program in Hybrid Electric Vehicle Design and Analysis
coursePost Graduate Program in Computational Fluid Dynamics
coursePost Graduate Program in CAD
coursePost Graduate Program in CAE
coursePost Graduate Program in Manufacturing Design
coursePost Graduate Program in Computational Design and Pre-processing
coursePost Graduate Program in Complete Passenger Car Design & Product Development
Executive Programs
Workshops
For Business

Success Stories

Placements

Student Reviews

More

Projects

Blogs

Academic Training

Find Jobs

Informative Articles

We're Hiring!

phone+91 9342691281Log in
  1. Home/
  2. Jaswanth Kalyan Kumar Alapati/
  3. Week 11 - Simulation of Flow through a pipe in OpenFoam

Week 11 - Simulation of Flow through a pipe in OpenFoam

The following is the simulation of a laminar flow of an incompressible fluid through the pipe in OpenFoam.  The following figure depicts the physical situation of the flow. For a laminar flow, the hydrodynamic length, Lh=0.06⋅D⋅ReDLh=0.06⋅D⋅ReD, where DD is pipe diameter, and ReDReD is Reynolds number…

  • CFD
  • MATLAB

  • Jaswanth Kalyan Kumar Alapati

    updated on 07 Jan 2022

The following is the simulation of a laminar flow of an incompressible fluid through the pipe in OpenFoam. 

The following figure depicts the physical situation of the flow.

For a laminar flow, the hydrodynamic length, Lh=0.06⋅D⋅ReDLh=0.06⋅D⋅ReD, where DD is pipe diameter, and ReDReD is Reynolds number based on diameter.

Flow parameters:

DD = 20 mm, LL (pipe length) = 3000 mm, and ReDReD = 2100. Fluid is the water of density (ρρ) = 996.59 kgm3kgm3 and viscosity (μμ) = 0.000852 kgm−skgm-s. The inlet velocity (VV) is determined as VV = ReD⋅μρ⋅DReD⋅μρ⋅D = 0.089766102 msms. 

Transient analysis of flow is performed using the icoFoam solver. The fluid domain for the simulation is prepared using blockMesh as follows. The wedge angle used is 3030.

 

A MATLAB file (attached below) is created to write the blockMesh file for different flow parameters.

scale=0.001;
R=10;                                % In mm
theta=3;                             % In degrees
x=3000;                              % Length of pipe in mm
y=R*cos((theta/2)*pi/180);           % y coordinate of corner points in mm
z=R*sin((theta/2)*pi/180);           % z coordinate of corner points in mm
nx=3000;                             % no of cells along pipe length
ny=40;                               % no of cells along radial direction
gradef=0.1;                          % grading factor in radial direction

f=fopen('blockMeshDict.txt','w');
fprintf(f,'%s','/*--------------------------------*- C++ -*----------------------------------*\');
fprintf(f,'\n%s','| =========                 |                                                 |');
fprintf(f,'\n%s','| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |');
fprintf(f,'\n%s','|  \\    /   O peration     | Version:  v2012                                 |');
fprintf(f,'\n%s','|   \\  /    A nd           | Website:  www.openfoam.com                      |');
fprintf(f,'\n%s','|    \\/     M anipulation  |                                                 |');
fprintf(f,'\n%s','\*---------------------------------------------------------------------------*/');
fprintf(f,'\n%s','FoamFile');
fprintf(f,'\n%s','{');
fprintf(f,'\n%s','    version     ');
fprintf(f,'%.1f',2.0);
fprintf(f,'%s',';');
fprintf(f,'\n%s','    format      ');
fprintf(f,'%s','ascii;');
fprintf(f,'\n%s','    class       ');
fprintf(f,'%s','dictionary;');
fprintf(f,'\n%s','    object      ');
fprintf(f,'%s','blockMeshDict;');
fprintf(f,'\n%s','}');
fprintf(f,'\n%s','// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //');
fprintf(f,'\n');
fprintf(f,'\n%s','scale   ');
fprintf(f,'%.3f%s',scale,';');
fprintf(f,'\n');
fprintf(f,'\n%s','vertices');
fprintf(f,'\n%s','(');
fprintf(f,'\n%s%d %d %d%s','    (',0,0,0,')');
fprintf(f,'\n%s%d %.8f %.9f%s','    (',0,y,-1*z,')');
fprintf(f,'\n%s%d %.8f %.9f%s','    (',0,y,z,')');
fprintf(f,'\n%s%d %d %d%s','    (',x,0,0,')');
fprintf(f,'\n%s%d %.8f %.9f%s','    (',x,y,-1*z,')');
fprintf(f,'\n%s%d %.8f %.9f%s','    (',x,y,z,')');
fprintf(f,'\n%s',');');
fprintf(f,'\n');
fprintf(f,'\n%s','blocks');
fprintf(f,'\n%s','(');
fprintf(f,'\n    %s','hex (');
fprintf(f,'%d %d %d %d %d %d %d %d%s',0,3,4,1,0,3,5,2,')');
fprintf(f,' %s%d %d %d%s','(',nx,ny,1,')');
fprintf(f,' %s','simpleGrading');
fprintf(f,' %s%d %.1f %d%s','(',1,gradef,1,')');
fprintf(f,'\n%s',');');
fprintf(f,'\n');
fprintf(f,'\n%s','edges');
fprintf(f,'\n%s','(');
fprintf(f,'\n    %s','arc ');
fprintf(f,'%d %d',1,2);
fprintf(f,' %s%d %d %d%s','(',0,R,0,')');
fprintf(f,'\n    %s','arc ');
fprintf(f,'%d %d',4,5);
fprintf(f,' %s%d %d %d%s','(',x,R,0,')');
fprintf(f,'\n%s',');');
fprintf(f,'\n');
fprintf(f,'\n%s','boundary');
fprintf(f,'\n%s','(');
fprintf(f,'\n    %s','inlet');
fprintf(f,'\n    %s','{');
fprintf(f,'\n        %s','type patch;');
fprintf(f,'\n        %s','faces');
fprintf(f,'\n        %s','(');
fprintf(f,'\n            %s%d %d %d %d%s','(',0,2,1,0,')');
fprintf(f,'\n        %s',');');
fprintf(f,'\n    %s','}');
fprintf(f,'\n    %s','wall');
fprintf(f,'\n    %s','{');
fprintf(f,'\n        %s','type wall;');
fprintf(f,'\n        %s','faces');
fprintf(f,'\n        %s','(');
fprintf(f,'\n            %s%d %d %d %d%s','(',1,2,5,4,')');
fprintf(f,'\n        %s',');');
fprintf(f,'\n    %s','}');
fprintf(f,'\n    %s','axis');
fprintf(f,'\n    %s','{');
fprintf(f,'\n        %s','type empty;');
fprintf(f,'\n        %s','faces');
fprintf(f,'\n        %s','(');
fprintf(f,'\n            %s%d %d %d %d%s','(',0,3,3,0,')');
fprintf(f,'\n        %s',');');
fprintf(f,'\n    %s','}');
fprintf(f,'\n    %s','front');
fprintf(f,'\n    %s','{');
fprintf(f,'\n        %s','type wedge;');
fprintf(f,'\n        %s','faces');
fprintf(f,'\n        %s','(');
fprintf(f,'\n            %s%d %d %d %d%s','(',0,3,5,2,')');
fprintf(f,'\n        %s',');');
fprintf(f,'\n    %s','}');
fprintf(f,'\n    %s','back');
fprintf(f,'\n    %s','{');
fprintf(f,'\n        %s','type wedge;');
fprintf(f,'\n        %s','faces');
fprintf(f,'\n        %s','(');
fprintf(f,'\n            %s%d %d %d %d%s','(',0,1,4,3,')');
fprintf(f,'\n        %s',');');
fprintf(f,'\n    %s','}');
fprintf(f,'\n    %s','outlet');
fprintf(f,'\n    %s','{');
fprintf(f,'\n        %s','type patch;');
fprintf(f,'\n        %s','faces');
fprintf(f,'\n        %s','(');
fprintf(f,'\n            %s%d %d %d %d%s','(',3,4,5,3,')');
fprintf(f,'\n        %s',');');
fprintf(f,'\n    %s','}');
fprintf(f,'\n%s',');');
fprintf(f,'\n');
fprintf(f,'\n%s','mergePatchPairs');
fprintf(f,'\n%s','(');
fprintf(f,'\n%s',');');
fprintf(f,'\n');
fprintf(f,'\n%s','// ************************************************************************* //');
fprintf(f,'\n');
fclose(f);

The blockMesh file generated is as follows. 

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2012                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

scale   0.001;

vertices
(
    (0 0 0)
    (0 9.99657325 -0.261769483)
    (0 9.99657325 0.261769483)
    (3000 0 0)
    (3000 9.99657325 -0.261769483)
    (3000 9.99657325 0.261769483)
);

blocks
(
    hex (0 3 4 1 0 3 5 2) (3000 40 1) simpleGrading (1 0.1 1)
);

edges
(
    arc 1 2 (0 10 0)
    arc 4 5 (3000 10 0)
);

boundary
(
    inlet
    {
        type patch;
        faces
        (
            (0 2 1 0)
        );
    }
    wall
    {
        type wall;
        faces
        (
            (1 2 5 4)
        );
    }
    axis
    {
        type empty;
        faces
        (
            (0 3 3 0)
        );
    }
    front
    {
        type wedge;
        faces
        (
            (0 3 5 2)
        );
    }
    back
    {
        type wedge;
        faces
        (
            (0 1 4 3)
        );
    }
    outlet
    {
        type patch;
        faces
        (
            (3 4 5 3)
        );
    }
);

mergePatchPairs
(
);

// ************************************************************************* //

Boundary conditions are as follows.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2012                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 101.6717005;

boundaryField
{
    inlet
    {
        type            zeroGradient;
    }

    wall
    {
        type            zeroGradient;
    }

    axis
    {
        type            empty;
    }

    front
    {
	type		wedge;
    }

    back
    {
	type		wedge;
    }

    outlet
    {
        type            fixedValue;
	value		uniform 101.6717005;
    }
}

// ************************************************************************* //

 

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2012                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    inlet
    {
        type            fixedValue;
        value		uniform (0.089766102 0 0);
    }

    wall
    {
        type            noSlip;
    }

    axis
    {
        type            empty;
    }

    front
    {
	type		wedge;
    }

    back
    {
	type		wedge;
    }

    outlet
    {
        type            zeroGradient;
    }
}

// ************************************************************************* //

The controlDict is as follows.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2012                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     icoFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         40;

deltaT          0.005;

writeControl    runTime;

writeInterval   2;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;


// ************************************************************************* //

The simulation reached a steady state at the time, tt = 26 s.

Analytically, the hydrodynamic length, LhLh = 0.06*2100*0.02 = 2.52 mm.

The velocity (magnitude) distribution along the axial direction at steady state is obtained as follows.

From the above plot, the velocity profile is fully developed approximately at x = 2.5 m.

Radial distributions of velocity at x = 2.8 m.

Radial distributions of velocity at x = 3 m.

At the inlet, velocity is mentioned. At outlet, pressure is mentioned.

Maximum velocity (at the centerline) through simulation is 0.1784 msms while the analytical value is 0.1795 msms.

Leave a comment

Thanks for choosing to leave a comment. Please keep in mind that all the comments are moderated as per our comment policy, and your email will not be published for privacy reasons. Please leave a personal & meaningful conversation.

Please  login to add a comment

Other comments...

No comments yet!
Be the first to add a comment

Read more Projects by Jaswanth Kalyan Kumar Alapati (8)

Week 1- Mixing Tee

Objective:

This assignment aims to evaluate the mixing effectiveness of a Tee joint with two different outlet pipe lengths, namely small and long. The required Tee geometry is provided, and the interior volume for CFD analysis is extracted as shown below.    Tee geometry with shorter outlet pipe:  Extracted…

calendar

03 Sep 2022 08:13 PM IST

  • CFD
Read more

Week 12 - Validation studies of Symmetry BC vs Wedge BC in OpenFOAM vs Analytical H.P equation

Objective:

Unlike in the previous assignment, where the simulation is performed using a transient solver icoFoam, the simulation is carried out using a steady-state solver simpleFoam since the emphasis is on the steady-state flow field.  This assignment aims to compare the boundary conditions of Wedge and Symmetry…

calendar

11 Jan 2022 11:09 AM IST

    Read more

    Week 11 - Simulation of Flow through a pipe in OpenFoam

    Objective:

    The following is the simulation of a laminar flow of an incompressible fluid through the pipe in OpenFoam.  The following figure depicts the physical situation of the flow. For a laminar flow, the hydrodynamic length, Lh=0.06⋅D⋅ReDLh=0.06⋅D⋅ReD, where DD is pipe diameter, and ReDReD is Reynolds number…

    calendar

    07 Jan 2022 10:13 AM IST

    • CFD
    • MATLAB
    Read more

    Week 9 - FVM Literature Review

    Objective:

    Finite Volume Method (FVM) is a numerical technique for solving partial differential equations governing the phenomena. The method involves discretizing the domain into smaller volumes. These control volumes are connected by common faces. The governing equation in integral form is applied for all the control volumes followed…

    calendar

    26 Dec 2021 07:15 AM IST

      Read more

      Schedule a counselling session

      Please enter your name
      Please enter a valid email
      Please enter a valid number

      Related Courses

      coursecardcoursetype

      Post Graduate Program in CFD Solver Development

      4.8

      119 Hours of Content

      coursecard

      Introduction to OpenFOAM Development

      4.9

      18 Hours of Content

      coursecardcoursetype

      Post Graduate Program in Battery Technology for Mechanical Engineers

      4.8

      81 Hours of Content

      coursecard

      Simulation and Design of Power Converters for EV using MATLAB and Simulink

      4.9

      22 Hours of Content

      coursecard

      Introduction to Hybrid Electric Vehicle using MATLAB and Simulink

      4.8

      23 Hours of Content

      Schedule a counselling session

      Please enter your name
      Please enter a valid email
      Please enter a valid number

      logo

      Skill-Lync offers industry relevant advanced engineering courses for engineering students by partnering with industry experts.

      https://d27yxarlh48w6q.cloudfront.net/web/v1/images/facebook.svghttps://d27yxarlh48w6q.cloudfront.net/web/v1/images/insta.svghttps://d27yxarlh48w6q.cloudfront.net/web/v1/images/twitter.svghttps://d27yxarlh48w6q.cloudfront.net/web/v1/images/youtube.svghttps://d27yxarlh48w6q.cloudfront.net/web/v1/images/linkedin.svg

      Our Company

      News & EventsBlogCareersGrievance RedressalSkill-Lync ReviewsTermsPrivacy PolicyBecome an Affiliate
      map
      EpowerX Learning Technologies Pvt Ltd.
      4th Floor, BLOCK-B, Velachery - Tambaram Main Rd, Ram Nagar South, Madipakkam, Chennai, Tamil Nadu 600042.
      mail
      info@skill-lync.com
      mail
      ITgrievance@skill-lync.com

      Top Individual Courses

      Computational Combustion Using Python and CanteraIntroduction to Physical Modeling using SimscapeIntroduction to Structural Analysis using ANSYS WorkbenchIntroduction to Structural Analysis using ANSYS Workbench

      Top PG Programs

      Post Graduate Program in Hybrid Electric Vehicle Design and AnalysisPost Graduate Program in Computational Fluid DynamicsPost Graduate Program in CADPost Graduate Program in Electric Vehicle Design & Development

      Skill-Lync Plus

      Executive Program in Electric Vehicle Embedded SoftwareExecutive Program in Electric Vehicle DesignExecutive Program in Cybersecurity

      Trending Blogs

      Heat Transfer Principles in Energy-Efficient Refrigerators and Air Conditioners Advanced Modeling and Result Visualization in Simscape Exploring Simulink and Library Browser in Simscape Advanced Simulink Tools and Libraries in SimscapeExploring Simulink Basics in Simscape

      © 2025 Skill-Lync Inc. All Rights Reserved.

                  Do You Want To Showcase Your Technical Skills?
                  Sign-Up for our projects.