Week 11 - Simulation of Flow through a pipe in OpenFoam
Aim:- Simulation of flow through a pipe in OpenFoam
Objective:-
Write a program in Matlab that can generate the computational mesh automatically for any wedge angle and grading schemes
Hint: wedge angle should be less than 5 degrees
Make sure that number of cells along the "axi symmetric"
For a baseline mesh, show that the velocity profile matches with the Hagen poiseuille's equation
Show that the velocity profile is fully developed
Post process velocity and shear stress
Theory:-
Hagen Poiseuille's equation:
In nonideal fluid dynamics, the Hagen–Poiseuille equation, also known as the Hagen–Poiseuille law, Poiseuille law or Poiseuille equation, is a physical law that gives the pressure drop in an incompressible and Newtoian fluid in laminar flow flowing through a long cylindrical pipe of constant cross section.
The pressure drop is given by:
`DeltaP=frac{32muLV}[D^2}`
For a pipe with laminar flow there are basically two regions. Entrance length developing region where the flow is not fully developed and the laminar flow layers are at equal velocity with respect to each other whereas in fully deveoped region the flow is fully developed and follows the hagen-Poiseuille law.
Assumed parameters for simulation:
1) Geometry consideration - axi-symmeteric
2) Wedge angle(`theta`) = 4 degrees
3) Working fluid = water (density - 997`(kg)/m^3`
4) Temperature of working fluid = 25°C
5) Reynold's number(Re) = 2100
6) Dynamic viscosity of working fluid(`mu`) = 8.9 X`10^-4` Pa.sec
7) Kinematic viscosity of working fluid(`nu`) = 8.926 X`10^-7` `m^2/sec`
8) Diameter of pipe(D) = 0.02m
Analytical solution:
1) Average velocity:
`Re=(V_(avg)xxDxxrho)/mu`
`implies V_(avg)=(8.9xx10^(-4)xx2100)/(997xx0.02)`
`implies V_(avg)=0.0937m/sec`
2) Maximum velocity:
`V_(max)=2xxV_(avg)`
`V_(max)=2xx0.0937=0.187m/sec`
3) Hydrodynamic Entry Length:
`L_h=0.06xxRexxD`
`L_h=0.06xx2100xx0.02=2.52m`
This means that minimum length of pipe should be 2.52m. The total length of pipe can be assumed as 2.7m.
4) Pressure Drop:
`DeltaP=(32muLV_(avg))/D^2`
`DeltaP=(32xx8.9xx10^-4xx2.7xx0.093)/0.02^2=17.878Pa`
5) Kinematic pressure drop:
`P_k=(DeltaP)/rho=(17.878)/997=0.0179m`
Matlab program to generate a blockMesh file for any angle of the wedge (< 5 degrees):
clear all
close all
clc
d = 0.02; %diameter
r = d/2;
L = 2.7;
theta = input('Enter the value of wedge angle =');
x = input('Enter the grading factor along x =');
y = input('Enter the grading factor along y =');
z = input('Enter the grading factor along z =');
V0 = [0 0 0];
V1 = [0 r*cosd(theta/2) -r*sind(theta/2)];
V2 = [0 r*cosd(theta/2) r*sind(theta/2)];
V3 = [L 0 0];
V4 = [L r*cosd(theta/2) -r*sind(theta/2)];
V5 = [L r*cosd(theta/2) r*sind(theta/2)];
A1= '/*--------------------------------*- C++ -*----------------------------------*\';
A2= ' ========= | ';
A3= ' \\ / F ield | OpenFOAM: The Open Source CFD Toolbox ';
A4= ' \\ / O peration | Website: https://openfoam.org ';
A5= ' \\ / A nd | Version: 8 ';
A6= ' \\/ M anipulation | ';
A7= '\*---------------------------------------------------------------------------*/';
A8= 'FoamFile ';
A9= '{ ';
A10=' version 2.0; ';
A11=' format ascii; ';
A12=' class dictionary; ';
A13=' object blockMeshDict; ';
A14='} ';
A15='// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //';
f1 = fopen('blockMeshDict.txt','wt');
fprintf(f1,'%s\n',A1);
fprintf(f1,'%s\n',A2);
fprintf(f1,'%s\n',A3);
fprintf(f1,'%s\n',A4);
fprintf(f1,'%s\n',A5);
fprintf(f1,'%s\n',A6);
fprintf(f1,'%s\n',A7);
fprintf(f1,'%s\n',A8);
fprintf(f1,'%s\n',A9);
fprintf(f1,'%s\n',A10);
fprintf(f1,'%s\n',A11);
fprintf(f1,'%s\n',A12);
fprintf(f1,'%s\n',A13);
fprintf(f1,'%s\n',A14);
fprintf(f1,'%s\n',A15);
fprintf(f1,'\n');
fprintf(f1,'%s\n','convertToMeters 1;');
fprintf(f1,'\n');
fprintf(f1,'%s\n','vertices');
fprintf(f1,'(\n');
fprintf(f1,'\t(%f %f %f)\r',V0(1),V0(2),V0(3));
fprintf(f1,'\t(%f %f %f)\r',V1(1),V1(2),V1(3));
fprintf(f1,'\t(%f %f %f)\r',V2(1),V2(2),V2(3));
fprintf(f1,'\t(%f %f %f)\r',V3(1),V3(2),V3(3));
fprintf(f1,'\t(%f %f %f)\r',V4(1),V4(2),V4(3));
fprintf(f1,'\t(%f %f %f)\r',V5(1),V5(2),V5(3));
fprintf(f1,');\r\n');
fprintf(f1,'blocks\r(\r');
fprintf(f1,'\t hex (0 3 4 1 0 3 5 2) (300 50 1) simpleGrading (%f %f %f)\r',x,y,z);
fprintf(f1,');\r\n');
fprintf(f1,'edges\r(\r');
fprintf(f1,'\t\t arc 1 2 (%f %f %f)\r',0,r,0);
fprintf(f1,'\t\t arc 4 5 (%f %f %f)\r',L,r,0);
fprintf(f1,');\r\n');
fprintf(f1,'boundary\r(\r');
fprintf(f1,'\tinlet\r\t{\r');
fprintf(f1,'\t\ttype patch;\r');
fprintf(f1,'\t\tfaces\r\t\t(\r');
fprintf(f1,'\t\t\t(0 2 1 0)\r');
fprintf(f1,'\t\t);\r');
fprintf(f1,'\t}\r');
fprintf(f1,'\toutlet\r\t{\r');
fprintf(f1,'\t\ttype patch;\r');
fprintf(f1,'\t\tfaces\r\t\t(\r');
fprintf(f1,'\t\t\t(3 4 5 3)\r');
fprintf(f1,'\t\t);\r');
fprintf(f1,'\t}\r');
fprintf(f1,'\ttop\r\t{\r');
fprintf(f1,'\t\ttype wall;\r');
fprintf(f1,'\t\tfaces\r\t\t(\r');
fprintf(f1,'\t\t\t(1 2 5 4)\r');
fprintf(f1,'\t\t);\r');
fprintf(f1,'\t}\r');
fprintf(f1,'\tback\r\t{\r');
fprintf(f1,'\t\ttype wedge;\r');
fprintf(f1,'\t\tfaces\r\t\t(\r');
fprintf(f1,'\t\t\t(0 1 4 3)\r');
fprintf(f1,'\t\t);\r');
fprintf(f1,'\t}\r');
fprintf(f1,'\tfront\r\t{\r');
fprintf(f1,'\t\ttype wedge;\r');
fprintf(f1,'\t\tfaces\r\t\t(\r');
fprintf(f1,'\t\t\t(0 3 5 2)\r');
fprintf(f1,'\t\t);\r');
fprintf(f1,'\t}\r');
fprintf(f1,'\taxis\r\t{\r');
fprintf(f1,'\t\ttype empty;\r');
fprintf(f1,'\t\tfaces\r\t\t(\r');
fprintf(f1,'\t\t\t(0 3 3 0)\r');
fprintf(f1,'\t\t);\r');
fprintf(f1,'\t}\r);\r\n');
fprintf(f1,'mergePatchPairs\n(\n);\n');
fprintf(f1,'\n// ************************************************************************* //');
fclose(f1);
blockMeshDict file:-
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 8
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 1;
vertices
(
(0.000000 0.000000 0.000000)
(0.000000 0.009994 -0.000349)
(0.000000 0.009994 0.000349)
(2.700000 0.000000 0.000000)
(2.700000 0.009994 -0.000349)
(2.700000 0.009994 0.000349)
);
blocks
(
hex (0 3 4 1 0 3 5 2) (300 50 1) simpleGrading (1.000000 1.000000 1.000000)
);
edges
(
arc 1 2 (0.000000 0.010000 0.000000)
arc 4 5 (2.700000 0.010000 0.000000)
);
boundary
(
inlet
{
type patch;
faces
(
(0 2 1 0)
);
}
outlet
{
type patch;
faces
(
(3 4 5 3)
);
}
top
{
type wall;
faces
(
(1 2 5 4)
);
}
back
{
type wedge;
faces
(
(0 1 4 3)
);
}
front
{
type wedge;
faces
(
(0 3 5 2)
);
}
axis
{
type empty;
faces
(
(0 3 3 0)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //controlDict file:-
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 8
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application icoFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 25;
deltaT 0.01;
writeControl timeStep;
writeInterval 20;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
// ************************************************************************* //Pressure condition:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 8
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
inlet
{
type zeroGradient;
}
outlet
{
type fixedValue;
value uniform 0.0179;
}
top
{
type zeroGradient;
}
front
{
type wedge;
}
back
{
type wedge;
}
axis
{
type empty;
}
}
// ************************************************************************* //Velocity condition:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 8
\\/ 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 (0.0937 0 0);
}
outlet
{
type zeroGradient;
}
top
{
type noSlip;
}
front
{
type wedge;
}
back
{
type wedge;
}
axis
{
type empty;
}
}
// ************************************************************************* //transportProperties file:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 8
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
nu [0 2 -1 0 0 0 0] 0.0000008927;
// ************************************************************************* //Generated mesh:
Velocity line plot:
Shear stress line plot:
Conclusion:-
The parabolic stable curve shows that flow is fully developed.
Shear stress plot also shows that the flow is fully developed.