Pipe flow simulation in OpenFOAM
LAMINAR INCOMPRESSIBLE FLOW SIMULATION THROUGH A PIPE IN OPENFOAM:
[PART 2/2]: SYMMETRY BOUNDARY CONDITION:
OBJECTIVES:
1. Creating the Mesh-Script (blockMeshDict file) with symmetry boundary condition.
2. Simulation Results and post processing the velocity profile at different points of the pipe for fully developed flow.
3. Comparison of Wedge Boundary Condition and Symmetry Boundary Condition against Hagen Poiseuille Equation.
_______________________________________________________________________
PART [2/2]:
[I] INTRODUCTION:
In the previous part we looked into the simulation results for a laminar, incompressible flow through a pipe in OpenFOAM. Now in this section, we would attempt the same problem with the symmetry boundary conditions.
[II] MATLAB Program:
The required MATLAB Program to automatically generate the blockMeshDict file for a given wedge angle is given below. The syntax is same as before with the exception of the boundary conditions.
%% MATLAB program to Auto-generate the blockMeshDict file for a Wedge geometry:
clear all;
close all;
clc;
%% Input Parameters
Re = 2100; % Given Reynold's Number
d = 0.02; % Diameter of the pipe
r = d/2; % Radius of the pipe
L_entrance = 0.06*Re*d; % Length of the pipe
fprintf('Enter 2, 3, 4, 5 for wedge boundary condition \nEnter 10, 25, 45 for symmetry boundary condition\n');
theta = input('Enter the angle in angles:\n '); % Angle of wedge
mu = 0.89e-3; % Viscosity of water at 25 deg C
rho = 997.0; % Density of water at 25 deg C
nu = mu/rho; % Kinematic Viscosity of water at 25 deg C
%% Calculation of pressure and velocity:
L = L_entrance + 0.3; % Length of the Wedge
v_avg = Re*mu/(d*rho); % Average Velocity
v_max = 2*v_avg; % Max Velocity
del_P = (32*mu*v_avg*L)/(d^2); % Pressure Drop
kin_P = del_P/rho; % KinematicPressure Drop
%% Calculating the vertices of the wedge:
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)];
%% String format specifying for BlockMesh File:
head1 = "/*--------------------------------*- C++ -*----------------------------------*\";
head2 = " ========= | ";
head3 = " \\ / F ield | OpenFOAM: The Open Source CFD Toolbox ";
head4 = " \\ / O peration | Website: https://openfoam.org ";
head5 = " \\ / A nd | Version: 6 ";
head6 = " \\/ M anipulation | ";
head7 = "\*---------------------------------------------------------------------------*/";
b4 = blanks(4);
b8 = blanks(8);
b12 = blanks(12);
b16 = blanks(16);
dict1 = " version 2.0;";
dict2 = " format ascii;";
dict3 = " class dictionary;";
dict4 = " object blockMeshDict;";
dict5 = "// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //";
conv = "convertToMeters 1;";
vertex1 = "vertices";
blocks1 = b4 + "hex (0 1 2 0 3 4 5 3) (50 1 200) simpleGrading (0.2 1 1)";
footer = "// ************************************************************************* //";
%% Creating BlockMeshDict file for OpenFOAM:
f1 = fopen('blockMeshDict_45.txt','wt');
% Printing the Header File
fprintf(f1,'%s\n',head1);
fprintf(f1,'%s\n',head2);
fprintf(f1,'%s\n',head3);
fprintf(f1,'%s\n',head4);
fprintf(f1,'%s\n',head5);
fprintf(f1,'%s\n',head6);
fprintf(f1,'%s\n',head7);
fprintf(f1,'FoamFile\n{\n');
fprintf(f1,'%s\n',dict1);
fprintf(f1,'%s\n',dict2);
fprintf(f1,'%s\n',dict3);
fprintf(f1,'%s\n}\n',dict4);
fprintf(f1,'%s\n',dict5);
fprintf(f1,'\n%s\n',conv);
% Printing the vertices
fprintf(f1,'\nvertices\n(\n');
fprintf(f1,'%s(%d %d %d)\n',b4,v0(1),v0(2),v0(3));
fprintf(f1,'%s(%d %f %f)\n',b4,v1(1),v1(2),v1(3));
fprintf(f1,'%s(%d %f %f)\n',b4,v2(1),v2(2),v2(3));
fprintf(f1,'%s(%f %d %d)\n',b4,v3(1),v3(2),v3(3));
fprintf(f1,'%s(%f %f %f)\n',b4,v4(1),v4(2),v4(3));
fprintf(f1,'%s(%f %f %f)\n',b4,v5(1),v5(2),v5(3));
% Printing the blocks
fprintf(f1,');\n\nblocks\n(\n');
fprintf(f1,'%s\n);\n\n',blocks1);
fprintf(f1,'edges\n(\n');
% Printing the edges
fprintf(f1,'%sarc 1 2 (0 %0.3f 0)\n',b4,r);
fprintf(f1,'%sarc 4 5 (%0.4f %0.3f 0)\n',b4,L,r);
% Printing the boundaries
fprintf(f1,');\n\nboundary\n(\n');
fprintf(f1,'%saxis\n%s{\n',b4,b4);
fprintf(f1,'%stype empty;\n%sfaces\n%s(\n%s(0 3 3 0)\n%s);\n%s}\n',b8,b8,b8,b12,b8,b4);
fprintf(f1,'%swall\n%s{\n',b4,b4);
fprintf(f1,'%stype wall;\n%sfaces\n%s(\n%s(2 5 4 1)\n%s);\n%s}\n',b8,b8,b8,b12,b8,b4);
fprintf(f1,'%sinlet\n%s{\n',b4,b4);
fprintf(f1,'%stype patch;\n%sfaces\n%s(\n%s(0 0 2 1)\n%s);\n%s}\n',b8,b8,b8,b12,b8,b4);
fprintf(f1,'%soutlet\n%s{\n',b4,b4);
fprintf(f1,'%stype patch;\n%sfaces\n%s(\n%s(3 4 5 3)\n%s);\n%s}\n',b8,b8,b8,b12,b8,b4);
fprintf(f1,'%swedgeFront\n%s{\n',b4,b4);
fprintf(f1,'%stype symmetry;\n%sfaces\n%s(\n%s(0 3 5 2)\n%s);\n%s}\n',b8,b8,b8,b12,b8,b4);
fprintf(f1,'%swedgeBack\n%s{\n',b4,b4);
fprintf(f1,'%stype symmetry;\n%sfaces\n%s(\n%s(0 1 4 3)\n%s);\n%s}\n',b8,b8,b8,b12,b8,b4);
fprintf(f1,');\n\nmergePatchPairs\n(\n);\n\n');
fprintf(f1,'%s',footer);
The generated blockMeshDict file fro wedge angle = 25 degree is given below:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 6
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 1;
vertices
(
(0 0 0)
(0 0.009763 -0.002164)
(0 0.009763 0.002164)
(2.820000 0 0)
(2.820000 0.009763 -0.002164)
(2.820000 0.009763 0.002164)
);
blocks
(
hex (0 1 2 0 3 4 5 3) (50 1 200) simpleGrading (0.2 1 1)
);
edges
(
arc 1 2 (0 0.010 0)
arc 4 5 (2.8200 0.010 0)
);
boundary
(
axis
{
type empty;
faces
(
(0 3 3 0)
);
}
wall
{
type wall;
faces
(
(2 5 4 1)
);
}
inlet
{
type patch;
faces
(
(0 0 2 1)
);
}
outlet
{
type patch;
faces
(
(3 4 5 3)
);
}
wedgeFront
{
type symmetry;
faces
(
(0 3 5 2)
);
}
wedgeBack
{
type symmetry;
faces
(
(0 1 4 3)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //The boundary conditions are same as before however the wedge faces have a symmetry condition imposed.
Pressure Boundary Condition:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 6
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
axis
{
type empty;
}
inlet
{
type zeroGradient;
}
outlet
{
type fixedValue;
value uniform 0.0168682;
}
wall
{
type zeroGradient;
}
wedgeFront
{
type symmetry;
}
wedgeBack
{
type symmetry;
}
}
// ************************************************************************* //
Velocity Boundary Conditions:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 6
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0.0937312 0 0);
boundaryField
{
axis
{
type empty;
}
inlet
{
type fixedValue;
value uniform (0.0937312 0 0);
}
outlet
{
type zeroGradient;
}
wall
{
type fixedValue;
value uniform (0 0 0);
}
wedgeFront
{
type symmetry;
}
wedgeBack
{
type symmetry;
}
}
// ************************************************************************* //[III] MESH PROFILE:
The mesh geometry for wedge angle = 25 degree is given below:
Symmetry Boundary Condition: The symmetry boundary condition defines a mirror face/surface. The symmetry condition is used if the physical object or geometry and the expected flow field pattern of the developed solution is mirrored along that surface. This boundary condition helps to reduces the computational domain in size and enables the modeling of a sub-domain of the complete setup.
[IV] SIMULATION RESULTS:
1. WEDGE ANGLE: `25^o`
A. Geometry near the entrance:
The simulation shows a developing hydrodynamic boundary layer at the entrrance. The free stream velocity keeps increases as we move farther from the entrance of the pipe.
B. Geometry near the exit (Fully Developed flow):
C. Velocity Profile curves:
i. Velocity profile at x = 0.02 m from the entrance:
The velocity profile near the entrance shows three distinct regions:
A. Viscous Sublayer: The effect of velocity boundary layer is seen in formation in this region of the pipe.
B. Transitional Buffer layer: This layer gradually decreases with the viscous sublayer merges with the turbulent core with increasing distance from the entrance.
C. Turublent Core: The velocity profile is almost flat in this region and is comprised of the turbulent component of the flow.
ii. Velocity profile at x = 0.1m from the entrance:
The above velocity profile shows a shrinking turbulent core.
iii. Velocity profile at x = 0.25 m from the entrance:
iv. Velocity profile at x = 0.5m from the entrance:
v. Velocity profile at x = 1.0m from the entrance:
vi. Velocity profile at entrance length `L_(entrance) = 2.52m` (Fully developed flow):
(uni-directional flow along the x axis indicating fully laminar velocity profile)
Shear Stress Profile:
Almost linear shear stress profile obtained by the simulation. Shear stress is zero at the walls and maximum at the centerline.
Linear fit of Shear stress data:
(The following curves were obtained using OriginPro 2018 Graphing software)
2. SIMULATION RESULTS FOR OTHER ANGLES:
A. WEDGE ANGLE: `10^o`
i. Mesh Profile:
ii. Geometry near the entrance:
iii. Geometry at the fully developed flow region:
Cross sectional velocity profiles at different distances from entrance:
iv. Velocity Profile at x = 0.2m from the entrance:
v. Velocity Profile at x = 2.52m from the entrance showing fully developed flow:
Exactly identical as before with minor variations in magnitude of `V_(max)`
B. WEDGE ANGLE `45^o`
i. Mesh Profile:
ii. Geometry near the entrance region:
iii. Geometry at the fully developed region:
iv. Velocity Profile at x = 0.2m from the entrance:
v. Velocity Profile Depicting the fully formed region:
[V] CONCLUSION AND REMARKS:
Comparison of maximum velocities `V_(max)`
Comparison of courant numbers and execution times for various wedge angles:
CONCLUSIONS:
1. SYMMETRY BOUNDARY CONDITION IS MORE ACCURATE THAN WEDGE BOUNDARY CONDITION.
2. EXECUTION TIME IS GREATER FOR SYMMETRY BOUNDARY CONDITION THAN WEDGE BOUNDARY CONDITION FOR THE SAME COMPUTATIONAL MESH.
3. COURANT NUMBER FOR SIMULATION INCREASES WITH INCREASING WEDGE ANGLES
4. TIME STEP OF THIS PROBLEM IS 0.01s WITH A WRITE TIME OF 1000 TIMESTEPS.
- Minam TungekarHow did you create a complete velocity profile? was it done in OpenFOAM? Any help would be appreciated!