Week 11 - Simulation of Flow through a pipe in OpenFoam
Pipe flow simulation in OpenFoam
Aim: Simulate axisymmetric flow in a pipe through foam.
Objective:
- Verify the hydrodynamic length using the numerical result
- Verify a fully developed flow rate profile with its analytical profile
- Verify the maximum velocity and pressure drop for fully developed flow
- Post-process Shear Stress and verify wall shear stress for fully developed flow
Solution:
Consider the flow of water through a 20 mm diameter pipe at a velocity of 0.0935 m/s Reynolds number less than 2100, i.e. laminar flow. Thanks to the non-slip condition, the liquid particles come to a complete stop in contact with the pipe.
Boundary Layer Theory:
Consider a fluid entering a circular pipe with uniform velocity and no slip.
The fluid velocity in the middle section must increase to keep the mass flow through the pipe constant, resulting in a velocity gradient.
The hydrodynamic inlet region is the area from the inlet to the point at which the velocity profile is fully developed, and its length is the hydrodynamic inlet length.
Reynolds number is the ratio of inertial force to viscous force.
Hagen- Poiseuille's flow: It is the pressure drop in incompressible fluid in laminar flow through the long cylindrical pipe of constant cross section. Flow is caused to flow by pressure difference between the points, from higher pressure to lower pressure.
It is assumed to have no acceleration of flow. Flow resistance offered is shear stress.
Matlab code:
clear all
close all
clc
D=0.02;
Re=2100;
rho=1000; %density
theta=4;
nu=8.91e-7; %kinematic viscocity
%dynamic vis
mu=rho*nu;
v_avg= mu*Re/(rho*D);
v_max=2*v_avg;
L_w=0.3;
L_entrance= 0.06* Re*D;
L=L_entrance+L_w;
%pressure drop in flow
delta_p= 32*mu*v_avg*L_w/D^2;
r=D/2;
R=linspace(0,r,500);1.
for i=1:length(R)
tau(i)=2*mu*v_max*(abs(R(i)))/r^2;
end
for j=1: length(R)
vel_p(j)=2*v_avg*(1-(abs(R(j))^2/r^2));
end
figure(1)
plot(R,tau)
ylabel('shear stress')
xlabel('Radial length')
figure (2)
plot(R,vel_p)
ylabel('velocity')
xlabel('Radial length')
%blockmeshdict file
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)];
f1=fopen('blockMeshDict','w');
fprintf(f1,'\t FoamFile \n')
fprintf(f1,'\t { \n')
fprintf(f1,'\t \t format ascii;\n')
fprintf(f1,'\t\t class dictionary;\n')
fprintf(f1,'\t\t object blockMeshDict;\n')
fprintf(f1,'\t } \n')
%vertices
fprintf(f1,'%s \n','convertToMeters 1 ;')
fprintf(f1,'\n %s \n','vertices')
fprintf(f1,'%s \n','(')
fprintf(f1,'\t(%d %d %d)\n',v0(1), v0(2), v0(3))
fprintf(f1,'\t(%d %d %d)\n',v1(1), v1(2), v1(3))
fprintf(f1,'\t(%d %d %d)\n',v2(1), v2(2), v2(3))
fprintf(f1,'\t(%d %d %d)\n',v3(1), v3(2), v3(3))
fprintf(f1,'\t(%d %d %d)\n',v4(1), v4(2), v4(3))
fprintf(f1,'\t(%d %d %d)\n',v5(1), v5(2), v5(3))
fprintf(f1,'%s \n',');')
%blocks
fprintf(f1,'%s \n','blocks')
fprintf(f1,'%s \n','(')
fprintf(f1,'\t hex(0 3 4 1 0 3 5 2) (%d %d %d) simpleGrading (%d %d %d)\n', 200,20,1,1,0.1,1)
fprintf(f1,'%s \n',');')
%edges
fprintf(f1,'\n %s \n','edges')
fprintf(f1,'%s \n','(')
fprintf(f1,'\t arc 1 2 (%d %d %d) \n',0,r,0)
fprintf(f1,'\t arc 1 2 (%d %d %d) \n',L,r,0)
fprintf(f1,'\n %s',');')
%boundary
fprintf(f1,'\n %s \n','boundary')
fprintf(f1,'%s \n','(')
fprintf(f1,'\n %s \n','axis')
fprintf(f1,'{ \n \t type empty; \n')
fprintf(f1,'\t faces \n( \n')
fprintf(f1,'\t (%d %d %d %d) \n',0,3,3,0)
fprintf(f1,'\t ) ; \n }\n')
%wall
fprintf(f1,'\n %s \n','wall')
fprintf(f1,'%s \n','{')
fprintf(f1,'\t type wall; \n')
fprintf(f1,'\t faces \n ( \n')
fprintf(f1,'\t (%d %d %d %d) \n',1,4,5,2)
fprintf(f1,'\t ) ; \n }\n')
%inlet
fprintf(f1,'\n %s \n','inlet')
fprintf(f1,'%s \n','{')
fprintf(f1,'\t type patch; \n')
fprintf(f1,'\t faces \n ( \n')
fprintf(f1,'\t (%d %d %d %d) \n',0,1,2,0)
fprintf(f1,'\t ) ; \n }\n')
%outlet
fprintf(f1,'\n %s \n','outlet')
fprintf(f1,'%s \n','{')
fprintf(f1,'\t type patch; \n')
fprintf(f1,'\t faces \n ( \n')
fprintf(f1,'\t (%d %d %d %d) \n',3,5,4,3)
fprintf(f1,'\t ); \n }\n')
%front
fprintf(f1,'\n\t front \n { \n')
fprintf(f1,'\t type wedge ; \n')
fprintf(f1,'\t faces \n ( \n')
fprintf(f1,'\t (%d %d %d %d) \n',0,3,4,1)
fprintf(f1,'\t ) ; \n \t }\n')
%back
fprintf(f1,'\n\t back \n { \n')
fprintf(f1,'\t type wedge ; \n')
fprintf(f1,'\t faces \n ( \n')
fprintf(f1,'\t (%d %d %d %d) \n',0,2,5,3)
fprintf(f1,'\t ) ; \n \t }\n')
fprintf(f1,');')Explanation:
1. Assign initial Hagen-Pousville flow rates.
2. Calculation of properties such as dynamic viscosity, average speed, maximum speed, inlet length.
3. Change in pressure
4. Calculate the shear stress and velocity profile using a for loop.
5. Plotting values to obtain an analytical solution.
Create a BlockMeshDict file using the write function:
1. Assign vertices at all points of the wedge. (v1, v2, v3, v4, v5)
2. Drawing the blockMeshDict file using the write function in MATLAB.
3. The drawing should be done with a similar pattern as the blockMeshDict file used in openFoam.
4. Writing the vertices of the wedge.
5. Creating a hexagonal block with a gradation factor of 0.1 along the Y axis (finer mesh near the walls).
6. Assignment of edges, wall, boundary, entry, exit, front and back of blocks.
Flow simulation procedure:
A. To select the solver and copy the folder
1. Open terminal command in ubuntu.
2. open tutorials, code: tut
3. Open the incompressible folder and select icofoam, then cavity. (code: icoFoam)
4. Copy the cavity folder to the startup folder. using code: 'cp -r pipr/$FOAM_RUN'
5. Type the run command to open the run folder.
6. Open the pipe. (code: cd pipe)
(6a. Also copy and paste the blockMeshDict file created by MATLAB into the system folder)
7. Open the system file.
8. Run the blockMeshDict code file. (code: blockMesh)
BlockMeshDict file:
FoamFile
{
format ascii;
class dictionary;
object blockMeshDict;
}
convertToMeters 1 ;
vertices
(
(0 0 0)
(0 9.993908e-03 -3.489950e-04)
(0 9.993908e-03 3.489950e-04)
(2.820000e+00 0 0)
(2.820000e+00 9.993908e-03 -3.489950e-04)
(2.820000e+00 9.993908e-03 3.489950e-04)
);
blocks
(
hex (0 3 4 1 0 3 5 2) (200 20 1) simpleGrading (1 0.1 1)
);
edges
(
arc 1 2 (0 1.000000e-02 0)
arc 4 5 (2.820000e+00 1.000000e-02 0)
);
boundary
(
axis
{
type empty;
faces
(
(0 3 3 0)
) ;
}
wall
{
type wall;
faces
(
(1 4 5 2)
) ;
}
inlet
{
type patch;
faces
(
(0 1 2 0)
) ;
}
outlet
{
type patch;
faces
(
(3 5 4 3)
);
}
front
{
type wedge ;
faces
(
(0 3 4 1)
) ;
}
back
{
type wedge ;
faces
(
(0 2 5 3)
) ;
}
);
ControlDict file:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 9
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application icoFoam;
startFrom startTime;
startTime 5;
stopAt endTime;
endTime 15;
deltaT 0.05;
writeControl runTime;
writeInterval 0.1;
purgeWrite 10;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
// ************************************************************************* /Eplaination:
1. open control dict file in system folder (code: gedit controlDict).
2. Assign start time as 5 and end time 15, delta t 0.05.
p and U files:
p file:
1. Open 0 folder in block_test
(code: cd..
code :cd 0)
2. Open files p file( code: gedit p)
code for p:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 9
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
outlet
{
type fixedValue;
value uniform 0;
}
inlet
{
type zeroGradient;
}
axis
{
type empty;
}
wall
{
type zeroGradient;
}
front
{
type wedge;
}
back
{
type wedge;
}
}
// ************************************************************************* 1. Assign outlet as uinform 0.
2. Inlet and oulet as zerogradient, front and back as wedge.
Open file U file( code: gedit U)
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 9
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0.0936 0 0);
boundaryField
{
inlet
{
type fixedValue;
value uniform (0.0936 0 0);
}
outlet
{
type zeroGradient;
}
axis
{
type empty;
}
wall
{
type noSlip;
}
front
{
type wedge;
}
back
{
type wedge;
}
}
// ************************************************************************* //Explaination:
1. Assign outlet and fixedwalls as zero gradient.
2. Front and back empty.
3. Inlet as uniform (0.0936 0 0) fixed value, extracted from MATLAB value.
Transient properties as :
1. Open constant foler
2. Open transientProperties file. (code: gedit transientProperties)
3. Give value for nu = 8.91e-7 (Kinematic viscosity of water)
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 9
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "constant";
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
nu [0 2 -1 0 0 0 0] 8.91e-7;
// ************************************************************************* //Open paraview:
1. Change directory to block_test
2. Run code: checkMesh
3. Run code:icoFoam
4. Run code: paraFoam
5. In paraview click apply.
Results and discussion:
Paraview:
Geometry of wedge:
Blockmesh:
Select options 'surface with edges' and 'solid color'
Geometry velocity profile:
Select option 'U'
Plots generated at different points:
Velocity profile at 0.25
Velocity profile at 0.5
Velocity profile at 1
Velocity profile at 1.5
Velocity profile at entrance length (2.52)
The Analytical velocity profile obtained from the Matlab :
Analytical shear stress graph obtained by MATLAB:
Pressure drop:
Pressure drop graph of fully developed area.
The value of point at 2.52 is 0.002031
The value of point at 2.82 is 4.53e-6
Difference between them is ∇p∇�= 0.002030547,
obtained from the graph,
analytical value of pressure drop ∇p∇� =2.006 in mm.
Conclusion:
The hydrodynamic length is obtained at 2.52 units where the velocity profile is fully developed.
The velocity profile gradually increases from inlet to outlet. After the flow is fully developed, it remains constant.
The analytical velocity profile and the velocity obtained in openfoam agree very well, where the velocity is maximum in the center and decreases parabolically towards the wall.
The shear stress is zero at the center of the pipe and increases linearly towards the wall, the graph obtained from openfoam is close to the analytical result.
The maximum velocity and pressure drop value is achieved for fully developed flow.