Week 8 - Simulation of a backward facing step in OpenFOAM

Simulation of a backward-facing step in OpenFOAM

AIM:

• Transient simulation of incompressible-laminar-viscous flow through the backward-facing step geometry using OpenFOAM.

THEORY:

• Fluid is a substance that deforms continuously when subjected to tangential stress, it does not matter how small the tangential stress is.
• According to Newton's law, the shear stress on the fluid is directly proportional to the rate of shear strain.
• `tau = mu * frac{delu}{dely}`
• Dynamic viscosity ( `mu` ) is the resistance offered by the below fluid layer to the upper fluid layer in the fluid flow.
• Kinematic viscosity is the ratio of dynamic viscosity to the density of the fluid.
• In the incompressible flow of fluid, the density of the fluid does not change, it remains constant throughout the flow no matter what amount of pressure changes

Laminar Flow

• Fluid flows in the form of layers.
• Generally, this type of flow is due to low velocity and high viscosity.
• There is no mixing between the layers.
• For the internal flow, it occurs at the Reynolds number is below 2000.
• It obeys Newton's law of viscosity.

Turbulent Flow

• In turbulent flow, fluid flow in a disordered manner.
• Occurs due to high velocity and low viscosity.
• Due to fluctuating velocity components, a large amount of additional shear stress comes into play (Eddy shear stress).
• For the internal flows it occurs at Reynolds number greater than 4000.
• It does not follow Newton's law of viscosity.

No-Slip, and Boundary Layer

• No-slip is the boundary condition, which states that the relative velocity of fluid layers at the wall of duct/pipe is zero.
• It is due to the surface roughness of the wall and the adhesion effect between fluid and solid surfaces.
• This makes the velocity of the fluid at the wall zero and in the transverse direction of the flow, velocity varies.
• Velocity variation in the transverse direction is either parabolic or linear for laminar flow
• Velocity variation in the transverse direction is either logarithmic or follows the power law for turbulent flow.
• And due to No-slip, there is momentum disturbance in the transverse direction of the flow, which causes the formation of a boundary layer near the wall.
• Kinematic viscosity is the property of the fluid responsible for the momentum diffusivity, and the effect of viscosity is dominated in the flow.
• In solving viscous dominated flow only Navier-stokes equation is used.

OpenFOAM SETUP:

• "IcoFoam" is used to solve the incompressible laminar Navier-Stokes equations.
• The general form of Navier-stokes equation.
• 

• In OpenFOAM, any solver folder usually contains an example, and each example contains, 0 folders, constant folder, and system folder.
• And the files are edited within the predefined algorithm of the OpenFOAM to set up our problem.
• In the system file, in the blockMeshDict file, the vertices section is edited to create the required geometry.
• Using vertices index number, blocks are defined and meshed (discretized), Grading factor is also specified at the same time according to the problem case.
• According to OpenFOAM algorithm the walls are edited into the inlet, outlet, no-slip walls, and frontAndBackwalls.Inlet and outlet walls are patch type, noslipwalls are wall type and frontAndBack walls are empty type.
• Faces are defined for the inlet, outlet, noslipwalls, and forntAndBackwalls.
• Grading factor(GF) is the ratio of (length of end cell/length of the first cell)
• First case GF=1 and second case GF=0.2.
• case 1: blockMeshDict

• /*--------------------------------*- 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 0.01;
  
  vertices
  (
      (0 1 0)
      (8 1 0)
      (8 1.5 0)
      (0 1.5 0)
      (8 2 0)
      (0 2 0)
      (20 2 0)
      (20 1.5 0)
      (20 1 0)
      (20 0 0)
      (8 0 0)
      (0 1 0.01)
      (8 1 0.01)
      (8 1.5 0.01)
      (0 1.5 0.01)
      (8 2 0.01)
      (0 2 0.01)
      (20 2 0.01)
      (20 1.5 0.01)
      (20 1 0.01)
      (20 0 0.01)
      (8 0 0.01)
      
  );
  
  blocks
  (
      hex (0 1 2 3 11 12 13 14) (80 5 1) simpleGrading (1 1 1)
      hex (3 2 4 5 14 13 15 16) (80 5 1) simpleGrading (1 1 1)
      hex (2 7 6 4 13 18 17 15) (120 5 1) simpleGrading (1 1 1)
      hex (1 8 7 2 12 19 18 13) (120 5 1) simpleGrading (1 1 1)
      hex (10 9 8 1 21 20 19 12) (120 10 1) simpleGrading (1 1 1)
      
  );
  
  edges
  (
  );
  
  boundary
  (
      inlet
      {
          type patch;
          faces
          (
              (0 11 14 3)
              (3 14 16 5)
              
          );
      }
      outlet
      {
          type patch;
          faces
          (
              (9 8 19 20)
              (8 7 18 19)
              (7 6 17 18)
              
          );
      }
      noslipwalls
      {
          type wall;
          faces
          (
              (16 15 4 5)
              (15 17 6 4)
              (10 21 12 1)
              (11 0 1 12)
              (21 10 9 20)
          );
      }
      frontAndBack
      {
          type empty;
          faces
          (
              (11 12 13 14)
              (14 13 15 16)
              (21 20 19 12)
              (12 19 18 13)
              (13 18 17 15)
              (0 3 2 1)
              (10 1 8 9)
              (1 2 7 8)
              (2 4 6 7)
              
          );
      }
  );
  mergePatchPairs
  (
  );
  
  // ************************************************************************* 

• Case 2:blockMeshDict

• /*--------------------------------*- 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 0.01;
  
  vertices
  (
      (0 1 0)
      (8 1 0)
      (8 1.5 0)
      (0 1.5 0)
      (8 2 0)
      (0 2 0)
      (20 2 0)
      (20 1.5 0)
      (20 1 0)
      (20 0 0)
      (8 0 0)
      (0 1 0.01)
      (8 1 0.01)
      (8 1.5 0.01)
      (0 1.5 0.01)
      (8 2 0.01)
      (0 2 0.01)
      (20 2 0.01)
      (20 1.5 0.01)
      (20 1 0.01)
      (20 0 0.01)
      (8 0 0.01)
      
  );
  
  blocks
  (
      hex (0 1 2 3 11 12 13 14) (80 5 1) simpleGrading (5 5.0 1)
      hex (3 2 4 5 14 13 15 16) (80 5 1) simpleGrading (5 0.2 1)
      hex (2 7 6 4 13 18 17 15) (120 5 1) simpleGrading (5 0.2 1)
      hex (1 8 7 2 12 19 18 13) (120 5 1) simpleGrading (5 5.0 1)
      hex (10 9 8 1 21 20 19 12) (120 10 1) simpleGrading (5 5.0 1)
      
  );
  
  edges
  (
  );
  
  boundary
  (
      inlet
      {
          type patch;
          faces
          (
              (0 11 14 3)
              (3 14 16 5)
              
          );
      }
      outlet
      {
          type patch;
          faces
          (
              (9 8 19 20)
              (8 7 18 19)
              (7 6 17 18)
              
          );
      }
      noslipwalls
      {
          type wall;
          faces
          (
              (16 15 4 5)
              (15 17 6 4)
              (10 21 12 1)
              (11 0 1 12)
              (21 10 9 20)
          );
      }
      frontAndBack
      {
          type empty;
          faces
          (
              (11 12 13 14)
              (14 13 15 16)
              (21 20 19 12)
              (12 19 18 13)
              (13 18 17 15)
              (0 3 2 1)
              (10 1 8 9)
              (1 2 7 8)
              (2 4 6 7)
              
          );
      }
  );
  mergePatchPairs
  (
  );
  
  // ************************************************************************* 

• In the same system folder, in the controlDict file, simulation time is set up to 1.5sec and timestep by 0.0001.
• controlDict

• /*--------------------------------*- 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         1.5;
  
  deltaT          0.0001;
  
  writeControl    timeStep;
  
  writeInterval   20;
  
  purgeWrite      0;
  
  writeFormat     ascii;
  
  writePrecision  6;
  
  writeCompression off;
  
  timeFormat      general;
  
  timePrecision   6;
  
  runTimeModifiable true;
  
  
  // ************************************************************************* //

• In zero folder it contains, the initial conditions and boundary conditions of the flow variables to solve the problem
• In the pressure p File, only outlet pressure is edited as 0.
• P

• /*--------------------------------*- 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;
      }
  
      noslipwalls
      {
          type            zeroGradient;
      }
  
      frontAndBack
      {
          type            empty;
      }
  }
  
  // *************************************************************************

• In the velocity u folder, inlet velocity is edited as 0.5m/sec in x-direction only, "noslipwalls" are edited as "noSlip" boundary condition.
• U

• /*--------------------------------*- 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 (0.5 0 0);
      }
      
      outlet
      {
          type            zeroGradient;
      }
  
      noslipwalls
      {
          type            noSlip;
      }
  
      frontAndBack
      {
          type            empty;
      }
  }
  
  // ************************************************************************* //

• In the constant folder, it contains the transport properties file, in which the kinematic viscosity of water "0.0000008"is set to meter square/sec.
• transport properties

• /*--------------------------------*- 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] 0.0000008;
  
  
  // ************************************************************************* //

• To simulate, first we have to run 'blockMesh' to check the correctness of flow geometry.
• Paraview is used for postprocessing of the simulation, to visualise and manipulate the result in a required form.
• It is called using paraFoam.

RESULT:

• The simulation ran successfully.
• Near the inlet flow is fully developed laminar flow and in this region velocity profile along the length becomes the same and remains constant.
• Near the step, the flow starts to diverge due to sudden increase in area, hence fluid velocity drops, pressure increases, it creates a back pressure, due to which extreme layers of the fluid detached from the wall and starts flow in the reverse direction of the fluid flow.
• Due to which rapid mixing of the fluid layer takes place at the diverging region of fluid, due to which flow becomes unstable and becomes turbulent near the outlet.

	CASE 1: For GF =1	CASE 2: For GF =0.2 near the walls and critical section.
Velocity variation Near inlet, velocity is uniform along the length till x =0.08 Due to sudden increase in area at x =0.08, pressure decreases, back pressure is created due to this fluid flows in reverse direction. From diverging section to outlet, velocity is not uniform and fluctuating along the length. This behaviour is captured well by case2
Pressure variation Fluid flow from high-pressure region to low-pressure region. Near inlet, pressure is high compared to the section at x =0.08 After that, pressure drops in the region of fluid mixing due to eddies formation. This behaviour is captured well by case2 compared to case1
Velocity profile The velocity profile is logarithmic at y above 0.01 to 0.02 The velocity profile is negative in y below 0.01, indicating that fluid is flowing in the reverse direction. In case1: at Y=0.01 velocity is 0.3 m/sec In case2: at Y=0.01 velocity is 0.1 m/sec

Conclusion

• The variation of pressure and velocity is captured well, at the near inlet, no-slip walls, and diverging section by case 2.
• Velocity profile obtained from GF=0.2 are accurate and smooth compared to the GF=1 cases.

THANK YOU