OpenFOAM guide/The SIMPLE algorithm in OpenFOAM

From OpenFOAMWiki
Jump to: navigation, search

Valid versions: OF version 14.png OF version 15.png OF version 16.png


1 The Navier-Stokes equations

The Navier-Stokes equations for a single-phase flow with a constant density and viscosity are the following:

 \nabla \cdot \left( \rho \vec{U} \right) = 0

 \frac{\partial U}{\partial t} + \nabla \cdot \left( \vec{v} \vec{v} \right) - \nabla \cdot \left( \nu \nabla \vec{v} \right) = - \nabla p

The solution of this couple of equations is not straightforward because an explicit equation for the pressure is not available. One of the most common approaches is to derive an equation for the pressure by taking the divergence of the momentum equation and by substituting it in the continuity equation.

2 The pressure equation

The momentum equation can be re-written in a semi discretised form as follows:

 a_p \vec{U_p} = H(\vec{U}) - \nabla p \Longleftrightarrow \vec{U_p} = \frac{H(\vec{U})}{a_p} - \frac{\nabla p}{a_p}


H(\vec{U}) = - \sum_n a_n \vec{U}_n + \frac{\vec{U}^o}{\Delta t}

The first term of H(\vec{U}) represents the matrix coefficients of the neighbouring cells multiplied by their velocity, while the second part contains the unsteady term and all the sources except the pressure gradient.

The continuity equation is discretised as:

 \nabla \cdot \vec{U} = \sum_f \vec{S} \vec{U}_f = 0

where \vec{S} is outward-pointing face area vector and \vec{U}_f the velocity on the face.

The velocity on the face is obtained by interpolating the semi discretised form of the momentum equation as follows:

 \vec{U}_f = \left( \frac{H(\vec{U})}{a_p}\right)_f - \frac{\left( \nabla p\right)_f }{\left( a_p\right)_f}

By substituting this equation into the discretised continuity equation obtained above, we obtain the pressure equation:

 \nabla \cdot \left( \frac{1}{a_p} \nabla p \right) = \nabla \cdot \left( \frac{H(\vec{U})}{a_p} \right) = \sum_f \vec{S} \left( \frac{H(\vec{U})}{a_p}\right)_f

3 The SIMPLE algorithm

The SIMPLE (Semi-Implicit Method for Pressure-Linked Equations) allows to couple the Navier-Stokes equations with an iterative procedure, which can be summed up as follows:

  1. Set the boundary conditions.
  2. Solve the discretized momentum equation to compute the intermediate velocity field.
  3. Compute the mass fluxes at the cells faces.
  4. Solve the pressure equation and apply under-relaxation.
  5. Correct the mass fluxes at the cell faces.
  6. Correct the velocities on the basis of the new pressure field.
  7. Update the boundary conditions.
  8. Repeat till convergence.

The steps 4 and 5 can be repeated for a prescribed number of time to correct for non-orthogonality.

4 Implementation of the SIMPLE algorithm in OpenFOAM

The SIMPLE algorithm can be implemented in OpenFOAM as follows (The complete implementation of the algorithm can be seen in the source code of the simpleFoam solver provided with OpenFOAM):

  • Store the pressure calculated at the previous iteration, because it is required to apply under-relaxation
  • Define the equation for U
 tmp<fvVectorMatrix> UEqn
      fvm::div(phi, U) - fvm::laplacian(nu, U)

tmp< > is used to reduce peak memory.

  • Under-relax the equation for U
  • Solve the momentum predictor
 solve (UEqn == -fvc::grad(p));
  • Update the boundary conditions for p
  • Calculate the ap coefficient and calculate U
 volScalarField AU = UEqn().A();
 U = UEqn().H()/AU;
  • Calculate the flux
 phi = fvc::interpolate(U) & mesh.Sf();
 adjustPhi(phi, U, p);
  • Define and solve the pressure equation and repeat for the prescribed number of non-orthogonal corrector steps
 fvScalarMatrix pEqn
   fvm::laplacian(1.0/AU, p) == fvc::div(phi)
 pEqn.setReference(pRefCell, pRefValue);
  • Correct the flux
 phi -= pEqn.flux();
  • Calculate continuity errors
# include "continuityErrs.H"
  • Under-relax the pressure for the momentum corrector and apply the correction
 U -= fvc::grad(p)/AU;
  • Check for convergence and repeat from the beginning until convergence criteria are satisfied.

Note: In OpenFOAM 1.6. and 1.6.x the convergence check has been implemented in simpleFoam by defining

    • eqnResidual: Initial residual of the equation
    • maxResidual: Maximum residual of the equations after one solution step
    • convergenceCriterion: Convergence criterion specified by the user

The value of the initial residual can be obtained when solving the corresponding equation using the initialResidual() method. Two syntax are possible:

eqnResidual = solve
                UEqn() == -fvc::grad(p)

or, equivalently, for the pressure equation, since it has been already defined,

 eqnResidual = pEqn.solve().initialResidual();

5 References

J. H. Ferziger, M. Peric, Computational Methods for Fluid Dynamics, Springer, 3rd Ed., 2001.

H. Jasak, Error Analysis and Estimation for the Finite Volume Method with Applications to Fluid Flows, Ph.D. Thesis, Imperial College, London, 1996.