1.1. OpenFOAM Language

This is the OpenFOAM language.

1.1.1. What are features of C++?

Feature Meaning
typedefs Alias for a possibly complex type name
function Group of statements that perform a task
pointers Data type that holds addresses to refer to values in memory (e.g. for dynamic memory allocation)
data structures Data members grouped under one name (e.g. the nodes in a linked list)
classes Data members and function members grouped under one name
constructor Function member that initialises the instance of it’s class
destructor Function member that destroys the instance of it’s class
friends Allows a function or class access to private or protected members of a class
inheritance Allows a class to be created based on another class (so code can be reused)
virtual member functions Member function that will be redefined in a derived class
abstract class Class that contains at least one virtual function
template Family of classes (class template), functions (function template), variables (variable template) or alias of a family of types (alias template)
namespace Prevents name conflicts in large projects

1.1.2. What is explicit evaluation?

  • Evaluate spatial derivatives at the current timestep
  • Uses known values

1.1.3. What is implicit evaluation?

  • Evaluate spatial derivatives at future timestep
  • Uses unknown values - generates a matrix equation to be solved

1.1.4. What are the higher level data types?

Type Meaning
volScalarField
scalar, e.g. pressure
volVectorField
vector, e.g. velocity
volTensorField
tensor, e.g. Reynolds Stress
surfaceScalarField
surface scalar, e.g. flux
dimensionedScalar
constant, e.g. viscosity

1.1.5. What are fields?

  • Arrays of data stored at cell centres in the mesh

  • Include bouundary information

  • Three types
    • volScalarField
    • volVectorField
    • volTensorField
  • Values are stored in named dictionary files in named timestep directories e.g. case/0/p for pressure

1.1.6. What are the three types?

<Type> refers to:

  • scalar
  • vector
  • tensor

1.1.7. What are the five basic classes?

Class Meaning
fvPatchField

(and derived classes)

Boundary conditions
lduMatrix
fvMatrix

(and linear solvers)

Sparse matrices

1.1.8. What are the three space-time classes?

Class Meaning
polyMesh
  • Stands for polyhedral mesh

  • Most basic mesh class

  • Contains:
    • pointField
    • faceList
    • cellList
    • polyPatchList
fvMesh
  • Extends polyMesh contains:
    • Cell volumes (volScalarField)
    • Cell centres (volVectorField)
    • Face area vectors (surfaceVectorField)
    • Face centres (surfaceVectorField)
    • Face area magnitudes (surfaceScalarField)
    • Face motion centres (surfaceScalarField)
Time
  • Class to control time during OpenFOAM
    • Declared as variable runTime
    • Provides list of saved times runTime.times()
    • Timestep = deltaT()
    • Return current directory name = name()
    • Time increments = operator++() operator+=(scalar)
    • Write objects to disk = write()
    • Start time, end time = startTime(), endTime()

1.1.9. What are the three field algebra classes?

Class Meaning
Field<Type>
  • Array template class, e.g. Field<vector> = vectorField

  • Renamed using typedef as:
    • scalarField
    • vectorField
    • tensorField
    • symmTensorField
    • tensorThirdField
    • symmTensorThirdField
dimensionedField
 
geometricField<Type>
  • Combination of:
    • Field
    • GeometricBoundaryField
    • fvMesh
    • dimensionSet
  • Defines values at all locations in domain with aliases:
    • volField<Type>
    • surfaceField<Type>
    • pointField<Type>

1.1.10. What are the two discretisation classes?

Class Meaning
fvc
  • Stands for finite volume calculus
  • Explicit derivative evaluation
  • Input = known geometricField<Type>
  • Output = geometricField<Type> object
fvm
  • Stands for finite volume method
  • Implicit derivative evaluation
  • Input = unknown geometricField<Type>
  • Output = fvMatrix<Type> object, which can be inverted in the matrix equation Mx=y

1.1.11. What is a geometricField<Type>?

  • volField<Type>
  • surfaceField<Type>
  • pointField<Type>

1.1.12. What is the objectRegistry?

Object registry of entities (dictionaries, fields) which are to be read in or written out

1.1.13. What is the IOobject?

Defines I/O attributes of entities managed by the object registry.

1.1.14. How is a dictionary object read?

Code Meaning
Info << "Reading transportProperties" << endl;
Send message to screen
IOdictionary transportProperties
(
    IOobject
    (
        "transportProperties",
        runTime.constant(),
        mesh,
        IOobject::MUST_READ
        IOobject::NO_WRITE
    )
);
Read in at creation
dimensionedScalar nu
(
    transportProperties.lookup("nu")
);
Lookup viscosity in dictionary

1.1.15. How is volVectorField read from disk?

Code Meaning
volVectorField U
(
    IOobject
    (
        "U",
        Times[i].name(),
        runTime,
        IOobject::MUST_READ
    ),
    mesh
)
  • volVectorField read in from disk
  • Associated with runTime database
  • Must be read

1.1.16. How is volScalarField constructed?

Code Meaning
volVectorField magU
(
    IOobject
    (
        "magU",
        Times[i].name(),
        runTime,
        IOobject::NO_READ
        IOobject::AUTO_WRITE
    ),
    ::mag(U)
);
magU.write();
  • construct mag(U) object of type volScalarField called magU
  • write it out

1.1.17. What are the read and write options?

Class Meaning
NO_READ
Object created
MUST_READ
READ_IF_PRESENT
Object asked to read
NO_WRITE
Object destroyed
AUTO_WRITE
Object asked to write

1.1.18. How are objects represented in OpenFOAM?

How to create an object that writes the magnitude of a velocity vector?

Class Meaning
#include "fvCFD.H"
int main(int argc, char argv[])
{
# include "addTimeOptions.H"
# include "setRootCase.H"
# include "createTime.H"
instantList Times = runTime.times();
# include "createMesh.H"
  • One block called main is needed
  • #include to store commonly used code
  • runTime is a variable of the OpenFOAM Time class - for timestepping through code
for(label i=0; i<runTime.size(); i++)
{
    runTime.setTime(Times[i],i);
    Info << "Time: " << runTime.value() << endl
    volVectorField U
    (
        IOobject
        (
            "U",
            Times[i].name(),
            runTime,
            IOobject::MUST READ
        ),
        mesh
    );
  • Loop over all possible times
  • Read in a volVectorField U
    volScalarField magU
    (
        IOobject
        (
            "magU",
            Times[i].name(),
            runTime,
            IOobject::NO READ,
            IOobject::AUTO WRITE
        ),
        ::mag(U)
    );
    magU.write();
} return 0;}
  • Construct a volScalarField magU
  • Write out the velocity

1.1.19. How is matrix inversion done in fvm?

  • Each operator in fvm constructs particular entries in known M and y as a fvMatrix object
  • fvMatrix is a template class (actual classes are fvScalarMatrix etc)
  • fvMatrix handles storage via lduMatrix class
  • fvMatrix class also handles solution

1.1.20. What are lists?

Class Meaning
List<Type>
  • Array template class
  • Allows creation of a list of any object of a class e.g. List<vector>
PtrList<Type>
List of pointers
SLList<Type>
Non-intrusive singly-linked list

1.1.21. What are fields?

Class Meaning
Field<Type>
  • Array template class, e.g. Field<vector> = vectorField

  • Renamed as scalarField, vectorField, tensorField, symmTensorField,

    tensorThirdField and symmTensorThirdField

1.1.22. How is memory accessed?

  • Arrays
  • Pointers
  • References

1.1.23. How is IO Communication done?

Code Meaning
Info << "Time = " << runTime.timeName() << nl << endl;
Info object is output to the screen

1.1.24. How are derivatives of fields evaluated?

  • Time derivative

  • Divergence (div)
    • Spatial derivative
    • Discretised using the flux at the faces
    • e.g. \(\nabla \cdot (\mathbf{u}q)\) (the advection term)
  • Gradient (grad)
    • Spatial derivative
    • e.g. \(\nabla p\) in the momentum equation
  • Laplacian
    • Spatial derivative

    • Discretised as \(\nabla \cdot \mu \nabla q\)
      • gradient scheme for \(\nabla q\)
      • interpolation for \(\mu\)
      • discretisation for \(\nabla \cdot\)
    • e.g. \(\mu \nabla^2 q\) in the momentum equation

1.1.25. What are the functions for discretisation?

Function Meaning
fvc::ddt(A)
fvm::ddt(A)
  • Time derivative
  • \(\partial A / \partial t\)
  • \(A\) can be a scalar, vector or tensor
fvc::ddt(rho,A)
fvm::ddt(rho,A)
  • Density weighted time derivative
  • \(\partial \rho A / \partial t\)
  • \(\rho\) can be any scalar field
fvc::d2dt2(rho,A)
fvm::d2dt2(rho,A)
  • Second density weighted time derivative
  • \(\partial / \partial t ( \rho \partial A / \partial t)\)
fvc::grad(A)
fvm::grad(A)
  • Gradient
  • \(A\) can be a scalar or a vector
  • Result is a volVectorField (from scalar) or a volTensorField (from vector)
fvc::div(A)
fvm::div(A)
  • Divergence
  • \(A\) can be a vector or a tensor
  • Result is a volScalarField (from vector) or a volVectorField (from tensor)
fvc::laplacian(A)
fvm::laplacian(A)
  • Laplacian
  • \(\nabla^2 A\)
fvc::laplacian(mu, A)
fvm::laplacian(mu, A)
  • Laplacian
  • \(\nabla \cdot(\mu \nabla A)\)
fvc::curl(A)
fvm::curl(A)
  • Curl
  • \(\nabla \times A\)
fvm::div(phi,A)
  • Divergence using flux to evaluate this
  • \(A\) can be a scalar, vector or a tensor
fvm::Sp(rho,A)
  • Implicit evaulation of source term
fvm::SuSp(rho,A)
  • Implicit or explicit evaulation of source term (depending on sign of rho

1.1.26. How can are equations translated into code?

Equation Code
\({{\partial q} \over {\partial t}} + \nabla \cdot q \mathbf{u} = \mu \nabla^2 q\)
fvScalarMatrix transport
(
     fvm::ddt(q)
     + fvm::div(phi,q)
     - fvm::laplacian(mu,q)
);

// phi is the flux from the momentum equation
\({{\partial T} \over {\partial t}} = \kappa \nabla^2 T\)
solve(fvm::ddt(T) == kappa*fvc::laplacian(T))

// T is a volScalarField defined on the mesh
// A discretised representation of the field variable T
// solve performs matrix inversion for one step
\({{\partial k} \over {\partial t}} + \nabla \cdot k \mathbf{u} - \nabla \cdot [(\nu + \nu_t)\nabla k ]=\nu_t[1/2(\nabla \mathbf{u} + \nabla \mathbf{u}^T ]^2 - \varepsilon/k\)
solve(
     fvm::ddt(k)
     + fvm::div(phi,k)
     - fvm::laplacian(nu()+nut,k)
     == nut*magSqr(symm(fvc::grad(U)))
     - fvm::Sp(epsilon/k,k)
);

1.1.27. How is the PISO algorithm programmed?

The PISO (Pressure Implicit with Splitting of Operators) is an efficient method to solve the Navier-Stokes equations

The algorithm can be summed up as follows:

  • Set the boundary conditions.
  • Solve the discretized momentum equation to compute an intermediate velocity field.
  • Compute the mass fluxes at the cells faces.
  • Solve the pressure equation.
  • Correct the mass fluxes at the cell faces.
  • Correct the velocities on the basis of the new pressure field.
  • Update the boundary conditions.
  • Repeat from 3 for the prescribed number of times.
  • Increase the time step and repeat from 1.

The implementation:

  • Define the equation for U
fvVectorMatrix UEqn
(
   fvm::ddt(U)
 + fvm::div(phi, U)
 - fvm::laplacian(nu, U)
);
  • Solve the momentum predictor
solve (UEqn == -fvc::grad(p));
  • Calculate the ap coefficient and calculate U
volScalarField rUA = 1.0/UEqn().A();
U = rUA*UEqn().H();
  • Calculate the flux
phi = (fvc::interpolate(U) & mesh.Sf())
   + fvc::ddtPhiCorr(rUA, U, phi);
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(rUA, p) == fvc::div(phi)
);
pEqn.setReference(pRefCell, pRefValue);
pEqn.solve();
  • Correct the flux
if (nonOrth == nNonOrthCorr)
{
    phi -= pEqn.flux();
}
  • Calculate continuity errors
# include "continuityErrs.H"
  • Perform the momentum corrector step
U -= rUA*fvc::grad(p);
U.correctBoundaryConditions();

The following is from the OpenFOAM UK Users Group:

1.1.28. What are header files?

Sections of code in separate files that are widely used - all function prototypes in a header file

Equation Code
#include "CourantNumber.H"
File containing code for calculating Courant number

1.1.29. What is wmake?

  • wmake is a make system – directs the compiler to compile specific files in particular ways.

  • Controlled through files in Make:
    • files – specifies which user-written files to compile and what to call the result
    • options – specifies additional header files/libraries to be included in the compilation.