[Table of Contents] [Index] [ **Version 7** | Version 6 | Version 5 | Version 4 ]

## 4.5 Numerical schemes

The fvSchemes dictionary in the system directory sets the numerical schemes for terms, such as derivatives in equations, that are calculated during a simulation. This section describes how to specify the schemes in the fvSchemes dictionary.

The terms that must typically be assigned a numerical scheme in fvSchemes range from derivatives, e.g. gradient , to interpolations of values from one set of points to another. The aim in OpenFOAM is to offer an unrestricted choice to the user, starting with the choice of discretisation practice which is generally standard Gaussian finite volume integration. Gaussian integration is based on summing values on cell faces, which must be interpolated from cell centres. The user has a wide range of options for interpolation scheme, with certain schemes being specifically designed for particular derivative terms, especially the advection divergence terms.

The set of terms, for which numerical schemes must be specified, are subdivided within the fvSchemes dictionary into the categories below.

- timeScheme: first and second time derivatives, e.g.
- gradSchemes: gradient
- divSchemes: divergence
- laplacianSchemes: Laplacian
- interpolationSchemes: cell to face interpolations of values.
- snGradSchemes: component of gradient normal to a cell face.
- wallDist: distance to wall calculation, where required.

Each keyword in represents the name of a sub-dictionary which contains terms of a particular type, e.g. gradSchemes contains all the gradient derivative terms such as grad(p) (which represents ). Further examples can be seen in the extract from an fvSchemes dictionary below:

18ddtSchemes

19{

20 default Euler;

21}

22

23gradSchemes

24{

25 default Gauss linear;

26}

27

28divSchemes

29{

30 default none;

31

32 div(phi,U) Gauss linearUpwind grad(U);

33 div(phi,k) Gauss upwind;

34 div(phi,epsilon) Gauss upwind;

35 div(phi,R) Gauss upwind;

36 div(R) Gauss linear;

37 div(phi,nuTilda) Gauss upwind;

38

39 div((nuEff*dev2(T(grad(U))))) Gauss linear;

40}

41

42laplacianSchemes

43{

44 default Gauss linear corrected;

45}

46

47interpolationSchemes

48{

49 default linear;

50}

51

52snGradSchemes

53{

54 default corrected;

55}

56

57

58// ************************************************************************* //

The example shows that the fvSchemes dictionary contains 6 …Schemes subdictionaries containing keyword entries for each term specified within including: a default entry; other entries whose names correspond to a word identifier for the particular term specified, e.g. grad(p) for If a default scheme is specified in a particular …Schemes sub-dictionary, it is assigned to all of the terms to which the sub-dictionary refers, e.g. specifying a default in gradSchemes sets the scheme for all gradient terms in the application, e.g. , . When a default is specified, it is not necessary to specify each specific term itself in that sub-dictionary, i.e. the entries for grad(p), grad(U) in this example. However, if any of these terms are included, the specified scheme overrides the default scheme for that term.

Alternatively the user can specify that no default scheme by the none entry, as in the divSchemes in the example above. In this instance the user is obliged to specify all terms in that sub-dictionary individually. Setting default to none may appear superfluous since default can be overridden. However, specifying none forces the user to specify all terms individually which can be useful to remind the user which terms are actually present in the application.

OpenFOAM includes a vast number of discretisation schemes, from which only a few are typically recommended for real-world, engineering applications. The user can get help with scheme selection by interrogating the tutorial cases for example scheme settings. They should look at the schemes used in relevant cases, e.g. for running a large-eddy simulation (LES), look at schemes used in tutorials running LES. Additionally, foamSearch provides a useful tool to get a quick list of schemes used in all the tutorials. For example, to print all the default entries for ddtSchemes for cases in the $FOAM_TUTORIALS directory, the user can type:

foamSearch $FOAM_TUTORIALS fvSchemes ddtSchemes.default

default backward;

default CrankNicolson 0.9;

default Euler;

default localEuler;

default none;

default steadyState;

### 4.5.1 Time schemes

The first time derivative () terms are specified in the ddtSchemes sub-dictionary. The discretisation schemes for each term can be selected from those listed below.

- steadyState: sets time derivatives to zero.
- Euler: transient, first order implicit, bounded.
- backward: transient, second order implicit, potentially unbounded.
- CrankNicolson: transient, second order implicit, bounded; requires an off-centering coefficient where:

generally = 0.9 is used to bound/stabilise the scheme for practical engineering problems. - localEuler: pseudo transient for accelerating a solution to steady-state using local-time stepping; first order implicit.

Solvers are generally configured to simulate either transient or steady-state. Changing the time scheme from one which is steady-state to transient, or visa versa, does not affect the fundamental nature of the solver and so fails to achieve its purpose, yielding a nonsensical solution.

Any second time derivative () terms are specified in the d2dt2Schemes sub-dictionary. Only the Euler scheme is available for d2dt2Schemes.

### 4.5.2 Gradient schemes

The gradSchemes sub-dictionary contains gradient terms. The default discretisation scheme that is primarily used for gradient terms is:

default Gauss linear;

In some tutorials cases, particular involving poorer quality meshes, the discretisation of specific gradient terms is overridden to improve boundedness and stability. The terms that are overridden in those cases are the velocity gradient

grad(U) cellLimited Gauss linear 1;

grad(k) cellLimited Gauss linear 1;

grad(epsilon) cellLimited Gauss linear 1;

Other schemes that are rarely used are as follows.

- leastSquares: a second-order, least squares distance calculation using all neighbour cells.
- Gauss cubic: third-order scheme that appears in the dnsFoam simulation on a regular mesh.

### 4.5.3 Divergence schemes

The divSchemes sub-dictionary contains divergence terms, i.e. terms of the form …, excluding Laplacian terms (of the form ). This includes both advection terms, e.g. , where velocity provides the advective flux, and other terms, that are often diffusive in nature, e.g. .

The fact that terms that are fundamentally different reside in one sub-dictionary means that the default scheme in generally set to none in divSchemes. The non-advective terms then generally use the Gauss integration with linear interpolation, e.g.

div(U) Gauss linear;

The treatment of advective terms is one of the major challenges in CFD numerics and so the options are more extensive. The keyword identifier for the advective terms are usually of the form div(phi,…), where phi generally denotes the (volumetric) flux of velocity on the cell faces for constant-density flows and the mass flux for compressible flows, e.g. div(phi,U) for the advection of velocity, div(phi,e) for the advection of internal energy, div(phi,k) for turbulent kinetic energy, etc. For advection of velocity, the user can run the foamSearch script to extract the div(phi,U) keyword from all tutorials.

foamSearch $FOAM_TUTORIALS fvSchemes "divSchemes.div(phi,U)"

Ignoring ‘V’-schemes (with keywords ending “V”), and rarely-used schemes such as Gauss cubic and vanLeerV, the interpolation schemes used in the tutorials are as follows.

- linear: second order, unbounded.
- linearUpwind: second order, upwind-biased, unbounded (but much less so than linear), that requires discretisation of the velocity gradient to be specified.
- LUST: blended 75% linear/ 25%linearUpwind scheme, that requires discretisation of the velocity gradient to be specified.
- limitedLinear: linear scheme that limits towards upwind in regions of rapidly changing gradient; requires a coefficient, where 1 is strongest limiting, tending towards linear as the coefficient tends to 0.
- upwind: first-order bounded, generally too inaccurate to be recommended.

Example syntax for these schemes is as follows.

div(phi,U) Gauss linear;

div(phi,U) Gauss linearUpwind grad(U);

div(phi,U) Gauss LUST grad(U);

div(phi,U) Gauss LUST unlimitedGrad(U);

div(phi,U) Gauss limitedLinear 1;

div(phi,U) Gauss upwind;

div(phi,U) Gauss limitedLinearV 1;

div(phi,U) Gauss linearUpwindV grad(U);

The bounded variants of schemes relate to the treatment of the material time derivative which can be expressed in terms of a spatial time derivative and convection, e.g. for field in incompressible flow

| (4.1) |

div(phi,U) bounded Gauss limitedLinearV 1;

div(phi,U) bounded Gauss linearUpwindV grad(U);

The schemes used for advection of scalar fields are similar to those for advection of velocity, although in general there is greater emphasis placed on boundedness than accuracy when selecting the schemes. For example, a search for schemes for advection of internal energy (e) reveals the following.

foamSearch $FOAM_TUTORIALS fvSchemes "divSchemes.div(phi,e)"

div(phi,e) bounded Gauss upwind;

div(phi,e) Gauss limitedLinear 1;

div(phi,e) Gauss LUST grad(e);

div(phi,e) Gauss upwind;

div(phi,e) Gauss vanLeer;

There are specialised versions of the limited schemes for scalar fields that are commonly bounded between 0 and 1, e.g. the laminar flame speed regress variable . A search for the discretisation used for advection in the laminar flame transport equation yields:

div(phiSt,b) Gauss limitedLinear01 1;

The multivariateSelection mechanism also exists for grouping multiple equation terms together, and applying the same limiters on all terms, using the strongest limiter calculated for all terms. A good example of this is in a set of mass transport equations for fluid species, where it is good practice to apply the same discretisation to all equations for consistency. The example below comes from the smallPoolFire3D tutorial in $FOAM_TUTORIALS/combustion/fireFoam/les, in which the equation for enthalpy is included with the specie mass transport equations in the calculation of a single limiter.

div(phi,Yi_h) Gauss multivariateSelection

{

O2 limitedLinear01 1;

CH4 limitedLinear01 1;

N2 limitedLinear01 1;

H2O limitedLinear01 1;

CO2 limitedLinear01 1;

h limitedLinear 1 ;

}

### 4.5.4 Surface normal gradient schemes

It is worth explaining the snGradSchemes sub-dictionary that contains surface normal gradient terms, before discussion of laplacianSchemes, because they are required to evaluate a Laplacian term using Gaussian integration. A surface normal gradient is evaluated at a cell face; it is the component, normal to the face, of the gradient of values at the centres of the 2 cells that the face connects.

A search for the default scheme for snGradSchemes reveals the following entries.

default corrected;

default limited corrected 0.33;

default limited corrected 0.5;

default orthogonal;

default uncorrected;

The basis of the gradient calculation at a face is to subtract the value at the cell centre on one side of the face from the value in the centre on the other side and divide by the distance. The calculation is second-order accurate for the gradient normal to the face if the vector connecting the cell centres is orthogonal to the face, i.e. they are at right-angles. This is the orthogonal scheme.

Orthogonality requires a regular mesh, typically aligned with the Catersian co-ordinate system, which does not normally occur in meshes for real world, engineering geometries. Therefore, to maintain second-order accuracy, an explicit non-orthogonal correction can be added to the orthogonal component, known as the corrected scheme. The correction increases in size as the non-orthonality, the angle between the cell-cell vector and face normal vector, increases.

As tends towards 90, e.g. beyond 70, the explicit correction can be so large to cause a solution to go unstable. The solution can be stabilised by applying the limited scheme to the correction which requires a coefficient where

| (4.2) |

The corrected scheme applies under-relaxation in which the implicit orthogonal calculation is increased by , with an equivalent boost within the non-orthogonal correction. The uncorrected scheme is equivalent to the corrected scheme, without the non-orthogonal correction, so includes is like orthogonal but with the under-relaxation.

Generally the uncorrected and orthogonal schemes are only recommended for meshes with very low non-orthogonality (e.g. maximum 5). The corrected scheme is generally recommended, but for maximum non-orthogonality above 70, limited may be required. At non-orthogonality above 80, convergence is generally hard to achieve.

### 4.5.5 Laplacian schemes

The laplacianSchemes sub-dictionary contains Laplacian terms. A typical Laplacian term is , the diffusion term in the momentum equations, which corresponds to the keyword laplacian(nu,U) in laplacianSchemes. The Gauss scheme is the only choice of discretisation and requires a selection of both an interpolation scheme for the diffusion coefficient, i.e. in our example, and a surface normal gradient scheme, i.e. . To summarise, the entries required are:

Gauss <interpolationScheme> <snGradScheme>

foamSearch $FOAM_TUTORIALS fvSchemes laplacianSchemes.default

default Gauss linear corrected;

default Gauss linear limited corrected 0.33;

default Gauss linear limited corrected 0.5;

default Gauss linear orthogonal;

default Gauss linear uncorrected;

### 4.5.6 Interpolation schemes

The interpolationSchemes sub-dictionary contains terms that are interpolations of values typically from cell centres to face centres, primarily used in the interpolation of velocity to face centres for the calculation of flux phi. There are numerous interpolation schemes in OpenFOAM, but a search for the default scheme in all the tutorial cases reveals that linear interpolation is used in almost every case, except for 2-3 unusual cases, e.g. DNS on a regular mesh, stress analysis, where cubic interpolation is used.

© 2011-2019 OpenFOAM Foundation