The fvSchemes dictionary in the system directory sets the numerical schemes for terms, such as derivatives in equations, that appear in applications being run. 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 , and interpolations of values from one set of points to another. The aim in OpenFOAM is to offer an unrestricted choice to the user. For example, while linear interpolation is effective in many cases, OpenFOAM offers complete freedom to choose from a wide selection of interpolation schemes for all interpolation terms.
The derivative terms further exemplify this freedom of choice. The user first has a choice of discretisation practice where standard Gaussian finite volume integration is the common choice. Gaussian integration is based on summing values on cell faces, which must be interpolated from cell centres. The user again has a completely free choice of interpolation scheme, with certain schemes being specifically designed for particular derivative terms, especially the convection divergence terms.
The set of terms, for which numerical schemes must be specified, are subdivided within the fvSchemes dictionary into the categories listed in Table 4.5. Each keyword in Table 4.5 is 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:
20 default Euler;
25 default Gauss linear;
26 grad(p) Gauss linear;
31 default none;
32 div(phi,U) Gauss linear;
37 default none;
38 laplacian(nu,U) Gauss linear orthogonal;
39 laplacian((1|A(U)),p) Gauss linear orthogonal;
44 default linear;
45 interpolate(HbyA) linear;
50 default orthogonal;
55 default no;
56 p ;
60 // ************************************************************************* //
The example shows that the fvSchemes dictionary contains the following:
- 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
- a fluxRequired sub-dictionary containing fields for which the flux is generated in the application, e.g.p in the example.
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 may insist on no default scheme by the none entry. 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.
The following sections describe the choice of schemes for each of the categories of terms in Table 4.5.
The interpolationSchemes sub-dictionary contains terms that are interpolations of values typically from cell centres to face centres. A selection of interpolation schemes in OpenFOAM are listed in Table 4.6, being divided into 4 categories: 1 category of general schemes; and, 3 categories of schemes used primarily in conjunction with Gaussian discretisation of convection (divergence) terms in fluid flow, described in section 4.4.5. It is highly unlikely that the user would adopt any of the convection-specific schemes for general field interpolations in the interpolationSchemes sub-dictionary, but, as valid interpolation schemes, they are described here rather than in section 4.4.5. Note that additional schemes such as UMIST are available in OpenFOAM but only those schemes that are generally recommended are listed in Table 4.6.
A general scheme is simply specified by quoting the keyword and entry, e.g. a linear scheme is specified as default by:
The convection-specific schemes calculate the interpolation based on the flux of the flow velocity. The specification of these schemes requires the name of the flux field on which the interpolation is based; in most OpenFOAM applications this is phi, the name commonly adopted for the surfaceScalarField velocity flux . The 3 categories of convection-specific schemes are referred to in this text as: general convection; normalised variable (NV); and, total variation diminishing (TVD). With the exception of the blended scheme, the general convection and TVD schemes are specified by the scheme and flux, e.g. an upwind scheme based on a flux phi is specified as default by:
default upwind phi;
Some TVD/NVD schemes require a coefficient where corresponds to TVD conformance, usually giving best convergence and corresponds to best accuracy. Running with is generally recommended. A limitedLinear scheme based on a flux phi with is specified as default by:
default limitedLinear 1.0 phi;
There are enhanced versions of some of the limited schemes for scalars that need to be strictly bounded. To bound between user-specified limits, the scheme name should be preceded by the word limited and followed by the lower and upper limits respectively. For example, to bound the vanLeer scheme strictly between -2 and 3, the user would specify:
default limitedVanLeer -2.0 3.0;
There are improved versions of some of the limited schemes for vector fields in which the limiter is formulated to take into account the direction of the field. These schemes are selected by adding V to the name of the general scheme, e.g.limitedLinearV for limitedLinear. ‘V’ versions are available for the following schemes: limitedLinearV, vanLeerV, GammaV, limitedCubicV and SFCDV.
The snGradSchemes sub-dictionary contains surface normal gradient terms. 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 surface normal gradient may be specified in its own right and is also required to evaluate a Laplacian term using Gaussian integration.
The available schemes are listed in Table 4.7 and are specified by simply quoting the keyword and entry, with the exception of limited which requires a coefficient where
A limited scheme with is therefore specified as default by:
default limited 0.5;
The gradSchemes sub-dictionary contains gradient terms. The discretisation scheme for each term can be selected from those listed in Table 4.8.
The discretisation scheme is sufficient to specify the scheme completely in the cases of leastSquares and fourth, e.g.
The Gauss keyword specifies the standard finite volume discretisation of Gaussian integration which requires the interpolation of values from cell centres to face centres. Therefore, the Gauss entry must be followed by the choice of interpolation scheme from Table 4.6. It would be extremely unusual to select anything other than general interpolation schemes and in most cases the linear scheme is an effective choice, e.g.
grad(p) Gauss linear;
grad(p) cellLimited Gauss linear 1;
The laplacianSchemes sub-dictionary contains Laplacian terms. Let us discuss the syntax of the entry in reference to a typical Laplacian term found in fluid dynamics, , given the word identifier laplacian(nu,U). 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>
laplacian(nu,U) Gauss linear corrected;
The divSchemes sub-dictionary contains divergence terms. Let us discuss the syntax of the entry in reference to a typical convection term found in fluid dynamics , which in OpenFOAM applications is commonly given the identifier div(phi,U), where phi refers to the flux .
The Gauss scheme is the only choice of discretisation and requires a selection of the interpolation scheme for the dependent field, i.e. in our example. To summarise, the entries required are:
div(phi,U) Gauss upwind;
The first time derivative () terms are specified in the ddtSchemes sub-dictionary. The discretisation scheme for each term can be selected from those listed in Table 4.11.
There is an off-centering coefficient with the CrankNicholson scheme that blends it with the Euler scheme. A coefficient of corresponds to pure CrankNicholson and and corresponds to pure Euler. The blending coefficient can help to improve stability in cases where pure CrankNicholson are unstable.
When specifying a time scheme it must be noted that an application designed for transient problems will not necessarily run as steady-state and visa versa. For example the solution will not converge if steadyState is specified when running icoFoam, the transient, laminar incompressible flow code; rather, simpleFoam should be used for steady-state, incompressible flow.
Any second time derivative () terms are specified in the d2dt2Schemes sub-dictionary. Only the Euler scheme is available for d2dt2Schemes.
The fluxRequired sub-dictionary lists the fields for which the flux is generated in the application. For example, in many fluid dynamics applications the flux is generated after solving a pressure equation, in which case the fluxRequired sub-dictionary would simply be entered as follows, p being the word identifier for pressure:
This User Guide is licensed under a Creative Commons Attribution-NonCommercial-NoDerivs 3.0 Unported License .