3.3 Conditions

The final section of the file defines parameters and boundary conditions which define the nature of the problem to be solved. These are enclosed in the CONDITIONS tag.

3.3.1 Parameters

Parameters may be required by a particular solver (for instance time-integration parameters or solver-specific parameters), or arbitrary and only used within the context of the session file (e.g. parameters in the definition of an initial condition). All parameters are enclosed in the PARAMETERS XML element.

2    ... 

A parameter may be of integer or real type and may reference other parameters defined previous to it. It is expressed in the file as


For example,

1<P> NumSteps = 1000              </P> 
2<P> TimeStep = 0.01              </P> 
3<P> FinTime  = NumSteps*TimeStep </P>

3.3.2 Solver Information

These specify properties to define the actions specific to solvers, typically including the equation to solve, the projection type and the method of time integration. The property/value pairs are specified as XML attributes. For example,

2  <I PROPERTY="EQTYPE"                VALUE="UnsteadyAdvection"    /> 
3  <I PROPERTY="Projection"            VALUE="Continuous"           /> 
4  <I PROPERTY="TimeIntegrationMethod" VALUE="ClassicalRungeKutta4" /> 

The list of available solvers in Nektar++ can be found in Part III. Drivers

Drivers are defined under the CONDITIONS section as properties of the SOLVERINFO XML element. The role of a driver is to manage the solver execution from an upper level.

The default driver is called Standard and executes the following steps:

  1. Prints out on screen a summary of all the conditions defined in the input file.
  2. Sets up the initial and boundary conditions.
  3. Calls the solver defined by SolverType in the SOLVERINFO XML element.
  4. Writes the results in the output (.fld) file.

In the following example, the driver Standard is used to manage the execution of the incompressible Navier-Stokes equations:

2    <I PROPERTY="EQTYPE" VALUE="UnsteadyNavierStokes" /> 
3    <I PROPERTY="SolverType" VALUE="VelocityCorrectionScheme" /> 
4    <I PROPERTY="Projection" VALUE="Galerkin" /> 
5    <I PROPERTY="TimeIntegrationMethod" VALUE="IMEXOrder2" /> 
6    <I PROPERTY="Driver" VALUE="Standard" /> 

If no driver is specified in the session file, the driver Standard is called by default. Other drivers can be used and are typically focused on specific applications. As described in Sec. 10.3.1 and 10.4.1, the other possibilities are:

3.3.3 Variables

These define the number (and name) of solution variables. Each variable is prescribed a unique ID. For example a two-dimensional flow simulation may define the velocity variables using

2  <V ID="0"> u </V> 
3  <V ID="1"> v </V> 

3.3.4 Global System Solution Information

Many Nektar++ solvers use an implicit formulation of their equations to, for instance, improve timestep restrictions. This means that a large matrix system must be constructed and a global system set up to solve for the unknown coefficients. There are several approaches in the spectral/hp element method that can be used in order to improve efficiency in these methods, as well as considerations as to whether the simulation is run in parallel or serial. Nektar++ opts for ‘sensible’ default choices, but these may or may not be optimal depending on the problem under consideration.

This section of the XML file therefore allows the user to specify the global system solution parameters, which dictates the type of solver to be used for any implicit systems that are constructed. This section is particularly useful when using a multi-variable solver such as the incompressible Navier-Stokes solver, as it allows us to select different preconditioning and residual convergence options for each variable. As an example, consider the block defined by:

2  <V VAR="u,v,w"> 
3    <I PROPERTY="GlobalSysSoln"             VALUE="IterativeStaticCond" /> 
4    <I PROPERTY="Preconditioner"            VALUE="LowEnergyBlock"/> 
5    <I PROPERTY="IterativeSolverTolerance"  VALUE="1e-8"/> 
6  </V> 
7  <V VAR="p"> 
8    <I PROPERTY="GlobalSysSoln"             VALUE="IterativeStaticCond" /> 
9    <I PROPERTY="Preconditioner"     VALUE="FullLinearSpaceWithLowEnergyBlock"/> 
10    <I PROPERTY="IterativeSolverTolerance"  VALUE="1e-6"/> 
11  </V> 

The above section specifies that the variables u,v,w should use the IterativeStaticCond global solver alongside the LowEnergyBlock preconditioner and an iterative tolerance of 10-8 on the residuals. However the pressure variable p is generally stiffer: we therefore opt for a more expensive FullLinearSpaceWithLowEnergyBlock preconditioner and a larger residual of 10-6. We now outline the choices that one can use for each of these parameters and give a brief description of what they mean.

Note: Defaults for all fields can be defined by setting the equivalent property in the SOLVERINFO section. Parameters defined in this section will override any options specificed there. GlobalSysSoln options

Nektar++ presently implements four methods of solving a global system:

Both the Xxt and PETSc solvers are considered advanced and are under development – either the direct or iterative solvers are recommended in most scenarios.

These solvers can be run in one of three approaches:

The GlobalSysSoln option is formed by combining the method of solution with the approach: for example IterativeStaticCond or PETScMultiLevelStaticCond. Preconditioner options

Preconditioners can be used in the iterative and PETSc solvers to reduce the number of iterations needed to converge to the solution. There are a number of preconditioner choices, the default being a simple Jacobi (or diagonal) preconditioner, which is enabled by default. There are a number of choices that can be enabled through this parameter, which are all generally discretisation and dimension-dependent:

Name Dimensions Discretisations
Null All All
Diagonal All All
FullLinearSpace 2/3D CG
LowEnergyBlock 3D CG
Block 2/3D All
FullLinearSpaceWithDiagonal All CG
FullLinearSpaceWithLowEnergyBlock 2/3D CG
FullLinearSpaceWithBlock 2/3D CG

For a detailed discussion of the mathematical formulation of these options, see the developer guide. SuccessiveRHS options

The SuccessiveRHS option can be used in the iterative solver only, to attempt to reduce the number of iterations taken to converge to a solution. It stores a number of previous solutions, dictated by the setting of the SuccessiveRHS option, to give a better initial guess for the iterative process. PETSc options and configuration

The PETSc solvers, although currently experimental, are operational both in serial and parallel. PETSc gives access to a wide range of alternative solver options such as GMRES, as well as any packages that PETSc can link against, such as the direct multi-frontal solver MUMPS.

Configuration of PETSc options using its command-line interface dictates what matrix storage, solver type and preconditioner should be used. This should be specified in a .petscrc file inside your working directory, as command line options are not currently passed through to PETSc to avoid conflict with Nektar++ options. As an example, to select a GMRES solver using an algebraic multigrid preconditioner, and view the residual convergence, one can use the configuration:

-ksp_type gmres 
-pc_type gamg

Or to use MUMPS, one could use the options:

-ksp_type preonly 
-pc_type lu 
-pc_factor_mat_solver_package mumps 
-mat_mumps_icntl_7 2

A final choice that can be specified is whether to use a shell approach. By default, Nektar++ will construct a PETSc sparse matrix (or whatever matrix is specified on the command line). This may, however, prove suboptimal for higher order discretisations. In this case, you may choose to use the Nektar++ matrix-vector operators, which by default use an assembly approach that can prove faster, by setting the PETScMatMult SOLVERINFO option to Shell:

1<I PROPERTY="PETScMatMult" VALUE="Shell" />

The downside to this approach is that you are now constrained to using one of the Nektar++ preconditioners. However, this does give access to a wider range of Krylov methods than are available inside Nektar++ for more advanced users.

3.3.5 Boundary Regions and Conditions

Boundary conditions are defined by two XML elements. The first defines the boundary regions in the domain in terms of composite entities from the GEOMETRY section of the file. Each boundary region has a unique ID and are defined as,

2    <B ID=[id]> [composite-list] </B> 
3    ... 

For example,

2  <B ID="0"> C[2] </B> 
3  <B ID="1"> C[3] </B> 

The second XML element defines, for each variable, the condition to impose on each boundary region, and has the form,

2    <REGION REF="[regionID]"> 
3      <[type1] VAR="[variable1]" VALUE="[expression1]" /> 
4      ... 
5      <[typeN] VAR="[variableN]" VALUE="[expressionN]" /> 
6    </REGION> 
7    ... 

There should be precisely one REGION entry for each B entry defined in the BOUNDARYREGION section above. For example, to impose a Dirichlet condition on both variables for a domain with a single region,

2  <REGION REF="0"> 
3    <D VAR="u" VALUE="sin(PI*x)*cos(PI*y)" /> 
4    <D VAR="v" VALUE="sin(PI*x)*cos(PI*y)" /> 
5  </REGION> 

Boundary condition specifications may refer to any parameters defined in the session file. The REF attribute corresponds to a defined boundary region. The tag used for each variable specifies the type of boundary condition to enforce. Dirichlet (essential) condition

Dirichlet conditions are specified with the D tag.

Projection Homogeneous support Time-dependent support Dimensions
CG Yes Yes 1D, 2D and 3D
DG Yes Yes 1D, 2D and 3D
HDG Yes Yes 1D, 2D and 3D


1<!-- homogeneous condition --> 
2<D VAR="u" VALUE="0" /> 
3<!-- inhomogeneous condition --> 
4<D VAR="u" VALUE="x^2+y^2+z^2" /> 
5<!-- time-dependent condition --> 
6<D VAR="u" USERDEFINEDTYPE="TimeDependent" VALUE="x+t" /> Neumann (natural) condition

Neumann conditions are specified with the N tag.

Projection Homogeneous support Time-dependent support Dimensions
CG Yes Yes 1D, 2D and 3D
DG No No 1D, 2D and 3D
HDG ? ? ?


1<!-- homogeneous condition --> 
2<N VAR="u" VALUE="0" /> 
3<!-- inhomogeneous condition --> 
4<N VAR="u" VALUE="x^2+y^2+z^2" /> 
5<!-- time-dependent condition --> 
6<N VAR="u" USERDEFINEDTYPE="TimeDependent" VALUE="x+t" /> 
7<!-- high-order pressure boundary condition (for IncNavierStokesSolver) --> 
8<N VAR="u" USERDEFINEDTYPE="H" VALUE="0" /> Periodic condition

Periodic conditions are specified with the P tag.

Projection Homogeneous support Dimensions
CG Yes 1D, 2D and 3D
DG No 2D and 3D


2  <B ID="0"> C[1] </B> 
3  <B ID="1"> C[2] </B> 
7  <REGION REF="0"> 
8    <P VAR="u" VALUE="[1]" /> 
9  </REGION> 
10  <REGION REF="1"> 
11    <P VAR="u" VALUE="[0]" /> 
12  </REGION> 

Periodic boundary conditions are specified in a significantly different form to other conditions. The VALUE property is used to specify which BOUNDARYREGION is periodic with the current region in square brackets.

Caveats: Time-dependent boundary conditions

Time-dependent boundary conditions may be specified through setting the USERDEFINEDTYPE attribute and using the parameter t where the current time is required. For example,

1<D VAR="u" USERDEFINEDTYPE="TimeDependent" VALUE="sin(PI*(x-t))" /> Boundary conditions from file

Boundary conditions can also be loaded from file. The following example is from the Incompressible Navier-Stokes solver,

1<REGION REF="1"> 
2  <D VAR="u" FILE="Test_ChanFlow2D_bcsfromfiles_u_1.bc" /> 
3  <D VAR="v" VALUE="0" /> 

Boundary conditions can also be loaded simultaneously from a file and from an analytic expression. For example in the scenario where a spatial boundary condition is read from a file, but needs to be modulated by a time-dependent analytic expression:

1<REGION REF="1"> 
2  <D VAR="u" VALUE="USERDEFINEDTYPE="TimeDependent" VALUE="sin(PI*(x-t))" 
3             FILE="bcsfromfiles_u_1.bc" /> 

In the case where both VALUE and FILE are specified, the values are multiplied together to give the final value for the boundary condition.

3.3.6 Functions

Finally, multi-variable functions such as initial conditions and analytic solutions may be specified for use in, or comparison with, simulations. These may be specified using expressions (<E>) or imported from a file (<F>) using the Nektar++ FLD file format

1<FUNCTION NAME="ExactSolution"> 
2  <E VAR="u" VALUE="sin(PI*x-advx*t))*cos(PI*(y-advy*t))" /> 
4<FUNCTION NAME="InitialConditions"> 
5  <F VAR="u" FILE="session.rst" /> 

A restart file is a solution file (in other words an .fld renamed as .rst) where the field data is specified. The expansion order used to generate the .rst file must be the same as that for the simulation. .pts files contain scattered point data which needs to be interpolated to the field. For further information on the file format and the different interpolation schemes, see section 5.3.11. All filenames must be specified relative to the location of the .xml file.

With the additional argument TIMEDEPENDENT="1", different files can be loaded for each timestep. The filenames are defined using boost::format syntax where the step time is used as variable. For example, the function Baseflow would load the files U0V0_1.00000000E-05.fld, U0V0_2.00000000E-05.fld and so on.

1<FUNCTION NAME="Baseflow"> 
2       <F VAR="U0,V0" TIMEDEPENDENT="1"FILE="U0V0_%14.8E.fld"/> 

For .pts files, the time consuming computation of interpolation weights in only performed for the first timestep. The weights are stored and reused in all subsequent steps, which is why all consecutive .pts files must use the same ordering, number and location of data points.

Other examples of this input feature can be the insertion of a forcing term,

1<FUNCTION NAME="BodyForce"> 
2  <E VAR="u" VALUE="0" /> 
3  <E VAR="v" VALUE="0" /> 
5<FUNCTION NAME="Forcing"> 
6  <E VAR="u" VALUE="-(Lambda + 2*PI*PI)*sin(PI*x)*sin(PI*y)" /> 

or of a linear advection term

1<FUNCTION NAME="AdvectionVelocity"> 
2  <E VAR="Vx" VALUE="1.0" /> 
3  <E VAR="Vy" VALUE="1.0" /> 
4  <E VAR="Vz" VALUE="1.0" /> 
5</FUNCTION> Remapping variable names

Note that it is sometimes the case that the variables being used in the solver do not match those saved in the FLD file. For example, if one runs a three-dimensional incompressible Navier-Stokes simulation, this produces an FLD file with the variables u, v, w and p. If we wanted to use this velocity field as input for an advection velocity, the advection-diffusion-reaction solver expects the variables Vx, Vy and Vz.

We can manually specify this mapping by adding a colon to the

1<FUNCTION NAME="AdvectionVelocity"> 
2  <F VAR="Vx,Vy,Vz" FILE="file.fld:u,v,w" /> 

There are some caveats with this syntax: Time-dependent file-based functions

With the additional argument TIMEDEPENDENT="1", different files can be loaded for each timestep. The filenames are defined using boost::format syntax where the step time is used as variable. For example, the function Baseflow would load the files U0V0_1.00000000E-05.fld, U0V0_2.00000000E-05.fld and so on.

1<FUNCTION NAME="Baseflow"> 
2  <F VAR="U0,V0" TIMEDEPENDENT="1" FILE="U0V0_%14.8R.fld" /> 

Section 3.6 provides the list of acceptable mathematical functions and other related technical details.

3.3.7 Quasi-3D approach

To generate a Quasi-3D appraoch with Nektar++ we only need to create a 2D or a 1D mesh, as reported above, and then specify the parameters to extend the problem to a 3D case. For a 2D spectral/hp element problem, we have a 2D mesh and along with the parameters we need to define the problem (i.e. equation type, boundary conditions, etc.). The only thing we need to do, to extend it to a Quasi-3D approach, is to specify some additional parameters which characterise the harmonic expansion in the third direction. First we need to specify in the solver information section that that the problem will be extended to have one homogeneouns dimension; here an example

2  <I PROPERTY="SolverType"            VALUE="VelocityCorrectionScheme"/> 
3  <I PROPERTY="EQTYPE"                VALUE="UnsteadyNavierStokes"/> 
4  <I PROPERTY="AdvectionForm"         VALUE="Convective"/> 
5  <I PROPERTY="Projection"            VALUE="Galerkin"/> 
6  <I PROPERTY="TimeIntegrationMethod" VALUE="IMEXOrder2"/> 
7  <I PROPERTY="HOMOGENEOUS"           VALUE="1D"/> 

then we need to specify the parameters which define the 1D harmonic expanson along the z-axis, namely the homogeneous length (LZ) and the number of modes in the homogeneous direction (HomModesZ). HomModesZ corresponds also to the number of quadrature points in the homogenous direction, hence on the number of 2D planes discretized with a specral/hp element method.

2  <P> TimeStep      = 0.001   </P> 
3  <P> NumSteps      = 1000    </P> 
4  <P> IO_CheckSteps = 100     </P> 
5  <P> IO_InfoSteps  = 10      </P> 
6  <P> Kinvis        = 0.025   </P> 
7  <P> HomModesZ     = 4       </P> 
8  <P> LZ            = 1.0     </P> 

In case we want to create a Quasi-3D approach starting form a 1D spectral/hp element mesh, the procedure is the same, but we need to specify the parameters for two harmonic directions (in Y and Z direction). For Example,

2  <I PROPERTY="EQTYPE"                VALUE="UnsteadyAdvectionDiffusion" /> 
3  <I PROPERTY="Projection"            VALUE="Continuous"/> 
4  <I PROPERTY="HOMOGENEOUS"           VALUE="2D"/> 
5  <I PROPERTY="DiffusionAdvancement"  VALUE="Implicit"/> 
6  <I PROPERTY="AdvectionAdvancement"  VALUE="Explicit"/> 
7  <I PROPERTY="TimeIntegrationMethod" VALUE="IMEXOrder2"/> 
10  <P> TimeStep      = 0.001 </P> 
11  <P> NumSteps      = 200   </P> 
12  <P> IO_CheckSteps = 200   </P> 
13  <P> IO_InfoSteps  = 10    </P> 
14  <P> wavefreq      = PI    </P> 
15  <P> epsilon       = 1.0   </P> 
16  <P> Lambda        = 1.0   </P> 
17  <P> HomModesY     = 10    </P> 
18  <P> LY            = 6.5   </P> 
19  <P> HomModesZ     = 6     </P> 
20  <P> LZ            = 2.0   </P> 

By default the opeartions associated with the harmonic expansions are performed with the Matix-Vector-Multiplication (MVM) defined inside the code. The Fast Fourier Transofrm (FFT) can be used to speed up the operations (if the FFTW library has been compiled in ThirdParty, see the compilation instructions). To use the FFT routines we need just to insert a flag in the solver information as below:

2  <I PROPERTY="EQTYPE"                VALUE="UnsteadyAdvectionDiffusion" /> 
3  <I PROPERTY="Projection"            VALUE="Continuous"/> 
4  <I PROPERTY="HOMOGENEOUS"           VALUE="2D"/> 
5  <I PROPERTY="DiffusionAdvancement"  VALUE="Implicit"/> 
6  <I PROPERTY="AdvectionAdvancement"  VALUE="Explicit"/> 
7  <I PROPERTY="TimeIntegrationMethod" VALUE="IMEXOrder2"/> 
8  <I PROPERTY="USEFFT"                VALUE="FFTW"/> 

The number of homogenenous modes has to be even. The Quasi-3D apporach can be created starting from a 2D mesh and adding one homogenous expansion or starting form a 1D mesh and adding two homogeneous expansions. Not other options available. In case of a 1D homogeneous extension, the homogeneous direction will be the z-axis. In case of a 2D homogeneous extension, the homogeneous directions will be the y-axis and the z-axis.