In the following the possible options are shown for the incompressible Navier-Stokes. The
Expansion section for an incompressible flow simulation can be set as for other solvers
regardless of the projection type. Here an example for a 3D simulation (for 2D simulations the
specified fields would be just u,v,p).
In case of a simulation using the Direct Solver we need to set FIELDS=u,v as the pressure
expansion order will be automatically set to fulfil the inf-sup condition. Possible choices for
the expansion TYPE are:
| Basis | TYPE |
Modal | MODIFIED |
Nodal | GLL_LAGRANGE |
Nodal SEM | GLL_LAGRANGE_SEM |
The following parameters can be specified in the SOLVERINFO section of the session
file:
EqType: sets the kind of equations we want to solve on the domain as:
Possible values are:
| Equations | EQTYPE | Dim. | Projections | Alg. |
| Steady Stokes (SS) | SteadyStokes | All | CG | VCS |
| Steady Oseen (SO) | SteadyOseen | All | CG | DS |
| Unsteady Stokes (US) | UnsteadyStokes | All | CG | VCS |
| Steady Linearised NS (SLNS) | SteadyLinearisedNS | All | CG | DS |
| Unsteady Linearised NS (ULNS) | UnsteadyLinearisedNS | All | CG | VCS,DS |
| Unsteady NS (UNS) | UnsteadyNavierStokes | All | CG,CG-DG | VCS |
SolverType: sets the scheme we want to use to solve the set of equations as
Possible values are:
| Algorithm | SolverType | Dimensions | Projections |
| Velocity Correction Scheme | VelocityCorrectionScheme | 2D, Quasi-3D, 3D | CG, CG-DG |
| Direct solver | CoupledLinearisedNS | 2D, Quasi-3D, 3D | CG |
Driver: this specifies the type of problem to be solved:
| Driver | Description | Dimensions | Projections |
Standard | Time integration of the equations | All | CG, DG |
SteadyState | Steady-state solver (see Sec. 8.1.4) | All | CG, DG |
Projection: sets the Galerkin projection type as
Possible values are:
| Galerkin Projection | Projection | Dimensions | Equations | Algorithms |
| Continuous (CG) | Continuous | All | All | All |
| Discontinuous (DG) | DisContinuous | All | ... | ... |
| Mixed CG and DG (CG-DG) | MixedCGDG | just 2D | just UNS | just VCS |
TimeIntegrationMethod: sets the time integration method as
Possible values are
| Time-Integration Method | TimeIntegrationMethod | Dimensions | Equations | Projections |
| IMEX Order 1 | IMEXOrder1 | all | US, UNS | CG |
| IMEX Order 2 | IMEXOrder2 | all | US, UNS | CG |
| IMEX Order 3 | IMEXOrder3 | all | US, UNS | CG |
| Backward Euler | BackwardEuler | all | US, UNS | CG-DG |
| BDF Order 1 | BDFImplicitOrder1 | all | US, UNS | CG-DG |
| BDF Order 2 | BDFImplicitOrder2 | all | US, UNS | CG-DG |
GlobalSysSoln: sets the approach we use to solve the the linear systems of the type
Ax = b appearing in the solution steps, such as the Poisson equation for the pressure in
the splitting-scheme. It can be set as
Possible values are
| System solution | GlobalSysSoln | Parallel |
| Direct Solver (DS) | DirectFull | just quasi-3D |
| DS with Static Condensation | DirectStaticCond | just Quasi-3D |
| DS with Multilevel Static Condensation | DirectMultiLevelStaticCond | just Quasi-3D |
| Iterative Solver (IS) | IterativeFull | just Quasi-3D |
| IS with Static Condensation | IterativeStaticCond | quasi-3D |
| IS with Multilevel Static Condensation | IterativeMultiLevelStaticCond | quasi-3D |
Default values are DirectMultiLevelStaticCond in serial and IterativeStaticCond in
parallel.
SmoothAdvection: activates a stabilization technique which smooths the advection term
using the pressure inverse mass matrix. It can be used just in combination with nodal
expansion basis for efficiency reasons.
SpectralVanishingViscosity: activates a stabilization technique which increases the
viscosity on the highest Fourier frequencies of a Quasi-3D approach.
DEALIASING: activates the 3/2 padding rule on the advection term of a Quasi-3D
simulation.
SubSteppingScheme: activates the sub-stepping routine which uses the mixed CG-DG
projection
SPECTRALHPDEALIASING: activates the spectral/hp dealiasing to stabilize the simulation.
This method is based on the work of Kirby and Sherwin [7].
ShowTimings: activates the blocks timing of the incompressible Navier-Stokes solver.
The CPU time spent in each part of the code will be printed at the end of the
simulation.
The following parameters can be specified in the PARAMETERS section of the session
file:
TimeStep: sets the time-step for the integration in time formula
NumSteps: sets the number of time-steps
Kinvis: sets the cinematic viscosity coefficient formula
Noise: sets the white-noise amplitude we want to add on the velocity initial
conditions
SubStepCFL: sets the CFL safety limit for the sub-stepping algorithm (default
value = 0.5)
SVVCutoffRatio: sets the ratio of Fourier frequency not affected by the SVV
technique (default value = 0.75, i.e. the first 75
SVVDiffCoeff: sets the SVV diffusion coefficient (default value = 0.1)
This force type allows the user to solve the interaction system of an incompressible fluid flowing past a flexible moving bodies [?]. By this forcing function, one can eliminate the difficulty of moving mesh by using body-fitted coordinates, so that an additional acceleration term(i.e., forcing term) is introduced to the momentum equations by the non-inertial transform from the deformed and moving coordinate system to non-deformed and stationary one.
Available options of the motion type for the moving body include free, constrained and forced
vibrations, which can be specified in the SOLVERINFO section. The free type of motion allows
the body to move in both streamwise and crossflow directions, while the constrained type
limits the motion only in the crossflow direction. For the forced type, the vibration profiles of
the body should be specified as a given function or read from input file in MovingBody section.
here an example,
A moving body type boundary condition should be specified in BOUNDARYCONDITIONS for the
velocities on the far field and in-flow boundaries such as,
For the simulation of low mass ratio, there is an option to activate fictitious mass method for
stabilizing explicit coupling between the fluid solver and structural dynamic solver. Here
we need to specify the values of fictitious mass and damping in PARAMETERS, for
example,
A filter calles as MovingBody is encapsulated in this module to evaluate the aerodynamic
forces along the moving body surface. The forces for each computational plane are projected
along the Cartesian axes and the pressure and viscous contributions are computed in each
direction.
The following parameters are supported:
| Option name | Required | Default | Description |
OutputFile | ✗ | session | Prefix of the output filename to which the forces are written. |
Frequency | ✗ | 1 | Number of timesteps after which output is written. |
Boundary | ✓ | - | Boundary surfaces on which the forces are to be evaluated. |
To enable the filter, add the following to the FORCE tag::
During the execution a file named DragLift.frc will be created and the value of the
aerodynamic forces on boundary 0, defined in the GEOMETRY section, will be output every 10
time steps.evaluates the aerodynamic forces along the moving body surface. The forces for
each computational plane are projected along the Cartesian axes and the pressure and viscous
contributions are computed in each direction.