Overview

First, the flow solver has to be turned on, and the grid solver off by selecting following boolean values in the properties file:

gridGenerator = false

flowSolver = true

When starting an FV simulation, the user has to choose the following solver property :

solvertype.0 = "MAIA_FINITE_VOLUME"

Next, an appropriate solver method for the time integration has to be chosen. For the finite volume solver the Runge-Kutta method can be chosen as:

solverMethod = "MAIA_RUNGE_KUTTA"

The dimensionality of the simulation can be chosen by setting the value of nDim to 2 or 3.

Choosing the set of equations

The set of equations to be solved is implemented in the FV-solver through the sysEqn class. It can be set in the properties.toml file through the fvSystemEquations property.

Following options exist:

Navier-Stokes (FV_SYSEQN_NS): Standard Navier-Stokes equations, non-dimensional, closed with the ideal gas equation. Constant heat capacities are assumed.
RANS (FV_SYSEQN_RANS): Reynolds-Averaged-Navier-Stokes equations. Similar to the aforementioned NS-equations, but require of additional modelling and equations to close the system.
Detailed Chemistry (FV_SYSEQN_DETCHEM): Dimensional Navier-Stokes equations expanded with additional transport and reaction equations. Non-constant heat capacities.
EE-Gas (FV_SYSEQN_EEGAS): ...

Property	Type	Description
gamma	Float	Ratio of specific heats. Default value of 1.4 for fluid simulations concerning air.

Infinity values

Infinity values for the primitive variables are defined through the dimensionless numbers and are needed in the B.C. definitions. Depending of the problem at hand, a different amount of them will be necessary, but the Reynolds number and Mach number will always have to be defined. In order to have a proper understanding about the non-dimensionalization procedure used in the code, see (mmNonDim).

Special attention when using the detailed chemistry equation set has to be taken. Since this equation system has not been non-dimensionalized the infinity values are specified directly and not through the dimensionless numbers.

Property	Type	Description
Re	Float	Reynolds number
Ma	Float	Mach number
angle	Array of Floats	Angle of the incoming infinity velocity. For example a value [90, 0] would equal to an infinity velocity defined in Y+ direction.

Initial Conditions

Initial conditions describe the starting values of all your variables at the first timestep of your simulation. The closer they are to reality, the faster the convergence and stability of your simulation will be. The initial conditions are implemented in the code, and tend to describe the distribution for a given specific problem. It is assigned by a numerical value to the property initialCondition in fvcartesiansolverxd.cpp.

If the case to simulate has not been performed to date, it may be necessary to specify a new initial condition in the code.

Numerical settings

Surface-value reconstruction

The surface value reconstruction is given by the property surfaceValueReconstruction. As the name implies, this property controls what type of algorithm is used to reconstruct the primitive variables at the surfaces from the values at the cell centroids.

Depending on your problem at hand, for example for supersonic simulations where shock-capturing is required, it may be important to switch from the default "HOCD". In this situation, a limited approach may be beneficial to avoid spurious oscillations across the shock.

Property	Type	Description
surfaceValueReconstruction	String	Selects the reconstruction method. Possible values are: HOCD: unlimited high-order surface data reconstruction. HOCD_LIMITED: limited high-order surface data reconstruction. LOCD: unlimited low-order (pressure)/high-order surface data reconstruction.

RK-Method

A five-step Runge-Kutta Scheme of second-order accuracy is commonly applied to the temporal integration of the conservative variables. The number of coefficients of the RK method have to be equal to the number of steps specified. An example of the properties is given in the following, where the chosen RK order is set to two, a total of five iteration steps is conducted and the coefficients are chosen in such a way to maximize numerical stability.

noRKSteps = 5
rkalpha-step = [0.25, 0.16666666666, 0.375, 0.5, 1.0]
rungeKuttaOrder = 2

Property	Type	Description
noRKSteps	Int	Number of steps in the Runge-Kutta time-stepping method.
rkalpha-step		Coefficients of the Runge-Kutta time-stepping method. Possible values are: Floating point numbers (as many as Runge-Kutta steps).
rungeKuttaOrder	Int	Defines the runge kutta method (order). Possible values are: 2 - second order 3 - third order

Time step size and CFL number

The chosen time step has a great influence on the numerical stability of the employed methods. It is chosen by assigning a non-negative, non-zero value to the CFL-number cfl (Courant–Friedrichs–Lewy number). This number governs the necessary condition for convergence when solving partial differential equations with explicit time integration schemes. Usual values in the theoretical sense range from 0 to 1 for a stable computation, however depending on the method used to compute the time step from the CFL number bigger numbers than 1 can also produce stable solutions. It is encouraged to try different values and find the highest value that still produces stable solutions, since this will speed up the convergence of the simulation while not negatively affecting the accuracy of the simulation if performed properly.

The exact method used to compute the time step from the given CFL number can be defined by the property timeStepMethod by assigning an integer value to it. For exact details about how each of the methods works, refer to the code found in fvcartesiansolverxd.cpp.

Property	Type	Description
cfl	Float	CFL number
timeStepComputationInterval	Int	Specifies on which interval the time-step will be recomputed. -1 -> default (when restart): never - read from restart file, requires m_restart == true. 0 -> default (when no restart): once at the beginning 1 -> every time-step N -> every N time-steps
timeStepMethod	Int	Time step computation method. 1 -> computes the time step based on the CFL condition of the Euler equations \( \Delta t = \min \left[ C * \dfrac{\Delta x}{\|u_i\| + a} \right], \quad i = 0..d \) 6 -> time step method based on the cell length of the GCells. For level set only. 1000 -> time step method for enthalpy solver 17511 -> use flame based time steps but write the time step of case 1 in the solution files 100 -> Same as 1, but uses the infinity values and fulfills additionally the viscous cfl number

Numerical diffusion

Numerical diffusion can be fine tuned through the property globalUpwindCoefficient, which sets the upwind coefficient for the pressure splitting

This property is normally used with values close to zero (around 0.01), meaning vanishing numerical diffusion and could lead to non-physical, high-frequent pressure oscillations for certain simulations. A case by case study may be necessary.

Viscous flux computation

The numerical method for the computation of the viscous flux can impact numerical stability of the problem. By default, the five point discretization scheme is used.

Property	Type	Description
viscousFluxScheme	String	Scheme for the calculation of the viscous flux Possible values are: THREE_POINT FIVE_POINT FIVE_POINT_STABILIZED

Memory settings

These settings control the memory allocation of the solver for each computational rank. These values can heavily impact code performance if not chosen appropiately. Trial and error may be required for fine-tuning memory allocation for a given case. A detailed explanation on these settings can be found in (@ugGeneralApplication).

Boundary condition

Boundary conditions govern the behaviour of the solution in the boundary regions. A distinction is made in the solver between:

regular boundary conditions : are applied directly at the boundary and computed with the help of external ghost cells.
cut-off boundary conditions : are applied to surfaces that have been previously "cut-off" the grid.

Common boundary conditions used in CFD, such as inlet, outlet, wall and symetry are present in the code. More exotic B.C., such as the Navier-Stokes Characteristic Boundary Condition (NSCBC) can also be used. This type of B.C. allows outgoing pressure waves to pass through the boundary without reflecting them, and are useful for acoustic applications or pressure-sensitive simulations.

A list of the available boundary conditions is generated here: List of FV Boundary Conditions.

The regular boundary conditions are specified in the geometry file by assigning a numerical value (corresponding to the dessired B.C.) to the desired surface. Cut-off B.C. are specified in the properties file (after cut-off treatment) by the following properties:

Cut-Off treatment

Property	Type	Description
cutOff	Boolean	Flag to switch the cut-off treatment
cutOffMethod	String	Method to define the cut-off. Accepted values are: B: Box (keeps everything inside the box) iB: inverse Box (keeps everything ouside the box) P: Plane C: Cylinder
cutOffCoordinates	Array of Floats	Coordinates to define the cut-off positions. Definition depends on the chosen method.

Cut-Off B.C.

Property	Type	Description
createBoundaryAtCutoff	Boolean	Switch to turn the creation of cut-off B.C. on and off
cutOffDirections	Array of Ints	Defines the cartesian direction of the cut-off surfaces away from the domain. This means in which direction the cut-off can be found. Following convention is held: 0: X- 1: X+ 2: Y- 3: Y+ 4: Z- 5: Z+
cutOffBndryIds	Array of Ints	The cut-off B.C. associated with the directions given in `cutOffDirections`.

Sponge layer

A sponge layer is an artificial modification of the RHS of the discretized conservation equation, such that the difference between the current value of a variable and a given value is dampened. There exists the possibility to define sponge layers around existing, already defined B.C. or to define them on the general boundaries of the domain. Depending on the used sponge layer type, one or more of the variables are dampened.

For setting the boundaries on the general boundaries of the domain, a spongeLayerThickness > 0 has to be defined. The spongeLayerThickness is given as a factor of \(L_{ref}\) and controls the thickness of the sponge layer in which the sponge layer forcing is applied. The spongeLayerType gives the type of sponge chosen for the forcing. A comprehensive list of sponge layer types can be found here.

The property sigmaSponge controls the amplitude of the forcing term. Bigger numbers should lead a stronger dampening of the difference. The spongeFactor is an array and consists of a total of 2 * nDim floating point numbers. It controls on which domain boundaries a sponge layer is active. Each entry corresponds to the respecive direction (0: -x, 1: +x, 2: -y, ...) and controls the specific sponge layer thickness on this domain boundary. If a factor is zero, no sponge layer is generated in this direction.

spongeLayerThickness = 1.0  
spongeLayerType = 91900  
sigmaSponge = 15.0  
spongeFactor = [0.5, 0.5, 2.0, 1.0, 0.5, 0.5] 

RANS

A RANS simulation is started by setting

fvSystemEquations = FV_SYSEQN_RANS

RANS-specific settings:

Property	Type	Description
ransMethod	String	Chooses the RANS equations to be solved.
fullRANS	Boolean	Triggers a full RANS simulation.
noRansEquations	Integer

A mathematical description of the turbulence modeling is given here. Currently, the Spalart-Allmaras turbulence model is implemented. To use it set ransMethod = "RANS_SA" and noRansEquations = 1.

Adaptive mesh refinement

If you want to learn how to enable AMR for you simulation, read here. The list of all available sensors for the FV solver can be found here.