4. Solver Configuration#

The Flow360.json file defines the solver settings used during the CFD solution. Most input quantities in the case configuration file (Flow360.json) are dimensionless. The conventions of nondimensional inputs in Flow360 are explained in detail at the nondimensional inputs knowledge base and the non-dimensionalization in Flow360 tutorial.

4.1. `geometry`#

OPTIONAL

The geometry section defines the geometric reference values. These parameters are used in the calculation of nondimensional loads reported (e.g., $CL$, $CMy$, etc.). Please refer to nondimensional inputs knowledge base and the non-dimensionalization in Flow360 tutorial for further information on how to define these.

Options	Default	Freestream
`refArea`	1.0	[float] The reference area of the geometry
`momentCenter`	[0.0, 0.0, 0.0]	[3-array(float)] The x, y, z moment center of the geometry in grid units
`momentLength`	[1.0, 1.0, 1.0]	[3-array(float)] The x, y, z component-wise moment reference lengths

Example

"geometry" : {
   "refArea" : 45.604,
   "momentCenter" : [0.0, 0.0, 0.0],
   "momentLength" : [3.81, 3.81, 3.81]
}

4.2. `freestream`#

REQUIRED

The freestream section defines the flow conditions at the freestream. Please refer to nondimensional inputs knowledge base and the non-dimensionalization in Flow360 tutorial for further information on how to define these.

Options	Default	Description
`Reynolds`	Either `Reynolds` or `muRef` is REQUIRED	[float] The Reynolds number, = $\frac{\rho_\infty U_{ref} L_{gridUnit}}{\mu_\infty}$. Note that Flow360 differs from traditional calculations with the use of $L_{gridUnit}$.
`muRef`	Either `muRef` or `Reynolds` is REQUIRED	[float] The freestream dynamic viscosity (nondimensional), = $\frac{\mu_\infty}{\rho_\infty C_\infty L_{gridUnit}}$.
`Mach`	REQUIRED	[float] The Mach number, the ratio of freestream velocity to the speed of sound
`MachRef`	`Mach`, REQUIRED if `Mach` == 0.0	[float] The reference Mach number to compute nondimensional quantities, = $U_{ref}/C_\infty$.
`Temperature`	REQUIRED	[float] The freestream temperature in Kelvin. -1 means globally constant viscosity.
`alphaAngle`	REQUIRED	[float] The angle of attack in degrees.
`betaAngle`	REQUIRED	[float] The side slip angle in degrees.
`turbulentViscosityRatio`	DEPENDS	[float] The ratio between the freestream turbulent viscosity and freestream laminar viscosity, used at freestream boundary and to set initial condition. The default depends on the turbulence model and if the transition model is enabled. For `"SpalartAllmaras"` = 0.210438, `"kOmegaSST"` = 0.01, and `"AmplificationFactorTransport"` = $2.794\times10^{-7}$.

Example

"freestream" :
{
   "muRef" : 4.29279e-08,
   "Mach" : 1.46972e-02,
   "MachRef" : 0.70,
   "Temperature" : 288.15,
   "alphaAngle" : -90.0,
   "betaAngle" : 0.0
}

4.3. `boundaries`#

REQUIRED

The boundaries section defines the boundary conditions. Each boundary condition is specified by associating the boundary type for each boundary name in the mesh file, as follows:

"boundary_name" :    
{
	"type" : "boundary_type"
}

The “boundary_name” is the name of each individual patch of the grid and is typically of the form “1” for .ugrid files and “vol-1/wall” for .cgns files. Additionally, for .ugrid meshes an optional parameter “name” can be specified within each boundary dictionary to overwrite the numeric “boundary_name” in results. The “name” option takes a string entry.

Numerous boundary conditions require the specification of additional options, which are outlined in the table below. For a number of boundaries such as NoSlipWall, IsothermalWall and Freestream, mathematical expressions can be used to define the inputs. Please refer to the boundary conditions knowledge base for more information.

Type	Additional Options	Description
`SlipWall`	None	[string] Slip wall condition. Also used for symmetry boundary.
`NoSlipWall`		[string] Sets no-slip wall condition
	`Velocity`, default: [0.0, 0.0, 0.0]	[3-array(float or expression)] Optionally, a tangential velocity can be prescribed on the wall.
`IsothermalWall`		[string] Isothermal wall boundary condition
	`Temperature` (REQUIRED)	[float or expression] Wall temperature specified in Kelvin
	`Velocity`, default: [0.0, 0.0, 0.0]	[3-array(float or expression)] Optionally, a tangential velocity can be prescribed on the wall.
`Freestream`		[string] Freestream condition, set by parameters in freestream. The default values are set based on the alpha and beta angles.
	`Velocity`, default: freestream	[3-array(float or expression)] The default values are set according to the freestream alpha and beta angles. Optionally, an expression for each of the velocity components can be specified.
`SubsonicOutflowPressure`		[string] Subsonic outflow, set through static pressure ratio
	`staticPressureRatio` (REQUIRED)	[float] Static pressure ratio, $\frac{p_{outflow}}{p_{\infty}}$
`SubsonicOutflowMach`		[string] Subsonic outflow, set through Mach number
	`MachNumber` (REQUIRED)	[float] Mach number, $\frac{U_{outflow}}{C_{\infty}}$
`SubsonicInflow`		[string] Subsonic inflow set through total pressure ratio and total temperature ratio for nozzle or tunnel plenum
	`totalPressureRatio` (REQUIRED)	[float] Total pressure ratio, $\frac{p_{t, inflow}}{p_{s, inflow}}$
	`totalTemperatureRatio` (REQUIRED)	[float] Total temperature ratio, $\frac{T_{t, inflow}}{T_{s, inflow}}$
	`rampSteps`	[integer] Number of ramp steps during solution initialization
`MassOutflow`		[string] Mass outflow
	`massFlowRate` (REQUIRED)	[float] Mass flow rate at outlet (non-dimensional), $=\frac{\dot{m}_{outflow}}{{\rho C_{\infty}} L_{gridUnit}^2}$
`MassInflow`		[string] Mass inflow
	`massFlowRate` (REQUIRED)	[float] Mass flow rate at inlet (non-dimensional), $=\frac{\dot{m}_{inflow}}{{\rho C_{\infty}} L_{gridUnit}^2}$
`SlidingInterface`	None	[string] Sliding interface boundaries. Details of each pair (inner/outer patches) must be prescribed separately: slidingInterfaces.
`WallFunction`	None	[string] This boundary type uses wall functions to estimate the velocity field close to the solid boundaries

Example

"boundaries": {
	"boundary_name_A": {
		"type": "SlipWall"
	},
	"boundary_name_B":{
    		"type":"NoSlipWall",
    		"Velocity":["0.0","0.1*x+exp(y)+z^2","cos(0.2*x*pi)+sqrt(z^2+1)"]
	},
	"boundary_name_C": {
		"type": "IsothermalWall",
		"Temperature": 300
	},
	"boundary_name_D": {
        	"type": "Freestream"
	},
	"boundary_name_E": {
		"type": "SubsonicOutflowPressure",
		"staticPressureRatio": 1.0
	},
	"boundary_name_F": {
        	"type": "SubsonicOutflowMach",
        	"MachNumber": 0.2
	},
	"boundary_name_G": {
		"type": "SubsonicInflow",
        	"totalPressureRatio":  1.0,
		"totalTemperatureRatio": 1.0
	},
	"boundary_name_H": {
        	"type": "MassOutflow",
        	"massFlowRate":  0.2
	},
	"boundary_name_I": {
        	"type": "MassInflow",
        	"massFlowRate":  0.2
	},
	"boundary_name_J": {
        	"type": "SlidingInterface"
	},
	"boundary_name_K": {
        	"type": "WallFunction"
	}
}

4.4. `navierStokesSolver`#

OPTIONAL

This section of the configuration file defines the numerical parameters for the Navier-Stokes solver. For more information on setting up these parameters refer to Navier-Stokes solver knowledge base.

Options	Default	Description
`absoluteTolerance`	1.00E-10	[float] Tolerance for the NS residual, below which the solver progresses to the next physical step (unsteady) or completes the simulation (steady)
`relativeTolerance`	0.0	[float] Tolerance to the relative residual, below which the solver goes to the next physical step.
`CFLMultiplier`	1.0	[float] Factor to the CFL value in the timeStepping section
`linearIterations`	30	[int] Number of linear solver iterations
`kappaMUSCL`	-1.0	[float] Kappa for the MUSCL scheme, range from [-1.0, 1.0].
`updateJacobianFrequency`	4	[int] Frequency at which the jacobian is updated
`equationEvalFrequency`	1	[int] Frequency at which to update the NS equation
`maxForceJacUpdatePhysicalSteps`	0	[int] For physical steps less than the input value, the jacobian matrix is updated every pseudo-step overriding the `updateJacobianFrequency` value
`orderOfAccuracy`	2	[int] Order of accuracy in space
`limitVelocity`	FALSE	[boolean] Limiter for velocity
`limitPressureDensity`	FALSE	[boolean] Limiter for pressure and density

Example

"navierStokesSolver" : {
	"absoluteTolerance" : 1e-9,
	"relativeTolerance" : 1e-2,
	"linearIterations" : 35,
	"kappaMUSCL" : -1.0,
	"orderOfAccuracy" : 2,
	"updateJacobianFrequency" : 4,
	"equationEvalFrequency" : 1
    }

4.5. `turbulenceModelSolver`#

OPTIONAL

This section of the configuration file defines the numerical parameters for the turbulence model solver. For more information on setting up these parameters refer to the turbulence model solver knowledge base.

Options	Default	Description
`modelType`	"SpalartAllmaras"	[string] `"SpalartAllmaras"`, `"kOmegaSST"`, or `"None"`
`absoluteTolerance`	1.00E-08	[float] Tolerance for the turbulence model residual, below which the solver progresses to the next physical step (unsteady) or completes the simulation (steady)
`relativeTolerance`	0.0	[float] Tolerance to the relative residual, below which the solver goes to the next physical step.
`linearIterations`	20	[int] Number of linear solver iterations
`updateJacobianFrequency`	4	[int] Frequency at which the jacobian is updated
`equationEvalFrequency`	4	[int] Frequency at which to update the turbulence equation
`reconstructionGradientLimiter`	1.0	[float] The strength of gradient limiter used in reconstruction of solution variables at the faces (specified in the range [0.0, 2.0]). 0.0 corresponds to setting the gradient equal to zero, and 2.0 means no limiting.
`rotationCorrection`	FALSE	[boolean] Rotation correction for the turbulence model. Only supported for `SpalartAllmaras`
`quadraticConstitutiveRelation`	FALSE	[boolean] Quadratic constitutive relation for turbulence shear stress tensor instead of Boussinesq Approximation
`orderOfAccuracy`	2	[int] Order of accuracy in space
`maxForceJacUpdatePhysicalSteps`	0	[int] For physical steps less than the input value, the jacobian matrix is updated every pseudo-step overriding the `updateJacobianFrequency` value
`DDES`	FALSE	[boolean] `"TRUE"` enables Delayed Detached Eddy Simulation. Supported for all turbulence and transition models
`gridSizeForLES`	"maxEdgeLength"	[string] Specifies the length used for the computation of LES length scale. The allowed inputs are `"maxEdgeLength"` and `"meanEdgeLength"`.
`modelConstants`	{}	[dict] A dictionary containing the DDES coefficients in the solver: SpalartAllmaras: `"C_DES"` (= 0.72), `"C_d"` (= 8.0), kOmegaSST: `"C_DES1"` (= 0.78), `"C_DES2"` (= 0.61), `"C_d1"` (= 20.0), `"C_d2"` (= 3.0), (values shown in the parentheses are the default values used in Flow360)

Example

"turbulenceModelSolver" : {
	"modelType" : "SpalartAllmaras",
	"absoluteTolerance" : 1e-8,
	"relativeTolerance" : 1e-2,
	"linearIterations" : 25,
	"DDES" : true,
	"orderOfAccuracy" : 2,
	"updateJacobianFrequency" : 4,
	"equationEvalFrequency" : 1,
	"rotationCorrection" : true,
	"modelConstants" : {
		"C_DES": 0.85,
		"C_d": 8.0
	}
}

4.6. `transitionModelSolver`#

OPTIONAL

This section of the configuration file defines the numerical parameters for the transition model solver. For more information on setting up these parameters refer to the transition model solver knowledge base.

Options	Default	Description
`modelType`	"None"	[string] `"None"` (disabled) or `"AmplificationFactorTransport"` (enabled)
`absoluteTolerance`	1.00E-07	[float] Tolerance for the transition model residual, below which the solver progresses to the next physical step (unsteady) or completes the simulation (steady)
`relativeTolerance`	0.0	[float] Tolerance to the relative residual, below which the solver goes to the next physical step.
`linearIterations`	20	[int] Number of linear solver iterations
`updateJacobianFrequency`	4	[int] Frequency at which the jacobian is updated
`equationEvalFrequency`	4	[int] Frequency at which to update the transition equation
`orderOfAccuracy`	2	[int] Order of accuracy in space
`Ncrit`	8.15	[float] Critical Amplification Factor, Range from [1-11]. Only valid when `turbulenceIntensityPercent` is not specified.
`turbulenceIntensityPercent`	0.1	Turbulence Intensity, Range from [0.03-2.5]. Only valid when `Ncrit` is not specified.
`maxForceJacUpdatePhysicalSteps`	0	[int] For physical steps less than the input value, the jacobian matrix is updated every pseudo-step overriding the `updateJacobianFrequency` value

Example

"transitionModelSolver": {
	"modelType": "AmplificationFactorTransport",
	"absoluteTolerance": 1e-10,
	"linearIterations": 25,
	"orderOfAccuracy": 2,
	"updateJacobianFrequency": 4,
	"equationEvalFrequency": 4,
	"Ncrit": 9
}

4.7. `initialCondition`#

OPTIONAL

This section of the configuration file specifies the initial condition for the simulation.

Options	Default	Description
`type`	"freestream"	[string] `"freestream"` or `"expression"` with expression allowing to specify values for constants (`constants`) and each of the primitive variables (`p`, `rho`, `u`, `v`, `w`) using mathematical expressions.

Example

"initialCondition": {
	"type": "expression",
	"constants": {
		"gamma": "1.4"
	},
	"rho": "1.0",
	"u": "0.0",
	"v": "0.0",
	"w": "0.0",
	"p": "1/gamma"
}

4.8. `timeStepping`#

OPTIONAL

This section of the configuration file defines the numerical parameters for time stepping. Please refer to the time stepping knowledge base for further guidance regarding these parameters.

Options	Additional Options	Default	Description
`physicalSteps`		1	[int] Number of physical steps. "maxPhysicalSteps" is a supported alias for this entry.
`timeStepSize`		"inf"	[string or float] Nondimensional time step size in physical step marching, it is calculated as $\frac{\Delta t_{physical} C_\infty}{L_{gridUnit}}$, where the $\Delta t_{physical}$ is the physical time (in seconds) step size. “inf” means steady simulation.
`maxPseudoSteps`		2000	[int] Maximum pseudo steps within one physical step
`CFL`			CFL settings within each physical step
	`type`	"ramp"	When `"ramp"` is specified, CFL will ramp from `initial` to `final` over `rampSteps` number of pseudo steps. With `"adaptive"` specified, the CFL value is calculated internally based on the quality of solver convergence at each pseudo step.
	`initial`	5	[int] Initial CFL for solving pseudo time step (applicable to `"ramp"`)
	`final`	200	[int] Final CFL for solving pseudo time step (applicable to `"ramp"`)
	`rampSteps`	40	[int] Number of pseudo steps before reaching CFL `final` within 1 physical step (applicable to `"ramp"`)
	`min`	0.1	The minimum allowable value for CFL (applicable to `"adaptive"`)
	`max`	10000	The maximum allowable value for CFL (applicable to `"adaptive"`)
	`maxRelativeChange`	1	The maximum allowable relative change of CFL (%) at each pseudo step (applicable to `"adaptive"`)
	`convergenceLimitingFactor`	0.25	This factor specifies the level of conservativeness when using `adaptive` CFL. Smaller values correspond to a more conservative limitation on the value of CFL. In general, values smaller than 1 are recommended.

Note

The timeStepSize is in solver units (nondimensional), where time-scale is mesh unit divided by freestream speed of sound. So a time of timeStepSize=1 means the time it takes for sound to travel 1 mesh unit at freestream.

Example

"timeStepping": {
	"timeStepSize": "inf",
	"maxPhysicalSteps": 1,
	"maxPseudoSteps": 10000,
	"CFL": {
		"initial": 1,
		"final": 100,
		"rampSteps": 2000
		}
}

4.9. `slidingInterfaces` (list)#

OPTIONAL

This section of the configuration file defines the simulation parameters of a sliding interface. Please refer to the knowledge base on sliding interfaces for further information.

Options	Default	Description
`interfaceName`	REQUIRED	[string] Name of the `slidingInterface` patch
`stationaryPatches`	REQUIRED	[list(string)] A list of static patch names of an interface
`rotatingPatches`	REQUIRED	[list(string)] A list of dynamic patch names of an interface
`thetaRadians`	DEPENDS	[math] Expression for rotation angle (in radians) as a function of time. Required if `isDynamic` = FALSE and none of: `thetaDegrees`, `omegaRadians`, `omegaDegrees` are specified.
`thetaDegrees`	DEPENDS	[math] Expression for rotation angle (in degrees) as a function of time. Required if `isDynamic` = FALSE and none of: `thetaRadians`, `omegaRadians`, `omegaDegrees` are specified.
`omegaRadians`	DEPENDS	[float] Nondimensional rotating speed, radians/nondim-unit-time, = $\frac{\Omega*L_{gridUnit}}{C_\infty}$, where the SI unit of $\Omega$ is rad/s. Required if `isDynamic` = FALSE and none of: `thetaDegrees`, `thetaRadians`, `omegaDegrees` are specified.
`omegaDegrees`	DEPENDS	[float] Nondimensional rotating speed, degrees/nondim-unit-time, = $\text{omegaRadians}*180/PI$. Required if `isDynamic` = FALSE and none of: `thetaDegrees`, `thetaRadians`, `omegaRadians` are specified.
`centerOfRotation`	REQUIRED	[3-array(float)] Origin of rotation
`axisOfRotation`	REQUIRED	[3-array(float)] Axis of Rotation
`volumeName`	REQUIRED	[list, string)] A list of dynamic volume zones related to the above {omega, centerOfRotation, axisOfRotation}
`parentVolumeName`	DEPENDS	[string] Name of the volume zone that the rotating reference frame is contained in, used to compute the acceleration in the nested rotating reference frame. Required when using nested rotating interfaces.
`isDynamic`	FALSE	[boolean] Whether rotation of this interface is dictated by `userDefinedDynamics`

Example

"slidingInterfaces" : [
{
	"stationaryPatches" : ["farField/rotationInterface"],
	"rotatingPatches" : ["innerRotating/rotationInterface"],
	"axisOfRotation" : [0,0,-1],
	"centerOfRotation" : [0,0,0],
	"omega" : 1.84691e-01,
	"volumeName" : ["innerRotating"]
}

4.10. `actuatorDisks` (list)#

OPTIONAL

The actuator disk inputs are defined in this section. Please refer to the actuator disk knowledge base for further information.

Options	Default	Description
`center`	REQUIRED	[3-array(float)] center of the actuator disk
`axisThrust`	REQUIRED	[3-array(float)] direction of thrust, it is a unit vector
`thickness`	REQUIRED	[float] thickness of the actuator disk
`forcePerArea->radius`	REQUIRED	[list(float)] radius of the sampled locations in grid unit
`forcePerArea->thrust`	REQUIRED	[list(float)] force per area in the axial direction, positive means the axial force follows the same direction as `axisThrust`. It is non-dimensional: $\frac{\text{thrustPerArea}(SI=N/m^2)}{\rho_\infty C^2_\infty}$.
`forcePerArea->circumferential`	REQUIRED	[list(float)] force per area in the circumferential direction, positive means the circumferential force follows the same direction as `axisThrust` with the right hand rule. It is non-dimensional: $\frac{\text{circumferentialForcePerArea}(SI=N/m^2)}{\rho_\infty C^2_\infty}$.

Example

"actuatorDisks":
[
 	{
 	"centerOfRotation":[0.0, 0.0, 0.0],    
	"axisThrust":[0.0,0.0,1.0],
	"thickness": 0.01,
        "forcePerArea":[
        	"radius":[0.01, 0.05, 0.1],
		"thrust":[0.001, 0.02, 0],
		"circumferential":[-0.0001, -0.003, 0]
	]
	}
]

4.11. `BETDisks` (list)#

OPTIONAL

In this section, the Blade Element Theory (BET) model inputs are defined. For detailed information on the parameters, please refer to the BET knowledge Base. To generate the sectional polars the BET translators can be used which are outlined here with best-practices for the sectional polars inputs available here. A case study of the XV-15 rotor using the steady BET Disk method is available in Case Studies. Because a transient BET Line simulation is simply a time-accurate version of a steady-state BET Disk simulation, most of the parameters below are applicable to both methods.

Options	Default	Description
`rotationDirectionRule`	"rightHand"	[string] the rule for rotation direction and thrust direction, “rightHand” or “leftHand”.
`centerOfRotation`	REQUIRED	[3-array(float)] center of the Blade Element Theory (BET) disk
`axisOfRotation`	REQUIRED	[3-array(float)] rotational axis of the BET disk, i.e. (+) thrust axis
`numberOfBlades`	REQUIRED	[int] number of blades to model
`radius`	REQUIRED	[float] nondimensional radius of the rotor disk, = $\text{Radius}_\text{dimensional}/L_{gridUnit}$
`omega`	REQUIRED	[float] nondimensional rotating speed, radians/nondim-unit-time, = $\frac{\Omega*L_{gridUnit}}{C_\infty}$, where the SI unit of $\Omega$ is rad/s.
`chordRef`	REQUIRED	[float] nondimensional reference chord used to compute sectional blade loadings
`nLoadingNodes`	REQUIRED	[float] Number of nodes used to compute the sectional thrust and torque coefficients $C_t$ and $C_q$, defined in BET Loading Output
`thickness`	REQUIRED	[float] nondimensional thickness of the BET disk
`bladeLineChord`	0.0	[float] nondimensional chord to use if performing an unsteady BET Line simulation. Default of 0.0 is an indication to run a steady BET Disk simulation.
`initialBladeDirection`	Required if `bladeLineChord` is not = 0	[3-array(float)] Orientation of the first blade in the BET model. Must be specified if performing an unsteady BET Line simulation.
`twists`	REQUIRED	[list(dict)] A list of dictionary entries specifying the twist in degrees as a function of radial location. Entries in the list must already be sorted by radius.
`chords`	REQUIRED	[list(dict)] A list of dictionary entries specifying the blade chord as a function of the radial location. Entries in the list must already be sorted by radius.
`sectionalPolars`	REQUIRED	[list(dict)] A list of dictionaries for every radial location specified in `sectionalRadiuses`. Each dict has two entries, “liftCoeffs” and “dragCoeffs”, both of which have the same data storage format: 3D arrays (implemented as nested lists). The first index of the array corresponds to the `MachNumbers` of the specified polar data. The second index of the array corresponds to the `ReynoldsNumbers` of the polar data. The third index corresponds to the `alphas`. The value specifies the lift or drag coefficient, respectively.
`sectionalRadiuses`	REQUIRED	[list(float)] A list of the radial locations in grid units at which $C_l$ and $C_d$ are specified in `sectionalPolars`
`alphas`	REQUIRED	[list(float)] alphas associated with airfoil polars provided in `sectionalPolars` in degrees
`MachNumbers`	REQUIRED	[list(float)] Mach numbers associated with airfoil polars provided in `sectionalPolars`
`ReynoldsNumbers`	REQUIRED	[list(float)] Reynolds numbers associated with the airfoil polars provided in `sectionalPolars`
`tipGap`	"inf"	[float] Nondimensional distance between blade tip and solid bodies to define a tip loss factor.

Example

"BETDisks": [
        {
            "rotationDirectionRule": "leftHand",
            "centerOfRotation": [0, 0, 0],
            "axisOfRotation": [0, 0, 1],
            "numberOfBlades": 3,
            "radius": 150,
            "omega": 0.0046,
            "chordRef": 14,
            "thickness": 15,
            "nLoadingNodes": 20,
            "MachNumbers": [0],
            "ReynoldsNumbers": [1000000],
            "alphas": [
                -180,
                0,
                180
            ],
            "sectionalRadiuses": [
                13.5,
                120,
                150
            ],
            "twists": [
                {
                    "radius": 13.5,
                    "twist": 40.29936539609504
                },
                {
                    "radius": 76.5,
                    "twist": 16.596477306554306
                },
                {
                    "radius": 150,
                    "twist": 3.97516
                }
            ],
            "chords": [
                {
                    "radius": 13.4999999,
                    "chord": 0
                },
                {
                    "radius": 13.5,
                    "chord": 17.69622361
                },
                {
                    "radius": 150.0348189415042,
                    "chord": 14.004512929656503
                }
            ],
            "sectionalPolars": [
                {
                    "liftCoeffs": [
                        [
                            [
                                8.998801703796744e-12,
                                0.019549999999999998,
                                -8.998801703796744e-12
                            ]
                        ]
                    ],
                    "dragCoeffs": [
                        [
                            [
                                0.03000000000109987,
                                0.007595,
                                0.03000000000109987
                            ]
                        ]
                    ]
                },
                {
                    "liftCoeffs": [
                        [
                            [
                                8.998801703796744e-12,
                                0.18164999999999998,
                                -8.998801703796744e-12
                            ]
                        ]
                    ],
                    "dragCoeffs": [
                        [
                            [
                                0.03000000000109987,
                                0.0062699999999999995,
                                0.03000000000109987
                            ]
                        ]
                    ]
                },
                {
                    "liftCoeffs": [
                        [
                            [
			        -8.998801703796744e-12,
                                0.0589,
                                -8.998801703796744e-12
                            ]
                        ]
                    ],
                    "dragCoeffs": [
                        [
                            [
                                0.03000000000109987,
                                0.004765,
                                0.03000000000109987
                            ]
                        ]
                    ]
                }
            ],

	    "tipGap": "inf"
        }
    ]

4.12. `porousMedia` (list)#

OPTIONAL

This section defines the inputs for the porous media model. For further information please refer to the porous media knowledge base.

Options	Additional Options	Default	Description
`DarcyCoefficient`		REQUIRED	[3-array(float)] Darcy coefficient of the porous media model which determines the scaling of the viscous loss term. The 3 values define the coefficient for each of the 3 axes defined by the reference frame of the volume zone.
`ForchheimerCoefficient`		REQUIRED	[3-array(float)] Forchheimer coefficient of the porous media model which determines the scaling of the inertial loss term
`volumeZone`		REQUIRED	[dict] Dictionary defining the properties of the region of the grid where the porous media model is applied
	`zoneType`	REQUIRED	[string] Type/Shape of volume zone. Possible values: “box”
	`center`	REQUIRED	[3-array(float)] For “zoneType”: “box”, it is the center point of the box
	`axes`	REQUIRED	[[3-array(float)], [3-array(float)]] For “zoneType”: “box”, it is 2 axes which define the x and y directions of the box. Also, used to define the reference frame of the volume zone.
	`lengths`	REQUIRED	[3-array(float)] For “zoneType”: “box”, it is the length of the box in each of the x, y, z directions
	`windowingLengths`	[0.02lengths[0], 0.02lengths[1], 0.02*lengths[2]]	[3-array(float)] For “zoneType”: “box”, it is the total length of the box in x, y, z directions over which a window function is applied on the edges

Example

 "porousMedia": [
    {
        "DarcyCoefficient": [1000000, 0, 0],
        "ForchheimerCoefficient": [1, 0, 0],
        "volumeZone": {
            "zoneType": "box",
            "center": [0, 0, 0],
            "lengths": [0.2, 0.2, 2],
            "axes": [[0, 1, 0], [0, 0, 1]]
        }
    }
]

4.13. `userDefinedDynamics`#

OPTIONAL

This section defines the user defined dynamics inputs. An example of how to use the userDefinedDynamics is available here.

Options	Default	Description
`dynamicsName`	REQUIRED	[string] Name of the dynamics defined by the user
`inputVars`	REQUIRED	[list(string)] List of the inputs to define the user defined dynamics. Allowable inputs are: `"CL"`, `"CD"`, `"bet_NUM_torque"` (NUM is the index of the BET disk starting from 0), `"rotMomentX"`, `"rotMomentY"` and `"rotMomentZ"` (X/Y/Z moments with respect to momentCenter)
`constants`	Empty	[list(dict)] A list of dictionary entries specifying the constants used in the updateLaws and outputLaws
`outputVars`	REQUIRED	[list(string)] Name of the output variables for the defined dynamics and the relation between the output variables and input/state variables. e.g. `"theta[plate]: "state[2];""` Allowable output variables are: `"alphaAngle"`, `"betaAngle"`, `"bet_NUM_omega"` (NUM is the index of the BET disk starting from 0), `"theta[$interfaceName]"`, `"omega[$interfaceName]"` and `"omegaDot[$interfaceName]"` (rotation angle/velocity/acceleration in radius of `interfaceName`, specified in slidingInterfaces. Only one slidingInterface is allowed in one UDD item.)
`stateVarsInitialValue`	Empty	[list(string)] The initial value of state variables are specified here. The entries could be either values (in the form of strings, e.g., `"0.0"`) or name of the variables specified in the configuration file (e.g., `"alphaAngle"`). The list entries correspond to the initial values for `state[0]`, `state[1]`, …, respectively.
`updateLaw`	Empty	[list(string)] List of equations for updating state variables. The list entries correspond to the update laws for `state[0]`, `state[1]`, …, respectively.
`inputBoundaryPatches`	Empty	[list(string)] List of boundary names (if any) related to the input variables

Example

"userDefinedDynamics": [
    {
        "dynamicsName": "alphaController",
        "inputVars": [
            "CL"
        ],
        "constants": {
            "CLTarget": 0.4,
            "Kp": 0.2,
            "Ki": 0.002
        },
        "outputVars": {
            "alphaAngle": "if (pseudoStep > 500) state[0]; else alphaAngle;"
        },
        "stateVarsInitialValue": [
            "alphaAngle",
            "0.0"
        ],
        "updateLaw": [
            "if (pseudoStep > 500) state[0] + Kp * (CLTarget - CL) + Ki * state[1]; else state[0];",
            "if (pseudoStep > 500) state[1] + (CLTarget - CL); else state[1];"
        ],
        "inputBoundaryPatches": [
            "1"
        ]
    }
]

4.14. Output#

This section presents all the configuration file inputs regarding solution output. This includes, the surface and volume solutions, as well as slices, isosurfaces and point monitors. Universal nondimensional variables supported by all types of output are presented below: [note]

Name	Description
`Cp`	Coefficient of pressure. $C_p=(\frac{p-p_\infty}{\frac{1}{2}\rho_\infty{U_{ref}}^2})$
`gradW`	Gradient of primitive solution
`kOmega`	k and omega when using the kOmegaSST model
`Mach`	Mach number
`mut`	Turbulent viscosity
`mutRatio`	Ratio between turbulent viscosity and freestream dynamic viscosity, $\mu_t/{\mu_\infty}$
`nuHat`	Spalart-Almaras variable, nuHat
`primitiveVars`	Outputs rho, u, v, w, p (density, 3 velocities and pressure)
`qcriterion`	Q criterion
`residualNavierStokes`	5 components of the N-S residual
`residualTransition`	Residual for the transition model
`residualTurbulence`	Residual for the turbulence model
`s`	Entropy
`solutionNavierStokes`	Solution for the N-S equation in conservative form
`solutionTransition`	Solution for the transition model
`solutionTurbulence`	Solution for the turbulence model
`T`	Temperature
`vorticity`	Vorticity
`wallDistance`	Wall distance
`lowNumericalDissipationSensor`	Sensor showing where the numericalDissipationFactor has been increased

Additional nondimensional variables supported by volumeOutput and sliceOutput:

Name	Description
`betMetrics`	Outputs BET disk related metrics, including variables such as `VelocityRelative`, `AlphaRadians`, `CfAxial`, `CfCircumferential`, `TipLossFactor`, `LocalSolidityIntegralWeight` for all BETDisks with possible overlapping.
`betMetricsPerDisk`	Same as above but each BETdisk has its own `betMetrics` so overlapping is avoided.
`kOmegaSST_DDES`	Outputs `DDES_fd` (1 in the LES region, and 0 elsewhere), `DDES_lengthRANS` (RANS length scale), and `DDES_lengthLES` (LES length scale)

Additional nondimensional variables supported by surfaceOutput:

Name	Description
`CfVec`	Viscous stress coefficient vector, = $C_{f_{Vec}}[3]=\frac{\tau_{wall}[3]}{\frac{1}{2}\rho_\infty U_{ref}^2}$
`Cf`	Magnitude of `CfVec`
`CfNormal`	Magnitude of `CfVec` normal to the wall
`CfTangent`	Magnitude of `CfVec` tangential to the wall
`heatFlux`	Heat flux
`nodeNormals`	Wall normal direction (may not be a unit vector). Note: This variable does not support time average.
`nodeForcesPerUnitArea`	$\frac{\tau_{wall}[3]-(p-p_\infty)*normal[3]}{\rho_\infty C_\infty^2}$, where the $normal[3]$ is the unit normal vector pointing from solid to fluid
`VelocityRelative`	Velocity in rotating frame
`yPlus`	non-dimensional wall distance, $y^+$
`wallFunctionMetric`	(beta feature) : This metric is a local indicator for quality of the wall model. A value less than 1.25 shows good estimation of wall shear stress. Between 1.25 and 10 is a region of less validity, and values greater than 10 are not reliable for wall shear stress estimation.

4.14.1. `volumeOutput`#

OPTIONAL

Options	Default	Description
`animationFrequency`	-1	[int] Frequency (in number of physical time steps) at which volume output is saved. -1 is at end of simulation.
`animationFrequencyOffset`	0	[int] Offset (in number of physical time steps) at which volume output animation is started. 0 is at beginning of simulation.
`computeTimeAverages`	FALSE	[boolean] Enables computation of time-averaged quantities
`animationFrequencyTimeAverage`	-1	[int] Frequency (in number of physical time steps) at which time averaged volume output is saved. -1 is at end of simulation.
`animationFrequencyTimeAverageOffset`	0	[int] Offset (in number of physical time steps) at which time averaged volume output animation is started. 0 is at beginning of simulation.
`startAverageIntegrationStep`	0	[int] Physical time step to start calculating averaging
`outputFields`	[]	[list(string)] List of output variables. Including universal output variables, and variables specific to volumeOutput.
`outputFormat`	"paraview"	[string] `"paraview"`, `"tecplot"` or `"both"`

Example

"volumeOutput": {
	"outputFormat": "tecplot",
	"animationFrequency": -1,
	"animationFrequencyOffset": 0,
	"animationFrequencyTimeAverage": -1,
	"animationFrequencyTimeAverageOffset": 0,
	"computeTimeAverages": false,
	"startAverageIntegrationStep": 0,
	"outputFields": ["primitiveVars", "betMetrics", "qcriterion"]
}

4.14.2. `surfaceOutput`#

OPTIONAL

Options	Default	Description
`animationFrequency`	-1	[int] Frequency (in number of physical time steps) at which surface output is saved. -1 is at end of simulation.
`animationFrequencyOffset`	0	[int] Offset (in number of physical time steps) at which surface output animation is started. 0 is at beginning of simulation.
`outputFormat`	"paraview"	[string] `"paraview"` or `"tecplot"` or `"both"`
`computeTimeAverages`	FALSE	[boolean] Enables computation of time-averaged quantities
`animationFrequencyTimeAverage`	-1	[int] Frequency (in number of physical time steps) at which time averaged surface output is saved. -1 is at end of simulation.
`animationFrequencyTimeAverageOffset`	0	[int] Offset (in number of physical time steps) at which time averaged surface output animation is started. 0 is at beginning of simulation.
`startAverageIntegrationStep`	0	[int] Physical time step to start calculating averaging
`outputFields`	[]	[list(string)] List of output variables. Including universal output variables and variables specific to surfaceOutput. `outputFields` specified under `surfaceOutput` will be added to all surfaces. See example below.
`surfaces`	{}	[dict] Dictionary of output surfaces. The name of the surface is used as the key. These surface names have to be the patch name in the grid file or the alias name specified in case JSON. See example below.

Example

"surfaceOutput": {
    "animationFrequency": -1,
    "animationFrequencyOffset": 0,
    "animationFrequencyTimeAverage": -1,
    "animationFrequencyTimeAverageOffset": 0,
    "computeTimeAverages": false,
    "outputFormat": "paraview",
    "startAverageIntegrationStep": 0,
    "outputFields": [ "yPlus" ],
    "surfaces": {
        "freestream": {
            "outputFields": [ "Cp", "Mach" ]
            # Will output "Cp", "Mach", "yPlus"
        },
        "symmetry": {
            "outputFields": [ "T", "heatFlux" ]
            # Will output "T", "heatFlux", "yPlus"
        },
        "wing": {
            "outputFields": [ "CfVec" ]
            # Will output "CfVec", "yPlus"
        }
    }
}

4.14.3. `sliceOutput`#

OPTIONAL

Options	Default	Description
`animationFrequency`	-1	[int] Frequency (in number of physical time steps) at which slice output is saved. -1 is at end of simulation.
`animationFrequencyOffset`	0	[int] Offset (in number of physical time steps) at which slice output animation is started. 0 is at beginning of simulation.
`outputFormat`	"paraview"	[string] `"paraview"` or `"tecplot"` or `"both"`
`computeTimeAverages`	FALSE	[boolean] Enables computation of time-averaged quantities
`animationFrequencyTimeAverage`	-1	[int] Frequency (in number of physical time steps) at which time averaged slice output is saved. -1 is at end of simulation.
`animationFrequencyTimeAverageOffset`	0	[int] Offset (in number of physical time steps) at which time averaged slice output animation is started. 0 is at beginning of simulation.
`startAverageIntegrationStep`	0	[int] Physical time step to start calculating averaging
`outputFields`	[]	[list(string)] List of output variables. Including universal output variables and variables specific to sliceOutput. `outputFields` specified under `sliceOutput` will be added to all slices. See example below.
`slices`	{}	[dict] Dictionary of output slices. The name of the slice is used as the key. See example below.
`sliceNormal`	[]	[3-array(float)] Normal direction of the slice (within slices dictionary)
`sliceOrigin`	[]	[3-array(float)] Coordinates of a point on the slice (within slices dictionary)

Example

"sliceOutput": {
    "animationFrequency": -1,
    "animationFrequencyOffset": 0,
    "coarsenIterations": 0,
    "outputFormat": "tecplot",
    "outputFields": [ "Cp" ],
    "slices": {
        "x0": {
            "sliceNormal": [ 1, 0, 0 ],
            "sliceOrigin": [ 0, 0, 0 ],
            "outputFields": [ "Mach" ]
            # Will output "Mach", "Cp"
        },
        "y1": {
            "sliceNormal": [ 0, 1, 0 ],
            "sliceOrigin": [ 2, 1, 0 ],
            "outputFields": [ "T" ]
            # Will output "T", "Cp"
        }
    }
}

4.14.4. `isoSurfaceOutput`#

OPTIONAL

Options	Additional Options	Default	Description
`outputFormat`		"paraview"	[string] `"paraview"`, `"tecplot"` or `"both"`
`isoSurfaces`		{}	[dict] Dictionary of iso-surfaces. The key of the dictionary is the name of the iso-surface file to be written.
	`surfaceField`		[string] Isosurface field variable to be written. One of `p`, `rho`, `Mach`, `qcriterion`, `s`, `T`, `Cp`, `mut`, `nuHat`.
	`surfaceFieldMagnitude`		[float] The iso-value of `surfaceField` to compute
	`outputFields`		[list(string)] List of output variables, see universal output variables
`animationFrequency`		-1	[int] Frequency (in number of physical time steps) at which volume output is saved. -1 is at end of simulation.
`animationFrequencyOffset`		0	[int] Offset (in number of physical time steps) at which volume output animation is started. 0 is at beginning of simulation.

Example

"isoSurfaceOutput": {
    "outputFormat": "tecplot",
    "animationFrequency": 10,
    "isoSurfaces": {
        "q_1e-3": {
            "surfaceField": "qcriterion",
            "surfaceFieldMagnitude": 1e-3,
            "outputFields": [ "Cp", "Mach" ]
        }
    }
},

4.14.5. `monitorOutput`#

OPTIONAL

Options	Additional Options	Default	Description
`monitors`		{}	[dict] Dictionary of monitor groups. Data probed at the monitor points are printed to file every 10 pseudo step and at the end of each physical time step. The key of the dictionary is the name of the monitor group.
	`monitorLocations`		[list(3-array(float))] A list of coordinates of the monitor points belonging to this monitor group
	`outputFields`		[list(string)] List of output fields which will be added to all monitors within the monitor group, see universal output variables

Note

Please increase the precision of the input coordinates when probing near the grid boundaries to ensure that the probing location is within the mesh.

Example

"monitorOutput": {
    "monitors": {
        "Group1": {
            "monitorLocations": [
                [ 0.12, 0.34, 0.262 ],
                [ 3.124e-1, 0.01, 0.03 ]
            ],
            "outputFields": [ "primitiveVars", "vorticity", "T", "s", "Cp", "mut" ]
        }
    }
}

note: Since release-23.1.1.0, previous syntax to specify output variables is being deprecated and not all variables are supported. Users are encouraged to use the new syntax as described in this documentation.

Options	Default	Description
`Reynolds`	Either `Reynolds` or `muRef` is REQUIRED	[float] The Reynolds number, = \(\frac{\rho_\infty U_{ref} L_{gridUnit}}{\mu_\infty}\). Note that Flow360 differs from traditional calculations with the use of \(L_{gridUnit}\).
`muRef`	Either `muRef` or `Reynolds` is REQUIRED	[float] The freestream dynamic viscosity (nondimensional), = \(\frac{\mu_\infty}{\rho_\infty C_\infty L_{gridUnit}}\).
`Mach`	REQUIRED	[float] The Mach number, the ratio of freestream velocity to the speed of sound
`MachRef`	`Mach`, REQUIRED if `Mach` == 0.0	[float] The reference Mach number to compute nondimensional quantities, = \(U_{ref}/C_\infty\).
`Temperature`	REQUIRED	[float] The freestream temperature in Kelvin. -1 means globally constant viscosity.
`alphaAngle`	REQUIRED	[float] The angle of attack in degrees.
`betaAngle`	REQUIRED	[float] The side slip angle in degrees.
`turbulentViscosityRatio`	DEPENDS	[float] The ratio between the freestream turbulent viscosity and freestream laminar viscosity, used at freestream boundary and to set initial condition. The default depends on the turbulence model and if the transition model is enabled. For `"SpalartAllmaras"` = 0.210438, `"kOmegaSST"` = 0.01, and `"AmplificationFactorTransport"` = \(2.794\times10^{-7}\).

Name	Description
`Cp`	Coefficient of pressure. \(C_p=(\frac{p-p_\infty}{\frac{1}{2}\rho_\infty{U_{ref}}^2})\)
`gradW`	Gradient of primitive solution
`kOmega`	k and omega when using the kOmegaSST model
`Mach`	Mach number
`mut`	Turbulent viscosity
`mutRatio`	Ratio between turbulent viscosity and freestream dynamic viscosity, \(\mu_t/{\mu_\infty}\)
`nuHat`	Spalart-Almaras variable, nuHat
`primitiveVars`	Outputs rho, u, v, w, p (density, 3 velocities and pressure)
`qcriterion`	Q criterion
`residualNavierStokes`	5 components of the N-S residual
`residualTransition`	Residual for the transition model
`residualTurbulence`	Residual for the turbulence model
`s`	Entropy
`solutionNavierStokes`	Solution for the N-S equation in conservative form
`solutionTransition`	Solution for the transition model
`solutionTurbulence`	Solution for the turbulence model
`T`	Temperature
`vorticity`	Vorticity
`wallDistance`	Wall distance
`lowNumericalDissipationSensor`	Sensor showing where the numericalDissipationFactor has been increased

Name	Description
`CfVec`	Viscous stress coefficient vector, = \(C_{f_{Vec}}[3]=\frac{\tau_{wall}[3]}{\frac{1}{2}\rho_\infty U_{ref}^2}\)
`Cf`	Magnitude of `CfVec`
`CfNormal`	Magnitude of `CfVec` normal to the wall
`CfTangent`	Magnitude of `CfVec` tangential to the wall
`heatFlux`	Heat flux
`nodeNormals`	Wall normal direction (may not be a unit vector). Note: This variable does not support time average.
`nodeForcesPerUnitArea`	\(\frac{\tau_{wall}[3]-(p-p_\infty)*normal[3]}{\rho_\infty C_\infty^2}\), where the \(normal[3]\) is the unit normal vector pointing from solid to fluid
`VelocityRelative`	Velocity in rotating frame
`yPlus`	non-dimensional wall distance, \(y^+\)
`wallFunctionMetric`	(beta feature) : This metric is a local indicator for quality of the wall model. A value less than 1.25 shows good estimation of wall shear stress. Between 1.25 and 10 is a region of less validity, and values greater than 10 are not reliable for wall shear stress estimation.

Solver Configuration

Contents

4. Solver Configuration#

4.1. geometry#

4.2. freestream#

4.3. boundaries#

4.4. navierStokesSolver#

4.5. turbulenceModelSolver#

4.6. transitionModelSolver#

4.7. initialCondition#

4.8. timeStepping#

4.9. slidingInterfaces (list)#

4.10. actuatorDisks (list)#

4.11. BETDisks (list)#

4.12. porousMedia (list)#

4.13. userDefinedDynamics#

4.14. Output#

4.14.1. volumeOutput#

4.14.2. surfaceOutput#

4.14.3. sliceOutput#

4.14.4. isoSurfaceOutput#

4.14.5. monitorOutput#

4.1. `geometry`#

4.2. `freestream`#

4.3. `boundaries`#

4.4. `navierStokesSolver`#

4.5. `turbulenceModelSolver`#

4.6. `transitionModelSolver`#

4.7. `initialCondition`#

4.8. `timeStepping`#

4.9. `slidingInterfaces` (list)#

4.10. `actuatorDisks` (list)#

4.11. `BETDisks` (list)#

4.12. `porousMedia` (list)#

4.13. `userDefinedDynamics`#

4.14.1. `volumeOutput`#

4.14.2. `surfaceOutput`#

4.14.3. `sliceOutput`#

4.14.4. `isoSurfaceOutput`#

4.14.5. `monitorOutput`#