4. Solver Configuration#

The current Mesh processor and Solver input configuration parameters for Flow360 are:

4.1. Flow360Mesh.json#

Type	Options	Default	Description
boundaries	noSlipWalls	[]	list of names of boundary patches, e.g. [2,3,7] (for .ugrid), [“blk-1/wall1”,”blk-2/wall2”] (for .cgns)
slidingInterfaces		[]	list of pairs of sliding interfaces
	stationaryPatches	[]	list of names of stationary boundary patches, e.g. [“stationaryField/interface”]
	rotatingPatches	[]	list of names of dynamic boundary patches, e.g. [“rotatingField/interface”]
	axisOfRotation	[]	axis of rotation, e.g. [0,0,-1]
	centerOfRotation	[]	center of rotation, e.g. [0,0,0]

Warning

“slidingInterfaces” can be only used for multi-block meshes.

4.2. Flow360.json#

Most input quantities in case configuration file Flow360.json is dimensionless. The convention of non-dimentionalization in Flow360 can be found at Non-dimensionalization. Some commonly used variables in the table below:

$L_{gridUnit}$ (SI unit = $m$): physical length represented by unit length in the given mesh file, e.g. if your grid is in feet, $L_{gridUnit}=1 \text{ feet}=0.3048 \text{ meter}$; if your grid is in millimeter, $L_{gridUnit}=1 \text{ millimeter}=0.001 \text{ meter}$.
$C_\infty$ (SI unit = $m/s$): speed of sound of freestream
$\rho_\infty$ (SI unit = $kg/m^3$): density of freestream
$\mu_\infty$ (SI unit = $N \cdot s/m^2$): dynamic viscosity of freestream
$p_\infty$ (SI unit = $N/m^2$): static pressure of freestream
$U_\text{ref} \triangleq \text{MachRef}\times C_\infty$ (SI unit = $m/s$): reference velocity

4.2.1. geometry#

Options	Default	Description
refArea	1	The reference area of the geometry
momentCenter	[0.0, 0.0, 0.0]	The x, y, z moment center of the geometry in grid units
momentLength	[1.0, 1.0, 1.0]	The x, y, z moment reference lengths

4.2.2. freestream#

Options	Default	Description
Reynolds	Not required if muRef exists	The Reynolds number (non-dimenstional) in our solver, = $\frac{\rho_\infty U_{ref} L_{gridUnit}}{\mu_\infty}$. For example, for a mesh with phyiscal length 1.5m represented by 1500 grid units (i.e. mesh is in mm), the $L_{gridUnit}$ in the numerator is 0.001m.
muRef	Not required if Reynolds exists	The refererence dynamic viscosity (non-dimenstional) in our solver, = $\frac{\mu_\infty}{\rho_\infty C_\infty L_{gridUnit}}$
Mach	REQUIRED	The Mach number, the ratio of freestream speed to the speed of sound.
MachRef	Required if Mach == 0	The reference Mach number to compute nondimensional quantities, e.g. CL, CD, CFx, CFy, CFz, CMz, CMy, CMz, etc…, = $U_{ref}/C_\infty$. Its default value is “freestream”->”Mach”.
Temperature	REQUIRED	The reference temperature in Kelvin. -1 means globally constant viscosity.
alphaAngle	REQUIRED	The angle of attack in degrees, see: Eq.(4.2.1).
betaAngle	REQUIRED	The side slip angle in degrees, see: Eq.(4.2.1).
turbulentViscosityRatio	DEPENDS	The ratio between the freestream turbulent viscosity and freestream laminar viscosity. This value is used by the turbulence models to determine the reference values for solution variables for freestream boundary conditions and also to set the initial condition. For SpalartAllmaras turbulence model, the default value is $0.210438$ if transition is not used and $2.794\times10^{-7}$ if transition model is used. For kOmegaSST, the default value is $0.01$.

According to Flow360’s definitions of the angle of attack $\alpha$ and the sideslip angle $\beta$, as given in the above table, with respect to the grid coordinates, the following values of velocity components are imposed at a “Freestream” farfield boundary as defined in the next subsection.

(4.2.1)#\[\begin{split} U^*_{\infty} &= M_{\infty} \cdot cos(\beta) \cdot cos(\alpha) \\ V^*_{\infty} &= - M_{\infty} \cdot sin(\beta) \\ W^*_{\infty} &= M_{\infty} \cdot cos(\beta) \cdot sin(\alpha)\end{split}\]

Where, the velocity components are non-dimensionalized by the freestream speed of sound $C_{\infty}$. Also, the effects of these two angles are intrinsically taken into account by the solver in the computed $C_l$ and $C_d$ values, etc.

4.2.3. boundaries#

Type	Format	Description
SlipWall	"boundary_name" : { "type" : "SlipWall" }	Slip wall condition. Also used for symmetry.
NoSlipWall	"boundary_name" : { "type" : "NoSlipWall", "Velocity": (default: [0, 0, 0]) [ float or "expression", float or "expression", float or "expression"] }	Sets no-slip wall condition. Optionally, a tangential velocity can be prescribed on the wall using the keyword “Velocity”. An example: sample
IsothermalWall	"boundary_name" : { "type" : "IsothermalWall", "Temperature": float or "expression" (REQUIRED), "Velocity": (default: [0, 0, 0]) [ float or "expression", float or "expression", float or "expression"] }	Isothermal wall boundary condition. “Temperature” is specified in Kelvin. Optionally a tangential velocity can be presribed on the wall using the keyword “Velocity”.
Freestream	"boundary_name" : { "type" : "Freestream", "Velocity": (default: freestream) [ float or "expression", float or "expression", float or "expression"] }	External freestream condition. Optionally, an expression for each of the velocity components can be specified using the keyword “Velocity”.
SubsonicOutflowPressure	"boundary_name" : { "type" : "SubsonicOutflowPressure", "staticPressureRatio" : float }	Subsonic outflow, enforced through static pressure ratio.
SubsonicOutflowMach	"boundary_name" : { "type" : "SubsonicOutflowMach", "MachNumber" : float }	Static pressure outflow boundary condition set via a specified subsonic Mach number.
SubsonicInflow	"boundary_name" : { "type" : "SubsonicInflow", "totalPressureRatio" : float, "totalTemperatureRatio" : float, "rampSteps" : Integer }	Subsonic inflow (enforced via total pressure ratio and total temperature ratio) for nozzle or tunnel plenum.
MassOutflow	"boundary_name" : { "type" : "MassOutflow", "massFlowRate" : float }	Specification of massflow out of the control volume.
MassInflow	"boundary_name" : { "type" : "MassInflow", "massFlowRate" : float }	Specification of massflow into the control volume.
SlidingInterface	"boundary_name" : { "type" : "SlidingInterface" }	Sliding interface condition. Details of each sliding interface need to be prescribed in a seperate section: slidingInterfaces

Note

Note: “expression” is an expression with “x”, “y”, “z” as independent variables. An example of NoSlipWall boundary with prescribed velocity is NoSlipWall with velocity.

4.2.4. volumeOutput#

Options	Default	Description
outputFormat	paraview	"paraview" or "tecplot" or "both"
animationFrequency	-1	Frequency (in number of physical time steps) at which volume output is saved. -1 is at end of simulation
animationFrequencyOffset	0	Offset (in number of physical time steps) at which volume output animation is started. 0 is at beginning of simulation
animationFrequencyTimeAverage	-1	Frequency (in number of physical time steps) at which time averaged volume output is saved. -1 is at end of simulation
animationFrequencyTimeAverageOffset	0	Offset (in number of physical time steps) at which time averaged volume output animation is started. 0 is at beginning of simulation
startAverageIntegrationStep	0	Physical time step to start averaging forces/moments, only if computeTimeAverages is True. Fields that can be averaged: primitiveVars, vorticity, T, s, Cp, mut, Mach, qcriterion
computeTimeAverages	FALSE	Whether or not to compute time-averaged quantities
primitiveVars	TRUE	Outputs rho, u, v, w, p
vorticity	FALSE	Vorticity
residualNavierStokes	FALSE	5 components of the N-S residual
residualTurbulence	FALSE	Residual for the turbulence model
residualTransition	FALSE	Residual for the transition model
solutionTurbulence	FALSE	Solution for the turbulence model
solutionTransition	FALSE	Solution for the transition model
T	FALSE	Temperature
s	FALSE	Entropy
Cp	TRUE	Coefficient of pressure. $C_p=(\frac{p-p_\infty}{\frac{1}{2}\rho_\infty{U_{ref}}^2})$.
mut	TRUE	Turbulent viscosity
nuHat	TRUE	nuHat
kOmega	FALSE	k and omega when using kOmegaSST model
mutRatio	FALSE	$\mu_t/{\mu_\infty}$
Mach	TRUE	Mach number
VelocityRelative	FALSE	relative velocity respect to the rotating frame, see the explaination.
qcriterion	FALSE	Q criterion
gradW	FALSE	Gradient of W
wallDistance	FALSE	wall distance
betMetrics	FALSE	8 quantities related to BET solvers: velocityX, velocityY and velocityZ in rotating reference frame, alpha angle, Cf in axial direction, Cf in circumferential direction, tip loss factor, local solidity multiplied by integration weight
betMetricsPerDisk	FALSE	similar to `betMetrics` but the metrics of different BET disks are dumped seperately.

4.2.5. surfaceOutput#

Options	Default	Description
outputFormat	paraview	"paraview" or "tecplot"
animationFrequency	-1	Frequency (in number of physical time steps) at which surface output is saved. -1 is at end of simulation
animationFrequencyOffset	0	Offset (in number of physical time steps) at which surface output animation is started. 0 is at beginning of simulation
animationFrequencyTimeAverage	-1	Frequency (in number of physical time steps) at which time averaged surface output is saved. -1 is at end of simulation
animationFrequencyTimeAverageOffset	0	Offset (in number of physical time steps) at which time averaged surface output animation is started. 0 is at beginning of simulation
primitiveVars	TRUE	Outputs rho, u, v, w, p
vorticity	FALSE	Vorticity
residualNavierStokes	FALSE	5 components of the N-S residual
residualTurbulence	FALSE	Residual for the turbulence model
residualTransition	FALSE	Residual for the transition model
solutionTurbulence	FALSE	Solution for the turbulence model
solutionTransition	FALSE	Solution for the transition model
T	FALSE	Temperature
s	FALSE	Entropy
Cp	TRUE	Coefficient of pressure. $C_p=(\frac{p-p_\infty}{\frac{1}{2}\rho_\infty{U_{ref}}^2})$.
mut	TRUE	Turbulent viscosity
nuHat	TRUE	nuHat
kOmega	FALSE	k and omega when using kOmegaSST model
mutRatio	FALSE	$\mu_t/{\mu_\infty}$
Mach	TRUE	Mach number
VelocityRelative	FALSE	velocity in rotating frame
qcriterion	FALSE	Q criterion
gradW	FALSE	Gradient of W
wallDistance	FALSE	wall distance
Cf	FALSE	Skin friction coefficient
heatFlux	FALSE	Heat Flux
CfVec	FALSE	Viscous stress coefficient vector. For example, $C_{f_{Vec}}[3]=\frac{\tau_{wall}[3]}{\frac{1}{2}\rho_\infty U_{ref}^2}$. The $\tau_{wall}$ is the vector of viscous stress on the wall.
yPlus	FALSE	y+
nodeForcesPerUnitArea	FALSE	$nodeForcesPerUnitArea=\frac{\tau_{wall}[3]-(p-p_\infty)*normal[3]}{\rho_\infty C_\infty^2}$, where the $normal[3]$ is the unit normal vector pointing from solid to fluid.

4.2.6. sliceOutput#

Options	Default	Description
outputFormat	paraview	"paraview" or "tecplot"
animationFrequency	-1	Frequency (in number of physical time steps) at which slice output is saved. -1 is at end of simulation
animationFrequencyOffset	0	Offset (in number of physical time steps) at which slice output animation is started. 0 is at beginning of simulation
slices	[]	List of slices to save after the solver has finished
sliceName		string
sliceNormal		[x, y, z]
sliceOrigin		[x, y, z]
primitiveVars	TRUE	Outputs rho, u, v, w, p
vorticity	FALSE	Vorticity
residualNavierStokes	FALSE	5 components of the N-S residual
residualTurbulence	FALSE	Residual for the turbulence model
residualTransition	FALSE	Residual for the transition model
solutionTurbulence	FALSE	Solution for the turbulence model
solutionTransition	FALSE	Solution for the transition model
T	FALSE	Temperature
s	FALSE	Entropy
Cp	TRUE	Coefficient of pressure. $C_p=(\frac{p-p_\infty}{\frac{1}{2}\rho_\infty{U_{ref}}^2})$.
mut	TRUE	Turbulent viscosity
nuHat	TRUE	nuHat
kOmega	FALSE	k and omega when using kOmegaSST model
mutRatio	FALSE	$\mu_t/{\mu_\infty}$
Mach	TRUE	Mach number
VelocityRelative	FALSE	velocity in rotating frame
qcriterion	FALSE	Q criterion
gradW	FALSE	Gradient of W
wallDistance	FALSE	wall distance
betMetrics	FALSE	8 quantities related to BET solvers: velocityX, velocityY and velocityZ in rotating reference frame, alpha angle, Cf in axial direction, Cf in circumferential direction, tip loss factor, local solidity multiplied by integration weight
betMetricsPerDisk	FALSE	similar to `betMetrics` but the metrics of different BET disks are dumped seperately.

An example sliceOutput configuration is shown below.

"sliceOutput": {
  "outputFormat": "tecplot",
  "animationFrequency": 10,
  "primitiveVars": true,
  "Cp": true,
  "Mach": true,
  "slices": [
    {
      "sliceNormal": [ 0, 1, 0 ],
      "sliceOrigin": [ 0, 0, 0 ],
      "sliceName": "ExampleSlice1"
    }
  ]
}

4.2.7. monitorOutput#

Options	Default	Description
monitors	{}	Dictionary of monitor groups. Data probed at the monitor points are printed to file every 10 pseudo step and at the endy of each physical time step. The key of the dictionary is the name of the monitor group. The value of the dictionary is another dictionary, containing the following keys/values: 1. `monitorLocations`: A list/array of coordinates of the monitor points belonging to this monitor group. 2. `outputFields`: A list of variables to be probed. Any field available in `volumeOutput`.

An example monitor configuration is shown below. In the example a monitor group with name Group1 is created which contains two monitor points with coordinates (0.12, 0.34, 0.262) and (0.3124, 0.01, 0.03) respectively.

Note: Please increase precision of the input coordinates when probing near the boundaries of volume grid (for example noSlipWalls) as the actual point may be out of grid volume when precision is insufficient.

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

4.2.8. isoSurfaceOutput#

Options	Default	Description
outputFormat	paraview	"paraview" or "tecplot" or "both"
isoSurfaces	{}	Dictionary of iso-surfaces to write. The key of the dictionary is the name of the iso-surface file to be written. The value of the dictionary is another dictionary, containing the following keys/values: 1. `surfaceField`, any scalar field computable in `volumeOutput`. 2. `surfaceFieldMagnitude`, the iso-value of `surfaceField` to compute. 3. `outputFields`, any field available in `volumeOutput` which is to be evaluated on the iso-surface.
animationFrequency	-1	Frequency (in number of physical time steps) at which volume output is saved. -1 is at end of simulation
animationFrequencyOffset	0	Offset (in number of physical time steps) at which volume output animation is started. 0 is at beginning of simulation

An example isoSurface configuration is shown below, in which the pressure, p, and Mach number are evaluated on an iso-surface of qcriterion with an iso-surface magnitude of 1e-3.

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

4.2.9. navierStokesSolver#

Options	Default	Description
absoluteTolerance	1.00E-10	Tolerance for the NS residual, below which the solver goes to the next physical step
relativeTolerance	0	tolerance to the ratio of residual of current pseudoStep to the initial residual, below which the solver goes to the next physical step
CFLMultiplier	1	factor to the CFL definitions defined in “timeStepping” section
linearIterations	30	Number of linear solver iterations
kappaMUSCL	-1	Kappa for the MUSCL scheme, range from [-1, 1], with 1 being unstable. The default value of -1 leads to a 2nd order upwind scheme and is the most stable. A value of 0.33 leads to a blended upwind/central scheme and is recommended for low subsonic flows leading to reduced dissipation
updateJacobianFrequency	4	Frequency at which the jacobian is updated.
equationEvalFrequency	1	Frequency at which to update the NS equation in loosely-coupled simulations
maxForceJacUpdatePhysicalSteps	0	when which physical steps, the jacobian matrix is updated every pseudo step
orderOfAccuracy	2	order of accuracy in space
limitVelocity	FALSE	limiter for velocity
limitPressureDensity	FALSE	limiter for pressure and density

4.2.10. turbulenceModelSolver#

Options	Default	Description
modelType	SpalartAllmaras	Turbulence model type can be: “SpalartAllmaras” or “kOmegaSST”
absoluteTolerance	1.00E-08	Tolerance for the turbulence model residual, below which the solver goes to the next physical step
relativeTolerance	0	Tolerance to the ratio of residual of current pseudoStep to the initial residual, below which the solver goes to the next physical step
linearIterations	20	Number of linear iterations for the turbulence moddel linear system
updateJacobianFrequency	4	Frequency at which to update the Jacobian
equationEvalFrequency	4	Frequency at which to evaluate the turbulence equation in loosely-coupled simulations
reconstructionGradientLimiter	1.0	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	Rotation correction for the turbulence model. Only support for SpalartAllmaras
quadraticConstitutiveRelation	FALSE	Use quadratic constitutive relation for turbulence shear stress tensor instead of Boussinesq Approximation
orderOfAccuracy	2	Order of accuracy in space
maxForceJacUpdatePhysicalSteps	0	When which physical steps, the jacobian matrix is updated every pseudo step
DDES	FALSE	“true” enables Delayed Detached Eddy Simulation. Supported for both SpalartAllmaras and kOmegaSST turbulence models, with and without AmplificationFactorTransport transition model enabled

4.2.11. transitionModelSolver#

The laminar to turbulence transition model supported by Flow360 is the 2019b version of the Amplification Factor Transport Model created by James Coder, University of Tennessee. This models adds two additional equations to the flow solver in order to solve for the amplification factor and intermittency flow quantities. More details about the model can be found at: https://turbmodels.larc.nasa.gov/aft_transition_3eqn.html. Below are a list of configuration parameters for the transition model. Either Ncrit or turbulenceIntensityPercent can be used to tune the location of transition from laminar to turbulent flow.

Options	Default	Description
modelType	None	Transition model type can either be: “None” (disabled) or “AmplificationFactorTransport” (enabled)
absoluteTolerance	1.00E-07	Tolerance for the transition model residual, below which the solver goes to the next physical step
relativeTolerance	0	Tolerance to the ratio of residual of current pseudoStep to the initial residual
linearIterations	20	Number of linear iterations for the transition model linear system
updateJacobianFrequency	4	Frequency at which to update the Jacobian
equationEvalFrequency	4	Frequency at which to evaluate the turbulence equation in loosely-coupled simulations
orderOfAccuracy	2	Order of accuracy in space
turbulenceIntensityPercent	0.1	Used to compute Ncrit parameter for AFT transition model. Range: 0.03 - 2.5. Higher values result in earlier transition
Ncrit	8.15	Scalar parameter for transition model. Range: 1-11. Higher values delays onset of laminar-turbulent transition. Only one of “Ncrit” or turbulenceIntensityPercent” can be specified in this section
maxForceJacUpdatePhysicalSteps	0	When which physical steps, the jacobian matrix is updated every pseudo step

4.2.12. initialCondition#

Options	Default	Description
type	“freestream”	Use the flow conditions defined in freestream section to set initial condition. Could be “freestream” or an “expression”

4.2.13. timeStepping#

Options	Default	Description
physicalSteps	1	Number of physical steps. "maxPhysicalSteps" is a supported alias for this entry
timeStepSize	"inf"	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 solver.
maxPseudoSteps	2000	Maximum pseudo steps within one physical step
CFL->initial	5	Initial CFL for solving pseudo time step
CFL->final	200	Final CFL for solving pseudo time step
CFL->rampSteps	40	Number of steps before reaching the final CFL within 1 physical step

Note

The timeStepSize is in solver units (non-dimensional), 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.

4.2.14. slidingInterfaces (list)#

Options	Default	Description
interfaceName	Empty	name of slidingInterface
stationaryPatches	Empty	a list of static patch names of an interface
rotatingPatches	Empty	a list of dynamic patch names of an interface
thetaRadians	Empty	expression for rotation angle (in radians) as a function of time
thetaDegrees	Empty	expression for rotation angle (in degrees) as a function of time
omegaRadians	Empty	non-dimensional rotating speed, radians/nondim-unit-time, = $\Omega*L_{gridUnit}/C_\infty$, where the SI unit of $\Omega$ is rad/s.
omegaDegrees	Empty	non-dimensional rotating speed, degrees/nondim-unit-time, = $\text{omegaRadians}*180/PI$
centerOfRotation	Empty	a 3D array, representing the origin of rotation, e.g. [0,0,0]
axisOfRotation	Empty	a 3D array, representing the rotation axis, e.g. [0,0,1]
volumeName	Empty	a list of dynamic volume zones related to the above {omega, centerOfRotation, axisOfRotation}
parentVolumeName	Empty	name of the volume zone that the rotating reference frame is contained in, used to compute the acceleration in the nested rotating reference frame
isDynamic	FALSE	whether rotation of this interface is dictated by userDefinedDynamics

4.2.15. actuatorDisks (list)#

Options	Default	Description
center	Empty	center of the actuator disk
axisThrust	Empty	direction of the thrust (acted on rotors), it is an unit vector
thickness	Empty	thickness of the actuator disk
forcePerArea->radius (list)	Empty	radius of the sampled locations in grid unit
forcePerArea->thrust (list)	Empty	force (acted on rotors) per area along the axisThrust, positive means the axial force follows the same direction of “axisThrust”. It is non-dimensional,= $\frac{\text{thrustPerArea}(SI=N/m^2)}{\rho_\infty C^2_\infty}$.
forcePerArea->circumferential (list)	Empty	force (acted on fluid) per area in circumferential direction,positive means the circumferential force follows the same direction of “axisThrust” based on right hand rule. It is non-dimensional,= $\frac{\text{circumferentialForcePerArea}(SI=N/m^2)}{\rho_\infty C^2_\infty}$. Two examples with positive and negative values are shown in negative and positive respectively.

4.2.16. BETDisks (list)#

An introduction of blade element theory model in Flow360 is available at BET solver. A case study of the XV-15 rotor based on steady blade element disk model is available at BET case study.

Options	Default	Description
rotationDirectionRule	rightHand	[string] the rule for rotation direction and thrust direction, “rightHand” or “leftHand”. A detailed explanation and some examples are shown at BET input.
centerOfRotation	Empty	[3-array] center of the Blade Element Theory (BET) disk
axisOfRotation	Empty	[3-array] rotational axis of the BET disk, i.e. (+) thrust axis
numberOfBlades	Empty	[int] number of blades to model
radius	Empty	[float] non-dimensional radius of the rotor disk, = $\text{Radius}_\text{dimensional}/L_{gridUnit}$
omega	Empty	[float] non-dimensional rotating speed, radians/nondim-unit-time, = $\Omega*L_{gridUnit}/C_\infty$, where the SI unit of $\Omega$ is rad/s. An example can be found at the case study XV15 BET
chordRef	Empty	[float] non-dimensional reference chord used to compute sectional blade loadings.
nLoadingNodes	Empty	[float] Number of nodes used to compute the sectional thrust and torque coefficients $C_t$ and $C_q$, defined in BET Loading Output. Recommended value is 20.
thickness	Empty	[float] non-dimensional thickness of the BET disk. Should be less than the thickness of the refined region of the disk mesh.
bladeLineChord	0.0	[float] non-dimensional chord to use if performing an unsteady blade-line (as opposed to steady blade-disk) simulation. Recomended value is 1-2x the physical mean aerodynamic chord (MAC) of the blade for blade line analysis. Default of 0.0 is an indication to run blade-disk analysis instead of blade-line.
initialBladeDirection	Empty	[3-array]. Orientation of the first blade in the blade-line model. Must be specified if performing blade-line analysis.
twists	Empty	[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. Example entry in the list would be {“radius” : 5.2, “twist” : 32.5}.
chords	Empty	[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. Example entry in the list would be {“radius” : 5.2, “chord” : 12.0}.
sectionalPolars	Empty	[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	Empty	[list(float)] A list of the radial locations in grid units at which $C_l$ and $C_d$ are specified in sectionalPolars
alphas	Empty	[list(float)] alphas associated with airfoil polars provided in sectionalPolars in degrees.
MachNumbers	Empty	[list(float)] Mach numbers associated with airfoil polars provided in sectionalPolars.
ReynoldsNumbers	Empty	[list(float)] Reynolds numbers associated with the airfoil polars provided in sectionalPolars.
tipGap	inf	[float] non-dimensional distance between blade tip and multiple peripheral instances, e.g. duct, shroud, cowling, nacelle, etc. The peripheral structures must be effective at reducing blade tip vortices. This parameter affects the tip loss effect. Being close to a fuselage or to another blade does not affect this parameter, because they won’t effectively reduce tip loss. tipGap=0 means there is no tip loss. It is $\infty$ (default) for open propellers. An example with finite tipGap would be a ducted fan.

4.2.17. porousMedia (list)#

The porous media model supported by Flow360 is the Darcy-Forchheimer model which has two coefficients: Darcy coefficient for viscous losses and Forchheimer coefficient for inertial losses. The model acts by adding a sink term to the momentum equations. More details about the model can be found at https://openfoamwiki.net/index.php/DarcyForchheimer. Below are a list of configuration parameters for the porous media model.

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

4.2.18. userDefinedDynamics#

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)] Name of the inputs for the 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 intital 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.

4.3. Examples of Flow360.json#

a NoSlipWall boundary with a prescribed velocity

"boundary_name":{
    "type":"NoSlipWall",
    "Velocity":["0","0.1*x+exp(y)+z^2","cos(0.2*x*pi)+sqrt(z^2+1)"]
}

an actuator disk modelling of left-hand-rotation rotor in quiescent flow:

"actuatorDisks":[
    {
        ...
        "axisThrust":[0,0,1],
        "forcePerArea":[
           "radius":[0.01, 0.05, 0.1],
           "thrust":[0.001, 0.02, 0],
           "circumferential":[-0.0001, -0.003, 0]
        ]
    }
]

an actuator disk modelling of right-hand-rotation rotor in quiescent flow:

"actuatorDisks":[
    {
        ...
        "axisThrust":[0,0,-1],
        "forcePerArea":[
           "radius":[0.01, 0.05, 0.1],
           "thrust":[0.001, 0.02, 0],
           "circumferential":[0.0001, 0.003, 0]
        ]
    }
]

Solver Configuration

Contents

4. Solver Configuration#

4.1. Flow360Mesh.json#

4.2. Flow360.json#

4.2.1. geometry#

4.2.2. freestream#

4.2.3. boundaries#

4.2.4. volumeOutput#

4.2.5. surfaceOutput#

4.2.6. sliceOutput#

4.2.7. monitorOutput#

4.2.8. isoSurfaceOutput#

4.2.9. navierStokesSolver#

4.2.10. turbulenceModelSolver#

4.2.11. transitionModelSolver#

4.2.12. initialCondition#

4.2.13. timeStepping#

4.2.14. slidingInterfaces (list)#

4.2.15. actuatorDisks (list)#

4.2.16. BETDisks (list)#

4.2.17. porousMedia (list)#

4.2.18. userDefinedDynamics#

4.3. Examples of Flow360.json#