5. API Reference

5.1. Installing Flow360 Client

The Flow360 client can be installed (and updated) from PyPI. Make sure you have the Python setuptools. If not, sudo apt-get install python3-setuptools.

pip3 install flow360client
pip3 install --upgrade flow360client

5.2. Sign in with you Account and Password

An account can be created at https://client.flexcompute.com/app/signup.

python3
>>> import flow360client
enter your email registered at flexcompute:********@gmail.com
Password: ***********
Do you want to keep logged in on this machine ([Y]es / [N]o)Y

Once you have installed the Flow360 client and signed into it, you can run your first case using the ONERA M6 Wing tutorial in the Quick Start section of this document.

5.3. Configuration Parameters

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

5.3.1. 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]

5.3.2. Flow360.json

Some commonly used symbols in Flow360.json:

\(L_{gridUnit}\) (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

\(U_\text{ref}\) (SI unit = \(m/s\))

reference velocity

5.3.2.1. 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

5.3.2.2. runControl

Options	Default	Description
restart	FALSE	the solutions are initialized from restarting files or not (no need to set by users)
startAlphaControlPseudoStep	-1	pseudo step at which to start targetCL control. -1 is no trim control. (steady only)
targetCL	-1	The desired trim CL to achieve (assocated with startAlphaControlPseudoStep)

5.3.2.3. freestream

Options	Default	Description
Reynolds	Not required if muRef exists	Non-dimensional Reynolds number based on grid unit, = \(\frac{\rho_\infty U_\infty L_{gridUnit}}{\mu_\infty}\). 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 the mu, CL/CD, coefficients, 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
betaAngle	REQUIRED	The side slip angle in degrees
turbulentViscosity	1.0	The multiplicative factor for the freestream turbulent viscosity for the turbulence model
turbulenceIntensity	0.0	The turbulence intensity in the freestream in percent. If greater than zero, activates the transition model. A value of 0.5 in this field means turbulenceIntensity=0.5 %.

5.3.2.4. boundaries

Type	Format	Description
SlipWall	"boundary_name" : { "type" : "SlipWall" }	Slip wall condition. Also used for symmetry.
NoSlipWall	"boundary_name" : { "type" : "NoSlipWall", "Velocity": [ float or "expression" (default: 0), float or "expression" (default: 0), float or "expression" (default: 0)] }	Sets no-slip wall condition. Optionally, a tangential velocity can be prescribed on the wall using the keyword “Velocity”.
IsothermalWall	"boundary_name" : { "type" : "IsothermalWall", "Temperature": float or "expression" (REQUIRED), "Velocity": [ float or "expression" (default: 0), float or "expression" (default: 0), float or "expression" (default: 0)] }	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": [ float or "expression" (default: freestream), float or "expression" (default: freestream), float or "expression" (default: freestream)] }	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.

Note: “expression” is an expression with “x”, “y”, “z” as independent variables.

5.3.2.5. volumeOutput

Options	Default	Description
outputFormat	paraview	“paraview” or “tecplot”
animationFrequency	-1	Frequency at which volume output is saved. -1 is at end of simulation
startAverageIntegrationStep	0	Sub-iteration or time-step to start averaging forces/moments
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	velocity in rotating frame
qcriterion	FALSE	Q criterion
gradW	FALSE	Gradient of W
wallDistance	FALSE	wall distance
wallDistanceDir	FALSE	wall distance direction
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

5.3.2.6. surfaceOutput

Options	Default	Description
outputFormat	paraview	“paraview” or “tecplot”
animationFrequency	-1	Frequency at which surface output is saved. -1 is at end of simulation
primitiveVars	FALSE	rho, u, v, w, p
Cp	FALSE	Coefficient of pressure
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+
wallDistance	FALSE	Wall Distance
Mach	FALSE	Mach number
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.
residualSA	FALSE	Spalart-Allmaras residual magnitude

5.3.2.7. sliceOutput

Options	Default	Description
outputFormat	paraview	“paraview” or “tecplot”
animationFrequency	-1	Frequency at which slice output is saved. -1 is at end of simulation
primitiveVars	TRUE	Outputs rho, u, v, w, p
vorticity	FALSE	Vorticity
T	FALSE	Temperature
s	FALSE	Entropy
Cp	FALSE	Coefficient of pressure
mut	FALSE	Turbulent viscosity
mutRatio	FALSE	\(mut/mu_\infty\)
Mach	TRUE	Mach number
gradW	FALSE	gradient of W
slices	[]	List of slices to save after the solver has finished
sliceName		string
sliceNormal		[x, y, z]
sliceOrigin		[x, y, z]

5.3.2.8. navierStokesSolver

Options	Default	Description
absoluteTolerance	1.00E-10	Tolerance for the NS residual, below which the solver goes to the next physical step
relativeTolerance	1.00E-02	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.
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
extraDissipation	0	add more dissipation to the NS solver
limitVelocity	FALSE	limiter for velocity
limitPressureDensity	FALSE	limiter for pressure and density
viscousWaveSpeedScale	0	Scales the wave speed according to a viscous flux. 0.0 is no speed correction, with larger values providing a larger viscous wave speed correction.

5.3.2.9. 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	1.00E-02	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
kappaMUSCL	-1	Kappa for the muscle scheme, range from [-1, 1] with 1 being unstable.
rotationCorrection	FALSE	Rotation correction for the turbulence model. Only support for SpalartAllmaras
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. Only supported for SpalartAllmaras model

5.3.2.10. transitionModelSolver

Options	Default	Description
modelType	AmplificationFactorTransport	Transition model type can be: “AmplificationFactorTransport”
absoluteTolerance	1.00E-07	Tolerance for the transition model residual, below which the solver goes to the next physical step
relativeTolerance	1.00E-02	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
maxForceJacUpdatePhysicalSteps	0	When which physical steps, the jacobian matrix is updated every pseudo step

5.3.2.11. initialCondition

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

5.3.2.12. timeStepping

Options	Default	Description
maxPhysicalSteps	1	Maximum physical steps
timeStepSize	“inf”	Nondimensional time step size in physical step marching, it is calculated as \(\frac{\Delta t_{physical} C_\infty} {L_{gridUnit}}\). \(\Delta t_{physical}\) is the physical time 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

5.3.2.13. slidingInterfaces (list)

Options	Default	Description
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 names related to the above {omega, centerOfRotation, axisOfRotation}

5.3.2.14. actuatorDisks (list)

Options	Default	Description
center	Empty	center of the actuator disk
axisThrust	Empty	direction of the thrust, 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 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 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,= \(\frac{\text{circumferentialForcePerArea}(SI=N/m^2)}{\rho_\infty C^2_\infty}\)

5.3.2.15. BETDisks (list)

Option	Default	Description
centerOfRotation	Empty	[3-array] center of the Blade Element Theory (BET) disk
axisOfRotation	Empty	[3-array] rotational axis of the BET disk
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.
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 coeffcient \(C_t\) and \(C_q\), defined in BET Loading Output. Recomended 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 indicates 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 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.