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-dimensional input in Flow360 can be found at Non-dimensional input. 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

WallFunction

(beta feature)

 
"boundary_name" :
{
 "type" : "WallFunction"
}

This boundary type uses wall functions to estimate the velocity field close to the solid boundaries.

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. Output#

Universal non-dimensional variables suppoprted by all types of output : [note]

Name

Description

Cp

Coefficient of pressure. \(C_p=(\frac{p-p_\infty}{\frac{1}{2}\rho_\infty{U_{ref}}^2})\).

gradW

Gradient of W

kOmega

k and omega when using kOmegaSST model

Mach

Mach number

mut

Turbulent viscosity

mutRatio

\(\mu_t/{\mu_\infty}\)

nuHat

nuHat

primitiveVars

Outputs rho, u, v, w, p

qcriterion

Q criterion

residualComponentsSA

Residual for the turbulence model

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

Additional non-dimensional variables suppoprted by volumeOutput and sliceOutput:

Name

Description

betMetrics

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 non-dimensional variables suppoprted by surfaceOutput:

Name

Description

CfVec

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.

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

\(y^+\).

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.

4.2.4.1. volumeOutput#

Options

Default

Description

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.

computeTimeAverages

FALSE

Whether or not to compute time-averaged quantities.

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 calculating averaging.

outputFields

[]

List of output variables. Including universal output variables, and variables specific to volumeOutput.

outputFormat

paraview

"paraview" or "tecplot" or "both".

4.2.4.2. surfaceOutput#

Options

Default

Description

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.

outputFormat

paraview

"paraview" or "tecplot"

computeTimeAverages

FALSE

Whether or not to compute time-averaged quantities.

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.

startAverageIntegrationStep

0

Physical time step to start calculating averaging.

outputFields

[]

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

{}

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.

An example surfaceOutput configuration is shown below.

 1"surfaceOutput": {
 2    "animationFrequency": -1,
 3    "animationFrequencyOffset": 0,
 4    "animationFrequencyTimeAverage": -1,
 5    "animationFrequencyTimeAverageOffset": 0,
 6    "computeTimeAverages": false,
 7    "outputFormat": "paraview",
 8    "startAverageIntegrationStep": 0,
 9    "outputFields": [ "yPlus" ],
10    "surfaces": {
11        "freestream": {
12            "outputFields": [ "Cp", "Mach" ]
13            # Will output "Cp", "Mach", "yPlus"
14        },
15        "symmetry": {
16            "outputFields": [ "T", "heatFlux" ]
17            # Will output "T", "heatFlux", "yPlus"
18        },
19        "wing": {
20            "outputFields": [ "CfVec" ]
21            # Will output "CfVec", "yPlus"
22        }
23    }
24}

4.2.4.3. sliceOutput#

Options

Default

Description

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.

outputFormat

paraview

"paraview" or "tecplot"

computeTimeAverages

FALSE

Whether or not to compute time-averaged quantities.

animationFrequencyTimeAverage

-1

Frequency (in number of physical time steps) at which time averaged slice output is saved. -1 is at end of simulation.

animationFrequencyTimeAverageOffset

0

Offset (in number of physical time steps) at which time averaged slice output animation is started. 0 is at beginning of simulation.

startAverageIntegrationStep

0

Physical time step to start calculating averaging.

outputFields

[]

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

{}

Dictionary of output slices. The name of the slice is used as the key. See example below.

sliceNormal

[]

Normal direction of the slice.

sliceOrigin

[]

Cooridinates of a point on the slice.

An example sliceOutput configuration is shown below.

 1"sliceOutput": {
 2    "animationFrequency": -1,
 3    "animationFrequencyOffset": 0,
 4    "coarsenIterations": 0,
 5    "outputFormat": "tecplot",
 6    "outputFields": [ "Cp" ],
 7    "slices": {
 8        "x0": {
 9            "sliceNormal": [ 1, 0, 0 ],
10            "sliceOrigin": [ 0, 0, 0 ],
11            "outputFields": [ "Mach" ]
12            # Will output "Mach", "Cp"
13        },
14        "y1": {
15            "sliceNormal": [ 0, 1, 0 ],
16            "sliceOrigin": [ 2, 1, 0 ],
17            "outputFields": [ "T" ]
18            # Will output "T", "Cp"
19        }
20    }
21}

4.2.4.4. 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: See universal output variables. outputFields specified under monitorOutput will be added to all monitors

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.

 1"monitorOutput": {
 2    "monitors": {
 3        "Group1": {
 4            "monitorLocations": [
 5                [ 0.12, 0.34, 0.262 ],
 6                [ 3.124e-1, 0.01, 0.03 ]
 7            ],
 8            "outputFields": [ "primitiveVars", "vorticity", "T", "s", "Cp", "mut" ]
 9        }
10    }
11}

4.2.4.5. 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, one of p, rho, Mach, qcriterion, s, T, Cp, mut, nuHat.
2. surfaceFieldMagnitude, the iso-value of surfaceField to compute.
3. outputFields, See universal output variables.

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.

 1"isoSurfaceOutput": {
 2    "outputFormat": "tecplot",
 3    "animationFrequency": 10,
 4    "isoSurfaces": {
 5        "q_1e-3": {
 6            "surfaceField": "qcriterion",
 7            "surfaceFieldMagnitude": 1e-3,
 8            "outputFields": [ "p", "Mach" ]
 9        }
10    }
11},

4.2.6. 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 relative residual, below which the solver goes to the next physical step. Relative residual is defined as the ratio of the current pseudoStep’s residual to the maximum residual present in the first 10 pseudoSteps within the current physicalStep. NOTE: relativeTolerance is ignored in steady simulations and only absoluteTolerance is used as the convergence criterion

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

gridSizeForLES

“maxEdgeLength”

Specifes the length used for the computation of LES length scale. The allowed inputs are "maxEdgeLength" (default) and "meanEdgeLength"

modelConstants

{}
Here, user can change the default values used for 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)
An example with kOmegaSST mode would be:
"modelConstants" : {
      "C_DES1": 0.85,
      "C_d1": 8.0
}

4.2.7. 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 relative residual, below which the solver goes to the next physical step. Relative residual is defined as the ratio of the current pseudoStep’s residual to the maximum residual present in the first 10 pseudoSteps within the current physicalStep. NOTE: relativeTolerance is ignored in steady simulations and only absoluteTolerance is used as the convergence criterion

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

4.2.8. initialCondition#

Options

Default

Description

type

“freestream”

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

4.2.9. 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.

4.2.10. 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

4.2.11. 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.

4.2.12. 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 Disk and BET Line.

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.

4.2.13. 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

[0.02*lengths[0], 0.02*lengths[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.

4.2.14. 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#

  1. a NoSlipWall boundary with a prescribed velocity

1"boundary_name":{
2    "type":"NoSlipWall",
3    "Velocity":["0","0.1*x+exp(y)+z^2","cos(0.2*x*pi)+sqrt(z^2+1)"]
4}

  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]
        ]
    }
]
../_images/leftHand_thrust_z+1.svg

  1. 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]
        ]
    }
]
../_images/rightHand_thrust_z-1.svg
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.