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. runControl

Options

Default

Description

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)

4.2.3. 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.

betaAngle

REQUIRED

The side slip angle in degrees.

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.

4.2.4. 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”. An example: sample

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

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

4.2.5. volumeOutput

Options

Default

Description

outputFormat

paraview

"paraview" or "tecplot"

animationFrequency

-1

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

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

4.2.6. 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

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

4.2.7. 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

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]

4.2.9. 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. Supported for both SpalartAllmaras and kOmegaSST turbulence models, with and without AmplificationFactorTransport transition model enabled

4.2.10. 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

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

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

4.2.11. initialCondition

Options

Default

Description

type

“freestream”

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

4.2.12. 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.

4.2.13. 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 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

4.2.14. 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,= \(\frac{\text{circumferentialForcePerArea}(SI=N/m^2)}{\rho_\infty C^2_\infty}\)

4.2.15. BETDisks (list)

A introduction of blade element theory model in Flow360 is available at BET solver. A case study on 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

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 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 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.

4.2.16. 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.

4.3. 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}