Flow Solution Parameters dialog box (Multiphysics)

Modeling Object
Name	Sets the name for the modeling object.
Label	Sets a unique numeric identifier for the modeling object.
Properties
Description	Lets you enter a description for the modeling object.
Convergence Control
Steady State - Relaxation Time Step	Specifies the steady state time step.PhysicalDefines the time step as a fraction of a physical time scale for the model. You can define the physical time step as a constant value or expression, or varying with each iteration based on a linear interpolation of the table data. You set a physical time step for the model in the Time Step box.LocalDefines the time step based on local velocity and the element length scale at each node in the domain. The software multiplies the local reference time step by the factor that you specify in the Time Step Factor box.
Convergence Criteria	Specifies the convergence criteria for the simulation.Max ResidualsDetermines the convergence criteria for each transport equation on the maximum residual over all nodes.RMS ResidualsDetermines the convergence criteria for each transport equation on the RMS residual computed over all nodes.
Maximum Residuals	Sets the maximum value for either the maximum residual or the RMS residual for each transport equation. The flow solver stops iterating when the maximum residual at any node in the domain, or the RMS residual over all nodes in the domain reaches the specified maximum value for each transport equation.
Global Flow Imbalance Fraction Option	Adds the flow imbalance fraction convergence criterion to the flow solver. The flow solver continues iterating until the mass and momentum imbalances are within the fraction you specify in the Global Flow Imbalance Fraction box. Enter a value between 0 and 1.
Global Heat Imbalance Fraction Option	Adds the heat imbalance fraction convergence criterion to the flow solver. The flow solver continues iterating until the heat flow imbalance is within the fraction you specify in the Global Heat Imbalance Fraction box. Enter a value between 0 and 1.
Steady State - Iteration Limit	Sets the maximum number of iterations the flow solver performs, for a steady state solution. When the solver reaches this limit, it stops the simulation, even if the solution has not converged.
Transient - Iteration Limit	Sets the maximum number of iterations the flow solver performs at each time step, for a transient solution. When the solver reaches this limit, it proceeds to the next time step even if the current time step has not converged.
Freeze Flow Field at Convergence for Steady State
Freeze Flow Field at Convergence	Stops solving the flow field equations one by one when they reach the specified convergence criteria.When you clear this option, the flow solver continues solving the flow field equations until they all reach the specified convergence criteria.
Restart Flow Field	Appears when Freeze Flow Field at Convergence is selected.Restarts the resolution of flow field equations when the temperature change between the current iteration and the iteration when the flow solve froze the flow field is greater than the value you specify in the Restart Temperature Change box.
Freeze Flow Field for Transient
Freeze Flow Field Based on Solution Evolution	Stops solving the mass and momentum equations, when they reach the specified convergence criteria. The flow solver continues to iterate the energy equation coupled with the thermal solver.The flow solver freezes the flow field when one of the following criteria is met:The difference between the normalized velocity of two consecutive time steps is less than the value you specify in the Maximum Normalized Velocity Change box.The difference between the normalized pressure of two consecutive time steps is less than the value you specify in the Maximum Normalized Pressure Change box.When you clear this option, the flow solver continues solving the mass, momentum, and energy equations until all three reach convergence.
Restart Flow Field	Appears when Freeze Flow Field Based on Solution Evolution is selected.Restarts the solution of mass and momentum equations when the temperature change between the current timestep and the timestep when the flow solver froze the flow field is greater than the value you specify in the Restart Temperature Change box.
Freeze Flow Field at Specified Times	Stops solving the mass and momentum equations at the times you specify in the Freeze Flow Field Specified Times text box.
Reactivate Flow Calculation at Specified Times	Appears when Freeze Flow Field at Specified Times is selected.Reactivates the resolution of mass and momentum equations at the times you specify in the Reactivate Flow Calculation Specified Times text box.
Relaxation Factors
For all relaxation factors, enter a value between 0 and 1.
Global	Sets the relaxation factor for the momentum and energy equations assigned to the boundary node to improve the convergence of the iterative linear solver. This relaxation factor also controls the default values for the Mass and Fan Curves (Recirculation Fans) boxes.
Mass	Sets the relaxation factor for the mass equation at each integration point to control the convergence of the iterative solution. This value overrides the value you specify in the Global box.
Fluids	Sets the relaxation factor for the main diagonal terms of the assembled momentum equations to improve the convergence of the iterative linear solver.
Turbulence	Sets the relaxation factor for the additional turbulence equations.
Screen Resistance	Sets the relaxation factor the software uses when you define a head loss coefficient on for a Screen simulation object.
Fan Curves (I/O/Internal Fans)	Sets the relaxation factor the software uses when you define a Fan Curve for the Inlet Flow, Outlet Flow, and Internal Fan type of a Flow Boundary Condition simulation object.
Fan Curves (Recirculation Fans)	Sets the relaxation factor the software uses when you define a Fan Curve for a Recirculation Loop type of a Flow Boundary Condition simulation object. This value overrides the value you specify in the Global box at integration points on the recirculation fan curves.
Advection Schemes
Momentum, Energy, Two-Equation Turbulence Model, and Humidity, Tracer Fluids and Homogeneous Mixtures	Specify the advection scheme used for the mass and momentum equations, the energy equation, the two-equation turbulence models, or the scalar equations. The advection scheme specifies the numerical discretization method of the flow solver.First-orderSpecifies the first-order Upwind Differencing Scheme (UDS) as the numerical discretization method. Use this advection scheme for a robust solution that converges quickly. This option provides accurate results only if the flow is aligned with the mesh.**Second-order (QUICK)**Specifies the second-order Quadratic Upwind Interpolation for Convective Kinematics (QUICK) scheme as the numerical discretization method. Use this advection scheme for the highest precision solution. This scheme has the lowest stability.**Second-order (SOU)**Specifies the Second-Order Upwind (SOU) scheme as the numerical discretization method. Use this advection scheme for more precise solution than the First-order advection scheme. It also provides better stability then the Second-order (QUICK) advection scheme.**Second-order (CDS)**Specifies a Central Differencing Scheme (CDS) as the numerical discretization method. This method is optimal for low speed flows with a Peclet number that is less than 10.CDS provides a more accurate representation of the advective fluxes on a given mesh than UDS. CDS also eliminates the severe smearing of the solution field that occurs when UDS is used on meshes that are not well-aligned with the local flow direction.The CDS scheme is computationally less time-consuming than the QUICK and SOU second-order schemes.**Second-order (HI-RES)**Specifies the second-order high resolution scheme (HI-RES) as the numerical discretization method. Unlike other second-order schemes, you are not required to define a limiter for the high resolution scheme because this scheme:Uses a special numerical technique to calculate the limiter at each node.Adapts the discretization to avoid any unwanted unboundedness.The high resolution scheme is often more robust than other second-order schemes. In the high resolution scheme, the limiter is formulated to avoid the switching instability that affects other limiters. Using the high resolution scheme, you can obtain converged solutions in cases where other second-order schemes are prone to stalling.
Limiter	Appears when Momentum, Energy, Two-Equation Turbulence Model, or Humidity, Tracer Fluids and Homogeneous Mixtures is set to Second-order (QUICK), Second-order (SOU), or Second-order (CDS).Specifies the calculation of the limiter for second order schemes. The flow solver uses the limiter to compute the advective flux as a weighted average of the first-order scheme approximation and second-order scheme approximation.AutomaticCalculates the appropriate value for the limiter based on the method you specify in the Momentum Limiter Stabilization, Energy Limiter Stabilization, Two-Equation Limiter Stabilization, and Humidity, Tracer Fluids and Homogeneous Mixtures Limiter Stabilization lists. Both automatic limiter methods compute the limiter value by searching for extreme values over a region surrounding a given node.General Convective Boundedness Condition searches for the extreme values over all neighboring nodes of the node of interest.Stabilized Convective Boundedness Condition searches for the extreme values over neighboring nodes that are upwind of the node of interest.SpecifyAssigns the value for the limiter that you specify in the Momentum Limiter, Energy Limiter, Two-Equation Limiter, and Humidity, Tracer Fluids and Homogeneous Mixtures Limiter boxes.
Buoyancy
Buoyancy Model	Specifies how the buoyancy is calculated in the momentum equations.BoussinesqAssumes that the fluid is incompressible.Full with Hydrostatic PressureAssumes that the fluid is compressible.
Particle Tracking Controls
Steady State Injection Duration	Sets the duration time of the injection of particles into the fluid domain for a steady state flow analysis.
Steady State Simulation Time	Specifies the time of the particle tracking simulation for a steady state flow analysis.Match Injection DurationDefines the particle tracking simulation time to be equal to the particle injection duration time.SpecifyLets you define the particle tracking simulation time. The value that you specify must be greater than the injection duration. You set the value in the Total Time box.
Steady State Output Option	Specifies how the particle time step is defined.Number of OutputsSets the number of time steps for the particle tracking simulation. You set the value in the Number of Outputs box.Output IntervalSets the duration of the time step for the particle tracking simulation. You set the value in the Output Interval box.
Neglect Stochastic Drag Terms	Neglects the Brownian and turbulent diffusivity terms in the particle tracking equations. Usually, you select this check box in conjunction with the Use Cunningham Correction Factor check box.
Use Cunningham Correction Factor	Applies the computed Cunningham correction factor to the particle traction force estimate. The Cunningham correction factor represents a reduction in the force that is exerted upon the particle by the flow due to the breakdown of the no-slip condition on the particle surface. The no-slip condition is invalid when the mean free path of the fluid molecules is of the same order as the particle length scale. This option is valid only for ideal gases. The flow solver computes the correction factor using the following constants:Sutherland constant for the viscosity of the gas. You set the value in the Sutherland Constant box.Slip correction reference temperature, pressure, and dynamic viscosity of the gas. You set these values in the following boxes:Slip Correction Reference TemperatureSlip Correction Reference PressureSlip Correction Reference Dynamic ViscosityNote: Because this option is valid only for ideal gases, make sure that you define the ideal gas constant of the fluid material.

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Flow Solution Parameters dialog box (Multiphysics), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });