Setting flow solver parameters

The described options are available on the 3D Flow Solver page in the Solver Parameters dialog box.

Convergence Criteria

The convergence criteria for the flow solver sets the level at which the solver is said to be converged. You can either base the convergence criteria on maximum residual or the RMS residual at each node (control volume). The residual, rn, is the difference between the right hand side of the system of equations, b, and the coefficient matrix, A, multiplied by the approximate solution at the nth iteration, xn: rn = b - Axn.

• Maximum residual is the maximum of all the residuals at a given node.

• Root mean square (RMS) residual is the root mean square average of all the residuals at a given node.

The number of residuals at a given node depends on the number of equations solved (one for mass, three for momentum, one for energy, two for turbulence, one for each scalar, and one for humidity). When the maximum or RMS residual error at any node (control volume) in the model is less than the defined value, then the solver stops iterating.

However, maximum residuals are not a true indication of model convergence, since even very small errors can accumulate across a large mesh domain. You should always check the global momentum, mass, and energy balance for the solution listed in the displayed messages.

Note:

When you apply the Flow Convergence simulation object in the analysis, the specified settings override the residual based convergence. For more information, see Flow Convergence.

Global heat and flow imbalance fractions

The Global Flow Imbalance Fraction and Global Heat Imbalance Fraction ensure that the flow solver continues iterating until the mass flow and heat flow into and out of the system are balanced to within specified percentages. These options use a physical approach to measuring convergence and may give a clearer picture of the solution's accuracy. If you select these options the software checks for mass flow balance and heat flow balance in addition to the convergence criteria.

Caution:

Even if you select these options, you should still check the solution’s global momentum, mass, and energy balances that are listed in the display messages.

3D Flow Iteration Limit

The Iteration Limit sets a hard stop for the flow solver at each time step. If the solver has not converged within this maximum number of iterations, it passes to the next time step. The Iteration Limit is small for a transient analysis. Since the time steps are small relative to the flow behavior, the change between each time step should be small and the solver should converge quickly. Highly non-linear models may require a larger Iteration Limit. Increase the Iteration Limit if the solver often reaches the maximum during the solution process. This may also indicate that the time step is too large for the solution.

Advection Schemes

Advection schemes provide numerical discretization methods to solve the partial differential equations of the momentum, energy, turbulence, and scalar equations. The following advection schemes are available for the flow solver.

First Order

This is the more robust and versatile scheme. Use this scheme when there are no major gradients in the flow field.

Second Order Upwind (SOU)

This scheme yields better precision especially for tetrahedral and wedge fluid elements.

Second Order (QUICK)

This scheme provides the highest precision but lower stability. Use this scheme to have a greater accuracy in the presence of significant gradients in a flow field.

Second-order (CDS)

This is a central differencing scheme which is optimal for low speed flows with a Peclet number that is less than 10.

Second order schemes are mathematically more accurate, but they are prone to overshoots, resulting in non physical results.

Second order advection schemes use limiters to avoid this type of inaccuracy. The limiter represents the proportion of the second order scheme that is blended with the first order scheme. You can either use automatic limiters or specify a value for each equation.

• A limiter value of 0 means that only the first order scheme is used.

• A limiter value of 1 means that only the second order scheme is used.

For LES — Large Eddy Simulation turbulence model, you should always use one of the second order advection schemes for momentum and energy equations.

The Two-Equation Turbulence Model option only applies if you selected the K-Epison, SST — Shear Stress Transport, or K-Omega two-equation turbulence model on the Solution Details page in the Solution dialog box.

The Humidity, Tracer Fluids and Homogeneous Mixtures option only applies when you are solving for humidity, tracer fluids, or homogeneous mixtures.

Example:

If a model shows convergence problems for the momentum equations but not for the energy equation, you can decrease the Momentum Limiter value or use the First Order advection scheme for Momentum, while using one of the second order schemes for the energy equations.

Buoyancy

When buoyancy exists in your model, you must include the gravity force in the source term of the momentum equations. To include the gravity force, select the Buoyancy check box on the Solution Details page in the Solution dialog box.

The Buoyancy option controls how the software calculates the buoyancy in the momentum equations. The following models available are:

Boussinesq

Adds the following buoyancy force per unit volume to the source term of the momentum equations:

-ρβ(T-Tr)g

where ρ is the fluid density, β is the coefficient of thermal expansion, T is the fluid temperature, Tr is a reference temperature evaluated by the solver, and g is the gravity constant. The software assumes that the density does not vary with pressure. Because flow results are outputted in terms of total pressure, the fluid pressure does not change with height. This is the recommended buoyancy model when you include buoyancy calculation with fluids that have constant density.

Full with Hydrostatic Pressure

Adds the following buoyancy force per unit volume to the source term of the momentum equations:

(ρ-ρr)g

where ρ is the fluid density, ρr is the reference density of the fluid evaluated by the solver, and g is the gravity constant. Because the flow results are outputted in terms of static pressure, the fluid pressure changes with height. This is the recommended buoyancy model when you include buoyancy calculation with fluids that have density that varies with pressure.

Steady state particle tracking

To run a particle tracking simulation using the steady state fluid domain, you need to specify the injection duration time, the particle tracking simulation time, and the number of particle tracking time steps.

Steady State Injection Duration box

Sets the duration time during which the particles are injected into the fluid domain.

Steady State Simulation Time list

Specifies the particle tracking simulation time. You can match the injection duration time or specify an alternate total time for the particle tracking simulation. The value that you specify must be greater than the injection duration.

Steady State Output Option list

Specifies how the number of particle tracking time steps is defined. You can directly set the number of particle time steps or the duration of a particle time step. In this case, the number of time steps is obtained by dividing injection duration time by output interval value and rounding to the nearest integer.

Other particle tracking controls

These controls apply to all particle tracking simulation types.

Neglect Stochastic Drag Terms option

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 option

Applies the computed Cunningham correction factor to the particle traction force estimate. The Cunningham correction factor represents the reduction in the force 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 that you specify:

• Sutherland constant for the viscosity of the gas

• Slip correction reference temperature, pressure, and dynamic viscosity of the gas

How do I

How to choose values for Maximum Normalized Velocity Change and Maximum Normalized Pressure Change

Learn more

Adjusting solver parameters

Setting thermal solver parameters

Setting coupled solver parameters

Understanding radiation parameters

Setting relaxation factors for the flow solver

Defining a time step for a flow analysis

Understanding the freeze flow field options

Modeling humidity

Homogeneous Gas Mixture

Flow Convergence

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Simcenter 3D Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal boundary conditions

Setting flow solver parameters, 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 } });