You are here: Numerics and Convergence > Numerics

14.2 Numerics

Numerics pertains to parameters and models used to control the numerical solver to discretize and solve the system of algebraic equations.

1. Select the module in the Model Panel.
2. Numerics related settings are accessed in the Properties Panel.

When a template is used, the template should be under Extended Mode to access the numerics for the simulation.

Time Accuracy

Time accuracy methods offer the following three temporal discretization schemes for solving the variables implicitly. First Order: The temporal updates are determined implicitly based on the previous time-step only. Second Order: This is the recommended scheme for higher order in time. The temporal updates are determined implicitly based on the previous two time-steps. The relative influence of the two previous time-steps depends on the Time Blending Factor and Blending Options. The Blending Options can be selected as Everywhere or Boundary Only with regard to location. Crank-Nicolson: The temporal updates are determined based on the previous time-step only, using a combination of an explicit/implicit formulation. The relative influence of implicit vs explicit depends on the Time Blending Factor and Blending Options.

Figure 14.3 - Time accuracy

 

Automatic Relaxation

When selected as Yes in Properties Panel > Model Tab, it adds linear relaxation automatically for the solution of the variable based on mesh quality as shown in equation 14.53.

Relaxation

Controls the amount of correction applied during each iteration, as shown in equation 14.34 and equation 14.53.

• Relaxation range from 0 to 1 whereas typical values of Relaxation range from 0.0 to 0.8.

• A Relaxation of 0 is the most liberal, allowing full application of the correction. It is recommended, assuming no problem with the convergence. Higher values (>0) are recommended if needed, to prevent the solution from diverging.

• A Relaxation value of 1 is the most restrictive, allowing no correction of the solution from one iteration to the next.

Note: For Pressure, there is also an Automatic Relaxation.

Diagonal Relaxation

Diagonal Relaxation is a form of relaxation applied to the diagonal of the solution matrix as shown in equation 14.25. It has an effect similar to the influence of an old value at a previous time-step. During the solution process, the solver provides an estimate of the amount of correction needed to obtain an accurate solution. In general, Relaxation refers to the amount of this suggested correction that is applied for the next iteration. For the Flow module, there are separate values for the velocity and pressure corrections.

• Diagonal Relaxation range from 0 to infinity, however typical values of Diagonal Relaxation range from 0.001 to 1.

• Default values are recommended, assuming no problem with the convergence. Higher values (> 0.3) are recommended if needed to prevent a solution from diverging.

• A Diagonal Relaxation of 0 is the most liberal, allowing full application of the correction.

• A large value of Diagonal Relaxation is the most conservative, slowing down the corrections from one iteration to the next.

 

Numeric Scheme

Numeric Scheme offers the following three spatial interpolation schemes for solving the variables. Upwind: The value at a cell interface is computed from the upwind (upstream) cell value. Central: The value at a cell interface is computed from an average value of cell values on both sides. Central differencing may be used with a Blending Factor and a Bounded Scheme to help control the convergence. 2nd Order Upwind: The value at a cell interface is computed from the face value on upwind side. The face value is calculated by upwind cell value and gradient correction term. This may be used with a Blending Factor and a Bounded Scheme to help control the convergence. High Resolution: The High Resolution provides for a more accurate determination of the value of the components crossing a cell interface based on a proprietary Simerics reconstruction scheme. This may be used with a blending factor to help control the convergence. This is available only for the Multiphase module.

Figure 14.4 - Numerics scheme

 

The Blending Factor and the Bounded Scheme are used to stabilize convergence. Blending Factor Blending Factor is used in conjunction with the higher order interpolation schemes (e.g. Central and 2nd Order Upwind) to help stabilize the convergence. Blending Factor can be set for either Central or 2nd Order Upwind schemes. Typical values of the Blending Factor range from 0.1 to 0.5. Higher values of the Blending Factor make the solution more stable. Bounded Scheme Bounded Scheme is used in conjunction with the higher order interpolation schemes (e.g. Central and 2nd Order Upwind) to help stabilize the convergence by limiting the range of the value of the interpolation to be no more or less than the maximum or minimum (respectively) of the cells neighboring the cell-face of interest.   14.54   A Bounded Scheme can be set for either Central or 2nd Order Upwind in the Properties Panel. There are three options: Unlimited: No bounds are placed on the interpolation. BC Only: Bounds are placed only on the faces next to the Boundaries. Everywhere: Bounds are applied throughout the entire domain.

Figure 14.5 - 2nd order upwind

 

Linear Solver Simerics-MP offers Algebraic Multi-Grid Solver (AMG) and Conjugate Gradient Squared (CGS) linear solvers for solving the equations. This can be selected as follows: Properties Panel > Model Tab > Numerics > Linear Solver > CGS, AMG These solvers may be specified independently for the solving the variables. CGS AMG While AMG is the default for the pressure and temperature solutions, CGS is the default for the solutions of other variables. The solver automatically switches between AMG and CGS, when the current setting does not converge.

Figure 14.6 - Linear solver

Linear Solver Tolerance

The solution process in Simerics-MP is iterative, including for the linear solvers. The user can control the iterative process for any module by setting the Linear Solver Tolerance to the desired convergence tolerance under:

Properties Panel > Model Tab > Numerics > Linear Solver Tolerance > Desired Values.

• Linear Solver Tolerance dictates the linear solver convergence criterion for solutions of the variables.

• A smaller value of Linear Solver Tolerance implies more precision.

• The cost of a smaller value of Linear Solver Tolerance is more sweeps, resulting in more computation time. In some cases, the added accuracy is not worth the additional expense. If the target converge criterion is too small, the solver may not be able to achieve it, in which case the solution will go the full number of sweeps allowed.

The tolerance is normalized relative to the first iteration at the start of the time-step or a steady-state simulation.

 

Sweeps

The solution process in Simerics-MP is iterative, including the linear solver. The user can control the iterative process for any module by setting the sweeps to a maximum allowed value under:

Properties Panel > Model Tab > Numerics > Sweeps > Desired Values.

• If the solver reaches the maximum sweeps, it will advance to the next variable. The default number for Sweeps is 50 for both the pressure and velocity solvers.
• Number of sweeps is also controlled by the Linear Solver Tolerance. In general the solver should attain the desired tolerance before hitting the maximum number of sweeps.

The number of sweeps used for a given iteration are displayed in the *.out file as follows:

INFO(Sim02:Flow:V:CGS): Residual: 4.19235 Sweeps = 1

INFO(Sim02:Flow:P:AMG): Residual: 52.4886 Sweeps = 2

 

Pressure Velocity Coupling Method Simerics-MP offers the following three Pressure Velocity Coupling Methods for coupling the pressure and velocity and solutions. SIMPLE: Semi-Implicit method for pressure linked equations 1Ref. Patankar, Numerical Heat Transfer and Fluid Flow, 1980, ISBN 0-07-048740-5. . SIMPLEC: A general curvilinear coordinates pressure correction scheme (SIMPLEC). Semi-Implicit method for pressure-linked equations, consistent 2Ref: DOORMAAL, J., AND G.D.RAITHBY. “Enhancements of the SIMPLE method for predicting incompressible fluid flows,” Num. Heat Transfer 7 (1984), 147–163. . SimpleS: A Simerics proprietary algorithm. The default Pressure Velocity Coupling Method for Simerics-MP is SimpleS.

Figure 14.7 - Pressure Velocity Coupling

 

Skew Term

Skew Terms in the Turbulence module for Turbulent Kinetic Energy (TKE) and the Turbulent Energy Dissipation Rate (TEDR) solution can be activated as follows:

Model Panel > Turbulence

Properties Panel > Model Tab > Numerics > Skew Term > [Yes or No]

Skew Terms refer to the links between diagonally connected cells in the mesh. These terms typically offer negligible improvement in the solution, while potentially slowing down the calculation. By default they are not used in the solution of the Turbulence module.

 

Max. Temperature Adjustment

The Max. Temperature Adjustment in the Heat module is accessed as follows:

Model Panel > Heat

Properties Panel > Model Tab > Numerics > Max. Temperature Adjustment > [Desired Value]

This limits the amount the temperature may vary during the predictor-corrector solution process. The Max. Temperature Adjustment is used to stabilize convergence similar to a Relaxation Factor. A smaller value of Max. Temperature Adjustment is more stable and could use more computer time.

 

Temperature Lower Limit

The temperature throughout the solution domain can be constrained to be at or above the Temperature Lower Limit. This can be set in the Heat module as follows:

Model Panel > Heat

Properties Panel > Model Tab > Numerics > Temperature Lower Limit > [Desired Value]

The default value for the Temperature Lower Limit is 0.1 K. and is very close to Absolute Zero. It is possible to set the Temperature Lower Limit less than 0 and to solve for negative temperatures in Simerics. In such cases, the absolute temperature scale becomes meaningless and unphysical results would result if the “temperature” were being used to determine physical properties. The setting of a Temperature Lower Limit is a constraint intended to help convergence by bounding the solution during the iterative solution process. If the final solution has temperatures equal to the Temperature Lower Limit, then the solution is over-constrained and the results are most likely unphysical.

 

Temperature Upper Limit

The temperature throughout the solution domain can be constrained to be at or above the Temperature Upper Limit. This can be set in the Heat module as follows:

Model Panel > Heat

Properties Panel > Model Tab > Numerics > Temperature Upper Limit > [Desired Value]

The default value for the Temperature Upper Limit is 6,000 K. This is greater than the temperature of the surface of the sun, so it is higher than what would typically be encountered in most applications. The setting of a Temperature Upper Limit is a constraint intended to help convergence by bounding the solution during the iterative solution process. If the final solution has temperatures equal to the Temperature Upper Limit, then the solution is over-constrained and the results are most likely unphysical.

 

Implicit and Explicit methods

This can be accessed as follows:

Model Panel > Multiphase

Properties Panel > Model Tab > Implicit Method > [Yes or No]

• Yes: Solves the Multiphase transport equations implicitly. This method can use larger time-steps than the explicit method but does not preserve the shape of the interface between components as accurately. This updates the transport of a component from one cell to the next based on the most recent iteration estimated volume fraction in each. The implicit method is the solution method used for other scalars (e.g. Heat, Pressure, Multiphase, etc.) and has similar numerical options as explained above and as shown in Figure 14.12.
• No: Solves the  Multiphase transport equations explicitly. The explicit method is more accurate than the implicit method in preserving the shape of the interface between components, but it does not work when energy equation is turned-on. This method updates the transport of a component from one cell to the next based on the volume fractions from the previous time-step.

 

Maximum Courant Number

The Courant Number () in three dimensions is:

14.55

where are the components of velocity and are the localized dimensions of the mesh cell in the directions respectively, and is the time-step. For the explicit method, the Courant Number is limited to a value less than 1 to avoid numerical instability.

The sub-time-step () is used in the calculation of the transport of the components for the Multiphase module and is computed based on the courant number.

The calculation of is performed only for the cells in the domain that have a mixture of components, and then the smallest of those calculations is used as the for updating the transport of the components.

This can be accessed as follows:

Model Panel > Multiphase

Properties Panel > Model Tab > Maximum Courant Number

For a transient simulation, if the sub-time-step () computed based on the Courant number is larger than the global time-step set via the Simulation Panel, the smaller of the two is used in the calculation of the transport of the components.

 

14.2.1 Flow

14.2.2 Cavitation

14.2.3 Turbulence

14.2.4 Heat

14.2.5 Multiphase

14.2.6 Multicomponent

14.2.7 Species