The parameters on the Advanced Options tab should not need to be changed for most simulations.

Optimization Level

For good solver performance in terms of convergence rate and robustness, it is sometimes necessary to modify the solver control Optimization Level setting. This setting selects different sets of pre-set parameter values that affect performance. Higher values generally result in higher convergence rate with lower convergence robustness. However, the effect on performance is case dependent.

Optimization level descriptions follow:

Pressure Level Information

Sets an X/Y/Z location for reference pressure and a pressure level.

For details, see Pressure Level Information in the CFX-Solver Modeling Guide.

Thermal Radiation Control

For details, see Thermal Radiation Control in the CFX-Solver Modeling Guide.

Body Forces

Under this option, Volume-Weighted should be generally used except for free surface cases.

For details, see Body Forces in the CFX-Solver Modeling Guide.

Interpolation Scheme

For details, see Interpolation Scheme in the CFX-Solver Modeling Guide.

Multicomponent Energy Diffusion

This option is available when a multicomponent flow is used with a heat transfer equation (that is, thermal or total energy). For details, see Multicomponent Energy Diffusion in the CFX-Solver Modeling Guide. The possible options are:

Temperature Damping

For details, see Temperature Damping in the CFX-Solver Modeling Guide.

Velocity Pressure Coupling

The Rhie Chow Option controls the details of the Rhie Chow pressure dissipation algorithm. Fourth Order ensures that the dissipation term vanishes rapidly under mesh refinement. However, it can sometimes induce wiggles in the pressure and velocity fields; for example, near shocks. The Second Order option damps out these wiggles more rapidly, but is also less accurate. The High Resolution option uses Fourth Order as much as possible, but blends to Second Order near pressure extrema. It is a good choice for high speed flow. The default is Fourth Order for most simulations, but High Resolution is automatically chosen if High Speed Numerics is activated under Compressibility Control on the Solver Control tab. The High Resolution option may occasionally be useful in other situations as well. For example, if you observe the simulation diverging and continuity residuals are significantly higher than the momentum residuals prior to divergence.

Compressibility Control

The following options control parameters that affect solver convergence for compressible flows.

The Total Pressure Option controls the algorithm used for static-to-total conversions (and vice versa). There are three possible settings:

For further details, see Total Pressure in the CFX-Solver Theory Guide.

The Automatic option may experience robustness problems for slightly compressible fluids (such as compressible liquids). In such cases, you should consider using the Incompressible option instead.

When the High Speed Numerics option is selected, special numerics are activated to improve solver behavior for high-speed flow, such as flow with shocks. This setting causes the following behavioral changes:

The Clip Pressure for Properties option enables the solver to accept negative absolute pressures in the converged solution. For simulations involving compressible flow, the absolute pressure should not be negative. However, the pressure field required to satisfy the governing equations on a finite mesh may not necessarily satisfy this condition. By default, the solver is robust to a pressure field that may want to temporarily lead to negative pressures, but not if negative pressures are present in the converged solution. The solver can be made robust to negative absolute pressures in the converged solution by activating this parameter, which clips the absolute pressure to a finite value when evaluating pressure-dependent properties such as density.

Linear Solver Control

With Option set to Automatic, you can select an optimization level.

For good solver performance in terms of convergence rate and robustness, it is sometimes necessary to modify the linear solver control Optimization Level setting. This setting selects different sets of pre-set parameter values that affect performance. Higher values generally result in higher convergence rate with lower convergence robustness. However, the effect on performance is case dependent.

Optimization level descriptions follow:

Multiphase Control

The following options handle control of solver details specific to multiphase flows.

When the Volume Fraction Coupling option is set to Segregated, the solver solves equations for velocity and pressure in a coupled manner, followed by solution of the phasic continuity equations for the volume fractions. With the Coupled option, the solver implicitly couples the equations for velocity, pressure, and volume fraction in the same matrix. The coupled volume fraction algorithm is particularly beneficial for buoyancy-dominated flows, such as buoyant free surface problems. The coupled volume fraction algorithm is also extremely beneficial when used in conjunction with models that include forces that are proportional to volume fraction gradients, such as the turbulence dispersion force in Eulerian multiphase flows and the solids pressure force in Eulerian multiphase models of granular flows (see Interphase Momentum Transfer Models in the CFX-Solver Theory Guide). For models of this nature, convergence of the segregated volume fraction algorithm tends to require much smaller physical time scales than are required by the coupled volume fraction algorithm.

The Initial Volume Fraction Smoothing option can be set to None or Volume-Weighted. If the initial conditions for volume fraction have a discontinuity, startup robustness problems may occur. Choosing Volume-Weighted smoothing of these volume fractions might improve startup robustness.

Under Optimization Level, you can select an optimization level.

For good solver performance in terms of convergence rate and robustness, it is sometimes necessary to modify the multiphase Optimization Level setting. This setting selects different sets of pre-set parameter values that affect performance. Higher values generally result in higher convergence rate with lower convergence robustness. However, the effect on performance is case dependent.

Optimization level descriptions follow:

Intersection Control

You can use the options described in this section to control the intersection of non-matching meshes. The parameters that you set here are applied to all interfaces where Intersection Control settings have not been applied individually in domain interface definitions. (See Intersection Control to learn how to apply Intersection Control settings to individual interfaces.)

CFX provides the GGI (General Grid Interface) capability, which determines the connectivity between the meshes on either side of the interface using an intersection algorithm. In general, two intersection methods are provided:

The Bitmap Resolution controls the number of pixels used to fill the 2D pixel map (see description of the bitmap intersection method above). The higher this number, the more accurate the final calculation of the area fractions. In general, the default resolution of 100 should be sufficient but large differences in the mesh resolution on both sides of the interface as well as other mesh anomalies may require the bitmap resolution to be increased. Larger numbers will cause longer intersection times, for example, doubling the bitmap resolution will approximately quadruple the GGI intersection time.

When the Permit No Intersection option is set, the solver will run when there is no overlap between the two sides of an interface. This parameter is mainly useful for transient cases where interface geometry is closing and opening during the run. For example, transient rotor-stator cases with rotating valves, or moving mesh cases where the GGI interface changes from overlap to non-overlap during the simulation both can exhibit this type of behavior. This parameter is not switched on by default.

The Discernible Fraction option controls the minimum area fraction below which partially intersected faces are discarded. The following default values used by the solver depend on the intersection method:

The idea is that intersection inaccuracies should not lead to tiny area fractions that have no impact on the solution.

The Edge Scale Factor option is used to control the detection of degenerate faces. Degenerate faces are detected by comparing the face edge lengths with a characteristic length of the volume touching the face. Degenerated faces will not be intersected and therefore, intersected faces of zero size are discarded so that problems with the 2D projection of those faces are avoided.

The Periodic Axial Radial Tolerance option is used when determining if the surface represented by the interface is a constant axial or radial surface. For a rotational periodic GGI interface, the solver ensures that the ratio of the radial and axial extent compared to the overall extent of each interface side is bigger than the specified value and therefore, the interface vertices do not have the same radial or axial positions.

The Circumferential Normalized Coordinates Option is used to set the type of normalization applied to the axial or radial position coordinates (η). Mesh coordinate positions on GGI interfaces using pitch change are transformed into a circumferential (θ) and axial or radial position (η). The η coordinates span from hub to shroud and are normalized to values between 0 and 1. In cases where the hub and/or shroud curves do not match on side 1 and side 2, different approaches are available to calculate the normalized η coordinates based on side local or global minimum and maximum η values:

The Face Search Tolerance Factor is a scaling factor applied to the element sized based separation distance used to find candidates for intersection. For a given face on side 1 of the interface, candidate faces for intersection are identified on side 2 using an octree search algorithm. The octree search uses this tolerance to increase the sizes of the bounding boxes used to identify candidates. Making this parameter larger will increase the size of the bounding boxes, resulting in possible identification of more candidates.

The Face Intersection Depth Factor is a scaling factor applied to the element sized based separation distance used when performing the direct or bitmap intersection. The final intersection of faces is only applied to those faces that are closer to each other than a specified distance. This distance is calculated as the sum of the average depth of the elements on side 1 and side 2 of the interface. This factor is applied as a scaling on the default distance. It might be necessary to adjust this factor if the normal element depth on the two interfaces sides varies a lot, or side 1 and 2 of the interface are separated by thin regions (for example, thin fin type geometries).

Injection Control

The Injection Control settings are available if any domain has an injection region defined with Injection Location Type set to Selected 2D Regions (see Injection Location Type).

The Injection Control > Surface Injection Control settings are described next.

The Surface Overlap Type options are:

In order for CFX-Solver to locate an injection position on a surface, the specified position (for example, a point from a .csv file) must lie within a certain distance of the surface. That distance is the product of:

If you do not specify a value for Extrusion Factor then the default value of 5 applies. The CFX-Solver Output file notes any injection positions that could not be located on a surface (even those that are intentionally not located on any surface).

The Intersection Control settings are available if Surface Overlap Type is set to Mapped Faces. These are identical to the Intersection Control settings of domain interfaces, described in Intersection Control: Option.

Stabilization Control

You can select Stabilization Control and select an available option to try to avoid solution divergence or, in transient simulations only, to try to avoid unconverged time steps. To try to avoid divergence, set Option to Repeat on Linear Solver Error. To try to avoid unconverged time steps, set Option to Repeat When Unconverged. Under each option, if the applicable type of problem arises, the solver reattempts to compute the failed/diverged timestep/iteration with a reduced timestep or time scale.

The maximum number of reattempts for any given timestep/iteration is specified by Max. Repetitions.

On a given reattempt, the timestep or time scale is scaled from the previous (failed) value by the specified Timestep Factor or Timescale Factor.

After the timestep or time scale is scaled down, it remains at the new value until there is any cause to change it, such as switching to the next value in a prescribed list, or editing a run in progress.

Stabilization Control is not supported for cases that involve any of the following features: