## 20.6. Advanced Options Tab

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

### Dynamic Model Control

When Global Dynamic Model Control is selected, it enables some special modes to be implemented in the solver for the first few iterations or timesteps. For details, see Advanced Options: Dynamic Model Control in the CFX-Solver Modeling Guide.

For details on Turbulence Control, see Turbulence Control in the CFX-Solver Modeling Guide.

For details on Combustion Control, see Advanced Combustion Controls in the CFX-Solver Modeling Guide.

For details on Hydro Control, see Hydro Control in the CFX-Solver Modeling Guide.

### 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:

- `Automatic`: uses unity Lewis number when no component diffusivities specified and no algebraic slip model; uses generic assembly when necessary

- `Generic Assembly`: sets default component diffusivities to unity Schmidt number Sc = 1; generic treatment of energy diffusion term with support for user defined component diffusivities and algebraic slip model

- `Unity Lewis Number`: sets Le = 1; single diffusion term, rather than separate term for contribution of every component, resulting in faster solver runs; the default molecular diffusion coefficient for components is derived from thermal conductivity

  Note: Forcing unity Lewis number mode when not physically valid may lead to inconsistent energy transport. Therefore this setting is not recommended.

### 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:

Incompressible

  The incompressible assumption is used in all situations.

Automatic

  The total pressure is calculated depending on the equation of state.

Unset

  This is equivalent to `Automatic` when the total energy model is used, and `Incompressible` otherwise.

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:

- It activates a special type of dissipation at shocks to avoid a transverse shock instability called the carbuncle effect (which may occur if the mesh is finer in the transverse direction than in the flow direction).

- It activates the High Resolution Rhie Chow option to reduce pressure wiggles adjacent to shocks.

- It sets the nodal pressure gradients to zero at all pressure boundaries as well as openings.

- For steady-state flows, it modifies the default relaxation factors for the advection blend factor and gradients.

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.

### 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.

Note: If you encounter convergence difficulties when using a turbulence dispersion model in conjunction with `Segregated` volume fraction coupling, then you should consider reducing the physical time scale, or switching to `Coupled` volume fraction coupling.

Note: If the residuals fail to drop reasonably well while solving a case that uses the `Coupled` option, it may be beneficial to reduce the mass flow under-relaxation parameter, `relax mass`, below its default value. For details on this parameter, see Convergence Control Parameters in the CFX-Solver Modeling Guide.

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 may improve startup robustness.

### 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:

- Bitmap Intersection:

  Two faces on either side of the interface which have to be intersected are both drawn into an equidistant 2D pixel map. The area fractions are determined by counting the number of pixels that reside inside both intersected faces (that is, within the union of the two faces). The area fraction for a face is then calculated by dividing the number of overlapping pixels by the total number of pixels in the face. This method is very robust.

- Direct Intersection (Default):

  Two faces on either side of the interface are intersected using the Sutherland-Hodgeman clipping algorithm. This method computes the exact area fractions using polygon intersection, and is much faster and more accurate than the bitmap method.

Note:

- If Direct (one-to-one) mesh connectivity is available, the solver will ignore the Intersection Control option and will instead use a 'topological intersection', that is, use the one-to-one information to generate the intersection data.

- If you are restarting a run, the intersection step is skipped and the intersection data is read from the results file. This behavior can be overridden by setting the expert parameter `force intersection` to `True`.

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:

- Bitmap Intersection: 1/(Bitmap Resolution)^1.5

- Direct Intersection: 1.0E-06

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:

- Mixed (Default for Fluid Fluid interfaces): Normalization of η is based on local minimum and maximum η values as well as the η range of side 1. This method forces the hub curves on side 1 and 2 to align. Non-overlap regions adjacent to the shroud may be produced if the shroud curves are not the same.

- Global (Default for Fluid Solid Interfaces): Normalization of η is based on global minimum and maximum eta values. This method intersects side 1 and 2 unchanged from their relative positions in physical coordinates. If the hub and shroud curves do not match then non-overlap regions will be produced.

- Local: Normalization of η is done locally for each side of the interface. This method will always produce an intersection of side 1 and 2, but may cause undesirable scaling of the geometry in some cases.

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).

Release 18.2 - © ANSYS, Inc. All rights reserved.