ANSYS CFX-Solver Expert Control Parameters

In the following section, the name and function of the available Expert Control Parameters for the ANSYS CFX-Solver is given. Each one is given either a logical, integer or real value. All of the parameters below can be inserted using the Command File editor and “written” back into the definition file before executing the ANSYS CFX-Solver.

Note that changing some of the ANSYS CFX-Solver Control Parameters may affect the output generated by the ANSYS CFX-Solver.

Note

The expert parameters found on the Particle Tracking tab in ANSYS CFX-Pre are described in detail in Expert Parameters for Particle Tracking.

Table 1. List of ANSYS CFX-Solver Expert Control Parameters

Name	`always output post processing`
Type	Logical
Default Value	F
Description	When set to T, makes the solver output flow summaries, variable ranges, forces, moments and scales to the output fie on intermediate adaption steps

Name	`apply ic fluctuations for les`
Type	Logical
Default Value	F
Description	If set to True to force the application of velocity fluctuations when restarting an LES. This is most useful when using a RANS solution as this initial guess. For details, see LES Initialization.

Name	`auto turnoff solve eq flag`
Type	Logical
Default Value	F
Description	This flag determines whether to stop solving individual equations when residuals have fallen below their convergence criteria. If either the U, V, W, P, H or . equations have fallen below their target residual by more than 10%, then each individual equation solution will be stopped in turn and the run completed when the Additional Variable equations have been solved satisfactorily. This is only functional for steady state models, and when the model contains one or more Additional Variables. It is automatically set to (T) if the Auto Timescale feature is invoked.

Name	`backup file at zero`
Type	Logical
Default Value	F
Description	Controls whether a backup file is written after zero timesteps (that is, showing the initial guess field for the run). The output control must also be set to write out backup files for this parameter to have any effect.

Name	`build artificial wall`
Type	Logical
Default Value	T
Description	Artificial walls are usually built during the solution if the Solver detects inflow at an Outlet boundary, or outflow at an Inlet boundary. Set this parameter to F to prevent artificial walls being built. Setting this to F also allows a static-pressure to static-pressure flow problem to be set up, by allowing flow to be ‘sucked' into the Domain through an Outlet boundary. Very small timestep sizes are usually required (an scale where approaches the mesh spacing at the inflow), and this method in general is susceptible to severe convergence difficulties.

Name	`check isolated regions`
Type	Logical
Default Value	T
Description	For serial runs, the solver checks if any fluid domain contains volumetric regions which are isolated pockets. This check cannot be performed for parallel solver runs.

Name	`cht diffusion scheme`
Type	Integer
Default Value	5
Description	Specifies the diffusion scheme for CHT solids: 1=central (interior), central (boundary); 2=posdef coefficients (interior), central (boundary); 3=posdef values (interior), posdef values (boundary); 4=blended scheme (interior), central (boundary); 5=posdef coefficients (interior), posdef values (boundary); 6=blended scheme (interior), posdef values (boundary).

Name	`coupled scalars`
Type	Logical
Default Value	T
Description	All combustion models that solve for the mixture fractions of the reactants and products (single or multiple step reaction models), are solved using a coupled multigrid linear solver. This means that all of the mixture fraction equations are solved simultaneously, with the mixture mass transfer source terms linearized in each equation. Under certain conditions, this coupling procedure can fail, leading to oscillatory convergence or divergence. In this case, you can disable the coupled solver and switch to a segregated approach to solving the mixture fraction equations. This is achieved by setting this parameter to F.

Name	`degeneracy check tolerance`
Type	Real
Default Value	1e-3
Description	On all GGI interfaces (fluid-fluid attachments, periodicity and frame change interfaces), a check is performed for each boundary face on each side of the interface to make sure each face is a finite area. Zero area faces are not permitted on GGI interfaces. The degeneracy check tolerance is used to control this check. Faces whose area is less than this tolerance times the representative cross sectional area of the element involved in the face, are automatically and silently deemed to be degenerate and removed from the interface connection. It is rare that this parameter should need adjustment.

Name	`delete backup files`
Type	Logical
Default Value	T
Description	When set to F, previous backup files are NOT overwritten by the next when using the `backup frequency` parameter.

Name	`force intersection`
Type	Logical
Default Value	F
Description	On all GGI interfaces (fluid-fluid attachments, periodicity and frame change interfaces), the solver performs an intersection procedure to connect the two sides of the interface together. This procedure is CPU intensive, so the result of the intersection is stored in the outgoing results file, for future use (for example, upon restart of the simulation). You can force a reintersection of the GGI interface if desired, upon restart, by setting this parameter to T. It is rare that this parameter should be needed, as it generally only results in wasted CPU time upon a restarted simulation.

Name	`ggi bitmap resolution`
Type	Integer
Default Value	100
Description	GGI intersection involves applying a bitmap to each of the integration point faces on either side of the interface, and examining which bits overlap. This parameter sets the number of pixels along one side of the logically square bitmaps. Increasing this parameter will improve the fidelity GGI intersections, but it will also significantly increase the CPU time required to execute the intersection.

Name	`ggi eta mode`
Type	Integer
Default Value	0
Description	A coordinate transformation is applied to each side of interfaces that involve frame change. This transformation involves creation of normalized circumferential and non-circumferential (i.e., radial or axial) coordinates. Three modes of normalizing the non-circumferential or eta coordinates exist (0 is default): 0) Mixed Normalization: The minimum eta value from either side of the interface is matched during intersection, but the range used for normalization is taken from the first side of the interface. This mode can yield non-overlap near the upper extent of eta values. 1) Global Normalization: The minimum and maximum of the non-circumferential physical coordinates on either side of the interface are used to form a single set of minimum, maximum and range values for eta. This set is used when calculating eta on both sides of the interface. This mode can yield non-overlap near both the lower and upper extents of eta values. 2) Local Normalization: The minimum, maximum and range of non-circumferential physical coordinates from each side of the interface are used when calculating eta for that side of the interface. Thus, eta varies between zero and unity on either side of the interface and non-overlap will not occur.

Name	`ggi periodic axial radial tolerance`
Type	Real
Default Value	0.01
Description	GGI periodic surfaces cannot be constant axial or radial surfaces. This parameter controls the tolerance used to determine if the surface is in one of these two invalid situations.

Name	`ggi permit no intersection`
Type	Logical
Default Value	f
Description	When true, the solver will run happily when there is zero intersection between two sides of a GGI/MFR interface. This is useful for TRS cases with rotating valves, etc. that sometimes are fully closed to the geometry.

Name	`ggi separation factor`
Type	Real
Default Value	1.0
Description	A normal direction tolerance is required when intersecting meshes from either side of an interface. This tolerance is the product of a separation factor and a separation distance. The separation distance is derived from the cube root of element volumes on either side of the interface. Increasing the factor will increase the likelihood of making one (and possibly multiple) intersections of mesh faces on either side of the interface.

Name	`ggi vertex weighting value`
Type	Real
Default Value	10
Description	Weighting applied to GGI vertices during MeTiS partitioning

Name	`ignore solve flag on restart`
Type	Logical
Default Value	F
Description	The solution of the wallscale equation stops after it has converged, even if the other equations have not yet converged. If you perform a restart and reduce the convergence criterion, it will not start solving again because the flag indicating it has converged is still set. To start solving the wallscale equation again on a restart, set this parameter to true.

Name	`imbalance normalisation type`
Type	Integer
Default Value	2
Description	Specifies how imbalances are normalised: 0 -no normalisation 1 -normalise by maximum contribution in domain 2 -normalise by maximum contribution in all connected domains

Name	`include associated fields`
Type	Logical
Default Value	T
Description	Specifies whether gradients or other associated fields should be written to minimal transient files.

Name	`include pref in forces`
Type	Logical
Default Value	F
Description	If set to T, the Solver will account for the specified reference pressure in the force and moment calculation.

Name	`laplacian stresses`
Type	Logical
Default Value	F
Description	When set to T, causes a Laplacian form of the viscous stresses to be used instead of the strictly-correct stress tensor form. When there are strong shear layers in regions of high mesh aspect ratio, the full viscous stress tensor can cause convergence slow-down or convergence stalling at a moderate level (e.g., maximum residuals at 1.0E-2). The Laplacian form converges better in such cases, but is formally less accurate.

Name	`linearly exact numerics`
Type	Logical
Default Value	F
Description	Controls whether numerics are linearly exact (i.e., give a zero error in the presence of a linear solution field). This is a new feature which has so far been found to be useful when there is quiescent flow in a hydrostatic pressure field and the mesh is a non-orthogonal hexahedral or mixed-element mesh.

Name	`max continuity loops`
Type	Integer
Default Value	1
Description	Sets the maximum number of continuity loops to perform within a timestep. The continuity loop iterates on the density*velocity nonlinearity in the continuity equation. The default value of 1 is usually appropriate. For high-speed supersonic flows (Mach numbers above 2), increasing the value to 2 may help convergence.

Name	`mcf concentrations output option`
Type	Integer
Default Value	2
Description	Controls the output of mass concentrations, molar concentrations and molar fractions to the results file. 0 - determine what data to write from the VARIABLES file (or CCL) 1 - do not write this data 2 - do not write this data for mixture fraction based models, and do write this data for other combustion models or no combustion model 3 - always write this data To achieve full backwards compatibility with version 10.0, set this parameter to 3. Note that, in the case of a large number of components (>20), the computational cost of writing the data may be unacceptably high.

Name	`mg solver option`
Type	Integer
Default Value	4 (hydrodynamic equations (u, v, w, p)) 3 (other equations (scalar))
Description	Determines the coarsening algorithm for algebraic multigrid of the fluid coupled equations. The default value of 4 means that the anisotropic coarsening is designed to give robust convergence for the widest possible range of flow conditions. Alternative coarsening algorithms are also available for comparison purposes. A value of 2 means that the anisotropic coarsening is based on the pressure coefficient. This was the previous default value. A value of 3 means that coarsening is based on the velocity coefficient. A value of 1 sets an isotropic coarsening based on topology only (similar to conventional geometric multigrid).

Name	`min timesteps`
Type	Integer
Default Value	None specified
Description	When specified, sets the minimum number of timesteps that must be completed before a solver run is terminated.

Name	`model coefficient relaxation`
Type	Real
Default Value	1.0
Description	Sometimes poor convergence is observed with the turbulence model, characterized by bouncy and residual graphs. Changing this under-relaxation parameter can help, but do not use values lower than 0.1.

Name	`monitor ftrans`
Type	Logical
Default Value	F
Description	When set to T, outputs false transient information (steady state only) to the Solver output file (`*.out`) file for each coefficient loop.

Name	`monitor ranges`
Type	Logical
Default Value	F
Description	When set to T, outputs variable ranges for each coefficient loop in a steady state simulation or for each timestep in a transient simulation.

Name	`monitor residuals`
Type	Logical
Default Value	F
Description	When set to T, outputs maximum residuals and locations for each coefficient loop in a steady state simulation or for each timestep in a transient simulation.

Name	`monitor scales`
Type	Logical
Default Value	F
Description	When set to T, outputs variable scales for each coefficient loop in a steady state simulation or for each timestep in a transient simulation.

Name	`multigrid solver`
Type	Logical
Default Value	T
Description	Control whether multigrid is used in ANSYS CFX-Solver.

Name	`outer loop relaxations default`
Type	Real
Default Value	0.75
Description	The default value for several underrelaxation parameters at the timestep loop level. Bouncy convergence, even with a small timestep, can sometimes be reduced by lowering this value to 0.5 or less. A value below 0.25 is not recommended as that would drastically slow down convergence.

Name	`overlap relaxation fluids`
Type	Real
Default Value	1.0
Description	Linear solver underrelaxation of overlap equations in a parallel run for hydrodynamics equations.

Name	`part cvs weighting`
Type	Logical
Default Value	F
Description	This parameter can be used to enable a more complex, experimental algorithm for parallel partitioning. This method attempts to assign different weights to each node/vertex in the domain, depending on the complexity of the elements surrounding a vertex. It attempts to make a more balanced partitioning for mixed element grids.

Name	`pressure diffusion scheme`
Type	Integer
Default Value	2 (tetrahedral) 1 (hexagonal)
Description	Specifies whether the standard central scheme (default) or the positive definite scheme is applied to the continuity equation. This parameter may be of use in obtaining convergence with poor quality meshes. A value of 2 sets the pressure diffusion scheme to be positive definite.

Name	`pressure reference node`
Type	Integer
Default Value	0
Description	If pressure is not set at any boundary, and the simulation is not transient compressible, the solver will set the pressure at the finite volume equation corresponding to this number. (For single-domain problems, the equation numbering is the same as the node numbering.) The default value is 0, which means the solver chooses the equation number automatically. You will not know which finite volume equation number corresponds to a particular location.

Name	`pressure reference value`
Type	Real
Default Value	0
Description	The relative pressure to set at the pressure reference node.

Name	`relax mass`
Type	Real
Default Value	0.75
Description	Changing the value of this parameter can aid convergence for problems that show residual oscillations in separation and re-attachment regions. As it relaxes, the mass flow calculation procedure, it should not be used for transient problems (or should be set to 1).

Name	`rfr domain rotation`
Type	Logical
Default Value	F
Description	When set to T, this will force the solver to write theta shift information to the results, backup and transient results files. This could be useful in a single domain transient case when the domain is rotating to allow you to see the domain rotation in ANSYS CFX-Post. It could also be used in single domain cases when you wish to see the circumferential location of the domain. This information is usually only output for MFR simulations to allow you to see the relative position of the domains in ANSYS CFX-Post.

Name	`scalar diffusion scheme`
Type	Integer
Default Value	5
Description	Specifies the diffusion scheme for scalars: 1=central; 1=central (interior), central (boundary); 2=posdef coefficients (interior), central (boundary); 3=posdef values (interior), posdef values (boundary); 4=blended scheme (interior), central (boundary); 5=posdef coefficients (interior), posdef values (boundary); 6=blended scheme (interior), posdef values (boundary).

Name	`solve energy`
Type	Logical
Default Value	T
Description	Flag for controlling whether or not the controller solves the energy equation.

Name	`solve fluids`
Type	Logical
Default Value	T
Description	Flag for controlling whether or not the controller solves the hydrodynamics equations. Use if you have obtained convergence and you need to continue solving other equation groups.

Name	`solve masfrc`
Type	Logical
Default Value	T
Description	Flag for controlling whether or not the controller solves for mass fraction.

Name	`solve mixture fraction`
Type	Logical
Default Value	T
Description	Flag for controlling whether or not the controller solves for mixture fraction mean and variance equations.

Name	`solve postproc masfrc`
Type	Logical
Default Value	T
Description	Flag for controlling whether or not the controller solves the mass fraction equations in chemistry post processing. This flag affects only post processed components. The equations for regular components of the mixture are solved in the main iteration and may be controlled using the solve `masfrc parameter`.

Name	`solve postproc tvariance`
Type	Logical
Default Value	T
Description	Flag for controlling whether or not the controller solves the temperature variance equation in chemistry post processing. This flag applies only if the temperature variance equation is solved as part of chemistry post processing. When solved as part of the main iteration, the corresponding solve temperature variance flag applies.

Name	`solve radiation`
Type	String
Default Value	T
Description	Flag for controlling whether or not the controller solves the radiation equations

Name	`solve reaction progress`
Type	Logical
Default Value	T
Description	Flag for controlling whether or not the controller solves for reaction progress equations. For details, see Other Parameters.

Name	`solve scalar`
Type	Logical
Default Value	T (if running with additional variables)
Description	Flag for controlling whether or not the controller solves equations for additional variables.

Name	`solve soot`
Type	Logical
Default Value	T
Description	Flag for controlling whether or not the controller solves equations for soot equations.

Name	`solve temperature variance`
Type	Logical
Default Value	T
Description	Flag for controlling whether or not the controller solves for the temperature variance equation.

Name	`solve turbulence`
Type	Logical
Default Value	T
Description	Flag for controlling whether or not the controller solves the turbulence model equations

Name	`solve volfrc`
Type	Logical
Default Value	T
Description	Flag for controlling whether or not the controller solves the volume fraction equations

Name	`solve wallscale`
Type	Logical
Default Value	T
Description	Flag for controlling whether or not the controller solves the wall scale (wall distance) equations.

Name	`solver relaxation fluids`
Type	Real
Default Value	0.9
Description	The under-relaxation value for the coupled U, V, W and P linear smoother within the multigrid solver. On a very poor mesh, coupled U, V, W and P linear solver failure can be helped by increasing this under-relaxation to, for example, 0.75.

Name	`solver relaxation scalar`
Type	Real
Default Value	0.9
Description	The under-relaxation value for the scalar linear smoother within the multigrid solver. On a very poor mesh, scalar equation linear solver failure can be helped by increasing this under-relaxation to, for example, 0.75.

Name	`solver target reduction fluids`
Type	Real
Default Value	0.1
Description	The linear solver for the coupled mass-momentum system iterates until the final RMS residual for the continuity equation is below this number times the initial RMS continuity residual. It is occasionally useful, for testing purposes for instance, to drive the linear solver to a tighter tolerance (e.g., to machine round-off).

Name	`solver target reduction scalar`
Type	Real
Default Value	0.1
Description	The linear solver for a scalar equation iterates until the final RMS residual is below this number times the initial RMS residual. It is occasionally useful, for testing purposes for instance, to drive the linear solver to a tighter tolerance (e.g., to a machine round-off).

Name	`stage reverse flow robustness`
Type	Logical
Default Value	f
Description	Flag to increase robustness when there is reverse flow on the downstream side of a Stage interface.

Name	`stress diffusion scheme`
Type	Integer
Default Value	2 (tetrahedral) 1 (hexagonal)
Description	Specify whether the standard central scheme (default) or the positive definite scheme is applied to the momentum equation. This parameter may be of use in obtaining convergence with poor quality meshes. A value of 2 sets the stress diffusion scheme to be positive definite.

Name	`target imbalance scalar`
Type	Real
Default Value	Set in ANSYS CFX-Pre
Description	The target imbalance for Additional Variables, is by default, equivalent to that of the governing equations. It may be useful to set the target imbalance of scalar quantities to a less-stringent tolerance to obtain convergence.

Name	`tbulk for htc`
Type	Real
Default Value	300 K
Description	When the Heat Transfer Coefficient (HTC) is computed for a temperature specified wall, by default a near-wall fluid temperature is used for a temperature scale. However, for consistency with traditional 1D analyses, the user may wish to enter a reference bulk temperature to compute the HTC. This parameter is that reference value. Thus the HTC computed when this parameter is provided is equal to the local heat flux calculated by the solver divided by the difference of the specified wall temperature and this specified bulk temperature.

Name	`tef numerics option`
Type	Integer
Default Value	0
Description	The and SST turbulence models sometimes give convergence difficulties in areas of extremely high gradients in , for example, at a blunt trailing edge or sudden rearward facing surface, in conjunction with a highly refined boundary layer grid (generally resolved into the viscous sub-layer). The SST model is most susceptible to this problem. Symptoms are generally a lack of convergence with residuals stuck at regions of extremely high gradients of omega, sometimes leading to sudden, early total failure of the solver. In these cases, a flux limiting numerics implementation can be used for the equation, activated by setting this parameter to 1. This setting may become the default setting in a future release.

Name	`tke eps timescale limiter`
Type	Logical
Default Value	F
Description	Specifies whether or not the tke dissipation and ted production terms use a ratio limited by the molecular viscosity. May help convergence for stably stratified buoyant flows.

Name	`topology estimate factor`
Type	Real
Default Value	1.0
Description	This parameter adjusts an internal factor used to help when the solver is estimating the total memory required to store the control volume equation matrix. Sometimes the internal factor is not sufficient and the solver will stop indicating that the “topology estimate factor” parameter must be increased. If this is the case, supply a number for this parameter that is larger than 1; for example, 1.2 will increase the internal memory estimate by 20%, which is often sufficient. Do not use this parameter unless informed to in a run-time error message.

Name	`transient initialization override`
Type	Logical
Default Value	F
Description	When set to T, allows solver default values to be used for initialization in a transient simulation.

Name	`use kolmogorov ts for extinction`
Type	Logical
Default Value	F
Description	This parameter is provided for backwards compatibility with the first release of the extinction model. It is not recommended for use (leave at default setting of F, which uses the turbulence time scale for the flame extinction model). When set to true, the Kolmogorov time scale is used in the extinction model (not recommended).

Name	`vector parallel tolerance`
Type	Real
Default Value	5.0
Description	The value of this parameter is the number of degrees tolerated by the solver in determining the maximum deviation of any element face normal from the calculated average element face normal in a Symmetry Plane boundary condition. This error may occur when element inflation is used on surfaces adjacent to the Symmetry Plane boundary. Increase this value to relax the tolerance.

Name	`volfrc sumapp`
Type	Logical
Default Value	T
Description	For multiphase calculations, the linear equations for phasic continuity (i.e., the volume fraction equations) are not always diagonally dominant. Setting this parameter to true will force the linear equations to be diagonally dominant. This may improve robustness in some situations, but may also considerably slow down the convergence rate.

Name	`wall clock time`
Type	Logical
Default Value	F
Description	Output wall clock time during the outer loop in a steady state run or timestep loop in a transient run.

Name	`wallscale diffusion scheme`
Type	Integer
Default Value	5
Description	Wallscale diffusion differencing scheme 1=central (interior), central (boundary); 2=posdef coefficients (interior), central (boundary); 3=posdef values (interior), posdef values (boundary); 4=blended scheme (interior), central (boundary); 5=posdef coefficients (interior), posdef values (boundary); 6=blended scheme (interior), posdef values (boundary).

Name	`wallscale relaxation factor`
Type	Real
Default Value	0.75
Description	This is a relaxation factor for the wallscale equation, which is solved for all and SST turbulence models.