### 17.3.1. Discretization Parameters

Diffusion Scheme
`bounded bnd diffusion tets`
Type | Logical
Default Value | f
Description | Controls whether or not a bounded diffusion scheme is used at boundaries for tetrahedral elements. The diffusion scheme for other element types is bounded by default through the default setting of 5 for the expert parameters 'cht diffusion scheme' and 'scalar diffusion scheme'. Tetrahedral elements are controlled separately because the bounded scheme may lead to less accurate results.
`cht diffusion scheme`
Type | Integer
Default Value | 5

Description

Specifies the diffusion scheme for CHT solids:

1 = Central (interior), central (boundary)
2 = Positive definite coefficients (interior), central (boundary)
3 = Positive definite values (interior), positive definite values (boundary)
4 = Blended scheme (interior), central (boundary)
5 = Positive definite coefficients (interior), positive definite values (boundary)
6 = Blended scheme (interior), positive definite values (boundary)

`diffusion at inlets`
Type | Logical
Default Value | f
Description | Indicates whether to include diffusion terms at inlets, openings, and outlets for scalar equations (for example, Additional Variables, species, turbulence, and so on).
`meshdisp diffusion scheme`
Type | Integer
Default Value | 2

Description

Specifies the diffusion scheme for mesh displacement equations:

1 = Central (interior), central (boundary)
2 = Positive definite coefficients (interior), central (boundary)
3 = Positive definite values (interior), positive definite values (boundary)
4 = Blended scheme (interior), central (boundary)

A value of 3 may improve the mesh quality is some cases, particularly when mesh folding occurs at sharp corners. For details, see Mesh Displacement Diffusion Scheme.

`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.
`scalar diffusion scheme`
Type | Integer
Default Value | 5

Description

Specifies the diffusion scheme for scalars:

1 = Central (interior), central (boundary)
2 = Positive definite coefficients (interior), central (boundary)
3 = Positive definite values (interior), positive definite values (boundary)
4 = Blended scheme (interior), central (boundary)
5 = Positive definite coefficients (interior), positive definite values (boundary)
6 = Blended scheme (interior), positive definite values (boundary)

`stress diffusion scheme`
Type | Integer
Default Value | 2 (tetrahedral) 1 (hexagonal)

Description

Specifies the diffusion scheme for scalars:

1 = Central (interior), central (boundary)
2 = Positive definite coefficients (interior), central (boundary)
3 = Positive definite values (interior), positive definite values (boundary)
4 = Blended scheme (interior), central (boundary)
5 = Positive definite coefficients (interior), positive definite values (boundary)
6 = Blended scheme (interior), positive definite values (boundary)

`wallscale diffusion scheme`
Type | Integer
Default Value | 5

Description

Wallscale diffusion differencing scheme:

1 = Central (interior), central (boundary)
2 = Positive definite coefficients (interior), central (boundary)
3 = Positive definite values (interior), positive definite values (boundary)
4 = Blended scheme (interior), central (boundary)
5 = Positive definite coefficients (interior), positive definite values (boundary)
6 = Blended scheme (interior), positive definite values (boundary)

Tolerances
`degeneracy check tolerance`
Type | Real
Default Value | 1e-4
Description | A face set is considered degenerate if the dimensionless area of the face set is less than this tolerance. The dimensionless area is calculated as the ratio of the area of the domain boundary (summed up over all integration point faces on the domain boundary) to a geometry length scale based on the volume of the elements adjacent to the domain boundary. If the dimensionless area is smaller that the specified tolerance, the whole domain boundary is flagged as degenerate. Note that no-slip wall boundaries that are flagged as degenerate are not allowed and the solver will stop with an error message. Also, when symmetry conditions are applied to a degenerate domain boundary, vectors and tensors on the domain boundary are modified to satisfy the required conditions. For example, all components of vectors that are orthogonal to the degenerate domain boundary are set to zero.
`tangential vector tolerance`
Type | Real
Default Value | 10.0
Description | The solver will trigger an error message when the angle between the specified direction at a total pressure inlet and the inlet face is smaller than this angle.
`vector parallel tolerance`
Type | Real
Default Value | 1.0

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.

Miscellaneous
`bcp arithmetic aver sum option`
Type | Integer
Default Value | 0

Description

Controls the interpolation of variables when calculating arithmetic averaging and sum quantitative CEL functions on boundary patches, as well as RMS averaging quantitative CEL functions. The results calculated by these quantitative CEL functions can differ between CFX-Solver and CFD-Post.

A value of 0 indicates that variables at face centers are used for the calculation, while a value of 1 indicates that variables at boundary vertices are used. The latter option leads to results that are more consistent between CFX-Solver and CFD-Post; however, the results can still differ due to edge and corner effects. This option can also lead to changes in the convergence of solutions computed by CFX-Solver, because sometimes the results of quantitative CEL functions of these types are used in the solver control area.

For details on how CFD-Post and CFX-Solver compute values differently, see ave in the CFX Reference Guide, rmsAve in the CFX Reference Guide, and sum in the CFX Reference Guide.

`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 from being built. Setting this to `'f'` also enables you to set up a static-pressure to static-pressure flow problem, by enabling 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.
`fsdamp efficiency scale`
Type | Real
Default Value | 0.01
Description | Scaling factor for the free stream damping used in the efficiency calculation. For details, see Isentropic Efficiency and Total Enthalpy.
`highres energy option`
Type | Integer
Default Value | 0

Description

This parameter controls how the high resolution blend factor is calculated for the energy equation.

Note that the blend factor is always shared with the species equations for multicomponent flow, with the actual blend factor taken as the most conservative of all contributions from the energy and mass fraction group.

The information below indicates which variable is used to calculate the energy equation blend factor for single-component flow and the energy equation's contribution to the shared blend factor for multicomponent flow:

0 = Enthalpy for single component flow, enthalpy for multicomponent flow.

1 = Enthalpy for single component flow, no contribution for multicomponent flow.

2 = Enthalpy for single component flow, temperature for multicomponent flow.

3 = Temperature for single component flow, temperature for multicomponent flow.

`ipmt area density clip`
Type | Logical
Default Value | t
Description | Controls whether the interfacial area density is clipped to a non-zero value for interphase mass transfer models. The value at which clipping occurs is obtained by using the specified minimum volume fraction (see Minimum Volume Fraction in the CFX-Solver Modeling Guide) in the calculation of interfacial area density. Using a clipped interfacial area density can serve as a crude nucleation model for some kinds of mass transfer, but can affect mass conservation within the solution.
`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 (for example, maximum residuals at 1.0E-2). The Laplacian form converges better in such cases, but is formally less accurate.
`linearly exact numerics`
Type | Logical
Default Value | f
Description | Controls whether numerics are linearly exact (that is, give a zero error in the presence of a linear solution field). This is a feature that 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.
`porous cs discretisation option`
Type | Integer
Default Value | 3

Description

Specifies how the pressure is treated at interfaces to a porous domain:

1 = Constant static pressure
2 = Constant total pressure
3 = Constant total pressure based on the normal component of velocity at the interface

Option 1 is the least physically realistic setting.

Option 2 is a more realistic setting. However, when using this setting the CFX-Solver may fail to converge in cases where sections of the porous interface have little or no flow normal to the interface.

Option 3 is the most realistic setting and also converges better than option 2.

`tef numerics option`
Type | Integer
Default Value | 1
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.
`transient startup option`
Type | Integer
Default Value | 0
Description | Controls the startup option for 2nd order transient discretization: 0 = 1st order scheme applied to first timestep (non-conservative). 1 = Modified 2nd order applied to first timestep (conservative). 2 = Standard 2nd order applied to first timestep, but with assumed at start.
`vfr gradient force option`
Type | Integer
Default Value | 2

Description

Used to switch between old and new discretization schemes for force terms proportional to volume fraction gradients, namely, turbulent dispersion force and solid pressure. The old scheme adds the force explicitly as a source term. The new formulation discretizes the term implicitly as a gradient term, hence allows the term to be taken into account in a coupled manner when used in conjunction with the coupled volume fraction algorithm.

Possible values are:

0 = Original formulation, added to source terms
1 = New formulation for turbulent dispersion forces, but excluded from Rhie-Chow
2 = New formulation for turbulent dispersion forces, including Rhie and Chow
3 = Include solids pressure as well

`virtual mass force option`
Type | Integer
Default Value | 1

Description

Used to switch between old and new discretization schemes for virtual mass forces. The old scheme adds the force explicitly as a source term, with velocity gradients discretized using central differences. The new formulation discretizes the term implicitly, and uses an upwind scheme to discretize velocity gradients. Possible values are:

0 = Original source term formulation
1 = New implementation upwind, ignoring mass imbalance
2 = New implementation upwind, including mass imbalance

`viscous work at ip`
Type | Logical
Default Value | f
Description | Discretizes the viscous work term in the energy equation at integration points (ip).
`volfrc sumapp`
Type | Logical
Default Value | t
Description | For multiphase calculations, the linear equations for phasic continuity (that is, 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.

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