|
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. | ||||||
|
Type |
Integer | ||||||
|
Default Value |
5 | ||||||
|
Description |
Specifies the diffusion scheme for CHT solids:
| ||||||
|
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). | ||||||
|
Type |
Integer | ||||||
|
Default Value |
2 | ||||||
|
Description |
Specifies the diffusion scheme for mesh displacement equations:
A value of 3 may improve the mesh quality in some cases, particularly when mesh folding occurs at sharp corners. For details, see Mesh Displacement 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. | ||||||
|
Type |
Integer | ||||||
|
Default Value |
5 | ||||||
|
Description |
Specifies the diffusion scheme for scalars:
| ||||||
|
Type |
Integer | ||||||
|
Default Value |
2 (tetrahedral) 1 (hexagonal) | ||||||
|
Description |
Specifies the diffusion scheme for stress:
| ||||||
|
Type |
Integer | ||||||
|
Default Value |
5 | ||||||
|
Description |
Wallscale diffusion differencing scheme:
| ||||||
|
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. | ||||||
|
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. | ||||||
|
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. | ||||||
|
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. | ||||||
|
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 Setting this to | ||||||
|
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. | ||||||
|
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. | ||||||
|
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. | ||||||
|
Type |
Integer | ||||||
|
Default Value |
0 | ||||||
|
Description |
Controls linearization of equation terms for specified interphase mass transfer. Choosing an appropriate option can help stabilize solution convergence by bounding volume fractions. Value can be set to one of the following options:
| ||||||
|
Type |
Real | ||||||
|
Default Value |
1.0 | ||||||
|
Description |
Multiplies the false timestep used for interphase mass transfer source terms. | ||||||
|
Type |
Logical | ||||||
|
Default Value |
f | ||||||
|
Description |
When set to 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. | ||||||
|
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. | ||||||
|
Type |
Integer | ||||||
|
Default Value |
3 | ||||||
|
Description |
Specifies how the pressure is treated at interfaces to a porous domain:
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. | ||||||
|
Type |
Integer | ||||||
|
Default Value |
1 | ||||||
|
Description |
The | ||||||
|
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 | ||||||
|
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:
| ||||||
|
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:
| ||||||
|
Type |
Logical | ||||||
|
Default Value |
t | ||||||
|
Description |
Discretizes the viscous work term in the energy equation at integration points (ip). It is highly recommended that this parameter is set to | ||||||
|
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. | ||||||
