Define/Models/Solver... menu item opens the
Solver panel allows you to specify various parameters associated with the solution method to be used in the calculation, like the dimensionality of the domain, whether the flow is steady or unsteady, the velocity formulation etc.
contains the solution methods available for computing a solution for your model. See Section
25.1 for details about these choices.
enables the pressure-based Navier-Stokes solution algorithm (the default).
enables the density-based Navier-Stokes coupled solution algorithm.
allows you to specify an implicit or explicit solution formulation.
enables an implicit solver formulation.
enables an explicit solver formulation. This formulation is available only for the
Density Based solver.
contains options related to the dimensionality of the problem.
indicates that the problem is two-dimensional. (This option is available only when you start the
2d version of the solver.)
indicates that the domain is axisymmetric about the
Axisymmetric is enabled, the 2D axisymmetric form of the governing equations is solved instead of the 2D Cartesian form. (This option is available only when you start the
2d version of the solver.) Be sure to change the zone type of the axis of rotation to
axis, using the
Boundary Conditions panel, as described in Section
specifies that the swirl component (circumferential component) of velocity is to be included in your axisymmetric model. You should turn on this option if you are solving swirling flow in an axisymmetric geometry
9.5 for more information).
indicates that the problem is three-dimensional. This option will be turned on automatically when you start the
3d version of the solver; you cannot change the setting in this panel.
contains options related to time dependence.
specifies that a steady flow is being solved.
enables a time-dependent solution. See Section
25.17 for details.
specifies the velocity formulation to be used in the calculation. See Section
10.7.1 for details.
enables the use of the absolute velocity formulation. This is the default setting.
enables the use of the relative velocity formulation. This option is available only with the
Pressure Based solver.
contains options related to transient calculations.
Non-iterative Time Advancement
enables non-iterative time-advancement (NITA) scheme. See Section
25.4.5 for details.
Frozen Flux Formulation
enables an option to discretize the convective part of Equation
25.4-25 using the mass flux at the cell faces from the previous time level
n. This option is available only for an
Unsteady solution. See Section
25.4.5 for details.
contains options for setting different time-dependent solution formulations. This option appears only when
Unsteady is enabled under
Time. See Section
25.17 for details.
enables a time-dependent solution using global time stepping. This option is available only for the
Density BasedExplicit solver.
enables a time-dependent solution using first-order-accurate dual time stepping.
enables a time-dependent solution using second-order-accurate dual time stepping.
contains options for setting method of computing the gradient in Equation
25.3-22. See Section
25.3.3 for details.
Green-Gauss Cell Based
enables the cell-based method where cell center values are considered for computing the gradient. This is the default option.
enables the node-based method where the nodal values are considered for computing the gradient.
Least Squares Cell Based
enables the least squares cell-based gradient evaluation which is recommended for accurate flow solutions on polyhedral meshes.
contains option for setting the velocity in the porous medium simulation. See Section
7.19.6 for details.
enables the superficial velocity in a porous medium simulation. This is the default method.
enables the physical velocity in a porous medium simulation for a more accurate simulation. This option is available only for a pressure-based solver. See Section
7.19.7 for details.