## 32.3.1 Define/Models/Solver...

The Define/Models/Solver... menu item opens the Solver panel.

Solver Panel

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.

Controls

Solver   contains the solution methods available for computing a solution for your model. See Section  25.1 for details about these choices.

Pressure Based   enables the pressure-based Navier-Stokes solution algorithm (the default).

Density Based   enables the density-based Navier-Stokes coupled solution algorithm.

Formulation   allows you to specify an implicit or explicit solution formulation.

Implicit   enables an implicit solver formulation.

Explicit   enables an explicit solver formulation. This formulation is available only for the Density Based solver.

Space   contains options related to the dimensionality of the problem.

2D   indicates that the problem is two-dimensional. (This option is available only when you start the 2d version of the solver.)

Axisymmetric   indicates that the domain is axisymmetric about the axis. When 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  7.1.3.

Axisymmetric Swirl   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 (see Section  9.5 for more information).

3D   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.

Time   contains options related to time dependence.

Unsteady   enables a time-dependent solution. See Section  25.17 for details.

Velocity Formulation   specifies the velocity formulation to be used in the calculation. See Section  10.7.1 for details.

Absolute   enables the use of the absolute velocity formulation. This is the default setting.

Relative   enables the use of the relative velocity formulation. This option is available only with the Pressure Based solver.

Transient Controls   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.

Unsteady Formulation   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.

Explicit   enables a time-dependent solution using global time stepping. This option is available only for the Density Based Explicit solver.

1st-Order Implicit   enables a time-dependent solution using first-order-accurate dual time stepping.

2nd-Order Implicit   enables a time-dependent solution using second-order-accurate dual time stepping.

Gradient Option   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.

Green-Gauss Node-Based   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.

Porous Formulation   contains option for setting the velocity in the porous medium simulation. See Section  7.19.6 for details.

Superficial Velocity   enables the superficial velocity in a porous medium simulation. This is the default method.

Physical Velocity   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.