37.3. General Task Page

The General task page allows you to set various generic problem settings, such as those related to the mesh or the solver. Note that these settings become available only after you read in a case or mesh file. See Reading Mesh Files and Reading and Writing Case Files for details.

Controls

Mesh

contains controls relating to mesh settings.

Scale...

opens the Scale Mesh Dialog Box.

Check

verifies the validity of the mesh. The check provides volume statistics, mesh topology and periodic boundary information, verification of simplex counters, and verification of node position with reference to the axis for axisymmetric cases. See Checking the Mesh for details.

It is recommended that you check the mesh right after reading it into the solver, in order to detect any mesh trouble before you get started with the problem setup.

Report Quality

displays various quantities related to the quality of the mesh in the console, such as Minimum Orthogonal Quality and Maximum Aspect Ratio. See Mesh Quality for details.

Display...

opens the Mesh Display Dialog Box.

Solver

contains controls relating to solver settings.

Type

contains the solution methods available for computing a solution for your model. See Using the Solver for details.

Pressure-Based

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

Density-Based

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

Velocity Formulation

specifies the velocity formulation to be used in the calculation. See Choosing the Relative or Absolute Velocity Formulation 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.

Time

contains options related to time dependence.

Steady

specifies that a steady flow is being solved.

Transient

enables a time-dependent solution. See Performing Time-Dependent Calculations for details.

2D Space

contains options available only when solving two-dimensional problems.

Planar

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 Task Page, as described in Changing Cell and Boundary Zone Types.

Axisymmetric Swirl

specifies that the swirl component (circumferential component) of velocity is to be included in your axisymmetric model. You should select this option if you are solving swirling flow in an axisymmetric geometry (see Swirling and Rotating Flows for more information).

Gravity

enables the specification of gravity.

Gravitational Acceleration

sets the , , and components of the gravitational acceleration vector. (The component is available only in 3D solvers.) See Natural Convection and Buoyancy-Driven Flows for details about buoyancy-driven flows. This option appears only when Gravity is enabled.

Units...

opens the Set Units Dialog Box.

For additional information, see the following sections:


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