The basic settings apply to the whole of the domain. When you create a new domain, the Basic Settings tab is initially shown.
The Location is the list of assemblies,
3D primitive regions and/or 3D composite regions that define the
volume of the domain. For details, see Mesh Topology in CFX-Pre.
Using an assembly or a composite region in the Location list implicitly
includes all 3D primitives contained within the object. You can use
more than one location by using the Shift or Ctrl keys to pick multiple entries from the drop-down list.
The 
icon to the right of the drop-down list can be
used to pick locations from an expanded list. Alternatively, clicking
a location in the viewer displays a small box containing the available
locations.
For details, see Domain and Subdomain Locations.
The Domain Type setting can be set to one of the following:
Fluid Domain
Fluid domains are used to model one fluid or a combination of fluids, with a wide range of modeling options. It is possible to deform the mesh to simulate movement of the boundaries of the domain; for details, see Mesh Deformation.
Solid Domain
Solid domains are used to model regions that contain no fluid or porous flow. Several modeling options are available, including heat transfer (see Conjugate Heat Transfer in the CFX-Solver Modeling Guide), radiation (see Radiation Modeling in the CFX-Solver Modeling Guide), and Additional Variables (see Additional Variables and Additional Variables in the CFX-Solver Modeling Guide). In addition, you can model the motion of a solid that moves relative to its reference frame; for details, see Solid Motion.
Porous Domain
Porous domains are similar to fluid domains, but are used to model flows where the geometry is too complex to resolve with a grid. For details, see Flow in Porous Media in the CFX-Solver Theory Guide.
Immersed Solid
Immersed Solid domains can be used in transient simulations to model rigid solid objects that move through fluid domains; for details, see Domain Motion and Immersed Solids in the CFX-Solver Modeling Guide.
By default in a fluid domain, Coordinate Frame is set to the default Cartesian frame, Coord 0, but you can select any predefined coordinate frame. To create a
new coordinate frame, select Insert > Coordinate Frame from the menu bar. For details, see Coordinate Frames and Coordinate Frames in the CFX-Solver Modeling Guide.
The coordinate frame set for a domain is local to only that domain and is used to interpret all x, y and z component values set in the domain details view. This includes the gravity components in a buoyant flow and the rotation axis definition in a rotating domain. The coordinate frame set here has no influence on boundary conditions for the domain. For details, see Global Coordinate Frame (Coord 0) in the CFX-Solver Modeling Guide.
To define a fluid, particle or solid (including the solid portion of a porous domain):
If required, click Add new item
to the right of the definition list, type a name
for the definition and click . For multiphase
simulation, more than one fluid is required. For details, see Multiphase Flow Modeling in the CFX-Solver Modeling Guide.For the definition Option select
Material Library(the default) to enable choosing a material from a supplied or user defined library orMaterial Definitionfor Reacting Mixtures.For the definition Material select from the drop-down list for some commonly used materials or click Select from extended list
to access a complete list of materials.After clicking
you may also choose to select Import Library Data 
to load library data from a file.
The specification of material properties (for example, density and viscosity) and the creation of custom materials is performed in the Materials details view. For details, see Materials. New materials are added to the relevant drop-down list.
A solid domain must be made from a single solid material.
Which morphology options are available depends on whether you are setting fluid-specific details for an Eulerian phase or for a particle phase. For Eulerian phases, the options are:
Continuous FluidDispersed FluidDispersed SolidDroplets (Phase Change)Polydispersed Fluid
For details, see Morphology in the CFX-Solver Modeling Guide.
For a particle phase, the options are:
Particle Transport FluidParticle Transport Solid
For details, see Particle Morphology Options in the CFX-Solver Modeling Guide.
For Dispersed Fluid and Dispersed
Solid phases, a mean diameter is required. For details,
see Mean Diameter in the CFX-Solver Modeling Guide.
This is available for dispersed phases, but you will not usually need to set a value. For details, see Minimum Volume Fraction in the CFX-Solver Modeling Guide.
This is available for the Dispersed Fluid and Dispersed Solid phases. For details, see Maximum Packing in the CFX-Solver Modeling Guide.
This restitution coefficient setting holds a value from 0 to 1 that indicates the degree of elasticity of a collision between a pair of particles. For such a collision, the restitution coefficient is the ratio of separation speed to closing speed. This restitution coefficient setting is used only for the kinetic theory model. For details, see Kinetic Theory Models for Solids Pressure in the CFX-Solver Theory Guide.
This is available for particle phases. For details, see Particle Diameter Distribution in the CFX-Solver Modeling Guide.
This is available for particle phases. For details, see Particle Shape Factors in the CFX-Solver Modeling Guide.
This option is available when multiphase reactions have been
enabled with particle tracking. When Particle Diameter Change is selected choose either Mass Equivalent or Swelling Model.
Select a reference material from the list. Enter a Swelling Factor greater than or equal to zero; a value of zero indicates no swelling, and CEL expressions are permitted. For details, see Particle Diameter Change Due to Swelling in the CFX-Solver Modeling Guide.
To include particles in the domain, define a particle in Fluid and Particle Definitions..., select the particle material and select the Particle Transport Fluid or Particle Transport Solid option for Fluid and Particle Definitions... > <particle definition> > Morphology on the Basic Settings tab. For details, see Particle Transport Modeling in the CFX-Solver Modeling Guide.
The Domain Models settings are described next:
The GT-SUITE Domain Models settings are available if the simulation is set up to be coupled with GT-SUITE with turboshaft coupling enabled. For details, see Coupling CFX to an External Solver: GT-SUITE Coupling Simulations in the CFX-Solver Modeling Guide.
Domains can be set up to receive angular velocity from a GT-SUITE Turboshaft function, with the shaft speed coming from GT-SUITE.
As prerequisites:
There must be at least one GT-SUITE Model object listed in the Outline tree view under Simulation > Expressions, Functions and Variables > GT-SUITE Models. The corresponding GT-SUITE model must include a turboshaft.
There must be at least one GT-SUITE Turboshaft function listed in the Outline tree view under Simulation > Expressions, Functions and Variables > User Functions.
To have the domain receive input from GT-SUITE:
Select GT-SUITE Domain Models > Use GT-SUITE Coupling to enable coupling of the domain with GT-SUITE in a coupled simulation.
Under Use GT-SUITE Coupling, set GT-SUITE Setup > GT SUITE Model to the name of an existing GT-SUITE Model object intended to send shaft speed data to the domain.
Under Domain Models > Domain Motion, set Option to
GT-SUITE Couplingand set Turboshaft Name to the name of a GT-SUITE Turboshaft function that corresponds to the domain.
For details about using GT-SUITE with CFX, see Coupling CFX to an External Solver: GT-SUITE Coupling Simulations in the CFX-Solver Modeling Guide.
This sets the absolute pressure level to which all other relative pressure set in a simulation are measured. For details, see Setting a Reference Pressure in the CFX-Solver Modeling Guide.
For flows in which gravity is important, you should include the buoyancy term. Gravity components in the x, y and z directions should be entered; these are interpreted in the coordinate frame for the domain. For details, see Coordinate Frames in the CFX-Solver Modeling Guide.
There are two different buoyancy models in CFX: the one used depends upon the properties of the selected fluid(s). Depending on the types of fluid selected, a Buoyancy Reference Temperature and / or a Buoyancy Reference Density must be set. This is because different fluids use either the full or Boussinesq buoyancy model. In multiphase flows, the reference density can have a significant effect.
The Buoyancy Reference Location can be set automatically, or to a specific location with X/Y/Z coordinates. For details, see:
The available Domain Motion options depend on the type of domain, and are described in Table 13.1: Domain Motion Options:
Table 13.1: Domain Motion Options
|
Option |
Eligible Domain Types |
Description |
|---|---|---|
|
Stationary |
All domain types |
The domain remains stationary in the absolute frame of reference. |
|
Rotating |
All domain types |
The domain rotates with a specified angular velocity about the given axis. For fluid, porous, and solid domains, a Rotational Offset setting exists. For fluid and porous domains, an Alternate Rotation Model option exists. |
|
Speed and Direction |
Immersed solid domain |
The domain translates at the specified speed in the specified direction. The translation direction can be specified by Cartesian components, or by a coordinate axis. |
|
Specified Displacement |
Immersed solid domain |
The domain is displaced according to the specified Cartesian components. For example, you could use CEL expressions that are functions of time to move the domain. |
|
General Motion |
Immersed solid domain |
Specify a reference origin that is considered to be attached to the domain. Then specify a motion for that origin, and a rotation of the domain about that origin. The reference origin location is specified by the Reference Location settings. The motion of the reference origin is specified
by Origin Motion settings that are
similar to those for the Domain Motion options (other than The rotation of the domain about the reference origin is specified by the Body Rotation settings. |
|
Rigid Body Solution |
Immersed solid domain |
Specify a mass, moment of inertia, and various dynamics settings. The dynamics settings include external forces and torques, translational and rotational degrees of freedom, and gravity. All of these settings are analogous to the settings of the rigid body object, which is described in Rigid Bodies. Note that, unlike for a rigid body object, you cannot specify initialization values for the rigid body solution that applies to an immersed solid domain; these initialization values (such as angular velocity and angular acceleration) are effectively initialized with values of magnitude zero. For additional information on modeling rigid bodies, see Rigid Body Modeling in the CFX-Solver Modeling Guide. |
Details of some of the settings mentioned in Table 13.1: Domain Motion Options:
Angular Velocity: The angular velocity gives the rotation rate of the domain, which can be a function of time.
Axis Definition: The axis of rotation can be a coordinate axis of the local coordinate frame or a local cylindrical axis defined by two points.
If
Coordinate Axisis selected, the available axes are all local and global coordinate axes.Coord 0is the global coordinate frame, and its axes are referred to asGlobal X,Global YandGlobal Z. A local coordinate frame's axes are referred to asmyCoord.1,myCoord.2,myCoord.3where 1,2,3 represent the local X,Y,Z directions.If
Two Pointsis selected, Rotation Axis From and Rotation Axis To must be set. The points are interpreted in the coordinate frame for the domain. If the coordinate frame is cylindrical, then the components correspond to the r,
, z directions. For details, see Coordinate Frames in the CFX-Solver Modeling Guide.
Rotational Offset: This setting transforms the domain by the specified rotation angle. The rotation axis used for this transformation is specified by the Axis Definition settings.
Alternate Rotation Model: For details, see Alternate Rotation Model in the CFX-Solver Modeling Guide.
Reference Location: The reference location is an origin point that should be defined to conveniently describe the body rotation of the immersed solid domain. When Body Rotation > Option is set to
None, the reference location will be neglected. Specify the reference location by choosing an existing coordinate frame origin, or by specifying Cartesian coordinates.A solver run that starts from a previous run should have the same domain motion options in the immersed solids domains, and must have identical reference location specifications if supplied.
Origin Motion: The origin motion can be specified in any of the ways that the domain motion can be specified (not counting the
General Motionoption for domain motion), and bySpecified Velocity, which accepts Cartesian components of velocity.Body Rotation: The body rotation options are:
NoneRotatingSpecify an angular velocity and the instantaneous axis of rotation.
Specified Angular VelocityUse Cartesian components to define a vector. The rotation axis passes through the reference location in the direction of the specified vector. The angular velocity is the magnitude of the specified vector.
Note:
CEL expressions used to define domain motion can be functions of time only.
If you create two or more fluid domains and modify a model setting of one of the domains, that setting is generally copied to all other fluid domains in the simulation. An exception to this is that if you edit the Domain Motion settings of a domain, those settings are not copied to any other domains; this enables each domain to rotate or remain stationary independently of the other domains.
Mesh deformation can be used to model flows with varying geometry, for both transient and steady-state simulations. The following mesh deformation model options are available for a domain:
NoneRegions of Motion Specified: permits wall boundaries and subdomains to move, and makes mesh motion settings available. These include a mesh motion model option and mesh stiffness settings. For details, see Regions of Motion Specified in the CFX-Solver Modeling Guide.Periodic Regions of Motion: permits wall boundaries to move, and makes mesh motion settings available. These include a Periodic Model setting, a mesh motion model option and mesh stiffness settings. ThePeriodic Regions of Motionoption can save computational time compared to theRegions of Motion Specifiedoption by taking advantage of the nature of periodic motion and solving the mesh motion equations only at the start of the simulation. However, thePeriodic Regions of Motionmesh deformation model implementation uses a linear approximation and has some limitations compared to theRegions of Motion Specifiedoption. For details, see Periodic Regions of Motion in the CFX-Solver Modeling Guide.Junction Box Routine: reads mesh coordinate datasets from a file into the CFX-Solver as the solution proceeds. This step requires the specification of a series of meshes and User Fortran routine(s). For details, see Junction Box Routine in the CFX-Solver Modeling Guide.
For transient blade row cases, specify the number of passages in 360° and the number of passages per component for the domain. This information may be used in the automatic calculation of time step size, depending on the Transient Method settings (which are described in Transient Method).