Boundary value settings depend on characteristics of the flow. For instance, temperature is required at a boundary only if heat transfer is being modeled.
If you are changing the characteristics of the flow, ensure that boundary conditions are correctly updated. In most cases, CFX-Pre alerts you of the need to update settings in the form of physics validation errors. For details, see Physics Message Window.
Example:
Suppose a domain is created, isothermal flow is specified, and an inlet boundary condition set. If flow characteristics are then altered to include heat transfer, the inlet specification must be changed to include the temperature of the fluid at that location.
More information on some of the settings is available:
Various settings are available on the Boundary Details tab, depending on the type of boundary condition:
Option can be set to one of Subsonic, Supersonic, or Mixed.
For details, refer to the following sections:
The option for Mesh Motion is set to Stationary by default. For details, see Mesh Deformation in the CFX-Solver Modeling Guide.
First, specify the flow regime option. For details, refer to the following sections:
For details, see Mass and Momentum in the CFX-Solver Modeling Guide.
This option appears when Average Static Pressure is selected under Mass and Momentum. For details,
see Average Static Pressure in the CFX-Solver Modeling Guide.
For details, see Thermal Radiation in the CFX-Solver Modeling Guide.
The option for Mesh Motion is set to Stationary by default. For details, see Mesh Deformation in the CFX-Solver Modeling Guide.
For details, see Mass and Momentum in the CFX-Solver Modeling Guide.
This option appears when a flow direction is required; that
is, when one of Opening Pres. and Dirn. or Static Pres. and Dirn. is selected under Mass
and Momentum. For details, see Flow Direction in the CFX-Solver Modeling Guide.
For details, see Loss Coefficient in the CFX-Solver Modeling Guide
For details, see Turbulence in the CFX-Solver Modeling Guide.
For details, see Heat Transfer in the CFX-Solver Modeling Guide.
This is the same as specifying thermal radiation at an inlet. For details, see Thermal Radiation in the CFX-Solver Modeling Guide.
The Component Details section appears when a variable composition/reacting mixture has been created for a single phase simulation, or a simulation with one continuous phase and particle tracking.
The mass fractions must sum to unity on all boundaries. With
this in mind, highlight the materials you want to modify and enter
the mass fraction. To enter an expression for the mass fraction, click Enter Expression 
and enter the name of your expression.
The option for Mesh Motion is set to Stationary by default. For details, see Mesh Deformation in the CFX-Solver Modeling Guide.
The Wall Boiling Model > Option setting is described in Using a Wall Boiling Model in the CFX-Solver Modeling Guide.
For details on the wall boiling model, see Wall Boiling Model in the CFX-Solver Modeling Guide.
Option can be set to one of No
Slip Wall, Free Slip Wall, Finite Slip Wall, Specified Shear, Counter-rotating Wall, Rotating
Wall or Fluid Dependent. For details,
see Mass and Momentum in the CFX-Solver Modeling Guide.
The Slip Model settings apply for finite slip walls.
The only available option is Power Law.
You must provide the nominal slip speed (Us
), the critical stress (
), the slip power (m), the pressure
coefficient (B), and the normalizing stress (
).
For details about the finite slip wall model, see Finite Slip Wall in the CFX-Solver Modeling Guide.
The Shear Stress settings apply for walls with specified shear.
You specify the shear stress value directly, using a vector that points tangentially to the wall. The normal component of the vector that you specify is ignored.
The Wall Velocity settings apply for no slip walls, and walls with finite slip.
The Wall Velocity Relative To option can
be used to set the wall velocity relative to either the Boundary Frame or Mesh Motion occurring
on the boundary. You can select only the Boundary Frame option if the wall mesh motion is set to either Unspecified, Parallel to Boundary or Surface
of Revolution. For details about no slip wall velocity,
see No Slip Wall in the CFX-Solver Modeling Guide.
If Wall Velocity > Option is set to Cartesian Components, you must specify
the velocity in the X, Y, and Z axis directions. Similarly, if you
choose Cylindrical Components then values are
required for Axial Component, Radial
Component, and Theta Component.
You can specify a counter rotating wall. For details, see Counter-rotating Wall in the CFX-Solver Modeling Guide.
Specifying a Rotating Wall requires an
angular velocity and, if the domain is stationary, an axis definition. For details, see Rotating Wall in the CFX-Solver Modeling Guide.
For details, see Wall Roughness in the CFX-Solver Modeling Guide.
If the boundary is for a domain that involves solid motion, then the Solid Motion > Boundary Advection option may be available. If the velocity for the solid motion (specified in the Boundary Details tab for the domain) is directed into the domain everywhere on a boundary, and if you specify a fixed temperature or a fixed value of an Additional Variable on that boundary, then you should consider turning on the Boundary Advection option.
If you have specified a fixed temperature, then turning on the Boundary Advection option causes the advection of thermal energy into the solid domain at a rate that is consistent with the velocity normal to the boundary, the specified fixed temperature, and the material properties.
If you have specified a fixed value for an Additional Variable, then turning on the Boundary Advection option causes the advection of that Additional Variable into the solid domain at a rate that is in accordance with the velocity normal to the boundary, the specified fixed value of the Additional Variable, and, for mass-specific Additional Variables, the density of the solid material.
For a boundary where the solid is moving out of the domain, consider turning on the Boundary Advection option in order to allow thermal energy and Additional Variables to be advected out.
For details on setting up the solid motion model for a domain, see Solid Motion. For details on Additional Variables, see Additional Variables.
For details, see Heat Transfer in the CFX-Solver Modeling Guide.
For details, see Wall Contact Model in the CFX-Solver Modeling Guide.
For details, see Thermal Radiation in the CFX-Solver Modeling Guide.
The option for Mesh Motion is set to Stationary by default. For details, see Mesh Motion in the CFX-Solver Modeling Guide.
Only Mesh Motion can be set in this tab
for Symmetry boundary conditions. The option for Mesh Motion is set to Unspecified by default. For details,
see Mesh Deformation in the CFX-Solver Modeling Guide.
The options for Mass and Momentum, Turbulence, Heat transfer, Mesh Motion, and Additional Variables are set to Conservative Interface Flux by default.
Important:
Conservative Interface Flux implies that
the quantity in question will "flow" between the current
boundary and the boundary on the other side of the interface. This
means that Conservative Interface Flux must also
be used on the boundary on the other side of the interface. Accordingly,
the CFX-Solver will not be able to handle cases where Conservative
Interface Flux is set on just one side of the interface,
or where the quantity being transferred does not exist on the other
side. CFX-Pre will issue a warning if either of these cases exist.
For details on Nonoverlap Conditions, refer to Non-overlap Boundary Conditions.
When mesh deformation is selected for the domain that contains a boundary condition, mesh motion can be specified for the boundary on the Boundary Details tab.
The available options are:
Conservative Interface FluxUnspecifiedStationarySpecified DisplacementSpecified LocationPeriodic DisplacementParallel to BoundarySurface of RevolutionRigid Body Solution
For details on these options, see Mesh Motion Options in the CFX-Solver Modeling Guide.
For details on mesh deformation, see Mesh Deformation in the CFX-Solver Modeling Guide.
See Mesh Deformation for information about activating mesh deformation for the domain.
When an electric field model is activated for a domain that contains a boundary condition, Electric Field can be specified for a boundary from the Boundary Details tab.
The available options are:
Voltage
Ground
Flux In
Zero Flux
Electrical Current Transfer Coefficient
Conservative Interface Flux
Electric Field Contact Resistance
For details, see Electric Field in the CFX-Solver Modeling Guide.
For information about activating an electric field model for a domain, see Electromagnetic Model.