The Fluid Values tab for a boundary condition object is used to set boundary conditions for each fluid in an Eulerian multiphase simulation and each particle material when particle tracking is modeled.
The Boundary Conditions list box contains the materials of the fluid passing through the boundary condition. Selecting a material from the list will create a frame with the name of the material and properties available to edit. These properties are detailed in the following sections.
Turbulence > Option can be set to any one of the following values. Unless otherwise specified, do not change any further turbulence settings.
Low (Intensity = 1%)Medium (Intensity = 5%)High (Intensity = 10%)Intensity and Length ScaleFor details, see Intensity and Length Scale.
Intensity and Eddy Viscosity RatioFor details, see Intensity and Eddy Viscosity Ratio.
k and EpsilonFor details, see k and Epsilon.
k and Omegak and Eddy Viscosity Ratiok and Length ScaleReynolds Stresses and EpsilonReynolds Stresses and OmegaReynolds Stresses and Eddy Viscosity RatioReynolds Stresses and Length ScaleDefault Intensity and Autocompute Length ScaleIntensity and Autocompute LengthFor details, see Intensity and Auto Compute Length.
Zero Gradient
Enter a numeric value or an expression for Value, and specify a value for the eddy length scale.
Enter a numeric value or an expression for Value, and specify a value for the eddy viscosity ratio.
Specify a turbulent kinetic energy value and a turbulent eddy dissipation value.
Volume Fraction > Option can be set to:
ValueIf set to
Value, you must enter a numeric value or an expression for the volume fraction for each fluid. Note that the total volume fractions of the fluids in the list box must be equal to 1.Zero GradientThe volume fraction can also be set to
Zero Gradient, which implies that the volume fraction gradient perpendicular to the boundary is zero. This setting can be useful for subcritical free surface flow when the free surface elevation is specified (via a pressure profile) at the outlet.
If Option is set to Static Temperature, you must specify a value for the static temperature.
Set the fluid velocity on the Boundary Details tab.
Select from the following:
Normal SpeedCartesian Velocity ComponentsMass Flow Rate
For details, see Mass and Momentum in the CFX-Solver Modeling Guide.
Set the static pressure on the Boundary Details tab.
Select from the following:
Normal to BoundaryDirectional Components
For details, see Mass and Momentum in the CFX-Solver Modeling Guide.
Set turbulence quantities at the inlet boundary (if applicable).
For details, see Turbulence in the CFX-Solver Modeling Guide.
Set the inlet temperature of each phase (if applicable).
For details, see Heat Transfer in the CFX-Solver Modeling Guide.
Enter the volume fraction of the selected fluid at the inlet.
The total volume fraction summed over all the fluids must be equal to 1.
If one of the fluids is a variable composition mixture, specify the mass fractions of each of the components.
For details, see Component Details: Opening.
When the fluid selected in the list box at the top of the Fluid Values tab has a morphology of Polydispersed
Fluid, size fractions must be specified for each of the
size groups. The size fractions can be set to Value or Automatic. All size fractions set to Automatic are calculated to have the same value such that
the overall sum of size fractions (including those that are specified
by value) is unity. If all size fractions are set to Value, you must ensure that the specified size fractions sum to unity.
Optionally, specify particle properties at the boundary.
When this check box is disabled, particles do not enter through this boundary.
For details, see Mass and Momentum in the CFX-Solver Modeling Guide.
For details, see Particle Position in the CFX-Solver Modeling Guide.
For details, see Particle Locations in the CFX-Solver Modeling Guide.
Select from Direct Specification or Proportional to Mass Flow Rate. For details, see Number of Positions in the CFX-Solver Modeling Guide.
For details, see Particle Mass Flow Rate in the CFX-Solver Modeling Guide.
For details, see Particle Diameter Distribution in the CFX-Solver Modeling Guide.
Available when heat transfer is selected. For details, see Heat Transfer in the CFX-Solver Modeling Guide.
Available when the particle phase has been set up as a variable composition mixture. For details, see Component Details in the CFX-Solver Modeling Guide.
If you are using the inhomogeneous multiphase model and have selected the Fluid Velocity option on the Boundary Details tab, the fluid-specific velocity information is set on the tab shown below at an outlet boundary.
Specify the Mass and Momentum as:
Normal SpeedCartesian Velocity ComponentsCylindrical Velocity ComponentsMass Flow Rate
For details, see Mass and Momentum in the CFX-Solver Modeling Guide.
This tab enables you to define particle behavior at walls. This is done by selecting a particle type from the list box and specifying its properties as outlined below:
Select a particle-wall interaction option - for details, see Settings for Particle-Wall Interaction.
Specify an erosion model - for details, see Erosion Model in the CFX-Solver Modeling Guide.
Specify a particle-rough wall model - for details see Particle-Rough Wall Model (Virtual Wall Model) in the CFX-Solver Modeling Guide.
Specify the amount of mass absorbed at a wall - for details, see Mass Flow Absorption in the CFX-Solver Modeling Guide.
Define the particle behavior - Select this option to control the entry of particles and to specify particle properties at wall boundaries. The settings for this option are similar to those available for inlets and openings. For details, see Particle Tracking Settings for Inlets and Openings.
The particle-wall interaction can be controlled by selecting one of the following Wall Interaction options:
Equation Dependent- This is the default option in Ansys CFX and requires the specification of the following Velocity settings:Restitution Coefficient- The droplet reflection at the wall can be controlled by specifying the values for Perpendicular Coefficient and Parallel Coefficient.The impact of droplet collision and the resulting momentum change across the collision can be described by specifying the perpendicular and parallel coefficients of restitution. For details, see Restitution Coefficients for Particles in the CFX-Solver Modeling Guide.
Minimum Impact Angle - Select this check box if you want to specify the minimum impact angle. Below this impact angle, particles will be stopped with the fate
Sliding along walls.
Wall Film- When Wall Interaction is set toWall Film, then the following Wall Film Interaction models can be selected:Stick to Wall- This model enforces all particles that hit a wall to become part of the wall film. This option does not require any further settings.Elsaesser- This model requires the specification of Wall Material.User Defined- The settings for this option are similar to those described for User Wall Interaction.
For details on various wall interaction options, see Wall Interaction in the CFX-Solver Modeling Guide.
User Wall Interaction - This option is available when a Particle User Routine has been created. For details, refer to the following sections:
For additional modeling information on particle transport, see Particle Transport Modeling in the CFX-Solver Modeling Guide.
The Fluid Values tab is available on the fluid side of a fluid-solid interface for an inhomogeneous multiphase setup.
When you are using the inhomogeneous multiphase model, you must use a no-slip wall or set a wall velocity. For details, see Mass and Momentum in the CFX-Solver Modeling Guide.
When particle transport is selected, additional settings are available. These contain the same options as those that appear for wall boundaries. For details, refer to the following sections:
Particles are introduced into the domain from this boundary. For details, see Fluid Values for Inlets and Openings.