When Inlet boundaries are present, use the Inlet Editor panel to define
the conditions of the gas at the inlet. For automatic meshing cases, the Inlet icon bar offers 4
icons for managing inlets: Rename
, Copy
, Paste
, and Delete
. You can create a new inlet by copying and pasting an existing one or by
using the New Inlet
icon on the Boundary Conditions icon bar. However, for body-fitted cases
the presence of the inlet(s) is determined by the mesh flags upon import of the mesh, such that
you cannot create new ones within the Simulation interface. For body-fitted mesh projects, then,
only the Rename option is available here.
Options on the Inlet Editor panel include:
Note: If you have a DISPERSED material defined in your chemistry set, and you have selected Moment Method for the Soot model option, and you want to define the presence of particles in the inlet, you will need the options on the Surface Composition and the Dispersed Phase Editor panels. Otherwise they usually are not present.
Composition: You need to specify the fluid species' composition at the inlet boundary. Use the Mixture Editor
to specify the details of the composition. See Mixture Editor for details. Select whether to specify
the inlet’s species composition in Mass Fraction or Mole
Fraction, and then use the Add Species button to select
species that are present in the inlet fluid mixture (see Figure 2.12: Specifying gas species composition for an inlet). In the resulting table, specify the
associated fractions (in the units selected) for each species. Note that if you have table
data with the same layout and species order, you can use cut/paste to enter the data in this
table. When all the species data are entered, you can optionally use the
Normalize button to assure that the resulting species composition sums to
1.0.Location: Select the location of the inlet in the location list.
Note: By default, surfaces included in the same open boundary condition are required to be contiguous, but including non-contiguous surfaces in the same open boundary is supported as long as these surfaces are connected to the same region. To disable the contiguity check, go to Edit Preferences > General Settings > Validation Settings and check the box Skip Open Surface Contiguity Check.
Inlet Options: Select from the list of inlet types: Static Pressure, Total Pressure, Velocity, or Mass Flow Rate, and any of these can be constant or Time Varying. Time Varying options can include a time-frame offset (see Time Frames). If you select Static Pressure or Total Pressure, the boundary type is regarded as Pressure Inlet. It is different from the Velocity Inlet or the Mass Flow Rate Inlet in their treatment of pressure and flow velocity at the boundary.
At a Pressure Inlet, pressure is specified by the user, and flow velocity is calculated by the flow solver based on the pressure difference across the boundary. The user must provide a constant value of the pressure, or a pressure profile (as a function of time or crank angle) if the pressure is Time Varying. In the Time Varying case, if the pressure profile is based on crank angle, you can select the Repeat Profile Each Cycle option to shift the crank angle in the profile to fit within 0-360 (for 2-stroke) or 0-720 (for 4-stroke) degrees. The adjusted pressure profile will then be treated as cyclic and repeated on a 720-degree schedule (4-stroke) or 360-degree schedule (2-stroke). You may choose to Use Global Crank Angle Limits to impose a global crank angle range for the cyclic repetition of the pressure profile. If the Repeat Profile Each Cycle option is not selected, then the crank angle provided in the pressure profile will not be converted to cyclic. A time-based pressure profile should be used in time-based simulation, and the profile can also be treated as cyclic. See Profile Editor for a detailed description of how to define the cyclic feature of the profile.
If Velocity Inlet or Mass Flow Rate Inlet is selected, the flow velocity/Mass Flow Rate's magnitude and direction must be provided and there are options for specifying Inflow Mixture Density. In this case, pressure only affects the thermodynamic state of the inlet fluid and does not directly affect the flow velocity. For low-speed flows, you can use the default Assume Zero Pressure Gradient. This option assumes the pressure of the inflow mixture is equal to the pressure in the nearest fluid cell inside the domain, and that the inflow pressure is used to compute inflow mixture density. For high-speed (supersonic) flows, the zero-pressure-gradient assumption is no longer suitable, and you can either specify the inflow density directly or specify an inflow pressure, which in turn is used to compute the inflow density. Both the density and pressure can be specified as either static or total.
If Mass Flow Rate Inlet is selected, the user-provided mass flow rate will be used to derive the inlet velocity magnitude using the following formula:
in which
is the velocity magnitude normal to the inlet boundary, 
is the mass flow rate, 
is the density of the inflow mixture, and 
is the total area of the inlet. The inflow density is determined based on
the interior fluid cells adjacent to the inlet boundary. The direction of inflow velocity
can be specified either as Normal to Boundary,
Vector, or Axisymmetric Vector. The
latter two options can also be specified as time-varyying profiles. See Profile Editor for a detailed description of how to specify a vector
profile or an axisymmetric vector profile. If a vector profile is used, the velocity
direction vectors will not be interpolated between tabulated points, instead, the profile
will be treated as a staircase function.
Turbulence: Select from the list a method for indicating inlet turbulence kinetic energy (TKE) and TKE dissipation rate; using the pull-down list, and then specify the corresponding parameter values and units where appropriate. Specification options include:
The above options allow you to specify absolute values for the TKE and TKE Dissipation rates or to use the relative values of Turbulent Intensity and Turbulent Length Scale. Turbulence Intensity is a dimensionless measure of the turbulent kinetic energy and is defined such that:
Temperature Option: You need select the option to determine the fluid temperature at the inlet boundary. You may choose to specify the temperature directly as a Static value, or Total Temperature, either of which can be constant or Time Varying. Time Varying options can include a time-frame offset (see Time Frames). Otherwise, you may specify the temperature behavior as Assume Isentropic. In this case, a reference state (density, pressure, specific heat ratio) will be picked at the beginning of the calculation based on the state in the neighboring region. During the calculation, the actual inflow temperature is calculated by assuming the mixture has gone through an isentropic compression/expansion process starting from the reference state.
If you have a DISPERSED material defined in your chemistry set, and you have selected Moment Method for the Soot model option, and you want to define the presence of particles in the inlet, the following options are of interest:
Surface Composition: Use the Solid Phase Editor
to specify the details of the surface composition. If no solid phase
exists in the mechanism, this property can remain unspecified. If the surface composition is
not specified, then the dispersed-phase composition at the inlet is assumed to be zero. See
Solid Phase Editor and Dispersed Phase Editor for Particle Tracking for details. Use
the Add Species button to select species that are present in the inlet
dispersed surface phase.Dispersed Phase: Use the Solid Phase Editor
to specify the details of the dispersed phase. See Solid Phase Editor and Dispersed Phase Editor for Particle Tracking for details. If no solid phase exists
in the mechanism, then this property can remain unspecified. If the dispersed phase is left
unset, then the dispersed phase composition at the inlet is assumed to be zero.