Information about general NRBCs is provided in the following sections.
The general non-reflecting boundary conditions in ANSYS Fluent are
based on characteristic wave relations derived from the Euler equations.
In the density-based solver, the non-reflecting boundary conditions
are applied only on pressure-outlet boundary conditions. In the pressure-based
solver they are applied on pressure-inlet, pressure-outlet, velocity-inlet
and mass-flux boundary conditions. To obtain the primitive flow quantities
(), reformulated Euler equations are solved on the
boundary of the domain in an algorithm similar to the flow equations
applied to the interior of the domain.
Unlike the turbo-specific NRBC, the general NRBC method is not restricted by geometric constraints or mesh type. However, good cell skewness near the boundaries where the NRBCs can be applied for better convergence.
Note the following restrictions and limitations on the general NRBCs:
The general NRBC is not available if the target mass flow rate is activated in the pressure-outlet dialog box.
The general NRBC using the density-based solver is available only with compressible flow while using the ideal-gas law.
Important: The general NRBC using the density-based solver should not be used with the wet steam or real gas models.
The general NRBCs using the density-based solver are not compatible with species transport and mixture fraction transport models (for premixed and partially-premixed models). They are mainly used to solve ideal-gas single-component flow.
The general NRBCs using the pressure-based solver are not compatible with steady-state cases, all multiphase models, and compressible liquids models.
General NRBCs are derived by first recasting the Euler equations
in an orthogonal coordinate system () such that
one of the coordinates,
, is normal
to the boundary Figure 6.66: The Local Orthogonal Coordinate System onto which Euler Equations
are Recasted for the General NRBC Method. The
characteristic analysis [123] [124] is then used to modify terms corresponding
to waves propagating in the
normal direction.
When doing so, a system of equations can be written to describe the
wave propagation as follows:
(6–182) |
Where ,
and
and
,
and
are the velocity
components in the coordinate system (
,
,
). The equations
above are solved on non-reflecting boundaries, along with the interior
governing flow equations, using similar time stepping algorithms to
obtain the values of the primitive flow variables (
).
Important: Note that a transformation between the local orthogonal coordinate
system (,
,
) and the global
Cartesian system (X, Y, Z) must be defined on each face on the boundary
to obtain the velocity components (
,
,
) in a global Cartesian system.
Figure 6.66: The Local Orthogonal Coordinate System onto which Euler Equations are Recasted for the General NRBC Method

The terms in the transformed Euler
equations contain the outgoing and incoming characteristic wave amplitudes,
, and are defined
as follows:
(6–183) |
From characteristic analyses, the wave amplitudes, , are given
by:
(6–184) |
The outgoing and incoming characteristic waves are associated
with the characteristic velocities of the system (i.e eigenvalues), ,
as seen in Figure 6.67: Waves Leaving and Entering a Boundary Face on Inflow and Outflow
Boundaries. The Wave Amplitudes are Shown with the Associated Eigenvalues
for a Subsonic Flow Condition. These eigenvalues
are given by:
(6–185) |
Figure 6.67: Waves Leaving and Entering a Boundary Face on Inflow and Outflow Boundaries. The Wave Amplitudes are Shown with the Associated Eigenvalues for a Subsonic Flow Condition

For subsonic flow leaving a boundary, four waves leave the domain
(associated with positive eigenvalues ,
,
, and
) and one enters
the domain (associated with negative eigenvalue
). For subsonic flow entering a boundary, four waves
enter the domain (associated with the negative eigenvalues
,
,
,
) and one leaves the domain (associated with a positive
eigenvalue
).
To solve Equation 6–182 on a boundary,
the amplitude of the incoming and outgoing waves must be first determined.
The amplitude of outgoing waves are computed from Equation 6–184 by using extrapolated values
of flow derivatives ,
,
,
, and
from inside the domain.
The amplitude of the incoming waves are computed as follows. The amplitude
of waves
,
, for tangential velocity components, is set to zero.
The amplitude of the incoming pressure and entropy waves are computed
from the Linear Relaxation Method (LRM) of Poinsot [85] [86]. The
LRM method sets the value of the incoming wave amplitude to be proportional
to the differences between the local primitive variable on a boundary
face and the imposed boundary value. The expression for the amplitudes
depends on the boundary type as shown below:
Pressure Outlet
(6–186) |
where is the imposed pressure at the exit boundary,
is the relaxation factor,
and
is the local pressure value at the boundary.
In general, the desirable average pressure on a non-reflecting boundary can be either relaxed toward a pressure value at infinity or enforced to be equivalent to some desired pressure at the exit of the boundary.
In the case of a backflow, the pressure-based solver has two options for specifying pressure at the boundary; static pressure or total pressure. If the static pressure option is selected, the pressure at infinity is equal to the pressure defined in the boundary dialog box. If the total pressure option is selected, the pressure at infinity is a total pressure that is computed from the value in the dialog box. For the density-based solver, the total pressure option is used and no other options are available.
If you want the average pressure at the
boundary to relax toward at infinity (that is
), the suggested
factor is given by:
(6–187) |
where is the acoustic speed,
is the domain size,
is the maximum Mach number in the domain, and
is the under-relaxation factor (default value is
0.15). On the other hand, if the desired average pressure at the boundary
is to approach a specific imposed value at the boundary, then the
factor is given by:
(6–188) |
where the default value for is 5.0
Important: The desired average pressure option is only available for the density-based solver.
Pressure Inlet:
(6–189) |
where the imposed pressure, , and density,
, are computed from the specified total pressure
and total temperature.
Mass Flux Boundary:
(6–190) |
where the imposed exit velocity and density are computed from specific mass flux and total temperature.
Velocity Inlet:
(6–191) |
where the imposed velocity, , is specified at the boundary and the imposed
density is computed from the specified boundary temperature and extrapolated
pressure.
The general NRBC is available for use in the Pressure Outlet dialog box when either the density-based (with ideal gas law) or pressure-based solvers are activated to solve for compressible flows. The general NRBC is available for use in the Pressure Inlet, Mass-Flow Inlet, and Velocity Inlet dialog boxes when the pressure-based solver is activated to solve for compressible flows.
The example below shows you how to enable the general NRBC in the Pressure Outlet dialog box. You would follow similar steps for the other boundary condition types mentioned above.
Select pressure-outlet from the Boundary Conditions task page and click the button.
In the Pressure Outlet dialog box, choose Non Reflecting under Acoustic Wave Model.
For the density-based solver, select one of the two Exit Pressure Specification options: Pressure at Infinity or Average Boundary Pressure. The pressure-based solver uses the Pressure at Infinity option and the Exit Pressure Specification drop-down list is not available.
The Pressure at Infinity boundary
is typically used in unsteady calculations or when the exit pressure
value is imposed at infinity. The boundary is designed so that the
pressure at the boundary relaxes toward the imposed pressure at infinity.
The speed at which this relaxation takes place is controlled by the
parameter, sigma, which can be adjusted in
the TUI:
define → boundary-conditions → non-reflecting-bc → general-nrbc → set
In the set/ submenu, you can set the sigma value. The
default value for sigma is 0.15.
The Average Boundary Pressure specification
is usually used in steady-state calculations when you want to force
the average pressure on the boundary to approach the exit pressure
value. The matching of average exit pressure to the imposed average
pressure is controlled by the parameter sigma2 which can be adjusted in the TUI:
define → boundary-conditions → non-reflecting-bc → general-nrbc → set
In the set/ submenu, you can set the sigma2 value. The default value for sigma2 is
5.0.
Important: There is no guarantee that the sigma2 value of 5.0 will force the average boundary pressure to match the
specified exit pressure in all flow situations. In the case where
the desired average boundary pressure has not been achieved, you can
intervene to adjust the sigma2 value so that
the desired average pressure on the boundary is approached.
For the pressure-based solver, you can select one of two Backflow Pressure Specification options: Static Pressure or Total Pressure. For the density-based solver, the Backflow Pressure Specification is not shown and the Total Pressure option is used by default. Note that backflow is not allowed for pressure inlets, mass-flow inlets, or velocity inlets.
Important: For the pressure-based solver, you should choose Direction Vector or From Neighboring Cell as the Backflow Direction Specification Method if the flow is tangential to the boundary. You should not select the Normal to the Boundary option for Backflow Direction Specification Method in this case because the face velocity components for this case will be computed from flux as zero during initialization. This initialization will cause the solver convergence to fail.
Usually, the solver can operate at higher CFL values without the NRBCs being turned on. Therefore, the best practice is to first achieve a good stable solution (not necessarily converged) before activating the non-reflecting boundary condition. In many flow situations, the CFL value must be reduced from the normal operation to keep the solution stable. This is particularly true with the density-based implicit solver since the boundary update is done in an explicit manner. A typical CFL value in the density-based implicit solver, with the NRBC activated, is 2.0 and 4.0 in the pressure-based solver.