(

- Explicit and Implicit Boundary Conditions
- Boundary Condition Types
- Wall Boundary Conditions
- Flow Interface Boundary Conditions
- Grid Topology Boundary Conditions
- Zonal Interface Boundary Conditions
- Miscellaneous Boundary Conditions

The boundary conditions are perhaps the most important factor in influencing the accuracy of the flow computation. The manner in which the boundary conditions are imposed also influences the convergence properties of the solution. Wind-US uses a cell-vertex discretization, which results in solution points located on the boundaries of the zones which comprise the flow domain. During the computation, Wind-US computes the boundary values for the conservative variables, the species (if present), and turbulence variables (if present).

Proper specification of the flow boundary conditions is aided by a basic understanding of characteristic theory of the incoming and outgoing waves normal to the boundary. The boundary normal is considered positive when it points into the flow domain. The wave speeds (eigenvalues) have convective and acoustic components. A positive wave speed indicates a wave entering the flow domain, and so, a physical boundary condition must be specified and some auxiliary information must be supplied to impose the boundary condition. A negative eigenvalue indicates a wave leaving the flow domain, and so, a numerical boundary condition can be specified using flow data within the domain. The waves moving tangential to the boundary are neglected in the boundary condition treatment.

Wind-US imposes the boundary conditions explicitly after the interior solution has been computed for each zone after each iteration, by default. An exception is the zone interface boundaries, which are updated after each cycle. Another exception is the mass flow boundary condition, which is updated after a specified number of iterations (the default is five iterations) in order to reduce computational effort. Errors due to explicit boundary conditions are reduced through the use of the multi-stage or iterative time integration methods.

The use of implicit boundary conditions with an implicit solver is known to
improve the stability of the method and lead to faster convergence at the
expense of greater computational effort and complexity.
Implicit boundary conditions are available in Wind-US in a limited manner,
primarily for wall boundary conditions.
The `IMPLICIT BOUNDARY`
keyword is used to turn on implicit boundary conditions.

*Keywords:* `IMPLICIT BOUNDARY`

The Grid MANipulation (GMAN) program is used to associate boundary condition
types with the solution points on the boundaries of the zones.
These boundaries represent the geometry model, fluid boundaries,
grid topological boundaries, and couplings between zones.
The type of boundary conditions available in GMAN, in the order
displayed by GMAN, include:
[In this User's Guide, GMAN boundary condition types are indicated by
lower-case words in a fixed-pitch font, `like this`; Wind-US keywords are
displayed in an upper-case fixed-pitch font, `LIKE THIS`.]:

`undefined``reflection``freestream``viscous wall``arbitrary inflow``outflow``inviscid wall``self-closing``singular axis``coupled``bleed``pinwheel axis``frozen``chimera`

It is possible to group some of these boundary condition types in a logical manner for detailed discussions, which are presented below. Some boundary conditions require further information, which is provided through keywords in the input data file, beyond being flagged in GMAN.

The `inviscid wall`,
`viscous wall`, and
`bleed`
boundary condition types are all wall boundary conditions which simulate
interaction of the flow with a real or imaginary solid surface.

The `inviscid wall` boundary condition imposes flow tangency at the
zone boundary (wall surface) while maintaining the same total velocity as
the point adjacent to the boundary.
One numerical boundary condition is imposed by computing the pressure
at the boundary through an interpolation of interior pressures.
A zero-order extrapolation is robust; however, the
pressures may not be smoothly varying at the boundary.
A first-order extrapolation works well for flows without discontinuity,
and for flows in which the pressure does not vary greatly normal to
the boundary.
The extrapolations across a discontinuity may result in nonphysical pressures.
One can use the `viscous wall`
boundary condition along with the
`TURBULENCE INVISCID`
keyword in the input data file.
This is useful if one wants to start a computation with the boundary as
inviscid and then later turn on the viscous boundary conditions.
In Wind-US, it is also possible to specify through
`TEST 138` that the normal
pressure gradient at the wall be
calculated rather than simply assuming it to be zero.
Also, a first-order extrapolation which accounts for grid spacing can be
used through the use of
`TEST 141`.

The `viscous wall` boundary condition imposes a no-slip condition of the
flow, a zero pressure gradient, and the appropriate heat transfer condition
(adiabatic or constant temperature) at the zone boundary (wall surface).
The no-slip condition can involve a non-zero velocity if the wall is moving.
(See the `MOVING WALL`
and `ROLL` keywords;
however, for moving walls, the boundary condition type should be set to
`bleed`.)
To minimize transients at the start of a Wind-US calculation, the
velocity at no-slip boundaries is actually reduced from its initial
value to the no-slip condition over a number of iterations.
The number of iterations may be specified using the
`WALL SLIP` keyword.

The choice of the heat transfer condition is determined through the use
of the `WALL TEMPERATURE`
keyword in the input data file.
The default is an adiabatic wall (zero temperature gradient).
The temperature for the constant temperature condition is specified
through the `WALL TEMPERATURE` keyword.
The `TTSPEC`
keyword is available for specifying a
point-by-point distribution of surface temperatures.

Wall function boundary conditions may be used at viscous walls, using the
White-Christoph law of the wall, through the
`WALL FUNCTION` keyword.
This feature is currently available for single-species flows only.

In Wind-US, it is also possible to specify through
`TEST 138`
that the normal pressure gradient at the wall be calculated rather
than simply assuming it to be zero.
Also, a first-order extrapolation which accounts for grid spacing can
be used through the use of
`TEST 141`.
Viscous flow is computed when the
`TURBULENCE`
keyword is used.

*Keywords:* `
MOVING WALL,
TTSPEC,
TURBULENCE,
WALL FUNCTION,
WALL SLIP,
WALL TEMPERATURE
`

The `bleed` boundary condition allows mass to flow through a porous,
viscous wall.
Bleed is mass flow out of the flow domain, while blowing is
mass flow into the flow domain.
Bleed and blowing systems are often an
integral part of aeropropulsion configuration design, helping to control
such flow phenomena as boundary layer growth and mixing.
Wind-US's bleed/blowing boundary condition was designed to provide a
means to model these systems with CFD.
Specification of the `bleed` boundary condition in GMAN, which involves
the identification of a particular bleed region number, triggers the
calculation of the area of the bleed region specified, which is then
stored in the grid file.
Wind-US uses this area and the bleed or blowing conditions specified in the
input data file to compute a normal velocity on the model surface.
Bleed may be specified as a mass flow, or as a porous surface
with a discharge coefficient and back pressure.
Blowing may be specified through mass flow, plenum, or valve conditions.

*Keywords:* `
BLEED,
BLOW
`

The `moving wall` boundary condition enables a tangential velocity to be
applied at no-slip walls in order to model rotating hubs or other components
in the flow.
The boundary solution points for the moving wall should be identified as
`bleed` regions in GMAN.
The translating or spinning motion of the wall is specified through the
`MOVING WALL`
keyword in the input data file.
The `ROLL` keyword allows
a rolling motion to be imposed on the grid.

*Keywords:* `
MOVING WALL,
ROLL
`

The `freestream`,
`arbitrary inflow`, and
`outflow` boundary condition types
form a group involving the simulation of the interaction of the flow
with other flow conditions at the domain boundaries.

The `freestream` boundary condition is intended for use
at freestream outer boundaries.
This boundary condition uses one-dimensional characteristic theory
to set boundary flowfield variables from freestream or flowfield
conditions, based on the flow direction at the boundary.

At freestream boundaries with inflow, the
`HOLD`
keyword may be used to specify whether total conditions or
characteristic values are to be held constant.
Total pressure is held constant in both cases, and
may result in initial Mach numbers being altered.

For some cases, this boundary condition may also be used at
unconfined outflow boundaries, but the
`outflow`
boundary condition
is generally recommended instead.
In particular, experience has shown that using the `freestream`
condition at outflow boundaries with a shear layer exiting the
computational domain may result in very slow convergence,
and the solution may not be very accurate.
There may also be the possibility of a mixed boundary, such as a
supersonic outflow with a small subsonic region in the wall boundary layer.
In this case, the pressure in the supersonic region is extrapolated to
the boundary from upstream, but the pressure in the subsonic region is
set from the freestream value.
This may cause a small disturbance at the boundary,
which can be corrected by specifying the boundary as an
`outflow`
boundary and imposing a constant pressure for the entire boundary.

*Keywords:* `
FREESTREAM,
HOLD,
EXTRAPOLATE
`

The `arbitrary inflow` boundary condition allows conditions to be
specified on regions of zonal boundaries where flow is entering the zone.
Such a capability may be required to describe a thermally stratified
nozzle input flow, or a jet emanating from a wall.
The inflow profile may be specified in a number of different ways:
as uniform flow, as a point-by-point (*xyz*) profile, or as
uniform flow over a range of grid indices.
The `ARBITRARY INFLOW` keyword
is used in the input data file to indicate desired flow properties.

*Keywords:* `
ARBITRARY INFLOW,
EXTRAPOLATE
`

The `outflow` boundary condition may be used for
internal flows at
boundaries where subsonic flow is leaving the computational domain, such as
at the exit plane of an inlet, diffuser, or auxiliary flow duct.
It is also recommended for downstream outflow boundaries in external flow
problems, especially if a shear layer is exiting the computational domain.

Characteristic theory indicates that only one physical condition is required to define the boundary condition. One may know one of the following at the outflow boundary: mass flow, exit pressure, or exit Mach number.

The mass flow (in lb_{m}/sec) may be specified at the
outflow boundary (see the
`MASS FLOW` keyword).
The mass flow may be the actual or corrected value.
One may alternatively specify the ratio of the desired mass flow to
the mass flow through the inflow capture area specified in GMAN.
During the solution, the mass flow boundary condition is applied every
five iterations by default, which reduces computational costs.
The integrated mass flow is compared with the desired value.
If the `PRESSURE` option is used with the
`MASS FLOW` keyword,
a spatially-constant pressure is set at the outflow boundary, and modified
as the solution proceeds until the desired mass flow is achieved.
If the `DIRECT` option is used, the momentum, and thus the mass
flow, is modified directly, and the pressure adjusts as the solution
proceeds.
For the `PRESSURE` option, Wind-US displays the ratio between the
computational and desired mass flows and the modified pressure at each
application of the boundary condition.
If you experience difficulty in converging the mass flow, you should
consider setting a constant back pressure at the duct exit.

A constant exit pressure may also be specified (see the
`DOWNSTREAM PRESSURE` keyword)
at the outflow boundary.
This option results in a very reflective boundary condition, which may
cause difficulties in convergence of the solution, especially for
internal flows.
One alternative is to allow the exit pressure to vary spatially according
to the distribution of the solution points adjacent to the boundary.
This option is selected through the `VARIABLE` option of the
`DOWNSTREAM PRESSURE` keyword.
The `UNSTEADY` option of the
`DOWNSTREAM PRESSURE` keyword
may be used to specify either a sinusoidal or user-defined pressure
oscillation at an outflow boundary.

The mass-averaged Mach number may be specified at the outflow boundary using
the `DOWNSTREAM MACH` keyword.
This boundary condition is identical to the Chung-Cole compressor face
boundary condition discussed below.
It simulates the uniform Mach number characteristics
that have been observed experimentally at compressor faces.
This boundary condition also corresponds to a fairly uniform mass flux
through the outflow boundary.

The compressor face models of
Chung and Cole
[Chung, J., and Cole, G. L. (1996)
"Comparison of Compressor Face Boundary Conditions for Unsteady
CFD Simulations of Supersonic Inlets," NASA TM-107194]
and of
Mayer and Paynter
[Mayer, D. W. and Paynter, G. C. (1994)
"Boundary Conditions for Unsteady Supersonic Inlet Analyses,"
AIAA Journal, Vol. 32, No. 6, pp. 1200-1206]
are also available at outflow boundaries, through the
`COMPRESSOR FACE`
keyword.
Both models are based on the observation that turbine engine conditions set
the corrected mass flow, and that this corresponds directly to the
average Mach number at the compressor face.
These boundary conditions have been implemented mainly for the analysis
of unsteady flow; however, they have also been shown to be robust
for the establishment of steady-state, supercritical inlet flows.

The computational grid at the outflow boundary should be such that it is
modeled with a single computational plane (constant *i*, *j*, or
*k*) in a single zone.
If two zones merge together near the exit, one should create a small
exit zone to accommodate the outflow boundary condition.

*Keywords:* `
COMPRESSOR FACE,
DOWNSTREAM MACH,
DOWNSTREAM PRESSURE,
MASS FLOW
`

The
`reflection`,
`self-closing`,
`singular axis`, and
`pinwheel axis` types of boundary conditions
form a group involving the simulation of the flow at topological surfaces
in the grid.

The `reflection` boundary condition simulates a plane of symmetry,
and is the same as a solid, slip wall boundary condition.
Therefore, within Wind-US, the `inviscid wall`
boundary condition is actually applied.
The `reflection` boundary condition type does provide a descriptive
label for the boundary solution points, which may be of use to several
auxiliary CFD codes which generate or use reflected grids.

The `self-closing` boundary condition can be used at boundaries for
which grid lines connect end-to-end (e.g., *i _{max}*
connecting to

The `singular axis` boundary condition is imposed at locations where an
entire or part of a zonal boundary has collapsed to a line
(*not a point*).
Thus, along the other boundary direction, the grid points are coincident.
The singular grid point is evaluated by taking the distance-weighted average
of the solution of the adjacent grid points encircling the axis.
This boundary condition is not to be used when the singularity line
collapses to a point.
For partially singular boundaries, the average is computed only
over the singular portion of the boundary.
Excessive use of this boundary condition is not recommended since flow
conservation is not preserved.
One should attempt to use non-singular grids whenever possible.
`TEST 118`
allows the choice of which variables are averaged.
`TEST 150`
can be used to explicitly set certain velocity
components to zero when the singular axis occurs on symmetry planes.
`TEST 199`
excludes the last grid point on the singular axis from being averaged.

The `pinwheel axis` boundary condition is used when there exists
multiple singularities at various locations on boundaries.
This boundary condition does not zero any velocity components - it
simply takes the average.
`TEST 118`
allows the choice of which variables are averaged.
`TEST 165`
allows input of the integer for the order of
magnitude of the tolerance for singularity
(the default is 10^{−8}).

The
`coupled` and
`chimera` boundary condition types
involve the interactions between zones of the domain.
Periodic boundaries are available as a type of `coupled` boundary
condition.

The `coupled` boundary condition is imposed at regions where zones
connect.
Zone coupling is the name of the process by which Wind-US transfers
flowfield information from one zone to another across conterminous
computational grid boundaries.
This process uses geometric interpolation factors stored in the grid file,
which have been previously computed in the GMAN program.
The zone interfaces occur at the boundaries of the zones, and so
are imposed as boundary conditions at the end of each cycle of the
computation.

The zone coupling algorithm that will be used depends on the explicit
differencing operator specified by the
`RHS` keyword.
For most of the higher-order operators, the default zone coupling
algorithm is a high-order method based on Roe's flux-difference
splitting scheme, including the passing of gradients between zones.
The `COUPLING` keyword
allows one to specify low-order Roe coupling, without passing gradients,
or (for structured grids) a coupling algorithm based on one-dimensional
characteristic theory.

Zone boundaries should be treated the same as you would treat interior grid planes; there should not be any large changes in grid stretching or orthogonality at the boundary. In addition, zone boundaries should not be placed in regions of strong flowfield gradients, especially horizontally along jet shear layers or aligned with normal shocks. In other words, use your best engineering judgment in placing zone boundaries in your solution.

Periodic boundaries are treated as normal coupled boundaries, with the
connection data stored in the common grid (*.cgd*) file when
setting boundary conditions with GMAN.
See the `PERIODIC` "keyword"
for details.

*Keywords:* `
COUPLING,
PERIODIC
`

The `chimera` boundary condition indicates that the zone boundary is in
an overlap region.

The
`undefined` and
`frozen` boundary condition types
are included in this section, mostly because they don't fit well
in any other section, and are fairly self-explanatory.

The default boundary condition type in GMAN is `undefined`.
If not set to another boundary condition type, the boundary solution point
is evaluated as an average of local solution points.
In practice, one should specify the actual boundary condition type for all
boundary solution points and avoid having undefined boundary solution points.

If all the points on a boundary surface have an undefined boundary
condition, an error message is printed and the solution will abort.
If only some points have an undefined boundary condition, a warning
message is printed and the solution will continue.
`TEST 75`
will force the code to stop instead.

The `frozen` boundary condition simply signals a boundary solution point
to retain its value as read in from the initial solution file.

Last updated 1 Apr 2016