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.]:
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
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
Viscous flow is computed when the
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,
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
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
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
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 lbm/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., imax connecting to i1 as in an O-grid) in a point-match manner. The boundary condition simply averages the flow variables from both sides of the boundary and assigns the average to the two boundaries. This condition was formerly used for polar-type grids in duct flowfields. Note: For best results, one should consider using the coupled boundary condition instead of self-closing.
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"
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