(

The following discussion briefly highlights some key items associated with using the unstructured flow solver in Wind-US.

For structured grids,
GMAN
provides some minimalistic grid generation options and
*cfcnvt*
can convert from some standard file formats. However, Wind-US
does not provide any grid-generation software for constructing or
converting unstructured meshes. Users should check with their
favorite grid-generation software to determine if it supports the
Wind-US format. In some software, the Wind output option is for
structured grids while Wind-US is for unstructured grids.

While the NPARC Alliance does not endorse any particular grid
generation *software*, several recommendations on grid
generation *strategy* have emerged from testing the
unstructured grid solver in Wind-US and from instruction provided
from our development partners at the Boeing Company. While one of
the motivations of using unstructured grids is potentially less
time-consuming grid generation for difficult geometries, this does
not mean that less care can be applied in generating high quality
meshes. For viscous flow problems, it is recommended that a layer
of prismatic or hexahedral cells be used in near wall regions.
It is not recommended that tetrahedra be used to pack important
boundary layer regions.

Away from walls, where tetrahedra are perhaps more appropriately used,
*isotropic* tetrahedra are preferable. High levels of skewness
and overly rapid grid stretching may adversely affect both the
convergence characteristics of the solver, as well as the accuracy
of a final converged solution. Shear layers away from walls
(such as in jet flows) also require special care. It is yet to be
determined whether hexahedral, prismatic, or tetrahedral cells are
optimal in such regions.

Wind-US does not support two-dimensional or axisymmetric
*unstructured* grids. To model such configurations, a planar
grid may be extruded via translation or rotation to form a
three-dimensional mesh that is at least one cell wide.
Also note that the unstructured solver does not accept
collapsed faces, so special care may be needed when
using rotational extrusion about a singularity axis.
To simulate an axisymmetric geometry, only a fraction
(i.e., five degrees) of the circumferential direction
need be modeled. See the discussion of
Mass Flow and Grid Areas
for additional details.

For viscous flow simulations, it is highly recommended that the
*cfpart*
utility be used with the `CREATELINES` keyword to generate
line groupings for use with the Gauss-Seidel line implicit
solver in Wind-US. Please note that the Gauss-Seidel line
solver is *not* the default option, and must be activated via the
`IMPLICIT UGAUSS LINE`
keyword.

Not all of the physical models in Wind-US are available in both the structured and unstructured solvers. The user documentation clearly indicates differences in keyword applicability and syntax.

Turbulence modeling is one area that falls into this category. For most turbulent flow problems, the currently recommended models for use with the unstructured solver are the Menter SST two-equation model and the Spalart-Allmaras one-equation model, which are also available in the structured solver. Through Wind-US validation activities, the performance of these two turbulence models has been found to be very similar in the structured and unstructured solvers. The Goldgerg Pointwise model, the Realizable k-epsilon model, and the Shih k-epsilon model are also available for unstructured grids.

The same finite rate chemistry capability in the structured solver is available in the unstructured solver, but has not been as thoroughly validated. Please report any issues with stability, convergence, and/or accuracy.

The default settings for the unstructured solver are in many cases
different from those for the structured grid solver. Some of these
differences are as follows:

**Structured Grids**

IMPLICIT BOUNDARY OFFIMPLICIT SCALAR (for Euler calculations)IMPLICIT FULL (for viscous calculations)RHS VISCOUS VISCOUS VISCOUS VISCOUS (i.e., Full)RHS ROE SECOND PHYSICALTVD MINMODFIXER OFFGRID LIMITER OFF |

IMPLICIT BOUNDARY ON (including implicit coupling) IMPLICIT UGAUSS EXACT_LHS VISCOUS_JACOBIAN FULL SUBITERATIONS 6RHS VISCOUS THIN-LAYERRHS HLLE SECONDTVD BARTH 3.0FIXER AVERAGEGRID LIMITER ANGLE 150Q LIMIT PRESSUREMIN 0.01 PRESSUREMAX 250 DENSITY 0.01 DENSITYMAX 250GRADIENTS LEAST_SQUARES |

Note that the `Q LIMIT` default is good for transonic problems,
but may need to be modified for high Mach number flows or those with
vastly differing pressures. Limited experience with expanding the range
of the `Q LIMIT` values has not shown any stability problems.
Also note that the default implicit solver is the `UGAUSS`
point implicit solver, but that `UGAUSS LINE` is preferred for
viscous simulations. Further, for flows with dominant free shear layers,
large separated flow zones, or mixing regions, `RHS VISCOUS FULL`
should be used.

To assist convergence rate, an adjustable CFL number may be activated
by using a keyword sequence as shown below, with a minimum starting
CFL number and a target maximum CFL number. Depending on the behavior
of the solution, the actual CFL number employed by the solver will
adjust, increasing the CFL number for well-behaved solutions, and
decreasing it when needed for solution stability:

`CFL AUTO DECREASE 2 CFLMAX 500 CFLMIN 1.0`

As with grid generation, the NPARC Alliance does not endorse any particular post-processing software package. File readers that are compatible with the unstructured grid capability are available for some plotting packages. Anyone wishing to know the current status of the available readers or willing to supply additional readers or plugins is encouraged to contact the NPARC Support Team (nparc-support@arnold.af.mil).

Users should note that post-processing an unstructured solution is
inherently different than that for structured grids due to the
nature of unstructured grids. For example, the CFPOST
`SUBSET`
command which is designed to work across specific ordered computational
lines in structured grid format, has no meaning for unstructured
grids. The CFPOST
`CUT`
command can be used to make cuts along specific surfaces to
extract flowfield data. Likewise, the
`RAKE`
command can be used
to specify interpolation locations. Named
surface groups
can also be used to simplify the post-processing task.

The Wind-US `LOADS`
keyword can be used to write integral properties to the list output
(*.lis*) file at regular intervals. These values can then be
extracted using the
*resplt* utility.
The CFPOST
`INTEGRATE FLUX` or
`INTEGRATE FORCE`
commands can also be used to compute integral values for a given
solution file.

During a Wind-US run, users can also output additional variables
to the solution (*.cfl*) file using the
`WRITE VARIABLES` keyword.

The Wind-US user documentation has been updated to reflect the large number of changes that affect the unstructured solver. The validation website has also been updated with a number of unstructured test cases, which may be a good source of detailed examples on how to effectively use the unstructured solver for a broad range of flow problems. Questions about the use of NPARC Alliance software may be addressed to the NPARCtalk mailing list or forwarded to the NPARC Support Team via email (nparc-support@arnold.af.mil).

Last updated 1 Apr 2016