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.Keywords: TURBULENCE
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:
IMPLICIT BOUNDARY OFF|
IMPLICIT SCALAR (for Euler calculations)
IMPLICIT FULL (for viscous calculations)
RHS VISCOUS VISCOUS VISCOUS VISCOUS (i.e., Full)
RHS ROE SECOND PHYSICAL
GRID LIMITER OFF
IMPLICIT BOUNDARY ON (including implicit coupling) |
IMPLICIT UGAUSS EXACT_LHS VISCOUS_JACOBIAN FULL SUBITERATIONS 6
RHS VISCOUS THIN-LAYER
RHS HLLE SECOND
TVD BARTH 3.0
GRID LIMITER ANGLE 150
Q LIMIT PRESSUREMIN 0.01 PRESSUREMAX 250 DENSITY 0.01 DENSITYMAX 250
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 (firstname.lastname@example.org).
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 (email@example.com).
Last updated 1 Apr 2016