__CONTENTS__

- 2D Cases
- Flat Plate (steady)
- Flat Plate with Grid Skew Effect (steady; demonstration of effect of grid skewing)
- Flat Plate with Min Y+ Effect (steady; demonstration of effect of different minimum wall spacing)
- Backward Facing Step (steady; patched grids)
- Transonic Diffuser (steady)
- NACA 4412 Airfoil (steady; point-match and overset grids)
- RAE 2822 Airfoil (steady; derivatives with respect to alpha)
- Supersonic Ramp (steady; inviscid; embedded grids)
- Circular Cylinder (unsteady; demonstration of temporal accuracy)
- NACA 0012 Airfoil (steady; demonstration of spatial accuracy)
- Ejector Nozzle Jet (steady; point-match grid)
- Sinusoidally Pitching Airfoil (unsteady; demonstration of moving grid capability)
- Rotor-Stator Simulation (unsteady; demonstration of sliding patched interface capability)
- Wall-Mounted Hump Model (unsteady; demonstration of flow control through time-dependent BCs)
- Curved Wall (demonstration of curvature correction model SARC)
- 3D Cases
- Axisymmetric Bump (steady; "2.5D")
- ONERA M6 Wing (steady)
- ARA M100 Wing-Body (steady; point-match grid)
- ARA M100 Wing-Body (steady; overset grid)
- Delta Wing (steady; demonstration of CGNS capability)
- Test Information

All test cases are available for downloading as Unix compressed tar files containing grid, input, and auxiliary files. Note that the files for the 3D cases can be quite large.

- Description:
- Download tar file Flatplate.tar.Z (76 kB)
**gunzip Flatplate.tar.Z****tar -xvf Flatplate.tar**- The tar file contains the following items:
**grdflat5.fmt**- single-block grid (cfl3d type, formatted) of dimensions j x k x i = 65 x 97 x 2
**grdflat5.inp**- cfl3d input file; total pressure, temperature and Mach number
set at inflow, using the SST turbulence model. Results for the
other turbulence models shown below can be obtained by simply
changing ivisc(k) to the appropriate value, e.g.
ivisc(k) = 5 for SA and ivisc(k) = 14 for EASM-ko. (Note:
for two equation models on this case, one
should add the keyword
**edvislim 100000.**to avoid possible convergence problems during the initial part of the run.) **split.inp_1blk**- input to block splitter that converts the single-block formatted grid to a single block unformatted grid that can be read by CFL3D
- To run the flat plate case, type:
- Expected Results:
- Comparison with theoretical results:
- Notes:
- Note that the EASM-ko was re-calibrated in 9/2002. Use of ivisc=14 in versions prior to V6.1 will not agree with the results given here.

Subsonic flow past a semi-infinite flat plate is modeled at Reynolds number 6 million per unit length. Inflow is set by specifying total pressure, total temperature, and Mach number. Results using using SA, SST, and EASM-ko turbulence models (#5, #7, and #14) are compared with theoretical data found one of the standard fluid mechanics references (White, "Viscous Fluid Flow," 1974). The following figures illustrate the case:

Then type:

This will create a subdirectory "Flatplate".

Case | Plots | Theory |
---|---|---|

SST, SA and EASM-ko |
Cf vs x u+ vs y+ |
Theoretical data contained within postprocessing programs |

FORTRAN program 1 (cf vs x) FORTRAN program 2 (u+ vs y+) |

The FORTRAN programs will extract the computed results from the printout (cfl3d.prout) and plot3d (plot3dg.bin and plot3dq.bin) files generated by CFL3D. The output files are formatted TECPLOT files, which should be easily adapted to other plotting packages as well.

__FLAT PLATE WITH GRID SKEW EFFECT__

- Description:
- Download tar file Flatplateskew.tar.Z (246 kB)
**gunzip Flatplateskew.tar.Z****tar -xvf Flatplateskew.tar**- The tar file contains the following items:
**grdflat5.fmt**,**grdflat5_skew15.fmt**,**grdflat5_skew30.fmt**,**grdflat5_skew45.fmt**- single-block grids (cfl3d type, formatted) of dimensions j x k x i = 65 x 97 x 2
**grdflat5_noskew.inp**,**grdflat5_15.inp**,**grdflat5_30.inp**,**grdflat5_45.inp**- cfl3d input files; total pressure, temperature and Mach number set at inflow, using the SA turbulence model. To avoid finite-trailing-edge effects, the total drag for this case is integrated only over the range 0 < x < 0.8333.
**split.inpnoskew**,**split.inp15**,**split.inp30**,**split.inp45**- inputs to block splitter that convert the single-block formatted grids to single block unformatted grids that can be read by CFL3D
- To run the flat plate case, type:
- Expected Results:
- Comparisons of results on the different grids:
- Notes:
- If you try to switch the turbulence model and run, for example, with
SST, it may be necessary to limit the maximum eddy viscosity by
employing the keyword
**edvislim**and setting it to, say, 100000.

Subsonic flow past a semi-infinite flat plate is modeled at Reynolds number 6 million per unit length. This is essentially the same as the previous flat plate case, except here the effect of grid skewness on the solution is demonstrated. The SA turbulence model is employed on 4 different grids with varying amounts of skewness. The following figure illustrates the case:

Then type:

This will create a subdirectory "Flatplateskew".

(Note: each run should be done independently, i.e., finish one before starting another if running in the same directory, and remember to save results between each run as needed.)

Case | No. Processors | Run Time | Memory | Convergence History | Test Date | Test Machine |
---|---|---|---|---|---|---|

Normal grid | 1 | 13 min | 13.9 MB |
cfl3d.res plot |
July 21 04 | Linux Workstation^{6} |

15-deg skew grid | 1 | 13 min | 13.9 MB |
cfl3d.res plot |
July 21 04 | Linux Workstation^{6} |

30-deg skew grid | 1 | 13 min | 13.9 MB |
cfl3d.res plot |
July 21 04 | Linux Workstation^{6} |

45-deg skew grid | 1 | 13 min | 13.9 MB |
cfl3d.res plot |
July 21 04 | Linux Workstation^{6} |

Comparative results are shown in terms of
skin friction coefficient,
velocity profile, and
drag coefficient.
It is shown that there is some impact from skewed grids,
but the influence is very small (up to 45-deg skew).
The drag coefficient plot also shows
the effect of grid density for this case: this integrated quantity is
converging to a solution of approximately 0.003175 on an
infinite grid. The spatial convergence rate is approximately 2nd order
(the variation is nearly linear plotted against 1/gridpoints, which is
proportional to Delta(h)^{2}. The error from an extrapolated
infinite grid is approximately 0.4% on the 65 x 97 grid, 1.8% on the
33 x 49 grid, and 6.8% on the 17 x 25 grid.

- Description:
- Download tar file Flatplateyplus.tar.gz (62 kB)
**gunzip Flatplateyplus.tar.gz****tar -xvf Flatplateyplus.tar**- The tar file contains the following items:
**grid_y+.02.fmt**,**grid_y+.23.fmt**,**grid_y+.51.fmt**,**grid_y+1.15.fmt**,**grid_y+2.3.fmt**,**grid_y+4.6.fmt**- single-block grids (plot3d type, formatted) of dimensions i x j x k = 2 x 65 x 97
**grid_y+.02sa.inp**,**grid_y+.23sa.inp**,**grid_y+.51sa.inp**,**grid_y+1.15sa.inp**,**grid_y+2.3sa.inp**,**grid_y+4.6sa.inp**,**grid_y+.02sst.inp**,**grid_y+.23sst.inp**,**grid_y+.51sst.inp**,**grid_y+1.15sst.inp**,**grid_y+2.3sst.inp**,**grid_y+4.6sst.inp**- cfl3d input files for SA and SST; here the total drag is integrated over the entire range 0 < x < 1
**splity+.02.inp**,**splity+.23.inp**,**splity+.51.inp**,**splity+1.15.inp**,**splity+2.3.inp**,**splity+4.6.inp**- inputs to block splitter that convert the single-block formatted grids to single block unformatted grids that can be read by CFL3D
- To run the flat plate case, type:
- Expected Results:
- Comparisons of results on the different grids:
- Notes:
- The wall normal grid stretching was stopped for these grids when the aspect ratio of the cells exceeded 1.
- The y+ values given here are approximate averages. Clearly, the y+ at each location on the plate
will vary. CFL3D computes the min, max, and
average y+ values for turbulent computations, and
these statistics are always output to the bottom of the
**cfl3d.out**standard output file. More detailed numbers (such as the y+ value at each wall location) can be output to the**cfl3d.prout**auxiliary file. - Although the new capability (as of V6.4) of full Navier-Stokes (
**ifullns**=1) was run for these cases, it has almost no influence on the results, as expected.

Subsonic flow past a semi-infinite flat plate is modeled at Reynolds number 6 million per unit length. This is similar to the previous two flat plate cases, except here the effect of changing the grid minimum spacing at the wall is demonstrated. The SA and SST turbulence models are employed on 6 different grids with varying minimum wall spacings (all grids are 65 x 97 in size). Unlike the previous flat plate cases, this case is also slightly different in that it (a) uses Riemann farfield-type BC at the inflow rather than setting total conditions, (b) solves using the new feature of FULL NAVIER-STOKES rather than thin-layer, and (c) uses constant temperature wall (set at the freestream total temperature), rather than using adiabatic wall.

Then type:

This will create a subdirectory "Flatplateyplus".

(Note: each run should be done independently, i.e., finish one before starting another if running in the same directory, and remember to save results between each run as needed.)

Case | No. Processors | Run Time | Memory | Convergence History | Test Date | Test Machine |
---|---|---|---|---|---|---|

SA, y+=0.02 | 1 | 6 min | 13.9 MB |
cfl3d.res plot |
Feb 28 07 | Linux Workstation^{7} |

SA, y+=0.23 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation^{7} |

SA, y+=0.51 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation^{7} |

SA, y+=1.15 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation^{7} |

SA, y+=2.3 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation^{7} |

SA, y+=4.6 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation^{7} |

SST, y+=0.02 | 1 | 6 min | 13.9 MB |
cfl3d.res plot |
Feb 28 07 | Linux Workstation^{7} |

SST, y+=0.23 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation^{7} |

SST, y+=0.51 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation^{7} |

SST, y+=1.15 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation^{7} |

SST, y+=2.3 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation^{7} |

SST, y+=4.6 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation^{7} |

Comparative results are shown in terms of drag coefficient and skin friction coefficient. (Recall that for the flat plate, all the drag is due to skin friction.) It is shown that the SST model is more sensitive to minimum wall grid spacing on a given grid size than the SA model (this is a well-known result; see, e.g., Bardina et al, NASA TM-110446, 1997). This greater sensitivity is likely related to the particular implementation of the wall boundary condition on omega. Currently, CFL3D uses the same approximate omega boundary condition as Bardina et al., as recommended by Menter (NASA TM 103975, 1992). Generally, when running turbulent computations, it is preferable to have a grid with minimum y+ spacing of no more than approximately 1 at walls. For the SA model for this case, the drag on the grid with y+ of about 1.15 is different from the result on the y+=0.02 grid by less than 1%. For the SST model, the difference is about 3.8%.

Further insight can be obtained by looking at the results not only on the finest grids (65 x 97), but also from the coarser grid levels. These results were obtained during the mesh sequencing operation during the run. Figures are shown in terms of 3-grid drag coefficient for SA and 3-grid drag coefficient for SST.

For SA, the drag coefficient generally decreases as the grid is refined (as 1/grdpts approaches 0). The lowest slope for this decrease occurs for the family of grids derived from the fine grid with y+=0.02, but there is not much difference between the three families of grids: y+=0.02, 0.23, and 0.51. For the family of grids with larger y+, the variation is greater (although all grid families tend toward the same answer on an infinitely refined grid). This SA result is a demonstration that supports the commonly held truism that one should use grids with y+ levels less than 1 (unless employing wall functions). Such a use will yield greater accuracy (in skin friction) on a given grid level. Note, however, that when these grids were created, the farfield extent of the grids was kept approximately the same. As a result, the grid stretching in the wall normal direction for each of the grids is different (approximately 1.2295, 1.18, 1.17, 1.151, 1.1377, and 1.128 for y+=0.02 through 4.6, respectively). Thus, the grid with the finest wall normal spacing also has the largest stretching factor. It is possible that very large stretching factors may negatively influence the code's accuracy, so use of y+ values that are "too small" may end up having negative consequences.

For SST, the picture is not as clear. Here, the greater sensitivity of the model to minimum y+ can be seen. (Recall that this greater sensitivity is likely due to the approximate wall boundary condition on omega.) On the 3 grids with the smallest fine-grid y+ (0.02, 0.2, and 0.51), the results generally tend toward a similar infinitely-refined result, although it appears that a finer grid level than 65 x 97 would be needed to better demonstrate asymptotic convergence. For the grids whose fine level has a y+ greater than 1, the results appear less consistent. Here it is unclear whether additional finer grid levels would yield consistent results or not. In any case, this study clearly demonstrates the need to use grids with y+ less than 1 for the SST model.

- Description:
- Download tar file Backstep.tar.gz (123 kB)
**gunzip Backstep.tar.gz****tar -xvf Backstep.tar**- The tar file contains the following items:
**step_grdgen.fmt**- 2 block patched grid (plot3d type, formatted)

block 1 dimensions i x j x k = 2 x 25 x 65

block 2 dimensions i x j x k = 2 x 129 x 113 **step_grdgen.inp**- CFL3D input file; an inflow velocity profile upstream of the step is set using bc type 2008. The profile is set for the Menter SST model.
**bc2008.data**- data file that CFL3D reads to set the inflow profile (valid for SST or Wilcox k-omega models only)
**ron_step_grdgen.inp**- RONNIE (patched grid preprocessor) input file
**split.inp_1blk**- input to block splitter that converts the single-block formatted grid to a single block unformatted grid that can be read by CFL3D
- To run the backward facing step case, type:
- Expected Results:
- Comparison with experimental data:
- Notes:

Subsonic flow past a backward-facing step is modeled. A velocity profile is specified at the inflow plane via a BC data file. This case employs patched grids that must be pre-processed with the "ronnie" grid patching code provided as part of the cfl3d package. The experimental data is taken from Driver, AIAA J., Vol 23 No 2, 1985, pp. 163-171. The following figures illustrate the case:

Then type:

This will create a subdirectory "Backstep".

Case | Plots | Exp. data |
---|---|---|

SST |
Cf vs x Cp vs x |
cflower.exp.dat cplower.exp.dat |

FORTRAN program |

The FORTRAN programs will extract the computed results from the printout (cfl3d.prout) file generated by CFL3D. The output files are formatted TECPLOT files, which should be easily adapted to other plotting packages as well.

- Description:
- Download tar file Transdiff.tar.Z (77 kB)
**gunzip Transdiff.tar.Z****tar -xvf Transdiff.tar**- The tar file contains the following items:
**transdiff_p3d.fmt**- single-block grid (plot3d, multigrid, whole, formatted) of dimensions i x j x k = 2 x 81 x 53
**cfl3d.inp_ws**- cfl3d input file; exit pressure set for the weak-shock case and the Spalart-Allmaras turbulence model. Results for the EASM-ko turbulence model shown below can be obtained by simply changing ivisc(k) to 14.
**cfl3d.inp_ss**- cfl3d input file; exit pressure set for the strong-shock case and the Spalart-Allmaras turbulence model. Results for the EASM-ko turbulence model shown below can be obtained by simply changing ivisc(k) to 14.
**split.inp_1blk**- input to block splitter that converts the single-block formatted grid to a single block unformatted grid that can be read by CFL3D
- To run the weak-shock and strong-shock cases, type:
- Expected Results:
- Comparison with experimental data:
- Notes:
- For this internal flow case, the difference in mass flow between inlet and exit is monitored as a convergence criterion (in addition to residual). This is achieved by setting ihstry=1 and specifying control surfaces at the inlet and outlet.
- If you try to run with a two-equation
model, it may be necessary to limit the maximum eddy viscosity by
employing the keyword
**edvislim**and setting it to, say, 100000.

Transonic flow through a converging diverging diffuser is modeled. Varying the exit pressure leads to different shock positions and strengths. Two exit-static-pressure to inlet-total-pressure ratios are considered, giving a weak shock and a strong shock condition, the latter of which results in separated flow on the top wall of the diffuser. Results using the "workhorse" Spalart-Allmaras turbulence model and a non-linear k-w EASM model are plotted with the experimental data. A complete description of this case can be found in the NPARC Alliance Validation Archive. The following figures illustrate the case:

Then type:

This will create a subdirectory "Transdiff".

(Note: each run should be done independently, i.e., finish one before
starting another if running in the same directory, and remember to save
results between each run as needed.)

Case | No. Processors | Run Time | Memory | Convergence History | Test Date | Test Machine |
---|---|---|---|---|---|---|

Weak Shock, SA | 1 | 5 min | 6.8 MB |
cfl3d.res plot |
March 21 03 | Octane2^{5} |

Weak Shock, EASM-ko | 1 | 5 min | 7.2 MB | cfl3d.res | March 21 03 | Octane2^{5} |

Strong Shock, SA | 1 | 2.3 min | 6.8 MB |
cfl3d.res plot |
September 9 03 | Linux Workstation^{6} |

Strong Shock, EASM-ko | 1 | 2.5 min | 7.2 MB | cfl3d.res | September 9 03 | Linux Workstation^{6} |

Case | Plots | Exp. Data |
---|---|---|

Weak Shock |
P vs x Velocity Profiles |
sajwpres.data sajwvel.data |

Strong Shock |
P vs x Velocity Profiles |
sajspres.data sajsvel.data |

FORTRAN program |

The FORTRAN program will extract the computed
results from the plot3d files generated
by CFL3D (with **nplot3d = -1**) and the experimental
data files. The output is a formatted TECPLOT file, which should
be easily adapted to other plotting packages as well.

- Description:
- Standard Grid
- Mach Contours,Standard Grid
- Chimera Grid using Pegsus
- Mach Contours, Chimera Grid using Pegsus
- Chimera Grid using Maggie
- Mach Contours, Chimera Grid using Maggie
- Download tar file NACA_4412.tar.Z (887 kB)
**gunzip NACA_4412.tar.Z****tar -xvf NACA_4412.tar**- The tar file contains the following items:
**4412_standard.fmt**- 1-block "standard" grid (plot3d, multigrid, whole, formatted)

block 1 dimensions i x j x k = 2 x 257 x 81

**4412_xmera.fmt**- 3-block "chimera" grid (plot3d, multigrid, whole, formatted)

block 1 dimensions i x j x k = 2 x 225 x 57

block 2 dimensions i x j x k = 2 x 113 x 73

block 3 dimensions i x j x k = 2 x 49 x 113

**cfl3d.inp_standard**- cfl3d input file for standard-grid case
**cfl3d.inp_xmera**- cfl3d input file for chimera-grid case
**split.inp_standard**- input to block splitter that converts 4412_standard.fmt to an unformatted grid that can be read by CFL3D
**split.inp_xmera**- input to block splitter that converts 4412_xmera.fmt to an unformatted grid that can be read by CFL3D
**peg41.inp**- input to PEGSUS
**4.1**that generates the overset grid connectivity file "XINTOUT". The conversion tool p3d_to_INGRID can be used to convert the formatted grid-point file into the unformatted cell-center file "INGRID" file that is input to PEGSUS. The conversion tool XINTOUT_to_ovrlp can be used to convert the output file from PEGSUS to the "ovrlp.bin" file required by CFL3D for the chimera-grid case **maggie.inp**- input to MAGGIE that generates overset grid connectivity file "ovrlp.bin" required by CFL3D for the chimera-grid case
**mag1.h**- parameter file for MAGGIE; must be placed in the cfl3dv6/header directory before compiling MAGGIE
- To run the standard-grid case, type:
- To run the overset-grid case using MAGGIE to generate the overset connectivity file, copy mag1.h to the header directory and compile MAGGIE. Then type:
- To run the overset-grid case using PEGSUS to generate the
overset connectivity file, compile PEGSUS as appropriate (in the
instructions below, it is assumed the PEGSUS executable is called
pegsus41). You will also need a couple of utilities from the cfl3d tools
directory, so make sure you have compiled cfl3d_tools. Then type:
(user inputs shown in
**bold**, interactive prompts for input shown in*italics*) - Expected Results:
- Comparison with experimental data:
- Notes:
- The overset-grid case is run using a W-cycle (as is the standard grid case); this type of multigrid cycle does not always work for overset grids (V-cycle is recommended in the Version 5 User's Manual).
- Mesh sequencing cannot be used with overset grids in CFL3D; in order to have a direct comparison with the overset-grid case, the standard-grid case is also run without mesh sequencing, contrary to recommended practice.
- When comparing timings, note that the overset grid contains roughly 26,000 cells compared to the standard grid with roughly 20,500 cells.
- The provided MAGGIE and PEGSUS input files were set up to provide resulting hole and outer boundaries as nearly identical as possible. The resulting solutions are very similar; therefore, only the Chimera results using Pegsus interpolation stencils are given in the tables (except for the MAGGIE residual history file).
- Both the spelling and the case used for the zone names when generating the INGRID file is important - they must match those in the PEGSUS input file.
- If you try to switch turbulence model, to run with a two-equation
model, it may be necessary to limit the maximum eddy viscosity by
employing the keyword
**edvislim**and setting it to, say, 100000.

Flow around an NACA airfoil section is computed using a "standard" body fitted C-grid as well as with "chimera" overset grids, using the SA turbulence model. For the overset case, the standard grid is used near the airfoil, with two nesting "box" grids providing connection to the far field. In both cases, the outer boundary is located at nominally the same distance away from the airfoil. However, the shapes of the outer boundaries differ between the two cases. Input files are provided for generating the overset connectivity data using either MAGGIE (provided as part of the CFL3D release package) of the widely-used PEGSUS code. The experimental data is taken from Coles and Wadcock, AIAA J., Vol 17 No 4, 1979, pp. 321-329. The following figures illustrate the case:

Then type:

This will create a subdirectory "NACA_4412".

file defaults:input grid files are plot3d typeinput grid files are unformattedoutput INGRID/plot3d file is unformatteddo you wish to use these defaults (y/n)?(alternate options include formattedfiles and cfl3d-type input grid files)ychoose the type of output file to createenter 0 to create an INGRID file (for PEGSUS 4.x)enter 1 to create a plot3d file (for PEGSUS 5.x)0enter the name of the output file to create (up to 80 char.)INGRIDenter 0 to create an output file with grid pointsenter 1 to create an output file with augmented cell centers1enter 0 to preserve input-grid i,j,k index definitions in the output gridyou may want this option if you have an existing PEGSUS input file thatwas generated for OVERFLOWNote: this will require the following translation ofindicies between CFL3D and PEGSUS input files:PEGSUS CFL3DJ = IK = JL = Kenter 1 to swap input-grid i,j,k index definitions in the output gridNote: this will require NO translation ofindicies between CFL3D and PEGSUS input files:PEGSUS CFL3DL = IJ = JK = K1enter number of separate grid files to convert into one output file1enter 0 to specify a name for each meshenter 1 to use default names (grid.n)0beginning processing of grid file number 1input name of unformatted plot3d grid file to read (up to 80 characters)4412_xmera.unfenter 0 if a single-grid plot3d fileenter 1 if a multiple-grid plot3d file1required array sizes: maxbl = 3lmax = 4jmax = 226kmax = 114input name (up to 40 char.) for zone 1wingreading zone 1input dimensions 2 225 57writing zone 1 with name wingoutput dimensions 226 58 4input name (up to 40 char.) for zone 2box1reading zone 2input dimensions 2 113 73writing zone 2 with name box1output dimensions 114 74 4input name (up to 40 char.) for zone 3box2reading zone 3input dimensions 2 49 113writing zone 3 with name box2output dimensions 50 114 4conversion of grid file 1 completeconversion of all grid files completedthe INGRID output file:INGRIDcontains (augmented) cell centers of the input grid(s)note: the mesh names in the INGRID file contain 40 charactersmake sure the PEGSUS parameter ICHAR is set to 40

enter 4 if pegsus version 4.X was usedenter 5 if pegsus version 5.X was used4enter the name of the COMPOUT file created by PEGSUS(unless you have renamed it, enter COMPOUT)COMPOUTenter 0 to leave overset data as 3denter 1 to convert overset data to 2d (2 i-planes)1enter 0 to use the maggie/CFL3D-ijk index definitionenter 1 to use the pegsus/OVERFLOW-jkl index definition0(additional output from XINTOUT_to_ovrlp is omitted... no further user input is needed)

Case | Plots | Exp. Data |
---|---|---|

both Standard and Chimera (Pegsus) |
Cp vs x/c Velocity Profiles |
4412.cpexp 4412.velexp |

FORTRAN program |

The FORTRAN program will extract the computed results for
either the standard or chimera cases from the plot3d files generated
by CFL3D (with **nplot3d = -1**) and the experimental
data files. The output is a formatted TECPLOT file, which should
be easily adapted to other plotting packages as well.

- Description:
- Download tar file RAE_Sensitivity.tar.gz (311 kB)
**gunzip RAE_Sensitivity.tar.gz****tar -xvf RAE_Sensitivity.tar**- The tar file contains the following items:
**rae10.fmt**- single-block grid (plot3d, multigrid, whole, formatted) of dimensions i x j x k = 2 x 257 x 97
**cfl3d.inp**- cfl3d input file for derivatives via complex variables.
**cfl3d.inp_+a**- cfl3d input file for a +10e-6 perturbation to the angle of attack, to be used for calculating the derivatives via finite differences.
**cfl3d.inp_-a**- cfl3d input file for a -10e-6 perturbation to the angle of attack, to be used for calculating the derivatives via finite differences.
**split.inp**- input to block splitter that converts the single-block formatted grid to a single-block unformatted grid that can be read by CFL3D
- To run the complex case, type:
- To run the finite-difference case, type:
(you will also need Get_FD from the cfl3d tools directory;
user inputs shown in
**bold**, interactive prompts for input shown in*italics*; be sure to finish one run before starting the next if running in the same directory) - Expected Results:
- Comparison with experimental data:
- Notes:
- The complex code generates both the solution and the derivative simultaneously; the solution convergence is found in the usual cfl3d.res file, while the derivatives of Cl, Cd, etc. may be found in cfl3d.sd_res.
- The complex derivatives require twice the memory of a single analysis, and roughly 3 times the CPU time of a single analysis. Thus, a finite-difference derivative requires 2 times the CPU time of a single analysis; this is the typical cost differential (but see the following note).
- For this particular case, the finite-difference results were accurately obtained with an "arbitrary" step size of 10e-6. However, more than one case has been encountered where several different finite-difference step sizes must be tried before one that gives accurate derivatives is found. If one factors in the trial and error test of step size that may be required, the cost of finite differences can easily be more than 2 times the CPU time of a single analysis.
- A complex step size of 10e-7 was used to obtain the derivatives with the complex version of CFL3D. To date, there has been no case for which 10e-7 was insufficient for the complex step.

Transonic viscous flow around an RAE 2822 airfoil is modeled with Menter's SST model. This case also appears in the Version 5 Users Manual; the difference here is that sensitivity (i.e. derivatives) of the solution with respect to angle of attack are calculated along with the standard solution. Input files are provided to calculate the sensitivity in two ways: 1) via complex variables, and 2) via finite differences. See the New Features page for additional information and results. The experimental data is taken from Cook, McDonald, and Firmin, AGARD-AR-138, 1979, p. A6. The following figures illustrate the case:

Then type:

This will create a subdirectory "RAE_Sensitivity".

**NOTE:** As of March, 2007, the Intel Version 9 compiler has major problems
with complex cases in CFL3D (the resulting executable **does not work** for this case). If you
use Intel, consider compiling with a different version.

enter first restart file to extract history data fromthis should be the "+" step filerestart.bin_+aenter second restart file to extract history data fromthis should be the "-" step filerestart.bin_-aenter step size1.e-6finite diffs to be calculated with central diffsenter file name for output finite differencesFinite_Diff_1.e-6enter 0 to output convergence of dcy/ddv,dcmy/ddventer 1 to output convergence of dcz/ddv,dcmz/ddv0

Case | No. Processors | Run Time | Memory | Convergence History | Derivative History | Test Date | Test Machine |
---|---|---|---|---|---|---|---|

Complex | 1 | 2 hr, 22 min | 75.2 MB |
cfl3d.res plot |
cfl3d.sd_res plot |
July 29 02 | Octane 2^{5} |

FD +alpha -alpha |
1 | 39 min (+a) 38 min (-a) |
37.7 MB both |
cfl3d.res_+a cfl3d.res_-a plot_+a plot_-a |
Finite_Diff_1.e-6 plot |
July 29 02 | Octane2^{5} |

Case | Plots | Exp. Data |
---|---|---|

Complex | Cp vs x/c |
2822.cpexp |

FORTRAN program |

The FORTRAN program will extract the computed results for any of the cases from the plot3d files generated by CFL3D and the experimental data file. The output is a formatted TECPLOT file, which should be easily adapted to other plotting packages as well.

- Description:
- Download tar file Ramp.tar.Z (134 kB)
**gunzip Ramp.tar.Z****tar -xvf Ramp.tar**- The tar file contains the following items:
**ramp_noembed.fmt**- single-block grid (plot3d type, formatted) of dimensions i x j x k = 2 x 73 x 45 for no embedding case
**ramp_noembed.inp**- cfl3d input file for no embedding case
**split_noembed.inp**- input to block splitter that converts the single-block formatted grid to a single block unformatted grid that can be read by CFL3D (for no embedding case)
**ramp_embed.fmt**- multi-block embedded grid (plot3d type, formatted) of dimensions i x j x k = 2 x 73 x 45, 2 x 33 x 21, 2 x 33 x 25, 2 x 29 x 21, 2 x 49 x 25, and 2 x 29 x 29 for embedding case
**ramp_embed.inp**- cfl3d input file for embedding case
**split_embed.inp**- input to block splitter that converts the multi-block formatted grid to a multi-block unformatted grid that can be read by CFL3D (for embedding case)
- To run the ramp case, type:
- Expected Results:
- Comparison with experimental data:
- Notes:
- We have chosen to run this case in 2 stages: first, we ran only on the global level (no embedded meshes). For this, the input file ramp_noembed.inp was used. Results from this run can be found in plot1. Next, we restarted with the embedded meshes included, using input file ramp_embed.inp. Results from this run can be found in plot2.
- Subsequent restarts, if desired, should have the "INEWG" parameters in the ramp_embed_2.inp input file all set to zero.
- When using embedded meshes, each subsequent embedded mesh level must be exactly double the spacing in each of the coordinate directions (j and k for 2-D, j, k, and i for 3-D) as the previous level.
- Embedded mesh cases CANNOT be run in parallel (requires data passing throughout the volume rather than just at the boundaries, so is unsuitable for the message passing approach).

Supersonic flow over an inviscid ramp (Euler flow) is modeled. This case demonstrates the use of embedded meshes. The following figure illustrates the case:

Then type:

This will create a subdirectory "Ramp".

(Note: finish one cfl3d_seq run before starting the next.)

No comparison is made with experiment. This case is included primarily as a simple example to demonstrate the use of embedded grids.

- Description:
- Download tar file Timeaccstudy.tar.Z (187 kB)
**gunzip Timeaccstudy.tar.Z****tar -xvf Timeaccstudy.tar**- The tar file contains the following items:
**cyl_129x81.fmt**- single-block grid (plot3d type, formatted) of dimensions i x j x k = 2 x 129 x 81
**cyl_start_1.inp****cyl_start_2.inp****cyl_start_3.inp****cyl_0.2.inp****cyl_0.1.inp****cyl_0.05.inp****cyl_0.025.inp****cyl_0.0125.inp**- cfl3d input files
**split.inp**- To run the circular cylinder time-accuracy study, type:
- Expected Results:
- Demonstration of 2nd order temporal accuracy and comparison with experiment:
- Notes:
- The method of perturbation used in cyl_start_2.inp, to get the cylinder to go unsteady quicker, uses an "artificial" wall BC of Euler (1005) over half of the cylinder for 50 iterations. Be sure NEVER TO INITIATE A SOLUTION FROM SCRATCH (irest=0) using this technique! If you do, the minimum distance function, which keys off of the BC type, will be INCORRECT for the entire computation - including subsequent restarts - even after the perturbation is removed.)
- If you try to switch turbulence model, to run with a two-equation
model, it may be necessary to limit the maximum eddy viscosity by
employing the keyword
**edvislim**and setting it to, say, 100000.

Subsonic flow past a circular cylinder is modeled at a Reynolds number of 10,000, with the Spalart-Allmaras turbulence model employed (at this low a Re, the turbulence is primarily confined to the wake region). This case is given to demonstrate the temporal order property of the code. Using ITA = 2 or -2, CFL3D employs a 2nd order backward difference scheme. (Prior to Version 6.1, turbulence models were advanced in time with a 1st order accurate backward difference scheme regardless of the temporal order of accuracy of the mean flow equations. This lower order accuracy in the turbulence models made the code overall less than 2nd order in time. Starting in Version 6.1, the turbulence models are advanced with the same temporal accuracy as the mean flow equations so that 2nd order temporal accuracy can now be achieved for time-accurate turbulent flows.) The following figures illustrates the case:

Then type:

This will create a subdirectory "Timeaccstudy".

(Note: each cfl3d_seq run should be done sequentially, i.e., finish one before starting the next.)

The following commands run various time steps, always starting from the same restart file:

(Note: each run should be done independently, i.e., finish one before starting another if running in the same directory, and remember to save results between each run.)

Case | No. Processors | Run Time | Memory | Convergence History | Test Date | Test Machine |
---|---|---|---|---|---|---|

initial run | 1 | 6 min | 17.5 MB |
cfl3d.res |
Aug 6 02 | Octane2^{5} |

perturbation run | 1 | 3 min | 17.5 MB |
cfl3d.res |
Aug 6 02 | Octane2^{5} |

run to achieve periodicity | 1 | 6 hr, 16 min | 17.8 MB |
cfl3d.res plot |
Aug 6 02 | Octane2^{5} |

dt=0.2 | 1 | 3 min | 17.8 MB |
cfl3d.res |
Aug 6 02 | Octane2^{5} |

dt=0.1 | 1 | 6 min | 17.8 MB |
cfl3d.res |
Aug 6 02 | Octane2^{5} |

dt=0.05 | 1 | 13 min | 17.8 MB |
cfl3d.res |
Aug 6 02 | Octane2^{5} |

dt=0.025 | 1 | 26 min | 17.8 MB |
cfl3d.res |
Aug 6 02 | Octane2^{5} |

dt=0.0125 | 1 | 49 min | 17.8 MB |
cfl3d.res |
Aug 6 02 | Octane2^{5} |

Using lift and drag coefficients, the 2nd order temporal order
convergence rate
is shown in clerrorplot and
cderrorplot. These results
can be post-processed using the FORTRAN postprocessing program
FORTRAN program
(hardwired for use with this particular case).

Using a time step of dt=0.4 on this 129 x 81 grid (2-D), the Strouhal number St = n*d/u_inf comes out to be 0.236. (In CFL3D's nondimensional units, St = d/(M_inf*T), where d = nondimensional cylinder diameter = 1.0, M_inf = 0.2, and T = the nondimensional time for one period.) The computed average drag coefficient on the cylinder is about 1.76. (These levels for St and Cd are not necessarily spatially or temporally converged enough. 129 x 81 is a rather coarse grid, and dt=0.4 yields only 53 steps per period.)

In experiments at Re = 10,000, St is roughly 0.2 and average drag coefficient is near 1.0-1.2 (see Cox et al, Theoret. Comput. Fluid Dynamics (1998) 12: 233-253). Thus, 2-D CFD yields too-high levels for St and Cd (overall conclusions are similar even if one were to use finer grids and lower time steps). However, experiments for Re > 200 or so always have inherent three-dimensionality (spanwise structures), so 3-D computations would be necessary to reproduce the physics, including St and Cd.

- Description:
- Grid (every 4th point shown for clarity)
- Typical Mach number
- Surface pressure coefficient
- Surface pressure coefficient (close-up near L.E.)
- Download tar file Spaceaccstudy.tar.Z (5.76 MB)
**gunzip Spaceaccstudy.tar.Z****tar -xvf Spaceaccstudy.tar**- The tar file contains the following items:
**n0012_1025.fmt**- single-block grid (plot3d type, formatted) of dimensions i x j x k = 2 x 1025 x 513
**n0012t0.inp_1****n0012t0.inp_2****n0012t0.inp_3****n0012t0.inp_4****n0012t0.inp_5**- cfl3d input files
**split.inp**- Before beginning, note that these runs, and especially the 2 finest-level runs, can be quite time-consuming because of the large number of grid points combined with the large number of cycles used to iterate to convergence (see note 1 below). To run the NACA 0012 space-accuracy study, type:
- Expected Results:
- Demonstration of 2nd order spatial accuracy and comparison with experiment:
- Notes:
- Each successive grid level was run for at least 10000 multigrid cycles. This is significantly more than is usually necessary to achieve an adequate level of convergence! However, this particular case does not converge very well past the first 2-order drop in residual; also, for performing this spatial accuracy study, it was desired to insure that the drag levels were converged to very tight accuracy (in the current case they were converged to within less than delta cd = 5.e-7). For a less restrictive convergence criterion, each grid level could be run an order of magnitude fewer cycles (1000 each as opposed to 10000 each), and cd would be obtained to within less than delta cd = 5.e-6 in this case.
- If you try to switch turbulence model, to run with a two-equation
model, it may be necessary to limit the maximum eddy viscosity by
employing the keyword
**edvislim**and setting it to, say, 100000.

Subsonic flow past a NACA 0012 airfoil is modeled at a Reynolds number of 10,000,000 and Mach number of 0.3, with the Spalart-Allmaras turbulence model employed and transition specified at x/c=2.5 percent chord. This case is given to demonstrate the global 2nd order spatial order property of the code. Using RKAP0 = 1/3, CFL3D employs a 3rd order upwind-biased difference scheme on the Euler fluxes. However, the viscous terms are treated 2nd order, so the resulting global order of accuracy of CFL3D ends up being approximately 2nd order. This case also demonstrates the use of mesh sequencing in CFL3D (starting on a coarse level grid, and running successively finer and finer grids). An extra-fine 1025x513 C-grid was used; its minimum spacing at the wall was such that the y+ at the first point off the wall was approximately 0.1 on the finest (1025x513) level and 2.3 on the coarsest (65x33) level. The following figures illustrates the case:

Then type:

This will create a subdirectory "Spaceaccstudy".

(Note: each run should be done sequentially, i.e., finish one before starting the next.)

Case | No. Processors | Run Time | Memory | Convergence History | Test Date | Test Machine |
---|---|---|---|---|---|---|

65x33 grid | 1 | 26 min | 655.0 MB |
cfl3d.res |
Nov 9 02 | Octane2^{5} |

129x65 grid | 1 | 1 hr, 22 min | 657.0 MB |
cfl3d.res |
Nov 9 02 | Octane2^{5} |

257x129 grid | 1 | 7hr, 19 min | 659.0 MB |
cfl3d.res |
Nov 9 02 | Octane2^{5} |

513x257 grid | 1 | 37 hr, 11 min | 661.0 MB |
cfl3d.res |
Nov 11 02 | Octane2^{5} |

1025x513 grid | 1 | 179 hr, 13 min | 785.5 MB |
cfl3d.res plot |
Nov 18 02 | Octane2^{5} |

Using drag coefficients, the 2nd order spatial order
convergence rate
is shown in cderrorplot.
These results can be post-processed using the FORTRAN postprocessing program
FORTRAN program
(hardwired for use with this particular case).

A plot of the CFD predicted drag coefficients in comparison with experiment is given in cd_vs_exp. The experiment is taken from McCroskey, W. J., "A Critical Assessment of Wind Tunnel Results for the NACA 0012 Airfoil", AGARD CP-429, July 1988, pp. 1.1-1.21. It is given as a range of drag values measured over several different wind tunnel experiments, as a function of Reynolds number. The converged CFD result lies within the data band. This plot also shows how the CFD results converge with grid refinement. To summarize, the result on the 65x33 grid is 18.6% in error from the extrapolated solution on an infinitely-refined grid, 129x65 is 3.4% in error, 257x129 is 0.74% in error, 513x257 is 0.20% in error, and 1025x513 is 0.05% in error. This grid-sensitivity analysis indicates that a grid of size 257x129 for this 2-D case is sufficient to capture the drag to within less than 1% of its "exact" (no discretization error) value.

- Description:
- Download tar file Ejectornozzle.tar.gz (181 kB)
**gunzip Ejectornozzle.tar.gz****tar -xvf Ejectornozzle.tar**- The tar file contains the following items:
**nozzle.p3dfmt**- 3-block grid (plot3d type, formatted) of dimensions i x j x k = 2 x 31 x 41, 2 x 31 x 71, 2 x 101 x 121
**nozzle.inp**- cfl3d input file; using the SST turbulence model. Results for the other turbulence models shown below can be obtained by simply changing ivisc(k) to the appropriate value, e.g. ivisc(k) = 5 for SA and ivisc(k) = 14 for EASM-ko
**split.inp**- input to block splitter that converts the 3-block formatted grid to a 3-block unformatted grid that can be read by CFL3D
- To run the ejector nozzle case, type:
- Expected Results:
- Comparison with experiment:
- Notes:
- This case has nozzle total pressure divided by atmospheric static pressure of 2.44, with total temperature = 644 R. The secondary flow has a total pressure equal to atmospheric and a temperature of 550 R. At the outflow used by this grid, the static pressure divided by the atmospheric static pressure is taken to be 0.9131. However, in CFL3D, we wish to choose a reference condition that corresponds with a non-zero Mach number: in this case it is taken to be M=0.22, which is the approximate Mach number at the secondary flow inlet in this grid. (Corresponding Reynolds number is taken to be approximately 1.64 million per unit "one" of the grid, which is in feet.) Using M=0.22 and isentropic relations, one can find that Pt/Pref = 1.0343 and Tt/Tref = 1.0097. These numbers are used as inflow conditions for the secondary flow. Because the "atmosphere" in this case has zero flow and Pt = constant from the atmosphere through to the secondary flow inlet, Patm/Pref = 1.0343 and Tatm/Tref = 1.0097. At the nozzle inlet, Pt/Patm = 2.44 so Pt/Pref = (Pt/Patm)*(Patm/Pref) = 2.5237. Also Tt/Tatm = 1.17091 so Tt/Tref = (Tt/Tatm)*(Tatm/Tref) = 1.1822. At the outflow, P/Pref = (P/Patm)*(Patm/Pref) = 0.9444.
- Note that the EASM-ko was re-calibrated in 9/2002. Use of ivisc=14 in versions prior to V6.1 will not agree with the results given here.

A subsonic 2-D jet flow entrains and mixes with a secondary outer flow. Inflow is set by specifying total pressure and total temperature. Results using using SA, SST, and EASM-ko turbulence models (#5, #7, and #14) are compared with experimental data from Gilbert and Hill, NASA CR-2251, 1973. See also Georgiadis et al, AIAA 99-0748, 1999. The following figure shows the grid:

Then type:

This will create a subdirectory "Ejectornozzle".

Case | Plots | Exp. Data |
---|---|---|

SST, SA and EASM-ko |
u vs y |
u_vs_yexp.dat |

FORTRAN program |

The FORTRAN program will extract the computed results from the printout (cfl3d.prout) file generated by CFL3D at the approximate locations (nearest gridpoints) corresponding with the experimental data. The output files are formatted TECPLOT files.

- Description:
- Grid
- Pressure contours at alpha=5.95 deg (increasing)
- Pressure contours at alpha=2.43 deg (decreasing)
- Download tar file Pitch0012.tar.Z (391 kB)
**gunzip Pitch0012.tar.Z****tar -xvf Pitch0012.tar**- The tar file contains the following items:
**n0012_257.fmt**- 1 block grid (plot3d type, formatted)

dimensions i x j x k = 2 x 257 x 97 **n0012_ss.inp**- CFL3D input file to generate a steady-state "starting" solution at alpha=4.86 deg.
**n0012_pitch.inp**- CFL3D input file to run pitching airfoil through approx. 6 cycles and stop near alpha=5.95 deg (increasing).
**n0012_pitch2.inp**- CFL3D input file to continue running pitching airfoil and stop near alpha=2.43 deg (decreasing).
**split.inp**- To run the pitching airfoil case, type:
- Expected Results:
- Comparison with experimental data:
- Density residual subiteration convergence
- Cl subiteration convergence
- Turbulence model residual subiteration convergence
- Notes:
- For this case, the frequency of pitching oscillation is 50.32 Hz. Chordlength in the experiment was 0.33333 ft. Assuming speed of sound to be 1084 ft/sec, this yields a nondimensional frequency of 0.01547. Thus, the angle of attack of the airfoil is governed by: alpha=alpha0 + alpha1*sin(2*pi*kr*t/Lref) where alpha0= 4.86 deg, alpha1= 2.44 deg, kr = 0.01547, Lref = 1 (the chord is unit one in the grid), t = nondimensional time. We take nondimensional time step of 0.4 (which corresponds with dimensional time 0.000123 sec).
- It may or may not be necessary to restart an unsteady run such as this from a steady-state solution. However, doing so often allows you to achieve repeatable periodicity faster. Note from current results showing Cl and Cm vs alpha that periodicity in these quantities is achieved within approximately one cycle in this case.
- If you try to switch turbulence model, to run with a two-equation
model, it may be necessary to limit the maximum eddy viscosity by
employing the keyword
**edvislim**and setting it to, say, 100000.

Turbulent flow past a NACA 0012 airfoil sinusoidally oscillating in pitch is modeled. The unsteady motion is accomplished by moving the grid itself (unsteady time metric terms are included in CFL3D's formulation). Mach number is 0.6 and Reynolds number is 4.8 million. The Spalart-Allmaras turbulence model is employed. The frequency of pitching oscillation is 50.32 Hz. The experimental data is AGARD Case 3 taken from Landon, AGARD-R-702, 1982. The following figures illustrate the case:

Then type:

This will create a subdirectory "Pitch0012".

(Note: each run should be done sequentially, i.e., finish one before starting the next.)

Case | No. Processors | Run Time | Memory | Convergence History | Test Date | Test Machine |
---|---|---|---|---|---|---|

steady | 1 | 27 min | 49.4 MB |
cfl3d_ss.res |
January 21 03 | Octane2^{5} |

pitching | 1 | 4hr, 47 min | 60.3 MB |
cfl3d.res |
January 21 03 | Octane2^{5} |

pitching (continuation) |
1 | 25 min | 60.3 MB |
cfl3d2.res plot |
January 21 03 | Octane2^{5} |

Case | Plots | Exp. data |
---|---|---|

SA |
Cl vs alpha Cm vs alpha Cp vs x/c at 5.95 deg Cp vs x/c at 2.43 deg |
alphaclcm_exp.dat cp_exp_5.95.dat cp_exp_2.43.dat |

FORTRAN program |

The FORTRAN program (hardwired for this case) will compute the alphas from the iteration numbers in the residual file (cfl3d.res) generated by CFL3D.

For this case we did not perform a time step study, in
which the time step and/or number of subiterations is varied to
determine their effect on the solution. The time step used (dt=0.4)
corresponds to between 161-162 time steps per cycle.
Six subiterations were used per time step. The convergence history
with subiterations is output by CFL3D to the files
cfl3d.subit_res for
density residual and forces/moments, and to
cfl3d.subit_turres for
turbulence model residual. These files do not maintain a
running history; they are reset for each successive restart. The files
given here correspond to the final run using **n0012_pitch2.inp**.

Sample plots showing typical subiteration convergence for this case are given here:

- Description:
- Download tar file Rotorstator.tar.Z (305 kB)
**gunzip Rotorstator.tar.Z****tar -xvf Rotorstator.tar**- The tar file contains the following items:
**rotstat.fmt**- 14 block overset grid (plot3d type, formatted)

block 1 dimensions i x j x k = 2 x 55 x 23

block 2 dimensions i x j x k = 2 x 61 x 21

block 3 dimensions i x j x k = 2 x 55 x 23

block 4 dimensions i x j x k = 2 x 61 x 21

block 5 dimensions i x j x k = 2 x 55 x 23

block 6 dimensions i x j x k = 2 x 61 x 21

block 7 dimensions i x j x k = 2 x 61 x 23

block 8 dimensions i x j x k = 2 x 61 x 21

block 9 dimensions i x j x k = 2 x 61 x 23

block 10 dimensions i x j x k = 2 x 61 x 21

block 11 dimensions i x j x k = 2 x 61 x 23

block 12 dimensions i x j x k = 2 x 61 x 21

block 13 dimensions i x j x k = 2 x 61 x 23

block 14 dimensions i x j x k = 2 x 61 x 21 **rotstat.inp**and**rotstat_new.inp**- CFL3D input files
**maggie.inp**- input to MAGGIE that generates overset grid connectivity file "ovrlp.bin" required by CFL3D
**mag1.h**- parameter file for MAGGIE; must be placed in the cfl3dv6/header directory before compiling MAGGIE
**split.inp**- input to block splitter that converts the 14-block formatted grid to a 14-block unformatted grid that can be read by CFL3D
**README**- file that describes changes to the code after V6.3 that require differences in the input file
- To run the rotor-stator case, copy mag1.h to the header directory and compile MAGGIE. Then type:
- Expected Results:
- Comparison with experimental data:
- Notes:
- Boundary condition type 2003 is used to specify total pressure and total temperature at the inlet. From isentropic flow relations or tables, for an inlet flow Mach number of 0.07, M_inlet = 0.07, Pt_inlet/Pinf = 1.0035, Tt_inlet/Tinf = 1.0010. Also, alphae = betae = 0 (purely axial flow is assumed). Boundary condition type 2002 is used to specify an exit pressure, which is taken to be pexit/pinf = 0.967 for this case.
- The inflow Mach number used in boundary condition type 2003 is an estimate; if the exit pressure were not set correctly for this internal flow case, the computed inflow Mach number would not be close to the specified inflow value (when a time-periodic state is reached or at convergence in steady state). By specifying control surfaces at the inflow plane, the user is able to verify (in cfl3d.prout) after the computation is complete that the average inflow Mach number is approximately 0.073; this was deemed to be close enough to the desired value. If desired, the exit pressure could be adjusted (raised in this case) and the solution re-run until a new time-periodic solution (and a new inlet Mach number) is established.
- The input grid is in PLOT3D format, with y as the "up" direction (ialph = 1; z is the spanwise, 2-d direction). For Version 6.3 or earlier, the grid motion parameters must be set as if z is the "up" direction. This is because: whenever the input grid has y as the "up" direction, CFL3D internally swaps y and z so that the code always computes on a grid in which z is "up". This "quirk" has been corrected in Updates to Version 6.3, so when using official versions of the code AFTER 6.3, one sets grid motion parameters as if y is "up".
- The translational velocity for this simulation is taken to be 96.6 ft/sec. This gives (uaxial/wtrans) = 75/96.6 = 0.78. The input value wtrans is wtrans/ainf, so with the reference Mach number 0.07, wtrans = 0.07/0.78 = (-)0.0897 (the negative gives a downward rotor motion).
- In order to be able to run an arbitrarily long simulation, the grid resetting option was employed. The top-to-bottom length of the grid is 24.23514 inches and the rotor and stator zones start out in alignment, so dzmax = 24.23514. Thus the rotor zones are reset whenever the displacement exceeds 24.23514 inches.
- CFL3D's overset grid preprocessor MAGGIE to date does not have dynamic memory capability. Thus you must ensure that mag1.h is sized appropriately for the problem at hand, and you must recompile MAGGIE for each different case. A mag1.h file is supplied for the current case: it must be placed in the cfl3dv6/header directory before compiling MAGGIE (if you have previously compiled MAGGIE, then (1) replace mag1.h in cfl3dv6/header, (2) go to cfl3dv6/build and type "make scrubmaggie", (3) type "make linkmaggie", (4) type "make maggie").
- An error was discovered in MAGGIE in January 2003; be sure you have the most up-to-date version of maggie.F before attempting this case.
- Among other things, the cfl3d.out output file lists geometric mismatch values for 1-to-1 blockings when they exceed certain criteria. When these occur, they indicate imperfect matching of the 1-to-1 blocks, and the user should check to make sure there are no problems with the grid or the input file. In the present case, several small mismatches are present, which were deemed to be small enough to be ignored. In addition, the user will notice that there are also some large geometric mismatch values of approximately 24.235. However, these are present because 1-to-1 interfacing has been utilized to connect the periodic faces, which is OK to do in 2-d because there is no angular rotation involved (the top of zone 5 matches with the bottom of zone 1, and the top of zone 13 matches with the bottom of zone 7). Therefore these mismatch values in this case represent the distance between the periodic faces. (Note that BC type 2005 could have been used instead on these periodic faces.)
- The mass flow is monitored in this case by employing control surfaces in the input file. The resulting mass flow and other statistics are output to cfl3d.prout. At the end of the run in this case, the mass flow through the downstream plane of the four outer rotor grids is: Mass flow / (rhoinf*vinf*(L_R)**2) = 0.25386E+02.
- If you try to switch turbulence model, to run with a two-equation
model, it may be necessary to limit the maximum eddy viscosity by
employing the keyword
**edvislim**and setting it to, say, 100000.

This case simulates, in two dimensions, the unsteady flow through a single stage turbine in which the ratio of stator to rotor blades is 3:4. The case exercises a number of capabilities of CFL3D including unsteady flow, moving (translating) zones, dynamic patching between zones in relative motion, and grid overlapping. The Spalart-Allmaras turbulence model is employed.

This grid models a generic rotor-stator configuration in 2-d (which does not correspond to any experimental configuration), with the moving rotor row downstream of the stationary stator row. The grid consists of fourteen zones with a total of 18374 points in one plane. The grid zones communicate with one another through both patching and overlapping. At a time step of 1.0, it takes 270 time steps for the eight rotor zones (containing four blades) to completely traverse the six stator zones (containing three blades). The rotor zones are reset after each complete traverse. The input file is set for 1500 time steps (using five multigrid sub-iterations per time step), which is sufficient to establish a time-periodic solution.

The 2-d simulation assumes a nominal axial velocity of 75 feet/second. The inlet Mach number is 0.07, and the Reynolds number/inch is 100,000. The following figures illustrate the case:

Then type:

This will create a subdirectory "Rotorstator".

No comparison is made with experiment. This case is included primarily as a simple example to demonstrate the use of moving grids with sliding patched interfaces.

__HUMP-MODEL FLOW CONTROL SIMULATION__

- Description:
- Download tar file Humpcase.tar.gz (3.6 MB)
**gunzip Humpcase.tar.gz****tar -xvf Humpcase.tar**- The tar file contains the following items:
**hump2_e_newtop.fmt**- 4 block grid (plot3d type, formatted)

block 1 dimensions i x j x k = 2 x 793 x 217

block 2 dimensions i x j x k = 2 x 161 x 121

block 3 dimensions i x j x k = 2 x 65 x 121

block 4 dimensions i x j x k = 2 x 49 x 217 **hump2_e_oscillate_newtop.inp_1**,**hump2_e_oscillate_newtop.inp_2**, and**hump2_e_oscillate_newtop.inp_3**- CFL3D input files
**split.inp**- input to block splitter that converts the 4-block formatted grid to a 4-block unformatted grid that can be read by CFL3D
**README**- file that describes the case
- To run the hump case (on 1-level-down grid), type:
- Expected Results:
- Comparison with experimental data:
- Notes:
- The flow-control BC is set at the bottom of the cavity for this case. For oscillatory control, CFL3D uses BC number 2028 (see New Features for more details on this). Using this BC, the input freq that corresponds to 138.5 Hz is 0.16812. The peak velocity amplitude at the bottom of the cavity is set to rho*w=.001 (nondimensionalized by freestream density and freestream speed of sound). This level of blowing was chosen in an attempt to approximate the peak velocity out of slot (Ujetmax) during blowing part of cycle of approximately 26 m/s. (Note that BC number 2028 extrapolates both density and pressure from the interior of the domain: this may not be appropriate for some uses, such as setting an oscillatory BC directly at a wall jet exit location.)
- In this case, the overall flowfield was first established to a reasonable degree with no-flow through the cavity. Then, this solution was restarted time-accurately with oscillatory blowing/suction. The time step was set for 360 steps per cycle of blowing/suction. A total of 20 subiterations per time step were employed. This was run for 7 cycles (until the periodic flow was established fairly well). Then, finally, 1 cycle was run in the third restart to obtain averaged statistics over 1 cycle (using the keyword input iteravg=1).
- A description on the usage of keyword
**iteravg**can be found in New Features. - One can see from the long-time-average Cp vs x results that the CFD predicts too large a time-averaged separation bubble behind the hump. This is a consistent problem seen with nearly all Reynolds-averaged Navier-Stokes (RANS) models for this case (see some of the summary papers given at the CFDVAL website). All RANS turbulence models investigated to date have been seen to yield turbulent shear stress levels in the separated shear region that are much too low in magnitude.
- If you try to switch turbulence model, to run with a two-equation
model, it may be necessary to limit the maximum eddy viscosity by
employing the keyword
**edvislim**and setting it to, say, 100000.

This is the oscillatory (synthetic jet) control case from the CFDVAL Workshop Case 3 (see the CFDVAL website). The conditions are as follows: M=0.1, Re=936,000 per chord length of hump, zero-net-mass-flux oscillatory suction/blowing, frequency = 138.5 Hz. The Spalart-Allmaras turbulence model is employed. Currently, although the fine grid is of size: 793x217, 161x121, 65x121, 49x217 (for the 4 zones, respectively), it is currently only run for this test 1-level-down (using every other gridpoint in each coordinate direction): 397x109, 81x61, 33x61, 25x109.

The experiment is nominally 2-d. (Note that tunnel blockage due to side-plates needs to be taken into account in the 2-d simulation. This is currently done by shaping the top tunnel wall to account for a tunnel area decrease.) The following figures illustrate the case:

Then type:

This will create a subdirectory "Humpcase".

(Note: each run should be done sequentially, i.e., finish one before starting the next.)

Case | No. Processors | Run Time | Memory | Convergence History | Test Date | Test Machine |
---|---|---|---|---|---|---|

hump (steady, no control) | 1 | 13 min | 251 MB |
cfl3d.res |
February 8 07 | Linux Workstation^{7} |

hump (unsteady, 7 cycles) | 1 | 4 hrs, 30 min | 292 MB |
cfl3d.res |
February 8 07 | Linux Workstation^{7} |

hump (unsteady, 1 cycle) | 1 | 41 min | 303 MB |
cfl3d.res plot |
February 8 07 | Linux Workstation^{7} |

Case | Plots | Exp. data |
---|---|---|

Hump with SA |
Long-time-average Cp vs x Instantaneous Cp vs x near 140 deg in cycle |
osc_cp_avg.dat osc_cp_instant.dat |

The instantaneous data is extracted at the end of the run from the final
data files output by CFL3D. For example, instantaneous Cp can be obtained from the
cfl3d.prout file. More detailed
instantaneous flowfield information can be obtained from the usual PLOT3D-output files.
Long-time-average flowfield data are stored in the files cfl3d_avgg.p3d and
cfl3d_avgq.p3d, when the keyword **iteravg** is activated.

The long-time-average Mach contours are shown in Long-time-average Mach contours, and the instantaneous vorticity contours at the end of the final run are shown in Instantaneous vorticity contours.

- Description:
- Download tar file SoMellor.tar.gz (849 kB)
**gunzip SoMellor.tar.gz****tar -xvf SoMellor.tar**- The tar file contains the following items:
**somellor_eul.p3dform**- single-block grid (plot3d type, formatted) of dimensions i x j x k = 2 x 257 x 161
**somellor_sa.inp**and**somellor_sarc.inp**- CFL3D input files; note that these require the inflow BC file bc2008.data to run.
**split_form_to_unform.inp****bc2008.data**- file needed by CFL3D for specifying inflow profiles in this case; this data is also included in a more readable format below in "Inflow profile specification"
- To run the curved wall case, type:
- Expected Results:
- Comparison with experimental data:
- Notes:
- Note that the Cp is referenced to the Cp value at the inflow. Also, experimental results are given in terms of "s", the distance along the channel inner wall.
- The file bc2008.data was created specifically for use with SA or SARC. It is incorrect to use it in conjunction with different turbulence models, because the turbulence variables would be improperly specified. To run with a different turbulence model, the inflow profile specification would have to be used to create a new bc2008.data file with appropriate turbulence values.
- The default "cr3" constant for the SARC model in CFL3D is taken to be 0.6, based
on this and other tests conducted with the model. In AIAA Journal 38(5), 2000, p.784-792
and in Aerospace Sci. Technol. 5, 1997, p.297-302 the value of cr3=1.0 is used, but
the authors of those references admit that this and
other constants used by the model are "open to refinement."
We found cr3=1.0 to yield too large a correction. It is given by keyword parameter
**sarccr3**(see New Features), so the user can adjust it to be different from 0.6 if desired. - If you try to switch turbulence model, to run with a two-equation
model, it may be necessary to limit the maximum eddy viscosity by
employing the keyword
**edvislim**and setting it to, say, 100000.

2-D subsonic flow through a curved duct (based on the So-Mellor experiment from J Fluid Mech 60 (part 1), 1973, pp. 43-62) is modeled at Reynolds number 36417 per inch and a nominal Mach number of 0.063 in the channel. In this case, the inflow is specified as a "turbulent boundary layer" by specifying crude inflow boundary conditions using BC2008, including turbulence. This is done to insure that the flow is fully turbulent well before it reaches the curved region of the duct. Both the Spalart-Allmaras (SA) and SA with rotation and curvature correction (SARC) models are employed, to demonstrate the influence of curvature for this flow. It should be noted that the outer wall shape was not given in the experimental reference, but was derived by using an optimization method in order to achieve the desired inner wall pressure distribution from experiment (see Int J Heat and Fluid Flow 22, 2001, pp. 573-582). As a consequence, the wall shape is not perfectly smooth, and solution results end up being somewhat "wavy." This case is being simulated with viscous inner wall and inviscid outer wall boundary conditions. The following figures illustrate the case:

Then type:

This will create a subdirectory "SoMellor".

Case | Plots | Exp. data |
---|---|---|

So Mellor experiment |
Cp vs s Cf vs s |
cp_exp.dat cfu24_exp.data.dat |

FORTRAN program 1 (cp vs s) FORTRAN program 2 (cf vs s) Inflow profile specification |

The FORTRAN programs will extract the computed results from the printout files (named cfl3d.prout) generated by CFL3D. The output files are formatted TECPLOT files, which should be easily adapted to other plotting packages as well. The Inflow profile specifications are given as a more readable version of bc2008.data (the file used by CFL3D in conjunction with SA and SARC). A plot of the admittedly crude u velocity and nu_wiggle (Spalart-Allmaras turbulence variable) inflow profiles can be seen by clicking here.

- Description:
- Download tar file Axibump.tar.gz (222 kB)
**gunzip Axibump.tar.gz****tar -xvf Axibump.tar**- The tar file contains the following items:
**bumpgrd.fmt**- single-block grid (plot type, formatted) of dimensions i x j x k = 2 x 181 x 101
**bumpperiodic.inp**- cfl3d input file; periodic boundary conditions
**bumpperiodic.inp_3blk**- cfl3d input file for a 3 block grid
**split.inp_1blk****split.inp_3blk**- input to block splitter that splits/converts the single-block formatted grid to a 3 block block unformatted grid that can be read by CFL3D. Note: this splitter input file is set up to only split the grid, not the input file - an already split input file is provided in the tar file. This is because the splitter does not handle the periodic boundary condition correctly (a known limitation with the splitter), and as a result, some correction to the split input file generated by splitter is needed.
- To run the single block axisymmetric bump case, type:
- To run the 3 block case on 3 processors (+ 1 host), type:
- Expected Results:
- Comparison with experimental data:
- Notes:

Transonic flow past a "bump" is modeled in 3-D using 2 computational planes (separated by an angle of 1 degree), with periodic boundary conditions. Menter's SST turbulence model is employed. The experimental data is from Bachalo, W., Johnson, D., "An Investigation of Transonic Turbulent Boundary Layer Separation Generated on an Axisymmetric Flow Model," AIAA 79-1479, 1979.

Then type:

This will create a subdirectory "Axibump".

Case | Plots | Exp. Data |
---|---|---|

1 Block |
Cp vs x |
bumpcp_exp.dat |

FORTRAN program |

The FORTRAN program will extract the computed
results for the **1 block case** from the printout (cfl3d.prout)
file generated by CFL3D. The output
is a formatted TECPLOT file, as is the experimental data file;
these should be easily adapted to other plotting packages as well.

- Description:
- Download tar file ONERA_M6.tar.Z (17.9 MB)
**gunzip ONERA_M6.tar.Z****tar -xvf ONERA_M6.tar**- The tar file contains the following items:
**m6i289.fmt.gr**- single-block grid (plot3d, multigrid, whole, formatted) of dimensions i x j x k = 289 x 65 x 49
**cfl3d.inp_1blk**- cfl3d input file for the single-block grid. You may want to reduce the number of iterations in the fine level to zero for your initial run.
**split.inp_1blk****split.inp_32blk**- input to block splitter that splits/converts the single-block formatted grid to a 32 block unformatted grid that can be read by CFL3D; also generates the corresponding input file cfl3d.inp_32blk
- To run the single-block case, type:
- To run the 32 block case on 8 processors (+ 1 host), type:
- Expected Results:
- Comparison with experimental data:
- Notes:
- The Cp vs x/c at eta = 0.99 is not shown in the comparison plots with experimental data below because of space limitations on a single page. However, the extraction program provided does output both the computed and experimental results at this station.
- If you try to switch the turbulence model and run, for example, with
SST, it is necessary to limit the maximum eddy viscosity by
employing the keyword
**edvislim**and setting it to, say, 100000.

This widely-used test case consists of an isolated wing in a transonic free stream of Mach 0.84 at an angle of attack of 3.06 degrees with a Reynolds number of 11.7 million based on mean aerodynamic chord (MAC). In the experiment, MAC=0.64607 m. The current grid is nondimensionalized to make the semispan 1 unit (in the experiment it is 1.1963 m), so the MAC of the current grid is 0.54 units. The Spalart-Allmaras turbulence model is employed. The experimental data is taken from Schmitt and Charpin, AGARD-AR-138, 1979, p. B1. The following figures illustrate the case:

Then type:

This will create a subdirectory "ONERA_M6".

Case | Plots | Exp. Data |
---|---|---|

1 Block | Cp vs x/c | exp.dat |

FORTRAN program |

The FORTRAN program will extract the computed
results for the **1 block case** from the plot3d files generated
by CFL3D (with **nplot3d = -1**) and the experimental
data files. The output is a formatted TECPLOT file, which should
be easily adapted to other plotting packages as well.

__ARA M100 WING-BODY (point-match grid)__

- Description:
- Download tar file ARA_M100.tar.Z (17.6 MB)
**gunzip ARA_M100.tar.Z****tar -xvf ARA_M100.tar**- The tar file contains the following items:
**m100sbj57k49twfix.gridp3d_fmt**- single-block grid (plot3d, multigrid, whole, formatted) of dimensions i x j x k = 321 x 57 x 49
**cfl3d.inp_1blk**- cfl3d input file for the single-block grid. You may want to reduce the number of iterations in the fine level to zero for your initial run.
**split.inp_1blk**- input to block splitter that converts the single-block formatted grid to a single-block unformatted grid that can be read by CFL3D
**split.inp_16blk**- input to block splitter that splits/converts the single-block formatted grid to a 16 block unformatted grid that can be read by CFL3d; also creates the corresponding input file, cfl3d.inp_16blk
- To run the single-block case, type:
- To run the 16 block case on 16 processors (+ 1 host), type:
- Expected Results:
- Comparison with experimental data:
- Notes:
- The Cp extraction program provided above works correctly for all but the first spanwise cut on which experimental data is available (eta = 0.019). Thus, this cut is not presented in the comparison with experimental data; rather the comparison starts at the second spanwise cut, eta = 0.123. Also, the comparison at eta = 0.939 is not shown because of space limitations on a single page. However, the extraction program does output both the computed and experimental results at these stations.
- The tables above show results for Flux Vector Splitting (FVS) in addition to the standard (and recommended) Flux Difference Splitting. As it turns out, the more dissipative FVS agrees much better with the experimental data at stations 2y/B = 0.455 and 2y/B = 0.633. The input file provided for this case is set up to run FDS; to run FVS instead, the CFL number needs to be lowered to 1. (dt = -1.0), and the flux-splitting flag, ifds, needs to be set to 0 in each of the three directions. In addition, to compensate for the lower CFL number, 1000 fine-level iterations were used, rather than 750.
- If you try to switch the turbulence model and run, for example, with
SST, it is necessary to limit the maximum eddy viscosity by
employing the keyword
**edvislim**and setting it to, say, 100000.

A complete description of this case, along with additional computational grids may be found in the MADIC Wing Body Test Archive. The case considered here is the one corresponding to an angle of attack of 2.873 degrees, Mach 0.8027, and a chord Reynolds number of 13.1 million. The Spalart-Allmaras turbulence model is employed. This test case utilizes point-matched grids; the following case uses the same geometry, but employing overset (chimera) grids. The following figures illustrate the case:

Then type:

This will create a subdirectory "ARA_M100".

Case | No. Processors | Run Time | Memory | Convergence History | Test Date | Test Machine |
---|---|---|---|---|---|---|

1 Block | 1 | 6 hr, 34 min | 357.0 MB |
cfl3d.res plot |
Sep 10 03 | Linux Workstation^{6} |

1 Block FVS |
1 | 73 hr, 55 min | 357.0 MB |
cfl3d.res plot |
Aug 01 02 | Origin 2000^{4} |

16 Block | 8 (+ host) | 2 hr, 20 min | 46.1 MB (per proc) |
cfl3d.res plot |
Jul 23 02 | Origin 2000^{4} |

Case | Plots | Exp. Data |
---|---|---|

1 Block | Cp vs x/c | exp.dat |

1 Block FVS |
Cp vs x/c | exp.dat |

FORTRAN program |

The FORTRAN program will extract the computed
results for the **1 block case** from the plot3d files generated
by CFL3D (with **nplot3d = -1**) and the experimental
data files. The output is a formatted TECPLOT file, which should
be easily adapted to other plotting packages as well.

__ARA M100 WING-BODY (overset grid)__

- Description:
- Download tar file ARA_M100_XMERA.tar.Z (12.9 MB)
**gunzip ARA_M100_XMERA.tar.Z****tar -xvf ARA_M100_XMERA.tar**- The tar file contains the following items:
**m100_xmera_6blk.fmt**- 6-block "chimera" grid (plot3d, multigrid, whole, formatted)

block 1 dimensions i x j x k = 161 x 25 x 49

block 2 dimensions i x j x k = 217 x 21 x 49

block 3 dimensions i x j x k = 217 x 21 x 49

block 4 dimensions i x j x k = 145 x 21 x 49

block 5 dimensions i x j x k = 73 x 73 x 41

block 6 dimensions i x j x k = 73 x 41 x 41 **cfl3d.inp_xmera**- cfl3d input file for the 6-block chimera grid
**split.inp_xmera**- input to block splitter that converts the 6-block formatted grid to a 6-block unformatted grid that can be read by CFL3D
**peg41.inp**- input to PEGSUS
**4.1**that generates the overset grid connectivity file "XINTOUT". The conversion tool p3d_to_INGRID can be used to convert the formatted grid-point file into the unformatted cell-center file "INGRID" file that is input to PEGSUS. The conversion tool XINTOUT_to_ovrlp can be used to convert the output file from PEGSUS to the "ovrlp.bin" file required by CFL3D for the chimera-grid case - To run the overset-grid case using PEGSUS to generate the
overset connectivity file, compile PEGSUS as appropriate (in the
instructions below, it is assumed the PEGUS executable is called
pegsus41). You will also need a couple of utilities from the cfl3d tools
directory, so make sure you have compiled cfl3d_tools. Then type:
(user inputs shown in
**bold**, interactive prompts for input shown in*italics*) - To run the case on a single processor, type:
- To run the case on 6 processors (+ 1 host),type:
- Expected Results:
- Comparison with experimental data:
- Notes:
- Mesh sequencing cannot be used with overset grids in CFL3D.
- If you try to switch the turbulence model and run, for example, with
SST, it is necessary to limit the maximum eddy viscosity by
employing the keyword
**edvislim**and setting it to, say, 100000.

A complete description of this case, along with additional computational grids may be found in the MADIC Wing Body Test Archive. The case considered here is the one corresponding to an angle of attack of 2.873 degrees, Mach 0.8027, and a chord Reynolds number of 13.1 million. The Spalart-Allmaras turbulence model is employed. This test case utilizes overset (chimera) grids; the preceding case uses the same geometry, but employing point-matched grids. The off-body grids differ between the two cases, although the wing surface grids are identical. The following figures illustrate the case:

Then type:

This will create a subdirectory "ARA_M100_XMERA".

file defaults:input grid files are plot3d typeinput grid files are unformattedoutput INGRID/plot3d file is unformatteddo you wish to use these defaults (y/n)?(alternate options include formattedfiles and cfl3d-type input grid files)ychoose the type of output file to createenter 0 to create an INGRID file (for PEGSUS 4.x)enter 1 to create a plot3d file (for PEGSUS 5.x)0enter the name of the output file to create (up to 80 char.)INGRIDenter 0 to create an output file with grid pointsenter 1 to create an output file with augmented cell centers1enter 0 to preserve input-grid i,j,k index definitions in the output gridyou may want this option if you have an existing PEGSUS input file thatwas generated for OVERFLOWNote: this will require the following translation ofindicies between CFL3D and PEGSUS input files:PEGSUS CFL3DJ = IK = JL = Kenter 1 to swap input-grid i,j,k index definitions in the output gridNote: this will require NO translation ofindicies between CFL3D and PEGSUS input files:PEGSUS CFL3DL = IJ = JK = K1enter number of separate grid files to convert into one output file1enter 0 to specify a name for each meshenter 1 to use default names (grid.n)0beginning processing of grid file number 1input name of unformatted plot3d grid file to read (up to 80 characters)m100_xmera_6blk.unfenter 0 if a single-grid plot3d fileenter 1 if a multiple-grid plot3d file1required array sizes: maxbl = 6lmax = 218jmax = 74kmax = 50input name (up to 40 char.) for zone 1FUSEreading zone 1input dimensions 161 25 49writing zone 1 with name FUSEoutput dimensions 26 50 162done writing grid 2*1input name (up to 40 char.) for zone 2WING_INreading zone 2input dimensions 217 21 49writing zone 2 with name WING_INoutput dimensions 22 50 218done writing grid 2*2input name (up to 40 char.) for zone 3WING_OUTreading zone 3input dimensions 217 21 49writing zone 3 with name WING_OUToutput dimensions 22 50 218done writing grid 2*3input name (up to 40 char.) for zone 4BOX1reading zone 4input dimensions 145 21 49writing zone 4 with name BOX1output dimensions 22 50 146done writing grid 2*4input name (up to 40 char.) for zone 5BOX2reading zone 5input dimensions 73 73 41writing zone 5 with name BOX2output dimensions 74 42 74done writing grid 2*5input name (up to 40 char.) for zone 6BOX3reading zone 6input dimensions 73 41 41writing zone 6 with name BOX3output dimensions 42 42 74done writing grid 2*6conversion of grid file 1 completeconversion of all grid files completedthe INGRID output file:INGRIDcontains (augmented) cell centers of the input grid(s)note: the mesh names in the INGRID file contain 40 charactersmake sure the PEGSUS parameter ICHAR is set to 40

enter 4 if pegsus version 4.X was usedenter 5 if pegsus version 5.X was used4enter the name of the COMPOUT file created by PEGSUS(unless you have renamed it, enter COMPOUT)COMPOUTenter 0 to leave overset data as 3denter 1 to convert overset data to 2d (2 i-planes)0enter 0 to use the maggie/CFL3D-ijk index definitionenter 1 to use the pegsus/OVERFLOW-jkl index definition0(additional output from XINTOUT_to_ovrlp is omitted... no further user input is needed)

Case | Plots | Exp. Data |
---|---|---|

6 Block | Cp vs x/c | exp.dat |

FORTRAN program |

The FORTRAN program will extract the computed
results for the **6 block case** from the plot3d files generated
by CFL3D (with **nplot3d = -1**) and the experimental
data files. The output is a formatted TECPLOT file, which should
be easily adapted to other plotting packages as well.

- Description:
- Download tar file Delta_cgns.tar.Z (1.65 MB)
**gunzip Delta_cgns.tar.Z****tar -xvf Delta_cgns.tar**- The tar file contains the following items:
**delta.fmt**- single-block grid (plot3d type, formatted) of dimensions i x j x k = 37 x 65 x 65
**delta_cgns.inp**- CFL3D input file - note keyword input "icgns 1" and "delta.cgns" CGNS file used as grid name input
**plot3dg_to_cgns.inp**- input to plot3dg_to_cgns tool that converts the single-block formatted grid to a CGNS grid file
- To run the case, use the following steps:
- Expected Results:
- How to view CGNS file:
- Notes:
- When using a CGNS grid file, NGRID (whose sign usually determines whether a grid of type CFL3D or PLOT3D is being read) in the delta_cgns.inp input file can be either + or -; i.e., its sign is irrelevant.
- If someone supplies you with a CGNS grid file, then the
initial translation step (step 2, using plot3dg_to_cgns) is unnecessary.
However, you must still create a CFL3D input file, including any 1-to-1
and BC information. The code
**cgns_to_cfl3dinput.F**in the Tools/ directory can help obtain a first-guess skeleton input file, with most of the needed relevant information in it. - Although not used for this delta wing case, note that PATCHING and OVERSET information have not yet been included in the CGNS-part of CFL3D. I.e., the CGNS files are purposefully missing this information. The user can still run patched and overset cases with CGNS, but the patched/overset connectivity information is never put into the CGNS file itself. This is similar to the "normal" mode of running CFL3D. In the "normal" mode, the user must have available a grid file, restart file, patched-info file, and overset-info file when running with patched/overset. With CGNS, the user must have available a CGNS file, patched-info file, and overset-info file.
- CFL3D can be installed with CGNS using "Install -cgnsdir=...", even if you plan to only rarely use CGNS. By default, the keyword input "icgns" is zero (meaning no CGNS). The user must set "icgns 1" in the CFL3D input file in order to turn on the CGNS capability.

Subsonic laminar flow past a delta wing at 20.5 degrees angle of attack is modeled at a Reynolds number of 0.5 million and and Mach number of 0.3. This case is given to demonstrate the CGNS capability in CFL3D. CGNS stands for CFD General Notation System. It is a method for standardizing CFD input and output, including grid, flow solution, connectivity, BC's, and auxiliary information. The method is in the process of becoming an international ISO standard. It is machine-independent, and will eventually eliminate most of the translator programs now necessary when working between machines and between CFD codes. Also, it eventually may allow for the results from one code to be easily restarted using another code. See the CGNS link on the Index bar of the CFL3D web page for more information. For this particular case, a grid size of 37x65x65 was used. The following figures illustrates the case:

Then type:

This will create a subdirectory "Delta_cgns".

**Step 1:**

Go to www.cgns.org and download CGNS (under "Download the Software"), and follow the instructions to compile it for your machine. The CGNS library is freely available open software. Be sure to download the latest version of the CGNS library. Ultimately, you should end up with a directory called something like: cgnslib_x.x/. In here you should have a file called cgnslib_f.h, and the compiled library libcgns.a should be in a subdirectory appropriately named for whatever system you are running on. See the Install file (in the build directory) under "CGNS_LLIBDIR=" for the subdirectory names currently expected by CFL3D for each machine. It is not guaranteed that this default name is correct... you may need to change this default name, depending on what name is created by the CGNS software for your machine.

When you install CFL3D, use the command "Install -cgnsdir=...", where "..." specifies the location of the cgnslib_x.x/ directory (for example: Install -cgnsdir=../../bin/cgnslib_x.x). If you have already installed CFL3D without CGNS, you must re-install it.

**Step 2:**

Be sure to make cfl3d_tools in the build directory, so that the tool "plot3dg_to_cgns" is created. Then type:

(translates formatted grid file in PLOT3D format to CGNS grid file named delta.cgns). Note that a small change was made to the plot3dg_to_cgns.F code prior to the general release of CFL3D Version 6.4; this change requires an additional line of input. Therefore, if the above command yields an error, be sure that you have the latest version of plot3dg_to_cgns.F.

**Step 3:**

Next, type:

Running with CGNS means that one file (the CGNS file) contains the grid, solution, and all necessary restart information. Thus, the "restart.bin" file is not needed, although it is still kept in the input file. Note that you can make use of links in CGNS in order to have the grid as a separate file from the solution file, if desired. But in this case everything is still accessed through a single file name. If your post-processing software supports CGNS, then you can plot results directly from the CGNS file also! However, note that CFL3D currently still outputs standard PLOT3D-type files for postprocessing, if desired.

After running CFL3D, the file delta.cgns will contain the grid and flow solution. (If desired, the final resulting CGNS file for this case can be obtained from the following link: delta.cgns.gz (8.07 MB).)

The delta.cgns CGNS file can be viewed using special CGNS
viewing software, "adfviewer," available from www.cgns.org.
The adfviewer software displays the CGNS file, and allows the user to
query and even manipulate it. A sample screen is shown in the
adfviewer screen.
Additional details can be found by clicking on the CGNS link on the Index bar to the left.
However, it is not necessary to be able to view the CGNS file; it
can be treated simply as a restart file (like the usual restart.bin file).
But it is better than the usual restart file because it contains more
archival information (including date-stamping, comments on how the solution was
obtained, BC information, and a record of the input file(s) employed).

- Test Platforms

Test Platform No. | Type | Vita | Notes |
---|---|---|---|

1 | SGI Origin 2000 | 32 procs @250 MHz 4MB Lev2 cache 24.5GB RAM total |
timings vary with system load |

2 | SGI Origin 2000 | 4 procs @250 MHz 4MB Lev2 cache 4.6GB RAM total |
timings vary with system load |

3 | SGI Origin 2000 | 8 procs @250 MHz 4MB Lev2 cache 9.2GB RAM total |
timings vary with system load |

4 | SGI Origin 2000 | 16 procs @250 MHz 4MB Lev2 cache 16.3GB RAM total |
timings vary with system load |

5 | SGI Octane2 | 2 procs @360 MHz 2MB Lev2 cache 2.3GB RAM total |
timings vary with system load |

6 | Linux Workstation | 2 procs @2.4 GHz 2GB DDR RAM total |
various compilers used |

7 | Linux Workstation | 2 dual-core procs @3.0 GHz 4GB FB-dims RAM total |
various compilers used |

**Responsible NASA Official:**
Christopher Rumsey

**Page Curator:**
Christopher Rumsey

**Last Updated:** 08/22/2014