CONTENTS
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.
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
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 Workstation6 |
| 15-deg skew grid | 1 | 13 min | 13.9 MB |
cfl3d.res plot |
July 21 04 | Linux Workstation6 |
| 30-deg skew grid | 1 | 13 min | 13.9 MB |
cfl3d.res plot |
July 21 04 | Linux Workstation6 |
| 45-deg skew grid | 1 | 13 min | 13.9 MB |
cfl3d.res plot |
July 21 04 | Linux Workstation6 |
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.
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 Workstation7 |
| SA, y+=0.23 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation7 |
| SA, y+=0.51 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation7 |
| SA, y+=1.15 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation7 |
| SA, y+=2.3 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation7 |
| SA, y+=4.6 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation7 |
| SST, y+=0.02 | 1 | 6 min | 13.9 MB |
cfl3d.res plot |
Feb 28 07 | Linux Workstation7 |
| SST, y+=0.23 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation7 |
| SST, y+=0.51 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation7 |
| SST, y+=1.15 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation7 |
| SST, y+=2.3 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation7 |
| SST, y+=4.6 | 1 | 6 min | 13.9 MB | cfl3d.res | Feb 28 07 | Linux Workstation7 |
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.
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.
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 | Octane25 |
| Weak Shock, EASM-ko | 1 | 5 min | 7.2 MB | cfl3d.res | March 21 03 | Octane25 |
| Strong Shock, SA | 1 | 2.3 min | 6.8 MB |
cfl3d.res plot |
September 9 03 | Linux Workstation6 |
| Strong Shock, EASM-ko | 1 | 2.5 min | 7.2 MB | cfl3d.res | September 9 03 | Linux Workstation6 |
| 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.
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 type
input grid files are unformatted
output INGRID/plot3d file is unformatted
do you wish to use these defaults (y/n)?
(alternate options include formatted
files and cfl3d-type input grid files)
y
choose the type of output file to create
enter 0 to create an INGRID file (for PEGSUS 4.x)
enter 1 to create a plot3d file (for PEGSUS 5.x)
0
enter the name of the output file to create (up to 80 char.)
INGRID
enter 0 to create an output file with grid points
enter 1 to create an output file with augmented cell centers
1
enter 0 to preserve input-grid i,j,k index definitions in the output grid
you may want this option if you have an existing PEGSUS input file that
was generated for OVERFLOW
Note: this will require the following translation of
indicies between CFL3D and PEGSUS input files:
PEGSUS CFL3D
J = I
K = J
L = K
enter 1 to swap input-grid i,j,k index definitions in the output grid
Note: this will require NO translation of
indicies between CFL3D and PEGSUS input files:
PEGSUS CFL3D
L = I
J = J
K = K
1
enter number of separate grid files to convert into one output file
1
enter 0 to specify a name for each mesh
enter 1 to use default names (grid.n)
0
beginning processing of grid file number 1
input name of unformatted plot3d grid file to read (up to 80
characters)
4412_xmera.unf
enter 0 if a single-grid plot3d file
enter 1 if a multiple-grid plot3d file
1
required array sizes: maxbl = 3
lmax = 4
jmax = 226
kmax = 114
input name (up to 40 char.) for zone 1
wing
reading zone 1
input dimensions 2 225 57
writing zone 1 with name wing
output dimensions 226 58 4
input name (up to 40 char.) for zone 2
box1
reading zone 2
input dimensions 2 113 73
writing zone 2 with name box1
output dimensions 114 74 4
input name (up to 40 char.) for zone 3
box2
reading zone 3
input dimensions 2 49 113
writing zone 3 with name box2
output dimensions 50 114 4
conversion of grid file 1 complete
conversion of all grid files completed
the INGRID output file:
INGRID
contains (augmented) cell centers of the input grid(s)
note: the mesh names in the INGRID file contain 40 characters
make sure the PEGSUS parameter ICHAR is set to 40
pegsus41 < peg41.inp > peg41.out enter 4 if pegsus version 4.X was used
enter 5 if pegsus version 5.X was used
4
enter the name of the COMPOUT file created by PEGSUS
(unless you have renamed it, enter COMPOUT)
COMPOUT
enter 0 to leave overset data as 3d
enter 1 to convert overset data to 2d (2 i-planes)
1
enter 0 to use the maggie/CFL3D-ijk index definition
enter 1 to use the pegsus/OVERFLOW-jkl index definition
0
(additional output from XINTOUT_to_ovrlp is omitted...
no further user input is needed)
cfl3d_seq < cfl3d.inp_xmera &
| 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.
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 from
this should be the "+" step file
restart.bin_+a
enter second restart file to extract history data from
this should be the "-" step file
restart.bin_-a
enter step size
1.e-6
finite diffs to be calculated with central diffs
enter file name for output finite differences
Finite_Diff_1.e-6
enter 0 to output convergence of dcy/ddv,dcmy/ddv
enter 1 to output convergence of dcz/ddv,dcmz/ddv
0
| 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 25 |
| 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 | Octane25 |
| 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.
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.
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 | Octane25 |
| perturbation run | 1 | 3 min | 17.5 MB |
cfl3d.res |
Aug 6 02 | Octane25 |
| run to achieve periodicity | 1 | 6 hr, 16 min | 17.8 MB |
cfl3d.res plot |
Aug 6 02 | Octane25 |
| dt=0.2 | 1 | 3 min | 17.8 MB |
cfl3d.res |
Aug 6 02 | Octane25 |
| dt=0.1 | 1 | 6 min | 17.8 MB |
cfl3d.res |
Aug 6 02 | Octane25 |
| dt=0.05 | 1 | 13 min | 17.8 MB |
cfl3d.res |
Aug 6 02 | Octane25 |
| dt=0.025 | 1 | 26 min | 17.8 MB |
cfl3d.res |
Aug 6 02 | Octane25 |
| dt=0.0125 | 1 | 49 min | 17.8 MB |
cfl3d.res |
Aug 6 02 | Octane25 |
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.
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 | Octane25 |
| 129x65 grid | 1 | 1 hr, 22 min | 657.0 MB |
cfl3d.res |
Nov 9 02 | Octane25 |
| 257x129 grid | 1 | 7hr, 19 min | 659.0 MB |
cfl3d.res |
Nov 9 02 | Octane25 |
| 513x257 grid | 1 | 37 hr, 11 min | 661.0 MB |
cfl3d.res |
Nov 11 02 | Octane25 |
| 1025x513 grid | 1 | 179 hr, 13 min | 785.5 MB |
cfl3d.res plot |
Nov 18 02 | Octane25 |
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.
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.
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 | Octane25 |
| pitching | 1 | 4hr, 47 min | 60.3 MB |
cfl3d.res |
January 21 03 | Octane25 |
| pitching (continuation) |
1 | 25 min | 60.3 MB |
cfl3d2.res plot |
January 21 03 | Octane25 |
| 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:
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
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 Workstation7 |
| hump (unsteady, 7 cycles) | 1 | 4 hrs, 30 min | 292 MB |
cfl3d.res |
February 8 07 | Linux Workstation7 |
| hump (unsteady, 1 cycle) | 1 | 41 min | 303 MB |
cfl3d.res plot |
February 8 07 | Linux Workstation7 |
| 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.
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".
(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 | 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.
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.
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)
This case is from M. P. Carr and K. C. Pallister, "Pressure distributions measured on Research Wing M100 mounted on an axisymmetric body," AGARD AR-138-ADDENDUM, Addendum to AGARD AR 138, Experimental Data Base for Computer Program Assessment, July 1984. 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 Workstation6 |
| 1 Block FVS |
1 | 73 hr, 55 min | 357.0 MB |
cfl3d.res plot |
Aug 01 02 | Origin 20004 |
| 16 Block | 8 (+ host) | 2 hr, 20 min | 46.1 MB (per proc) |
cfl3d.res plot |
Jul 23 02 | Origin 20004 |
| 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)
This case is from M. P. Carr and K. C. Pallister, "Pressure distributions measured on Research Wing M100 mounted on an axisymmetric body," AGARD AR-138-ADDENDUM, Addendum to AGARD AR 138, Experimental Data Base for Computer Program Assessment, July 1984. 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 type
input grid files are unformatted
output INGRID/plot3d file is unformatted
do you wish to use these defaults (y/n)?
(alternate options include formatted
files and cfl3d-type input grid files)
y
choose the type of output file to create
enter 0 to create an INGRID file (for PEGSUS 4.x)
enter 1 to create a plot3d file (for PEGSUS 5.x)
0
enter the name of the output file to create (up to 80 char.)
INGRID
enter 0 to create an output file with grid points
enter 1 to create an output file with augmented cell centers
1
enter 0 to preserve input-grid i,j,k index definitions in the output grid
you may want this option if you have an existing PEGSUS input file that
was generated for OVERFLOW
Note: this will require the following translation of
indicies between CFL3D and PEGSUS input files:
PEGSUS CFL3D
J = I
K = J
L = K
enter 1 to swap input-grid i,j,k index definitions in the output grid
Note: this will require NO translation of
indicies between CFL3D and PEGSUS input files:
PEGSUS CFL3D
L = I
J = J
K = K
1
enter number of separate grid files to convert into one output file
1
enter 0 to specify a name for each mesh
enter 1 to use default names (grid.n)
0
beginning processing of grid file number 1
input name of unformatted plot3d grid file to read (up to 80
characters)
m100_xmera_6blk.unf
enter 0 if a single-grid plot3d file
enter 1 if a multiple-grid plot3d file
1
required array sizes: maxbl = 6
lmax = 218
jmax = 74
kmax = 50
input name (up to 40 char.) for zone 1
FUSE
reading zone 1
input dimensions 161 25 49
writing zone 1 with name FUSE
output dimensions 26 50 162
done writing grid 2*1
input name (up to 40 char.) for zone 2
WING_IN
reading zone 2
input dimensions 217 21 49
writing zone 2 with name WING_IN
output dimensions 22 50 218
done writing grid 2*2
input name (up to 40 char.) for zone 3
WING_OUT
reading zone 3
input dimensions 217 21 49
writing zone 3 with name WING_OUT
output dimensions 22 50 218
done writing grid 2*3
input name (up to 40 char.) for zone 4
BOX1
reading zone 4
input dimensions 145 21 49
writing zone 4 with name BOX1
output dimensions 22 50 146
done writing grid 2*4
input name (up to 40 char.) for zone 5
BOX2
reading zone 5
input dimensions 73 73 41
writing zone 5 with name BOX2
output dimensions 74 42 74
done writing grid 2*5
input name (up to 40 char.) for zone 6
BOX3
reading zone 6
input dimensions 73 41 41
writing zone 6 with name BOX3
output dimensions 42 42 74
done writing grid 2*6
conversion of grid file 1 complete
conversion of all grid files completed
the INGRID output file:
INGRID
contains (augmented) cell centers of the input grid(s)
note: the mesh names in the INGRID file contain 40 characters
make sure the PEGSUS parameter ICHAR is set to 40
pegsus41 < peg41.inp > peg41.out enter 4 if pegsus version 4.X was used
enter 5 if pegsus version 5.X was used
4
enter the name of the COMPOUT file created by PEGSUS
(unless you have renamed it, enter COMPOUT)
COMPOUT
enter 0 to leave overset data as 3d
enter 1 to convert overset data to 2d (2 i-planes)
0
enter 0 to use the maggie/CFL3D-ijk index definition
enter 1 to use the pegsus/OVERFLOW-jkl index definition
0
(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.
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:
plot3dg_to_cgns < plot3dg_to_cgns.inp(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:
cfl3d_seq < delta_cgns.inp &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 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: 01/19/2022
