NPARC Alliance Validation Archive
Validation Home   >   Archive   >   RAE 2822 Transonic Airfoil   >   Study #1

RAE 2822 Transonic Airfoil: Study #1

Figure 1 is described in the surrounding text
Figure 1. The Mach number contours for the RAE 2822 transonic airfoil.

Introduction

This study is an example study demonstrating the use of WIND and accompanying programs for computing two-dimensional turbulent, transonic flows about an airfoil. Further, this study is a re-baseline of the documented validation case for the NPARC code. Those validation results can be found at the NPARC Validation Web page. The pressure coefficients obtained from the computation from WIND are compared to the values obtained by RAE as reported in Ref. 1. The values obtained from the NPARC validation study are also included in the comparison.

Download tar File

All of the archive files of this validation case are available in the Unix compressed tar file raetaf01.tar.Z. The files can then be accessed by the commands:

uncompress raetaf01.tar.Z
tar -xvof raetaf01.tar

Grid

The grid is a single-block, two-dimensional C-grid with dimensions of 369 x 65. It is contained in a PLOT3D grid file named raetaf.x.fmt (formatted, single-zone, 2D, whole). The airfoil surface and wake are located at the J1 boundary. The I-coordinate starts at the lower downstream boundary, intersects the trailing edge at I33, proceeds along the bottom of the airfoil, around the leading edge, downstream along the top of the airfoil, intersects the trailing edge again at I337, and continues to the outflow boundary. The JMAX grid line is the farfield boundary of the flow domain. The grid is non-dimensionalized by the chord length. Since WIND requires dimensional quantities and assumes English Engineering units, the airfoil grid is assumed to have a chord of 1.0 ft.

The CFCNVT utility is used to convert the PLOT3D grid file to the common grid file format (.cgd) for WIND. This is done using the command:

cfcnvt < cfcnvt.x.com

where the file cfcnvt.x.com is a command input file. A common grid file named raetaf.cgd is created. For simulating planar flows in WIND, the three-dimensional flow equations are applied. This requires that the grid plane be in the z = 1.0 plane. The CFCNVT utility creates the proper three-dimensional grid with KMAX = 1.

Initial Conditions

This study assumes freestream flow conditions as summarized in Table 1 below. These conditions correspond to a Reynolds number of 6.5 million based on the chord length of 1.0 ft. The static pressure was computed based on the specified Reynolds number and Mach number and an assumed value of static temperature.

Table 1. Freestream conditions.
Mach number Static Pressure (psia) Temperature(R) Angle-of-Attack (deg)
0.729 15.80734 460.0 2.31

The computational flow field is initialized with uniform flow corresponding to these freestream conditions.

Boundary Conditions

The boundary conditions must now be specified for the grid and this is done with the GMAN utility. First, the boundary condition types are summarized. A VISCOUS WALL boundary condition is applied at the J1 boundary at the airfoil surface, which extends from I33 to I337. The J1 boundary from I1 to I32 is coupled to the J1 boundary from I338 to IMAX (I369) to form the wake region. A FREESTREAM boundary condition is applied at the JMAX boundary, which should all be subsonic inflow at the freestream conditions. The I1 and IMAX boundaries are specified as OUTFLOW boundaries. The OUTFLOW allows the static pressure to be directly specified and is assumed to be equal to the freestream pressure.

The procedure for setting the boundary conditions using GMAN with the graphics interface is as follows:

  1. Start GMAN.
  2. gman
  3. Select the version of GMAN by accepting the default of 1) gman optimized version.
  4. Read in the common grid file by typing at the GMAN prompt.
  5. file raetaf.cgd
  6. Specify that units are feet / slugs / seconds.
  7. units fss
  8. Switch to graphics mode.
  9. swi
  10. Display the grid.
  11. Pick SHOW (upper right panel)
    Pick SHOW SURFACES
    Pick PICK K-PLANE

    At this point the grid will be displayed since there is only one grid plane, K=1. Moving the mouse so that the cross-cursor is near the upper-right most grid point and clicking the left mouse button will cause the coordinates of that point to be displayed in the middle right panel. It should indicate that the coordinates of point (369,65,1) are x = 27.0 ft, y = 24.2635 ft, and z = 1.0 ft. Note that the units are feet, which was desired from the units fss command. Also note that CFCNVT had converted the initial two-dimensional grid to a three-dimensional grid with z = 1.0 ft, which is required by WIND.

  12. Specify the boundary conditions.
  13. Pick BOUNDARY COND. (left panel)

    GMAN defaults to zone 1 since it is the only zone. The sequence is to select the boundary and specify the boundary condition type on that boundary. The initial boundary condition type is UNDEFINED. Since there is only one zone, GMAN defaults to picking zone 1. It is now waiting for the boundary to be specified.

    Pick I1 (lower left panel)

    At this point, the I1 grid plane is displayed. Since this case is planar, a line is displayed. To select the boundary condition type, execute the following menu choices:

    Pick MODIFY BNDY
    Pick CHANGE ALL
    Pick OUTFLOW

    At this point, the bottom panel should contain the text "65 points were changed". The boundary condition specification is now saved for this boundary by the following menu choices:

    Pick BOUNDARY COND. (top left panel)
    Pick YES-UPDATE FILE (middle left panel)

    The common grid file raetaf.cgd is modified to include this boundary condition specification.

    The boundary condition specification can be checked by selecting:

    Pick IDENTIFY PNTS. (left panel)
    Pick OUTFLOW

    The individual grid points will show up in color to indicate that those points are specified as OUTFLOW.

    The boundary conditions for the IMAX boundary are set in a similar manner. For the IMAX boundary,

    Pick BOUNDARY COND. (top left panel)
    Pick PICK ZONE/BNDY
    Pick 1 (from zone list)
    Pick IMAX
    Pick MODIFY BNDY
    Pick CHANGE ALL
    Pick OUTFLOW
    Pick BOUNDARY COND.
    Pick YES-UPDATE FILE

    The J1 boundary contains both the wake region and the airfoil surface. First, select the J1 boundary,

    Pick BOUNDARY COND. (top left panel)
    Pick PICK ZONE/BNDY
    Pick 1 (from zone list)
    Pick J1

    Now the boundary conditions will be specified for the wake region on the J1 boundary from I1 to I32, which will be coupled to the J1 boundary from I338 to I369. First, define a work subarea for I1 to I32,

    Pick Work Subarea (lower right box)

    A prompt will appear is the bottom center box asking for start and end i indices for the subarea.

    Enter the first index, 1 [ret]
    Enter the second index, 32 [ret]

    In the lower right panel, it should indicate that the work area is now (1) - (32). The boundary conditions on these points will now be specified as being coupled to the J1 boundary,

    Pick MODIFY BNDY
    Pick COUPLE
    Pick SEL OTHER BND
    Pick 1 (from zone list)
    Pick J1
    Pick COUPLE
    Pick BOUNDARY COND.
    Pick YES-UPDATE FILE

    The bottom panel will indicate that "32 undefined points were changed" and that "Boundary conditions have been updated".

    Now the subarea is defined for the airfoil surface and the boundary conditions are specified as viscous walls,

    Pick Work Subarea (lower right box)
    Enter the first index, 33 [ret]
    Enter the second index, 337 [ret]
    Pick MODIFY BNDY
    Pick CHANGE ALL
    Pick VISCOUS WALL
    Pick BOUNDARY COND.
    Pick YES-UPDATE FILE

    The bottom panel will indicate that "305 undefined points were changed" and that "Boundary conditions have been updated".

    Now the subarea is defined for the wake region from I338 to I369 which is coupled to the J1 boundary,

    Pick Work Subarea (lower right box)
    Enter the first index, 338 [ret]
    Enter the second index, 369 [ret]
    Pick MODIFY BNDY
    Pick COUPLE
    Pick SEL OTHER BND
    Pick 1 (from zone list)
    Pick J1
    Pick COUPLE
    Pick BOUNDARY COND.
    Pick YES-UPDATE FILE

    The bottom panel will indicate that "32 undefined points were changed" and that "Boundary conditions have been updated".

    The boundary condition types for the J1 boundary can be checked,

    Pick IDENTIFY PNTS. (left panel)
    Pick VISCOUS WALL
    Pick ZONE 1 J1

    The "ZONE 1 J1" indicates that the boundary grid points are coupled to boundary J1 of zone 1. Note that all we had to specify was which boundary the grid points are coupled and not the specific grid points. This is automatically determined within GMAN.

    The boundary conditions for the JMAX boundary are now specified in a similar manner as above,

    Pick BOUNDARY COND. (top left panel)
    Pick PICK ZONE/BNDY
    Pick 1 (from zone list)
    Pick JMAX
    Pick MODIFY BNDY
    Pick CHANGE ALL
    Pick FREESTREAM
    Pick BOUNDARY COND.
    Pick YES-UPDATE FILE

    While computationally there exists K1 and KMAX boundaries, which are both K1, they do not need to be specified for planar problems.

  14. Exit GMAN.
  15. Pick TOP (top left panel)
    Pick END
    Pick YES-TERMINATE

    The common grid file raetaf.cgd is now ready.

As GMAN operates, a journal file gman.jou is created which can later be used as a command file to re-run GMAN. Here this file has been renamed gman.com and GMAN can be re-run as:

gman < gman.com

Creating a command file from scratch represents an alternative to the graphical approach within GMAN. Further, it can be easily modified when the grid changes, such as for grid refinement studies.

Computation Strategy

The computation is performed using the time-marching capabilities of WIND to march to a steady-state (time asymptotic) solution. Local time stepping is used at each iteration. The time-marching is performed until convergence criteria is achieved.

Input Parameters and Files

The input data file for WIND is raetaf.dat. The freestream keyword indicates that the static freestream flow conditions are specified as Mach number, pressure (psia), temperature (R), angle-of-attack (degrees), and angle-of-sideslip (degrees). The downstream pressure keyword indicates that the freestream static pressure is to be used at the OUTFLOW boundaries. The turbulence model keyword indicates that the Spalart-Allmaras turbulence model is to be used. The implicit boundary keyword indicates that implicit boundary conditions are to be used on the viscous walls. The dq limiter keyword indicates that the change is solution is limited over an iterations. The loads keyword indicates that the lift on the airfoil is to be integrated every 10 iterations and displayed in the list file. This will be used to evaluate the convergence of the solution. The converge order keyword indicates that the computation will stop if the L2 norm of the solution drops by 9 orders-of-magnitude. The cycles keyword indicates that 500 cycles will be run. The iterations per cycle keyword indicates that 10 iterations will be run per cycle with a print frequency of 5 iterations. The cfl keyword indicates that a CFL number of 5.0 will be used. By default, WIND uses CFL number to determine the local time-step size.

Computation

The WIND solver is run by entering:

wind -runinplace

This runs the wind script which sets up the problem for solver. The runinplace option indicates that WIND is to be run in the current directory. Further details and options for the wind script can be found in the WIND documentation (wind script). A brief description of script options can be listed by typing:

wind -help

Some initial interactive prompts ask for information to set up the computation. First, enter a return to run the latest version.


Running command line version of WIND.

          
         
***** WIND Run Script *****

Current wind settings are:

--Wind test mode set to NODEBUG
--Wind debugger set to DEFAULT
--Wind run que set to PROMPT
--Wind run in place mode is set to NO
--Wind multi-processor mode set to NO
--Wind run directory set to PROMPT
--Wind bin directory set to /net/zargon/usr2/wind-1.0/wind
 
         
        Select the desired version
 
  0: Exit wind
  1: alpha version
  2: Version 2.0
  3: Version 3.0
  4: Version 4.0
  5: Version 5.0


Enter number or name of executable.......[5]: 5

The next question will ask for the name of the input data file. Enter the name without the "dat" file extension. So, for this case, enter:

raetaf
Enter number or name of executable.......[1]: 1
Basic input data................(*.dat): raetaf

The next few questions ask about "Output data", "Mesh file", and "Flow data file" file names. Entering a carriage return will select the default names. A common flow data file raetaf.cfl does not currently exists, so WIND initialize the flow from the freestream conditions and creates the new flow data file.

Output data.............(*.lis,<CR>=raetaf): 
Mesh file...............(*.cgd,<CR>=raetaf): 
Flow data file..........(*.cfl,<CR>=raetaf): 
 
***********************************************************
raetaf.cfl does not exist, a fresh start will be performed.
***********************************************************

The next question allows a choice between running the solution in real-time (interactive) or submitting it to a queue. First, try running it interactively by selecting 1.

Enter a queue number from the following list or <CR> for default:
  1: REAL (interactive)
  2: AT_QUE

Queue name.......................(<CR> for 1):

The next questions asks whether the output should be written to the screen or to a list file raetaf.lis. Enter n to create a list file.

Print output at screen?....................(y/n,[cr]=y): n

Some file information will be displayed.

Version...............: /net/zargon/usr2/wind/wind/SGIMP6.5/R12000/wind5.exe
Input file name.......: raetaf.dat
Wind output to........: raetaf.lis
Grid file name........: raetaf.cgd
Flow file name........: raetaf.cfl
Job run que type is...: REAL

A final carriage return will cause the job to be submitted.

  Press [cr] to submit job, another key (except space) and [cr] to abort:

The list file is raetaf.lis and contains the output from the computation and lists the residual information for both the flow equations and the turbulence model equation for each iteration. The integrated lift is also output every 10 iterations.

The flow data file is raetaf.cfl and contains the final solution.

Convergence

There are several ways to examine the convergence of the solution. The RESPLT utility is used for these to read information from the list file raetaf.lis. First the L2 norm of the residual of the conservation variables (change over a time step) can be read from the list file,

resplt < resplt.nsl2.com

The file resplt.nsl2.com is a command file containing the inputs for RESPLT to output the GENPLOT formatted plot data file named nsl2.gen of the residuals as a function of the iterations. This file can be plotted using CFPOST,

cfpost < cfpost.nsl2.com

where the file cfpost.nsl2.com is a command file containing the inputs for CFPOST. Fig. 2 shows the solution residual that is displayed by CFPOST.

Figure 2 is described in the surrounding text
Figure 2. Plot of the L2 solution residual history.

The convergence information for the Spalart-Allmaras turbulence variable can be obtained from the list file using RESPLT,

resplt < resplt.sal2.com

The file resplt.sal2.com is a command file containing the inputs for RESPLT to output the GENPLOT formatted plot data file named sal2.gen of the residuals as a function of the iterations. This file can be plotted using CFPOST,

cfpost < cfpost.sal2.com

where the file cfpost.sal2.com is a command file containing the inputs for CFPOST. Fig. 3 shows the turbulence residual that is displayed by CFPOST.

Figure 3 is described in the surrounding text
Figure 3. Plot of the L2 turbulence residual history.

A more significant indicator of solution convergence is to examine the convergence of the engineering quantity to be obtained from the analysis. Here it is lift and drag on the airfoil. The loads keyword in the input data file raetaf.dat output this information into the list file raetaf.lis. RESPLT is used to read this information and create plot files,

resplt < resplt.liftconv.com

The file resplt.liftconv.com is a command file containing the inputs for RESPLT to output the GENPLOT formatted plot data file named liftconv.gen of the residuals as a function of the iterations. This file can be plotted using CFPOST,

cfpost < cfpost.liftconv.com

where the file cfpost.liftconv.com is a command file containing the inputs for CFPOST. CFPOST will display in sequence the plots for drag, lift, and z-direction force. Fig. 4 and 5 shows the convergence of the drag and lift as displayed by CFPOST.

Figure 4 is described in the surrounding text
Figure 4. Plot of the sectional drag on the airfoil with iterations.

Figure 5 is described in the surrounding text
Figure 5. Plot of the sectional lift on the airfoil with iterations.

Post-Processing

The CFPOST utility can be used to generate engineering information from the the data files. First, the PLOT3D files can be obtained for displaying in FAST,

cfpost < cfpost.plot3d.com
fast fast.com

The PLOT3D grid file created is named raetaf.x and the solution file is raetaf.q. Both are unformatted, whole, 3D, and single-block. The FAST command file fast.com will read these files, calculate the pressure and Mach number and display the pressure contours. Fig. 6 shows the pressure contours near the airfoil.

Figure 6 is described in the surrounding text
Figure 6. The pressure contours near the RAE 2822 transonic airfoil.

For an airfoil calculation, one piece of important information is the distribution of pressure coefficients on the airfoil. CFPOST can directly output and plot this information,

cfpost < cfpost.cp.com

where cfpost.cp.com is the command input file for CFPOST. A GENPLOT file named cp.wind.gen is created and plotted. The pressure coefficient is negative for pressures less than freestream, which occurs on the top of the airfoil. In plots of pressure coefficients for airfoils, the negative of the pressure coefficient is usually plotted to indicate that the lower pressure region is on the top of the airfoil and the high pressure region is on the bottom of the airfoil. This is done in the CFPOST command file cfpost.cp.com.

Pressure coefficient data from a wind tunnel experiment is available for comparison and is in the GENPLOT file cp.exp.gen. Fig. 7 presents the comparison between the experiment data and WIND. Also plotted are the results from earlier computations using the NPARC code, which are contained in the GENPLOT file cp.nparc.gen.

Figure 7 is described in the surrounding text
Figure 7. Plot of the pressure coefficients on the airfoil.

For an airfoil calculation, another piece of important information is the forces on the airfoil which result from pressure and skin-friction. CFPOST can be used to integrate these forces over the surface of the airfoil,

cfpost < cfpost.forces.com

where cfpost.forces.com is the command input file for CFPOST. A list file named forces.lis is created in which the force information is printed.

The skin friction coefficients along the surface of the airfoil can be computed,

cfpost < cfpost.cf.com

where cfpost.cf.com is the command input file for CFPOST. A GENPLOT file named cf.wind.gen is created in which the skin friction coefficients are listed.

For a viscous computation, it is useful to examine how well the boundary layers were resolved. One measure of this is the y+ values at the grid points in the boundary layers. The list file forces.lis does contain information on the y+ values throughout the grid. To examine the boundary layer at a certain location, CFPOST can be used.

cfpost < cfpost.bl.com

The file cfpost.bl.com is a command file which writes out the x and y coordinates, u-velocity, v-velocity, and temperature at I330, which is on the top of the airfoil just before the trailing edge bl.gen.

Comparisons of the Results

Figure 7 shows the comparisons of the computed surface pressure coefficients with NPARC and experimental results. The WIND results follow the trend of the NPARC results with a slight improvement in the capture of the shock on the upper surface.

Sensitivity Studies

No sensitivity studies were performed.

References

1. Cook, P.H., M.A. McDonald, M.C.P. Firmin, "Aerofoil RAE 2822 - Pressure Distributions, and Boundary Layer and Wake Measurements," Experimental Data Base for Computer Program Assessment, AGARD Report AR 138, 1979.

Contact Information

This study was created on September 30, 1998 and updated on December 17, 2002 by John W. Slater, who may be contacted at:

NASA John H. Glenn Research Center, MS 86-7
21000 Brookpark Road
Cleveland, Ohio 44135
Phone: (216) 433-8513
e-mail: John.W.Slater@grc.nasa.gov

Last Updated: Friday, 11-Jul-2008 12:52:08 EDT