PEGASUS has been developed and tested on SGI, LINUX, and Cray platforms. Every attempt has been made to conform to standard Fortran 90 conventions; therefore, compilation on other platforms with compliant Fortran 90 compilers should be straightforward.

To compile and install PEGASUS and all of the utility programs and scripts, follow these steps:

1. Run the configure script. Type "configure -help" to see a list of options. Examples include:

   configure --enable-dp	To enable double-precision
   configure --enable-mpi	To enable MPI parallel execution (See MPI Compilation below)
   configure --enable-mpilog	To enable MPI parallel exection with MPE logging
   configure --enable-mips2	SGI -mips2 compiler option
   configure --enable-mips3	SGI -mips3 compiler option
   configure --enable-mips4	SGI -mips4 compiler option
   configure --enable-debug	To enable debug compiler flags and output
   configure --with-pgi	Use Portland Group compilers
   configure --installdir=DIR	Executables will be installed in directory DIR

   
    
2. Compile: type "make"
    
3. Install: type "make CMD=install"

The executable will be named pegasus5.

It is recommended that PEGASUS be compiled and run in double precision when viscous grids are used. Running viscous cases in single precision has been seen to sometimes adversely affect the hole-generation process, and in some cases can affect interpolation as well.

3.1.1 MPI Compilation

As of version 5.1g, PEGASUS5 has a parallel execution option which utilizes Message-Passing Interface (MPI) standard. This option must be enabled when the code is compiled. Use of the --enable-mpi or the --enble-mpilog configure options will produce a peg/Makefile which enables MPI, and will produce an executable named pegasus5mpi. The MPI version of PEGASUS5 has been tested using the mpich implementation of MPI. The MPI version of the peg/Makefile utilizes mpif90, which is a script interface to your f90 compiler that is created when you install mpich. If another implemntation of mpi is to be used, you need to edit your peg/Makefile appropriately. See http://www-unix.mcs.anl.gov/mpi/mpich/ for more information about mpich. See Section 4.2 for information about running pegasus5mpi.

3.2 User Inputs

Two types of input must be supplied: the volume grids, and the standard input file. There are some utility codes, which are described in Section 3.3, which help in the preparation of this input. The details of these inputs are described in this section.

The individual volume grids are stored in a sub-directory within the project directory called X_DIR. See Section 3.5 for a description of the directory structure used by PEGASUS5 code. The grids are to be stored as unformatted, single-zone, PLOT3D grid files. These grid files are named "mesh_nameA.x", "mesh_nameB.x", etc, where mesh_nameA, mesh_nameB, ... correspond to the NAME variables in the $MESH namelists in the standard input file.

All of the user inputs to PEGASUS are read from the standard input. All inputs are in a form similar to FORTRAN NAMELISTS. The following is a list of all of the NAMELISTS defined in PEGASUS . Not all of these NAMELISTS have to be included in the input, and the order in which the NAMELISTS appear in the input does not matter. Most problems will only require input to be specified in the first three of these NAMELISTS:

• $GLOBAL
• $MESH
• $BCINP
• $HCUT
• $OUTER
• $BOUNDARY
• $SURFACE
• $BOX
• $REGION
• $VOLUME
• $LEVEL2

In the namelists which require grid indices, negative numbers can be used to specify indices relative to the last index. For example, an index of j=-1 is equivalent to j=jmax, j=-2 is equivalent to j=jmax-1, etc.

$GLOBAL

This input sets global values for all meshes. Each record can be overridden for any individual mesh by using the $MESH input. However, the mesh override is limited to that individual mesh. For subsequent meshes, the global values are used unless specifically overridden.
 

This input is like the BCINP namelist in the OVERFLOW flow solver. This namelist specifies all of the boundary conditions for each mesh. PEGASUS uses this information to automatically cut holes (based on the specification of the solid walls), and to automatically determine the outer boundary points which will require interpolation. It also uses these boundary conditions to determine certain mesh topologies, such as o-grid periodic meshes, 2D meshes, and symmetry planes.

This input specifies a group of meshes that be used to create a hole cutting boundary, as well as which meshes will be cut by this hole cutting boundary. Entries in the $BCINP namelist must be present for this method to work. Both solid boundary and symmetry plane information must be present in the $BCINP namelist for the meshes that are used for the hole cutting boundary. If no $HCUT namelist groups are specified and HCUT is equal to .TRUE. (in namelist group $GLOBAL), a hole cutting boundary will be created from all solid boundaries in all of the $BCINP namelists, and this hole cutting boundary will cut a hole in all meshes. There can be zero to many $HCUT namelist groups specified in the user inputs.

If this input is not specified and OUTER is equal to .TRUE. (in namelist group $GLOBAL) outer boundaries for all meshes will be specified automatically. This means that meshes which do not have boundary condition data given in the $BCINP namelist will have outer boundary points specified on all mesh faces. The $OUTER namelist group should be used only if a specific group of meshes needs to be included or excluded from automatic outer boundary specification. Only one $OUTER namelist group can be specified.

There are two types of BOUNDARY entities: a hole BOUNDARY and an outer BOUNDARY. To create a hole BOUNDARY, include the MHOLEIN variable in the namelist input and set it to a list of mesh names. Otherwise, if MHOLEIN is not included in the namelist, it will be an outer BOUNDARY. Any number of $BOUNDARY namelists may be included in the input.

A hole BOUNDARY has an associated set of one or more $SURFACE namelists, or a set of $BOX namelists. The $SURFACE namelist(s) define the surfaces that will bound the manual hole. The $BOX namelist(s) define a range of X, Y, and Z coordinates: any target grid points inside that range of coordinates will be turned into hole points.

A surface BOUNDARY has an associated set of one or more $SURFACE namelists, whose range of J, K, and L indices define an outer-boundary surface whose points require interpolation. In general, all outer-boundaries of meshes are determined automatically, and this is only used in special circumstances.

A SURFACE namelist must be associated with a BOUNDARY using the ISPARTOF variable.

A BOX namelist must be associated with a BOUNDARY using the ISPARTOF variable.

If this input is not specified and LEVEL2 is equal to .TRUE. (in namelist group $GLOBAL) "level 2" interpolation for all meshes will be specified automatically. The $LEVEL2 namelist group should be used only if a specific group of meshes needs to be included or excluded from "level 2" interpolation. Only one $LEVEL2 namelist group (INCLUDE or EXCLUDE) can be specified.

3.3 Utility Codes
 

Several utility codes are supplied with PEGASUS in the /tools directory:
 

• peg_setup
• peg_in
• peg_hole_surf
• p3d2peg
• make_WORK
• mesh_lister
• clean_holes
• peg_plot
• peg_plot_center
• peg_diag
• peg_hole
• peg_proj
• peg_orph
• peg_mem
• peg_sym
• XINtegrity
• dcintegrity
• XIN2sp
• cmpxint

peg_setup - This is a menu-driven script which gives the user options to initialize a PEGASUS problem, remove a PEGASUS problem, prepare to restart a PEGASUS run from the beginning, or redo the hole-cutting from the beginning. The first option requires that the user supply a multi-zone PLOT3D grid file containing all of the volume grids to be used. Also, you can supply an OVERFLOW input file to provide the boundary conditions. It executes mesh_lister, peg_in, make_WORK, p3d2peg, and peg_hole_surf. This option will split up the user-supplied multi-zone grid into individual meshes and place them in the X_DIR directory, ready for PEGASUS5. It creates a standard input file called peg.in.raw to help get you started. If an OVERFLOW input file is supplied, it will add the boundary condition data to the input file, and will also create a PLOT3D file of the solid surfaces of the configuration, called hcutter.g. This file makes it easy to plot and check that the solid-wall boundaries form a closed surface, which is necessary for the automatic hole cutting to work. See Section 4.2 for more information on the use of peg_setup.
 

The following six utility codes can be executed by running peg_setup, but can also be executed as stand-alone codes:

peg_in [-no_add_te] - Creates a minimal PEGASUS5 input file. It is written to a file called peg.in.raw with the intention that it be reviewed and edited if necessary before use. It requires the mesh_list file, which can be generated with the mesh_lister program. peg_in will also read the boundary condition data from an OVERFLOW input file and add this information into peg.in.raw The mesh names must be present in the OVERFLOW input file, otherwise the boundary condition information can not be used by PEGASUS.

The -no_add_te flag will cause it to not add an extra solid surface (ibtyp=-1) at the trailing edge of a component where a flow-through boundary starts.
 

peg_hole_surf [-sp] - creates one unformatted, multi-zone PLOT3D grid file for each HCUT namelist in the pegasus input file (or just one grid file if there is no HCUT namelist). The grid file will contain all of the no-slip and slip-wall surfaces from the meshes which are members of the HCUT hole cutter. This is very useful for verifying that the HCUT hole-cutter surfaces comprise an airtight surface.

This program requires the pegasus input file, and it reads the grid coordinates from the mesh files in the X_DIR directory. If the code was compiled using double-precision, one can produce a single-precision grid file by adding the command-line argument -sp.

p3d2peg - breaks up the user-supplied PLOT3D file into single grid files which are placed in the /X_DIR directory.
 
 

make_WORK. -creates the WORK directory and its sub-directories which are needed within the project directory. If these are not created before-hand, PEGASUS5 will create them when it is executed.
 

mesh_lister - generates a list of mesh names for use by the other utility codes. The names will be generated from an OVERFLOW input file, if it exists; otherwise, the user will be prompted to either enter mesh names or assign default names to each grid in the user-supplied PLOT3D grid file.
 

clean_holes - removes the contents of /WORK sub-directories which are relevant to hole generation. Use this script if it is desired to re-run only the hole-generation processes again. If one one wants to re-run the entire PEGASUS process from the beginning, simply remove or rename the WORK directory.
 
 

The following utility codes are supplied for diagnostic purposes:
 

peg_plot [-sp] [-noorphfix] - produces an unformatted, multiple grid PLOT3D file (with IBLANKs) of the grid system. It reads the iblank and stencil data from the XINTOUT file, and so can only be used after PEGASUS5 has been run to completion (THRU = 'xintout'). Use peg_hole to plot the holes if you have only run with THRU = 'comp_hole'. The program prompts for the name of the output file, and for the level of fringes to plot, where the fringe level can be:

1 = single fringe: blank out level-2 and higher fringe points
2 = double fringe: blank out level-3 and higher fringe points
3 = all: only the minimum holes are blanked out

If the code was compiled using double-precision, one can produce a single-precision grid file by adding the command-line argument -sp.

It assigns an iblank value of 101 to first level ORPHAN points so they can be plotted; for example, use function 3 in PLOT3D. The code will automatically assign second-level ORPHAN points an iblank value of 1 (a valid interior point) unless used with the -noorphfix argument, in which case the iblank will be assigned a value of 101.

peg_plot_center [-sp] [-noorphfix] - produces an unformatted, multiple grid PLOT3D file (with IBLANKs) of the grid system for cell-centered grids. The cell-center coordinates are written to the grid file. It reads the iblank and stencil data from the pegasus5.dci file. The program prompts for the name of the output file, and for the level of fringes to plot, where the fringe level can be:

1 = single fringe: blank out level-2 and higher fringe points
2 = double fringe: blank out level-3 and higher fringe points
3 = all: only the minimum holes are blanked out

If the code was compiled using double-precision, one can produce a single-precision grid file by adding the command-line argument -sp.

It assigns an iblank value of 101 to first level ORPHAN points so they can be plotted; for example, use function 3 in PLOT3D. The code will automatically assign second-level ORPHAN points an iblank value of 1 (a valid interior point) unless used with the -noorphfix argument, in which case the iblank will be assigned a value of 101.

peg_diag [-sp] - produces a diagnostic file for plotting. It can be produced after PEGASUS execution has been completed. The file that is created allows the user to visualize quality and cell difference parameter with PLOT3D or FAST (as well as any visualization software that reads PLOT3D grid and solution files). This file can be used with the grid file produced with peg_plot. There are no PHANTOM meshes included in this file. The values in this file are as follows:

peg_hole [-sp] - creates a grid file with IBLANK for the hole system that has been created. PEGASUS must be executed through (at least) the "comp_hole" process in order to use this utility. An unformatted, multiple grid, with IBLANK, PLOT3D file is produced. This code must be executed in the project directory.

If the code was compiled using double-precision, one can produce a single-precision grid file by adding the command-line argument -sp.

peg_proj [-sp] - creates diagnostic multi-zone PLOT3D grid and solution files, named peg_proj.g and peg_proj.q, which contain a zone for each solid-wall boundary surface. The grid file contains the grid-cooridnates at the surface points, and the q file contains fields 1, dx, dy, dz, and 1. The dx, dy, and dz data are the components of the projection vector at each surface point for the projection of that point with the greatest magnitude. This data is best used by plotting velocity vectors at all the points, and coloring the vectors by velocity magnitude. Typically, it is best to scale the velocity vectors by a factor in the range 10 - 100. peg_proj creates a PLOT3D command file named peg_proj.com, which can be used to create this type of plot using PLOT3D. peg_proj also reports the maximum distance moved for each mesh, and onto which mesh that maximum projection occured.

If the code was compiled using double-precision, one can produce a single-precision grid file by adding the command-line argument -sp.

peg_orph [-noorphfix] - Lists the orphan points for all of the meshes or for a specified mesh. The output can be sent to a file or to the screen. If the -noorphfix command-line argument is given, it will not fix the 2nd-fringe orphans, and they will be included in the list.
 

peg_mem - estimates memory requirements for a given PEGASUS problem. Requires the pegasus5 input file, and the grid files in the X_DIR directory.
 

peg_sym - checks for bilinear symmetry. This utility program should be run from the pegasus5 run directory. It reads the grid coordinates and determines which zones have bi-lateral symmetry. It then reads the XINTOUT file and determines if the iblank array and the interpolation stencils are also symmetric.
 

XINtegrity - checks the XINTOUT file produced by PEGASUS for internal consistency. This utility checks the accuracy of interpolations and determines whether interpolated boundary points are receiving information from the correct mesh elements.
 

dcintegrity - checks the pegasus5.dci file produced by PEGASUS for internal consistency for cell-centered grids. This utility checks the accuracy of interpolations and determines whether interpolated boundary points are receiving information from the correct mesh elements.
 

XIN2sp - converts a double precision XINTOUT file to single precision. This utility is used if it is desired to run the flow solver in single precision, but PEGASUS was run in double precision.
 

cmpxint - compares two XINTOUT files. If they have the same grid dimensions and number if stencils, it reports the maximum difference in the stencils weights and number of differences in the iblank arrays.
 

It is recommended that all of the utility codes be executed from the project directory, as most of them require information from the /WORK and /X_DIR directories.
 

3.4 Output File Formats

Standard Output

Only error messages are written to stdout.

Log File

PEGASUS5 writes all of its output to a log file with the name of log.dddd.tttt, where dddd is the current date and tttt is the current time. The log file contains the following:

• A summary of all user inputs.
• A summary of each sub-process associated with the run
• A final summary containing the following:
  • The total number of hole points
  • Number of interpolated boundary points for each mesh
  • Number of interpolation stencils for each mesh
  • Number of orphans in each mesh

XINTOUT

The XINTOUT file contains all of the interpolation stencils for the fringe points and outer-boundary points, as well as an iblank array defining the hole-cuts. The file is unformatted, and contains the following four records for each mesh M.
 

where I1 = 1 and I2 = MJMAX(M)*MKMAX(M)*MLMAX(M)

3.5 Directory Structure
 

PEGASUS 5.1 stores its files and information in a specific directory structure which it will create when it is first executed in a particular project directory. These directories can also be created in advance using the make_WORK script, which is also executed by the peg_setup script.

Execution of PEGASUS 5.1 must be performed in the project directory (see Figure 10). The user must supply the standard input file, see Section 3.2 for input descriptions) and the individual volume grids. The individual volume grids are stored in the X_DIR directory as unformatted, single-zone, PLOT3D grid files. These grid files are named "mesh_nameA.x", "mesh_nameB.x", etc, where mesh_nameA, mesh_nameB, ... correspond to the NAME variables in the $MESH namelists.