File and Report Generation Commands

• analyze - Analyze/synthesize engine face data
• artis - Generate QWIKPLOT files for ARTIS
• calculate - Calculate a new or predefined special function
• cfdfem - Generate a CFDFEM file for CGSA
• copy - Copy or append to common files
• delta - Create a delta .cfl file
• genplot - Create x-y plot files
• genplot surface - Create surface files for contour plotting
• integrate - Perform area-weighted, mass-weighted, or mass-flux-weighted integration
• integrate flux - Integrate fluxes through a surface
• integrate force - Integrate forces on a surface
• integrate volume - Integrate forces and fluxes on volume faces
• interpolate - Interpolate to rake point locations
• list - List data to screen or a file
• neumcp - Generate a NEUMCP file
• plot3d - Generate files for PLOT3D
• smooth - Smooth a polar rake .cgf file

analyze - Analyze/synthesize engine face data

The analyze synthesis command generates a peak dynamic distortion pattern using the method defined by the type option. The data generated is stored in the .cgf file in a variable called p0_type, where type is T45, PW, or GE. The output file contains data similar to the analyze engine output, but tailored to the T45. Currently only the T45 methodology is supported and the peak distortion pattern is created using correlations established from the 26% T45 inlet database. The accuracy of the peak dynamic patterns is a very strong function of the accuracy of the steady-state or time-averaged total pressure pattern.

The analyze engine command creates a report of conditions and performance parameters for the specified rake using the total pressure data specified with the type option. If no type is specified then p0 is used. The input for this command must have been created by a previous interpolate command with rakes specified by the rake polar command, or using the cfcnvt option "Convert ASCII rake to Common File rake CGF" (available in cfcnvt 1.40 and later) followed by an analyze synthesis command. If more that one rake was specified to interpolate, each rake will be analyzed and reported individually. If rake file was used to generate the .cgf file, then you must store the rake code 1.0 in zonal fpar(40) and the rake angle in zonal fpar(42) for this command to operate. The utility fpro has the capability to store these numbers.

Note: This command is not available for unstructured grids.

Example

   grid cfd10.cgf
   solution cfd10.cgf
   unit in
   zone 1
   analyze synthesis type T45 output cfd10.lis
   clear all
   grid cfd10.cgf
   solution cfd10.cgf
   zone 1
   analyze engine type T45 output cfd10dsyn.lis

See Also: The rake polar and interpolate commands for how to generate the input file to this command.

artis - Generate QWIKPLOT files for ARTIS

The artis command generates files for use by the ARTIS (Aerodynamic Real-Time Imaging System) that runs on Silicon Graphics workstations.

The ARTIS program requires surfaces as input. surface commands may be used to define the surfaces or subset commands may be used to specify surfaces or groups of surfaces. Each surface will become a "section" in the output file. If the subset command is used to define the surfaces, the surface should be defined so that the surface normal vector would point towards the viewer if viewed from the "front" or "outside" of the surface.

Note: This command is not available for unstructured grids.

Example

   units inches              ! Specify default length unit for geometry
   zone 1
      surface j 1 i 9,last   ! Omit the singular axis
   zone 2
      surface j 1
      surface i last
   variable Cp; M; T Tinf
   artis output tma2 iris4

See Also: The surface command for how to define surfaces; the subset command on how to define surfaces and normal vectors; the units command on how the define the default length unit; the variable command on how to select variables and their units.

calculate - Calculate a new or predefined special function

The calculate command gives the user the ability to use one of the built in functions or to define their own user function. Predefined functions in general are complex functions which are not just simple combinations of other variables. All functions are calculated and stored as a predefined or user defined variable in the .cfl file. Once the variable is saved in the file it may be operated on like any other variable except that automatic unit conversions are not supported for user defined functions. The function is calculated in all zones specified with the zone command on the entire zone, regardless of any subset specified on that zone.

Note that since the calculated function is written into the .cfl file, for CFPOST versions 4.1 and later the solution command must use the mode option to open the file in read-write mode.

For user defined functions all data is calculated and stored in the metric system. Since the variable units are not known standard unit conversions are not supported, but may be performed using the scale option in the variable command. Thus any constants which are input as part of the function must be in metric units. All CFPOST supported infinity conditions (pinf, Tinf, etc.) may be used in the equation as well as the constants gamma, R, Pr, and Prt. The values stored in the .cfl file for these constants will be used in the calculation. Remember that the variable names and predefined constant names are case sensitive. The operations available are +, -, *, /, **, sinh, cosh, tanh, sin, cos, tan, atan, atan2, log, ln, exp, erf, erfi, min, max, and abs. All variables and operators in the equation must be separated by white space. For single operator functions like sin, a dummy argument must be supplied (see following examples).

Warning: If you are writing over an existing variable which has reference and scaling data, you must renormalize the data in the function definition since the function is overwritten into the file as specified and reference and scaling data is not modified.

The following examples assume that the CFPOST version being used is 4.1 or later, and thus the .cfl file must be opened in read-write mode.

Example 1

Calculate the Reynolds shear stress tensor using the stress tensor shown below, and list it to a file.

       |  0.1  -0.5    0.0  |
   B = | -0.5  -0.06   0.01 |
       |  0.0   0.01  -0.1  |

   solution testke.cfl mode read_write
   zone 1
   calculate reynolds b11 +0.1 b22 -0.06 b33 -0.1 b12 -0.5 b13 0.0 b23 0.01
   clear variable
   units english
   variable R11;R22;R33;R12;R13;R23
   list output test.lst

Note: The variable list is cleared after the calculate command since it sets the variable list to the variables required to calculate the function.

Example 2

Calculate the normalized turbulent kinetic viscosity (nut) and plot the variable on a cut at z = 0.0. The functions are defined using standard CFPOST variables as nut = mut/rho and nutinf = muinf/rhoinf.

   solution test.cfl mode read_write
   zone 1 to last
   calculate function nut = mut rho / muinf / rhoinf *
   clear variable
   variable nut
   unit inches
   cut at z 0.0
   plot color contours

   nut/nutinf = (mut/rho)/(muinf/rhoinf)
              = (mut/rho)*(rhoinf/muinf)
              = (mut/rho/muinf)*(rhoinf)
              = mut/rho/muinf*rhoinf

Example 3

Calculate the corrected airflow at each point weighted by the total area, average the results in units of lb_m/s and write to a file. The function is defined using standard CFPOST variables as follows:

   CMF = rho*A*V*(T0/Tref)**0.5/(p0/pref)

   solution test.cfl mode read_write
   zone 5
      surface I l
   calculate function CMF = t0 270.39 / 0.5 ** rho * V * 1.5 * 101353.0 * p0 /
   clear variable
   variable CMF scale 2.204
   list average output cmf.lis

Note: The scale in the variable command above converts the variable CMF from the metric system (kg/s) to the english system (lb_m/s).

Example 4 - Using the sine function

   calculate function fsine = a 1.0 sin   ! gives sin(a), the 1.0
                                          !    is a dummy

Example 5 - Using the tangent function

   calculate function ftan = a b tan2   ! gives tan2(a,b)

See Also: The subset command on how to define surfaces and normal vectors; the units command on how to define the default length unit; the variable command on how to select variables and their units; the clear command for clearing subsets and variables; the list command for listing variables; the plot command for plotting data.

cfdfem - Generate a CFDFEM file for CGSA

The cfdfem command produces a file for use in Boeing structural analysis.

The subsets must specify surfaces. surface commands may be used to define the surfaces or subset commands may be used to specify surfaces or groups of surfaces. If the subset command is used to define the surfaces, the surface should be defined so that the surface normal vector would point towards the viewer if viewed from the "front" or "outside" of the surface.

If a variable command is not specified, a standard CFDFEM file will be produced which will contain the geometry and pressure coefficient. The units of the geometry information will be the default length unit. If a variable command is specified then the geometry and the selected variables will be written to the file. Such a file will probably be usable only by a custom program.

The orientation of the axes as determined by the orientation command determine the order of appearance of the x, y, and z data in the output file. The first coordinate is the "side" or buttline coordinate, the second is the downstream or fuselage station coordinate and the last is the up or waterline coordinate.

Note: This command is not available for unstructured grids.

Example

   units inches              ! Specify the default length unit
                             !    for the geometry
   zone 1
      surface j 1 i 9,last   ! Omit the singular axis
   zone 2
      surface j 1
   cfdfem output tma2

See Also: The subset command on how to define surfaces and normal vectors; the units command on how to define the default length unit; the variable command on how to select variables and their units.

copy - Copy or append to common files

The copy command is used to create new common files from data extracted from the input files. This command is useful for extracting pertinent data from large CFD solutions for transmittal to other locations for other post-processing or for re-partitioning an existing solution due to memory constraints.

Each subset becomes a zone in the output file(s). All variables from the input grid and solution files are copied to their respective output files (i.e., any variable commands are ignored). Global information from the input file (flow conditions, reference and scaling data, etc.) is copied to directly to the output file. A zone in the output file inherits all zone information from the source zone in the input file. Boundary condition and zone coupling information is not transferred to the output file, so the boundary conditions must be reset if the output file is going to be used by a flow solver. For unstructured grids only unstructured surfaces can be copied, the interior cannot be.

Example

A two-zone solution was started and it was determined that first zone was too dense in the k direction, and the second needed to be split into two zones so it would require less memory.

   grid test2z.cgd
   solution test2z.cfl
   zone 1
      subset i all j all k all,2   ! Every other point in K
   zone 2
      subset i 1,51 j a k a        ! This will be the new zone 2
      subset i 52,last j a k a     ! This will be the new zone 3
   copy grid to test3z.cgd solution to test3z.cfl
   ! Be sure to reset the boundary conditions and recouple after
   !    performing this operation!!!

delta - Create a delta .cfl file

The delta command is used to create a .cfl file containing the difference between two solutions. The difference is just point to point, there are no projections performed, thus only the zone dimensions must match between the two solutions. Deltas will be computed for all variables specified with the variable command or the default of all variables in the .cfl file will be delta'ed. The reference conditions in the output .cfl file will be the same as the .cfl file specified with the solution command. All output variables will be written in the metric system of units.

Warning: You cannot derive new variables from delta variables, you must specify all desired variables in the variable command before performing the delta command.

Example

   solution base.cfl
   zone 1
      surface j 1
   zone 2
      surface u 3
   copy grid to delta.cgd
   variable Cp;p;M
   delta difference cfl new.cfl output delta.cfl

See Also: The subset command on how to define surfaces and normal vectors; the variable command on how to select variables and their units; the copy command for copying subsets to another grid or flow file.

genplot - Create x-y plot files

The genplot command generates x-y plot files for use by the plot command. The variable command defines the variables that are to be included in the output file. The first variable will be the independent variable for all plots and will appear on the x-axis. The second and subsequent variables will be the dependent variables and will always occur on the y-axis. There must always be at least two variables active at the time of the genplot command.

The data to be output will be curves. One way to explicitly define a curve is with the subset command. The second method is to define a cutting plane with the cut command that will intersect a surface defined with the subset command.

For unstructured grids, a cutting plane on a surface is the only way to create a GENPLOT file.

Example 1

Generate a plot file for C_p versus x.

   zone 1
      subset i all j 1 k 15
   variable x inches; Cp
   genplot output pltfile

Just like the previous example except use a cutting plane to generate the curve rather than plotting along a grid line on the surface.

   zone 1
      surface j 1   ! Define the surface to be cut
   units inches     ! Specify default length unit
   cut at z 150.0   ! Constant z cutting plane
   variable x inches; Cp
   genplot output pltfile

Example 3

An unstructured example:

   zone 1
      surface u 7   ! Define the surface to be cut
   units inches     ! Specify default length unit
   cut at y 20.0    ! Constant y cutting plane
   variable x inches; M
   genplot output pltfile

See Also: The subset and surface commands on how to define curves and surfaces; the cut command on how to define cutting planes; the variable command on how to select variables and their units; the plot command on how to plot the data.

genplot surface - Create surface files for contour plotting

The genplot surface command generates an unstructured grid file for use by the plot contours command or any other program that can process an unstructured grid. The file contains geometry information and the variables. Variables may be specified by the variable command or defaulted to all variables in the .cfl file. The units of the geometry and variables will be in the metric system.

A surface is defined as the intersection of a plane defined with the cut command and one or more volumes defined with subset commands. Each surface will be written into an unstructured zone as a unique unstructured surface for each zone intersected. Each surface will be individually displayed when processed by the plot contours command.

Note: When using cut with a 2-D solution (KDIM = 1), always specify "k all" rather than "k 1" in all subset commands.

Example 1

Generate a plot file of Mach number and normalized static pressure for several fuselage station cuts.

   subset i all j all k all   ! Specify a default subset
   zone 1
   zone 2
   units inches               ! Specify default length unit
   cut at x 50.0              ! Constant FS cutting planes
   cut at x 75.0
   cut at x 100.0
   variable M; p pinf
   genplot surface output pltfile overwrite

Example 2

An unstructured example.

   subset u all    ! Specify a default subset
   zone 1
   zone 2
   units inches    ! Specify default length unit
   cut at x 10.0   ! Constant FS cutting planes
   variable M; Cp
   genplot surface output pltfile

See Also: The subset command on how to define volumes; the cut command on how to define a cutting planes; the variable command on how to select variables and their units; the plot contours command on how to plot the data.

integrate - Perform area-weighted, mass-weighted, or mass-flux-weighted integration

Each of the currently selected variables is integrated over each of the surfaces or cutting planes in the current subsets. The output file contains a listing of the result of the integration on each of the surfaces. The output file includes the area of the surface and the area weighted average, mass or mass flux weighted average, average, standard deviation, minimum value and maximum value for each of the specified variables. If a plot file is requested then a curve will be generated where each point represents either the area or mass or mass flux averaged value (depending on which is selected) of a variable on a surface.

For a surface defined with a surface or subset command, the perimeter of the area to be integrated is defined by the grid lines at the extremes of the subset. The interior of the region is viewed as a collection of independent polygons bound by grid lines. A surface defined with a cutting plane is also an independent collection of polygons, created by intersecting the plane with the grid lines in the subsets. In either case, each polygon is processed independently and added to the total. The value of a variable in a cell is considered to be the average of the values at the verticies.

Note: When using this command with a 2-D solution (KDIM = 1), always specify "k all" rather than "k 1" in all subset commands.

Note: For unstructured grids the surface(s) to be integrated must be defined with the surface command.

Note: CFPOST integrates on the cell vertex, whereas Wind-US integrates on the cell center. These methods are equivalent when integrating the entire surface, but small differences will occur when integrating on a subset of a zone surface.

Example 1

Determine the area averaged total pressure recovery and Mach number at the engine face (assume i last is the engine face):

   zone 4
      subset j all k all i last
   variable p0 p0inf; M
   integrate area output areaint

Maybe the engine face was not at a constant i-plane! Use the cut command to specify the engine face plane.

   zone 4
      subset j all k all i all   ! Select a bigger subset
   units inches                  ! Set default length unit
   cut at x 150.0                ! Engine face location in inches
   variable p0 p0inf; M
   integrate area output areaint

Generate a plot file of total pressure recovery, normalized pressure and Mach number versus the x coordinate in a duct. Note that all i-planes are selected. The plot file intplot would be plotted with the plot command.

   zone 4
      subset j all k all i all
   variable p0 p0inf; p pinf; M
   integrate area output intlist plot x intplot

Unstructured Example 1

   zone 4
      subset u 3
   variable p0 p0inf; M
   integrate area output areaint

Unstructured Example 2

   zone 4
      subset u 200 370   ! Select a bigger subset
   units inches          ! Set default length unit
   cut at x 150.0        ! Engine face location in inches
   variable p0 p0inf; M
   integrate area output areaint

See Also: The subset and cut commands for how to define surfaces; the variable command for how to select variables and their units; the plot command for how to plot data; "Equations Used by CFPOST."

integrate flux - Integrate fluxes through a surface

The integrate flux command integrate the fluxes through surfaces. Mass flux, momentum flux, pressure flux and gross thrust are displayed for each surface. A total of all surfaces will be included at the end of the listing.

A surface may be defined directly with a surface command (for structured or unstructured grids), a subset command (structured grids only), or as the intersection of a cutting plane defined by the cut command. If a subset command is used to define a surface, it should be defined so that the surface normal vector would point into or out of the volume as desired. The same consideration should also be given when defining cutting planes.

For a surface defined with a surface or subset command, the perimeter of the area to be integrated is defined by the grid lines at the extremes of the subset. The interior of the region is viewed as a collection of independent polygons bound by grid lines. A surface defined with a cutting plane is also an independent collection of polygons, created by intersecting the plane with the grid lines in the subsets. In either case, each polygon is processed independently and added to the total. The value of a variable in a cell is considered to be the average of the values at the verticies.

Note: When using this command with a 2-D solution (KDIM = 1), always specify "k all" rather than "k 1" in all subset commands.

Example

Generate a plot file of mass flow, momentum, and energy versus the x coordinate in a duct. Note that all i-planes are selected. The plot file intplot would be plotted with the plot command.

   zone 4
      subset j all k all i all
   integrate flux output intlist plot x intplot

See Also: The surface command for how to define surfaces; the subset command for how to define surfaces and normal vectors; the units command for how to define units.

integrate force - Integrate forces on a surface

The integrate force command integrates the pressure and viscous forces and heat transfer rates on a surface and produces a report of the the integrated values, moments and lift and drag coefficients. An individual report is provided for each surface as well as for the sum of the contributions for all surfaces. Only pressure terms are integrated for unstructured surfaces.

surface commands (for structured or unstructured grids) or subset commands (structured grids only) must be used to define the surfaces. If subset commands are used they should be defined so that the surface normal vector is directed into the volume.

The perimeter of the area to be integrated is defined by the grid lines at the extremes of the subset. The interior of the region is viewed as a collection of independent polygons bounded by grid lines. Each polygon is processed independently and added to the total. The value of a variable in a cell is considered to be the average of the values at the vertices. Forces are assumed to act at the centroid of the polygon.

Note: When using this command with a 2-D solution (KDIM = 1), always specify "k all" rather than "k 1" in all subset commands unless noviscous has been specified and a set zcoordinate command has been issued.

Structured Example

   zone 1
      surface j 1 i 9,last   ! Omit the singular axis
   zone 2
      surface j 1
   integrate force output intfrc iviscous -
         reference length 30.0 -
         reference area 100.0 -
         reference moment 15.0 0.0 1.5

Unstructured Example

   zone 2
      surface u 5
   zone 3
      surface u 3
   integrate force output intfrc iviscous -
         reference length 70.0 -
         reference area 300.0 -
         reference moment 1.0 25.0 15.0

See Also: The surface command for how to define surfaces; the subset command for how to define surfaces and normal vectors; the units command for how to define units.

integrate volume - Integrate forces and fluxes on volume faces

All parameters are identical to the parameters for the integrate flux and/or integrate force commands, with the exception of the following:

The integrate volume command produces a report on the degree of conservation of mass, momentum and energy within a control volume. The report gives a summary of the forces and fluxes on each face of the control volume as well as a summary of conservation resulting from adding the contributions from each face in the volume. Each volume will be reported independently.

This command calls the integrate flux and integrate force commands internally. Thus, all of the information supplied in the description of those commands is applicable to this command.

Note: This command is not implemented for unstructured grids.

Example

Get a summary for all zones in a three-zone solution.

   grid test.cgd
   solution test.cfl
   ! Define a default control volume
   surface i 1
   surface i last
   surface j 1
   surface j last
   surface k 1
   surface k last
   zone 1
   zone 2
   zone 3
   integrate volume iviscous output intvol

See Also: The integrate flux and integrate force commands; the surface and subset commands for how to define surfaces.

interpolate - Interpolate to rake point locations

The interpolate command is used to retrieve information from the input files at specified Cartesian coordinates rather than computational (i, j, k) coordinates. The command would most often be used to extract data at experimental probe point locations. The rake command is used to specify the locations of the points for which information is desired. This command may also be used to interpolate onto a surface. If only surface subsets are specified, the program will perform a bilinear interpolation on the surface. This is very useful for extracting values at experimental tap locations or for interpolating a solution on one grid onto a different grid. For unstructured grids only volume interpolation is supported.

The output from this command is another common file that contains the specified x, y, and z locations and the interpolated values of the selected variables organized into a structured grid format. If no variables have been selected, all variables from the input files are copied to the output file. The information for each rake command is written into its own zone with the I dimension being the number of x points, the J dimension being the number of y points, and the K dimension being the number of z points. The x, y, and z coordinates are sorted into ascending order along each of the coordinate directions.

The variables are written to the file in metric units, and all reference conditions are copied. Note that if the original solution data was stored on cell centers, then the interpolation factors are calculated on cell centers.

Example 1

   grid test.cgd
   solution test1.cfl
   units inches         ! set default length unit for rake input
   ! rake 1, dimension 101 x 20 x 1
   rake x 120.2 130.3 0.1 y 50.5 60.5 0.5 z 82.0
   ! rake 2, dimension 101 x 40 x 1
   rake x 120.2 130.3 0.1 y 50.5 60.5 0.5 z 82.0
   ! rake 3, dimension 201 x 80 x 1
   rake x 120.2 130.3 0.1 y 50.5 60.5 0.5 z 82.0
   ! rake 4, dimension 13 x 1 x 1
   rake line begin 1.0 6.2 8.3 end 1.5 6.5 9.2 num 11
   ! select variables to be interpolated
   variable M;p;T;u;v;w
   ! interpolate variables and write a save file for a later
   ! interpolation on a different solution with the same grid
   interpolate write test.int cgf test1.cgf
   ! now we want to list the results
   clear all            ! reset CFPOST
   grid test1.cgf       ! select new file as the grid file
   solution test1.cgf   ! also select it as the solution file
   ! select the variables to list
   variable x inches; y inches
   variable M
   variable locbeta     ! locbeta is derived for u and w
   ! select the subsets
   subset i a j a k a   ! create a default subset
   zone 1               ! zone 1 contains data from rake 1
   zone 2               ! zone 2 contains data from rake 2
   zone 3               ! zone 3 contains data from rake 3
   zone 4               ! zone 4 contains data from rake 4
   list output test1    ! test1.lis contains the results

Example 2

   ! Use interpolation save file to get the data from the
   ! same points in a new solution
   solution test2.cfl
   variable M;p;T;u;v;w
   ! Use the interpolation save file created in example 1
   interpolate read test.int cgf test2.cgf

Example 3

   units inches
   ! Specify rake locations using a file
   rake file taps.egl
   zone 1
      surface j 1
   zone 2
      surface k 1
   ! Since only surfaces are specified interpolation is bilinear on the surface
   interpolate cgf taps.cgf tolerance .01

Example 4

This example uses the bledge command to generate an interpolation file, performs the interpolation, and then uses the calculate command to calculate pressure fluctuations on the boundary layer edge.

   grid 3post.cgd
   solution 3psau.cfl
   units inches
   zone 2
      surface j last
   zone 4
      surface j last
   zone 5
      surface j last
   zone 7
      surface j last
   zone 8
      surface j last
   boundary layer is y+ of 300
   bledge surface output bledge.int
   clear all
   interpolate read bledge.int cgf bledge.cgf
   clear all
   grid bledge.cgf
   solution bledge.cgf
   zone 1
      subset i a j 30,last k 1,2
   zone 2
      subset i a j 30,last k 1,2
   zone 3
      subset i a j a k 1,2
   zone 4
      subset i a j a k 1,2
   zone 5
      subset i a j a k 1,2
   units metric
   clear variable
   calculate prms
   clear variable
   variable M;p pinf;T Tinf;q qinf;prms
   plot3d q bledgeq.plt iris

Example 5

A minus sign should not be used on variables written to an interpolation file, because CFPOST will not be able to read those variables later and will assign zero to those values. Instead, apply the minus sign when reading variables from the interpolation file.

   grid test.cgd
   solution test1.cfl
   units inches         ! set default length unit for rake input
   ! rake 1, dimension 101 x 20 x 1
   rake x 120.2 130.3 0.1 y 50.5 60.5 0.5 z 82.0
   ! select variables to be interpolated
   ! do not apply minus sign here, or variables cannot be read later
   variable uu; vv; ww; uv; uw; vw
   interpolate cgf test1.cgf
   ! list the results
   clear all            ! reset CFPOST
   grid test1.cgf       ! select new file as the grid file
   solution test1.cgf   ! also select it as the solution file
   ! select the variables to list
   ! apply minus sign here as desired
   variable x inches; y inches
   variable uu; vv; ww; -uv; -uw; -vw
   ! select the subsets
   subset i a j a k a   ! create a default subset
   zone 1               ! zone 1 contains data from rake 1
   list output test1    ! test1.lis contains the results

See Also: The bledge command for how to specify the interpolation points; the boundary layer command for specifying how to find the boundary layer; the subset command for how to define the domain to be searched; the variable command for how to select variables and their units; the clear command for how to clear subsets and variables; the calculate command for calculating special functions; the plot3d command to create a plot3d file.

list - List data to screen or a file

The list command lists the values of all of the selected variables in all of the selected subsets. The command can be used to find the minimum and maximum value of the selected variables and their location. It can also be used to find values that are inside or outside a specified range. The raw and nowrap formats are useful for writing data for programs to read.

For subsets of unstructured grids selected with the surface command, all points associated with the selected surface are listed.

Example 1

   zone 1
      subset i all j 1 k 15
   variable x inches; p pinf; T Tinf
   list

Example 2

   ! Find all bad points in a solution
   variable p pinf
   list outside range 0.0 to 100.0

See Also: The subset command for how to define the domain to be listed; the variable command for how to select variables and their units.

neumcp - Generate a NEUMCP file

The neumcp command produces a NEUMCP file that is used by several organizations within Boeing.

surface commands may be used to define the surfaces or subset commands may be used to specify surfaces or groups of surfaces. If a subset command is used to define a surface, it should define the surface so that the normal vector would point towards the viewer if viewed from the "front" or "outside" of the surface.

If a variable command is not specified, a standard NEUMCP file will be produced which contains the geometry and pressure coefficient. The units of the geometry information will be the default length unit. If a variable command is specified then the geometry and the selected variables will be written to the file. Such a file will probably be usable only by a custom program.

Note: This command is not available for unstructured grids.

Example

   units inches              ! Default length unit for geometry
   zone 1
      surface j 1 i 9,last   ! Omit the singular axis
   zone 2
      surface j 1
   neumcp output tma2

plot3d - Generate files for PLOT3D

This command produces files for the program PLOT3D or any other program that accepts files in PLOT3D format. Currently the output is always single precision.

The data written to the xyz file will be written in units of default length units.

If a variable command has not been specified, the standard five variables (four if 2D) will be written to the q or function file with the standard PLOT3D normalization. (I.e., the variables written are static density, momentum in the Cartesian coordinate directions, and total energy per unit volume, with density non-dimensionalized by the freestream static density ρ_∞, velocity non-dimensionalized by the freestream speed of sound a_∞, and total energy per unit volume non-dimensionalized by ρ_∞a_∞².)

If a variable command is specified then exactly five variables (four if 2D) must be selected for output to the q file. If the user wants to plot fewer than five variables, the remaining variables in the q file must be filled with any valid variable. If using PLOT3D the resultant file must be read with the /NOCHECK qualifier. The first variable is plotted as FUNCTION 100, second as 160, third as 161, fourth as 162 (if not 2D) and the last as 163.

Alternatively, an arbitrary number of variables may be selected for output to a PLOT3D function file. When reading function files with PLOT3D, be sure to use the READ/NOCHECK command to avoid warning messages. Note that some software products, such as Tecplot, will only read function files if the file structure (i.e., 2D, mgrid, formatted, etc.) is described manually and the solution file style is set to Plot3d Function rather than Plot3d Classic (i.e., q files). The function names file is a simple text file used by some commercial software products (i.e., Fieldview, Tecplot) to identify the names of the variables stored in the PLOT3D function file.

Note: This command is not available for unstructured grids.

Example 1

Create standard PLOT3D "xyz" and "q" files for all of the solid body surfaces.

   units inches                   ! Default units for the "xyz" file
   zone 1
      subset i 9,last j 1 k all   ! Omit the singular axis
   zone 2
      surface j 1
   plot3d xyz test.xyz q test.q unformatted

Example 2

Create a non-standard 3D "q" file for plotting two chemical species mass fractions. Note that three other variables must be specifed just to fill up five slots.

   units inches
   subset i all j all k all   ! Define a default subset
   zone 1
   zone 2
   variable H2O; CO2; u; u; u
   plot3d q species.q unformatted

The resultant file must be read with the PLOT3D READ/NOCHECK qualifier. H2O will be plotted with function 100 and CO2 with function 160.

Example 3

Create a 3D "function" file and function "names" file for plotting two chemical species mass fractions. Note that this function file will only contain two variables.

   units inches
   subset i all j all k all   ! Define a default subset
   zone 1
   zone 2
   variable H2O; CO2
   plot3d function species.fun names species.nam unformatted

The resultant file must be read with the PLOT3D READ/NOCHECK qualifier. H2O will be plotted with function 100 and CO2 with function 160.

Example 4

Create a 3D "function" file and function "names" file for plotting more than five variables. Note that such files can become quite large, depending on the number and size of subsets selected.

   subset i all j all k all           ! Define a default subset
   zone 1 to last
   units inches                       ! Default units for the "xyz" file
   plot3d xyz plot3d.xyz unformatted
   units fps                          ! Default units for the "function" file
   variable rho; u; v; w; p lbf inch; T; M
   plot3d function plot3d.fun names plot3d.nam unformatted

See Also: The subset command for how to define the domain; the units command for how to define the default length unit; the variable command for how to select variables and their units.

smooth - Smooth a polar rake .cgf file

The smooth command creates new rings and legs between existing rings and legs using radial and linear interpolation. The user specifies the number of rings and legs to add between the current rings and legs, all original points are maintained. The rake must be in the same order that the rake polar command generates, that is I running from the inner ring to the outer ring and J running around the legs.

Note: The new grid and solution is saved over the old grid and so no new file is generated! This command only works on polar 2D structured grids.

Example

   grid polar.cgf
   solution polar.cgf
   zone 1
   smooth rake rings 3 legs 5
   unit inches
   cut at z 0.0
   plot color contours

See Also: The subset command for how to define the domain; the units command for how to define the default length unit; the cut command for how to set cutting planes; the plot command for how to plot color contours.