ADDVARiable [Name] is [Formula]
Command creates new field variable (PHI-variable) with the name [Name] (1 .. 4 symbols) , using formula [Formula]. The formula can contain:
You should use in formula the next rules:
For example:
ADDVAR DEM1 is 1.0+Y*:AC1:+sin(PI*((x*165)^2)/3)*sin(PI*y*82.7)
ADDVAR DEM2 is SQRT((U1^2)+(V1^2)+(W1^2))
AUTOPLOT
AUTOPLOT can now be used from within PHOTON. In command mode, type AUTOPLOT and press ENTER. The whole range of AUTOPLOT commands are then available to the user. To finish AUTOPLOT and return to PHOTON, type E. Note that each time you switch between PHOTON and AUTOPLOT it is necessary to reload files (phi, patgeo &c).
BL[ock]....defines blocked regions for the plot, in which no contours or vectors will be plotted. PHOTON prompts for the number of blocked regions, and for the extent of the region in the X,Y and Z directions. Up to 10 blocked regions may be specified, and subsequent use of the block command will clear all previously defined regions.
Break of processing command which take a lot of time.
Cancel of continuing plotting after PAUSE state. It is analog of command ENDUSE in processing of USE file.
for GRID: [Centre] causes a grid to be plotted at the cell centre, rather than at the cell face. This may be useful when it is necessary to plot contours or vectors directly onto a grid, rather than in the space between two grids, as happens with the normal GRID setting.
for VECTOR: [Centre] toggles the vector-plotting mode. Two modes are available, with vectors being plotted either radiating from cell centres (Yes) or centred about the cell centre (No). The default is to plot vectors radiating from cell centres (No).
CL[ear]....clears the screen, and deletes all grid, vector, contour, surface and text elements currently saved.
COL[our] [element] [colour] [element range]....changes the colour of existing grid, vector, surface or contour elements on subsequent plots or redraws. The range of valid colour numbers depends on the colour capabilities of the display device. For example, COL GR 4 5 will change the colour of grid element 5 to colour 4. The command COL VEC 8 2 5 will change the colour of the vector elements 2 through to 5 to colour 8.
You can see the changing of colour setting of command REDRAW.
CON[tour] CL[ear]....deletes all contour elements, whether switched on or off.
You can see the changing by setting of command REDRAW.
See also : CONTOUR DELETE, CONTOUR OFF, CONTOUR ON
CON[tour] DEL[elete]....deletes the last contour element, whether switched on or off.
See also : CONTOUR CLEAR, CONTOUR OFF, CONTOUR ON
CON[tour] OF[f] [element range]....switches off the specified contour element(s). It will not appear in subsequent plots until switched on again.
See also : CONTOUR ON
CON[tour] ON [element range]....switches on the specified contour element(s). It will then appear in subsequent plots.
See also : CONTOUR OFF
CON[tours] [domain] [variable] [plane] [number] [subregion] [options]....
plots contours of the variable specified over a plane,
or subregion of the plane into selected domain.
Selected domain is need for Fine Grid Embedding cases only.
A subregion consists of the extent
of the grid in the other two coordinate directions, and either
or both may be omitted if the total extent in that direction
is to be used. If domain omitted then domain 1 is selected. For example,
CON DOM 2 P1 Y 1 Z 7 M
will contour in domain 2 variable P1 over the Y 1 plane, for all cells in
X, and cells 7 to the maximum in Z. NOTE the use of M to denote
the maximum grid extent.
Options available are SHADE, which produces coloured contours, with colours ranging from blue (minimum values) to red (maximum values) and FILL, which produces colour-filled contours; and NOSMTH, which produces colour-filled contours, when each cell is painted by single colour; DASH, which plots contours as dotted lines (available dash types are 1-3). For example,
CON P1 Y 1 Z 7 M DASH 1
will perform the same as the last example, but with contours plotted as dashed lines.
The program will prompt for the number and range of contours to be plotted. These may be specified in 4 ways:
a) the upper and lower bounds, and number of values, e.g. 100 200 10;
b) INT [n] to give n contours equally spaced over the whole range;
c) VAL [n] to allow you to enter n individual values; and
d) OLD to use the previous setting.
If calculation was produced with using of method PARSOL, and user wants to draw borders of PARSOL cells, user must used variable "*PSC". For example,
CON *PSC Y 2 X 1 M Z 1 M DASH 0
to plot borders of PARSOL cells on Y = 2 plane.See also : CONTOUR CLEAR, CONTOUR DELETE, CONTOUR OFF, CONTOUR ON
Three different coordinate systems may be used by PHOTON, which are:
(1) The position and orientation of the plot are defined in cartesian (X,Y,Z) space, and are shown by the axes plotted at the lower left of the plot. You can change the orientation of the plot using the VIEW and UP commands.
(2) The location of quantities within the solution domain is defined in terms of grid-coordinate space (I,J,K). For non-BFC cases the (I,J,K) axes will coincide with (X,Y,Z), but for BFC cases the curvilinear nature of the grid may mean that (I,J,K) bears a complex relationship to the cartesian axes. You specify grid locations using (I,J,K), e.g. GRID I 1, GRID K 7.
(3) Cells are numbered in terms of an (IX,IY,IZ) coordinate system, so that IX=1 represents the first cell in the I direction, IZ=4 the fourth cell in the K direction, and so on. Since PHOENICS variables are calculated for cell centres, the VECTOR and CONTOUR commands use the cell-centre notation, i.e. VEC IX 1.
Right-handed and left-handed coordinate systems may be used. The default is right-handed, and the commands RHAND and LHAND are used to switch between the two.
See also : SET LHAND, SET RHAND
D[ash] [dash type] [element type] [range]....changes the dash type for subsequent plotting of grid, vector and contour elements. Dash types range from 1 to 3. Example : DASH 2 CON 2 4 will change the dash type to 2 for contour elements 2, 3 and 4.
Dash type 0 denotes a solid line, and -1 denotes colour shading for contours and vectors.
DO [ var ] = [ start value ] [ end value ] [ inc value ]
[ PHOTON commands ]
ENDDO
The DO command enables a series of PHOTON commands to be repeated over a range of values. The syntax is similar to a DO loop in FORTRAN, however there is no label nor it is possible as yet to do nested DO loops. It is available under both command mode and use files. As in FORTRAN the increment value is optional.
For example to plot vectors over each of the Z planes:
DO IZ = 1 M
VEC Z IZ SH
ENDDO
When plotting contours it is necessary to provide additional values, eg a sub-division size with the fill option. These must be supplied on the same record otherwise the DO loop will fail. So that:
DO IX = 1 M 5
CON TEM1 X IX FILL ; 0.01
ENDDO
will provide colour fill contours, but
DO IX = 1 M 5
CON TEM1 X IX FILL
0.01
ENDDO
will cause an error. However, if the subdivision size is ommitted then the user will be prompted for it when the line is processed.
DO[main].... prompts for the extent of the domain in Cartesian coordinates. It is used when PHOTON is run without PHI or XYZ files attached, in order to develop geometry files. The default domain extent is 0.0-1.0 in X,Y and Z.
After pressing the button, type in the name of the screen dump file. A screen dump will be saved in the file and can be sent to a plotter for hard copy.
E[nd]....terminates the plotting session, closes all open files and returns to the operating system.
[E]xit from the current PHOTON session.
EXT[rapolate]....is a command that enables PHOTON to plot to the boundaries of the grid.
EXTRAPOLATE is entered as an alternative to PHI for the processing of the "fields" file from EARTH. It generates an additional "layer" of cells at both ends of the computational domain in each direction, and assigns values to each new node by extrapolation of the values at the two adjacent, inner nodes. The values assigned to the new nodes are truncated, if needed, so that they do not exceed the maximum and minimum values in the original domain. (Use the command EXTRAPOLATE NOLIM to extrapolate without these limits.)
EXTRAPOLATE can also be used to obtain contour plots of one-dimensional problems.
See also: PHI
EXT[rapolate] NOL[im]....is similar in function and usage to the EXTRAPOLATE command, but will allow the extrapolated values of the variables to lie outside the original range of values for the domain.
The GEOMETRY feature in PHOTON allows you to 'draw' geometric elements on the plot. Lines, arcs, circles and polygons can be drawn in 3D space for a variety of purposes - outlining blockages, adding realism by drawing objects in and around the domain (such as car outlines), and highlighting features within the domain. For ease of use, individual elements may be grouped together into segments, which can then be manipulated as a whole.
Geometry commands may be read in from a disk file, or entered from the terminal. Elements may be added, switched on and off, deleted, and the final geometry saved back to disk.
See the HELP entry for GEOMETRY_CMDS for a brief description of the geometry commands.
See also : GEOMETRY DELETE, GEOMETRY OFF, GEOMETRY ON, GEOMETRY READ,GEOMETRY SAVE,GEOMETRY CLEAR, GEOMETRY_CMDS
GE[ometry] CL[ear] .... deletes all geometry elements.
See also : GEOMETRY, GEOMETRY_CMDS
GE[ometry] DE[lete] [n].... deletes geometry element 'n', where 'n' may be an element number, or 'ALL' to delete all elements.
See also : GEOMETRY, GEOMETRY_CMDS
GE[ometry] OFF [n].... switches off geometry element 'n', where 'n' may be an element number, or 'ALL' to delete all elements.
See also : GEOMETRY, GEOMETRY ON
GE[ometry] ON [n].... switches on geometry element 'n', where 'n' may be an element number, or 'ALL' to delete all elements.
See also : GEOMETRY, GEOMETRY OFF
GE[ometry] RE[ad].... reads user geometry for display on the plot. Geometry may be read in from a file, or typed in from the keyboard. If entry from the keyboard is desired, press [Return] when the geometry file name is requested, otherwise enter the file name.
To exit interactive geometry entry, press [Return] until the 'Option?' prompt appears.
Geometry elements may be added to the currently stored elements using GEOM READ more than once.
See also : GEOMETRY, GEOMETRY SAVE
GE[ometry] SA[ve] [filename].... saves the currently stored geometry elements into a file. If no filename is given, it will be prompted for.
A saved geometry file may be subsequently read in using GEOM READ.
See also : GEOMETRY, GEOMETRY READ
This is a brief description of the available geometry commands. Further details appear in the PHOTON User Guide.
(1) LINE x1 y1 z1 x2 y2 z2 [dash] [colour]
x1 y1 z1 - Cartesian coordinates of start of line.
x2 y2 z2 - Cartesian coordinates of end of line.
dash - Line type, 0=solid line, 1-4=broken lines Default=solid line.
colour - Line colour, default=default colour for device
(2) PLINE x1 y1 z1 x2 y2 z2 [dash] [colour] + x3 y3 z3
x1 y1 z1 - Cartesian coordinates of start of first line.
x2 y2 z2 - Cartesian coordinates of end of first line.
dash - Line type, 0=solid line, 1-4=broken lines Default=solid line.
colour - Line colour, default=default colour for device
Subsequent records continue the line to as many points as desired.
(3) PGON x1 y1 z1 [dash] [fill] + x2 y2 z2
x1 y1 z1 - Cartesian coordinates of first vertex.
dash - Boundary line type, 0=solid line, 1-4=broken lines. Default=solid line.
fill - fill colour or pattern. Default=no fill.
Subsequent records define the remaining vertices of the polygon.
(4) ARC dash colour circle
+ x1 y1 z1
+ x2 y2 z2
+ x3 y3 z3
dash - Line type, 0=solid line, 1-4=broken lines Default=solid line.
colour - Line colour, default=default colour for device
circle - 0=draw arc, 1=draw circle.
x1 y1 z1 - Cartesian coordinates of first point on arc.
x2 y2 z2 - Cartesian coordinates of second point on arc.
x3 y3 z3 - Cartesian coordinates of third point on arc.
The 'circle' parameter indicates whether a circle is to be drawn through the three points, or whether an arc is to be drawn from point 1 to point 3 via point 2.
(5) BEGIN segname
Start definition of a segment. All subsequent LINE, PLINE, PGON and ARC commands will be stored in the segment until the next END command. Note segments may now be nested.
(6) END
Terminate definition of the current segment.
G[rid] CE[ntre] [plane] [number] [subregion] [options].... plots a grid at a cell centre, rather than at a cell face.
This may be useful when it is necessary to plot contours or vectors directly onto a grid, rather than in the space between two grids, as happens with the normal GRID command.
All parameters are the same as for the GRID command.
See also : GRIDS
G[rid] C[lear]....deletes all grid elements, whether switched on or off.
See also : GRID DELETE, GRID OFF, GRID ON
G[rid] D[elete]....deletes the last grid element, whether switched off or on.
See also : GRID CLEAR, GRID OFF, GRID ON
G[rid] H[atch] [plane] [number] [subregion] [options].... plots a hatched grid or subregion of grid. A hatched grid consists of vertical and/or horizontal lines with a user-specified spacing, and is often used to improve the appearance of a plot where too many grid lines might obscure the picture.
The program will then prompt for hatch direction, which may be any or all of X, Y and Z, and a hatch spacing for each direction, which represents a fraction of the grid size in that direction.
NOTE that once set, these parameters will be retained for all subsequent hatched grids, unless reset by the HATCH command.
G[rid] OF[f] [element range]....switches off the specified grid element(s), which will not appear in subsequent plots until switched on again.
See also : GRID ON
G[rid] ON [element range]....switches on the specified grid element(s), which will appear in subsequent plots.
See also : GRID OFF
G[rid] OU[t] [plane] [number] [subregion] [options].... plots an outline of the specified grid, i.e. one with no interior detail.
See also : GRIDS
G[rids] [domain] [plane] [number] [subregion] [options]....plots the grid for a given plane and number in selected domain. If a subregion is specified, only that part of the grid will be drawn. You could set selected domain for Fine Grid Embedding cases only.
A subregion consists of the extent of the grid in the other two coordinate directions, and either or both may be omitted if the total extent in that direction is to be used. For example, GRID DOM 2 X 1 Y 5 M Z 1 4 will plot the X 1 grid over the region Y cells 5 to the maximum, Z cells 1 to 4 into domain 2.
Options available are COLOUR [number] to plot the grid in a specified colour, and DASH [number] to plot the grid in a specified line-style. For example, GRID X 1 Y 5 7 DASH 1.
See also : GRID CLEAR, GRID DELETE, GRID OFF, GRID ON, GRID OUT, GRID HATCH, GRID CENTRE
HA[tch]....sets up or changes the grid-hatching parameters. It will prompt for hatching directions, which may be any or all of X, Y and Z, and hatch spacing for each direction, which is specified as a fraction of the grid length in that direction.
See also : GRID HATCH
LOG [file name] opens the named LOG file in which all subsequent commands in the current interactive session or from a USE file are recorded. The LOG file can be used as a USE file in a later session.
To create macro-variable you must use commands:
MACro INTeger [list of variables]
MACro REAL [list of variables]
MACro CHAR [list of variables]
Command for calculation of value macro-variable is used:
MACro [Macro Name] = [Formula]
for example:
MAC Int N,NF,NL
Mac real R
Mac char S
N = :NX: + :NY: + :NZ:
NF = 0.25*NX
NL = 0.75*NX
R = PI/3.0
S = A:N:.dat
You should use in formula the next rules:
Three macro-variable is determined in results of calculation immediately, these are NX, NY and NZ.
You can use macro-variable in any other commands PHOTON, for example:
Macro real FI
FI = 1.e-4
con TEMP iy M fi;:FI:
For working with macro-variable you can use following commands:
MACro CLEar - delete all macro-variables (except NX,NY,NZ);
MA[gnify] G[rid] [factor]....sets the grid-magnification factor. Following the execution of this command, the graphics cursor will appear and should be positioned at the desired centre of the magnified image. Pressing any key except [Return] will cause a redraw of the plot.
NOTE that magnifications are not cumulative; to return to original size, use MAG GRID 1. Note also that changing the viewpoint or up vector for a magnified grid will result in the magnification being reset to 1.
MAGNIFY GRID can be used within USE files in order to perform a non-interactive grid magnification. The grid is magnified by the specified factor, about the point (X,Y), where coordinates are given in PHOTON Internal Coordinates (PICS). For example, UMAG GR 5 1000. 1000. will magnify the picture by a factor of 5 about the point (1000.,1000.).
NOTE that to return to normal size, the command MAG GR 1 can still be used.
MCO[NT] command
MCONT [block number] [parameters as for CONTOURS command]
The MCONT command is used to display contours of the specified variable over a plane (or part of a plane) within an individual block of a multi-block case. The MCONT command is similar to the CONTOURS command but it takes as its first parameter the block number that it is to work from. The block number should range between 1 and the number of multi-blocks present. Note that the other contour commands such as CONTOUR CLEAR, CONTOUR DELETE, CONTOUR OFF, CONTOUR ON and the various SET CONTOUR commands can also be applied to contours produced using the MCONT command. If the SHOW CONTOURS command is used to list out the contours that have been displayed, the contours produced with the MCONT command will appear in the list, but the I/J/K/X/Y/Z values displayed for them will be the values in terms of the overall domain rather than in terms of each multi-block.
examples:
MCONT 1 P1 X 2 FI
Displays filled contours of the variable P1 on the second X ( or I ) plane of the first multi-block. Note that it will prompt for the subdivision size before plotting.
MCONT 2 P1 Y 4 X 1 5 Z 1 3
Displays contours of the variable P1 on the fourth Y (or J) plane of the second multi block. This will prompt for the range and number of intervals over which the contours should be plotted.
MCONT 2 P1 Y 3 SH
Displays shaded contours of the variable P1 on the third Y (or J) plane of the second multi block. This will prompt for the range and number of intervals over which the contours will be plotted.
MGR[ID] [block number] [parameters as for GRID command]
The MGRID command is used to display a grid within an individual block of a multi-block case. For single block cases the GRIDS command should be used instead. If the GRIDS command is used for multi-block cases, strange output may result. The MGRID command is similar to the GRIDS command but it takes as its first parameter the block number that it is to work from.
The block number should range between 1 and the number of multi-blocks present.
Note that the other GRID commands, such as GRID CENTRE, GRID CLEAR, GRID DELETE, GRID OFF and GRID ON can also be applied to grids produced using the MGRID command. If the SHOW GRIDS command is used to list out the grids that have been displayed, the grids produced with the MGRIDS command will appear in the list, but the I/J/K/X/Y/Z values displayed for them will be the values in terms of the overall domain rather than in terms of each multi-block.
examples:
MGRID 1 X 2
Displays the second X ( or I ) grid within the first multi-block.
MGRID 2 Y 4 X 1 5 Z 1 3
Displays the fourth Y ( or J ) grid within the second multi-block, but restricted to the subregions 1-5 in X and 1-3 in Z. Note that the subregions are specified relative to the multi-block specified, so the range of acceptable values for the sub-region restrictions start from one, with the upper limit dependant on the grid size of the multi-block.
MGRID 2 OUT Y 3 COL 5
Displays the outline of the third Y ( or J ) grid within the second multi block using colour five.
MI[rror] [axis]....produces a plot mirrored in a plane normal to the axis specified, which may be X, Y or Z. This will reflect all plot elements, and will become active at the next redraw.
NOTE that the original and reflected planes are always seen; it is not possible only to view the reflected plane.
MVE[CT] command
MVECT [block number] [parameters as for VECTORS command]
The MVECT command is used to display vector information over a plane (or part of a plane) within an individual block of a multi-block case. The MVECT command is similar to the VECTORS command but it takes as its first parameter the block number that it is to work from. The block number should range between 1 and the number of multi-blocks present. When displaying vectors with a multi-block case, it is recommended to turn vector averaging off. This can be done with the SET VECTOR AVERAGE OFF command. Note that the other VECTOR commands, such as VECTOR CLEAR, VECTOR DELETE, VECTOR OFF, VECTOR ON and the various SET VECTOR commands can also be applied to vectors produced with the MVECT command. If the SHOW VECTORS command is used to list out the vectors that have been displayed, the vectors produced with the MVECT command will appear in the list, but the I/J/K/X/Y/Z values displayed for them will be the values in terms of the overall domain rather than in terms of each multi-block.
examples:
MVECT 1 X 2 SH
displays shaded (coloured according to magnitude) vectors in the second X ( or I ) plane of the first multi-block.
MVECT 2 Y 4 X 1 5 Z 1 3
Displays the fourth Y ( or J ) plane of vectors within the second multi-block, but restricted to the subregions 1-5 in X and 1-3 in Z. Note that the subregions are specified relative to the multi-block specified, so the range of acceptable values for the sub-region restrictions start from one, with the upper limit dependant on the grid size of the multi-block.
MVECT 2 Y 4 COL 5
Displays the fourth Y ( or J ) plane of vectors within the second multi block. They are displayed using colour 5.
PA[use]....suspends program execution until you press [Return]. This command is intended mainly for use in USE files.
See also : USE
PHI.... is used to specify the name of a PHOENICS PHI or PHIDA file which PHOTON will attach. Before loading the grid, PHOTON enables you to specify grid scaling factors. If the file is for a BFC run, PHOTON will prompt for the name of an XYZ file. Entering a slash '/' in response to the filename prompt will abort the file-opening command.
See also : XYZ
PICS (PHOTON Internal Coordinate System) is the coordinate system used by PHOTON to draw graphical elements (line, text etc) on output devices. It is a two-dimensional system (say x-y), with the origin located at the bottom left-hand corner of the display are (eg, the screen or paper). The coordinates used are normalised to the ranges 0 to 4095 (in the x direction) and 0 to 3120 (in the y direction).
PICS units are used to specify the position of the text drawn through the TEXT command (when issued within a USE file), and the geometry features drawn through the GEOMETRY command.
The PREFIX file allows the PHOENICS user to over-ride the default file-handling parameters set up for the system when PHOENICS was installed. Each user has their own PREFIX file, and the following list represents those parameters that you may most commonly reset.
(a) IPRE=T or F. Use default filenames as defined at installation time, or allow interactive input of data file names.
(b) PHIDA=T or F. Use direct-access or sequential PHI file.
(c) XYZDA=T or F. Use direct-access or sequential XYZ file.
(d) LPHI=T or F. When IPRE=T, specifies whether a PHI file is to be used.
(e) LXYZ=T or F. When IPRE=T, specifies whether an XYZ file is to be used.
(f) DF09US=T or F. When set true, specifies that input to PHOTON is a DF09 file from PHOENICS version 1.3 or earlier.
[Quit] the current PHOTON session.
RED[raw]....clears the screen, and redraws the current picture.
RO[tate] AX[is] [axis specification] ANG[le] [angle].... causes the rotation of the plot about an arbitrary axis in 3D. The axis may be specified in the same way as for VIEW and UP; angles are in degrees, and may be positive or negative. In order to rotate about the VIEW direction, enter ROT [angle]. For example, ROT AX 1 1 1 ANG 30 will cause a rotation of 30 degrees about the 1 1 1 axis.
NOTE that rotations are cumulative. This command causes an immediate redraw.
SA[ve] [file] [TITLE] .... the SAVE command saves the current picture to a plot file. The file name must be specified the first time SAVE is used; thereafter plots will be added to that file unless a new file name is given. Entering the old file name will over write the original file.
The keyword TITLE will cause PHOTON to prompt for a picture title, which will be saved, and which can be used in the replay program to identify pictures.
SAVPHI [file] .... the SAVPHI command saves the new PHI-file. If user set new variables the they will be saved into new PHI-file.
Rescale the plots and fit it into the current window.
SC[reen]....clears the display, but does not delete any data elements.
See also : CLEAR
SE[ndp].... Redraws the current picture on a plotter or into a plot-file. If more than one plot device is configured in the Graphics Interface, a plot device can be selected from a menu of the available devices. If a file-name is required, PHOTON will prompt for it.
See also : DUMP
SET.... permits the user to set the following switches and parameters :
SET VECTOR REFERENCE - reference value for vector
plotting (formerly TYPVEC)
AVERAGE - set vector averaging on/off
KEY - set vector key display on/off
CENTRE - plot vector arrows centred or
radiating from cell centres
UNITS - set label for vector key
COMPONENTS - change vector components
PHASE - set vector components to phase
1 or phase 2 velocities
SET CONTOUR SCALE - set contour scaling to plane
or field values
UNITS - set label for contour key
FILL - set method to fill contours
SET AXES - display/hide axes
SET BOX - display/hide box
SET HOLD - set deferred plotting on/off
SET LHAND - set left-hand coordinate system
SET RHAND - set right-hand coordinate system
SET POROSITY - enable/disable porosity checking.
SET GEOMETRY - set geometry scaling factors
These can either be specified as a complete command (eg. SET VECTOR AVERAGE ON), or by entering 'SET' and following the sequence of prompts. The sequence may be terminated at any point by entering a slash '/'.
SET AX[es] [ON or OFF]....controls the visibility of the axis orientation marker in bottom right-hand corner of the plot. The result of this command will be seen after the next REDRAW.
See also : SET BOX
SET BO[x] [ON or OFF].... controls the visibility of the border and other information drawn around the plot. The result of this command will be seen after the next REDRAW.
See also : SET AXES
SET CO[ntour] FI[ll]....determines which fill method is used to perform the contour fills. One of three methods can be selected from :- SIZE, NUMBER and DEPTH.
SIZE cells are filled with polygons of a specified size.
NUMBER cells are filled with a specified number of polygons. (minimium 4)
DEPTH cells are filled using the Warnock method: each cell is subdivided until :-
i) a subdivision can be filled with one colour
ii) the size of the subdivision is smaller than pixel size.
iii) the cell has been subdivided a specified number of times. This is the parameter DEPTH. Suggested values of DEPTH range from 1 to 8.
1 fills each cell with one polygon.
8 fills each cell to pixel level.
SET CO[ntour] SC[ale] [FI[eld] or PL[ane]] ....determines whether the colour scale for shaded and filled contours is determined by the maximum and minimum values of the whole field (SCALE FIELD) or those of the plane on which the contour is being plotted (SCALE PLANE). Use of FIELD scaling will ensure that contours on different planes show consistent colours, while PLANE scaling may be used to plot contours on a single plane where the range of values is narrow compared to the overall field range.
SET CO[ntour] UN[its]....sets the units used for labelling the key on shaded and filled contour plots. The default is no contour key labelling. Any string of up to 20 characters may be entered to denote the units, and will appear when the colour key is plotted.
See also : SET VECTOR UNITS
SET GE[ometry] ... This enables you to scale geometry to be in proportion with the current grid proportions. This command can be used only if no geometry elements have been defined. The command GEOMETRY SAVE will save the GEOMETRY unscaled.
See also : GEOMETRY READ, GEOMETRY SAVE
SET HO[ld] [ON or OFF].... controls whether output from plotting commands (eg. GRID, VECTOR, CONTOUR, TEXT) will appear immediately on the screen. If HOLD has been set ON, no output will appear on the screen until HOLD is reset to OFF.
SET LH[and]....changes to a left-handed coordinate system. The default coordinate system is right-handed.
See also : SET RHAND
SET OR[der].... enables you to change the order in which PHOTON plots the various types of graphical elements (grids, vectors etc) when redrawing. The default order is 1=grids, 2=contours, 3=vectors, 4=geometry, 5=surfaces, 6=streamlines, 7=text
The SET ORDER command causes PHOTON to prompt for a new plotting order.
SET PO[rosity] [ON or OFF]....where the variable VPOR has been stored, PHOTON will automatically disable plotting vectors and contours within cells where VPOR=0.0. If it is required to plot within blocked cells, then SET POROSITY OFF will disable the porosity checking within PHOTON. The command SET POROSITY ON will restore checking.
SET RH[and]....changes to a right-handed coordinate system. As this is the default, SET RHAND should be needed only to reset the sense of the coordinate system when SET LHAND has been used.
See also : SET LHAND
SET VE[ctor] AV[erage] [OFF or ON]....sets the averaging method for vector calculation in BFC cases. When AVERAGE is set OFF, only the High, North and East values of the Cartesian components for each cell are used, whereas if it is set ON, all six Cartesian components are used. This may affect the resulting velocity vector in some cases.
SET VE[ctor] BO[undary] [OFF or ON] ....By default, PHOTON does not use velocity values at domain boundaries. Use of the SET VECTOR BOUNDARY OFF command will cause PHOTON not to ignore the boundary values, and to process the vector field exactly as it was read in.
SET V[ector] CE[ntre] [ON or OFF].... is used to set the vector-plotting mode. Two modes are available, with vectors being plotted either radiating from cell centres (SET VECTOR CENTRE ON) or centred about the cell centre (SET VECTOR CENTRE OFF). The default is to plot vectors radiating from cell centres.
See also : VECTORS
SET V[ector] CO[mponents] [v1] [v2] [v3].... selects the three stored variables that are to be used as vector components.
Although three variables must be specified, for 2D runs the third variable may be specified as a dash, e.g. VC - V1 W1 for a 2D Y-Z run. In this case, component 1 is taken as zero. The default setting is U1,V1,W1, and the PHASE command can be used to switch to second-phase velocity vectors.
See also : SET VECTOR PHASE
SET V[ector] K[ey] [ON or OFF].... controls the visibility of the key displayed at the bottom of vector plots.
SET VE[ctor] PH[ase] [1 or 2]....enables you to select the plotting of first- or second-phase velocity vectors. PHASE 1 is the default, and second-phase vectors may be plotted by issuing the PHASE 2 command. This command is inactive for single-phase runs.
See also : SET VECTOR COMPONENTS
SET V[ector] RE[ference] [value]....is used to change the reference velocity used for vector plotting. If a value is not given, the program will prompt for one. The reference velocity is the value associated with the reference arrow in the vector key, and all vectors in the plot are scaled to this value.
See also : VECTORS
SET V[ector] UN[its] [value].... sets the units used for labelling vector plots. The default value for vector units is meters/second (m/s). Any string of up to 20 characters may be entered to denote the units, and will appear when the reference arrow is plotted at the bottom of a vector plot.
See also : SET VECTOR KEY, SET CONTOUR UNITS
SH[ow] [keyword] .... the SHOW command displays the current state of the program. The following keywords may be specified :-
(no keyword) - general information on switch settings etc
VA[riables] - information from the 'fields' file
GR[ids] - information on grid elements
VE[ctors] - information on vector elements
CO[ntours] - information on contour elements
SU[rfaces] - information on surface elements
STR[ream] - information on streamline elements
TE[xt] - information on text elements
BL[ocks] - information on blocked regions
GE[ometry] - information on user geometry
For grids, vectors and contours, the display shows the plane and region over which the element is plotted, the colour and line type, and whether that element is currently switched on or off. For grids, the type of grid (HATCH, GRID or OUTLINE) is also given.
For geometry, the element number, the element name and the status are shown.
ST[op]....terminates the plotting session, closes all open files and returns to the operating system.
See also : END
STR[eam] [dim][plane][number][options]........ the STREAM command plots streamlines either in a 2D plane (2D problems only) or a 3D domain where [dim] is 2D or 3D (the default). For 2D streamlines [plane], [number], [subreg] and [options] are specified as for a CONTOURS command. For 3D streamlines, [plane], [number] and [subreg] specify the plane (or subregion of a plane) from which the streamlines start; [options] are COLOUR, DASH and SHADE.
For example,
STREAM Z 1 SH
will plot streamlines in 3D starting from the plane IZ=1, coloured according to velocity from blue (low velocity) to red (high velocity).
For 3D streamlines only, you are asked whether control parameters are to be reset: answer NO for the program to prompt for the number of streamlines to be plotted. Answer YES for the following prompt:
Choose a keyword:
EXIT, QUIT, STEPS, TIME DOWN, UP, WHOLE, POSITIONS, SUBREGION
The meaning of these options is as follows:
EXIT sets the new parameters, leaves the reset mode,
and prompts for the number of streamlines.
QUIT retuns to the Command?-] prompt without resetting
the parameters.
STEPS is the number of tracking steps plotted for each
streamline. (Default=100)
TIME is the non-dimensional time-step for tracking;
it is equivalent to the size of tracking steps.
(Default=1.0)
DOWN plots streamlines downstream of the starting plane.
UP plots streamlines upstream of the starting plane.
WHOLE plots streamlines up and downstream of the starting
plane.
POSITIONS sets the distribution of streamline on the starting
plane: there are three options - on a line,
on a circle or individual points. (Default is
diagonal of starting plane.)
SUBREGION sets the region over which the streamlines are to be
plotted. (Default is whole domain.)
To choose an option, enter the appropriate keyword; some will require further input for which a prompt will appear on the screen. Enter EXIT when parameter resetting is completed.
Note: In the current version of PHOTON, the STREAM command should only be used for single phase cases and the 3D streamlines can not be drawn under EXTRAPOLATE.
See also : STREAM CLEAR, STREAM DELETE, STREAM OFF, STREAM ON, STREAM 2DIMENSION, STREAM 3DIMENSION
STR[eam] 2D[imension] [plane][number][subregion][option]... draws streamlines over the specified plane for 2 dimensional cases. All the options available with the CONTOURS command, including FILL, can be used. For example,
STR 2D Z 1 SH
will plot streamlines over IZ=1 plane in coloured according to volume flow rate (from blue to red).
Note: This command is only effective in 2-dimensional cases, for 3D cases it has the same effect as STREAM.
See also : STREAM, STREAM 3DIMENSION,CONTOURS
STR[eam] 3D[imension] [plane][number][subregion][option]... draws streamlines in multidimensional space starting from the specified plane. This command is equivalent to STREAM.
See also : STREAM, STREAM 2DIMENSION
STR[eam] CL[ear]....deletes all streamline elements, whether switched on or off.
See also : STREAM
STR[eam] DEL[elete]....deletes the last streamline element, whether switched on or off.
See also : STREAM
STR[eam] OF[f] [element range]....switches off the specified streamline element(s). It will not appear in subsequent plots until switched on again.
See also : STREAM ON
STR[eam] ON [element range]....switches on the specified streamline element(s). It will then appear in subsequent plots.
See also : STREAM OFF
SU[rface] [variable] [direction] [value].... generates a contour surface for a given value of a stored variable. The 'direction', may be 'X','Y' or 'Z', and specifies the planes over which the surface contours will be generated. Usually two out of three will need to be specified, to generate a cross-hatched surface,
eg. SURF P1 X 10.0
SURF P1 Y 10.0
will generate a contour surface for P1=10.0 in the X-Y plane.
See also : SURFACE CLEAR, SURFACE DELETE, SURFACE OFF, SURFACE ON.
SU[rface] C[lear]....clears all current surface elements, whether switched on or off.
See also : SURFACE
SU[rface] DE[lete]....clears the last vector element, whether switched on or off.
See also : SURFACE
SU[rface] OF[f] [element number]....switches off the specified surface element, which will not appear in subsequent plots until it has been switched on again.
See also : SURFACE
SU[rface] ON [element number]....switches on the specified surface element, which will appear in subsequent plots.
See also : SURFACE
TEXT opens the window for adding, deleting and editing text elements.
TRANSience [prefix] [NoBeg] [NoEnd] [NoStep] [USE_file] [trWait] [ here: This command is used for viewing the results of the transient cases. For each PHI-file PHI_Name = [PHI-directory][Prefix][Step] , [Step] = [NoBeg],[NoEnd],[NoStep] executed two commands Photon PHI [PHI_Name];;;; USE [PHI-directory][USE_Name] If [trWait] is more or equal to zero then before execution the next commands delay on specified number of milliseconds is realized.
You can interrupt show by pressed ESCAPE key.
[NoBeg], [NoEnd] [NoStep] - number of first file, number of last file and step interval;
[USE_file] - name of USE-file;
[trWait] - time of waiting in msec, if trWait = -1, that used mode of frame viewing.
UMAG[nify] GR[id] [factor] [X] [Y].... in versions prior to 1.6.2, this command replaced MAGNIFY GRID in USE files. From 1.6.2 onwards, either UMAGNIFY or MAGNIFY can be used in use files. See MAGNIFY GRID for details.
U[p] [direction]....changes the orientation of the plot. The 'up direction' is any vector is 3D space which appears vertical when projected onto the screen. See the help entry for VIEW for details on how to specify directions.
For example, UP Y sets the Y-axis as the up direction.
NOTE that the UP and VIEW directions cannot coincide, by definition.
See also : VIEW
UPA[use] [nsecs].... is used within USE files to perform a timed pause. It differs from PAUSE in that no user input is required; instead, a timed pause of length proportional to the nsecs parameter is performed. The value of nsecs needed to produce a given time interval will be machine dependent.
URE[wind].... is used within USE files to rewind the file and restart processing from the start of the file. It should be used with extreme care, as it will put PHOTON into an endless loop. This facility can be used to generate a repetitive display of a set of pictures.
USE [file specification]....causes command input to be read from the specified file rather than from the terminal. While the commands are being executed, no command dialogue is displayed. PHOTON commands may be entered exactly as they would be from the terminal, and the following extra commands are available in USE files:
- any line beginning with an asterisk in column 1 will be treated as a comment line;
- the command MSG [text string] will display the text string;
- the PAUSE, UPAUSE and #113 commands permit control of the execution of the USE file;
- the UTEXT and UMAGNIFY commands provide non-interactive analogues of TEXT and MAGNIFY, in order to permit fully automatic operation of USE files.
NOTE that only one USE file may be in use at any one time, i.e. nesting of USE files is not allowed.
See also : PAUSE, UPAUSE, UREWIND, UTEXT, UMAGNIFY
UTE[xt].... in versions prior to 1.6.2, this command replaced TEXT in USE files. From 1.6.2 onwards, either UTEXT or TEXT can be used in use files. See TEXT for details.
VE[ctor] C[lear]....clears all current vector elements, whether switched on or off.
See also : VECTORS
VE[ctor] D[elete]....deletes the last vector element, whether it is switched on or off.
See also : VECTORS
VE[ctor] OF[f] [element range]....switches off the specified vector element(s), which will not appear in subsequent plots until it has been switched on again.
See also : VECTORS
VE[ctor] ON [element range]....switches on the specified vector element(s), which will appear in subsequent plots.
See also : VECTORS
VE[ctors] [domain] [plane] [number] [subregion] [options].... will plot vector information over the whole or a subregion of a specified plane into selected domain. A subregion consists of the extent of the grid in the other two coordinate directions, and either or both may be omitted if the total extent in that direction is to be used. You could set selected domain for Fine Grid Embedding cases only. If you don't set selected domain then domain 1 is selected by default.
For example, VEC DOM 2 Y 1 X 3 5 Z 7 M will plot vectors in domain 2 on the Y 1 plane, over the region X cells 3 to 5, Z cells 7 to the maximum.
Options for vector plotting are DASH [number], which will set the linetype of the vectors to dashed. Values may be between 1 and 3; COLOUR [number], which will draw the vectors coloured, the colour lying between 0 and 15; SHADE, which will produce coloured contours, ranging from blue (low values) to red (high values).
Vector arrows are scaled relative to the current reference velocity. This is prompted for by PHOTON when the first set of vectors is plotted, and may be subsequently changed by use of the TYPVEC command.
Vector arrows may be positioned relative to the cell centres in one of two orientations - see VCEN for details.
Other vector quantities may be plotted apart from the first- phase velocities - see SET VECTOR PHASE and SET VECTOR COMPONENTS for details.
NOTE that a 'fields' file (PHI) is necessary for vector plotting.
See also : VECTOR CLEAR, VECTOR DELETE, VECTOR OFF, VECTOR ON, SET VECTOR KEY, SET VECTOR CENTRE, SET VECTOR PHASE, SET VECTOR COMPONENTS, SET VECTOR REFERENCE, SET VECTOR BOUNDARY SET VECTOR AVERAGE
VI[ew] [direction]....sets the view direction, which is the conceptual line, perpendicular to the display surface, along which the plot is viewed.
It may be specified either as an axis direction (e.g. VIEW Z), or by treating the three direction cosines to specify an arbitrary 3D line (e.g. VIEW 1 1 1 defines the commonly used 3D viewpoint at 45 degrees to all 3 axes).
A combination of the VIEW and UP directions specifies the orientation of the plot.
NOTE that these two directions cannot coincide, by definition.
See also : UP
XYZ.... is used to specify the name of a PHOENICS BFC grid file (XYZ or XYZDA file) which PHOTON will attach, in order to allow viewing of BFC grids. Before attaching the grid, PHOTON enables you to specify grid scaling factors.
If a PHI file is attached with a BFC grid, and the dimensions of the BFC grid file is identical, you are given the option either to view the grid or to view the PHI variables upon the grid.
When a grid file has been attached for viewing, by means of the XYZ command, all commands which rely upon data from a PHI file (eg. VECTOR,CONTOUR, SURFACE and so on) are invalid, and the PHI command must be used to attach a PHI file before these commands can be used.
See also : PHI
Escape sequence