>>Main Screen                   (this file is text, read or print with your WP)

          Help for LaserPC... Advanced Plotting for AutoTrax       (c)1989-2002

LaserPC....  is the fast and easy way to step-and-repeat Protel PCB's for
             economical production and prototype pcb manufacture
LaserPC....  Significantly reduces Phototooling and PCB prototype costs, often
             paying for itself in the first job.

<Higher plot quality than Autotrax, with Additional features:

  Automatic step and repeat placement
  Component numbering unaffected by repeats
  Integrated NC Drill files for stepped plots
  Double Sided Plotting
  Support for non-pth double sided: removes unconnected topside pads
  Copper Pour/ Minimum etch plots
  Automatic shifting of pcbs into film position
  High quality check plots for documentation
  EPS (encapsulated postscript) output to put pcb's&overlays into documentation
  Drag and Drop Operation

LaserPC.... Is now completely FREE.
http://traxlaserplot.sourceforge.net
LaserPC was written by Simon Bridger, Broadcast Equipment Ltd.
In support of Protels free release of Autotrax, we are releasing LaserPC
under a BSD license.


<>
LaserPC generates PostScript files for printing on LaserWriters and Linotypes
from <.pcb> files generated by Protel AutoTrax PCB. Users without a postscript
printer can use Ghostscript. Details are near the
end.
LaserPC is DOS program, but runs (and compiles) on Linux using DOSEMU 1.02

To run LaserPC you need the program,dictionary file,and help file.The help file
is plain text so you can add to or alter it to suit yourself.Print it out for
reference.

Because of the automatic offsetting of the pcb, we recommend that you have a
track either around the pcb, or at the four corners. This should be placed on
all layers to ensure that there are no unexpected complications occurring
during the automatic placement operations. I also recommend that you do a
delete outside block operation to clean up anything that might get accidently
get left outside the periphery when you have finished your pcb.
PCB's can be edited anywhere in the Autotrax space, they will be automatically
shifted and sized when read. Note that the program does not check the extent of
text strings when it determines the size of a pcb, so you do not need to worry
about text spilling off the board, unless you are planning to screen an overlay
<>

If you are using a free copy, please drop me an e-mail, and feel free to
send suggestions and bugs. You will be added to the mail list so you know when
new versions are loose on the net.

We can add new paper sizes and printer types. See under printers below.

<>
Veiwing Postscript Files: See the end for more information

Differences:
  LaserPC has many new features that do not exist in Protel. The only important
  difference in the output PCBs is the use of Postscript fonts for text. They
  are different sizes (shorter) than Protels font. They are also user
  customisable.

MENU System: The Key letter to select a function is Highlighted.


<I>  Specify the input (Pcb)Filename.It defaults to <.PCB> The PCB will load
     automatically. (also loads at start up, or if it is on the command line)

<O>  Specify the output filename.Default=<.ps> and <.PCB> is not allowed
     You can choose direct to printer which defaults to LPT1.Choosing Printer
     again will toggle LPT1 <-> LPT2.For other printer names if you use any
     DOS printer alias for the filename(eg COM1-4),it will become the printer
     default.Remember that the printer must be online before plotting, if serial
     the Com port initialised with Mode.Normally use MODE COM1: 9600,N,8,1,P
     Note that if AutoMask and AutoPaste and AutoOverlay options are set then
     there will be a soldermask file (.psm) and a solder paste file (.psp) and
     a componentoverlay file (.psv) output also.
     When you are outputting direct to a printer, there can be a significant
     wait while it digests each plot. Installing a print spooler can eliminate
     this. Windows 9? print spools nicely for you.
     If you don't have a PS printer an experimental Emulator option is provided
     This behaves like a printer, but simply writes to a file, that the
     emulator will notice, then print, then delete. (See Ghostscript at end)

<G>  GET the input file and generate an intermediate file. GET happens
     automatically when you set the input file,or start. The size and extent of
     pcb will be shown,and an Offset automatically generated to move the pcb
     to the bottom of the page.Note that it is recommended that your PCB's have
     a fine track around the border so the plot area is properly defined.You
     may choose other offsets or scaling.
     If you have selected AutoOrient then the paper orientation will changed to
     best suit the PCB.

<F>  Offset may be set manually.You primarily use this to print a large PCB in
     several pieces.Units are Thou ,on the PCB.

<S>  Scaling can be set manually over a wide range,and can put much of the PCB
     off the paper.Normally set to 1 or 2.

<A>  Auto Scaling, automatically sets the scale and orientation so the PCB
     fills the page.

<C>  Copper can be printed as black (positives) or clear/white (a negative).

<L>  Layers are toggled by typing their first letter,and are highlighted when
     active.Pads are always active if any track layer is ON.
     If Top and Bottom (or TopOV and BotOV) are on, then double sided plots
     will automatically be selected.
     If GND/PWR, and no other layers, then a GND/PWR plane will be plotted.
     If GND/PWR and another copper layer are active, then Copper Pour / RF
     plots result.
     The top_as_Rf and bot_as_rF (press R or F to toggle) control what happens
     when GND/PWR are selected, and both Top and Bottom layers are selected.
     You can set these so that only the top or the bottom layer in a double
     sided plot will be a Copper Pour / RF plot.
     The LABEL and COMMENT virtual layers control printing of component
     labels (eg R103) and component comments (eg 1K2) when either overlay is
     enabled. HIDDEN will enable display of label and comment strings that are
     hidden. (see also Text Size in Custom screen)
     When <No Unused Pads> is highlighted, top side pads that do not have
     tracks ending in them are automatically stripped out. This is ideal for
     hand soldered, non-pth production or prototypes. It is also beneficial
     with Copper Pour/RF top side plots. At present, tracks that pass across a
     pad, but do not end within it, are no detected as connecting, so that pad
     will be stripped. You should ensure that topside tracks end at each pad
     they connect to (for the time being anyway)

<T>  Type of plot is stepped through with this.
<T>  Layer: Simple plotting of active layers.If power or ground only is active
           others will be ignored and a gnd/pwr plane will be plotted.
           If only overlay is active pads are not plotted otherwise pads+all
           active layers are overlaid.
           Gnd/Pwr planes are negative plots of the pads.Currently no dots are
           printed where pads are connected to the active layer.

<T>  Solder Mask:Plots out all pads with no holes(white in black background).
           Pads are normally printed oversize (eg 15 thou) on the solder mask
           and this is cUstomisable.

<T>  Pad Master:All pads plotted with holes in them. (obsolescent now)

<T>  Check Plot:Plots overlay in black,and other active layers/pads in shades
           of grey.Normally viewed from top, unless the bottom overlay only, is
           active. KEEPOUT layer plots in very pale grey underneath.
           GND/PWR pads plot darker. RF plots when GND/PWR and copper side.

<T>  RF Plot:Also known as Minimum-Etch or Copper Pour/Fill
	   This option is now available in LAYER plots, by selecting GND/PWR
           and another copper layer simultaneously.
           Plots active track layers and pads which are not connected to
           the (active) gnd or pwr plane, with a fine gap around them, in a
           continuous background of copper. Connected pads only plot the hole.
           This Gap can be cUstomised. Note that either gnd OR pwr must be
           active.Text will be plotted as <NOT copper> unlike other plots.


<T>  Paste Master: Plots a screen for solder paste masking. Plots only SMD pads,
           actual size for the selected layers. Pads with holes are not plotted
	   NB: The new auto mask/paste/overlay feature makes this mostly
           redundant now.


<T>  Drill Guide:Plots a Solder Side veiw in a light grey. Obsolescent. Broken.
           Any pad which is has tool>1 will be plotted a darker grey,and the
           tool number printed on it.The Drill Sizes line(in DRFile) will be
           printed on the sheet edge

<V>  The veiw on the paper is important to the type of manufacturing process
     used.Readable means layers are printed seen from the component side unless
     the SolderLayer is Active,when they are veiwed from the solder side.
     When making direct Negs on a compugraphic set this to Non-Readable.
     This is the same as the process instruction "Emulsion Non-Readable"
     Note that currently the autoMASK/PAste/Overlay plots will have the same
     veiw and positive/negative sense as the main plot. This means that you
     will need to get the typesetting bureau to mirror them if appropriate.
     You can see how they were plotted by veiwing the postscript files with any
     text veiwer, the header contains a line describing the mirror state.
     Double-Sided plots canNOT be topveiw (by definition)

<P>  Plot produces a single plot on a sheet.It is disabled when a multiple
     plot page is open.

<E>  Encapsulated Postscript is like plot but produces encapsulated postscript
     without the scale line at the edge of the page,for inclusion in documents.
     To use it you need a program like Pagemaker,Wordperfect etc.Normally plots
     would be done in Portrait mode,1:1,to be oriented correctly in documents.
     EPS also lacks any paper selection commands , and so can be of use with
     printers that do not recognise the supported paper sizes.
     MICROSOFT WORD 2 will not read compliant postscript. Thanks Bill.
     LaserPC automatically uses EPSFIX to make them WORD 2 readable. It does
     this by moving the bounding box to the start of the file. It also is able
     to comment out the page activator line of straight postscript files LAX
     produces. You can use Ghostscript to add previews to EPS documents, and
     to turn them into Adobe Illustrator format (which several drawing packages
     can deal to)

<M>  Multiple plotting opens a sheet for several plots.Plots may be of any type
     but must be all the same scale. You can go back and forth, getting new
     PCB's, and plotting more plots onto the page, until you CLOSEPAGE. You can
     do automatic Step and Repeat of a pcb. (see below for more details)

<Z>  This command closes a multiple plot page.It is the same as the closepage
     choice in the Multiple plot menu.Until you have closed a page,you cannot
     change scales,output file,pages sizes etc. Until you have closed the page,
     you can keep adding more and more plots to it.

<U>  Customise to change setups, Printers, and plot parameters, options
     (See below)

<N>  Number of copies instructs the printer to duplicate the sheet.It doesn't
     send the whole file again.If you need copies,this is much faster.

<R>  Deleted

<D>  Directory.Sets the working dir.<return> sets the current dir,and is best.
     If you want a directory list, sorry sHell to dos and do it.

<H>  Shell to Dos.DO NOT alter LPC files or run TSR's.

<Q>  Quit. Also <Alt X> <Alt F4>

<X>  Not on the menu,this quits without deleting the Intermediate File that has
     been created.

<1>  Load Drill Reference file.This file must be loaded before Get to be
     effective

<2>  NCDrill Support ON/OFF.Can be turned off during multiple plots.

>>Multiple Plot Screen
     Multiple plotting opens a sheet for several plots. What I mean is a single
     sheet of film, (possibly with both sides) of several pcbs on it.
     Plots may be of any type but must be all the same scale.
     It brings up a window showing a list of the plots on the page and their
     sizes and positions.
     The Plot that you are about to add is shown on the bottom line.It will
     have been given a default X,Y Offset to position it on the film.
     The default offsetting puts plots 0.2" above the last plot. Pressing
     <Next> will start a new column of PCB's
     Up to 50 plots can be placed on a single piece of film.
     You can use manual offsets to pack plots onto a page but must be carefull
     they do not overlap. You must manually allow for the gaps between plots in
     your offset values. Offset values are in thou. Around each plot
     is a 0.15" border so plots must have offsets that put them 0.3" apart.
     At the end of each Plot line are a set of letter describing the particular
     plot type and enabled layers during that plot.
     eg 3:CðTOCLH  =plot 3, Checkplot, Top+Overlay+Labels+Comments+Hidden

<>DoubleSided Plotting     (see orientation drawings below)

     For economy and ease of manufacture the unique Double-Sided plot exists.
     The double sided plot allows top and bottom sides of PCB's to be plotted
     on a single sheet of film. The film emulsion will be on the correct side
     for both layers. When different pcbs, or multiple copies of a pcb are
     put on a single sheet, the two sides will match up properly. Similarly,
     the drill file will match the filmwork properly, and will only contain
     a single set of holes. Note that double sided plots must be either
     readable or non-readable.

<Automatic Double siding during Multiple Plotting

     When the Doublesided paper orientation is chosen, and the Layers selected
     are a top/bottom pair (eg Top & Bottom tracks, or Top & bottom overlays),
     the plot will automatically double side. The top layer will plot first,
     then the bottom layer. Note that the offsets are the same, but that the
     HiY value of the non-readable plot will be -ve.

     You can automatically double side different pcbs, multiple pcbs, and
     different plot types (eg Layers, Masks, Paste) for a job, onto a single
     sheet of film. This is no longer recommended, the autoPaste/Mask/Overlay
     feature is a better approach now.

<Manual Double Siding during Multiple Plotting

     Where the other side is in a different file, or is a different plot type
     (eg bottom=layerplot; top=RFplot), you can still double side.
     Just do the first plot. When you do the next plot, it is checked to see
     if could be the other side. If it is the offsets are automatically set to
     the same value. Note that the obverse must be plotted next, and that the
     pcbs must be exactly the same size.

     Orientation and Scaled Page Size show you the limits to plot within.The
     dimensions and Offsets shown are all in final (pcb) size units,So a page
     that is 12x6 inches at 1x is only 6x3 inches at 2x.

     Paper size/orientation and scale cannot be altered during multiple plots.
     NCDrill commands are only output during plotting of the bottom track layer

<P>  Plot this plot

<O>  Manually set offsets.Use this to patch many plots on one sheet.The Default
     offset gives .300 inch between PCBs,and stacks them vertically.

<N>  NewColumn: starts a new column of pcbs in the multiple plot

<C>  ClosePage (<z> on main screen) closes a multiple plot file.

<D>  Closes a botched multiple plot and dumps it without printing.

<Q>  return to main screen without doing any thing.

>>Customise Screen

<R>  RF Plots : RF Plots put a continuous gap around all pads and tracks not
     connected to the Ground/Power planes.This gap is chosen for best results
     on each particular pcb.

<L>  Solder Mask Oversize : It is normal for the solder mask silk screen to be
     slightly larger than the pads.This extra gap can be set here.

<D>  Dots in Pads: This is set for your pcb maker. NCDRilled, pth boards will
     normally have dots OFF, though not many manufacturers care. Note that dot
     size can be changed in the dictionary

<H>  Holes and Dots in SMD pads: Some users have single sided pads with holes.
     A pad with a hole size of 0 will never have a hole or dot. Note that the
     option to suppress unused top side pads removes much of the rationale for
     single sided pads with holes.

<F>  Thermal Relief Gap: sets the width of the gap around thermal reliefs

<M>  SMD Thermal Reliefs: Where an smd pad is tagged to gnd, when an RF PLOT is
     done it can be connected to the background copper either directly or by a
     Thermal relief.

<V>  Vias can be either octagonal or round.

<1>  When you are only plotting the bottom copper layer, then the program would
     have automatically put the bottom component overlay into the .psv file.
     With this option turned on, it will put the top side overlay into the .psv
     file instead. This will only happen when the bottom copper layer only is
     being printed.

<2>  Size Only from Copper Layers: Laser PC automatically determines the
     programs extent from the pcb file and uses this to offset the pcb during
     printing. However, if the overlay has lines going beyond the PCB, for
     example a connector or LED, then these will be included in the pcb's size.
     The problem arises when we try to do a multiple plot, and suddenly the
     pcbs are a long way apart. So if you set this then it will only take the
     size from the copper layers. But, beware that at present there is no
     clipping, so the .psv file may have one overlay extending onto the
     adjacent ones.

<3>  Multiplot Gap: Allows you to set the gap between pcbs in multiplots.
     When your boards are being routed to separte them, you may wish to set
     this to the tool size your pcb maker uses. The size is in thou. Eg 2.4mm
     is a 94 thou gap.

<P>  Sets the type of printer to be used.Different printers have different
     paper sizes and commands,so may produce incompatible files. We can add new
     printers for you, or new paper sizes. We need the PPD file for your
     printer, which you should get from the company that plots the files, or
     from ftp.adobe.com

<A>  Paper Size : 2 sizes (roughly A4,A3) are set for each printer.

<O>  Orientation:This changes the way the paper is oriented,and where the Plots
                 fall on the sheet.The DoubleSided is for multiple plotting
                 both sides of a PCB on 1 sheet of film.The plots match up when
     folded along the scale line,ÚÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄ¿  ÚÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄ¿
     and the emulsion is correct ³                    ³  ³ ÚÄÄÄÄÄÄÄÄÄ¿       ³
     on both top and solder sides³                    ³  ³ ³Top 2    ³       ³
                                 ³                    ³  ³ ÀÄÄÄÄÄÄÄÄÄÙ       ³
                                 ³                    ³  ³ ÚÄÄÄÄÄÄ¿          ³
                                 ³ÚÄÄÄÄÄÄÄÄÄÄÄÄ¿      ³  ³ ³top side         ³
                                 ³³            ³      ³  ³ ³plot 1³          ³
 ÚÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄ¿ ³³            ³      ³  ³ ÀÄÄÄÄÄÄÙ          ³
 ³ ÚÄÄÄÄÄÄÄÄÄÄ¿                ³ ³³            ³      ³  ³ scale......       ³
 ³ ³2nd Plot  ³                ³ ³³2nd Plot    ³      ³  ³ ÚÄÄÄÄÄÄ¿          ³
 ³ ÀÄÄÄÄÄÄÄÄÄÄÙ                ³ ³ÀÄÄÄÄÄÄÄÄÄÄÄÄÙ      ³  ³ ³Bottom³          ³
 ³ ÚÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄ¿        ³ ³ÚÄÄÄÄÄÄÄÄ¿          ³  ³ ³plot 1³          ³
 ³ ³                  ³        ³ ³³        ³          ³  ³ ÀÄÄÄÄÄÄÙ          ³
 ³ ³1st Plot          ³        ³ ³³1st Plot³          ³  ³ ÚÄÄÄÄÄÄÄÄÄ¿       ³
 ³ ÀÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÙ        ³ ³ÀÄÄÄÄÄÄÄÄÙ          ³  ³ ³Bottom 2 ³       ³
 ³ scale.......                ³ ³ scale......        ³  ³ ÀÄÄÄÄÄÄÄÄÄÙ       ³
 ÀÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÙ ÀÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÙ  ÀÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÙ
            Landscape                 Portrait          DoubleSided

<G>  Background Grid: This is useful for determining the printable area or
     accuracy of new printers.It puts a 1" labelled grid down,then plots PCB's
     over it.

<D>  Drill Support : Turns all Drill Reference functions on/off,this reduces
     memory/disk use,and speeds up conversion. (see below)

<F>  Default Drill Reference File : If this is set it will be used for loads/
     saves.If empty then they will default to the same name as the input file.

<I>  Laser PC works by converting the autotrax file to a postscript metafile.
     When you make a plot, selected layers of the metafile are sent to the
     printer. The DICTIONARY is all the commands the printer uses to execute
     the postscript lines in your plot. The dictionary is sent first to the
     printer, the the scaling, rotating, mirroring and other control commands
     for each particular plot, then the metafile lines needed for that plot.
     The DICTIONARY can be edited to change characteristics like thermal
     reliefs, text fonts (eg to make labels or comments bold) and so on.

<Z>  Text Sizes : You can change the scaling factor used when printing out
     the text on your PCBS. There are also several constants in LAX.DIC that
     can be altered to customise text. There is a default scale factor that
     makes a particular font match the height of the protel font, and you can
     change the fonts used for each type of text.

<C>  Client Name : This puts a Client name in the commemts at the page edge


>>Drill Support

LaserPC.. supports both NCDrilling (with RS274d files) and manual drilling
(with Drill Guides). Laser PC gets drill information from a Drill Reference.
This can be a Protel TOL file. However it will accept metric sizes, and comment
lines at the end.
-------------
T01  23           <------ thou
T02  1 mm         <------ will convert to thou
T03  1.5mm        <------ !!! BAD:crashes !!! put a gap before the <mm>
T04  1.2 mm       <------ Bad: drills must be in ascending order
T05  1.2 mm       <------ Warns you about a duplicate
T12  120          <------ accepts missing tools OK
T14  35 mm        <------ SORRY biggest drill is 1.024 inches
This is a comment line. Any line not starting in <T> terminates the file
You can have up to 20 Tools

<> Using Drill Support requires several steps.

1) Create .TOL file
2) LOAD Drill Reference
3) Plot files. Pad holes will be matched to the 1st drill that is >= diameter

3) NCDrill files will be generated only when plotting SOLDER LAYER,LAYER TYPE
   plots.They are always Top Veiw.They are only active when plotting to file,
   and are called <outputFilename>.NCD

4) You cannot Load another drill reference halfway through a multiple plot
5) A report file <PLOT_FILENAME.RPT> lists all the tools, holes sizes found,
   and what they were mapped to.
6) The Report File contains a list of all holes in the pcb, that can be used
   for a drill reference

<>
If you are doing multiple plots of the same PCB which will be drilled by a gang
drill machine,you can turn NCDRILLFILE OFF after the first plot.

Drill Co-Ordinates:When plotting the 0,0 point will be the bottom left corner
    ÚÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄ¿   of the first plot done.()
    ³  ÚÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄ¿                  ³   The NC co-ordinates are all
    ³  ³  plot 2        ³                  ³   generated Top veiwed,Drilling
    ³  ³                ³                  ³   machines however vary,and will
    ³  ÀÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÙ                  ³   often produce boards drilled
    ³  ÚÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄ¿               ³   from the bottom veiw.
    ³                     ³               ³   Before saving an .NCD the holes
    ³  Y                   ³               ³   are sorted into inch squares for
    ³  ³                   ³               ³   rapid drilling.
    ³  ÄÄÄÄ X ->ÄÄÄÄÄÄÄÄÄÄÙ               ³
    ³ scale........                        ³
    ÀÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÄÙ


<> General Stuff

Along the edge of each plot is the size,PCB filename,and Pcb file Date/time.
It also has the plot type string eg L T   means Layer plot; Top
If it ends with >>:N there has been a stack error (see below)
At the edge of the whole sheet the scale and plot date/time is shown.

<Text on PCB's: Note that LaserPC.... does not produce identical results to
              Protel Plot. In particular,text is a little shorter and much
              narrower. You can change fonts, sizes, and boldness, by editing
              the DICTIONARY.

<Copyright Symbol can now bu put on PCBs.If a text string is (c) or (C) then a
              copyright symbol will be printed instead.
              Note that strings containing \ (backslash) are not allowed
              (a space will be substituted). [ to be fixed]

<Config files (.cfg) are automatically saved.They are in plain text/numbers.The
first line is a title,and begins with the config file version number.LPC checks
this and only loads its current type.Config files include all the information
about the printers supported,the types of paper size,printable regions for each
paper type and special postscript strings needed to activate non-default sizes.
To change any of these you can edit the CFG file directly. Have a look in the
.cfg file, several important switches can only be changed by editing them
directly. From V6.24, LAX endeavours to read older cfg files, but it may not
succeed. If evrything turns to shit after upgrading, try deleting the cfg file.

< Running Under Windows
There are no real problems running under windows apart from the messy way
windows has to use to pass more than 1 parameter to dos programs. You will also
find that you cannot send a PS file straight to the printer under windows, but
will have to shell to dos to do this.

<Drag and Drop operation:
To do this you will need to edit the PIF files, so that all the paths refer to
your system not ours! To use, you drag and drop a file on the PIF icon, and it
will launch a batch file that will run LAX, with the appropriate .cfg file for
the type of plot you are doing. The basic LAX icon just runs LAX and loads the
PCB for you. There are a variety of icons for variuos things. For each special
configuration you need to make a suitable .cfg file and batch file. Set LAX up
with the options you want , the go into the customise screen, and SAVE the CFG
file. When you quit the program, it only saves into LAX.CFG, any changes to
other .cfgs must be saved explicitly.


<> Inside the Postscript Files

If you look in the PS files there are a number of informative comment lines,
in particular, they tell you about positive/negative and readable/non-readable
state of this file.

<Debugging Postscript Files:

When you start playing with the Postscript dictionary, you may well have
problems. One of the most common problems is caused by routines that do not use
all the operands that have been placed on the stack. Small test PCB's will
print perfectly, but large files crash. The routine CHECKSTACK is run after
each plot. If there was anything left on the stack, the pcb's string will end
with >>:N   where N is the number of operands left on the stack.
2.12 by 2.54 inch digmix.pcb 21:11 1994 11 23 L T>>:16
  ie the stack was not empty when finished, 16 operands left on it.

<> So You Don't have a POSTSCRIPT Printer?

Ghostscript:

GS is a free interpreter for the PC. I use it under Windows. You can use it in
two ways. Either with GVIEW as a viewer/printer program, ie you load the file
into the program and look at it, or by using GSGRAB, which looks for a file
called GSGRAB to appear, the automatically renders and/or prints it. This is
what the "Output Emulator" option supports.
With the release of v3 of Ghostscript, it is finally able to reliably deal with
the graphics load of PCB's (not that they are very complicated).
Ghostscript is free. You find the latest copy on the internet. The home site
for Web browsers is http://www.cs.wisc.edu/~ghost/index.html, and you get the
files from ftp.cs.wisc.edu/pub/ghost
You will require 4 files, get at least this version.
 gs333w32.zip gs333ini.zip gs333fn1.zip gsview13.zip
This gives you a full windows program for viewing and printing postscript files
which can print to a wide range of printers. You will see that text quality is
poor if you need better text quality, you need to get a set of basic Adobe
Type 1 fonts.
The file that is used is set by a commented line in the .cfg file. It is also
possible to run a batch file after the spool file has been written to trigger
or perform the rendering. How you trigger a windows process from dos I have no
idea...

There are a number of commercial systems that do the same sort of thing,
probably much more elegantly. Some GDI laser printers now come with a PC hosted
PS interpreter.

Corel Draw 5 : Users have reported that using this a a viewer works well
<>
<New Features:
     TabloidExtra paper size 18x12 inch
     Client name on the edge of sheets.
     4 Postscript machines are supported (with different printable areas)
     Background Grid to find printable area of your machine.
     LPC is now CRC checked against viruses
     LPC <Pcbfile> will load the file automatically on entry
     Copyright Symbol on PCBs.
     Encapsulated Postscript Now supported.
     Debug puts "executive" in files.
     Shell to Dos
     Drilling guides for manual drilling
     NCDrill files.
     Thermal Reliefs.
     Octagonal Pads.
     Check plots now do Ground and power planes.
     Possible to use fine Halftone screens.(see Config Files)
     Vias can have a larger size for non-pth prototypes.
     LPT3,COM3,COM4 added to printer list
     Autotrax support (v6)
     Automatic placement of multiple plots
     Automatic multiple plotting of double-sided plots
     Increased number of multiple plots to 50
     Multiple plot now checks for overflowing the page
     New Column always places beyond any pcb in previous columns
     Vias can be covered in solder mask(pth) or uncovered (DS, no pth)
     EPS files automatically modofied for MSWOrd compatibitiy
     plot key string on film in multiple plots
     Stack monitor added to postscript to aid dictionary debugging
     Now shows number of holes in pcbs 6.06
     Drill file correctly matches all mirroring options (6.07)
     Changable text sizes (6.08)
     added %%Page comment in psfile, to aid browsers
     modified EPSfix to strip out the device specific line from PS files so
       that they can be read with GhostScript.
     Now you choose to display hidden labels & comments
     Auto stripping of unused top side pads. (layer,mask,rf,check plots)(6.1)
     Check Plots of bottom side & bottom overlay will be readable
     GETs automatically after input file is changed, and at startup.
     Automatic orientation of paper for best fit (6.20)
     Automatic selection of paper size that fits during command line loads
     Automatic Step and Repeat operation
     Generates solder mask and solder paste plots automatically during plot
     Automatic operation from command line, support for Drag and Drop
     Double sided plots can have either or both sides RF or normal plots
     <esc> to abort printer jobs
     <AltX> <AltF4> quits
     Forces double sided plots to readable or unreadable not topveiw
     Automatic generation of component overlays.
     6.22-better interlocks, auto-overlays added
     6.23-minor fix to auto double siding detection in multiple plot screen
     6.24 Added Print to PS Emulator support for users with Laserjet,Inkjet etc
          add moire&target to dictionary, fix arc sector problem
          Option for holes and dots in smd pads on/off
	  added new DSC comments to help GS
	  epsfix 1.1 comments out page activator line
	  fix soldermask problems in Ground Planes
	  improve boundary accuracy
     6.25 When single sided (bottom) plots, the overlay can be of the top overlay
	     in the .psv file
	  When getting files, the size is taken from the pcb. Some components
	     eg connectors protrude outside the pcb on the overlay. Size can
	     be taken solely from the copper layers (incl gnd,pwr,board)
	     At present this will mean overlays speading onto adjacent pcbs in
             the silkscreen
	  The gap between pcbs can be altered to get better packing, or to
            allow a single router cut for routing (gap=108thou ->3mm router)
	  Unused Pads can be stripped on the bottom layer as well.
	  fix bug in ps arc draw routine
	  autoscale always fits in plot
	  Check plots now support separate (doble-sided) top and bottom
     6.27
        remove unused tool numbers from header of the NCD
        change page numbering to stop ghostscript bitching
        fix negative NCStr problem
     6.28
        remove duplicate drill holes
        Increased number of holes to 4366 per pcb + 13100 total
        during multiple plots, use a clip-path to prevent overlap in the .psv


<Problems:

What to do if you find a problem.

Make a simple demo pcb that illustrates the problem. Printout an example of
the problem and mark and describe it. Send (by disk or preferably e-mail)
the following: The pcb, a description of how to get the problem, the sample, and
all your LAX files. I am probably using a more recent version than you.

Known problems and plans:
date in plot edge in wrong order.too hard to fix.
Doesn't handle Insufficient Disk Space problems in Get adequately.
Crashes if insufficient disk space writing NCDrill file

Drill Plots flakey (they are obsolescent now)

Limits:
  Number of multilayer holes in a single pcb during GET phase: 4366
  Total number of NC Drill holes it is capable of sorting : 13100
  Maximum number of plots on a single sheet : 50
  Size of PCB's and Film : 32"

Goals: ver7.
generates .tol files without a manual drill read command
.tol files ignore header lines
.tol file copes with tools in any order
display of primitive numbers
automate drill file load and generate,
BOM operation?
Unused pad stripping could detect lines that cross pads not just end in them
look at ps3 dsc: new media selection regime
look at ppd file format
some recent features are not saved to the config file.

detect offset overlapping holes
count of holes sizes
small annulus left on top side when pads are removed. Tagged to the actual drill size?
seems to take size from copper track layers, but not from pads


Please add any other problems or better explanations to this file and send me
a copy. (with your program version number and details)
<
________________________________________________________________________________

		   License and Registration

Broadcast Equipment releases this application for the use of anyone under the BSD sytle
license. see sourceforge for details.

If you require support or customisation of this program for your commercial purposes
feel free to enquire about buying assitance from Broadcast Equipment
+64 21 623-402
crun@users.sourceforge.net