Provided by: gerbv_2.6.0-1_amd64 bug

NAME

       gerbv - Gerber Viewer

SYNOPSIS

       gerbv [OPTIONS] [gerberfile[s]]

DESCRIPTION

       gerbv  is  a  viewer  for  RS274-X,  commonly  known  as Gerber, files.  RS274-X files are generated from
       different PCB CAD programs and are used in the printed circuit board manufacturing process.   gerbv  also
       supports  Excellon/NC  drill  files  as  well  as  XY  (centroid)  files  produced  by  the  program  PCB
       (http://pcb.sf.net).

OPTIONS

       Warning!  On some platforms, which hasn't long option available, only short options are available.

   gerbv General options:
       -V|--version Print the version number of gerbv and exit.

       -h|--help
              Print a brief usage guide and exit.

       -b<hex>|--background=<hex>
              Use background color <hex>. <hex> is specified as an html-color code, e.g. #FF0000 for Red.

       -f<hex>|--foreground=<hex>
              Use foreground color <hex>. <hex> is specified as an html-color code, e.g. #00FF00 for Green. If a
              user  also wants to set the alpha (rendering with Cairo) it can be specified as an #RRGGBBAA code.
              Use multiple -f flags to set the color for multiple layers.

       -l <filename>|--log=<filename>
              All error messages etc are stored in a file with filename <filename>.

       -t <filename>|--tools=<filename>
              Read Excellon tools from the file <filename>.

       -p <project filename>|--project=<project filename>
              Load a stored project. Please note that the project file must be stored in the same  directory  as
              the gerber files.

   gerbv Export-specific options:
       The  following  commands  can  be used in combination with the -x flag: -B<b>|--Border=<b> Set the border
       around the image <b> percent of the width and height.  Default <b> is 5%%.

       -D<XxY>or<R>|--dpi=<XxY>or<R>
              Resolution (Dots per inch) for the output bitmap. Use <XxY>  for  different  resolutions  for  the
              width  and  height  (only  when  compiled  with  Cairo as render engine). Use <R> to have the same
              resolution in both directions.  Defaults to 72 DPI in both directions.

       -T<X,Y>|--translate=<X,Y>
              Translate the image by the distance <X,Y>. Use multiple -T flags to translate multiple files.

       -O<XxY>|--origin=<XxY>
              Set the lower left corner of the exported image to coordinate <XxY>.  Coordinates are in inches.

       -a|--antialias
              Use antialiasing for the generated output-bitmap.

       -o <filename>|--output=<filename>
              Export to <filename>.

       -W<WxH>|--window_inch=<WxH>
              Window size in inches <WxH> for the exported image.

       -w<WxH>|--window=WxH>
              Window size in pixels <WxH> for the  exported  image.  Autoscales  to  fit  if  no  resolution  is
              specified  (note that the default 72 DPI also changes in that case). If a resolution is specified,
              it will clip the image to this size.

       -x<png/pdf/ps/svg/rs274x/drill>|--export=<png/pdf/ps/svg/rs274x/drill>
              Export to a file and set the format for the output file.

   GTK Options
       --gtk-module=MODULE Load an additional GTK module

       --g-fatal-warnings
              Make all warnings fatal

       --gtk-debug=FLAGS
              GTK debugging flags to set

       --gtk-no-debug=FLAGS
              GTK debugging flags to unset

       --gdk-debug=FLAGS
              GDK debugging flags to set

       --gdk-no-debug=FLAGS
              GDK debugging flags to unset

       --display=DISPLAY
              X display to use

       --sync Make X call synchronous

       --no-xshm
              Don't use X shared memory extension

       --name=NAME
              Program name as used by the window manager

       --class=CLASS
              Program class as used by the window manager

GENERAL

       When you start gerbv you can give the files to be loaded  on  the  command  line,  either  as  each  file
       separated with a space or by using wildcards.

       The  user  interface  is graphical. Simply press left mouse button and the image will pan as you move the
       mouse. To manipulate a layer, right-click on one of the rightmost buttons. That will bring  up  a  pop-up
       menu where you can select what you want to do with that layer (load file, change color, etc).

       If  you hold the mouse button over one the rightmost button a tooltips will show you the name of the file
       loaded on that layer.

ACTIVATION AND DEACTIVATION OF LAYERS

       You can load several files at one time. You can then turn displaying of the layers on and off by clicking
       on one of the rightmost buttons.

       You  can  also  control  this  from  the  keyboard.  Press  Alt,  enter  the number on the layer you want
       activate/deactivate on the numerical keypad and then release the Alt key.

ZOOMING

       Zooming can be handled by either menu choices, keypressing, middle mouse button or scroll wheel.  If  you
       press  Alt+I  you will zoom in and if you press Alt+O you will zoom out. If you press middle mouse button
       you will zoom out, and if you press Shift and middle mouse button you will zoom in.  Scroll  wheel  works
       if  you enabled that in your X server and mapped it to button 4 and 5. You can also zoom in by pressing z
       and zoom out by pressing shift+z (ie Z). You can make the image fit by pressing f (there is also  a  menu
       alternative for this).

       You  can  also do zooming by outline. Press right mouse button, draw, release.  The dashed line shows how
       the zooming will be dependent on the resolution of the window. The non-dashed outline will show what  you
       actually selected. If you change your mind when started to mark outline, you can always abort by pressing
       escape. By holding down the shift key when you press the right mouse button,  you  will  select  an  area
       where the point you started at will be the center of your selection.

MEASUREMENTS

       You  can do measurement on the image displayed. By pressing shift, the cursor changes to a plus. By using
       left mouse button you can draw the lines that you want to measure.  The result of the last measurement is
       also displayed on the statusbar.  All measurements are in the drawing until you either zoom, pan or press
       the escape key.

       The statusbar shows the current mouse position on the layer in the same coordinates as in the file. Ie if
       you  have (0,0) in the middle of the image in the gerber files, the statusbar will show (0,0) at the same
       place.

SUPERIMPOSING

       When you load several Gerber files, you can display them "on top of each other",  ie  superimposing.  The
       general  way  to  display them are that upper layers cover the layers beneath, which is called copy (GTK+
       terms).

       The other ways selectable are and, or, xor and invert. They map directly to  corresponding  functions  in
       GTK.  In  GTK  they  are  described  as:  "For  colored images, only GDK_COPY, GDK_XOR and GDK_INVERT are
       generally useful. For bitmaps, GDK_AND and GDK_OR are also useful."

PROJECTS

       gerbv can also handle projects. A project consist of bunch of loaded layers with their  resp.  color  and
       the  background  color.  The easiest way to create a project is to load all files you want into the layer
       you want, set all the colors etc and do a "Save Project As...".

       You load a project either from the menu bar or by using the commandline switches -p or --project.

       Currently there is a limit in that the project file must be in the same directory as the gerber files  to
       be loaded.

SCHEME

       The  project  files  are simple Scheme programs that is interpreted by a built in Scheme interpreter. The
       Scheme interpreter is TinyScheme and needs a Scheme program called init.scm  to  initialize  itself.  The
       search  path  for  init.scm  is  (in the following order) /usr/share/gerbv/scheme, the directory with the
       executable gerbv, the directory gerbv was invoked from and finally according to the environment  variable
       GERBV_SCHEMEINIT.

TOOLS FILE

       Not  every  Excellon  drill  file  is  self-sufficient. Some CADs produce .drd files where tools are only
       referenced, but never defined (such as what diameter of the tool is.) Eagle CAD is one of such CADs,  and
       there are more since many board houses require Tools files.

       A Tools file is a plain text file which you create in an editor. Each line of the file describes one tool
       (the name and the diameter, in inches):

            T01 0.024
            T02 0.040
            ...

       These are the same tools (T01 etc.) that are used in the Drill file.  A standard practice with  Eagle  is
       to  create  an  empty  Tools  file, run the CAM processor, and the error report tells you which tools you
       "forgot".  Then you put these tools into the file and rerun the CAM processor.

       You load a tool file by using the commandline switches -t or --tools.  The file can  have  any  name  you
       wish,  but  Eagle  expects  the file type to be ".drl", so it makes sense to keep it this way. Some board
       houses are still using CAM software from DOS era, so you may  want  to  excercise  caution  before  going
       beyond the 8.3 naming convention.

       When  gerbv  reads  the  Tools file it also checks that there are no duplicate definitions of tools. This
       does happen from time to time as you edit the file by hand, especially if  you,  during  design,  add  or
       remove parts from the board and then have to add new tools into the Tools file. The duplicate tools are a
       very serious error which will stop (HOLD) your board until you fix the Tools file and maybe the  Excellon
       file. gerbv will detect duplicate tools if they are present, and will exit immediately to indicate such a
       fatal error in a very obvious way. A message will also be printed to standard error.

       If your Excellon file does not contain tool  definitions  then  gerbv  will  preconfigure  the  tools  by
       deriving  the diameter of the drill bit from the tool number. This is probably not what you want, and you
       will see warnings printed on the console.

ENVIRONMENT

       GERBV_SCHEMEINIT
              Defines where the init.scm file is stored. Used by  scheme  interpreter,  which  is  used  by  the
              project reader.

AUTHOR

       Stefan Petersen (spetm at users.sourceforge.net): Overall hacker and project leader
       Andreas Andersson (e92_aan at e.kth.se): Drill file support and general hacking
       Anders Eriksson (aenfaldor at users.sourceforge.net) : X and GTK+ ideas and hacking

COPYRIGHT

       Copyright ©  2001, 2002, 2003, 2004, 2005, 2006, 2007, 2008 Stefan Petersen

       This document can be freely redistributed according to the terms of the
       GNU General Public License version 2.0