Provided by: gerbv_2.6.0-1_amd64 bug


       gerbv - Gerber Viewer


       gerbv [OPTIONS] [gerberfile[s]]


       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 (


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

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

              Print a brief usage guide and exit.

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

              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

       -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%%.

              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.

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

              Set  the  lower left corner of the exported image to coordinate <XxY>.  Coordinates
              are in inches.

              Use antialiasing for the generated output-bitmap.

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

              Window size in inches <WxH> for the exported image.

              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.

              Export to a file and set the format for the output file.

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

              Make all warnings fatal

              GTK debugging flags to set

              GTK debugging flags to unset

              GDK debugging flags to set

              GDK debugging flags to unset

              X display to use

       --sync Make X call synchronous

              Don't use X shared memory extension

              Program name as used by the window manager

              Program class as used by the window manager


       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.


       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  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.


       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.


       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


       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

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

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


       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.


       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.


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


       Stefan Petersen (spetm at Overall hacker and project leader
       Andreas Andersson (e92_aan at Drill file support and general hacking
       Anders Eriksson (aenfaldor at : X and GTK+ ideas and hacking


       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