Provided by: gerbv_2.6.1-3_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:

              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 and drag middle mouse button (scroll wheel)
       and the image will pan as you move the mouse. To manipulate a layer, right-click on one of
       the  rightmost  list items. That will bring up a pop-up menu where you can select what you
       want to do with that layer (reload 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 check boxes near the layer names.

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


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

       You can also do zooming by outline. Select Zoom Tool, press 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 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. Select Measure Tool, 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 select other Tool.

       The statusbar shows the current mouse position on the layer in the same coordinates as  in
       the  file.  I.e.  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",  i.e.
       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