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.geda-project.org/).

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<XxYrR|X;YrR>|--translate=<XxYrR|X;YrR>
              Translate image by X and Y and rotate by R degree. Use multiple -T  flags  to  translate  multiple
              files. Distance defaults to inches but may be changed with --units.  Only evaluated when exporting
              as RS274X or drill.

       -O<XxY|X;Y>|--origin=<XxY|X;Y>
              Set  the  lower  left  corner  of the exported image to coordinate <XxY>.  Coordinates defaults to
              inches but may be changed with --units.

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

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

       -u<inch/mm/mil>|--units=<inch/mm/mil>
              Use given unit for coordinates. Default to inches.

       -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 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.

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 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.

ALIGNING OF LAYERS

       You can align two layers by selected elements. Select one element on each of two layers and  click  Align
       layers from context menu.

ZOOMING

       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.

MEASUREMENTS

       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.  To measure distance between elements select two of them and switch to Measure 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.

SUPERIMPOSING

       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 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 exercise 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.

PICK&PLACE FILE

       Supported comma separated file (CSV) with fixed order of data:

            # X,Y in mils.
            Designator,"Description","Value",X,Y,"Rotation (deg)",top/bottom

            or

            Designator,"Footprint","Mid X","Mid Y","Ref X","Ref Y",
                      "Pad X","Pad Y",T/B,"Rotation","Comment"

       Units  can  be  specified  in  format  "#  X,Y in mils." or as suffix for X/Y-coordinates, i.e ",10mil,".
       Supported units: in, mil, cmil, dmil, km, m, dm, cm, mm, um, nm.

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

Version                                           Jule 13, 2013                                         gerbv(1)