Provided by: gerbv_2.7.0-1_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.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