Skip site navigation (1)Skip section navigation (2)

FreeBSD Manual Pages

  
 
  

home | help
gerbv(1)			     2.7.0			      gerbv(1)

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  pro-
       duced 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  lay-
	      ers.

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

       -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 com-
	      piled with Cairo as render engine). Use <R>  to  have  the  same
	      resolution  in  both directions.	Defaults to 72 DPI in both di-
	      rections.

       -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 ex-
	      porting 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 num-
       ber  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  but-
       ton,  draw,  release. The dashed	line shows how the zooming will	be de-
       pendent 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	selec-
       tion.

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 se-
       lect 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  di-
       rectly to corresponding functions in GTK. In GTK	they are described as:
       "For colored images, only GDK_COPY, GDK_XOR and GDK_INVERT  are	gener-
       ally 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/lo-
       cal/share/gerbv/scheme, the directory with the  executable  gerbv,  the
       directory  gerbv	was invoked from and finally according to the environ-
       ment 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	dupli-
       cate  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	inter-
	      preter, 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 (C)  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)

NAME | SYNOPSIS | DESCRIPTION | OPTIONS | GENERAL | ACTIVATION AND DEACTIVATION OF LAYERS | ALIGNING OF LAYERS | ZOOMING | MEASUREMENTS | SUPERIMPOSING | PROJECTS | SCHEME | TOOLS FILE | PICK&PLACE FILE | ENVIRONMENT | AUTHOR | COPYRIGHT

Want to link to this manual page? Use this URL:
<https://www.freebsd.org/cgi/man.cgi?query=gerbv&sektion=1&manpath=FreeBSD+12.2-RELEASE+and+Ports>

home | help