gerbv(1) cvs-20051023 gerbv(1)
NAME
gerbv - Gerber Viewer
SYNOPSIS
gerbv [OPTIONS] [gerberfile[s]]
DESCRIPTION
gerbv is a viewer for Gerber files. Gerber files is generated from dif-
ferent PCB CAD programs and are sent to subcontractors to actually make
the PCB. gerbv also supports Excellon/NC drill files.
OPTIONS
Warning! On some platforms, which hasn’t long option available, only
short options are available.
gerbv Options
-V|--version Prints the version number of gerbv and exits.
-h|--help
Prints a brief usage guide.
-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>.
--geometry=<width>x<height>[<+->x-position[<+->y-position]]
Sets the the size of the window. X-position and y-position are
currently ignored by gerbv.
-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.
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 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.
Default of concurrently loaded files are 20 layers. You can change this
during configure with:
./configure with-maxfiles=<number>
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 the rightmost buttons.
You can also control this from the keyboard. Press Alt, enter the num-
ber on the layer you want activate/deactivate on the numerical keypad
and then release the Alt key.
ZOOMING
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 alternativ 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 out-
line, 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 selec-
tion.
MEASUREMENTS
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.
SUPERIMPOSING
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 gen-
erally 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/local/gEDA-20060124/share/gerbv/scheme/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 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.
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 © 2001-2004 Stefan Petersen
This document can be freely redistributed according to the terms of the
GNU General Public License version 2.0
Version Feb 8th, 2004 gerbv(1)