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.

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