X-Authentication-Warning: delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient: geda-user AT delorie DOT com
Message-ID: <4F119E96.4060305@mcmahill.net>
Date: Sat, 14 Jan 2012 10:26:14 -0500
From: Dan McMahill <dan AT mcmahill DOT net>
User-Agent: Mozilla/5.0 (Windows NT 6.0; rv:8.0) Gecko/20111105 Thunderbird/8.0
MIME-Version: 1.0
To: geda-user AT delorie DOT com
Subject: Re: [geda-user] Standalone DRC for Gerber files
References: <57691326464791 AT web158 DOT yandex DOT ru>
In-Reply-To: <57691326464791@web158.yandex.ru>
Content-Type: text/plain; charset=ISO-8859-1
Content-Transfer-Encoding: 7bit
Reply-To: geda-user AT delorie DOT com

On 1/13/2012 9:26 AM, Dmitry Dzhus wrote:
> Hello!
> 
> I'm looking for a tool which would allow to perform design rule checking
> for PCB files in Gerber format. Any ideas if the code from gEDA's pcb
> can be used for that? At first glance it seems like pcb can only check
> files of its own format and its code is tied with GUI. I need something
> capable of doing batch testing.
> 
> Any relevant book recommendations about how DRC is implemented in general,
> since I think I'll start writing it if no suitable free software solution comes up?
> 

pcb only checks a database in its own format.  I think adding some
ability to do checking with the gerbv program would be useful.  I
mention gerbv since that project already has a complete RS274-X parser.
 You may also find some useful ideas in the program called "boolean".
Also you may want to look at "magic" which is an IC layout tool and see
what DRC capabilities it has.

If you were looking to write a more or less general purpose DRC engine
it is most useful to have a programming interface that allows you to do
various operations on layers such as grow/shrink, boolean operations
like and/not/or/xor, etc.  This would allow both a sort of standard drc
deck to be written as well as allowing users to expand into more
difficult tests.  As an example, here is how you may do a rudimentary
minimum spacing rule.

// import top copper
top = layer("top")

// grow the layer and then shrink it back.  If any copper
// started to touch after the grow operation, then the gap
// will not reappear after the shrink and we'll get a different
// answer than we started with
top2 = shrink( grow( top, 5 mil), 5 mil)

top_min_gap_error = error("violated min spacing", xor(top, top2))

hope this makes sense.  The boolean program offers some of these
operations.  No idea about magic.  You'd probably need to do some work
on how layers are represented in either pcb or gerbv to make it
compatible with layer manipulation like this.

-Dan