X-Authentication-Warning: delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient: geda-user AT delorie DOT com
From: geda AT psjt DOT org (Stephan =?utf-8?Q?B=C3=B6ttcher?=)
To: "Nicklas Karlsson \(nicklas.karlsson17\@gmail.com\) \[via geda-user\@delorie.com\]" <geda-user AT delorie DOT com>
Subject: Re: [geda-user] Re: DRC clearance work in progress
References: <CAJXU7q-STU6GSxZSoes5DozwVVZunXCzWt8QVhU8iAXWwSt=dA AT mail DOT gmail DOT com>
	<001a1134f920c49e910527d3a068 AT google DOT com>
	<CAJXU7q-N=dNaK=3pV8t14pxDNFROqW4u4MjAc8EEWODmOYVYbA AT mail DOT gmail DOT com>
	<s6n8u4frkhi DOT fsf AT blaulicht DOT dmz DOT brux>
	<20151227173145 DOT 4f52bd9239ac5e14b8966e07 AT gmail DOT com>
Date: Sun, 27 Dec 2015 17:55:36 +0100
In-Reply-To: <20151227173145.4f52bd9239ac5e14b8966e07@gmail.com> (Nicklas
	Karlsson's message of "Sun, 27 Dec 2015 17:31:45 +0100")
Message-ID: <s6nio3jq19z.fsf@blaulicht.dmz.brux>
User-Agent: Gnus/5.13 (Gnus v5.13) Emacs/24.5 (gnu/linux)
MIME-Version: 1.0
Content-Type: text/plain
Reply-To: geda-user AT delorie DOT com
Errors-To: nobody AT delorie DOT com
X-Mailing-List: geda-user AT delorie DOT com
X-Unsubscribes-To: listserv AT delorie DOT com
Precedence: bulk

"Nicklas Karlsson (nicklas DOT karlsson17 AT gmail DOT com) [via
geda-user AT delorie DOT com]" <geda-user AT delorie DOT com> writes:

>> "Peter Clifton (petercjclifton AT googlemail DOT com) [via
>> geda-user AT delorie DOT com]" <geda-user AT delorie DOT com> writes:
>> 
>> > Focus on within-layer clearances for now.
>> >
>> > Any more complex design rules (such as dielectric breakdown through
>> > the layer stack) requires more data than we have in PCB's data-model,
>> > and may actually belong in a separate calculation utility that would
>> > calculate out a geometric design rule that can be applied in PCB.
>> 
>> I am playing with the idea to build a DRC tool that works on the gerber
>> output, using libgerbv and the clipper library (C++)
>> 
>>  http://angusj.com/delphi/clipper.php
>> 
>> I have made Python bindings for importing gerbers into clipper polygon
>> data structures, perform bloating/shrinking and clipping operations.
>> 
>> Design rules would be specified as boolean operations on suitably bloated
>> layer data, and anything left in the end is a violation.
>> 
>> An example that I have working now:
>> 
>>  from pyclipper import Clipper, gerbv, OffsetPolygons
>>  proj = gerbv.project()
>>  proj.load("v01.front.gbr")
>>  proj.load("v01.plated-drill.cnc")
>>  scale=10000
>>  raw     = proj[0].polygons(scale)
>>  drill   = proj[1].polygons(scale)
>>  clip = Clipper()
>>  clip.clear() 
>>  clip.addsubject(raw)
>>  # clean up, and remove keyholes
>>  routing = OffsetPolygons(clip.union(),1)
>>  # require 12 mil annuklar rings
>>  annular = OffsetPolygons(drill, 120)
>>  clip.clear()
>>  clip.addsubject(annular)
>>  clip.addclip(routing)
>>  annular = clip.difference()
>> 
>> Any polygon left in annular is a violation.
>> 
>> For net specific rules I'd need to add some input that gives for each
>> net at least one coordinate (per relevant layer).  And some code to find
>> the polygon at the given coordinate.  Some rules, like clearance checks,
>> require iterations over the individual ploygons in a layer.  At that
>> point they could be tagged with a netname by the given coordinates.  And
>> then there could be overrides of bloat values for specifiv nets.
>> 
>> I plot the ploygons with gnuplot right now.  A gerber export may be
>> usefull to visualize the violations in gerbv.  Or some gui.
>
> Great!
>
> I think your work will would be useful within pcb to.
>
> Simple scale will give a little bit to large distance value in outer
> corner, attached picture, there need to be a circle segment but it
> could be fixed later at any point and to large distance is usually
> less of a problem than to small distance.

Currently my Python bindings only support circle segments, but the
Clipper library can do other corner handling as well :-)

> Nicklas Karlsson

-- 
Stephan