X-Authentication-Warning: delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient: geda-user AT delorie DOT com
X-Original-DKIM-Signature: v=1; a=rsa-sha256; c=relaxed/relaxed;
        d=gmail.com; s=20120113;
        h=date:from:to:subject:message-id:in-reply-to:references:mime-version
         :content-type:content-transfer-encoding;
        bh=DFT1A7/SUBw0ECHkJ/IRvuqxS28NKo+bXaLFL9EvoPg=;
        b=u9qQj5/RT+Z1dWozw4dnk2nDPx09QiCyb55hvOrScQmoZSgrdYYhPJVYIJ5SNwXzsa
         f9RTCJpxbU41CNgQIEUTUEiD0wWnuBgnIrfWGj0eupoMpgpRVBkPZk0jjXuJEyzoeNpy
         nx08meejiX53gFygasPZQChn8Zps9Y/UZZeiiyC1X4dHXTSiZYiuyPQ7NVdbiVgg6zQ8
         ekS8lFXpX22aRNi/mty3FiwNmCqrH21R389+j4FzJREoBEPL7tCp3Q7KFB21ob6u25PR
         Nnl/nv2+zOti2lFgIJfJCG/VaGo0rB7H/oZWNw/XORMSQ62uhLoLZIldQgauTIjvcF34
         onoQ==
X-Received: by 10.28.22.199 with SMTP id 190mr21389774wmw.54.1451378416153;
        Tue, 29 Dec 2015 00:40:16 -0800 (PST)
Date: Tue, 29 Dec 2015 09:40:14 +0100
From: "Nicklas Karlsson (nicklas DOT karlsson17 AT gmail DOT com) [via geda-user AT delorie DOT com]" <geda-user AT delorie DOT com>
To: geda-user AT delorie DOT com
Subject: Re: [geda-user] Gerber designrule checking with libgerbv and
 Clipper
Message-Id: <20151229094014.33731b1cbe1c3f48673c42ea@gmail.com>
In-Reply-To: <s6nr3i6hsvy.fsf_-_@blaulicht.dmz.brux>
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>
	<s6nio3jq19z DOT fsf AT blaulicht DOT dmz DOT brux>
	<s6nr3i6hsvy DOT fsf_-_ AT blaulicht DOT dmz DOT brux>
X-Mailer: Sylpheed 3.5.0beta1 (GTK+ 2.24.25; x86_64-pc-linux-gnu)
Mime-Version: 1.0
Content-Type: text/plain; charset=ISO-8859-1
Content-Transfer-Encoding: 8bit
X-MIME-Autoconverted: from quoted-printable to 8bit by delorie.com id tBT8eM07016729
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

You are spot on!

This is the way to do it. It should work equally if part of pcb.



> 
> Moin,
> 
>              A tool to perform DRC on Gerber files.
> 
> This new project is working for me now.  Not much documentation yet, but
> it's not a lot of code, and includes a test case.
> 
>    http://www.psjt.org/code/
>    http://www.psjt.org/code/drc
>    http://www.psjt.org/code/drc.tar.gz
> 
> The Clipper library can do polygon operations, including offsetting.  I
> am using the C++ version.
> 
>    http://angusj.com/delphi/clipper.php
> 
> Libgerbv is used to read Gerber and drill files into Clipper polygons,
> and to write Clipper polygons to Gerber files.  I needed to patch
> gerbv a bit:
> 
>    http://www.psjt.org/code/drc/gerbv-create-polygon.patch
> 
>  * utility functions to create libgerbv polygons
> 
>  * implement gerbv_image_create_rectangle_object() using those
>    functions
>   
>  * fix a buf in gerbv_export_rs274x_file_from_image() (pointer lifetime)
> 
> Clipper is also patched to make it accept a single point as a polygon,
> that can then be offset into a circle.
> 
>    http://www.psjt.org/code/drc/polyclipping-degenerate-ploynoms.patch
> 
> All that is wrapped into Python bindings.
> 
> 
> As I said, it works for me, but I don't know why.  I know next to
> nothing about Gerber, and I looked at the Gerbv code just enough to make
> it do what I want.  The Gerber export is broken as soon as there are
> holes in the exported polygons.  Most DRC violations don't have holes,
> and when they do, they are drawn without.
> 
> Four generic tests are included in the main program.  The idea is that
> special tests can be easily added by the user, in Python.
> 
> Here's a screenshot with some clearance and width violations:
> 
>   http://www.psjt.org/code/drc/screenshot.png
> 
> 
>  * minimum drill size.
>     - shrink the drill layer by the minimum radius
>     - rebloat the layer 
>     - subtract the rebloated layer from the drill layer
>    Small holes will be lost when shrinking and remain on the result layer.
> 
>  * minimum annular ring size.
>     - bloat the plated drill layer
>     - subtract the routing layer
>     What is left is missing annular ring
> 
>  * minimum trace width.
>    This one gives false positives at pointy
>    angles.  Those can be reduced with a --min_area parameter.
>     - shring the routing layer by half the trace width
>     - rebloat the layer
>     - subtract the rebloatd layer from the routing layer
>     - discard violations smaller that min_area
>    When a trace is to thin it will be lost while shrinking, and the
>    subtraction leaves the original trace in place.
>    The bloating uses circle segments at the corners.  So there will be
>    a small remaining area in all corners.  The check has a min_area
>    parameter, all residue smaller than this area will be discarded.
> 
>  * minimun clearance.
>    This test is slow, because it works on each
>    individual outer shape of the routing layer.
>    - bloat the shape
>    - compute the intersection of the bloated shape with the rest of the
>      layer
>    Anything left is a clearance violation.
> 
> 
> Next steps: write a script that extracts center coordinates of pins and
> pads, netnames and layer names from a pcb file, and find a way to import
> that for net-specific rules.
> 
> Stephan
> 
> 
> geda AT psjt DOT org (Stephan Böttcher) writes:
> 
> >>> 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
>