X-Authentication-Warning: delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient: geda-user AT delorie DOT com
X-Envelope-From: paubert AT iram DOT es
Date: Thu, 12 Jun 2014 03:35:54 +0200
From: Gabriel Paubert <paubert AT iram DOT es>
To: geda-user AT delorie DOT com
Subject: Re: [geda-user] another (hopefully) quick question
Message-ID: <20140612013554.GA14352@visitor2.iram.es>
References: <5397A1B7 DOT 1000600 AT neurotica DOT com>
 <201406110026 DOT s5B0Qb8x009612 AT envy DOT delorie DOT com>
 <20140611070346 DOT GA10408 AT visitor2 DOT iram DOT es>
 <5398ECA0 DOT 2090908 AT neurotica DOT com>
MIME-Version: 1.0
Content-Type: text/plain; charset=us-ascii
Content-Disposition: inline
In-Reply-To: <5398ECA0.2090908@neurotica.com>
User-Agent: Mutt/1.5.21 (2010-09-15)
X-Spamina-Bogosity: Unsure
X-Spamina-Spam-Score: -0.2 (/)
X-Spamina-Spam-Report: Content analysis details:   (-0.2 points)
  pts rule name              description
 ---- ---------------------- --------------------------------------------------
 -1.0 ALL_TRUSTED            Passed through trusted hosts only via SMTP
  0.8 BAYES_50               BODY: Bayes spam probability is 40 to 60%
                             [score: 0.4962]
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

On Wed, Jun 11, 2014 at 07:56:16PM -0400, Dave McGuire wrote:
> On 06/11/2014 03:03 AM, Gabriel Paubert wrote:
> > On Tue, Jun 10, 2014 at 08:26:37PM -0400, DJ Delorie wrote:
> >>
> >> two options:
> >>
> >> 1. Turn the waveguide into an element, so you can edit the soldermask
> >>    big enough.
> >>
> >> 2. Create a new layer called "extra top soldermask" that has the edits
> >>    you want, and merge the gerbers in post-processing.
> > 
> > Solution 2 is what I've been doing for years. Merging the photoplotter
> > files manually is relatively easy (even if having tools for this would 
> > be nice).
> 
>   Got it...Thanks for the suggestions, guys.
> 
>   Gabriel, can you tell me how you do the gerber merge, and what tool(s)
> you use?  

cat and emacs :-)

cat to concatenate the two files to a new one (always keep the originals!).

Then under a text editor (I use emacs since it keeps the DOS line breaks)):
- eliminate the M02 at the end of the first file,
- move the header which is just after this removed item to after
  the header of the first file
- merge the headers by hand, this is easy since right now pcb allocates
  non overlapping aperture ranges for each file. You must remove the 
  duplicate %MO and %FS parameter lines, which must be identical,
  (same for %IP if it were present). The other parameters are less critical
  but I prefer to keep the %LN from the first file.
- for the comment (G04) lines, do what you want, keeping in mind that
  only printable ASCII characters are allowed with the exception of % and *.

That's about all, but I may have forgotten something.
Then I always check the results under gerbv.

> Can gerbv do this?

Not as far as I know, and last time I tried, saving under gerbv used
imperial units (even if you feed it exclusively metric files) and
lost precision in the process. With these caveats, I believe that the 
only thing that gerbv allows is to delete items.

	Gabriel