X-Authentication-Warning:	delorie.com: mail set sender to geda-user-bounces using -f
Date:	Mon, 21 May 2012 00:49:12 -0400
Message-Id:	<201205210449.q4L4nCkQ029344@envy.delorie.com>
From:	DJ Delorie <dj AT delorie DOT com>
To:	geda-user AT delorie DOT com
In-reply-to:	<4FB9C7CB.8040700@innocent.com> (message from Gus Fantanas on
	Mon, 21 May 2012 00:42:51 -0400)
Subject:	Re: [geda-user] Rat Thickness and Trace Transparency in Updated PCB; Other Questions
References:	<4FB9B947 DOT 90404 AT comcast DOT net> <201205210344 DOT q4L3iNfC027519 AT envy DOT delorie DOT com> <4FB9C7CB DOT 8040700 AT innocent DOT com>
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

> 1.  I tried to change the default rat thickness in PCB by including
> the line 'rat-thickness = 2' in the file '~/.pcb/preferences',
> according to the online documentation (which may be out of date?).
> This works as expected the first time I start PCB after that file
> edit, but when I quit PCB, that line seems to disappear!  If I don't
> re-edit '~/.pcb/prefernces', next time I start PCB the rats have
> their default thickness.

Use ~/.pcb/settings instead

"preferences" is for the GTK preferences only, "settings" is for
global settings (entries match command line options) for all GUIs and
exporters.

You might need to use "2nm" instead of just "2" though, as I don't
know if your version has the "px" suffix for pixels.

> 2.  In the version of PCB that came with Ubuntu 11.11, traces were not 
> transparent if I remember correctly, so the trace of the active layer 
> was in the foreground.  Is there any way to revert to that behavior in 
> the PCB version which came with the upgrade to  Ubuntu 12.04 LTS?

You'll have to rebuild without the GL renderer.

> 3. Is there any documentation on how the 'Import Schematics' option
> works?

Yes, in the pcb documentation under "Action Reference" for Import()

Basically, if your "foo.sch" and "foo.pcb" have the same base name
("foo" in this example) File->Import is a one-step schematics to
layout tool.  The documentation tells you how to do more complex
imports with it.

> 4. If the new PCB has 1nm resolution, as has been discussed on this
> board, I don't see it.  The finest grid available as an option is
> only 0.01mm, just like before the upgrade to Ubuntu 12.04 LTS.  Am I
> missing something?

The nanometer resolution is *internal*.  The net result is that metric
grids are "perfectly accurate" so you don't have tiny jogs in lines
connecting things on metric grids.  You can manually set the grid
lower than 0.01mm if you like using the SetValue() action.

Previously, we used an inch-based grid, so metric dimensions could not
be stored "exactly" internally.

- Raw text -