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=mime-version:in-reply-to:references:from:date:message-id:subject:to;
	bh=ViF0Gsqk8/MpvdlN2cqFQdifqFtrtQNhorwf/qkqDKQ=;
	b=0tp5utZIX2f6hfKkimVInUm8LF/DmMfzFFiagJs45RIw9LvmODbc7SqS3D70WSL+6d
	XANKGzSeJC62/JNTeiCICP1C7If/2YXB8nedgslyJiot5BiGS5t5cvtn5hlvc6ZfV83p
	5kuJs/yC+GM3T9gAMONiG8631qS3G7LZgc9bxN3c4bQ2Psn8g7xoGTiU63M3n9dWNOir
	LEGGvbTvRzDZj+B4FEcmcrWIraRDkbIhSt/V3W92ClLuwRYgpdF5QysyOnwkW40qxthU
	g8Q9VrdSY9H1hXh//tMHG/VF0Ik0MqG9Pqz+Lx/exlFc6Ib3nHrpEL/v2fUUWdXLlz9R
	Nx5A==
X-Google-DKIM-Signature:	v=1; a=rsa-sha256; c=relaxed/relaxed;
	d=1e100.net; s=20130820;
	h=x-gm-message-state:mime-version:in-reply-to:references:from:date
	:message-id:subject:to;
	bh=ViF0Gsqk8/MpvdlN2cqFQdifqFtrtQNhorwf/qkqDKQ=;
	b=iI4i/1HBVlBmxnVPO1n7ejWHKziVOHrcOeQquZFIuYaIv6GwMc7Su7sFzDpXdSCAFA
	7/r4iyhLTVwuXWDD+L1bEwQahoxWJqlAZGBzPpLdJWXPIW8iq6S6uKYAIqZhxAO77zJQ
	ZmeAlqkyHxgZHCM9lnm71KeP5pRc46uqTajC2/zzER585AWgonKHX4hC5UTpW0lxiuwz
	p8QtRY6QEO/f98MZZYT3O76qgmGPJD+ueLqlp8eGs6fjWKMcml7TCE5bPv0isz76hP/H
	S0jRCLVJNBU7ou/1tbJIz5wC06+Tqps8rMf43q70lzC9TJTBTIXOJCS1ZlmIMNT7xKYS
	iFJw==
X-Gm-Message-State:	AA6/9RkzcMB8+Ev8wGhOmhFqyci/SbkImF42jcZ9rsMA256CP4FIsjVAVbKighZOK52BgILTbdGEs+TdZv53GA==
X-Received:	by 10.157.58.35 with SMTP id j32mr11443195otc.166.1476709903564;
	Mon, 17 Oct 2016 06:11:43 -0700 (PDT)
MIME-Version:	1.0
In-Reply-To:	<20161017115637.0f1566f6@jive>
References:	<CAHUm0tMw2Zzvq-X=xjhugpkmR5F9gEYRRuzqcSQ=0mxC=9Dthw AT mail DOT gmail DOT com>
	<20161017115637 DOT 0f1566f6 AT jive>
From:	"Erich Heinzle (a1039181 AT gmail DOT com) [via geda-user AT delorie DOT com]" <geda-user AT delorie DOT com>
Date:	Mon, 17 Oct 2016 23:41:43 +1030
Message-ID:	<CAHUm0tPR-K8KkTtMda9eTnBCUqfEYy_FFhfQE6RTP1zmbdY5iw@mail.gmail.com>
Subject:	Re: [geda-user] [pcb-rnd] Layout and footprint export to Kicad now working
To:	geda-user <geda-user AT delorie 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

I usually turn kicad libraries into pcb footprints with
https://github.com/erichVK5/KicadModuleToGEDA ...

but if you want to go in the other direction, there are three simple
ways that now come to mind

1) export an existing PCB layout to a kicad .brd file in pcb-rnd, by
using the File->Save Layout As dialog, selecting the appropriate file
format in the pull down menu, which will produce a kicad .brd layout
containing the footprints as embedded elements. Upon loading the .brd
file in kicad's pcbnew, you can use the File->Archive Footprints
command to create a new kicad footprint library (.mod) which can then
be added to your default kicad libraries. This method at present will
export in decimils, and theoretically has the potential to lose a
little accuracy with rounding.

If batch conversion is desired, you could do a shell script to get
pcb-rnd to convert multiple existing layouts in headless CLI mode to
kicad .brd layouts, which can then have footprint archives created
from them within kicad. You will get a lot of archives this way, which
may be annoying to manage or require combination and elimination of
duplicates.

2) Place all of your desired footprints in a new PCB layout in
pcb-rnd, select all, copy to buffer, then save elements to file, and
in the save dialog, save it as something like exportedLibrary.mod, and
select "kicad legacy format" in the pulldown file format menu, and
then press save. This will save the selected elements as distinct
kicad modules in a .mod library. The advantage of this method is it
will export dimensions in millimetre format to three decimal places,
essentially eliminating the potential for loss of accuracy due to
rounding. In kicad's pcbnew, you can add this library to your default
kicad libraries with the Preferences->Library menu item.

3) hybrid approach. Make an enormous layout, paste copies of all of
your existing designs into it, and either export it as a single kicad
layout as in 1) above, or select all the footprints, and proceed as in
2) above.

As mentioned before, once s-expression export is implemented, exported
layouts will also be exported in millimetre units. Kicad legacy format
will remain for backwards compatibility for those running older
versions of kicad.

Cheers,

Erich

On Mon, Oct 17, 2016 at 8:26 PM, Lev (leventelist AT gmail DOT com) [via
geda-user AT delorie DOT com] <geda-user AT delorie DOT com> wrote:
> On Mon, 17 Oct 2016 00:56:46 +1030
> "Erich Heinzle (a1039181 AT gmail DOT com) [via geda-user AT delorie DOT com]"
> <geda-user AT delorie DOT com> wrote:
>
>> - PCB footprint(s) as a "kicad pcbnew" legacy format module library
>> (.mod)
>
> Could you suggest how to create a KiCad footprint from a gEDA footprint? I'd
> like to make it scriptable.
>
> Thanks,
> Lev
>
> --
> 73 de HA5OGL
> Op.: Levente
>

- Raw text -