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=20161025;
	h=mime-version:references:in-reply-to:from:date:message-id:subject:to;
	bh=sP8Jxn6QpKELH+pEjj6m5uGgsUQGooWewnk2CUC/ChI=;
	b=Duv6ghy5wIPulEjIhkYpNzhnxJnEEmVw2Tjp2VqmrlZ+azC5r36Tz+vC31zi9PiJBp
	PvsC/rpG9hCEVYNUCPXA5TRec48ldbsGlcTt7thw9vJ+7T9u/8KfWuyZLYm0W/recJLV
	QtBcPYgSoR2wUnSaYYCMK4HwwUIdJLQBUfp4HoSJcE2551SKbOLtUizW3D2zGqrNWljg
	fzXyUEcPRu1Kc3r+dvtPm2j69vs/18hROVl+G0aTWteztIUrcc88snlhREBdBIiKcwZh
	HPmhtc4y1donkruW4gsJdEWdUx5fh3KaX1esDr6FNCOPVtU4JG5MECkglBrAVitkxgrv
	ODMQ==
X-Google-DKIM-Signature:	v=1; a=rsa-sha256; c=relaxed/relaxed;
	d=1e100.net; s=20161025;
	h=x-gm-message-state:mime-version:references:in-reply-to:from:date
	:message-id:subject:to;
	bh=sP8Jxn6QpKELH+pEjj6m5uGgsUQGooWewnk2CUC/ChI=;
	b=gIvMZIDW9MmopQWmnwh++hikF49ri9CkI7x9t1wlmaGET3gZoMzFH9/5mJBq8Fm8bU
	Zu3NftaXtVSanDEk8eznB9VwAT0ey7RAugMNgYuwhdIJn1C5Q6BC4KossApMZrVjqIlP
	S+CJd782ObUouDJnpCJiGQ9eB2SGpB4QPah1hLG4+UQulvrBasCUbPTBpk7opxixetJM
	XEEOwoHpX4HYDn/wXOh2IULAhP9rQFUuqcXpen7lc2QvFFOU14K0+DpL7TG1+u51BakH
	sPWb9cTMBGCZ6lD8CRNpLvWVzqID8PYs1yDYs/8fE7g2K+GKEjzwiVV7WjafFGp3FFWe
	PSrw==
X-Gm-Message-State:	ABuFfoghtytNmtAMv7DZn5HiODHUNhbU8w0QNajCCg+A2iX818ewuX51
	SDRCfGXApO+EHj8MleOiQeogXJHHGSKlNDS157mMszgF
X-Google-Smtp-Source:	ACcGV61RSerQDEKoMgMoXVR4QiCACKZoHETmx2bnWSi2pE1bTYMx74+3j4OGWRrvMPp0R/6n64rsBh5StUjCQMDs44c=
X-Received:	by 2002:a25:2a02:: with SMTP id q2-v6mr10469455ybq.323.1538888279231;
	Sat, 06 Oct 2018 21:57:59 -0700 (PDT)
MIME-Version:	1.0
References:	<e5759ba1-9de0-4e54-e499-5283eb79a7a4 AT neurotica DOT com>
In-Reply-To:	<e5759ba1-9de0-4e54-e499-5283eb79a7a4@neurotica.com>
From:	"Erich Heinzle (a1039181 AT gmail DOT com) [via geda-user AT delorie DOT com]" <geda-user AT delorie DOT com>
Date:	Sun, 7 Oct 2018 15:27:46 +1030
Message-ID:	<CAHUm0tMEUJBbkHCNJUGzn8fhc4PXZi15Ce1SEnkk0xfkqVT--A@mail.gmail.com>
Subject:	Re: [geda-user] PCB footprint for APA102-2020?
To:	geda-user <geda-user AT delorie DOT com>
Reply-To:	geda-user AT delorie DOT com

The footprint is attached below, plus here's a quick howto for importing.....

A quick google search for

APA102-2020 kicad_mod

or

APA102-2020 eagle

gets us pretty quickly to

a) an Eagle layout (.brd) with the component in it

https://raw.githubusercontent.com/urish/utility-pcbs/master/apa102-2020-stick.brd

and

b) a Kicad footprint (.kicad_mod in this case, older formats are just .mod)

https://raw.githubusercontent.com/greatscottgadgets/gsg-kicad-lib/master/gsg-modules.pretty/APA102-2020.kicad_mod

either of the above can be imported pretty easily in a number of ways:

1) using the translate2geda utility available at
https://github.com/erichVK5/translate2geda

we trick translate2geda into thinking the board is a library, by
renaming it (.lbr), then convert:

user AT box:~/Source/translate2geda$ cp apa102-202-stick.lib apa102-202-stick.lbr
user AT box:~/Source/translate2geda$ java translate2geda apa102-202-stick.lbr
Using filename: apa102-202-stick.lbr
Polygon omitted in: APA102_2020
<polygon width="0.05" layer="21" spacing="0.01" pour="hatch">
APA102_2020.fp
1X04_LOCK.fp

and we get the desired footprint
translate2geda will flag failure to convert polygons in elements, as
it is constrained by gEDA PCBs footprint format, which lacks polygons,
but in this case, it does not affect the pad layer.

2) using the KicadModuleToGEDA utility available at
https://github.com/erichVK5/KicadModuleToGEDA

user AT box:~/Source/KicadModuleToGEDA$ java KicadModuleToGEDA -k
APA102-2020.kicad_mod
Using APA102-2020.kicad_mod as input file
APA102-2020.fp

3) the simplest option, if you are running pcb-rnd, involves going go
to the menu

"File->Import->Load subcircuit data to paste buffer"

and select the kicad footprint, and it will appear in your paste
buffer, ready to place on the layout. It can also be exported from
pcb-rnd with the menu option

"Buffer:Save buffer subcircuits to file"

at which point it can be saved in gEDA PCB mainline (.fp) format.

4) a more obscure option is to use the "layout as library" option in
pcb-rnd, where you tell pcb-rnd to treat a board as a footprint
library, and the footprint will then become available in the library
window

Regards,

Erich..



>   Hey folks.  Has anyone here done up a PCB footprint for the
> APA102-2020 RGB LED?
>


Element["hidename" "" "APA102-2020" "VAL**" 132500 110000 0 0 0 100 ""]
(
Attribute("refdes" "APA102-2020")
Attribute("value" "VAL**")
Pad[-3937 -3543 -2756 -3543 1969 1969 2953 "" "2" "square"]
Pad[-4331 0 -2362 0 1181 1969 2165 "" "3" "square"]
Pad[-3937 3543 -2756 3543 1969 1969 2953 "" "4" "square"]
Pad[2756 3543 3937 3543 1969 1969 2953 "" "5" "square"]
Pad[2362 0 4331 0 1181 1969 2165 "" "6" "square"]
Pad[2756 -3543 3937 -3543 1969 1969 2953 "" "1" "square"]
ElementLine [3543 -1575 787 -1575 1378]
ElementLine [787 -1575 787 -3543 1378]
ElementLine [-3937 -3937 3937 -3937 591]
ElementLine [3937 -3937 3937 3937 591]
ElementLine [3937 3937 -3937 3937 591]
ElementLine [-3937 3937 -3937 -3937 591]

)

- Raw text -