X-Authentication-Warning:	delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient:	geda-user AT delorie DOT com
X-Virus-Scanned:	amavisd-new at neurotica.com
X-Original-DKIM-Signature:	v=1; a=rsa-sha256; c=relaxed/simple; d=neurotica.com;
	s=default; t=1539233735;
	bh=6ejhsugxlCccW6TMKLxay7YIzyJ+YFKKLj+FKHcNFKc=;
	h=Subject:To:References:From:Date:In-Reply-To;
	b=QhjGoBrGnVwWOwt5+Dg09J5tm70fJt24TheBtc+t8v0msd94xuNjfIEx92T7/ztVq
	s+frJ0wJvztjer2AO0haLZRbYzi1vaTwoeNAFFerWbLrtVkcqnNM5wfF90INPKdZ6J
	qrSXkJs4W0g50gBNHqDsfuG4RRErQL7+DWRBpLBQ=
Subject:	Re: [geda-user] PCB footprint for APA102-2020?
To:	geda-user AT delorie DOT com
References:	<e5759ba1-9de0-4e54-e499-5283eb79a7a4 AT neurotica DOT com>
	<CAHUm0tMEUJBbkHCNJUGzn8fhc4PXZi15Ce1SEnkk0xfkqVT--A AT mail DOT gmail DOT com>
From:	"Dave McGuire (mcguire AT neurotica DOT com) [via geda-user AT delorie DOT com]" <geda-user AT delorie DOT com>
Openpgp:	preference=signencrypt
Autocrypt:	addr=mcguire AT neurotica DOT com; prefer-encrypt=mutual; keydata=
	xsBNBE90TjYBCACrtN5OyxdOGHWrUcxe4e6fFLaXpA7GIjN9pkTmbb2ozKNxgDKl6Gfk7ywx
	19E+jUbO4KQ4/nhDvXXtWIH2J1a0eiRiDdaENzBtGxoiDIf6vJshMY0vKUn2OQfVn6kaQ5PY
	so5oPrNaJCphJDT/G8S6UzpvjB5UXrUb8625cD08H2Sx1Id79p8JYxs8tFZ1b9qViq8HisDB
	nmziw6oQoqpdMt3D1TX6XdeybfVCigyR26pQ60C/kzOVqT6BzR5ZxP3eTQQQnXc/MQxF3gkP
	49g0/HdLjtDd9HyoDGydK83oDVgECxSXaAy/IO4rWgYJlQCaTScZLyJSn7uXPbSCHXTfABEB
	AAHNJERhdmUgTWNHdWlyZSA8bWNndWlyZUBuZXVyb3RpY2EuY29tPsLAfgQTAQIAKAIbIwYL
	CQgHAwIGFQgCCQoLBBYCAwECHgECF4AFAlr2Br0FCQ9EH10ACgkQTm0vsniSDMRRlQgAjNlC
	jNJpfcMz8YIELVzpTkPyKHAjHAsuuWzORCRpCP5i67FaOnP2jpdTEP50gxHiB4SqfVPshN4+
	DEjsXiCLjqMIrR/5vgXRGa/F0Q4x5TbylzECmikv2zkRUnTnjt3g3o0ByCRSmGvZtIOaNTX5
	Zc/EKrDPlRLKNYNHxmRWH54nrflDBvpxHMx38ZH5wXIL34RFozdafqb+C1uJkxx0/X1DS/Ct
	iIfsOX+FgqMRrS4855p1rYyWnxrsyPU09TNx1cYbL4lIQtlDJpibLnbCo/y0u6IcfrEA8t4p
	nj7QD3TLI01+FrK5Q9vkZ4vyM+XXs6ANoe/p47z+3l9AxtOj8c7ATQRPdE42AQgAuBxBsLxu
	AyyexLICB3NJ4Fu85/Wx0bESlBDPia3+jCfR8sjZ5PWlklJUlpBOc3CXmxwk4QPVTKDHM6kB
	GBq2etfMq9tGMrIhG68kY4KxcRw8mMTVMNeZaJQTa0+6X2MTNvesnutmYqiTEtnsv2R7WfU+
	VAV5Fp9Opmb7bkkQ0uEKazDsLzYnaeg54hALx286inLN/T26eF6UwfrIRQpnYyEE3ip7BNlV
	YvrypzAFu+xlt+4o+yue67YZDrDX8qx/TQeSuGYUAfpdLro2t3w9Bg5qjMdwi4kA20BUgCiZ
	2dS0ApgJwuKnY79YgKq92tD557Ky8m1MM84UNNfnO2ln+QARAQABwsBlBBgBAgAPAhsMBQJa
	9gbYBQkPRB+fAAoJEE5tL7J4kgzEFToH/A5iL95Lou/0eDN1fBNUYj+00PlT5K+3h4QobhOx
	UWUPwJck2/SoIJPOkjk25FnMEsFvPBlkENdf6LmENWskOv5pvZqnc8IKLr5U3RIdkzw/OwGZ
	/imF+XdYhtGSlhAoxbJ8aTSJ2rkviBVLXH8m1zdKZveEnTJg620LBMbfKuZLwcTJ37oUdOYn
	eEbH5tb/eOKxGLId3Z59CGfsDXzwkk8PZn2U+vU0W5NPpOmg20q3iX0STsaFTIlCrOgTmFmh
	woJYFp7FNsv1Qmxbbvk8kvUe+VCsHiZa+UeYlk1GlJwKmLqJyM4IHi3e+TfsIYLjxsacu4eu
	M9oEb/I2cu6GcfA=
Message-ID:	<cc3e1bbb-142e-b54a-7b4b-a68d832c412d@neurotica.com>
Date:	Thu, 11 Oct 2018 00:55:34 -0400
User-Agent:	Mozilla/5.0 (X11; Linux x86_64; rv:52.0) Gecko/20100101
	Thunderbird/52.9.1
MIME-Version:	1.0
In-Reply-To:	<CAHUm0tMEUJBbkHCNJUGzn8fhc4PXZi15Ce1SEnkk0xfkqVT--A@mail.gmail.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

  Got it.  Thank you Erich!

           -Dave

On 10/07/2018 12:57 AM, Erich Heinzle (a1039181 AT gmail DOT com) [via
geda-user AT delorie DOT com] wrote:
> 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]
> 
> )
> 


-- 
Dave McGuire, AK4HZ
New Kensington, PA

- Raw text -