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: In-Reply-To: From: "Erich Heinzle (a1039181 AT gmail DOT com) [via geda-user AT delorie DOT com]" Date: Sun, 7 Oct 2018 15:27:46 +1030 Message-ID: Subject: Re: [geda-user] PCB footprint for APA102-2020? To: geda-user Content-Type: text/plain; charset="UTF-8" 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 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] )