X-Authentication-Warning: delorie.com: mail set sender to geda-user-bounces using -f X-Recipient: geda-user AT delorie DOT com X-Authority-Analysis: v=2.0 cv=AtpsLZBP c=1 sm=0 a=6jktZp3dcHAl1vye2O6wCg==:17 a=jl9P3j1e7_0A:10 a=2xJ3G-9csIsA:10 a=4VVfh522gFYA:10 a=6WB07kdHjWAA:10 a=8nJEP1OIZ-IA:10 a=wR-FlJDvAAAA:8 a=ibD6AiJIMGf-LqXMDbkA:9 a=wPNLvfGTeEIA:10 a=6jktZp3dcHAl1vye2O6wCg==:117 X-Cloudmark-Score: 0 X-Originating-IP: 70.113.67.117 Message-ID: <4FF4E840.8070401@ecosensory.com> Date: Wed, 04 Jul 2012 20:05:04 -0500 From: John Griessen User-Agent: Mozilla/5.0 (X11; Linux i686; rv:10.0.4) Gecko/20120510 Icedove/10.0.4 MIME-Version: 1.0 To: geda-user AT delorie DOT com Subject: Re: [geda-user] pcb work flow question References: <20120704234442 DOT GA17749 AT nome02 DOT eecs DOT oregonstate DOT edu> In-Reply-To: <20120704234442.GA17749@nome02.eecs.oregonstate.edu> Content-Type: text/plain; charset=ISO-8859-1; format=flowed Content-Transfer-Encoding: 7bit Reply-To: geda-user AT delorie DOT com On 07/04/2012 06:44 PM, Traylor Roger wrote: > Gang, > I have a quick question about pcb work flow. I see that through the menus > I can set up the layers, drc clearances, etc. Is that how most folks setup > pcb for each new project? You can set defaults that are there at turn on in a couple of places. One global place is a file ~/.pcb/settings See mine below. Another is in a project dir and it overrides the global one, it is named/located like: ~/boards/project-dir1/pcb.settings and can have the same contents as the global file or what have you... My local footprint library is added on in addition to a repoitory by changing oneline: lib-newlib = /home/john/EEProjects/now-svn-ecosensory/circuitboards/footprints_pcb:./footprints Now, ./footprints can contain new footprints as I make them and access them per project, so they can be different from same named ones in the repository. I'm not recommending to do that, it just happens sometimes... > > I would rather have a separate script that could be edited and executed once > to set the tool up. Is that possible or even a good idea? Not sure it's easily possible, yes it's a good idea and has been discussed, but it's waiting for more general improvements before it is easily possible. > > How do other folks set up pcb for a new project? I drive layout from the schematic in project dirs. A local file called gafrc will be read by gschem and mine is below. John =======================~/boards/project-dir1/gafrc======================= cat gafrc (source-library ".") (component-library "${HOME}/EEProjects/ecosensors-pub.git/gschem-cibolo") (component-library "${HOME}/EEProjects/ecosensors-pub.git/gschem-cibolo/two-terminal") (component-library "${HOME}/EEProjects/ecosensors-pub.git/gschem-cibolo/thru-hole") (component-library "${HOME}/EEProjects/ecosensors-pub.git/gschem-cibolo/transistors") (component-library "${HOME}/EEProjects/ecosensors-pub.git/gschem-cibolo/pwrgnd") (component-library "${HOME}/EEProjects/ecosensors-pub.git/gschem-cibolo/boards") (component-library "${HOME}/EEProjects/ecosensors-pub.git/gschem-cibolo/probes") (component-library "${HOME}/EEProjects/ecosensors-pub.git/gschem-cibolo/borders") (component-library "${HOME}/EEProjects/ecosensors-pub.git/gschem-cibolo/conn-smt") (component-library "${HOME}/EEProjects/ecosensors-pub.git/gschem-cibolo/ic-gull-wing") (component-library "./symbols") ========================~/boards/project-dir1/gafrc======================= ==============================~/.pcb/settings============================== lib-newlib = /home/john/EEProjects/now-svn-ecosensory/circuitboards/footprints_pcb groups = 1,2,3:4:5,6:7:8,9,10 route-styles = Signal,1000,3600,2000,1000:Power,2500,6000,3500,1000:Fat,4000,6000,3500,1000:Skinny,600,2402,1181,600 color-file = /home/john/.pcb/colors/Default layer-name-1 = top-carbon-print layer-name-2 = top-insulator layer-name-3 = top-sig1 layer-name-4 = top-sig2 layer-name-5 = top-PWR-GND layer-name-6 = bot-sig1 layer-name-7 = bot-sig2 layer-name-8 = bot-PWR-GND top-window-width = 1145 top-window-height = 799 log-window-width = 548 log-window-height = 270 library-window-width = 888 library-window-height = 537 grid-increment-mil = 1.000000 grid-increment-mm = 0.200000 size-increment-mil = 5.000000 size-increment-mm = 0.200000 line-increment-mil = 5.000000 line-increment-mm = 0.100000 clear-increment-mil = 2.500000 clear-increment-mm = 0.050000 min-width = 1000 min-silk = 1000 min-drill = 1500 min-ring = 1000 via-thickness = 3600 bloat = 699 shrink = 400 via-drilling-hole = 2000 line-thickness = 1000 rat-thickness = 1000 backup-interval = 60 text-scale = 113 default-PCB-width = 300000 default-PCB-height = 200000 background-color = #fffada element-color = #000000 via-color = #7f7f7f pin-color = #4d4d4d rat-color = #ddc317 rat-selected-color = #f5e707 rat-thickness = 3 warn-color = #ff69b4 off-limit-color = #ffffff invisible-objects-color = #cccccc invisible-mark-color = #b3b3b3 connected-color = #00ff00 crosshair-color = #ff0000 cross-color = #ffff00 grid-color = #ffffff mask-color = #ff0000 element-selected-color = #00ffff via-selected-color = #00ffff pin-selected-color = #00ffff layer-color-1 = #dea620 layer-color-2 = #c5ef50 layer-color-3 = #0c649b layer-color-4 = #076677 layer-color-5 = #0b3f88 layer-color-6 = #d54006 layer-color-7 = #b13606 layer-color-8 = #982407 layer-color-9 = #8bb63f layer-color-10 = #c8933f layer-color-11 = #6060c0 layer-color-12 = #fffada layer-color-13 = #e1d1e5 layer-color-14 = #000000 layer-color-15 = #b8860b layer-color-16 = #8f7fd0 layer-selected-color-1 = #00ffff layer-selected-color-2 = #00ffff layer-selected-color-3 = #00ffff layer-selected-color-4 = #00ffff layer-selected-color-5 = #00ffff layer-selected-color-6 = #00ffff layer-selected-color-7 = #00ffff layer-selected-color-8 = #00ffff ===========================~/.pcb/settings==============================