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 <john AT ecosensory DOT com>
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>
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==============================

- Raw text -