X-Authentication-Warning: delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient: geda-user AT delorie DOT com
X-Injected-Via-Gmane: http://gmane.org/
To: geda-user AT delorie DOT com
From: Kai-Martin Knaak <kmk AT familieknaak DOT de>
Subject: Re: [geda-user] pcb layers & shortcuts
Date: Wed, 03 Apr 2013 02:56:27 +0200
Lines: 129
Message-ID: <kjfunn$42o$1@ger.gmane.org>
References: <5150341D DOT 2050406 AT gmail DOT com> <201303251608 DOT r2PG8AfW026082 AT envy DOT delorie DOT com> <5153FEA0 DOT 1040801 AT gmail DOT com>
Mime-Version: 1.0
Content-Type: text/plain; charset="ISO-8859-1"
Content-Transfer-Encoding: 7Bit
X-Complaints-To: usenet AT ger DOT gmane DOT org
X-Gmane-NNTP-Posting-Host: a89-182-138-143.net-htp.de
User-Agent: KNode/4.4.11
Reply-To: geda-user AT delorie DOT com

Iain Paton wrote:

> On 25/03/13 16:08, DJ Delorie wrote:

>> The default is a 6-layer board (plus outline and "spare" layers),
>> with the layers set up so that you can simply ignore the inner
>> layers. There may be a way to change all that, but you shouldn't
>> need to change it to make a 2 or 4 layer board.
> 
> Ok, then I'm doing something wrong somewhere..
> 
> If I simply run 'pcb' at the command line I'm getting:
> 1. component
> 2. solder
> 3. gnd
> 4. power
> 5. signal1
> 6. signal2
> 7. signal3
> 8. signal4
> silk
> rat lines

This looks a bit dated. More recent versions of pcb use "top/bottom" 
rather than "component/solder". It does not necessarily mean that your 
pcb version is that dated. An update does not affect your default 
start-up layer stack as saved in $HOME/.pcb/preferences.


> some of my recent layouts have the outline,

Did you start these with gsch2pcb rather than by running pcb with no 
argument? gsch2pcb uses its own independent set of default layers. If 
I remember correctly, this gsch2pcb layer stack contained the outline 
layer for some years while the default of pcb did not. However, this 
gsch2pcb layer stack is hard coded in source. Customization would 
require a recompile. By contrast, pcb reads $HOME/.pcb/settings and  
$HOME/.pcb/preferences on start-up. 


> none have 'spare'.

The "spare" was introduced about the same time as the switch from 
"component/solder" to "top/bottom"


PCB likes to mess with .pcb/preferences. If you open and close a 
layout with some silly layer stack, this layyer stack will be written 
to preferences. The next time you start a fresh layout, you will get 
this silly layer stack. 

If you want to gain more control over initial layers you might:

1) remove $HOME/.pcb/preferences 

2) remove $HOME/.pcb/settings if it exists.

3) start pcb  
(This will give you the system default of pcb.)

4)  tweak layer names in Preferences -> Layers 
4a) tweak layer groups in Preferences -> Layers -> Groups

5) exit pcb 
  (This will save the current values in $HOME/.pcb/preferences

6)  copy the lines that start with "layer-name" to .pcb/settings. 
6a) also copy the groups line to the settings file. 

If you get weird initial layers, you can remove .pcb/preferences and 
make pcb fall back to .pcb/settings.

The same technique works with a number of options. Unfortunately, not 
all options of pcb behave like this. Some get read from settings, some 
not. I have yet to find a general rule.

An alternative is to explicitely give layers and layer stack as 
parameters on the command line. Here is the initialize layout section 
of my new_geda_project.sh shell script:


##########Create an empty layout###################################
# This starts pcb and executes a couple of actions through a pipe.#
echo "Create an empty layout"
echo \
"ChangeName(Layout) "\
"SaveTo(LayoutAs,"$name".pcb) "\
"Quit() "\
| pcb --listen \
 --fab-author \"$AUTHOR\" \
 --groups "1,2,3,c:4,5,5,s:7:8" \
 --layer-name-1 "top" \
 --layer-name-2 "top-polyg." \
 --layer-name-3 "top-GND" \
 --layer-name-4 "bottom" \
 --layer-name-5 "bott.-poly." \
 --layer-name-6 "bott.-GND" \
 --layer-name-7 "comment" \
 --layer-name-8 "outline" \
 --bloat 600 \
 --shrink 1000 \
 --min-width 600 \
 --min-silk 600 \
 --min-drill 1500 \
 --min-ring 1000 \
 --route-styles \
"Signal,1000,3600,2000,1000\
:Power,2500,6000,3500,1000\
:Fat,4000,6000,3500,1000\
:Skinny,600,2402,1181,600" \
 --default-PCB-width 600000 \
 --default-PCB-height 600000 \
 --grid-increment-mm 1.000000 \
 --grid-increment-mil 20.000000 \
 --size-increment-mm 0.200000 \
 --size-increment-mil 10.000000 \
 --line-increment-mm 0.100000 \
 --line-increment-mil 8.000000 \
 --clear-increment-mm 0.500000 \
 --clear-increment-mil 2.000000
##################################################


Hopethishelps,

---<)kaimartin(>---

-- 
Kai-Martin Knaak