X-Authentication-Warning:	delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient:	geda-user AT delorie DOT com
DKIM-Signature:	v=1; a=rsa-sha256; c=relaxed/relaxed;
	d=gmail.com; s=20120113;
	h=mime-version:in-reply-to:references:date:message-id:subject:from:to
	:content-type;
	bh=YtaRdFc9l40rggvJ42+MILPc1ztVHBFGizfo1P/9Y3E=;
	b=vmhIFB/7OAjId6xX6CnHqeFgb/iFUsMqDjQjMxUFADdu0I8/utE2ZJFFkcsJlnCKF1
	vuBWjVjHBzr8PhJQ/JdVc+4njM56y0ecgE9EdXSqOzixt4XlvUFajd9jcMfRUxaq41UY
	BQp9opt48t2eB6gNCLHbzhGf9sUFXPirO55N5qrrmsSA90OfuwBmXms35D1ybzDv3K3Q
	xIbyHhYw1IZrrm7tmqx+sGSl6OE9GGc5PHIbP2gRXz1S+71Xi4BEhMymH9f6z85rAnJW
	XRJk3W6KmnbhGuEK3wF1gZ+Mgh+KBJnxe6vc77hKtDj3PEB/LZ96wO+otQl2HhHTYmA+
	yVQA==
MIME-Version:	1.0
X-Received:	by 10.220.144.13 with SMTP id x13mr2359362vcu.21.1374812381411;
	Thu, 25 Jul 2013 21:19:41 -0700 (PDT)
In-Reply-To:	<20130630045911.22b7bbe8@warrawoona.sti>
References:	<20130630045911 DOT 22b7bbe8 AT warrawoona DOT sti>
Date:	Fri, 26 Jul 2013 08:19:41 +0400
Message-ID:	<CAMvDHVCzNcy9ADCAxOy_0raU353pK5k0dMhsvojjDJR3vCoz8Q@mail.gmail.com>
Subject:	Re: [geda-user] gschem and metric sizes for symbols
From:	Vladimir Zhbanov <vzhbanov AT gmail DOT com>
To:	geda-user AT delorie DOT 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

As for gost symbol and grid sizes and some gost discrepancies,
read the interesting comments at [1].  Then see at [2] what this
results in when a user wants to make, say, a resistor symbol (and
how users of proprietary CADs fight against the same issues). They
have just shifted the top pin up to get the 2.5mm vertical
distance between the pins. As for the transistor sizes, I didn't
found a symbol such as yours with fixed sizes in any gost. Where
did you find it? For your information, there are two pages [3] and
[4] where all gost requirements related to symbol sizes are
summarized, the symbols there are illustrated with their sizes.
See that the gost 2.730 requires keeping only relative ratios for
transistors. It also shows that the balloons representing
component packages may have different sizes and shapes.

By the way, you can learn at [5] how many rubels costs the library
containing gost symbols for one of proprietary CADs ;)

Now, my thoughts of the issue.

There are many possibilities, but I think only three of them are
really useful:
1) Use 1mm grid where 100 points = 1mm
2) Use 2.5mm grid where 100 points = 2.5mm
3) Use 1mm grid where 40 points = 1mm

The first one is inconvenient. Your symbols would be too large
over against the default library symbols. You would hardly use any
default symbols in your schematic if you even want to do so.

The second two are nearly but not quite the same.  There is one
advantage with these two: your symbols would be similar to the
default library symbols, so you could use them without any
restrictions.

A disadvantage with the second option is that you will have all
the issues you mentioned here. You can work around by changing
some symbol sizes as in the symbols at the above mentioned pages.

However, consider the last option.
The last option is to use the same scale but another grid size.

Nothing prevents you from using metric grid with 1mm pitch. Hit
'oS' and type 40 for the grid size.
You can set this as default if you add the line:
  (snap-size 40)
in your ~/gEDA/gschemrc.
Modern gschem has a nice grid having thin and thick lines and the
distance between the thick lines is five times as much as the
distance between the thin ones. So, if you use 40 as the grid
size, you will have a 1mm thin grid and a 5mm thick grid.
However, you have to create your own library, which will probably
have incompatible pin size with the default symbols. There is no
problem here, you can always use '[' and ']' to increase and
decrease your grid twice in some rare cases when you need to
connect nets to other people's symbols.

Then, when you want to export your schematic, use
  gaf export -k 2,5mm -m 0 -o schematic.pdf schematic.sch
The -m option is optional here.  (I use zero margins since all my
titleblocks contain rectangles corresponding to standard paper
sizes, such as A4, A3 and so on.)
To use the zero size margins by default, type:
  gaf config export margins "0;0;0;0"
and you will not need add '-m 0' every time.
There is no config setting for default scale yet, but you can add
the above 'gaf export' command in your Makefile.

There is an issue with this option, though. gsymcheck will barf if
your symbol's pins are not on 100 mil grid.

Finally, I want to remind you that there is a script for resizing
symbols at [6] written by DJ Delorie. It can help you in the case
if you want to change your symbols in order to use any different
grid size. I don't know, though, whether it does font scaling.

[1] http://elektroshema.ru/razmugostat
[2] http://elektroshema.ru/2009-02-05-22-57-45/ugo-2/41-2728r
[3] http://www.electromonter.info/handbook/symbol_size.html
[4] http://elektroshema.ru/2009-02-05-22-57-45/ugo-1/razmerugo
[5] http://elektroshema.ru/disk
[6] http://www.gedasymbols.org/user/dj_delorie/tools/scale-schematic

- Raw text -