Sorry, it was (and is) too late and my brain conked out. Let me see if
I can get it right.
I'd not realized that this was an ongoing debate, obviously the gEDA
community has thought long and hard about the 'heavy' vs 'light' symbols
debate.
As someone who is very recently trying to make the switch from
closed-source to open-source EDA packages but has a lot of experience
with open-source software in general, I should point out that a narrow
well-defined user operation flow is acceptable and preferrable in
day-to-day work. Keeping the package open-ended and not making any
assumptions about what the end-user wants are admirable goals, but
open-source software too often falls into the black hole of "lets keep
our options as open as possible" and avoids settling on a single way of
doing a given task. This usually makes the package a pain to wrestle with.
Most of the closed-source big-business EDA software packages I've used
(and I haven't seen them all, I'm sure) have a library that contains a
'light' version of most of the major components (for example, an "ideal
NPN transistor") to allow open-ended schematic design and 'ball-park'
simulations, and then an exhaustive list of 'heavy' device-specific
symbols and associated SPICE models to fascilitate quick design
building, accurate simulation, and convenient PCB layout. I think
having a symbol file that contains all the information about its
schematic representation, which simulation model it is associated with,
and what physical package it is manufactured in goes a long way toward
nailing down a single well-defined but still versatile and powerful
design flow from schematic capture to simulation to PCB layout. Having
to call separate programs in between these steps to fill in missing
information slows down the design loop and makes the package feel
cumbersome.
I should say at this point - PLEASE don't be offended by any criticism I
offer up here. I full respect the work that has gone into gEDA and am
mighty thankful that it's actively being developed. Most of my job is
software development, so I know what it's like to try to wrangle a large
product like this. But I also know that the best input is often a fresh
take by someone that's seeing your project for the first time. I hope
any comments I make are useful, even if only to give a feel for how the
uninitiated initially respond.
Ok, enough philosophy, let me lay out that problem i was having.
My first crack at building a .sym file for a 2N5551 transistor looks
like this. I know there's some pintype definitions left empty, I'm
still working on that.
v 20050820 1
L 300 900 600 700 3 0 0 0 -1 -1
L 600 400 600 800 3 0 0 0 -1 -1
L 470 410 500 370 3 0 0 0 -1 -1
L 440 450 470 410 3 0 0 0 -1 -1
L 440 450 421 381 3 0 0 0 -1 -1
L 500 370 421 381 3 0 0 0 -1 -1
L 600 500 469 412 3 0 0 0 -1 -1
L 421 381 300 300 3 0 0 0 -1 -1
P 300 1200 300 900 1 0 0
{
T 400 1000 5 10 0 1 0 0 1
pinseq=1
T 400 1000 5 10 0 1 0 0 1
pinnumber=1
T 400 1200 5 10 0 1 0 0 1
pinlabel=B
T 400 1400 5 10 0 1 0 0 1
pintype=
}
P 800 600 600 600 1 0 0
{
T 700 700 5 10 0 1 0 0 1
pinseq=2
T 700 700 5 10 0 1 0 0 1
pinnumber=2
T 900 700 5 10 0 1 0 0 1
pinlabel=A
T 900 900 5 10 0 1 0 0 1
pintype=
}
P 300 0 300 300 1 0 0
{
T 400 100 5 10 0 1 0 0 1
pinseq=3
T 400 100 5 10 0 1 0 0 1
pinnumber=3
T 0 0 5 10 0 1 0 0 1
pinlabel=C
T -700 200 5 10 0 1 0 0 1
pintype=
}
T 700 0 8 10 0 1 0 0 1
footprint=TO92
T 700 200 8 10 1 1 0 0 1
device=2N5551
T 700 400 8 10 0 1 0 0 1
description=Small signal transistor
T 0 600 8 10 1 1 0 0 1
refdes=Q?
Note at the bottom that there's text attributes for footprint, device,
description, and refdes. Also note that field 6 of the 'T' line for
footprint and description is set to 0 (invisible), while its set to 1
(visible) for device and refdes.
If I open gschem up and inset this symbol into a blank file, and then
save and open that .sch file in a text editor, it looks like this:
v 20050820 1
C 72300 52600 1 0 0 2N5551-1.sym
{
T 73000 52800 5 10 1 1 0 0 1
device=2N5551
T 72300 53200 5 10 1 1 0 0 1
refdes=Q?
}
Note that the device and refdes attributes where preserved, but the
description and footprint attributes have been 'cleaned off'. I can
make an attribute survive or fail this importing process by simply
flagging it as visible or invisible in the .sym file. Also, opening up
the device's properties inside gschem only shows the device and refdes
attributes.
What I wanted to do was define attributes in the .sym file that I did
not necessarily want to be visible on the schematic, but that were still
preserved and associated with the symbol so that it could be passed on
to PCB. For instance, I wanted 'footprint' to be invisible but still
there so that PCB could use that information.
It appears that gschem decides to keep any attribute that is marked as
visible, and throws away any attributes that are marked as invisible in
the .sym file. Is this how it was intended to work?
I can appreciate that the prevailing wisdom is that the library should
be 'light', but that shouldn't prevent me from building a custom 'heavy'
library of symbols if I want, should it? This behavior of gschem means
I either can leave attributes out of my .sym file and add them to my
symbols after I've inserted them into the schematic, or I can leave the
attributes visible in my .sym file and then manually make them invisible
after I've inserted them into the schematic. Either way, I have to open
the properties of every symbol I import, which is what I was trying to
avoid in the first place.
Thanks for reading this enormous post, and thanks for your patience, and
above all thanks for your continued development of this package. Have a
good one.
- Jonathan Hanson
Louisiana State University
Department of Physics and Astronomy
Stuart Brorson wrote:
I'm running into an issue with symbols and gschem.
I think gEDA and friends are a good idea, and I'm going to attempt to
make the switch from closed-source packages. However, one big glaring
issue I've noticed in gEDA is the state of the symbol library. The
organization is pretty bad. Also, according to the tutorials I've read
for capturing a schematic and then laying it out as a PCB, you have to
hand edit attributes like 'footprint' in several of the symbols after
dropping them into the schematic. This obviously isn't the best way to
have things set up; it would be better if these symbols were already
loaded with the useful information, even if that means a larger library
to choose from.
This is a subject which comes up frequently on the geda-user list. It
is called using "heavy" vs. "light" symbols. You can read about it here:
http://archives.seul.org/geda/user/Jun-2005/msg00000.html
FWIW, the main gEDA developers tend to prefer light symbols since it
provides maximum flexibility and makes minimum assumptions about the
user's requirements. OTOH, it makes the user do more work. . . .
[snip]
Anyway, I figured I would just build my own custom symbol library to my
own spec, since all I use are basic passive parts, a few transistors and
some diodes. It shouldn't be too hard to just build symbols as I need
them. I read through the guide at
http://www.geda.seul.org/docs/current/fileformats/index.html detailing
how to build a symbol, and starting building a 2N5551 transistor model.
Now the problem I have is in the visibility of attributes. I intend to
have all the useful attributes filled in (stuff like documentation and
footprint), but these aren't values that need to be visible on the
schematic once the device is inserted into the schematic. The problem
is, a section of the .sym file like:
T 1400 0 8 10 0 1 0 0 1
footprint=TO92
gets ignored by gschem when the symbol is inserted. Checking the
attributes of the symbol only shows attributes from the .sym file that
were marked as visible. The sixth field being set to '0' is supposed to
make the following attribute invisible, but instead, gschem just
considers it something to be thrown away. Saving the file that the
symbol was imported into and checking it with a text editor confirms
that anything that wasn't marked 'visible' is stripped off a symbol.
I am not sure why your attribs are disappearing. What do you mean
that gschem just throws the symbol away? Here are some suggestions:
* Maybe the attributes aren't thrown away, but you just can't see
them because they are invisible. Do "edit" -> show/hide invisible
text" to toggle attribute visibility.
* Are you attaching the attributes to the symbol itself? If so,
gschem doesn't promote most attributes. Most attributes should be
attached to teh symbol in the schematic. That is, create teh symbol
with only a "DEVICE" and "refdes" attribute, place it in your
schematic, then attach teh remaining attributes there.
BTW, if it is
too painful to attach the attributes individually using gschem, use
the utility "gattrib" (from teh command line) to input & edit attribs
using a spreadsheet. To use gattrib you must first place your
components, and then give them refdeses. After that, you can input
any attributes you want using gattrib.
* If the attributes really are disappearing from your symbols, please
make sure that you are using an up-to-date version of gEDA/gschem.
The file format has changed within the last year or two, and possibly
you are using older documentation for the file format (although your
line above looks fine to me & is the same as a recent schematic on my
machine).
* Finally, a small point: Make your symbol's Y coordinate something
positive, not zero. This will place your symbol in a good place when
you open it with the symbol editor. I tend to see values in teh 1000
range on good symbols.
There're lots of attributes that need to be kept associated with the
symbol in the file, but not necessarily displayed on the schematic.
Would it be possible to modify gschem so that attributes in the .sym
file that are marked as invisible still get stored in the .sch file, but
just stay marked invisible so as not to appear on the schematic?
You want to promote symbol attributes into the schematic, and then
leave them in the schematic? Can you please elucidate?
On the previous note: I don't know what the protocol is for building new
symbol sets, but once I'm done with the resistor and capacitor sets in
standard values, I'd be happy to tar them up and submit them. Would
there be any interest in them?
http://www.gedasymbols.org/ has been set up for this purpose. It is
currently incomplete. You can contact the guy who set it up and ask
him to put up some symbols. He may ask you to help by
running/maintaining the site.
Stuart
