> > 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
