On Mon, 25 Jul 2011 22:33:11 -0700 "bsali...@gmail.com" <bsali...@gmail.com> wrote:
> Thanks for the detailed steps Colin. > > Sorry I was not clear I was looking to migrate as a user. Although I > have a license for eagle but sometime get limited by the number of > schematic sheets. So far I haven't reached max board size. I have > moderately large customized libraries on eagle. I use git with my > current setup as my version control mech. > > Couple of days back I was able to create a test schematic on gschem > but it was not obvious to transfer the schematic to PCB. I guess it > will take time to learn. > > So far I made a few observations comparing eagle: > > 1. Schematic & board are decoupled so any changes to schematic need to > be re-synced to the board. I haven't figured out the way yet. There are two ways to do this: an old way, and a new way. I can't tell you too much about the differences since I've only really used the old way, but the new way is simpler. (a) The new way is to use the new File | Import Schematics command in pcb to update the layout from the schematic. (b) The old way is to use the gsch2pcb command line tool or the xgsch2pcb GUI tool. > 2. Symbol and footprint libraries are decoupled for the above reasons. Correct. Although, the symbol and footprint libraries do need to agree on some things like pin naming so that things are mapped correctly. For instance, in my custom symbols and footprints, I use “P” and “N” for my diode pin names, and “G”, “S”, and “D” for FET pins. (In the case of FETs, I prefer to have a single schematic symbol that is not dependent of physical pin configuration, and then a footprint that maps the logical pins to to proper pins on the package.) > 3. A schematic element doesn't necessarily have a footprint assigned > by default. Maybe because gschem can be used standalone (not for PCB) This is a controversial topic among the gEDA community. Symbols with a footprint attribute built-in are termed “heavyweight” symbols, and symbols that do not come with a pre-assigned footprint are called “lightweight” symbols. The problem with heavyweight symbols is that there is no one-size-fits-all answer. Are you making a through-hole design? Then you likely want 1/2 W through-hole resistor footprints. Are you making an SMT design? Then you may want 1206, 0805, 0603, 0402, or some other SMT size resistor. It much more difficult for the case of diodes, LEDs, transistors, capacitors, inductors, switches, etc., because of the wide range of package options in use (even down to transistors with different B/C/E or G/S/D pin mappings...). You can “heavyify” certain symbols for ease of use in specific applications, however, by taking a lightweight footprint, assigning a footprint, and saving it in a new symbol file. Personally, I find that I need to check and double-check every footprint assignment in my design anyway with the actual BOM parts to ensure there are no errors before I lay out the board. Therefore I prefer to have no default footprints, and force myself to assign the proper footprint rather than getting some incorrect default that might slip by my verification. > I would like to know any functional (not monetary) advantages of gEDA > over eagle, I assume that there are many. I think the simple fact that your designs are not locked into a proprietary system is the first advantage of gEDA. What if EAGLE's maker goes out of business? Will you be able to access and edit your designs when Windows 8 comes around if EAGLE is not ported to it? Regards, Colin _______________________________________________ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
