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. 2. Symbol and footprint libraries are decoupled for the above reasons. 3. A schematic element doesn't necessarily have a footprint assigned by default. Maybe because gschem can be used standalone (not for PCB) I would like to know any functional (not monetary) advantages of gEDA over eagle, I assume that there are many. Regards, Chetan Bhargava On Mon, Jul 25, 2011 at 10:11 AM, Colin D Bennett <co...@gibibit.com> wrote: > On Sun, 24 Jul 2011 19:17:39 -0700 > > Do you mean migration of particular designs (schematic/layout), > importing them to gEDA? > > Or do you mean migrating as a user? > > I have never used Eagle, so I can't be of any specific assistance in > that regard. However, I can say that while there are tutorial on > gschem/PCB and the general gEDA workflow, there is a need for a good, > complete tutorial for new users. > > Because gEDA is designed to support a wide variety of uses and workflow > methods, I feel it is not immediately clear to new users how to > proceed. > > Let me share my basic process for designing a circuit and PCB so you > can get a feel for how the tools might be used: > > 0.) Set up a revision control system. > Something modern like git or Bazaar is best. > Commit frequently, and write descriptive commit messages! > (I find this useful as a journal or log to come back to myself about > what I've done on the design, not to mention saving yourself from > screwups...) > > 1.) Draw schematic with gschem, placing symbols and drawing net > connections. > Various steps required as part of drawing the basic schematic: > > - Import any special symbols not in the default library from > gedasymbols.org > - If you can't find the symbol you need, draw custom symbol > in gschem, save as .sym file. > - Run a schematic design rule check (DRC) with “gnetlist”; > fix any DRC errors. > > 2.) Assign footprints to all components in the schematic. > You can do this in gschem or using gattrib (table view). > > - Import any special footprints from gedasymbols.org > - If you can't find an appropriate footprint, create one in the > “pcb” tool. (Takes some practice, but after a while it becomes > straightforward.) > - Make sure the footprints you are using are correct for the > parts you are going to use. > - Check footprints to make sure that pin assignments from > schematic symbol to PCB footprint is correct!! Watch out for > LEDs, diodes, polarized capacitors, etc. that may have pins > identified only as “1” and “2”. (I often use my own custom > symbols/footprints with more descriptive, logical pin identifiers > like “P” and “N” on diodes for P-type and N-type terminals.) > > 3.) Lay out the board. > - Import schematic into pcb. > - Set “preferences” for the design such as minimum copper > clearance, board dimensions, layer stackup, etc. > - Set up the grid as you prefer. > - Place components. > - Route tracks with lines. (You can use autorouter, but that is a > personal preference... I have always done manual routing.) > - Draw board outline on the “outline” layer. > - Add ground flood if desired. > > 4.) Verify design. > - Run DRC in the pcb program; fix any problems such as “copper areas > too close”, etc. > - Print out the PCB layout at 1:1 scale on paper and actually place > the parts on it. This is a sanity check to make sure footprints > are correct and spacing around certain parts are sufficient > (e.g., need enough spacing around some connectors, switches, > jumpers, sockets, heat sinks, etc.). > > I'm no wizard, just a novice, but I've done a few dozen designs and am > feeling very comfortable in gEDA myself so hopefully this is helpful. > > One thing that I've found is that it is worthwhile to “error-proof” > yourself through your process. Some of the common errors I've made are > related to incorrect pin assignments or footprint assignments, so I > take special care to validate those. > > Regards, > Colin > > > _______________________________________________ > geda-user mailing list > geda-user@moria.seul.org > http://www.seul.org/cgi-bin/mailman/listinfo/geda-user > _______________________________________________ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user