> Do I understand correctly that heavy symbols basically have certain nets > with predefined names (e.g. VCC, GND) implicitly included, whereas light > symbols offer the pins to connect those nets oneself?
The difference between light and heavy is specificity. A light resistor, for example, is just "resistor". A heavy resistor would be "Rohm 1.2k Resistor, 1%, p/n XYZ, 0603 package with RESC0603M footprint, from Digikey v/n RHM123H-ND" > I checked the PCB reference on this subject for my PCB build > (http://pcb.gpleda.org/pcb-20100929/pcb.html#Import-Action ), but it > isn't clear at all what I should do to import a set of schematic > files (say, myproject_page1.sch, myproject_page2.sch and > myproject_page3.sch, all located in > ~/electronics/customer_x/techfiles/). Simplest version: you have foo.sch and foo.pcb. Import() assumes that, does it all by default. Less simple: foo1.sch and foo2.sch become foo.pcb. Edit the layout attributes, add "import::src0" value "foo1.sch" and "import::src1" value"foo2.sch". Then Import() uses that list of schematics. Least simple: set import::mode to value "make" and do it all in a Makefile. > When I simply choose File -> Import Schematics, PCB's log shows the same > response as when I press "O" -- it tells me the number of remaining rat > lines. At this point, I'm not asked for any schematic files, changed or > not. Check the terminal too, for any gnetlist errors. If your pcb and geda were installed at different locations, gnetlist might not be able to find pcb's importer module. > Should I fill in a space-separated list for src0, pointing to the > various schematic files? And what to do about "(null)", if anything? one file per import::srcN, so src0 is one file, src1 is the next, etc. _______________________________________________ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
