On Fri, 7 Jan 2005 16:15:10 +0100 (MET) "Klaus Rudolph" <[EMAIL PROTECTED]> wrote:
> I found an footprint (element) in pcb library. I greped through all > directories in geda and pcb and could find it. > > The file is /usr/local/share/pcb/newlib/connectors/3terminal_screw_block ... > What footprint name I have to add to the footrpint attribute in gschem to > get > this symbol in pcb after running gsch2pcb? > I tried "3 TERM BLOCK" and "J2" and "DK ED1602-ND" and allways got: > CONN?: need new file element for footprint DK-ED1602-ND (value=unknown) > CONN?: can't find PCB element for footprint DK-ED1602-ND (value=unknown) > > > The data was lost and the layout could not be done. The footprint attribute is simply the filename, so use: 3terminal_screw_block > I have a file > ~/.gEDA/gnetlistrc > > Is this file correct for changing the path for the gsch2pcb or is there any > additional file? > > In the file I have: > (component-library "/usr/local/share/pcb/m4") > (component-library "/usr/local/share/pcb/newlib") > (component-library "/usr/local/share/pcb/newlib/connectors") > (component-library "/usr/X11R6/lib/X11/pcb/m4"); > ---- eof ---- No, gsch2pcb searches "elements-dir" directories. Was the tutorial you looked at: http://web.wt.net/~billw/gsch2pcb/tutorial.html because that does cover a sample design that creates a custom pcb element and shows how to add searching for it. gsch2pcb recursively searches directories for filenames matching footprint attributes. You give it directories to search with a command line or project line "elements-dir" option, this in addition to the default directories it will search: /usr/local/share/pcb/newlib /usr/share/pcb/newlib When you make a new pcb element, you could copy it to any subdirectory you create under those defaults, but it's better to have your own private directory of pcb elements. To illustrate, make a directory /tmp/nlib, then copy the 3terminal_screw_block file to /tmp/nlib/3t. Now if you make the footprint attribute in your gschem schematic be 3t, gsch2pcb should find it if you run: gsch2pcb --elements-dir /tmp/nlib Or put in a gsch2pcb project file: elements-dir /tmp/nlib > > I got no error message that there is something wrong but the gsch2pcb > process > did not run without errors. > > Is there any *actual* tuturial. I have an gsch2pcb tuturial which leaves me > totally alone with newlib components. The tutorial should cover these things, including the transistor issues you mentioned in your other list message. The tutorial does a transistor example design and there's a sample gschem and pcb transistor library set I link to there that is consistent. (It's true that there are some current gschem/pcb transistor symbol/elements that are inconsistent). Also, if you are stuck, post or send me what you are trying to do and the output you get with running: gsch2pcb -v -v ... It dumps a log of newlib directory searches of parts. Oh, and sorry if there ends up two list responses to this from me as I initially responded from an email address I'm changing to that wasn't yet list subscribed. Don't know if it will get through. Bill
