Re: gEDA-user: how to use an existing pcb newlib with gsch2pcb

[Bill Wilson <billw@xxxxxxxxxxxxxx>]

On Fri, 7 Jan 2005 16:15:10 +0100 (MET)
"Klaus Rudolph" <lts-rudolph@xxxxxx> 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