Re: gEDA-user: More questions about PCB footprints

[Bill Wilson <billw@wt.net>]

Stuart Brorson <sdb@cloud9.net> wrote:

> Now I have another issue:  On my system, I place
> gEDA & associated EDA
> stuff under /usr/local/geda.  This means that the
> footprint lib lives
> under /usr/local/geda/share/pcb.  
> 
> I am using Bill Wilson's wonderful gsch2pcb, and
> have a project file
> pointing where the various files live.  Here's my
> project file: 
> 
> --------------------  project file
> ------------------------
> schematics InorBoard.sch
>  
> m4-pcbdir /usr/local/geda/share/pcb/m4
> elements-dir /usr/local/geda/share/pcb/newlib
> elements-dir /usr/local/geda/share/pcb/pcb-elements
> elements-dir
> /usr/local/geda/share/pcb/pcb-elements/resistors
> elements-dir
> /usr/local/geda/share/pcb/pcb-elements/capacitors
>  
> output-name InorBoard
> --------------------  end project file
> ----------------------

gsch2pcb should recursively descend elements-dir directories, so I think
you don't need to explicitely list the "resistors" and "capacitors" dir.

> When I run gsch2pcb, the program can find the
> footprints living in
> pcb-elements, but it can't find the m4 footprints. 
> The output spew
> from gsch2pcb is below.
> 
> Questions:  
> 
> *  What other variables do I need to set in order to
> point
> gsch2pcb to my non-standard m4 location?  

That's all you need to redirect to the non-standard m4 install location.
If in addition you have extra m4 files somewhere (something like a
stand alone customized xxx.inc file), you add them with "m4-files"
lines.  But I don't think this is the problem.

> > *  I have seen some mention (via Google) about a
> > pcb.inc file.  I
> > don't have one of these.  What does pcb.inc do?  Do
> > I need to set one
> > up? 

The default PCB m4 install directory is set up to automatically
search a variety of xxx.inc files in that directory.  These are
all of the PCB defaults.  If you have customized some m4 files
you may have them named to something like yyy.inc and those files
are made known to gsch2pcb via m4-files project or command line
options.  gsch2pcb as a convenience additionaly looks for magic
files pcb.inc in the project directory and ~/.pcb/pcb.inc in your
home directory so you can set up some custom m4 files without
worrying about adding them to a project file.

> > *  Am I using the wrong footprint name for the DB-9
> > and DB-25
> > connectors?  Otherwise, any ideas why I can't find
> > the footprints for
> > these parts?

This may be the problem, I can't seem to find SUBD_25M parts defined
in any *.inc file in the PCB m4 directory.  They are referenced in
connector.inc and connector.m4 but have no actual package body
definition ... possibly left over remnants from a PCB library
revision.  Try using parts like DB25M and DB25F as these are
defined via a geda.inc redirection to SUBD_MALE_LAY and SUBD_FEMALE_LAY
parts in connector.inc.


Bill