Re: gEDA-user: adding footprints?!

[John Luciani <jcljr58@xxxxxxxxx>]

Here is what I do for PCB symbols ---

Any m4 symbols that I have checked I copy into a new
directory (/local/pcb/packages.m4 in my system). 
I use newlib methods for any symbols I create and copy
(or symlink) those to a different directory
(/local/pcb/packages in my system) that will be shared
among all projects.

Rather than create a "project" file for each project I
use the following shell script for all projects ---

#!/bin/bash
gsch2pcb --m4-pcbdir /local/pcb/packages.m4\
         --elements-dir /local/pcb/packages $@


(* jcl *)

--- Stuart Brorson <sdb@xxxxxxxxxx> wrote:

> Here are some recommendations:
> 
> 1.  Bill Wilson maintains an excellent tutorial
> about gsch2pcb & PCB
> here: 
> 
> http://web.wt.net/~billw/gsch2pcb/tutorial.html
> 
> Read it if you haven't already.
> 
> 2.  I recommend you create a
> footprints directory in your local project dir.
> Then, create a
> "project" file in your local project dir, and put
> the following in the
> "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 ./footprints
>  
> output-name InorBoard
> --------------------------------------------
> 
> Of course, replace all the stuff local to my system
> with stuff apropos
> to yours.   Of particular importance is the
> "elements-dir
> ./footprints", which points to my local footprints
> dir.  That's where
> you should stick all your footprints.
> 
> 3.  Avoid M4 footprints like the plague.  Make your
> footprints using
> the newlib constructs.  This simply is a text file
> holding definitions
> about all the graphical elements in your footprint. 
> Steve Meier wrote
> a nice doc about how to make newlib footprints; you
> can get his doc
> here:
> 
>
http://www.meierrippin.com/pcb_landpattern_design.pdf
> 
> 
> The doc is still in process, but there is enough
> useful info in there
> that it will get you 90% of the way to your goal.
> 
> 4.  You can (sort of) easily create a newlib
> footprint as follows:
> 
>   1.  Select the pcb-bin-library window.
>   2.  Click on and place a footprint similar to one
> which you want.
>       You must select a newlib footprint; M4
> footprints don't seem to
>       work.   The newlib footprints are in libraries
> whose names start
>       with ~.
>   3.  Select the footprint using the selection tool.
>   4.  Do "buffer->copy selection to buffer".  It
> will ask you to press
>       a  button at the element's location.  I
> usually just touch the
>       middle of the part.
>   5.  Then do "buffer->convert buffer to element". 
> Don't do anything
>       to get rid fo the ghost part which will
> accompany your cursor as
>       you move it around.  If this step works
>       successfully, PCB will emit a beep.
>   6.  Then do "buffer->save buffer elements to
> file".  Select your
>       local footprints dir and save it in there.
>   7.  Open the footprint up with a text editor &
> edit it.   Use the
>       info from Steve's doc to set parameters of
> your footprint.  You
>       may have to play around to make your
> footprints perfect, but
>       it's not hard once you get the hang of it.
> 
> Good luck!
> 
> Stuart
> 
> 
> 
> > 
> > i've been struggling to add my footprints (for
> mouser parts: 31VQ501,
> > 108-1MS1T1B1M1QE, and 502-RN-112APC) to my pcb and
> im having a ton of
> > trouble.  i THOUGHT i successfully added an m4
> definition to
> > /usr/share/pcb/m4 and ran the
> CreateLibrary{,Contents}.sh scripts to
> > maybe update the library (?) and nothing.  running
> gsch2pcb complains
> > that it can't find my package name.  i copied it
> from another one and
> > it still doesnt work.  i tried the graphical
> method (newlib i think
> > its called) to no avail because i never got the
> "save buffer elements
> > to file" menu item to actually DO anything (that i
> was aware of.)  am
> > i missing something?  how do you guys do it?  i am
> in fact having
> > problems with pcb ANYWAY, probably because of the
> motif dependencies
> > and misconfiguration... ALMOST enough reason to
> port it to gtk2. 
> > which, if i can finish this one freaking pcb by
> tomorrow night, i will
> > have enough free time to do. =)
> > 
> > thanks for any suggestions
> > handsome greg
> > 
> 
> 



		
__________________________________ 
Do you Yahoo!? 
Take Yahoo! Mail with you! Get it on your mobile phone. 
http://mobile.yahoo.com/maildemo