Re: gEDA-user: adding footprints?!

[handsome greg <xdissent@xxxxxxxxx>]

yeah.... apparently on the actual pcb website, their doc skips the
"copy selection to buffer" part.  thus, nothing actually happened.  i
get it now =)


On Sat, 15 Jan 2005 18:03:41 -0500 (EST), 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
> >
> 
>