Re: gEDA-user: adding footprints?!

[sdb@xxxxxxxxxx (Stuart Brorson)]

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
>