Re: gEDA-user: connecting symbols that look nothing like their footprint

[John Griessen <john_g@xxxxxxxxxx>]

Meador, Ryan D wrote:
my real problem has to do with the fact that my FET's package is SO8.
> 3 pins are source, 4 are drain and 1 is gate.  How to I convey to gschem that
> the single source and drain symbol pins should actually be connected to
> multiple physical pins? 

The secret is....   "connecting symbols that look nothing like their footprint"
is NOT the problem we need to solve....


I saw two replies already with concepts for you to think about, and here's 
another.  To do verbatim what you ask, you convey that to gschem by creating a 
symbol to match your situation, and attaching a footprint property with the name 
of a matching footprint you will make and put in your local pcb footprint 
element library.  Your symbol has a list of pairs, (plus more, but the pair of 
values are the key ones), of names and numbers of pins.  The below scripts use 
the bash command shell -- adjust to your situation...

djboxsym and jgboxsym, (gedasymbols.org), are ways to create a symbol box from a 
list of the form:

rmfet.symdef
======================
# rmfet symbol creation file
[labels]
rmfet
Ecosensory.com
refdes=Q?
! copryright=2006 Meador, Ryan D
! author=Meador, Ryan D
! uselicense=unlimited
! distlicense=GPL
! device=rmfet
! description=fet

! footprint=rmfet.fp
[left]
1 S
2 S
3 G
4 G
[right]
5 D
6 D
7 D
[top]
[bottom]
=============

then run:
djboxsym rmfet.symdef > rmfet.sym


and edit  rmfet.sym in gschem to tweak the appearance,
then put it in your dir like mine called 
~/EEProjects/now/circuitboards/gschem-cibolo/ic-gull-wing

that is listed in a file
~/.gEDA/gafrc
containing lines like:

(component-library 
"${HOME}/EEProjects/now/circuitboards/gschem-cibolo/ic-gull-wing")


and restart gschem or just the library chooser
and place that new symbol.


Next to do with pcb,
add a working dir file:
gafrc
with a line like:
lib-newlib = /home/john/EEProjects/now/circuitboards/footprints_pcb


(Where your new footprints will go)


Now make a footprint with rows of pads with DJ's dual in line pad layer outer 
footprint generator  (see gedasymbols.org)

if you got the layout just right, but the number order wrong use the n key in 
pcb to change the pad numbers,

or just regenerate the footprint again with a different numbering alignment -- 
the default is likely the way your package is.

John Griessen

I've written this in on swoop with no proofing, so...  let's turn it into a FAQ 
or guide, huh?


_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user