Re: gEDA-user: footprint

[Dan McMahill <dan@xxxxxxxxxxxx>]

watashi_metan@xxxxxxxxxxx wrote:
> Hi,
> I'm now developing some hardware and I have some problems with
> footprints.
> I'm working with smd 74hcxxx chips witch IMHO have SOXX footprints. Then
> when I add 7400 into schematics and set footprint to SO14 it runs
> correct. SO32
> works well too. But when I try to add 74373 ( witch have 20 pads ) and
> set 
> footprint to SO20 then gsch2pcb said:
>
> can't find PCB element for footprint SO20 (value=unknown)
>
> Where is the problem?

There is no single "SO20".  PCB has a SO20N, SO20M, and SO20W 
corresponding to 150, 200, and 300 mil widths.  This underscores a very 
important point.  Be sure to always double check your footprints.  This 
is important because

1)  There may be more than one package with the same name but different 
dimensions.  For example, SO-20 is not enough information.  ##-pin QFN 
is another since there may be two different pin pitches for a QFN that 
has the same pin count.  If you're using IPC-7351 names there is much 
less of a problem but at least right now, the libraries that come with 
PCB only have IPC names for things like chip resistors and capacitors.

2)  Whoever made the footprint may have messed up.  It is easy to do and 
I've seen both free and commercial footprints with errors.

3)  Your vendor may use non-standard pin numbering (CEL and their 
SOT-23's for example).

4)  Your manufacturing process may want some different sizes.  For 
example, IPC-7351 specifies a 3-tier library for Least, Nominal, and 
Most material conditions.  This just means that there is a range of 
sizes for the pads even for footprints covered by standards.

-Dan


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