Re: gEDA-user: Metric footprints in geda.inc (IPC-7351)

[Dan McMahill <dan@xxxxxxxxxxxx>]

David Kuehling wrote:
> Hi,
> 
> reading through the m4-style footprint definitions, I stumbled into the
> metric vs. non-metric footprint definitions
> (/usr/share/pcb/m4/geda.inc), i.e. 'RESC1005L', 'RESC1005N', 'CAPC1005L'
> etc which are approximately the same as '0402'.
> 
> Now I'm just wondering, for parts that the manufacturer claims to be
> 0402, is there any advantage in choosing one of the more specific metric
> footprints?  Also, reading through various datasheets, I cannot find any
> capacitors or resistors, for which the last part of the name 'L', 'N' or
> 'M' is specified, and the geda.inc file doesn't document its meaning
> (probably height of the part?).
> 
> Just wondering, whether to update one of my designs to (partially) use
> the newer footprints.  

"L" = Least material condition
"N" = Nominal material condition
"M" = Most material condition.

They represent a choice of 3 different size footprints that should all 
work with a 1005 package.  The choice between the 3 is governed by 
considerations like what the folks at your factory tell you is ok (if 
this is in a production environment), what you feel comfortable hand 
soldering if this is a home project, and how size critical your design 
is ("L" footprints are a fair amount smaller than "M" footprints).  But 
all 3 should give a reliable solder joint.

The "RESC" vs "CAPC" difference is a small difference in nominal package 
thickness.  There are some simple guidelines in IPC-7351 where for a 
given footprint family, min/max package manufacturing tolerances, 
min/max board manufacturing tolerances, and pick & place accuracy you 
get the footprints for the 3 different material conditions.


The 0402 is there because it had been there for a good bit and lots of 
folks were still very much wanting footprints with names like 0402, 
0603, 1206.  So whats there is roughly the "N" version thats between the 
CAPC and RESC ones.

-Dan


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