revisiting the 1000 faces of 0402

David Kuehling dvdkhlng at gmx.de
Sun Jan 23 11:10:32 EST 2011


>>>>> "Werner" == Werner Almesberger <werner at openmoko.org> writes:

> David Kuehling wrote:
>> Last time I was confronted with footprint selection in geda-pcb [1],
>> I found some interesting information in the footprint parameter list
>> geda.inc [2].  Note how they modify footprints for resistors
>> vs. inductors vs. capacitors.  The generic 0402 footprint (at the
>> bottom) is a compromise between all those (they use the metric naming
>> for the first footprints.  1005 is actuaully a 0402):

> Interesting, thanks ! But I must admit that I find the data somewhat
> puzzling. If I understand the logic right, then, say.

>> define(`PKG_INDC1005N', `PKG_SMT_2PAD_MM100( `$1', `$2', `$3', 70,
>> 50, 80, 170, 100, 0, 0)');

> would have pads 0.7 mm long (in the direction of the component's long
> axis), 0.5 mm wide, and a spacing of 0.8 mm between pad centers,
> leaving a gap of only 0.1 mm between pads. This seems awfully
> narrow. All the vendor data sheets unanimously specify 0.5 mm for the
> gap.

I think the geda-PCB folks pretty much know what they're doing :) Should
have sent a description of the the parameters with my last mail.  This
is from smt.inc [1]:

# -------------------------------------------------------------------
#
# internal: general purpose two pole surface mount
# $1:  canonical name
# $2:  name on PCB
# $3:  value
# $4:  pad X (size of pad in direction perpendicular to axis of part) [1/100 mm]
# $5:  pad Y (size of pad in direction parallel to axis of part) [1/100 mm]
# $6:  pad center to center spacing [1/100 mm]
# $7:  courtyard size in direction parallel to axis of part [1/100 mm] (V1)
# $8:  courtyard size in direction perpendicular to axis of part [1/100 mm] (V2)
# $9:  length of silk screen line [1/100 mm] (R1)
# $10: spacing of silk screen line [1/100 mm] (R2)
#
define(`PKG_SMT_2PAD_MM100',

So 0.7mm is the size perpendicular to the axis, along the axis it's only
0.5mm, giving a 0.3 mm gap, if I interpret it correctly.

[..]
> On page 51 of "The Circuit Designer's Companion, 2nd ed.", Tim
> Williams also gives a gap of 0.8 mm for 0603, noting that this leaves
> room for a 10 mil / 0.25 mm trace. Routing a trace across a 0603
> component seems to be a pretty common practice.

IIRC I was able to route small 6 mil traces through 0603 pads in PCB, so
that should be correct as well.

David

[1] http://pcb.cvs.sourceforge.net/viewvc/pcb/pcb/lib/smt.inc?content-type=text%2Fplain
-- 
GnuPG public key: http://user.cs.tu-berlin.de/~dvdkhlng/dk.gpg
Fingerprint: B17A DC95 D293 657B 4205  D016 7DEF 5323 C174 7D40
-------------- next part --------------
A non-text attachment was scrubbed...
Name: not available
Type: application/pgp-signature
Size: 189 bytes
Desc: not available
URL: <http://lists.en.qi-hardware.com/pipermail/discussion/attachments/20110123/baa17bd9/attachment.pgp>


More information about the discussion mailing list


interactive