Re: gEDA-user: pcb footprint for 100-pin TQFP, with 0.65mm pitch?

[DJ Delorie <dj@xxxxxxxxxxx>]

> http://download.cypress.com.edgesuite.net/design_resources/datasheets/contents/cy7c1380d_8.pdf
> 
> is the exact dimension of land pattern not given, and I was not able
> to find it somewhere else. So my home made footprint will only be an
> approximation.

The specs on page 27 are enough to make a land pattern.  Make the pads
at least as wide as the legs.  They should extend inwards far enough
to meet the minimum spacing specs, and outwards enough for the max
specs plus soldering room (20 mils in my case).

For example: the land portion of the leg is 0.60+-0.15 mm.  LONGEST is
0.75mm.  The NARROWEST the chip would be is 16-0.20mm or 15.8mm.  So
the space between pads on the board should be no more than
(15.8-0.75*2) 14.3mm.  Preferably 0.5mm or so less, as the fillet of
solder under that part of the leg gives it great strength.

For the outside, it's 16+0.2 + 2*solder = 17.2 for me.  That leaves a
pad length of (17.2-15.8)/2 or 0.7mm (28 mil).

Pad width is 0.30mm min (0.35mm gap leaves room for a 4 mil trace
between) but you could go bigger if you want.  0.4mm gives you ~10 mil
space between pads.

Then when you get the chip, print the land pattern on paper and put
the chip on it to make sure it all fits.  This step is FAR more
important than relying on math and spec sheets.


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