← Back to team overview

kicad-lib-committers team mailing list archive

Re: C_0805 footprint changes

 

Just as a follow up:
The pull request mentioned below has been merged. (Now the footprints should fully conform to IPC-7351B)

On 26/06/18 15:29, Rene Pöschl wrote:
This is because 0805 has larger tolerance ranges when compared to 0603.

For 0603 the tolerances are body length 0.2mm, "lead" length 0.25mm
For 0805 they are body length 0.3mm, "lead" length 0.5mm

I verified the tolerance ranges by checking 20 random resistors on
farnell. For both 0603 the components fall into the tolerance ranges
given by this ipc document. (I even found some 0805 parts that would
require increasing the tolerance ranges even further.)

You can look at the old IPC-SM-782 [1[ standard and check for your self.
That one still gives a suggested footprint. (The new IPC-7351B standard
does no longer do that. It gives equations how do derive the pad sizes
from the part sizes.)
The suggested footprints in that old standard use the same pad to pad
clearance for both 0603 and 0805. As that old standard gives no
explanation of how they derived that size i can only speculate that
their rounding base was larger.


There will however be some minor improvements to some of these
footprints. IPC-7351B uses slightly different equations compared to
IPC-7351. The pull request that updates this can be found at [2]

A very similar question arose over at the forum [3] (The later part of
the discussion is about footprints. The first part is a misconception on
how kicad works.)

[1] http://www.tortai-tech.com/upload/download/2011102023233369053.pdf
[2] https://github.com/KiCad/kicad-footprints/pull/689
[3]
https://forum.kicad.info/t/v5-heads-up-devs-dont-explain-here-the-upcoming-changes/11123/22
<https://forum.kicad.info/t/v5-heads-up-devs-dont-explain-here-the-upcoming-changes/11123/22?u=rene_poschl>



On 26/06/18 15:12, Wayne Stambaugh wrote:
Recently the SMT capacitor and resistor footprints where changed to use
rounded rectangular pads.  It looks like something may have gone wrong
with the Capacitors_SMD:C_0805_2012Metric footprint.  The spacing
between the pads is less than the 0603 footprint which doesn't make any
sense to me.  I looked at a few datasheets and I couldn't find a single
manufacturer where the 0805 spacing was less than the 0603 spacing.
Would someone please confirm that this is correct before I file a bug
report?  If this is correct, please include the reference document that
contains this information.  I want to understand how this is possible.

Thanks,

Wayne




References