Adam Wang wrote:
> About these footprints made by Fped, can be used in KiCad. So we collected
> footprints under KiCad Libraries, still some few footprints from else
> projects have not been added.
Great work ! A few comments:
- TO-252 component in to.fpd had a zero-width pad 2. This caused
fped to emit incorrect Postscript and I wouldn't be surprised
if KiCad could get confused, too.
So I've made it an error (in fped) to have pads of zero width
or height. I fixed to.fpd by simply deleting the table row for
pad 2 (commit 359ccc048dbe6300aa4ef5aeb4853aa9421fe910). I hope
that's correct.
- likewise, tssop5.fpd had a zero-width pad 5. Fixed in
c21e1f0424bbc860aadb9e17433d39cb65e442b5
- my meander-2450MHz.fpd also had a potential zero-sized "pad"
in the form of the optional tail for tuning the antenna for
different PCB thicknesses. Fixed in
711147c11d276b21cd017baa24ed603eceadbdaf.
- the distances between copper and outline in pads.fpd are a bit
strange, particularly for the circular pads. How about
introducing the distance as an explicit parameter and then
calculating the radius as
r = sqrt(x*x+y*y)/2+distance+w/2
or, since x = y in this case, simply
r = x/2+distance+w/2
- a lot of through-hole components only have a measurement on the
hole but not on the ring. You may want to consider adding the
ring diameter as well.
Examples: RCA-3-RA (rca-3-ra.fpd), USB-A-DUAL-RECEPT-RA
(usb-a-dual-recept-r.fpd), HE-1x2-100mil ... (he-2row-dip.fpd)
- in some of the c-t-smd.fpd components the measurements are very
close to the pads, making them overlap in the catalog. Maybe
"silk" (5 mil or 0.127 mm in this case) is a bit too tight a
spacing.
You could even consider expressing the distance in terms of
Y-V1. But just a larger constant step size should do, too.
- in c-smt.fpd, the lines in "outline" and "outline_slope" don't
always intersect at the same point. How about putting the two
elements in the same frame, so that you can simply share the
point ?
Also, you work a bit too hard in the tables. You could simply
have a table for a variable { d } { 1 } { -1 } and then
multiply py with it, without having to duplicate px, x, y, and
most of the formula of py.
- SOT-235 in sot.fpd: the overall width measurement intersected
with the pads. I placed it at a constant distance from the pads.
Commit 6ff4042bd2c480db411f41f7dd8c10c3cc3b6fc6
- eus.fpd (EUS): that's a terribly short name with a high risk of
clashing. How about renaming it at least to TI-EUS or maybe
R-PDSS-T6 (which seems to be synonymous) ?
- ir.fpd (TSOP348): very short name of the .fpd file. The
footprint looks very cool, though :-)
- spacer.fpd: the ones with copper have solder paste on them.
Are you sure you want this ? To get rid of the solder paste,
change the pad type from "normal" to "bare".
I also made a few small changes:
- pads-array.fpd: didn't have measurements. I also enabled a few
more pad types (all at a 100 mil spacing, up to 10 elements).
Commit 71075ec7050b7f39d1124ff03cfa62a35e67553c
- header.fpd: added measurement of overall length
Commit 6216a97c22b8a563fc35a616e8c353456a418ba6
- dip.fpd: didn't have any measurements, shame on me !
Commit: 563e5944e3d90c4b28613930558eb34f20040541
- meander-2450MHz.fpd: the measurements of the *-left-* variants
are at weird places. This is a known bug. Fped's logic for
picking the location of measurements isn't prepared for
handling mirroring. Not sure if there's a good way to fix this.
Updated catalog - now with 317 footprints - is at
http://downloads.qi-hardware.com/people/werner/tmp/kicad-libs-modules.pdf
- Werner
_______________________________________________
Qi Hardware Discussion List
Mail to list (members only): [email protected]
Subscribe or Unsubscribe:
http://lists.en.qi-hardware.com/mailman/listinfo/discussion
