[gta02-core] Layout - divide and conquer

Werner Almesberger werner at openmoko.org
Thu Aug 13 18:22:30 CEST 2009

?lvaro Lopes wrote:
> Good. But we have other ways to avoid reflections on RF side [1],
> like mitered bends.

Oh, sure. What I meant was "I don't need to implement angled pads in
fped anytime soon, because they don't exist in our design" :) Just
prioritizing my to do list.

> > - I couldn't find any distinct solder paste layer, so it seems that
> >   Openmoko put solder paste on the entire surface of each pad,
> >   including the center pads of QFNs.
> We can work that out, but will require some effort.

For now, I'd say we just do what Openmoko did. Once I've added a
separate solder paste layer in fped, we can replace the footprint.
All the pads would stay in place, so the layout isn't affected.

> > - the ATR610 is a little quirky, with pin 5 extending from the center
> >   pad. KiCad doesn't have pads of that shape, so we'll have to be a
> >   bit creative, e.g., separate the pads in the footprint, and join
> >   them with a trace.
> Can't we design a custom pad for it ?

KiCad only has rectangles, circles, rectangles with half-circles
("oval"), and "trapezoidal". The latter can actually do shapes that
aren't trapezoids, but they still have four corners.

Without looking at the code, I think the "trapezoid" geometry is
something like this:

(x0+dx, y1) (x1-dx, y1-dy)
(x0, y0)    (x1, y1+dy)

So this does doesn't give us the custom pad we need without making
significant changes to KiCad.  An easier path may be to teach KiCad
that pads with the same name are connected, and then just make two
adjacent rectangles.

> Lol, not GPS expert I'm afraid :) But yes, I'll gladly do GPS layout.

Great, thanks !

> I think we should come up with general layout rules first, layers
> specification,

Our goal should be to make a layout that doesn't depend on the
capabilities of a specific PCB house but that requires only generally
available technology. So the challenge is to find out what is
generally available ...

The 2442 BGA has a diagonal pad to pad clearance of about 15.7 mil.
Openmoko use 4 mil traces with a 4 mil clearance. Openmoko use a
12 mil diameter for external vias. The via drill diameter seems to be
1 mil. (Even if it isn't, 1 mil is good, because nothing else is that
thin, so we can find and replace it easily.)

I would make anything that carries power horizontally at least 10 mil
and short. If the amount of power is more than 100 mA, use a trace
width calculator, e.g.,

suggests that internal vias should be at least 16 mil in diameter
(but it's not clear if this refers only to peck drilling).  I think
Openmoko used 12-20 mil for internal vias.

Not sure how sophisticated we should get with vias before they become
hard to produce. Pad on via seems to be out. There's an interesting
variety of vias that are more or less possible, see page 5 of

If I read this right, and how I understand the process of making
multi-layer PCBs, I would say that we can have a through, blind, or
buried via at any x/y location and connected to any set of layers,
but not two blind/buried vias at the same x/y location.

If possible, I would also avoid buried vias altogether, because you
can't measure what's on them. I don't think we can avoid having
blind vias. I don't think peck drilling is an option, also because of
the board's thinness.

I wonder if all the simplifications we did would allow us to save a
pair of layers. If yes, that would be great.

> > - the part-to-footprint associations for the GPS subsystem
> I'll work on that. Won't be easy but we'll sync on IRC if needed.


> True. But reference designs are meant for "reference" only, not guaranteed
> to work or fit our purpose. :P We ought to be careful about those. I wonder
> if openmoko (former)people can give us a hand on this.

I think they're all quite busy elsewhere now. What we can do is have a
peek at the public gerbers, which pretty much tell us all there is to
know about the footprints, provided that we want to do exactly what
Openmoko did (which is the case most of the time but not always.)

You're making a good point that not all vendors can be trusted :) I
have a wonderful example that cost me one revision of IDBG. I'll
upload it in a bit.

> Unfortunately true. But can we live with that, ie, can't we simply
> have slight larger pads ?

I'm not sure. I would worry about some other metal bit sticking out
at unexpected places. But I don't think it's a big problem to
tweak those parameters if necessary.

> > - the footprint drawing. I hope we can do them with fped. I'll make
> >   it my first priority to fix any issues that pop up there.
> I'll do my best to help you on this, although it has been quite difficult
> for me lately.

Thanks ! Yeah, Gtk isn't easy. I did all the "core" stuff in about a
couple of days, and all the rest of the work has pretty much been
GUI ... Anyway, I still have to move lots of code around in fped, so
it's probably not very suitable for joint work yet.

> I wished :) That would allow for a small USB HUB, wouldn't it ? Or we
> just use the extra space to avoid RF interference.

Etch a little stop sign ? :)

- Werner

More information about the gta02-core mailing list