X-Authentication-Warning:	delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient:	geda-user AT delorie DOT com
X-Google-DKIM-Signature:	v=1; a=rsa-sha256; c=relaxed/relaxed;
	d=google.com; s=20120113;
	h=mime-version:in-reply-to:references:date:message-id:subject:from:to
	:content-type:x-gm-message-state;
	bh=A8yntEraPeCqNWkZNLPQKaVclqfbO42Z4F4CAQHbw8I=;
	b=G2EQVA7yiiu/sPcP/3NYFfx6nOzaYRYURoBjJyu6hNRNhQZFvrf1ucF0qhMpo4tX6x
	58K+UvRFiKBuu8Q+0egtoK/nj8xzJiWeLB57xQBXc4T00pFpNOAwcD1Zec3kpifsXUt8
	WlPaV3zmD9d4qMxg0ch34EAIQlTJrbZsrac3aA5sG/kD04jxBbl4fYJbUJ5FT1W7OBwq
	LNWmIRsfSH2mslLTQwQFfZh0ApmrDL6gylAnTpezEbRRzLLxqG2/9GzGXwfnKXNBPZwO
	lhyGLv6ny8i7dtlrgg4RZM0AmeIe3TGuFovKWQr+UOil4rSVwKNdOGhMXPFW/zMMBGPO
	5alA==
MIME-Version:	1.0
X-Received:	by 10.194.47.167 with SMTP id e7mr9091861wjn.57.1374162594815;
	Thu, 18 Jul 2013 08:49:54 -0700 (PDT)
In-Reply-To:	<CALSZ9goF9oRVUfHM_UDyM60Kr=x4ONsXVtnVe4VJdm=F9YmDBg@mail.gmail.com>
References:	<CALSZ9goF9oRVUfHM_UDyM60Kr=x4ONsXVtnVe4VJdm=F9YmDBg AT mail DOT gmail DOT com>
Date:	Thu, 18 Jul 2013 08:49:54 -0700
Message-ID:	<CAN0Jx-8bMxPQu5AkX80U-3qB=U2HWg0-astWEuDj2cWS-k0ApA@mail.gmail.com>
Subject:	Re: [geda-user] PCB BGA (ball grid array) Package/Footprint
From:	Russell Dill <Russ DOT Dill AT asu DOT edu>
To:	geda-user AT delorie DOT com
X-Gm-Message-State:	ALoCoQkUWpWd/1QfnhiHJBVeNNPW19nZmFTNAwbGTUOh0qFlr63BVQVp1Dxi1+kKqhd6v+17q/2U
Reply-To:	geda-user AT delorie DOT com
Errors-To:	nobody AT delorie DOT com
X-Mailing-List:	geda-user AT delorie DOT com
X-Unsubscribes-To:	listserv AT delorie DOT com

On Thu, Jul 18, 2013 at 6:19 AM, Rob Butts <r DOT butts2 AT gmail DOT com> wrote:
> Has anyone done a PCB using the new chips with the BGA (ball grid array)?
> If so, how did you define the footprint?  As through-holes?  Fab shops must
> be capable of accommodating these ICs otherwise they wouldn't exist.

Sure, its just a 2d array of round smd pads. Putting holes in BGA pads
would be bad, very bad. Some bga balls would be ok, but some would
wick through the hole and you'd have a no connect. For very small
pitch BGA (0.5mm and smaller) people will put the via in the center of
the pad, because there is no room between pads for vias. In this case
they fill/cap the via so that solder can't wick through it. Hopefully,
you are designing with 1mm or 0.8mm and don't need this.

Here's an example of such a footprint:
http://www.gedasymbols.org/user/russell_dill/footprints/FF784.fp

The document Bob Paddock linked, which is available here,
http://www.pa.msu.edu/hep/atlas/l1calo/reference/other/mentor/mentorpaper_bga_breakouts_and_routing_52590.pdf
is more of an advanced document.

Instead, start simple, take a look at the images on this page:

http://wiki.altium.com/display/ADOH/Fanout+and+Escape+Routes

The outer row of pads is of course easy, the 2nd row can route between
the pads of the outer row, the 3rd row needs vias connected to their
pad in a dogbone shape and can route out on another layer easily, the
4th row can also use vias and route between the vias of the 3rd row on
the same layer, and so forth.

> I'm thinking they must be easy to solder since it would simply fall into
> it's position with either pre-soldered holes or pre-soldered pins/balls.

I'm not sure exactly what you mean here, but there are two processes
hobbyists use for BGA. One is a stencil, usually with the stencil
window about 80% of the area of the pad. Stencils can be had from
ohararp or oshstencils. (NB: Don't use lead free solder balls with
leaded paste and vice versa). The other is applying a thin layer of
flux to the area of the BGA footprint. Both work well.

For reflow people use skillet, hot air, and ovens. If you are using
lead free components, you probably want to use an oven as it allows
you greater control over the temperature profile.

And yes, in my experience 1mm bga is easier than say, 0.5mm tqfp/tqfn.

- Raw text -