I have a question about 4 layer boards... If there is such a thing as
a typical layout, would it consist of signals & hardware on the top
layers, signals on the bottom layer, an internal power plane with all
3.3 volt connections to this plane via vias (sorry), and the other
internal layera ground plane with all grounds (from the two outer
layers) connected through vias?

Does this make sense, or do people normally route signals through the
two internal layers.

Thanks much, Tom

Blip wrote:
Unless it's an RF stripline or microstrip design that's pretty much how
it looks like. If it gets tight you can cram the decoupling caps on the
other side. Just keep the variety of parts on that bottom side low, like
only 0.1uF caps and 100k pull-ups.

Hint: If you've never done that have a professional layouter do the
first round and watch him/her carefully.

--
Regards, Joerg

http://www.analogconsultants.com/

On Mon, 17 Mar 2008 18:16:15 -0700, Joerg
<notthisjoergsch@removethispacbell.net> wrote:


Thanks Joerge -- I'm a hobbyist/hacker with this stuff - don't know
anywhere to go watch this; however, I'd be glad to watch some kind of
video of this if anyone's aware of any out there (probably should have
googled this first before I replied).

Best, Tom

Joerg wrote:
built by hand then put whatever the heck you want on the back.

Some space-sensitive boards in high-end systems don't make much
distinction between the 'top' and 'bottom' layers, as long as they can
cram everything they need onto the board. Fabrication costs go up
sharply, though.

--

Tim Wescott
Wescott Design Services
http://www.wescottdesign.com

Do you need to implement control loops in software?
"Applied Control Theory for Embedded Systems" gives you just what it says.
See details at http://www.wescottdesign.com/actfes/actfes.html

Blip wrote:
Personally, I've never had much use for power planes. Using one of the
internal layers as a ground plane is a big win, but I use the other
internal plane as a routing layer. Route your power with thicker
tracks, be careful about your bypass capacitors and routing from the
caps to the package pins, and use polygon pours to give you a mini-plane
(on any suitable layer) if you need it.

If you've got a higher speed board (> 50 MHz), or particularly high
current parts, you need to think more carefully - but for most boards,
dedicating a whole plane to 3.3V is a waste (IMHO, of course).

In article <CJEDj.4212$qS5.702@nlpi069.nbdc.sbc.com>,
notthisjoergsch@removethispacbell.net says...
There are times when it makes sense to put components on the bottom side
also. In my case, they were an RF comms module and a GPS module. You
have to be careful about putting surface mount components on the bottom
side as it can complicate automated assembly. Since my boards are
hand-soldered, that's not been a big problem.
crowd things too much. 20% extra room really makes the layout
go faster!.

Mark Borgerson

In article <47df6a73$0$8168$8404b019@news.wineasy.se>,
david.brown@hesbynett.removethisbit.no says...
can be very difficult to cut traces or add jumper wires to the
nets routed on the internal layer.

There is also a potential disadvantage to power and ground on
internal layers: you can end up drilling out a lot of holes
to find the short circuit! In my case, I forgot that the
prototype quick-turn service plates ALL holes so that only
one drill or mask step is required. Some mounting holes that
were specified as unplated ended up shorting power and ground
planes. Luckily, I had only 4 holes set up that way---
on a component I had cut and pasted from another designer's layout.

I've modified the part pad stack so that the inner layers are
set back from the holes (a good practice in any case, if you
plan to use metal mounting screws).


Mark Borgerson

Mark Borgerson wrote:
These are all general points about multi-layer cards, which apply no
matter what you do with the inner layers. Basically, if you expect to
be doing significant amounts of trial-and-error on your pcb tracks, you
should either take it into account when doing the layout (if you think a
track might not be right, route it through a 0-ohm resistor to make it
easy to test and "cut"), or stick to a two-sided pcb with a larger area
(to make it easier to route, and easier to modify after production).

David Brown wrote:

Another old trick is to order the first 10-20 boards in the form
of two double layer boards. Put a sheet of woven glass fiber
cloth (the kind used in fiberglass) between the two boards as a
spacer and solder a thin wire through every via. If everything
tests out, order the next batch in 4-layer. If there is a
problem, you can cut and jumper another set of 2-layer boards
and assemble them into another pseudo-4-layer board. Order
the thinnest standard board material if you do this.


--
Guy Macon
<http://www.guymacon.com/>

On Tue, 18 Mar 2008 08:08:28 +0100, David Brown
<david.brown@hesbynett.removethisbit.no> wrote:

Gentlemen -- I appreciate all of these answers & more importantly the
discussion about those answers - for me, this venue, google, & a
couple of good books are the fastest way for me to ramp up in a new
(to me) technology. Now that I've blown the smoke... I have a few
more board-related questions...

1 How is it possible to tell how many layers a board consists of? If
you only hace the board in hand? This seems to me a problem...

2. What can I expect when routing under a 256BGA? These are stoopid
questions, but I don't know, not can I find the answers to them. Since
I want to route on at least 1 bottom layer, do I have to put vias on
every bubble-pin that will route to a lower layer?

3. Can I route across the top layer between the pads? Can I put vias
between the top layer pads?

4. Last, is there a standard size for SMT caps & resistors? I've gone
through the shapes & compared the different classes (ex 1402, 1210) at
mouser & it seems that any number of footprints will work in a given
situation. Do I go w/ the smallest pad? The cheapest (these are not
for big runs)?

Thanks for your time.. Best, Tom

Blip <blip@krumpli.com> writes:
Um, cut it open and look at a cross section under a microscope?

The more pin rows, and the closer the pins, means the smaller design
rules you'll need, and the more layers you'll need to route the
signals out from the bga. 256 balls means four rows, so if you can
route one trace between balls/vias, that's two layers - the top layer
is the first two rows, the next two rows via to the bottom. Normally,
each additional row is an additional layer, since the existing vias
are in the way, preventing you from bringing out two rows. If you can
fit two traces between balls/vias, the rules change, etc.

Normally, the vias go between the balls, not under them - unless
you're willing to pay extra for via-in-pad. Google for "dog bone
bga".

If they fit.

I'd go with the smallest you're comfortable with, that work with the
sizes you need (i.e. big caps don't come in small packages). In
general, smaller is better for bypass caps, and often cost (to a
point). 0603 seems to be the most cost-effective size these days, but
0402 is catching up.

For each standard size (like 0603 or 0402) part, there are usually a
couple of land patterns of varying sizes; these have more or less
extra copper around the part to ease soldering; use a larger pad for
hand soldering and a smaller pad for space-critical reflow soldering,
etc.

Another option which I use is to put an 0805 or 1206 land pattern
down, but put 0603 parts on it. The larger land allows me to change
the part if needed, like for power rail filter caps. It also allows
others to use the design even if they're not comfortable with parts as
small as I use.

DJ Delorie <dj@delorie.com> writes:
Gak, 256 balls is 16x16, or eight rows from the edge. That's 6 signal
layers (two rows on top, two "outer via" rows, and four more for rows
behind vias).

Often the innermost balls are for power/ground, which may save you
some routing layers.

A 64-ball BGA is four rows from the edge.

Blip wrote:

Shine a bright light through it.

Single layer: duh.

Two layer: With the light, you only see the traces you see on both sides.

Four layer: With the light, you see traces or a plane that
are not on either side. Also, without the light you see
component leads that appear to have no traces and vias that
have zero or one traces.

Six or more layers: Almost certainly one of the layers is a
plane, so your only way to tell it from a four layer is
usually to look at the edge with a microscope. Sometimes
you can tell by counting how many sides a large BGA needs
to reach the vias around it; if it needs all four layers
but your light shows a plane, it's six or more layers.

BTW, if it's a PC motherboard, they often brag about how
many layers they use. Check ads and website.


--
Guy Macon
<http://www.guymacon.com/>

Blip wrote:
Often they have a stack-up-strip : Results in a simple staircase
of one number per layer.
That helps the PCB house get the layers in the right order,
and avoids doing one twice!

Depends on your design rules. A good starting point, is the Vendors EVAL
PCB. Look at what they did, and the rules they used.
Often, you can import their File into your CAD package, and get
a head start.

Choose the one easiest to handle!
That's probably 0805 : 1206 are trailing off, and 0603 are
getting too small to handle manually.

-jg

On Mar 18, 4:34 pm, Blip <b...@krumpli.com> wrote:
Look for Xilinx XAPP 157. Altera also has a similar document. Most of
what I know about PCB layout is drawn from manufacturer app notes and
reference designs.

In article <47e087d1$1@clear.net.nz>, Jim Granville says...
And of course make sure they are large enough to handle the load.

Robert

--
Posted via a free Usenet account from http://www.teranews.com

Blip wrote:
I don't know any movie about it since I can't watch YouTube stuff (yet).
What helps is to disassemble things and take a look. For example an
antenna pre-amplifier or mast amplifier. They are not as dense as other
RF gear such as cell phones so they provide a better learning
experience. Distribution amps are often soldered shut so a mast
amplifier may be better because they are easier to open without
destroying them.

--
Regards, Joerg

http://www.analogconsultants.com/

Tim Wescott wrote:
Yes, then it won't matter. However, having active parts on the back side
can become a little nightmare in debugging if the whole thing is mounted
in a rigid housing and you can't easily get to the bottom.


That's why I suggested limiting those to bypass caps of the same kind
and such. I did that on a board end of last year and the cost increase
was quite minimal. I was told that it would have been major if they had
to do a full rigging for lots of different parts, basically like twice
the cost.

--
Regards, Joerg

http://www.analogconsultants.com/

On Mar 19, 1:34*am, Blip <b...@krumpli.com> wrote:
You'll find plenty of BGA routing info here:

http://www.pcblibraries.com/

Leon

Blip wrote:

[...]

Often you can take a strong magnifier and look at the side of the board,
even if the planes aren't routed to the edges (they shouldn't). Or look
into a large non-metallized mounting hole.


Careful with BGA, they need a very precise temperature profile. I avoid
them altogether where possible even if some call me a Luddite. This is
definitely a topic to discuss with a really seasoned layouter.


Yes and yes. But heed the clearance req's of the fab house. Old rule:
The finer the pitch, the less fab houses will do it, meaning more $$.


My layouter has his own libraries for that, he is older than I am and
thus knows what works. Don't simply take the ones in the CAD libraries,
always vet them with either a fab house, a data sheet or, better, with
an experienced layouter.

--
Regards, Joerg

http://www.analogconsultants.com/