PCB Power Trace Widths, Ground Planes, and Routing

[John Larkin]

It's just 4 layers. Where would you need more layers for? Most of the
chips are surface mounted on one side. There is no sense in using more
layers because you have no space to put the via's.
If you look carefully at a modern motherboard, you'll find most of the
signals are routed on the component side. This means the 2 inner
layers and most of the solder side can be used for power.

I recently did a couple of boards using some fine-pitch 456-ball BGAs,
Xilinx FPGAs. We needed 8 layers, 6 mil traces, and 10 mil via drills
to get all the signals out. It might have been possible in 6 layers,
if the Vcc-io and Vcc-core had shared a layer and we'd worked at it a
lot longer, but it would have been really nasty.

John

 

[John Larkin]

Did you mean modern, or modem?

Modern. Funny, I bet I've written a few million lines of code and at
least a hundred manuals, and I've never learned to type.

John

 

[Richard Henry]

Modern. Funny, I bet I've written a few million lines of code and at
least a hundred manuals, and I've never learned to type.

Most mispellings won't pass by a compiler. Tragically, some will.
\

 

[Mac]

That makes sense for cards (I've personally done 10 layers and met the
.062" PCI spec), but why the restriction for motherboards?

We only designed CompactPCI boards. CompactPCI is a spec put out by the
PICMG (http://www.picmg.org/aboutus.stm). It specifies the thickness of
all cards, regardless of whether they are master cards (like the ones
I worked on) or peripheral cards.

I believe it. Multiple layers aren't all *that* expensive. Certainly a
*dime* is expensive for cheapcrap Taiwaneese desktop motherboards, but
there are many other markets.

Yeah, the cost wasn't a big issue. But we had an upper limit on trace
impedance that was hard to meet with a 14-layer, 0.062" board. We had to
use 4 mil traces on all the inner layers, IIRC.

--Mac

 

[Nicholas O. Lindan]

You'll be amazed what can be accomplished by using only 2 layers if
the bypass capacitors are well placed and the power is well routed. I
actually have a 2 layer 386SX 33MHz motherboard which was available
commercially (not my design, just something that ended up in a box
with PC stuff).

Did this once. Worked great until it came to EMI susceptibility.
Never got as far as emissions. The board was mounted in a
fiberglass enclosure and that didn't help, but neither did all
the conductive spray paint and rf-gasket we could stuff into
the blighter. Went to 4-layers, just added Vcc and gnd planes
with thermal reliefs to the power vias, and it worked a charm.

FWIW, I would advise some caution if you are planning a grid
ground plane on a 2-sided board with a real (not an 8051...)
processor.

2-sided PC & AT motherboards were common on Taiwanese clones.

 

[Nico Coesel]

[email protected] (Nico Coesel)wrote:


Did this once. Worked great until it came to EMI susceptibility.
Never got as far as emissions. The board was mounted in a
fiberglass enclosure and that didn't help, but neither did all
the conductive spray paint and rf-gasket we could stuff into
the blighter. Went to 4-layers, just added Vcc and gnd planes
with thermal reliefs to the power vias, and it worked a charm.

Still a problem with the power on the 2 sided board I guess. I made
quite some combined audio / digital PCBs. Never had problems while
using 2 layer boards even when the CPU was running its software from
external memory and have several microphone inputs on the same board.

 

[Paul Burke]

How important are ground/power planes here? Since this is a two layer
board with close to 500 connections on the pcb, even with a 6x8" board,
space is tight around the SMT chips, so I would like to avoid planes if
possible. If I do add a plane, should I include dead/unconnected copper
portions of the plane? Should planes be placed before or after
auto-routing?

Very important. Ideally you want every signal trace to have a ground
return parallel to it all the way, on the next layer down. You also want
the power to be distributed without significant static or dynamic
voltage drops.

4 layers achieve this more closely than ever you can with 2, but I've
had very good success with the following approach:

Route good thick (0.1") power traces for VCC and ground in the form of
grid patterns. Ensure plenty of decoupling caps, you may also want to
insert ferrites in the supply to some very busy ICs.

Route your signals, bearing in mind what you will do with the next step.

Flood fill all the area that remains with ground.

Use vias to stitch together all the ground fill and tracks. Examine
closely to optimise the connectivity of the ground "plane"- many routes
are better than fewer.

Iterate over the last stages until you are fed up of the whole thing and
want to get a life.

Paul Burke