Dear Matthew Lamkin,

On my 4 layer boards, I try to keep the inner layer a solid ground plane and a
(segmented between +12V and +5V) power plane. In other words, I try to make
power planes that really are power planes in Protel-speak: negative image, with
colored circles at each via and hole that does not connect to ground, nothing
visible at vias that do connect to ground, colored spokes at holes that connect
to ground, and a colored board-perimeter trace.

I've never had to do blind vias.

I make the top (component) side have all horizontal traces, and the bottom side
have all vertical traces. A few short traces going "the wrong way" and diagonals
are OK, but they tend to block other wires. (Protel's autorouter does this all
too often -- it takes a short-cut of wiring one component directly to another on
the top layer. Then it gets stuck and can't push the next trace through that
area, and gives up. If it had gone up, over, then across with vias to the
appropriate layers, it would have left plenty of room for the other traces).

Try placing all the components in a plausible arrangement, then using Protel's
autorouter both ways ( top-vertical + bottom-horizontal and the other way) to
get a feel for which way is easiest for your board. (This also gives you clues
as to where there is congestion -- need more space between parts to get all the
traces through).

With one big QFP, you don't have much choice about routing wires straight out
from it. You might consider thinking about the areas immediately to left and
right of the QFP as "top-horizontal, bottom-vertical", and the areas immediately
up and down as "top-vertical, bottom-horizontal", no matter what the primary
routing direction is for the rest of the board.

[Since you do 2 layer boards, I imagine you already know all that better than I
do ... maybe you could write up a brief section "Tips for 2 layer boards" for
the Protel FAQ ?]

If you are convinced it's impossible to route everything with only 2 signal
layers (plus power planes), you're going to put some signals on an internal
layer.

I have one board where the "ground plane" really is a plane in Protel-speak. The
other internal layer (which I call a "power plane", since it's mostly +5V) is a
"signal layer" in Protel-speak, with a huge poured polygon (Net: +5V). That
polygon is a rectangle much bigger than the board. The board outline on the
keep-out layer and "Remove dead copper" make the polygon fit exactly the outline
of the board. (Also Grid Size:0 Track width:10). I have "Tools | Preferences |
[Y] plow through polygons" enabled to make it easy to pop to that layer, lay a
short trace, then pop back to an outer layer. With this style, you must manually
re-flow that polygon periodically to avoid millions of DRC errors (false
positive), and manually check to make sure that vias that should connect to that
layer don't get isolated (false negative -- an error that DRC doesn't detect).

Some designers here just make all layers "signal layers" the same way, even if
they're not going to squeeze any traces onto them, just the big polygon. That
way they can manipulate the polygon plane on the internal layers exactly the
same way they manipulate polygon planes on the outer layers, and they don't have
to deal with the confusion of "negative images" and the difficulty of placing
split planes.

The width of the board outline "track" on the keep-out layer, and the "board to
keep-out" clearance, are set to give me a total of 0.030 inch clearance between
the board edge and the +5V polygon on that internal layer. I have a copy of the
board outline on the ground plane layer using 0.060 inch tracks (of anti-copper)
to give me the same clearance. (Well, that's how I've done all my boards in the
past. Recently someone claimed that if I would give the +5V plane a larger
clearance, so that the ground plane sticks out further than the +5V plane, then
I would have less EMC radiated noise. Would that extra clearance of, say,
another 0.030 inch, really make any noticeable difference ?).

Signal layers and power planes are set up with "Design | layer stack manager".
You set the net of the power planes there.

Looks like I've rambled on long enough...

--
David Cary

Matthew Lamkin <[log in to unmask]> on 2001-03-12
02:21:29 AM
wrote:

...
The board will have amongst its components a MQFP208, and be a very tight
fit given the number of components
on it and where it is to fit (but then theyre all like that ar'nt they!).
...
Ok say I got the SMT components all placed on one side, are there any
suggestions or tips that you multilayer experts
can give me for designing with 4 layers?
I've got  funny feeling that I cannot get a power/groundplane on the inside.
I've been advised to steer clear of blind via's and have them all the way
through.
...

---------------------------------------------------------------------------------
DesignerCouncil Mail List provided as a free service by IPC using LISTSERV 1.8d
To unsubscribe, send a message to [log in to unmask] with following text in
the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
To set a vacation stop for delivery of DesignerCouncil send: SET DesignerCouncil NOMAIL
Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives
Please visit IPC web site (http://www.ipc.org/html/forum.htm) for additional
information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700 ext.5315
---------------------------------------------------------------------------------