Robison Michael R CNIN wrote:

> hello,
> i've got a negative (ECL) and a positive (TTL) power plane
> on a board i'm doing.  right now i'm figuring on a matching
> ground plane for each power supply, spaced close to the
> rail for switching capacitance.  here's the stack i'm
> thinking of:
> critical traces
> gnd
> -5.2V
> noncritical traces
> noncritical traces
> +5V
> gnd
> critical traces
> does this seem reasonable?  i have some semblance of controlled
> impedance with each trace layer referenced to a dc plane.
> other stacks suggestions are welcomed.

Well, depending on how the board fabricator will actually assemble the
"book" of laminates and prepregs, it should be doable.  I guess the
thing is to make sure the critical traces and ground are etched from a
double-sided laminate, then the non-crit traces and power will be on
laminates, so you end up with 4 double-sided laminates.  This could
cause the noncritical traces to be awfully close together, but also the
power and ground planes will be close together, giving more distributed

I have done a lot of ECL and mixed ECL/TTL/CMOS mixed analog/digital
boards, mostly on 4 layers.  I generally have only one gnd plane and one

split power plane.  Some of the power planes get very complicated, with
interdigitated (zig-zag) voltage regions to bring power under the pads
where it is needed.  Some of the inputs to these boards are pretty
controlled impedances, and so signals on one side are using the gnd for
a ground plane, and signals on the other side use the power planes for
ground plane.  I've never really had a problem with the ground plane
issues.  I have had crosstalk, and had to completely re place one board
to make the signal flow in, around and out without high level digital
signals ever crossing over low level analog signals (this was on a
board, so I ended up using two signal layers on one side of the
planes for analog, and the other side for digital.)

For a board like you propose, I would try to use only one gnd plane, and

use split planes for the + and - voltage supplies.  This might get you
down to a 6 layer board, and cut costs.

> but i need both the ground planes common to each other.
> can i EVEN have two planes called GND?  is having two ground
> planes a bad idea?  if two ground planes is not a bad idea,
> then how do i tie them together?  NOTE:  if i tie them together
> i would like to do it in a way that doesn't mess up my design
> rules check.  i've noticed that additional vias and traces
> added to a pcb outside the schematic can make the design rules
> check flag them.

Yeah, I think Protel may have a problem with this.  If you have 2
planes assigned to net GND, then every via or through-hole that
is assigned to net GND will probably have a thermal connection to
BOTH planes.  This may be fine, electrically, but may cause problems
in solderability, and certainly will drive techs doing any rework

> i have another question.  this is iffy, but i'm a heathen
> designer anyway.  this is just a proto board, and although i'd
> like controlled impedance, i don't want to pay for it.  SO,
> what i am thinking is that if i get an 8-layer board at the
> standard 62 mil thickness, that they are going to be just about
> forced to give me between 6 to 8 mils between layers, without
> me ever having to spec it.  does this sound right?

I don't think a good board house will charge extra for this, if
you figure it out in advance.  DON'T design the board in a vacuum,
ie. figure out what you want and then submit the design.  Call
the board fab of your choice, and get them to TELL YOU what
they will use for laminate thickness for this build-up.  THEN, you
just use that info to calculate trace width.  That way, your job
fits in with their preferred flow.

How tight a controlled impedance is this?  I routinely work with stuff
where analog signals need controlled impedance of 50 Ohms +/- 1 Ohm,
or there are serious reflections.  To keep ECL happy, you don't need
that tight a control, especially if the traces are short.  +/- 10 %
be close enough, and that is much easier to provide.


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* Contact the list manager:
* Forum Guidelines Rules:
* Browse or Search previous postings:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to