From: Barry Ma (email@example.com)
Date: Mon May 22 2000 - 10:55:26 PDT
I agree with what you said: "Splits in layer 6 will have no effect on your traces since none will be referenced to them." Thanks.
Another modification to my Email of last Friday is
"The plane cap would work well to let return signals go from 3.3V plane back to gnd pins on layer 9." should be changed to "Both the plane cap and decaps would work well to let ...."
On Mon, 22 May 2000, "Morse, Earl" wrote:
> Splits in layer 6 will have no effect on your traces since none will be
> referenced to them. You already have a lot of interplane capacitance since
> the power planes are already sandwiched between ground. Reducing the
> thickness of the dielectric is another way to increase that interplane
> capacitance. That may disturb the characteristic Z of the traces you route
> in layer 6. Trading off the interlayer capacitance for more routing space
> may be a good swap. What are the frequencies involved on this board?
> Earl Morse
> Portable Division EMC Design
> Compaq Computer Corporation
> Phone: 281.927.3607
> Pager: 713.717.0824
> Fax: 281.927.3654
> Email: firstname.lastname@example.org
> Emissions Control Laboratory
> 10320 Rodgers Road, EC106
> Houst, TX 77070
> -----Original Message-----
> From: Barry Ma [mailto:email@example.com]
> Sent: Friday, May 19, 2000 7:27 PM
> To: firstname.lastname@example.org
> Cc: email@example.com
> Subject: re: Split Plane
> Here is my two cents worth:
> Did you consider exchanging 7 and 8 for more capacitance between 5V and gnd
> planes? Suppose you have 10 mil or less plane spacing. I understand that
> you want to use a gnd plane as return plane for signals on layer 9. But it's
> OK to use 3.3V plane as return plane. The plane cap would work well to let
> return signals go from 3.3V plane back to gnd pins on layer 9.
> It's also OK using part of 5V plane as additional 3V area. You'd better
> stitch up the gap.
> Barry Ma
> From: "Brad Crowell" <firstname.lastname@example.org>, on 5/19/00 2:04 PM:
> I have been lurking in the shadows of the SI list for some time now, but
> have come across a situation that I could use some advice on:
> I am working on a board design that is using the following stackup:
> 1 - SIGNAL
> 2 - GROUND
> 3 - SIGNAL
> 4 - SIGNAL
> 5 - GROUND
> 6 - 5V PLANE
> 7 - 3.3V PLANE
> 8 - GROUND
> 9 - SIGNAL
> 10- SIGNAL
> 11- GROUND
> 12- SIGNAL
> My problem is that we are running out of routing resources. Thus,
> it has been suggested that a few traces could be routed on layer 6,
> the 5v plane. The intent would be to route some traces for the 3.3v
> devices which are located away from the 5v devices on the board. This
> would reduce the effect of any splits in the plane. Also, since there
> is a ground plane available as a reference for every signal layer,
> a split in a supply plane shouldn't have much effect, if any. I am
> inclined to think, with my limited SI experience, that this should
> be ok, but would appreciate comments from some of the experts.
> Brad Crowell
> Hardware Designer
> AMIRIX Systems
> Why pay when you don't have to? Get AltaVista Free Internet Access now!
> This message is from the IEEE EMC Society Product Safety
> Technical Committee emc-pstc discussion list.
> To cancel your subscription, send mail to:
> with the single line:
> unsubscribe emc-pstc
> For help, send mail to the list administrators:
> Jim Bacher: email@example.com
> Michael Garretson: firstname.lastname@example.org
> For policy questions, send mail to:
> Richard Nute: email@example.com
Why pay when you don't have to? Get AltaVista Free Internet Access now!
**** To unsubscribe from si-list or si-list-digest: send e-mail to
firstname.lastname@example.org. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
This archive was generated by hypermail 2b29 : Wed Nov 22 2000 - 10:50:26 PST