Re: [SI-LIST] : Split Plane

About this list Date view Thread view Subject view Author view

From: Christoph Hillen (Christoph.Hillen@aachen.utimaco.de)
Date: Thu Jun 08 2000 - 00:21:38 PDT


Dennis,

It took some time, but now: I have some pictures for you of a GND-Plane on the
top layer, there you will see that it's quite a good plane.
A "swiss cheese" is not the problem from my opinion. Anyway, you will always
have your planes with holes!
Of course you have to take care to avoid routing under "slots", e.g. under a
0.5mm pitch QFP, if the plane acts as the reference plane for these signals.
But measurements have shown that it's an improvement regarding EMC / radiation.

I have sent the pictures to you in a separate mail, I don't want to send them to
the group because they are around 100kB each.
If anyone of the others members is interested, I will send them to you.

Best Regards,
Christoph Hillen
Utimaco Safeware AG
Germany

Dennis Yarak <yarak@apple.com> on 24.05.2000 19:16:15

Please respond to si-list@silab.eng.sun.com

To: si-list@silab.eng.sun.com
cc: (bcc: Christoph Hillen/Aachen/Utimaco/DE)

Subject: Re: [SI-LIST] : Split Plane

Christoph,

I investigated microvias for my last project and while pricing is still high
(you need to eliminate more than 2 layers to even come close to making it
cost effective, unless you have microBGA's that force the issue), in long
conversations with my layout folks I became increasingly doubtful of the
actual routability improvements.

Secondly, a stack as you propose gives me pause. The top and bottom
"ground" plane references will be Swiss cheese or worse in a board of
significant density. Signals routed in the adjacent layer will see the
return path come as go as it traverses, say a BGA. It would seem to be a
signal quality and EMI nightmare rather than an improvement.

Would love to hear others' experiences with using microvias and the stack
you ended up with. The one that appealed to me the most was a 2-8-2 (blind
1-2, 1-3, 10-9, 10-8, no buried vias to save cost).
SIG
GND
PWR
SIG
SIG
GND
GND
SIG
SIG
PWR
GND
SIG

This way the power and ground connections would have minimal inductance to
the planes (via in pad to adjacent layers). All signal layers can be
nominal 50 Ohms with 4 mil traces in a standard 0.062 board thickness. You
can even go thinner if you push and weight is a factor.

Unfortunately, my designs having about 8 different power rails complicates
the execution of this board significantly.

Dennis Yarak
Apple

> From: Christoph Hillen <Christoph.Hillen@aachen.utimaco.de>
> Reply-To: si-list@silab.eng.sun.com
> Date: Wed, 24 May 2000 08:30:04 +0200
> To: si-list@silab.eng.sun.com
> Subject: RE: [SI-LIST] : Split Plane
>
>
>
> Brad,
>
> Did you think about doing this job using MicroVia technology?
> In this case you would be able to cover the top and bottom layer with ground,
> as
> the Fanout-Vias are in the pad.
> So the top and bottom ground plane will be real planes over the whole board!
> Then the stackup could look like this:
>
> GND
> Signal
> Signal
> 3.3V
> GND
> Signal
> Signal
> GND
> 5V
> Signal
> Signal
> GND
>
> Because of the MicroVias, you will be able to route much more effective, as
> they
> don't block other layers - perhaps you can even save one or two signal layers.
> If you are looking for good EMI performance, this would be a good idea.
>
> Christoph Hillen
> Utimaco Safeware AG
> Germany
>
>

**** To unsubscribe from si-list or si-list-digest: send e-mail to
majordomo@silab.eng.sun.com. 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
****

**** To unsubscribe from si-list or si-list-digest: send e-mail to
majordomo@silab.eng.sun.com. 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
****


About this list Date view Thread view Subject view Author view

This archive was generated by hypermail 2b29 : Wed Nov 22 2000 - 10:50:32 PST