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: Tue May 23 2000 - 23:30:04 PDT


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

"Brad Crowell" <crowell@amirix.com> on 23.05.2000 15:49:16

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

Michael and others who have replied,

Yes, we have included alot of ground on this board. The concern for EMC/EMI
issues is quite high for our client, this is for a medical application. We
pulled out all the stops to ensure every signal layer is referenced to a
ground plane, rather than a power plane, which I understand should give
better EMC performance. We are also trying to avoid routing on the outer
layers as much as possible. The stackup you attached to your reply would not
provide as much interplane capacitive coupling, which concerns me. Clock
rates on my board are about 100MHz max, not extremely fast but includes some
devices with pretty quick edges.

Thanks for all the comments,
Brad
***************************************
Brad Crowell
Hardware Designer
AMIRIX Systems
***************************************

> -----Original Message-----
> From: owner-si-list@silab.eng.sun.com
> [mailto:owner-si-list@silab.eng.sun.com]On Behalf Of Greim, Michael
> Sent: Sunday, May 21, 2000 9:09 PM
> To: 'si-list@silab.eng.sun.com'
> Cc: 'mgreim'
> Subject: RE: [SI-LIST] : Split Plane
>
>
> Hi Brad,
>
> Let me see if I can help out. My first thought is
> that you have alot of ground on this board. You
> also have two power planes coupling to each other.
> In the absence of how this stackup was arrived at
> and your board thickness requirements, I will offer
> some advice.
>
> On a properly decoupled board, the signal does
> not always have to run next to a ground or the
> power plane that it is referenced to. It appears that
> you are trying to run your signals next to only the
> ground planes.
>
> Here is a stackup that we have used with great
> success up to toggle rates of 100 Mhz. Signals
> have a local ground and you end up with 2 additional
> routing layers. Make sure that your copper weights
> are adequate for your needs, but I think this should
> do the trick. The board also fits into a 0.0625
> thickness with out any exotic thin core materials.
> As you can see, the impedance from layer to layer
> is very consistent.
>
> I hope that this helps out.
>
> <<pcilk_r1_stk.doc>>
>
> Best Regards,
>
> Michael Greim
>
> And all this science they don't understand
> It's just my job six days a week.....
>
> The time is gone, The email's over, thought I'd
> something more to say.........
>
> Michael C. Greim Consulting Engineer
> Mercury Computer Systems, Inc email: mgreim@mc.com
> 199 Riverneck Road V: 978-256-0052/x1607
> Chelmsford, MA 01824-2820 F: 978-256-4778
>
>
> > -----Original Message-----
> > From: Brad Crowell [SMTP:crowell@amirix.com]
> > Sent: Friday, May 19, 2000 5:05 PM
> > To: si-list@silab.eng.sun.com
> > Subject: [SI-LIST] : Split Plane
> >
> > 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.
> >
> >
> > Thanks,
> > Brad
> > ***************************************
> > Brad Crowell
> > Hardware Designer
> > AMIRIX Systems
> > ***************************************
> >
> > **** 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
****

**** 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 - 10:50:27 PST