[SI-LIST] Re: MGB/s pair crossing on adajent layers
- From: "Ken Cantrell" <Ken.Cantrell@xxxxxxxxxxxxxxxx>
- To: "steve weir" <weirsi@xxxxxxxxxx>, "Hirshtal Itzhak" <ihirshtal@xxxxxxxxxx>
- Date: Wed, 2 Jun 2010 09:26:46 -0600
Hirshtal,
Orthogonal routing introduces zero crosstalk at the intersection of the
orthogonal pair. Perpendicular E & H fields do not interact. Offset
broadside coupling should solve your problem, but you will need to have
software capable of that analysis. Hand calculations aren't accurate
enough. The idea is to interleave the two trace layers, with the layer 2
traces positioned in the spaces between the layer 1 traces (or vice-versa).
With a 4 mil separation between trace layers the coupling will be high. You
will probably need to spread the traces out 3x - 4x the trace width on each
layer.
If you don't have a solver, now would be a good time to get one.
Ken
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx]On Behalf Of steve weir
Sent: Wednesday, June 02, 2010 4:54 AM
To: Hirshtal Itzhak
Cc: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: MGB/s pair crossing on adajent layers
True perpendicular routing should not introduce any significant
cross-talk. If you are autorouting, I would be more concerned with
keeping the number of layer swaps and their associated vias / via stubs
in check.
On the other hand, if you have significant parallelism between offset
stripline layers then you can manually estimate or better use a field
solver to figure out how much cross-talk you are going to get. It
should come as little surprise that if you have 4 mils to your return
plane and 4 mils to parallel victim traces that you can couple a
significant amount of energy into the victim traces. You would want to
review that carefully to see if it is enough.
Steve
Hirshtal Itzhak wrote:
> Hi Experts!
>
>
> I use double-stripline layers for MGb (PCI-Ex, sRIO) pair routing. I
> ordered the PCB Designer not to route such pairs on adjacent layers,
> close to each other, not even PERPENDICULAR to each other.
>
>
>
> Now it seems I can't avoid it any more. My PCB Designer seems to run out
> of real-estate.
>
>
>
> I have 4-mil separation between the 2 layers and 4-mil from each one to
> a GND layer on each side.
>
>
>
> The pairs are running at 2.5 to 3.125 Gb/s
>
>
>
> What risks, if any, I run into, if I do permit routing the pairs
> perpendicular to each other? Are there any precautions I should take
> while doing it?
>
>
>
> Thanks
>
>
>
> Itzhak Hirshtal
>
>
>
> Elta
>
>
>
> The information contained in this communication is proprietary to Israel
Aerospace Industries Ltd., ELTA Systems Ltd.
> and/or third parties, may contain classified or privileged information,
and is intended only for
> the use of the intended addressee thereof. If you are not the intended
addressee, please be aware
> that any use, disclosure, distribution and/or copying of this
communication is strictly prohibited.
> If you receive this communication in error, please notify the sender
immediately and delete it from
> your computer. Thank you.
>
>
> This message is processed by the PrivaWall Email Security Server.
>
>
>
>
> ------------------------------------------------------------------
> To unsubscribe from si-list:
> si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
>
> or to administer your membership from a web page, go to:
> //www.freelists.org/webpage/si-list
>
> For help:
> si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>
>
> List technical documents are available at:
> http://www.si-list.net
>
> List archives are viewable at:
> //www.freelists.org/archives/si-list
>
> Old (prior to June 6, 2001) list archives are viewable at:
> http://www.qsl.net/wb6tpu
>
>
>
>
--
Steve Weir
IPBLOX, LLC
150 N. Center St. #211
Reno, NV 89501
www.ipblox.com
(775) 299-4236 Business
(866) 675-4630 Toll-free
(707) 780-1951 Fax
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List technical documents are available at:
http://www.si-list.net
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List technical documents are available at:
http://www.si-list.net
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
