[SI-LIST] Re: Routing of 12 GHz diff pairs
- From: "Jon Powell" <jonpowell@xxxxxxxxxxxx>
- To: <phillip.r.wellington@xxxxxxxxxx>, <emj14@xxxxxxxxxxxx>,<Giovanni.Guasti@xxxxxxxxxx>, <hannappe@xxxxxxxxxxxxxxxxxx>,<buck@xxxxxxx>
- Date: Wed, 2 Apr 2003 09:35:12 -0800
More of a question than an answer:
Wouldn't broadside coupling provide significantly more differential coupling
that may tend to mitigate the other factors and keep the signal skew
smaller?
It seems that differential pair coupling on the same layer is more on the
level of cross-talk than actual differential coupling.
jon
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]On
Behalf Of phillip.r.wellington@xxxxxxxxxx
Sent: Wednesday, April 02, 2003 6:59 AM
To: emj14@xxxxxxxxxxxx; Giovanni.Guasti@xxxxxxxxxx;
hannappe@xxxxxxxxxxxxxxxxxx; buck@xxxxxxx
Cc: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: Routing of 12 GHz diff pairs
Hi,
You really have to be careful with broad-side coupled pairs. If the pair
elements are on layers separated by prepregs you may have some
mis-registration because of layer float during manufacturing. The
mis-registration caused an impedance change due to the traces not aligning
on top of each other. There may be some mis-registration in the printing and
etching process as well even if a core is used. There is also a difference
between the foot of the trace and the top of the trace (trapezoid etch
factor related) which may affect your impedance prediction, work with your
target board house.
To help minimize the mis-registration, wider traces may be used to make the
mis-registration effects less of a percentage of impedance change. This of
course makes the dielectric separations wider making routing more difficult
and adds layers because of the high line-to-line impedance that you need.
Side-by-side routes eliminate the mis-registration errors. Side-by-side
traces present routability issues in high density connectors as you need to
route 2 traces between pins and clearances causing length differences
between the differential pair elements. With broad-side routed pairs, the
lengths can be kept reasonably close through pins to the destination. With
side-by-side routes it can be managed, it just requires more attention to
detail.
You have to be very careful what the return path is above and below both of
these configurations at this frequency. This includes what is on both
reference planes. They should be at the same potential (RF - equal noise
level) so that the pair elements do not have any differential currents other
than the intended differential signals. The planes should also be as quiet
as possible- certainly not near switching supply return paths. Obviously,
you would not want to route other traces adjacent to the pair (differential
noise coupled into one pair element at a higher level than the other pair
element). You would not want to route across any plane split (return path
problems and unplanned delays). It is desired not to route any traces under
the pair in the side-by-side configuration.
There are other things to watch for too, not enough time though.
Hope this helps.
Ross
-----Original Message-----
From: Erik Jacobs [mailto:emj14@xxxxxxxxxxxx]
Sent: Wednesday, April 02, 2003 7:22 AM
To: Giovanni.Guasti@xxxxxxxxxx; hannappe@xxxxxxxxxxxxxxxxxx; buck@xxxxxxx
Cc: Si-List
Subject: [SI-LIST] Re: Routing of 12 GHz diff pairs
> Hi Buck,
> I think the best way to satisfy your customer is to draw the pair on two
> faced layer.
> But ... this method has many drawback:
> 1)it's more difficult to control vertical than horizontal distance between
> pairs(due to PCB layers compression). So you could achieve a pair with a
> wrong impedance.
> 2)in order to obtain the right impedance, you could require a bigger
> distance between layers
> I would prefer to draw the pair on the same layer, making a compromise: a
> max difference of 2.5mm (l/10) could be enough?
> > We are working with a customer that is using 12 GHz
> diff-pair signals.
> > The customer "requires" that the time of flight across the pair
> > "must" be equal at all points in time. Can any one shed any light
> > on how this can be done?
>
> The easiest way to achieve this is to use broadside coupled pairs,
> because there both conductors are identical and routing is therefore
> much esier.
I'm about to do some 10GHz routing with similar requirements. It seems that
if you are using coupled pairs and you made the physical length almost
identical, wouldn't the electrical length and electrical parameters be
pretty close? I mean, assuming the signals got onto the PCB the same way
and assuming that the material was relatively uniform and assuming you had
good ground planes (or ground wires running under the diff pair traces)...
Also don't you kinda need to assume that there's nothing around the traces
that will couple INTO them? I.e. if p side of diff couple has coupling to
some other line but N side has no such coupling? Even if it's only
capacitive/inductive coupling (non-crosstalk)
-Erik
Test Engineering
LeCroy
------------------------------------------------------------------
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 archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
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 archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
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 archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
