[SI-LIST] Diif pair geometry trade offs
- From: tfox@xxxxxxxxx
- To: SI-List <si-list@xxxxxxxxxxxxx>
- Date: Thu, 14 Jun 2007 06:58:11 -0700
From: "Joel Brown" <joel@xxxxxxxxxx>
To: "SI-List" <si-list@xxxxxxxxxxxxx>
Subject: [SI-LIST] Diif pair geometry trade offs
Joel,
You have asked a very complicated question that would take some time even if I =
could sit down with you and do some simulations to illustrate the point.
Diff pairs generally want a line to line termination of 2X Z0 of a single line.
=
When you play with a nice lossy line simulator, you will find that the =
dimensions work out roughly to the numbers you specified. =20
For a given trace width and a given Er there is only one dielectric thickness =
that will work out to be Z0=85which is generally 50 ohms in most designs.
If you go to a narrower trace, you will need to move the trace closer to the =
plane in order to attain the 50 ohms.
If you have a fatter trace, the dielectric will need to be thicker and the =
trace moves farther away from the plane.
In other words, the dielectric thickness & dielectrict constant commbined will =
determine the thickness of the trace.
If you have the dielectric thickness and the trace width fixed, you will find =
that you can not get 2X Z0 for the "differential impedance" without getting the
=
traces fairly far apart. Ie 3x and 4x dielectric thickness being good =
representative numbers.
If you want greater routing density you will need to go to a thinner =
dielectric, because that will make the trace width thinner, etc.
That information would lead one to assume that a thinner dielectric is the =
answer to all of the routing density problems of the universe.
However, there is no free lunch. As you go to a thinner trace, closer to the =
plane, the attenuation per unit length goes up. As the frequency goes higher, =
the effect is more pronounced. I will try to post some pictures to illustrate =
the point.
If we had the pictures up you would find that fat traces far from the plane and
=
widely separated have less loss per unit length and hence result in a more open
=
eye on the receive end. =20
The narrow traces close to the plane, but still separated by 3x or 4x to get =
the "differential " line to line or single resistor termination value up close =
to 2X Z0 would have more attenuation and hence a more closed eye for the same =
trace length.
Now for the fire storm.
The actual impedance between the two traces makes very little difference. In =
other words, the separation between the traces has very little effect on the =
actual performance.
You can route the traces closer than 3X and get very little degradation in =
performance. I am not saying you can route them so close together that cross =
talk eats the signal, but the 3X 4X rules is somewhat like the Santa Clause and
=
the tooth fairy. It is a good notion to inspire people to do good things that =
can not possible hurt them, but it is not strictly true.
The two differential lines could be better though of as two complimentary =
single ended high speed signals. If they are 50 ohm lines, there need to see a
=
50 ohm termination at the receiver. If they are complimentary, their currents =
will be equal and opposite. Hence instead of having 2 ea Z0 resistors to the =
reference voltage, we can have 1 resistor of value 2X Z0=85.ie a 100 ohm =
resistor in most cases.
When we make the leap to believe that the difference impedance between the two =
transmission lines needs to be held at exactly 2X Z0, that is not actually =
true.
If you get too close, cross talk from the P to the N will become a factor, but =
using up a lot of real estate to route differential pairs is not necessary =
except in the most extreme cases.
If you either build some example designs or get a good lossy line simulator you
=
can really dial these things in.
I would also recommend some of Lee Richey's work. He has stirred up a hornet's
=
nest with this subject on a number of occasions.
TFox
Terry fox
tfox@xxxxxxxxxx
www.siemc.com
I am working with a layout that uses diff pairs routed as stripline on
internal layers and micro strip on outer layers. These include PCI Express,
USB, LVDS, Ethernet.
There are guidelines I have read that recommend spacing between pairs and
between other signals should be at least 3x dielectric height for stripline
and 4x dielectric height for microstrip.
I am using 13.5 mils dielectric height for the internal layers which means I
need spacing of 40 mils.
If I want to increase my routing density (decrease spacing) then I would
need to decrease the dielectric height.
In order to do this I would have to increase the inter pair spacing to
maintain 100 ohms impedance which would reduce the inter pair coupling and
increase the coupling to the reference plane.
This means more current would flow on the plane. My understanding is that
this plane current flows in a circular loop on the plane underneath the diff
pair traces essentially cancelling itself out to some degree. My question is
there any issue (EMI or other) with forcing more of the return current to
flow on the planes? If density was not an issue would it be desirable to
make the dielectric height as large as possible to reduce reference plane
current?
=A0
Thanks - Joel
------------------------------------------------------------------
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
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:
