Hi Amit
The matter of a loosely coupled differential pair or a tightly coupled pair
make little practical difference to EMI if we make the assumption that both
traces are over a good (unbroken) plane. If you have given due diligence to
the design and routing of the pair, it is reasonable to say that EMI is
unlikely to be an issue. When the spacing between the traces becomes large,
there is no significant coupling between them and each trace can now be 50
Ohms as Lee suggests. There is only one time when close coupling is a must
and that is when there is no reference plane or shield. Even then it is not
a panacea, it only means you don't generate EMI if you also have ensured
that the signals in the pair are matched to each other in both level-change
and dv/dt, and also have no time skew between them. Either of these leads
to common-mode components in the pair which usually does radiate strongly
(as most people who have designed Ethernet interfaces can tell you). In the
case of a PCB you have planes to allow displacement currents to flow in a
controlled way with a minimal loop area, so two 50 Ohms traces with correct
termination is sufficient to keep EMI under control. On a PCB it is fair to
say that close-coupling is only a benefit if you don't have the space and
can't add more layers to accommodate all your signals. Otherwise
loose-coupled pairs win hands down.
Widening traces does control insertion loss but it is not the whole story.
Here are a few other things that might be worth giving a little thought to.
You should also consider any surface finish applied to the trace. For
example ENIG is commonly used but the conductance of the Nickel compared to
the Copper is much worse, so half the skin-effect current flows through the
Copper but the other half flows through the Nickel. If you must use ENIG,
apply it selectively; leave all the Copper that you are not going to solder
to unplated.
Another possibility is the smoothness of the Copper foil (much has been
said on this matter in other threads in this list).
If you want to reduce losses further, look at changing your dielectric.
This is a fairly radical solution (and usually not a cheap one) but when
the dielectric constant changes from around 4 to somewhere around 3 your
losses improve because of this and also because to keep the same impedance
the traces are now rather wider and the spacings too. If you've never used
these materials before, either by themselves or as hybrid boards (most
layers separated by conventional materials, but just the top layer
separated by the special material) take advice first.
Regards
Jon
On 2 June 2015 at 19:12, Lee <leeritchey@xxxxxxxxxxxxx> wrote:
Differential impedance does not matter. What matters is two good 50 ohm
lines, each terminated in 50 ohms.
Widening traces to reduce insertion loss is not the best way to control
loss.
-----Original Message-----
From: Amit Kumar
Sent: Tuesday, June 02, 2015 10:59 AM
To: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] tight coupling vs EMI
Hello experts,
For high frequency signals, it becomes important to widen the traces to
reduce insertion loss(skin effect).
But if we widen the traces, the spacing between the diff pair will have to
be increased to maintain 100 ohm impedance.
For one of my package design which has 12.5 G serdes, I changed the diff
pair width/spacing ratio from 20um/50um to 25um/75um.
This does reduce the insertion loss a bit.
I want to know how is this configuration with respect to EMI.
As the diff pair is loosely coupled, I assume the EMI will be higher owing
to weaker field interaction between the diff pair.
Can this be a potential problem? If yes, how do we quantify the impact and
optimize the design.
Thanks
Amit
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
