My pleasure.
From: Amit Kumar [mailto:amit.j.kumar@xxxxxxxxxxxxx]
Sent: Saturday, June 6, 2015 9:44 AM
To: Jonathan Riley; leeritchey@xxxxxxxxxxxxx
Cc: si-list
Subject: RE: [SI-LIST] Re: tight coupling vs EMI
Thanks a lot Jon and Lee.
From: Jonathan Riley [mailto:jonathan.lloyd.riley@xxxxxxxxx]
Sent: Wednesday, June 03, 2015 3:23 AM
To: leeritchey@xxxxxxxxxxxxx <mailto:leeritchey@xxxxxxxxxxxxx>
Cc: Amit Kumar; si-list
Subject: Re: [SI-LIST] Re: tight coupling vs EMI
EXTERNAL EMAIL
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
<mailto: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 <mailto: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 <mailto: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 <mailto: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 <mailto: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 <mailto: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
