[SI-LIST] Re: Thick vs. thin diff. pairs
- From: Istvan Novak <istvan.novak@xxxxxxxxxxx>
- To: Mark_Burford@xxxxxxxxxxx
- Date: Sun, 26 Nov 2006 12:39:47 -0500
Mark and All,
Sorry for the late response, I was on the road...
In general, I am with Scott about using thin lines. The resistive
losses help to smooth out the transfer profile, which helps to
reduce data dependent jitter.
On the other hand, a narrower trace does not reduce the
dielectric loss or attenuation due to dielectric loss. The
dielectric loss term is the product of the radian frequency,
capacitance and loss tangent. Since capacitance is constant
for a given characteristic impedance in a given material,
C stays the same even if we use narrower traces (because
we need to make the dielectric layer proportionally thinner).
The same goes to the extra capacitance represented by the
corners; for a given material and characteristic impedance, it
does not depend on the trace width.
One parameter that carries significance is the trace separation.
Here the scaling works such that wider traces have a proportionally
bigger absolute separation to achieve the same coupling coefficient.
At bends and turns this translates to bigger skew.
Regarding microstrip versus stripline, I did see systems failing
with microstrip routing, whereas just putting the same routing
into stripline solved the problem. It depends on the size of
board, number and length of traces, skew and matching
conditions. A few short traces are usually not a concern.
Regards,
Istvan Novak
SUN Microsystems
Mark Burford wrote:
>Dear all,
>I would like to ask opinions, on the merits and disadvantages of using
>wide or narrow microstrip lines.
>
>>From where I am sitting it looks like narrow microstrip diff. pairs have
>it won hands down.
>
>
>
>Thick lines:
>
>More area...which gives more dielectric loss as dielectric loss over
>takes skin effect losses at higher frequencies.
>
>More S11 because any corner on the line will give a greater area and
>more capacitance.
>
>Thicker substrates to keep the impedance at the right value.
>
>As thicker microstrip lines go round a bend, the inter-pair skew will be
>more than for two narrow lines.
>
>There is also the possibility of increased EMI from thicker substrates
>(been reading antenna design books).
>
>
>
>So please someone tell me why should we use thicker lines? And also
>please could someone tell me the trip ups of HDI (high density
>interconnect) such as how small can one realistically go with back plane
>and inter-chip routing?
>
>
>
>Thanks
>
>Mark
>
>
>
>
>
>
------------------------------------------------------------------
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 FAQ wiki page is located at:
http://si-list.org/wiki/wiki.pl?Si-List_FAQ
List technical documents are available at:
http://www.si-list.org
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:
