From: Mike Saunders (firstname.lastname@example.org)
Date: Mon Oct 09 2000 - 06:58:39 PDT
Here is my general rule of thumb (for detailed rules, see below). I usally
attempt to keep trace-to-trace spacing at 3x the distance to the nearest
plane (ie- 3 times the dielectric height) when routing on the same layer.
I also restrict the length of parallel travel to less than 2 inches. This
usually cuts the crosstalk coupling coefficient to below 5%.
For adjacent layers, the same rules apply. That is why you should
alternate horizontal routing with vertical routing on adjacent layers.
Then, coupling is virtually non-existent since there is no parallel travel.
So, on layers 3 and 7, route horizontally. On layers 4 and 8 route
As to your stackup, if possible you should substitute an additional ground
plane where you have two power planes together (layers 5 & 6). This can be
done by splitting the power plane and changing L5 to GND. Otherwise, try
to keep the highest speed signals off of layers 4 & 7 for cleaner power
Detailed crosstalk stuff:
The amount of crosstalk depends not only on the separation of traces from
each other, but also on rise times and length of parallel travel. The
nominal coupling coefficient, expressed as a percentage received of the
aggressor signal, is as follows:
K / (1 + (D/H)^2)
D is centerline-to-centerline trace spacing (NOT edge-to-edge).
H is the height above the reference plane.
K is a constant which depends on the rise time and length of coupling, and
is always < 1.
K is usually determined empirically by comparing the impressed voltage
waveform to the driven waveform, then accounting for the 1 / (1 + (D/H)^2 )
factor. For higher D/H ratios, the coupling coefficient is proportional to
~ 1/(D^2). This is why a 2X increase in spacing accounts for roughly a 4X
decrease in the coupling coefficient. Coupling coefficients less than 3%
are ideal for most digital systems. Some emperical data:
|| Trace Trace Spacing (edge-to-edge) / Measured Crosstalk (mV)
(Inches) 5 MILs 10 MILs 15 MILs 20 MILs 30MILs
0.25 47 22 17 10 7
0.5 150 90 55 37 18
2.0 520 300 190 128 65
3.0 580 340 210 143 80
6.0 580 430 280 205 110
10.0 620 550 420 300 170
At 08:42 AM 10/9/2000 +0200, you wrote:
>I am wondering if exist some equation stating the amount of crosstalk
>induced on a signal trace by another trace running on a different PCB
>In my specific case I am working on a PCB with the following layup:
>L1 --- signal
>L2 ------------- Plane (Gnd)
>L3 --- signal
>L4 --- signal
>L5 ------------- Plane (Power)
>L6 ------------- Plane (Power)
>L7 --- signal
>L8 --- signal
>L9 ------------- Plane (gnd)
>L10 --- signal
>I would like to have some hint in order to evaluate a "safe" thickness
>between L3 and L4 (L7 and L8 either) in order to have
>an acceptable crosstalk level between two lines running one underneath
>the other in such a layers.
>Thanks in advance.
>Flextel s.p.a. - C.so Vercelli 328 - Ivrea (To) Italy
>Tel : +039 -125 -235307
>**** To unsubscribe from si-list or si-list-digest: send e-mail to
>email@example.com. In the BODY of message put: UNSUBSCRIBE
>si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
>si-list archives are accessible at http://www.qsl.net/wb6tpu
**** To unsubscribe from si-list or si-list-digest: send e-mail to
firstname.lastname@example.org. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
This archive was generated by hypermail 2b29 : Tue May 08 2001 - 14:29:41 PDT