FPGA Central

Hello Daniel,
as a rough rule of thumb for 50 Ohm microstrip lines, once the wide trace
(return trace / plane) extends about 2 line widths beyond the signal
trace, the influence of further widening is negligible with respect to
characteristic impedance. That's because for typical PCB dimensions at
already at very low frequencies (low MHz) most of the return current is
already flowing in a narrow band directly below the signal trace. For
frequencies below that the trace impedance is usually unimportant because
the trace is many orders of magnitude shorter than the signal wavelength
(1 MHz corresponds to a wavelength of approx. 200m on a stripline of FR-4
dielectric).

For quantitative results it is easy to simulate the effect of the line
width with a 2D field solver. I'd recommend TNT/MMTL (google for "TNT
field solver"), freely available from sourceforge. Model the wide trace
and the short trace as rectangular conductors, and make sure they are far
enough away from the (infinitely wide) ground plane. Define the wide trace
as gounded (start its name with "gr", not just "g" as the manual says).
TNT will directly report the impedance of the narrow trace.

I made a quick run; surface microstrip line, narrow trace width 20 mils,
spacing to wide trace 10 mils, eps_r = 4:, trace thickness 1 mil for both
traces

wide trace 200 mils --> Zo = 46.3 Ohms
wide trace 100 mils --> Zo = 46.5 Ohms
wide trace 60 mils --> Zo = 46.9 Ohms
wide trace 40 mils --> Zo = 47.7 Ohms
wide trace 20 mils --> Zo = 54.4 Ohms


Wolfgang






Daniel Bauer <daniel.bauer16 (AT) web (DOT) de>
Sent by: si-list-bounce (AT) freelists (DOT) org
02/25/2009 12:27 PM

To
si-list (AT) freelists (DOT) org
cc

Subject
[SI-LIST] trace width working as a plane






Hello,

could you tell me if there`s an rule of thumb at which width of the trace,
the trace is working as a plane depending on the signal frequency?

For example: the width of the trace for a signal-frequency 500kHz must be
0.15mm to get a 100 ohm impedance. If the width of the trace gets bigger,
the impedance gets smaller -> you will get more radiation (no exact
impedance matching).

But what will happen when the width of the trace gets more and more
bigger....? At which point will the "trace width" work as plane and how
do I have to calculate the correct impedance of this plane (microstrip
calculator do not work with such width of trace)? Are there any kind of
formulas?

best regards
Daniel

__________________________________________________ __________________
Psssst! Schon vom neuen WEB.DE MultiMessenger gehört?
Der kann`s mit allen: http://www.produkte.web.de/messenger/?did123

------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request (AT) freelists (DOT) org with 'unsubscribe' in the Subject field

or to administer your membership from a web page, go to:
http://www.freelists.org/webpage/si-list

For help:
si-list-request (AT) freelists (DOT) org with 'help' in the Subject field


List technical documents are available at:
http://www.si-list.net

List archives are viewable at:
http://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




------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request (AT) freelists (DOT) org with 'unsubscribe' in the Subject field

or to administer your membership from a web page, go to:
http://www.freelists.org/webpage/si-list

For help:
si-list-request (AT) freelists (DOT) org with 'help' in the Subject field


List technical documents are available at:
http://www.si-list.net

List archives are viewable at:
http://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