From: Ozgur Misman ([email protected])
Date: Wed Nov 22 2000 - 15:22:56 PST
Hi everybody,
I have a circuit that I use to design differential pairs. The circuit is based
on an optimization routine that minimizes the reflections ( S11) from a resistor
across the differential pair. Where the relections are zero or close to zero
the value of the resistor would be the differential impedance. Since we are in
the packaging business our trace widths are typically between 60 to 100 micron
range. A higher number would lead to routing inefficiency a lower number would
be very difficult to meet from manufacturing point of view in laminate based
packages.
Typically I set a target differential impedance and optimize the trace width and
spacing to meet target Zdiff. The simulation tool is Microwave design system.
I found out my optimum trace width and spacing greatly depends on the trace
thickness as well! I have been following the discussions very closely, and there
is no reference to trace thickness in the design of differential pairs!
One possibility is that the software might be using rectangular conductor cross
sections and therefore exagerates the effect of trace thickness. (We know a
trapezoid would be a better aproximation)!
Second possibilty is that since the aspect ratio is small in package traces as
opposed to PCB traces, the tighter coupling between the traces results in strong
dependence of Zdiff to trace height.
As an example a two layer stack up would be signal-ground with 100 micron
seperation and 75 micron trace spacing and width. ( Of course this is not 100
Ohms differential impedance)
Well, the physics supports the second option, however I am very interested in
hearing any opinions or perspectives on the importance of trace thickness in
Differential impedance calculations or simulations.
Thanks
Ozgur Misman
Sr. Engineer
Amkor Technology
"Ingraham, Andrew" <[email protected]> on 11/22/2000 02:46:37 PM
Please respond to "Ingraham, Andrew" <[email protected]>
To: "[email protected]"
<[email protected]>
cc:
Subject: RE: [SI-LIST] : Routing Differential Pairs as 100
differentially Vs individually 50 ohm lines
...
> Routing them close to each other produces interaction that reduces the
> final amplitude.
...
This "interaction" you speak of is the reduction in differential impedance
as the two lines are brought into one another's neighborhood. Simple
physics. You got reduced amplitude because your lines were less than 100
ohms differential, and if you didn't take that into account, you probably
mismatched the line's impedance.
Two widely separated 50 ohm lines give 100 ohm differential impedance.
Two less separated 60 ohm lines give 100 ohm differential impedance.
Two even less separated 70 ohm lines give 100 ohm differential impedance.
And so on.
What's different between these, is the common-mode impedance. Matching the
differential impedance is the first, and most important, step, but you often
want to look at how (or whether) you matched the pair's common-mode
impedance with the terminations at one or both ends, which affects
common-mode noise susceptibility.
There is nothing "wrong" about routing differential pairs close so they
"interact" with one another. After all, that's what a twisted pair cable
is. The wires are close to each other, producing interaction, and a lower
impedance than if the two wires were far apart.
Andy
**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected]. 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
[email protected]. 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 - 14:30:14 PDT