[SI-LIST] Re: stripline return paths etc.

  • From: Larry SMITH <Larry.Smith@xxxxxxx>
  • To: Tony.Cosentino@xxxxxxxxxxx
  • Date: Mon, 06 Dec 2004 14:01:44 -0800

This is an interesting and important question.  The further away a split
plane is from a signal trace, the less effect it will have on the trace.
 The closest reference plane carries most of the return current, no
matter what voltage level it happens to be.

An accurate way to model a 50 Ohm microstrip transmission line is with a
pair of transmission lines in parallel: one T-line for the lower
reference plane and another T-line for the upper reference plane.  If
the 50 Ohm line happens to be exactly in the center of the two reference
planes, is represented by a two 100 Ohm T-lines in parallel.  The return
current on each of the 100 Ohm T-lines represents the return current
that is on the respective reference planes.  This is very useful if you
are trying to establish the amount of power plane bounce that will occur
at the ends of the transmission lines when the signal goes through a
via.  (If both reference planes happen to be ground and you stitch the
planes together with ground vias at each end of the T-line, there is no
plane bounce, which is the beauty of ground referenced signals.  Some
would recommend a decoupling capacitor if one of the reference planes is
power rather than ground, but it will not be very effective at GHz edge

If the stackup is asymmetric and the T-line is much closer to one
reference plane than the other, the same concept works, but the parallel
transmission lines are not 50 Ohms.  The plane closest to the T-line
might be associated with a 60 Ohm line and the far plane might be
associated with a 300 Ohm line, the parallel combination of which is 50
Ohms.  The 60 Ohm T-line carries 5x the current of the 300 Ohm line and
less than 20% of the return current is on the far reference plane.  A
discontinuity on the far plane will have some effect on the signal but
the further it is away the less effect it will have.

To quantify the results for your stackup, use an EM solver that will
allow 3 conductors and allow ground to be at infinity.  The solver
should give you 3x3 matrices for L and C for the signal, upper plane and
lower plane.  Find the mutual inductance and mutual capacitance from
the trace to each plane.  The impedance of the transmission line
associated with each plane is sqrt(L/C) for the appropriate mutual terms.

Larry Smith
Sun Microsystems

Cosentino, Tony wrote:
> Content-Type: text/plain;
>       charset="us-ascii"
> Content-Transfer-Encoding: quoted-printable
>  To all,=20
> This is a great question. I too would also like to know this answer. I
> have seen stackups that are an asymmetric stripline (Split Plane -
> Signal - Ground) where the signal (5mil trace) is 3.5 mils from the
> ground and 10 mils from the split plane. If the signal is considered
> high speed then does 100% of the return go to the closest ground plane
> or is a small percentage of the return going to the split plane? If not
> all of the return is to the ground plane then how do you quantify how
> much is not?
> Thanks
> Tony Cosentino
Bharathan, Jayapratap wrote:
> Hello all,
> I have this general question with me. (I'm a beginner)
> Suppose, if a High Frequency Signal Line is surrounded by a solid GND
> on one side and a SPLIT GND plane on the other side, & supposing that the
> solid GND plane is closer to the signal Line, the return path will be
> the solid GND plane, since the High Frequency Signal takes the path of
> inductance (a smaller loop).
> If this is the case, will it still matter if a high frequency signal Line
> has a split plane next to it?
> Thank you,
> -JP
> (Bharathan, Jayapratap)
> From: "steve weir" <weirsp@xxxxxxxxxx>
> To: <lalexman@xxxxxx>; <si-list@xxxxxxxxxxxxx>
> Sent: Monday, December 06, 2004 11:16 AM
> Subject: [SI-LIST] Re: stripline return paths etc.
>>Leonard, what you have with all the plane breaks is much more like a
>>microstrip.  The signal layer closer to the solid plane will exhibit
>>impedance than a true stripline, and some modulation along the frequency
>>axis.  The signal layer closer to the split planes could look like a mess
>>depending on several factors.  You should avoid placing signals with high
>>edge rates close to those splits.  If you must run signals across the
>>splits then bypass the splits with capacitors.
>>It is all in the inductance.  If you have a high inductance loop, between
>>the two grounds, then you are setting yourself up for a lot of
>>trouble.  You really need to ask yourself, or whoever came up with this
>>scheme what it is they are trying to do, and why those grounds need to be
>>single pointed.  You really ought to consider getting some expert help.
>>At 07:55 AM 12/6/2004 -0800, Leonard Alexman wrote:
>>>Hi All,
>>>I am designing many pcb's with multiple power and ground planes and I was
>>>curious if some has an opinion or could point me to any articles on the
>>>following questions.
>>>1.      I know its best to have a sold ground plane (or solid power
>>>plane )
>>>on either side of the a stripline trace but is it acceptable to have a
>>>ground plane on one side and a power plane on the other side with many
>>>splits in the plane ?  The same question for a dual stripline
>>>2.      I have some high speed differential signals that have a separate
>>>ground (HSGND). HSGND is tied to digital ground thru a zero ohm
>>>am routing these signals in a stripline configuration with HSGND
planes on
>>>either side. Can I also route digital signals(that use the digital
>>>ground )
>>>on this layer ? I am concerned that the return path goes thru the
zero ohm
>>>resistor to the digital ground plane. and it will be a very long return
>>>path. Is my assumption correct ?
>>>Thanks for any help
>>>Leonard Alexman / American Electronics Group Inc.

To unsubscribe from si-list:


For help:

List FAQ wiki page is located at:

List technical documents are available at:

List archives are viewable at:     
or at our remote archives:

Other related posts: