[SI-LIST] Re: Reasons for the steep falloff in the observed S21 Profile for Microstrip Traces.

Ravindra-

The effect you are seeing of resonances in the S21 of loosely coupled
microstrip lines and not in similar loosely coupled striplines is due to the
difference in speed of common signals and differential signals in microstrip
and the fact you are launching single ended signals. 

If you look at S21, you will see a dip at certain frequencies. If you plot
S41 on top of S21, you will see peaks in the "far end noise" when S21 dips.
Energy is coupling back and forth between the two lines, as the signal
propagates. The length to get the full coupling from one line to the other
line depends on the difference in speed between the diff and common signals,
and the phase difference between the common and diff signals. 

When there is no coupling, the diff and common speeds are the same, and you
see no energy flow from line to line. As you increase the coupling in
microstrip, the distance for the signal to travel before the phase between
the comm. and diff signal to be 180 degrees shifted is less. The tighter the
coupling, the lower the frequency for the first resonance and each following
resonance.

It is like the coupling of motion between two loosely coupled swings. The
tighter the coupling, the shorter the  time for the motion of one swing
couple to the other, and back again.

When you launch a 1 v signal into line 1 and a 0 v signal in line 2, you are
really launching a combination differential and common signal in the pair.
In coupled microstrip, the diff and comm. signal travel at slightly
different speeds. The tighter the coupling, the bigger the difference in
speed. 

When the length and frequency of the path corresponds to a 1/2 wavelength
difference between the diff and comm. signal, the net signal on line 1 will
cancel out and the voltage on the two lines will appear to be opposite- 0v
on line 1 and 1v on line 2. When the phase between the diff and comm. signal
is again 180 deg shifted, the voltage pattern at the far end will be back to
1v and 0v. 

Do not think of this as a "problem" unless you intend to use the lines as
single ended, in which case the problem you will have is far end cross talk,
long before the resonances. If you send in a pure diff signal, you have no
comm. component, and the diff signal will propagate just fine. 

This effect is exactly why there is far end noise in microstrip, but not in
stripline, or with loosely coupled microstrip. As you point out, if you
embed the microstrip, the diff and comm. signals will have nearly the same
speed and this effect will disappear.

If you want more details, I describe this effect in my book, Signal
Integrity Simplified, and in some of my on-line lectures on interpreting TDR
responses in coupled lines. It is also one of the puzzles I offer in my
class on Signal Integrity Characterization techniques, which I am presenting
in Dallas on March 5-6.

Hope this helps.

--eric

**************************************
Dr. Eric Bogatin, President
Bogatin Enterprises, LLC
Setting the Standard for Signal Integrity Training
26235 w 110th terr
Olathe, KS 66061
v: 913-393-1305
f: 913-393-0929
c:913-424-4333
e:eric@xxxxxxxxxxxxxxx
www.BeTheSignal.com 

Spring 2008 Signal Integrity Training Institute
EPSI, SIAA, BBDP
April 7-11, 2008, San Jose, CA
**************************************** 

-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] On
Behalf Of Ravindra Gali
Sent: Monday, January 14, 2008 5:57 PM
To: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Reasons for the steep falloff in the observed S21 Profile
for Microstrip Traces.

Hello Experts,
 

I need some help in interpreting the measurement results that I am
observing on a test structures board.  The stackup for the test board is
as follows:

 

Signal                 ---------------------- Layer One

Nelco - 13 

Ref. Plane           ---------------------- Layer Two

Signal                 ---------------------- Layer Three

Ref. Plane           ---------------------- Layer Four

Core/Pre-preg

Ref. Plane           ---------------------- Layer Five

Nelco - 6 

Signal                 ---------------------- Layer Six

Nelco - 13           

Ref. Plane          ----------------------- Layer Seven

Rogers 4350

Signal                ----------------------- Layer Eight 

 

Total Board Thickness - 85 mils

All the SMAs are located only on the top layer of the board. 

 

On each of the signal layers (Layer 1, 3, 6, 8), I have 2 differential
pairs (25", 40") along with other test structures. The traces are routed
in a loosely coupled fashion to hit 100 ohm differential impedance. I
have taken the TDR measurements and they are meeting the impedance
specification within a 10% tolerance. The traces are routed with wide
trace widths to minimize conductor losses. The signal vias are back
drilled on layer 3 & 6 to remove the stubs.  I have done a four port VNA
measurement (single ended) on the same traces and the insertion loss
results (S21, S12, S34, S43) do not make sense to me. I would like to
understand as to what is the cause of this behavior

 

a)       The insertion loss profile for the stripline traces is as
expected

a)       Loss increases as a function of frequency & length. 

b)       S21 profile for Layer 3 is better than Layer 6

 

b)       The insertion loss profile for the microstrip traces show some
kind of resonance behavior. 

a)       There is a steep falloff in the S21 profile for the 40"
microstrip trace on layer one at frequency less than 2GHz (1.9GHz). I
see another steep falloff at 6GHz

b)       There is a steep falloff in the S21 profile for the 40"
microstrip trace on layer eight at frequency less than 2GHz (1.74GHz). I
see another steep falloff at 4.78GHz.

c)       The profile for 25" trace is similar to the 40" trace though
the frequency at which the falloff happens is different. In both the
cases the trace on layer one behaves slightly better than layer eight.

 

I was hoping to see the best S21 profile for the differential pair on
layer 8 followed by the diff pair on layer 1, layer 3 and layer 6
respectively.

 

 

My question to the group is as follows:

 

Why are the microstrip traces seeing a huge falloff in the S21 profile
at specific frequencies?

Is this an expected behavior for all the traces routed as microstrip?

Is this behavior due to the difference in wave propagation due to
non-homogenous system (Air/dielectric) material?

            If we route the diff. pair as an embedded microstrip instead
of a true microstrip (air/dielectric), can we avoid this issue?

 

I would really appreciate all your inputs on this issue.

 

 

Thanks,

Ravi.

 



Confidentiality Notice.  This message may contain information that is
confidential or otherwise protected from disclosure.
If you are not the intended recipient, you are hereby notified that any use,
disclosure, dissemination, distribution, 
or copying of this message, or any attachments, is strictly prohibited.  If
you have received this message in error, 
please advise the sender by reply e-mail, and delete the message and any
attachments.  Thank you.



------------------------------------------------------------------
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:
http://www.freelists.org/webpage/si-list

For help:
si-list-request@xxxxxxxxxxxxx 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@xxxxxxxxxxxxx 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@xxxxxxxxxxxxx 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
  

Other related posts: