[SI-LIST] Re: Diff.Pairs

  • From: Scott McMorrow <scott@xxxxxxxxxxxxx>
  • To: silist <si-list@xxxxxxxxxxxxx>
  • Date: Sat, 11 Oct 2003 14:02:23 -0700

All,
I'd like to be very clear about several things regarding differential 
routing:

1) Differential signals can be transmitted over stongly coupled, weakly 
coupled or uncoupled conductors.  There is no magic here, just 
engineering tradeoffs.

2) Given a fixed dielectric thickness, a strongly coupled traces will 
have higher losses, which are due to the the decreased width of the 
conductor, and their increased proximity.  This causes approximately a 
20% increase in loss at a 3.125 Gbps signalling rate.  If you can 
tolerate this additional loss and you need increased routing density, by 
all means use closely spaced, narrow differential pairs.  In some cases 
a little loss is a very good thing.

3) Thus, there is a tradeoff.  High coupling with higher losses, but 
greatly increased routing density.  Or weak coupling with lower losses, 
and greatly reduced routing density.

4) Differential skew is important for signal quality.  Keep your skew 
between signals low through all elements in the system.  This means 
matching the electrical delay from the die of one device to the die of 
another device.  Things such as trace layer differences, via differences 
and connector path differences must be accounted for.

5) Rouing the two lines of a differential net on different layers is a 
very bad thing, and should not be done without  great consideration.  
Layer to layer differences in Er will cause worst case layer to layer 
delay differences in FR-4 of from 2.5 ps/in  (for good Er matching) to 4 
ps/inor 8 ps/in (for poor Er matching.)  If you route a trace any 
distance on two layers, be prepared for the worst  case possibility of  
a large skew and common mode converstion.

6) Routing the two lines of a differential net on different layers will 
also cause increased skew due to different via transitions. The two 
signal path lengths through the two vias will be different, and the 
further away the two layers are, the larger the skew difference will 
be.  For a 100 mil board thickness, this skew can be from between 20 and 
30 ps, depending upon the via size, the pad size and the antipad size.  
It will also be increased if unused pads are not removed. 

6a) The noise environment for a differential trace that is routed on two 
different layers as single ended nets is significantly different.  Each 
reference plane pair will have a different noise profile that will be 
independently injected into each single ended trace.  The difference 
between the two is common mode noise that flows on the composite pair.  
If these traces are always referenced to the same plane everywhere, then 
there will be minimal common mode radiation.  (There will however be 
some common mode radiation as there has to be for any conductor spaced 
from a reference plane.)  But, if there is a break in the return path at 
any point, or a serious discontinuity, there will be a large injection 
of common mode current into this region.  Do not be deceived.  A 
differential pair signal that travels through differential Vias causes 
very minor disruptions to the fields in a power/ground plane pair.  BUT 
if you decouple them, and route them as single ended traces in totally 
different areas of a board, you will see significant power injections 
into the planes.  Multigigabit energy will end up on all of your power 
and ground supplies and have the opportunity to radiate everywhere.  
That is why we transition differential pairs through vias that are 
closely spaced, so that the energy they inject cancels and does not 
spread through the planes.  If we do not do this, then the noise they 
inject does not cancel.  Lee misses this point big time.  It is a total 
bear to design a high frequency via transition for a single ended via, 
without loosing a substantial amount of the signal to the planes in the 
multiple GHz region.  A differential transition is much easier.

7a) Most people agree that a closely spaced differential pair will cross 
a plane split with relative ease and that it is a bad thing to have a 
single ended trace cross a plane split.  But, think of the the 
differential pair that crosses plane splits all day in every PCB when 
the signal flows through vias.  As we move the vias further and further 
apart, more and more energy will be released into the planes, until soon 
we are transitioning two uncorrelated single ended signals.  Now, a slow 
speed single ended signal switching at 400 MHz and with 200 ps rise 
times is a big enough of a problem when it passes through a single ended 
via.  But a high energy signal such as a 2.5, 3.125 or 10 Gbps signal 
with an edge rate of between 70 and 25 ps, will cause all hell to break 
loose on the planes.  There will be significant rise time degradation of 
the signal as it passes through a single ended via.  To demonstrate, I 
have placed a presentation on single ended vias that was based upon 
simulations I've done in the frequency domain with CST Microwave on the 
Teraspeed website.  You  can find it a http://www.teraspeed.com and then 
follow the links to the presentations.  You'll find that if there is not 
a ground (or a complementary differential pair via) close to a single 
ended via transition through a 0.063" board, you will lose a large 
amount of that signal in the inter-plane region. This manifests itself 
as high frequency noise on the planes and additional EMI.

For vias spaced larger than 150 mils away from a ground via (most signal 
vias), there is about -0.8 dB insertion loss at 3 GHz.  This is 
comparable to a an 8.8% reduction in the signal amplitude of a 100 ps 
edge.  At 7 GHz (50 ps rise time) there is a -1.5 dB loss (16% amplitude 
reduction.)  These may or may not be significant losses in a design, but 
are extremely significant to the noise and EMI profile of a board, since 
all of this energy is being injected into the planes where it is not 
well contained.  The implication for 2.5, 3.125 and 10 Gbps PCB designs 
is profound.  Decouple the differential vias and get ready for increased 
losses, increased noise and increased EMI.


Best regards,

scott

-- 
Scott McMorrow
(Who's been Getting it Right the First Time for many years.)
Teraspeed Consulting Group LLC
2926 SE Yamhill St.
Portland, OR 97214
(503) 239-5536
http://www.teraspeed.com



Craig Twardy wrote:

>Most characterization I have done at 2.5 Gbps has started with a Pattern
>Generator
>sourcing complementary signals (+ and -). Each complementary signal is
>connected
>through a coaxial cable to a SMA connectors mounted on the PCB.
>I use this as a good quality differential signal source.
>Pretty sure there is no coupling between the coaxial cables.
>As long as the coaxial cable lengths match this seems to work well.
>
>
>Craig
>
>
>
>
>-----Original Message-----
>From: Knighten, Jim L [mailto:JK100005@xxxxxxxxxxxxxxxx] 
>Sent: October 9, 2003 1:40 PM
>To: leeritchey@xxxxxxxxxxxxx; Doug Brooks; si-list@xxxxxxxxxxxxx
>Subject: [SI-LIST] Re: Diff.Pairs
>
>
>Lee,
>
>Your post is interesting!
>
>Differential signaling is usually implemented with coupled transmission
>lines.  The mutual coupling between the traces affect the two modes that are
>always present (even and odd modes). In the traditional configuration, the
>two traces are parallel and of the same width and thickness and located
>adjacent to a plane.  The degree of coupling between the traces is usually
>described as "loosely coupled" or "tightly coupled."  In either case, if the
>signal and signal traces are perfectly differential (i.e., no imbalance,
>perfectly symmetrical), then there is always current in the adjacent ground
>plane, but the net current in the longitudinal direction (the direction of
>the traces) is zero.  The currents that exist in the adjacent plane are
>circulating currents that reflect the distributed coupling between the
>traces down the length of the transmission line.
>
>So, what if the two coupled traces are not co-planar, i.e., not in the same
>plane?  Well, you still have two coupled transmission lines, but the mutual
>capacitance and inductance between them may be different than if they were
>co-planar, hence the even and odd mode impedances may be different.  These
>non-co-planar coupled lines can still carry differential signals, though.  
>
>What if the two coupled lines were not co-planar and actually had the ground
>plane between them?  This is just a special case of the "loosely coupled"
>case, in that the lines are now not coupled at all.  Still, the lines can
>support differential signaling, but the relationships between even and odd
>modes are not quite the same as when they were coupled. (Perhaps even mode
>and odd mode impedances are equal?)
>
>So, how about current in the ground plane?  For perfect differential
>signaling, the net current in the plane is zero.  When you introduce
>imbalance, either in the signal source, or in the signal path, you create
>net longitudinal current in the ground plane.  This is the even mode signal,
>which has no bearing on your intended differential signal (the odd mode) and
>represents an EMI source on the ground plane.  
>
>If you route differential signals on different layers, it may be more
>difficult to maintain balance (symmetry) in the traces than if the traces
>were co-planar.  If this is true, you have more potential for EMI issues.
>
>...My thoughts
>
>Jim
>
>________________________
>James L. Knighten, Ph.D.
>Teradata, a division of NCR                 http://www.ncr.com
>17095 Via del Campo
>San Diego, CA 92127
>tel: 858-485-2537
>fax: 858-485-3788
>
>
>-----Original Message-----
>From: Lee Ritchey [mailto:leeritchey@xxxxxxxxxxxxx] 
>Sent: Thursday, October 09, 2003 9:30 AM
>To: Doug Brooks; si-list@xxxxxxxxxxxxx
>Subject: [SI-LIST] Re: Diff.Pairs
>
>If this discussion is about differential pairs travelling over the planes of
>a PCB, the return current for each member of the pair travels on the plane
>over which it travels, not on the other wire.  If they are very tightly
>coupled to each other, perhaps 5% of the current from one travels in the
>other.  It is coincidental that the two currents are equal in magnitude and
>opposite.  They don't have to be.  Their "return currents" still travel on
>the plane, not on the other wire.
>
>As far as EMI is concerned, it has been demonstrated many times, once in the
>paper done by Doug Brooks with the staff at UMR, that traces traveling over
>planes are not a detectable source of EMI.  Therefore, constraining the
>routing of differential pairs to prevent them from creating EMI is not
>appropriate or necessary.
>
>It is still true that the two members of a differential pair are two
>independent signals traveling on two independent transmission lines. All
>they have in common is that the have equal amplitudes and are 180 degrees
>out of phase with each other.  If the protocol is LVDS, each member of the
>pair should be parallel terminated in an impedance equal to Zo for that line
>to Vref (about 1.25V) which is half way between the two logic levels.
>
>As long as the two signals switch at the same time, the current flowing out
>of Vref into one line is the same magnitude an opposite in polarity to that
>flowing into the other.  The net current into and out of the Vref terminal
>is zero, so we can omit the connection.  When we do this, we have two
>resistors, each of value Zo across the ends of the two transmission lines. 
>For convenience, we use one resistor of value 2 X Zo.  This is not a
>differential impedance of 100 ohms, but two parallel terminations of value
>Zo terminating two transmission lines each of impedance Zo.
>
>As long as the two edges switch at the same time, there is no current
>imbalance and all is well.  Soon as one edge switches before the other,
>there is a need for a momentary current spike to flow into or out of the
>Vref terminal.  If there is no connection to Vref for the current flow, the
>result is the edges are degraded.  To avoid this degradation, a very small
>capacitor is often connected between the two resistors and ground.  This is
>a very common termination for 2.4 GB/S signal links. 
>
>It is time to stop representing differential signals as needing to be
>tightly coupled to each other in order to operate properly.  It is simply
>not so.  I have routed thousands of differential signal where each member of
>the pair is on a different layer.  If this were not possible, 1 mm pitch
>BGAs with differential signals would be un routable.  There are tens of
>thousands of such parts being shipped every month on PCBs where they are
>routed apart from each other.
>
>This is all described in my recently published book, "Right the First Time,
>A Practical Handbook on High Speed PCB and System Design".  It is also
>covered in Howard Johnson's new book whose title escapes me at the moment..
>
>Lee
>
>
>  
>
>>[Original Message]
>>From: Doug Brooks <doug@xxxxxxxxxx>
>>To: <si-list@xxxxxxxxxxxxx>
>>Date: 10/3/2003 1:02:25 PM
>>Subject: [SI-LIST] Re: Diff.Pairs
>>
>>Tight may be a relative word. But a differential pair constitutes a
>>    
>>
>"loop" 
>  
>
>>in EMI terms. That is, the loop is the area encompassed by the signal 
>>and
>>its return. Smaller loop areas perform better than larger loop areas when 
>>EMI is a concern. The closer the differential pair, the smaller is the 
>>loop. If we are NOT concerned about EMI, then this is not an issue. If we 
>>ARE, then we might want to pay attention to this and keep the loop small
>>    
>>
>by 
>  
>
>>routing the traces close together.
>>
>>The equal spacing "requirement" comes from the control of reflections 
>>(ie
>>transmission line termination issues.) IF we are concerned about 
>>reflections, THEN we need a constant impedance everywhere along the
>>    
>>
>trace. 
>  
>
>>IF the (differential) traces are close together (for EMI reasons) THEN
>>    
>>
>they 
>  
>
>>will interact (a very special case of crosstalk, which in this 
>>particular
>>case [signals --- being equal and opposite --- are exactly correlated
>>    
>>
>with 
>  
>
>>each other] is not a problem.) IF we want to keep a constant impedance
>>along the traces, THEN we must keep a "constant" spacing between them, 
>>because the coupling between them, and therefore the differential 
>>impedance, will vary if we don't.
>>
>>There is a further design rule you sometimes hear, that being that the
>>differential traces must be equal length. This is NOT for timing reasons, 
>>but for common mode reasons. A strong assumption we make about
>>    
>>
>differential 
>  
>
>>signals is that they are equal and opposite, and therefore there is no
>>return signal through the ground system. Even if the signals are perfect, 
>>if the traces are different length, then the signal will not arrive at
>>    
>>
>the 
>  
>
>>far end at exactly the same time and the signals will not be "equal 
>>and
>>opposite" at the receiver. Just a couple of degrees phase shift can make
>>    
>>
>a 
>  
>
>>surprising difference between the signals when we are talking about
>>(square-wave) clock signals. If the signals are not exactly equal and 
>>opposite, then there MUST be a net current flowing somewhere else. This 
>>will quite likely be a common mode noise current that might cause an EMI
>>    
>>
>issue.
>  
>
>>None of the differential signal trace design rules are necessary taken 
>>by
>>themselves. This is important to recognize. But if are concerned about 
>>certain SI issues, they might lead to some design considerations which
>>    
>>
>THEN 
>  
>
>>might cascade (like a domino effect) into other areas.
>>
>>This is in my book, too...............
>>
>>Doug Brooks
>>
>>
>>
>>
>>At 11:41 AM 10/3/2003 -0700, Lee Ritchey wrote:
>>    
>>
>>>More than that, it does not have any benefit.  Tight coupling of 
>>>differential pairs forces the traces to be narrower increasing the 
>>>skin effect losses.  Also, this tight coupling is going to result in 
>>>good old cross talk that actually degrades the edges.
>>>
>>>How the notion of tight coupling of differential pairs as beneficial 
>>>got started is a mystery to me.  There are several references that 
>>>show that tight coupling is not beneficial, one of them is Howard 
>>>Johnson's latest book, at least one column he has written and my 
>>>recently released book.
>>>
>>>Lee Ritchey
>>>
>>>
>>>      
>>>
>>>>[Original Message]
>>>>From: Duane Takahashi <duanet@xxxxxxxxxxxxxxxxxxxxxx>
>>>>To: <si-list@xxxxxxxxxxxxx>
>>>>Date: 10/2/2003 3:58:59 PM
>>>>Subject: [SI-LIST] Re: Diff.Pairs
>>>>
>>>>Hi Juergen:
>>>>
>>>>Aligning the stack up for the broadside coupled diff lines is
>>>>        
>>>>
>expensive.
>  
>
>>>>   You can do this, but it drives up the cost of the board.
>>>>
>>>>Duane
>>>>
>>>>        
>>>>
>>>>>Hi Juergen,
>>>>>You can find lots of  application notes
>>>>>especially with respect to process variation
>>>>>on differential pairs here:
>>>>>
>>>>>
>>>>>www.polarinstruments.com/support/cits/cits_index.html
>>>>>
>>>>>In particular this one may be of interest:
>>>>>
>>>>>
>>>>>How measured impedance may vary from field solver calculations 
>>>>>when using woven glass reinforced 
>>>>><http://www.polarinstruments.com/support/cits/AP139.html>laminat
>>>>>es
>>>>>
>>>>>www.polarinstruments.com/support/cits/AP139.html
>>>>>
>>>>>
>>>>>And this note:
>>>>>
>>>>>Copper thickness, edge coupled lines and
>>>>>characteristic 
>>>>><http://www.polarinstruments.com/support/cits/AP151.html>impedan
>>>>>ce
>>>>>
>>>>>
>>>>>www.polarinstruments.com/support/cits/AP151.html
>>>>>
>>>>>
>>>>>
>>>>>Hope this helps....
>>>>>
>>>>>
>>>>>Kind regards
>>>>>Martyn Gaudion
>>>>>www.polarinstruments.com
>>>>>T: +44 1481 253081
>>>>>F: +44 1481 252476
>>>>>M: +44 7710 522748
>>>>>E: martyn@xxxxxxxxxxxxxxxxxxxx
>>>>>
>>>>>============================================
>>>>>  Controlled Impedance & Signal integrity tools
>>>>>  for the Printed circuit fabrication industry 
>>>>>============================================
>>>>>
>>>>>
>>>>>
>>>>>
>>>>>
>>>>>
>>>>>At 19:00 02/10/2003, you wrote:
>>>>>
>>>>>          
>>>>>
>>>>>>I am seeking help in finding enlightenment regarding electrical 
>>>>>>performance pros and cons and how manufacturing tolerances play 
>>>>>>a
>>>>>>            
>>>>>>
>role
>  
>
>>>>>>when comparing side by side and tandem differential pairs. I'd
>>>>>>            
>>>>>>
>>>appreciate
>>>      
>>>
>>>>>>your opinion, experience, analysis, pointers to papers and 
>>>>>>articels,
>>>>>>            
>>>>>>
>>>etc.
>>>      
>>>
>>>>>>In return, I would offer to share a summary of the
>>>>>>            
>>>>>>
>finding/discoveries
>  
>
>>>>>>with interested parties.
>>>>>>
>>>>>>Thanks
>>>>>>
>>>>>>Juergen
>>>>>>
>>>>>>
>>>>>>
>>>>>>----------------------------------------------------------------
>>>>>>--
>>>>>>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: 
>>>>>>//www.freelists.org/webpage/si-list
>>>>>>
>>>>>>For help:
>>>>>>si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>>>>>>
>>>>>>List archives are viewable at:
>>>>>>               //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: 
>>>>>//www.freelists.org/webpage/si-list
>>>>>
>>>>>For help:
>>>>>si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>>>>>
>>>>>List archives are viewable at:
>>>>>            //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
>>>>>
>>>>>          
>>>>>
>>>>--
>>>>Duane Takahashi              phone: 408-720-4200
>>>>Greenfield Networks            fax: 408-720-4210
>>>>255 Santa Ana Court          email: duanet@xxxxxxxxxxxxxxxxxxxxxx
>>>>Sunnyvale, CA 94085
>>>>
>>>>* MOVING!  Please note new numbers and address *
>>>>
>>>>------------------------------------------------------------------
>>>>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: 
>>>>//www.freelists.org/webpage/si-list
>>>>
>>>>For help:
>>>>si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>>>>
>>>>List archives are viewable at:
>>>>              //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: 
>>>//www.freelists.org/webpage/si-list
>>>
>>>For help:
>>>si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>>>
>>>List archives are viewable at:
>>>                //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
>>>
>>>      
>>>
>>Doug Brooks' new book, "Signal Integrity Issues and Printed Circuit 
>>Board
>>Design" has just been released by Prentice Hall. See details and ordering 
>>info at www.ultracad.com
>>
>>    
>>
>____________________________________________________________________________
>__
>  
>
>>------------------------------------------------------------------
>>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: 
>>//www.freelists.org/webpage/si-list
>>
>>For help:
>>si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>>
>>List archives are viewable at:     
>>              //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:
>//www.freelists.org/webpage/si-list
>
>For help:
>si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>
>List archives are viewable at:     
>               //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:
>//www.freelists.org/webpage/si-list
>
>For help:
>si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>
>List archives are viewable at:     
>               //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:
>//www.freelists.org/webpage/si-list
>
>For help:
>si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>
>List archives are viewable at:     
>               //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:
//www.freelists.org/webpage/si-list

For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field

List archives are viewable at:     
                //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: