[SI-LIST] Re: Return path for stripline between two power planes
- From: steve weir <weirsi@xxxxxxxxxx>
- To: Joel Brown <joel@xxxxxxxxxx>
- Date: Tue, 18 Apr 2006 08:37:39 -0700
Joel, this is another "depends" situation. The way that I suggest to
look at this is to start with the driver and follow the transmission
path from the silicon through its package and to the PCB. If that
path is couples equally to Vcc and Vss, then continuing that
structure through the PCB introduces the minimum disturbance to the
transmission path. But, in systems that often have several to many
voltages, that is a bit impractical. From a standpoint of signal
propagation we are concerned with:
1) The impedance continuity of the path. A terminated nonvarying
impedance from driver to destination means that we won't have to
contend with reflections.
2) Reference at the destination.
Tight coupling between Vdd and Vss at the driver allows the driver
output to reference either rail or a combination going through the
package. When the signal gets out of the package we need to get it
into the wave guide we are using. If part or all of the signal
energy is imaged against Vdd and we want to use Vss, then we need
tight coupling on the board near the package between those two. The
same goes for the reverse situation. Once the signal launches down
our wave guide, as long as we maintain a constant impedance, it
continues on its merry way and doesn't care what is behind it. At
the far end of the line we have a voltage difference between the
metal that defines our signal trace and our image plane. If the
image plane is the same as the reference used by the IC, we are all
set. If the IC references something else, then once again we need to
couple between the image plane and now the receiver IC's reference
voltage rail close to the IC. Voila! We have a signaling path.
I have some decent graphics on this in my 2005 SVCEMC
presentation. You can get it from either the Teraspeed or the X2Y
web sites: www.teraspeed.com, www.x2y.com
Steve.
At 08:06 AM 4/18/2006, Joel Brown wrote:
>I have a question somewhat related to this.
>When using a stripline configuration, I always thought it was better
>to have ground planes on both sides of the signal layer and not
>Ground for one layer and VCC for the other layer. But then after
>reading an article by Howard Johnson on return currents, my thinking
>is that it does not matter if you use ground or VCC for the planes.
>This is because when an output driver switches low, the return
>current would prefer to flow on a ground plane. When an output
>driver switches high the return would prefer to flow on a VCC plane
>and if both planes are ground, the return current will end up
>flowing through a bypass cap or parasitic board capacitance to
>return to VCC. Is this thinking correct? The important thing is to
>have right bypass caps in the right locations to minimize the return
>current path.
>
>Thanks - Joel
>
>
>steve weir wrote:
>>Don, I am sorry, but I don't see the cause for your concern.
>>
>>The first and foremost issue is that George states that he is not
>>carrying daughter card PECL Vdd in this midplane. He has the task
>>of coupling PECL Vdd adequately to GND on each daughtercard across
>>the signal bandwidth. For 2GHz signaling that is hardly an
>>insurmountable task. Once he meets that burden, the rest of this
>>should perform very well. All signals traversing this midplane
>>reference GNDx. Layer 2 and 4 can pair as can 11 and 13 for
>>nearly seamless layer switches across the two sides of layer 3 and
>>layer 12 respectively. To my thinking, the via stubs will
>>contribute far more S11 reflection than layer switches done that
>>way. This should perform very nicely. His low speed logic relies
>>on stitching in parallel with displacement current from layer 6 -
>>9. Low speed stuff shouldn't have any problem with that.
>>
>>
>>Steve.
>>
>>
>>At 05:23 AM 4/18/2006, Faraydon Pakbaz wrote:
>>
>>>Steve;
>>>
>>>Your stack up suggestion will create different "Characteristic impedance"
>>>for signals that use VCC1 to power up and GND1 for return current as
>>>compared
>>>to the signals that power up from VCC1 and using GND2 for return. This
>>>would be
>>>due to different separation between power and ground. Since S1 and S2 are
>>>2.125 G PECL it may matter? Of course board decaps can be used to adjust.
>>>Is my understanding correct? Thanks.
>>>
>>>Regards;
>>>
>>>Don Pakbaz
>>>
>>>Silicon Solutions Engineering
>>>IBM Systems & Technology Group
>>>Email: pakbazf@xxxxxxxxxx
>>>Voice: (802) 769-5638 Tieline: 446-5638 Fax: (802) 769-5722
>>>
>>>
>>>
>>> steve weir
>>> <weirsi@xxxxxxxxx
>>> m> To
>>> Sent by: "Kidman Ma" <ma.kidman@xxxxxxxxx>
>>> si-list-bounce@fr cc
>>> eelists.org si-list@xxxxxxxxxxxxx
>>> Subject
>>> [SI-LIST] Re: Return path for
>>> 04/18/2006 04:27 stripline between two power planes
>>> AM
>>>
>>>
>>> Please respond to
>>> weirsi@xxxxxxxxxx
>>>
>>>
>>>
>>>
>>>
>>>
>>>George, I would definitely alter the stack-up of this system.
>>>I recommend looking carefully at a stack up more like this:
>>>
>>>-1 Top
>>>-2 S1
>>>-3 GND1
>>>-4 S2
>>>-5 L_In1
>>>-6 GND2
>>>-7 VCC1
>>>-8 VCC2
>>>-9 GND3
>>>10 L_In2
>>>11 S3
>>>12 GND4
>>>13 S4
>>>14 Bottom
>>>
>>>You will still have to figure out how to adequately couple the PECL
>>>Vcc to GND on each of the daughter cards. At 2GHz that should not be
>>>too hard to manage.
>>>
>>>Steve.
>>>
>>>
>>>sss
>>>At 12:35 AM 4/18/2006, Kidman Ma wrote:
>>>
>>>>Hi Steve,
>>>>
>>>>Yes, You're right. The stack up i posted before is part of the
>>>>following 14 layer stackup.
>>>>--------Top
>>>>--------GND1
>>>>--------L_In1 (Low speed signal <50MHz)
>>>>--------L_In2 (Low speed signal <50MHz)
>>>>--------VCC1 (continuous +5v plane)
>>>>--------S1 [2.125G PECL, 8mil to VCC1, 6mil to VCC2]
>>>>--------VCC2 (continuous +12v plane)
>>>>--------S2 [2.125G PECL]
>>>>--------GND2
>>>>--------S3 [2.125G PECL]
>>>>--------GND3
>>>>--------S4 [2.125G PECL]
>>>>--------GND4
>>>>--------Bottem
>>>>
>>>>This board is one midplane of system, no active data path component
>>>>on it. No PECL VCC, either. All driver and receiver is routed on
>>>>other "daughter card". No layer switching (no vias) over S1, except
>>>>the connectors to other active cards.
>>>>
>>>>Do you think it's better if I switch +5v plane to VCC2? That means,
>>>>let S1 reference to +5v power plane through 6mils gap.
>>>>
>>>>Regards,
>>>>George
>>>>On 4/17/06, steve weir <<mailto:weirsi@xxxxxxxxxx>weirsi@xxxxxxxxxx>
>>>>
>>>wrote:
>>>
>>>>George,
>>>>
>>>>This is primarily a common mode issue. I assume that the five layers
>>>>shown represent only part of your stack-up. Is VCC2 your PECL
>>>>Vcc? If not, how about moving the PECL Vcc to layer 3and adjusting
>>>>your dielectric spacing:
>>>>
>>>>Vxxx or Gnd
>>>>big gap
>>>>S1
>>>>little gap
>>>>PECL VCC
>>>>little gap
>>>>S2
>>>>big gap
>>>>Vxxx or Gnd
>>>>
>>>>First, there is nothing magic about "Gnd". To quote Dr.
>>>>Archambeault, ground is a place for potatoes and carrots. We are
>>>>concerned about wave guides, which means the return image path and
>>>>common mode reference voltage. If the same Vcc is used at both the
>>>>transmitter and receiver for PECL outputs and inputs, that is the
>>>>best but not only choice for the image return plane(s).
>>>>
>>>>The hierarchy of return paths from most desirable to least is:
>>>>
>>>>1) Single surface that matches the source and destination reference
>>>>
>>>voltage.
>>>
>>>>2) Two surfaces of a single sheet that match the source and
>>>>destination reference voltage
>>>>
>>>>3) Multiple surfaces tied together by stitch vias that match the
>>>>source and destination reference voltage.
>>>>
>>>>4) Single surface that does not match the source and destination
>>>>reference voltage
>>>>
>>>>5) Two surfaces of a single sheet that does not match the source and
>>>>destination reference voltage
>>>>
>>>>6) Multiple surfaces tied together by stitch vias that do not match
>>>>the source and destination reference voltage.
>>>>
>>>>7) Surfaces coupled together by interplane and bypass capacitors
>>>>
>>>>The reason for the hierarchy is uncertainty. 1 is the ideal. 2 is a
>>>>very close second. 3 can be a little or a lot worse. 4-7 all rely
>>>>on capacitive coupling through cavity dielectric and bypass
>>>>capacitors. At 3GHz, a bypass capacitor with 1nH mounted inductance
>>>>looks like 20 Ohms. To the 100ps rising edge of a 3GHz serdes,
>>>>anything further than about 0.3" away from any given signal
>>>>transition through the PCB cavity does not reflect back in time to
>>>>impact an incident edge. That means a bypass cap 0.3" away is all
>>>>but pointless for the incident edge. Suppressing resonances, is a
>>>>different issue. That radius increases inversely with the spectral
>>>>components. For the 2.4nS long worst case runs in 8b10b that radius
>>>>of action likely includes most of your board. Plane geometries,
>>>>stitch via patterns, and to a smaller extent bypass capacitor loading
>>>>will determine the location and magnitude of resonances. What you
>>>>pass through the cavities particularly in terms of single ended
>>>>busses determines excitation.
>>>>
>>>>If you make layer 3 your PECL Vcc it looks like you have #2 in the
>>>>bag. If you want to go another route, you have some homework to
>>>>do. Essentially, you need to determine what the impedance profile
>>>>looks like plane to plane in each of those cavities and the signal
>>>>spectra of what you will be injecting into the cavity(s) in
>>>>question. If you can tolerate both the losses that you will get for
>>>>the diff pairs going through, and the increased EMI and crosstalk
>>>>that will result from ALL of the signals you pass through those
>>>>cavities, then all is well. If you have few or no single ended
>>>>signals traversing the cavities, then there won't be that much to
>>>>mess with your diff signal common mode. Similarly, if you can get
>>>>the coupling impedance low enough between planes across your signal
>>>>spectra to tolerate whatever it is you do inject, then even 7) still
>>>>works. But, you need to figure out where you are with your signals
>>>>and those cavities first. Lee attests that he has made 7) work on
>>>>hundreds of boards. In the end, it all comes down to coefficients.
>>>>
>>>>Doug Smith's most recent "Technical Tidbit" is quite germane, and
>>>>should open your eyes to some of the differences between 1) and
>>>>7). Just appreciate that on Doug's test board, there are fewer
>>>>layers than your board, no ground stitch vias and no bypass
>>>>capacitors, all of which affect the results. Also appreciate that
>>>>what he tested is susceptibility / radiation. A different test on a
>>>>different configuration will yield different results.
>>>>
>>>>Additional resources include a study done by Scott McMorrow on our
>>>>website <http://www.teraspeed.com>www.teraspeed.com, and a number of
>>>>papers by Dr. Bruce Archambeault.
>>>>
>>>>Steve.
>>>>At 01:51 AM 4/17/2006, geor_dai wrote:
>>>>
>>>>>Dear All SI experts,
>>>>>
>>>>>One question regarding to return path for signals and signal quality
>>>>>concerns.
>>>>>
>>>>>If we have stripline configuration as below, a signal trace S1 between
>>>>>two power planes. Because limited routing space in the board, not all
>>>>>high speed signals can be on S2 layer, which is better for signal
>>>>>quality. So some of 2.125Gbps signals running on S1.
>>>>>
>>>>>--------VCC1
>>>>>--------S1 [2.125G PECL]
>>>>>--------VCC2
>>>>>--------S2 [2.125G PECL]
>>>>>--------GND
>>>>>
>>>>>My question is,
>>>>>When the signal S1 is transient from high to low or low to high, which
>>>>>plane would be the return path, VCC or GND? EMC/EMI impact? Any
>>>>>compensation suggestion?
>>>>>How much risk if we go to PCB fabrication like this stack up?
>>>>>
>>>>>Thanks very much!
>>>>>Best Regards,
>>>>>George
>>>>>
>>>------------------------------------------------------------------
>>>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 FAQ wiki page is located at:
>>> http://si-list.org/wiki/wiki.pl?Si-List_FAQ
>>>
>>>List technical documents are available at:
>>> http://www.si-list.org
>>>
>>>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 FAQ wiki page is located at:
>> http://si-list.org/wiki/wiki.pl?Si-List_FAQ
>>
>>List technical documents are available at:
>> http://www.si-list.org
>>
>>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 FAQ wiki page is located at:
http://si-list.org/wiki/wiki.pl?Si-List_FAQ
List technical documents are available at:
http://www.si-list.org
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:
