[SI-LIST] Re: GND Separation for Analog & Digital circuits
- From: "Scott McMorrow" <scott@xxxxxxxxxxxxx>
- To: "Peter Salmon" <psalmon2000@xxxxxxxxx>,"silist" <si-list@xxxxxxxxxxxxx>
- Date: Sat, 21 Feb 2004 09:48:41 -0800
Peter,
I've not seen that article, but I do remember the Power Mesh program at
the University of Arkansas. It was an interesting project designed
specifically for packages with microvia technology They produced one
test package that I know of, and then dropped from my sight. I've not
seen a production package created with this technology, which you should
know is patented by the University of Arkansas. However, Power noise
was definitely increased, due to a higher inductance. Whether this will
hurt your design is another matter from a power noise margin sort of
view. When you route in such a way , the assumption that the power
traces are ideal goes right out the window. They now affect the
neighbor signal lines. This is no different than signal-to-signal
crosstalk and can be analyzed accordingly. In fact, with a board level
SI tool like SpecctraQuest or Mentor ICX or Hyperlynx and a few tricks,
it is possible to actually analyze this. The trick is to fool the
tools into analyzing the power traces as signals, not as ideal power. A
tool like Sigrity Speed2000 or PowerSI can do this without any tricks,
and was designed for packages and power analysis.
You have several sources of noise.
1) increased power noise from the increased inductance of the traces.
This increases the impedance of the power grid and thereby increases the
noise. This can be modeled quite easily with a 2D field solver and
SPICE for the average power trace in the system.
2) Traces have resonant frequencies that are all over the place. When
you route these power traces and eventually tie them to the low
impedance of the package and the regulators, you create a 1/2 wave
resonator whos frequency of resonance is the inverse of the round trip
propagation delay of the structure. For stripline in FR 4, the delay is
about 175 ps/in, or a round trip delay of 350 ps/in. These resonances
will reduce the effectiveness of your power distribution network. They
will also tend to couple into other resonant structures like single
ended signal traces on a PCB. When two resonators are close to the same
frequency, large amounts of energy between them can be coupled. So,
there are two things to worry about. First, that the power grid does
not resonate at any of the switching frequencies of the core or I/O
sections. Second that resonant sections between signals and power do
not have similar resonant frequencies or multiples thereof.
3) Crosstalk between the power delivery grid and the signals. When
current flows on the grid, it induces crosstalk on the signal lines.
For differential signals, this will be okay, as long as the power is
delivered symmetrically around the diff pair, then the noise will be
common mode and will not affect the differential signals. It will,
however, increase the common mode voltage on the differential pair, and
may very well cause your EMI to become sky high if the differntial
signal goes outside the box and loses containment. By placing the power
adjacent to the signals, you force common mode currents to flow in a way
that will couple into the signals and increase the average noise.
Whereas, with a plane architecture, currents are able to flow in many
directions and can statistically cancel, or at least be significantly
reduced. For signals going outside of the box, you will need to be
very careful about isolating them from these power switching currents on
the mesh, otherwise your emissions will go through the roof. This will
be controlled by adequate spacing of the power grid away from the signals.
4) Layer 1 and 4 grounds will be torn up with holes from package escapes
and vias, which may be problematic for routing signals on the inner
layers. Without the additional containment that power/ground plane
pairs can provide, and the rather continuous nature of inner power and
ground planes, signals will become de-referenced causing noise,
radiating apertures and increased emissions, unless you are extremely
careful about routing on the adjacent signal layers.
I'm not saying that this approach won't work. Like any other solution,
it takes engineering, and is never as simple as it seems. Two layer
boards for high volume consumer applications have been designed like
this for years.
best regards,
scott
Peter Salmon wrote:
>Scott,
>
>I am planning to use a 4 layer circuit for multi-GHz signals, following
>the design approach called Power Mesh Architecture. This was written
>up by Happy Holden in the December 2000 issue of The Board Authority:
>"A Design Technology Innovation - The Power Mesh Architecture for
>PCBs". The approach uses the space between signals on each layer to
>route power traces, and can reduce the total number of required copper
>planes by roughly a factor of 2. I plan to have GND on layers 1 and 4,
>and the power mesh with signals on layers 2 and 3, with the layer 2
>routings orthogonal to the layer 3 routings. The signals include 100
>ohm differential pairs and 50 ohm single-sided.
>
>Your posting has me worried that cross-talk between power and signal
>traces may be the archilles heel of this approach. I've been unable to
>do any modeling so far, and I'd appreciate any comments you may have.
>
>Regards,
>Peter Salmon
>
>--- Scott McMorrow <scott@xxxxxxxxxxxxx> wrote:
>
>
>>All,
>>For these types of problems, visualize where the fields will go and
>>use
>>that to determine how to isolate them. At audio and video
>>frequencies,
>>remember that fields do penetrate planes, and that significant noise
>>can
>>occur when digital signals pass underneath analog sections separated
>>by
>>a plane. For good isolation, be sure that no digital signal flows
>>through the analog section on any nearby layer, even if it is
>>separated
>>by a plane. If this is unavoidable, use 1 oz or 2 oz copper instead
>>of
>>1/2 oz copper, to limit field penetration through the metal. Make
>>sure
>>that power planes and traces are totally isolated from noise sources,
>>
>>and digital power sources, with large amounts of separation (> 20 X
>>the
>>dielectric thickness between power and ground planes.) Use 2-D field
>>
>>solvers to determine the crosstalk levels (noise) that will occur.
>>These problems are not hard and can be easily be approached with
>>general
>>purpose quasi-static field solvers that can solve for field
>>penetration
>>thru metals, like Ansoft 2D.
>>
>>Visualize the fields.
>>Be the fields.
>>And all will be well.
>>
>>
>>scott
>>
>>--
>>Scott McMorrow
>>Teraspeed Consulting Group LLC
>>2926 SE Yamhill St.
>>Portland, OR 97214
>>(503) 239-5536
>>http://www.teraspeed.com
>>
>>
>>Geva wrote:
>>
>>
>>
>>>Hello Maheshwari,
>>>
>>>To answer your question on separate analog and digital GND for
>>>
>>>
>>Video and
>>
>>
>>>digital signals;
>>>I had very similar problem of CATV receiver with video at 43 and 5
>>>
>>>
>>MHz,
>>
>>
>>>combined with digital signals on same board.
>>>In the PCB layout design we completely separated the 2 grounds and
>>>
>>>
>>later
>>
>>
>>>on, in the lab, we found out the optimum
>>>locations of connections between the digital GND and the Analog GND,
>>>
>>>
>>and how
>>
>>
>>>many connections needed, for the best performance.
>>>
>>>in order to get the best signal to noise ratio, we used more than
>>>
>>>
>>one
>>
>>
>>>connections between grounds.
>>>
>>>You may come with many theoretical conclusions about one or more
>>>
>>>
>>connection,
>>
>>
>>>but the test will specified the best answer for you.
>>>
>>>Ehood Geva
>>>
>>>
>>>----- Original Message -----
>>>From: "Lee Ritchey" <leeritchey@xxxxxxxxxxxxx>
>>>To: "Zhangkun" <zhang_kun@xxxxxxxxxx>; <maheshwari@xxxxxxxxxx>;
>>><si-list@xxxxxxxxxxxxx>
>>>Sent: Friday, February 20, 2004 9:43 AM
>>>Subject: [SI-LIST] Re: Separate GND for Analog & Digital
>>>
>>>
>>>
>>>
>>>
>>>
>>>>Zhangkun,
>>>>
>>>>Thanks for sharing your results. It supports the concept of
>>>>
>>>>
>>keeping the
>>
>>
>>>>noise out of the analog section by careful routing of those traces.
>>>>
>>>>Lee
>>>>
>>>>
>>>>
>>>>
>>>>
>>>>
>>>>>[Original Message]
>>>>>From: Zhangkun <zhang_kun@xxxxxxxxxx>
>>>>>To: <maheshwari@xxxxxxxxxx>; <si-list@xxxxxxxxxxxxx>
>>>>>Date: 2/20/2004 9:13:05 AM
>>>>>Subject: [SI-LIST] Re: Separate GND for Analog & Digital
>>>>>
>>>>>Dear Maheshwari
>>>>>
>>>>>We have come cross the simular problem. The critial point is to
>>>>>
>>>>>
>>prevent
>>
>>
>>>>>
>>>>>
>>>>>
>>>>>
>>>>return path of digital signal disturbing the analog signal.
>>>>
>>>>
>>>>
>>>>
>>>>>In one of our PCB, there is too much digital noise in analog
>>>>>
>>>>>
>>signal. We
>>
>>
>>>>>
>>>>>
>>>>>
>>>>>
>>>>have to repair it. How to seperate the ground seemed to be the most
>>>>important problem. One is to seperate the ground and to connect the
>>>>
>>>>
>>>>
>>>>
>>>digital
>>>
>>>
>>>
>>>
>>>>ground and analog ground at one point. The other is not to seperate
>>>>
>>>>
>>the
>>
>>
>>>>ground. In order to make sure that the product is OK, we made two
>>>>
>>>>
>>boards,
>>
>>
>>>>seperated and not seperated. In the test, both boards are OK.
>>>>
>>>>
>>>>
>>>>
>>>>>It has nothing to do with seperating ground or not. Being care of
>>>>>
>>>>>
>>the
>>
>>
>>>>>
>>>>>
>>>>>
>>>>>
>>>>digital return path is the most important. Some CAD tools could do
>>>>
>>>>
>>such
>>
>>
>>>>simulation.
>>>>
>>>>
>>>>
>>>>
>>>>>I hope this will help.
>>>>>
>>>>>Best Regards
>>>>>
>>>>>Zhangkun
>>>>>2004.2.20
>>>>>
>>>>>----- Original Message -----
>>>>>From: "Maheshwari.P" <maheshwari@xxxxxxxxxx>
>>>>>To: <si-list@xxxxxxxxxxxxx>
>>>>>Sent: Thursday, February 19, 2004 7:41 PM
>>>>>Subject: [SI-LIST] Separate GND for Analog & Digital
>>>>>
>>>>>
>>>>>
>>>>>
>>>>>
>>>>>
>>>>>>Hi All,
>>>>>>
>>>>>>I am designing boards which contain Audio and Video codecs. I
>>>>>>
>>>>>>
>>need to
>>
>>
>>>>>>
>>>>>>
>>>>>>
>>>>>>
>>>>pass
>>>>
>>>>
>>>>
>>>>
>>>>>>analog signal to the corresponding decoders without much noise.
>>>>>>
>>>>>>Is it better to have separate analog and digital GND?
>>>>>>or
>>>>>>
>>>>>>Is it better to have a solid GND and have separate analog and
>>>>>>
>>>>>>
>>digital
>>
>>
>>>>>>sections?
>>>>>>
>>>>>>Which of the either way will give better results in terms of
>>>>>>
>>>>>>
>>audio and
>>
>>
>>>>>>
>>>>>>
>>>>>>
>>>>>>
>>>>video
>>>>
>>>>
>>>>
>>>>
>>>>>>quality?
>>>>>>
>>>>>>Thanks in advance,
>>>>>>Maheshwari
>>>>>>
>>>>>>
>>>>>>
>>>>>------------------------------------------------------------------
>>>>>
>>>>>
>>>>>>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 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 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 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
>>
>>
>>
>>
>
>
>
--
Scott McMorrow
Teraspeed Consulting Group LLC
2926 SE Yamhill St.
Portland, OR 97214
(503) 239-5536
http://www.teraspeed.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 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:
