[SI-LIST] Re: risetime effects of plane breaks
- From: Scott McMorrow <scott@xxxxxxxxxxxxx>
- To: ron@xxxxxxxxxxx
- Date: Sat, 22 Jan 2005 18:23:17 -0500
Ron
It's funny that Intel "discovered" slot lines, since they have been
around since the dawn of microwave engineering on printed circuit
boards. The literature goes back to at least the early 60's.
As for gap width, changing the width of the gap will change the coupling
across the slot and thus it's impedance. (This may make the coupling
into the slot more or less efficient.) However, this is only part of
the crosstalk problem. AC return path energy is still injected into the
cavity preceding the split and is available for crosstalk into the
adjacent conductors. Increasing gap width will actually increase the
amount of energy that is injected and contained by the preceding
cavity. Crosstalk in the power/ground cavity will then be controlled
by the resonant modes of the cavity. CST Microwave Studio is capable of
simulating all of these cavity modes without closed form equations and
thus will solve for the coupling into slot lines, along with all "lost
energy" that is injected into the surrounding cavities.
regards,
scott
ron@xxxxxxxxxxx wrote:
>A few years ago Intel discovered that when a trace crosses a split it
>can excite a transmission
>line mode into the slot between the panes called "slot line" strangely
>enough. If the gap is small
>it works quite well and all the traces crossing it become cross-talk for
>one another.
>
>To avoid it make the gap at least 2 or 3 times the thickness of the
>dielectric.
>
>ADS (Agilent) has a model for slot lines with the other transmission lines.
>
>Ron
>
>Chris Cheng wrote:
>
>
>
>>Scott,
>>Excellent summary. That was my concern on striplines crossing with a bus
>>rather than individual signals. In a way, it is like wire bond signal leads
>>without the ground leads mixed among them. The signals start referencing
>>each other instead. Or you can see it as a trade-off between adding
>>shielding layers or spreading the bus spacing (decreasing routing channels)
>>in a high density/performance design. My own rule of thumb is space them at
>>least equal or larger than the gap itself when crossing. That's is at least
>>a 3x decrease in routing channels so it is quite costly and has to be weight
>>against adding shielding layers. Sometimes its worth it, sometimes its not.
>>As for EMI, if you dig back some discussion I had with Steve, I always
>>prefer solid ground planes referencing microstrips on top and bottom of PCB
>>and then stitch the edges with ground vias. Hopefully any of those excited
>>noise on the cut power planes will be trapped inside.
>>
>>-----Original Message-----
>>From: Scott McMorrow [mailto:scott@xxxxxxxxxxxxx]
>>Sent: Thursday, January 20, 2005 2:39 PM
>>Cc: Si-List
>>Subject: [SI-LIST] Re: risetime effects of plane breaks
>>
>>
>>When this thread started I was on vacation. However, I found this
>>interesting enough to resurrect some previous simulations I'd performed
>>in CST Microwave Studio. After much playing, twiddling and generally
>>having fun I can say several things:
>>1) It's pretty easy to confirm Doug's results using 3D fullwave
>>simulation. In fact, in about 30 minutes I can replicate his case and
>>create a design that can be easily modified for many other
>>possibilites. The microstrip split plane crossing is a no-brainer.
>>Just don't do it and expect anything approaching an EMI "clean" system.
>>
>>2) Chris and Steve ... and eventually myself, wanted to know more about
>>the various different stripline plane crossing configurations, so I
>>setup a simulation with a VDD island not unlike what might be found in a
>>memory system, and performed multiple simulations with dual asymmeteric
>>stripline crossing the plane twice on it's way to the memory module. Not
>>surprisingly the following is true:
>>
>> It is best not to cross a split plane ... even with stripline.
>> If you do, it is better to cross a split that is adjacent to a
>> ground plane
>> It is even better if you cross a split adjacent to a ground plane on
>> the stripline layer furthest away from the split plane (i.e. next to
>> a ground plane)
>> It is worst to cross a split plane that has no adjacent ground.
>> The width of the gap in the plane makes very little difference until
>> it becomes really small or really big.
>> Crosstalk scales almost linearly with the number of aggressors
>> crossing the split. (i.e. - it can get really bad!)
>> Bypass of the split power island helps for frequencies below 500
>> MHz, provides no help for frequencies higher than 500 MHz, and as
>> such has no benefit to most of the noise and crosstalk created by
>> high speed signals crossing onto and off of the island.
>>
>>The energy released into the power/ground plane cavities by high speed
>>signal split plane crossings is huge and essentially cannot be
>>suppressed with bypass capacitors. Any attempt at supprerssion with
>>capacitors exhibits what I call a "Whack-A-Mole" property. You can
>>never get rid of those pesky little moles. All you can do is to move
>>them around by thumping them. Given that all this energy is rattling
>>around the PCB power planes from split plane crossings, it will
>>eventually go somewhere. Since it's really easy to develop all sorts of
>>resonant power island cavities that have primary resonant frequencies in
>>the 500 MHz to several GHz range, it is not at all unlikely that any
>>split plane crossing has an extremely strong potential to excite a
>>resonance in a frequency range that will cause most systems to fail EMC
>>compliance testing About all you can do is to shield the cavity patches
>>using ground layers. This should reduce the radiated energy
>>significantly, but will not totally eliminate it, since eventually it
>>will find it's way to all those pesky device and package leads.
>>
>>
>>best regards,
>>
>>Scott
>>
>>
>>
>>
>>
>
>
>
>
ron@xxxxxxxxxxx wrote:
>A few years ago Intel discovered that when a trace crosses a split it
>can excite a transmission
>line mode into the slot between the panes called "slot line" strangely
>enough. If the gap is small
>it works quite well and all the traces crossing it become cross-talk for
>one another.
>
>To avoid it make the gap at least 2 or 3 times the thickness of the
>dielectric.
>
>ADS (Agilent) has a model for slot lines with the other transmission lines.
>
>Ron
>
>Chris Cheng wrote:
>
>
>
>>Scott,
>>Excellent summary. That was my concern on striplines crossing with a bus
>>rather than individual signals. In a way, it is like wire bond signal leads
>>without the ground leads mixed among them. The signals start referencing
>>each other instead. Or you can see it as a trade-off between adding
>>shielding layers or spreading the bus spacing (decreasing routing channels)
>>in a high density/performance design. My own rule of thumb is space them at
>>least equal or larger than the gap itself when crossing. That's is at least
>>a 3x decrease in routing channels so it is quite costly and has to be weight
>>against adding shielding layers. Sometimes its worth it, sometimes its not.
>>As for EMI, if you dig back some discussion I had with Steve, I always
>>prefer solid ground planes referencing microstrips on top and bottom of PCB
>>and then stitch the edges with ground vias. Hopefully any of those excited
>>noise on the cut power planes will be trapped inside.
>>
>>-----Original Message-----
>>From: Scott McMorrow [mailto:scott@xxxxxxxxxxxxx]
>>Sent: Thursday, January 20, 2005 2:39 PM
>>Cc: Si-List
>>Subject: [SI-LIST] Re: risetime effects of plane breaks
>>
>>
>>When this thread started I was on vacation. However, I found this
>>interesting enough to resurrect some previous simulations I'd performed
>>in CST Microwave Studio. After much playing, twiddling and generally
>>having fun I can say several things:
>>1) It's pretty easy to confirm Doug's results using 3D fullwave
>>simulation. In fact, in about 30 minutes I can replicate his case and
>>create a design that can be easily modified for many other
>>possibilites. The microstrip split plane crossing is a no-brainer.
>>Just don't do it and expect anything approaching an EMI "clean" system.
>>
>>2) Chris and Steve ... and eventually myself, wanted to know more about
>>the various different stripline plane crossing configurations, so I
>>setup a simulation with a VDD island not unlike what might be found in a
>>memory system, and performed multiple simulations with dual asymmeteric
>>stripline crossing the plane twice on it's way to the memory module. Not
>>surprisingly the following is true:
>>
>> It is best not to cross a split plane ... even with stripline.
>> If you do, it is better to cross a split that is adjacent to a
>> ground plane
>> It is even better if you cross a split adjacent to a ground plane on
>> the stripline layer furthest away from the split plane (i.e. next to
>> a ground plane)
>> It is worst to cross a split plane that has no adjacent ground.
>> The width of the gap in the plane makes very little difference until
>> it becomes really small or really big.
>> Crosstalk scales almost linearly with the number of aggressors
>> crossing the split. (i.e. - it can get really bad!)
>> Bypass of the split power island helps for frequencies below 500
>> MHz, provides no help for frequencies higher than 500 MHz, and as
>> such has no benefit to most of the noise and crosstalk created by
>> high speed signals crossing onto and off of the island.
>>
>>The energy released into the power/ground plane cavities by high speed
>>signal split plane crossings is huge and essentially cannot be
>>suppressed with bypass capacitors. Any attempt at supprerssion with
>>capacitors exhibits what I call a "Whack-A-Mole" property. You can
>>never get rid of those pesky little moles. All you can do is to move
>>them around by thumping them. Given that all this energy is rattling
>>around the PCB power planes from split plane crossings, it will
>>eventually go somewhere. Since it's really easy to develop all sorts of
>>resonant power island cavities that have primary resonant frequencies in
>>the 500 MHz to several GHz range, it is not at all unlikely that any
>>split plane crossing has an extremely strong potential to excite a
>>resonance in a frequency range that will cause most systems to fail EMC
>>compliance testing About all you can do is to shield the cavity patches
>>using ground layers. This should reduce the radiated energy
>>significantly, but will not totally eliminate it, since eventually it
>>will find it's way to all those pesky device and package leads.
>>
>>
>>best regards,
>>
>>Scott
>>
>>
>>
>>
>>
>
>
>
>
--
Scott McMorrow
Teraspeed Consulting Group LLC
121 North River Drive
Narragansett, RI 02882
(401) 284-1827 Business
(401) 284-1840 Fax
http://www.teraspeed.com
Teraspeed is the registered service mark of
Teraspeed Consulting Group LLC
------------------------------------------------------------------
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:
