[SI-LIST] Re: [Bulk] Re: PCB Impedance Failure
- From: "Ken Cantrell" <Ken.Cantrell@xxxxxxxxxxxxxxxx>
- To: <ludwig@xxxxxxxxxxxxxxxxx>, <tom@xxxxxxxxxxxxx>
- Date: Thu, 12 Jan 2006 09:55:05 -0700
Ludwig,
Re: "I don't think anyone was claiming that one can achieve 100 Ohm
differential impedance using 50 Ohm SE traces."
I use 50 ohm SE, 100 ohm diff all the time. Example: stripline, trace and
plane thicknesses 0.64 mils, permittivity 4.0, dielectric thicknesses 4
mils, trace width 3.25 mils, run the pair on 15 mil centers. SE is 49.5,
Diff is 98.5. If I get 97 - 100 ohm diff, things work great, and I'm sure
it could be looser than that and still work fine for standard LVDS type
implementations. As someone else stated, this type of geometry (loosely
coupled spacing), although it yields a lower routing density, allows for a
smooth impedance transition in the pin field escape area since the increased
trace separation has little effect on the diff impedance.
If you need to go to higher routing densities, then the SE impedance must be
increased as you have pointed out.
Clayton,
If the board house can't produce a good cupon, I would get a re-spin soley
on those grounds. Be patient though, stuff happens.
Ken
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx]On Behalf Of Stefan Ludwig
Sent: Thursday, January 12, 2006 8:08 AM
To: tom@xxxxxxxxxxxxx
Cc: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: [Bulk] Re: PCB Impedance Failure
Hi Tom,
Just a clarification: I don't think anyone was claiming that one can
achieve 100 Ohm differential impedance using 50 Ohm SE traces. Given a
constant distance to the reference plane(s), your differential pairs of
100 Ohm will be built using, say, 60 Ohm SE traces of a certain width
and of a certain separation.
Your 50 Ohm SE traces on the same layer will have a different width
(wider) than the 60 Ohm SE traces. If you'd calculate the differential
impedance of two such 50 Ohm SE traces, given the same separation, you'd
end up with less than 100 Ohms.
Zdiff = 2*Z0*(1-a*exp(-b*D/H))
with a, b = positive constants, D = trace separation, H = height
over/between reference plane.
The exponential term of trace separation is what you refer to as
coupling impedance. But the point is that you can achieve Zdiff = 2*Z0
only if the distance between the traces goes to infinity.
In any case, the board house didn't deliver the goods and Clayton should
either ask for a refund or a respin of the board. The message, however,
sounded like there was no time for a respin, hence his request for
information.
Cheers,
Stefan Ludwig
Tom Dagostino wrote:
>Kai
>
>I think you are missing the point. The board was designed to have 50 Ohm
SE
>traces and at the same time 100 Ohm differential traces. What was received
>was 59 Ohm SE traces and 86 Ohm differential traces. When the impedance of
>the SE traces increases the differential impedance should also increase.
>The differential impedance is 2*SE - coupling impedance. If we assume the
>coupling did not change significantly since the original was no coupling
the
>as fabricated board's impedance should have been 118 Ohms.
>
>Tom Dagostino
>Teraspeed(R) Labs
>13610 SW Harness Lane
>Beaverton, OR 97008
>503-430-1065
>tom@xxxxxxxxxxxxx
>www.teraspeed.com
>
>Teraspeed Consulting Group LLC
>121 North River Drive
>Narragansett, RI 02882
>401-284-1827
>
>-----Original Message-----
>From: si-list-bounce@xxxxxxxxxxxxx
>[mailto:si-list-bounce@xxxxxxxxxxxxx]On Behalf Of Kai Keskinen
>Sent: Wednesday, January 11, 2006 2:47 PM
>To: Aubrey_Sparkman@xxxxxxxx; a.ingraham@xxxxxxxx; si-list@xxxxxxxxxxxxx
>Subject: [SI-LIST] Re: [Bulk] Re: PCB Impedance Failure
>
>
>Aubrey:
>
>That is really easy. Just closely couple the diff pairs and you can go from
>60 Ohms single ended to 90 Ohms differential with very little effort. It is
>not really what you want to do if you have complicated routing through pin
>fields since you then get a huge impedance hit if you have to separate the
>pairs. Just use any field solver that handles diff pairs and try it. Set up
>a 60 Ohm single ended line. Use the same cross-section and add the second
>line and move them closer together. You will get a lot lower than 2x single
>ended impedance.
>
>Cheers,
>
>-----Original Message-----
>From: si-list-bounce@xxxxxxxxxxxxx
>[mailto:si-list-bounce@xxxxxxxxxxxxx]On Behalf Of
>Aubrey_Sparkman@xxxxxxxx
>Sent: Wednesday, January 11, 2006 1:45 PM
>To: a.ingraham@xxxxxxxx; si-list@xxxxxxxxxxxxx
>Subject: [Bulk] [SI-LIST] Re: PCB Impedance Failure
>
>
>I'm a little puzzled about something else. Did you really get the diff
>impedance to be on the low side (100->86) on the same board / layer
>where the single ended impedance is on the high side (50->59)? Please
>explain how that was done!
>
>
>Aubrey Sparkman=20
>Enterprise Engineering Signal Integrity Team
>Dell, Inc.=20
>Aubrey_Sparkman@xxxxxxxx=20
>(512) 723-3592
>
>-----Original Message-----
>From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]
>On Behalf Of Andrew Ingraham
>Sent: Wednesday, January 11, 2006 11:40 AM
>To: si-list@xxxxxxxxxxxxx
>Subject: [SI-LIST] Re: PCB Impedance Failure
>
>Clayton,
>
>I was a little puzzled about two things you stated.
>
>One, that the specified differential impedance was exactly twice the
>specified single trace impedance. That requires no coupling between
>traces of a differential pair (if they are routed on the same layers
>with the same trace widths). Is that what you really intended? Since
>you got 86 ohms diff. and 59 ohms s.e., your differential pairs must not
>have been routed with nearly enough isolation.
>
>The other is about the error on the test coupon. Can you trust any
>measurements on those coupons?
>
>Did your company actually specify 50 +/- 10%, or was that only a
>recommendation? If it was in the spec, then I wouldn't even bother
>asking about the risk; I'd send the boards back to the board vendor and
>tell them to make new ones that satisfy what you paid them to do. The
>fact that they were made wrong, is reason enough to be concerned.
>
>Regarding the question of the impact on SI, that depends entirely on the
>application, on how long the traces are (vs. risetimes and/or frequency
>content), on the types of signals, on the chips used, and if and how
>lines are terminated. Sometimes it makes little difference whether the
>actual impedances are even close to the target. Sometimes it makes all
>the difference. 59 ohms isn't that far from 50 ohms, but if you were
>using leading edge technologies and pushing all the margins (which you
>probably aren't, since you didn't use SI tools), it could indeed be
>significant.
>
>Regards,
>Andy Ingraham
>
>
>
>>A board we just had fabricated failed the impedance test coupon. 59=20
>>ohm vs 50+/- 10%. They could not measure the diffferential pairs=20
>>because of an error on the coupon, but calculated 86 ohm impedance vs=20
>>100 +/- 10%
>>
>>
>
>
>------------------------------------------------------------------
>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: =20
> //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
> =20
>------------------------------------------------------------------
>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
>
>
>
>
>
--
Ludwig Systems Engineering Consulting - Design - Implementation
WWW: www.ludwigsystems.com System Architectures - FPGAs - PCBs
Ph/Fx: +41-43-355-58-73/74 Hardware - Firmware - Software
------------------------------------------------------------------
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
______________________________________________________________________
All email being sent to or from SRC Computers, Inc. will be scanned by a
third party scanning service.
______________________________________________________________________
------------------------------------------------------------------
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:
