[SI-LIST] Re: Diff line
- From: "Harvey, Wilbur" <Wilbur.Harvey@xxxxxxxxxxxxxx>
- To: si-list@xxxxxxxxxxxxx
- Date: Fri, 15 Feb 2002 06:45:37 -1000
I made a test board which has a 5mil 50ohm trace, launched with an SMA
connector, 2" to an 3/4" S bend, 2" to a via, 2" back to an identical 3/4"
"S" bend but with square corners, and 2" back to an 51ohm 0603 terminator
resistor under the SMA connector. The via is a 10mil finished drill size
with a 20mil pad, and a 34mil antipad to the planes. The stackup was
Top Trace
3 mil FR4
Ground Plane
1.8 mil FR4
Power Plane
36 mil FR4
Power Plane
1.8 mil FR4
Ground Plane
3 mil FR4
Bottom Trace
There was a ground shorting via between the two ground planes 75 mils from
the thru via at the end of the trace.
When looking at it with the TDR, you can clearly see both S bends, the via,
and the terminator resistor.
Both S bends are basically the same, rounded corners vs square (a total of 6
corners each) made no noticeable difference.
The via was clearly inductive, the impedance went up about 6 ohms, and the
pad on the terminator resistor was capacitive with an impedance dip of about
5 ohms.
I mention this in reference to the comment of untuned via's generally being
capacitive in nature. I have seen several reports of the effects of vias,
but no one ever puts actual numbers down as to the impedance and geometries.
My numbers might be slightly off, they are from memory, but they are close.
Wilbur Harvey - Engineer
Adtech Inc., www.adtech-inc.com
3465 Waialae Ave. Suite 200
Honolulu, HI 96816
Tel: +1 (808) 440 3363, Fax: +1 (808) 440 3494
email: wilbur.harvey@xxxxxxxxxxxxxx
-----Original Message-----
From: pikeda@xxxxxxxxxxx [mailto:pikeda@xxxxxxxxxxx]
Sent: Thursday, February 14, 2002 6:09 PM
To: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: Diff line
Scott, I agree with everything you said and would like to add that loss due
to
skin effect will increase since the extra capacitance in the lines will tend
to
squeeze the flow towards the inside edges. Fabrizio, Pravin, if the multigig
lines are that dense that you can't avoid tightly coupled lines than I would
suggest matching lengths near transitions such as at the via, bga or
connector.
After all if you look at an untuned vias, they generally look capacitive or
dip
in impedance. The seperated line is higher in impedance. So if the risetime
is
long compared to those two structures that are next to each other, than the
impedance should actually look more flat. For 2.5GHz I estimate that the 2
structures should be less than 300 mils (very rough estimate). Another tip
if
EMI is not too much of a concern such as for well referenced stripline, is
to
match some distance away from the driver where the losses have slowed down
the
risetime and the mismatch in impedance will have less of an impact.
No alternative solution is without a downside for certain circumstances or
it
wouldn't be an alternative, it would just be the only solution.
Paul
"zanella, fabrizio" <zanella_fabrizio@xxxxxxx> on 02/14/2002 06:39:44 PM
Please respond to zanella_fabrizio@xxxxxxx
To: Paul Ikeda/Marvell@xxxxxxxxxxx, si-list@xxxxxxxxxxxxx
cc:
Subject: [SI-LIST] Re: Diff line
Paul, a large percentage of nets on pc boards are now differential.
By using 20 mil spacing for your loosely coupled differential pairs, I don't
see how you can route high density boards without using 20-30 layers, which
increases cost, creates manufacturability problems, increases via
capacitance, etc. The trend is to pack more and more routes in a given
space. 5 mil lines with 5 mil spacing, edge coupled on stripline layers is
quite common for differential pairs and works very well for 2.5Gbs signals.
For the differential skew value, make sure you look at the entire path,
through the BGA, connectors, vias, etc, the total lenghts may be closer than
300 mils.
Regards,
Fabrizio Zanella
Signal Integrity
EMC Corporation
fzanella@xxxxxxx
-----Original Message-----
From: pikeda@xxxxxxxxxxx [mailto:pikeda@xxxxxxxxxxx]
Sent: Thursday, February 14, 2002 9:08 PM
To: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: Diff line
Pravin,
This is just one more argument to loosely couple your differential lines. If
they have around 20 mils seperation, you can treat them as single ended and
serpentining has no effect on impedance. Here is an article by Dr. Howard
Johnson on why you don't need to tightly couple your diff pairs which I
agree
with wholeheartedly. By the way I commonly do 3.125GHz loosely coupled and
they
work very well.
http://www.sigcon.com/news/2_30.htm
Paul
" pravin patel" <fairfax100@xxxxxxxxxxxxx> on 02/14/2002 06:25:04 AM
Please respond to fairfax100@xxxxxxxxxxxxx
To: si-list@xxxxxxxxxxxxx
cc: (bcc: Paul Ikeda/Marvell)
Subject: [SI-LIST] Diff line
I am doing layout of 2.5Ghz diff. line and having hard time to match length
of a
pair by 300 mil. I was going to make one line serpentine to make both line
matched. By doing serpentine, I am creating impedance discontinuty or I will
create skew.
Any Ideas. Thanks
--
------------------------------------------------------------------
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:
