Hi Tim
Have you ever tried the free tool provided by Rogers for calculating the
trace impedance?
https://www.rogerscorp.com/documents/8939/acs/2017-Microwave-Impedance-Calculator-Instructional-Manual.pdf
To me looked nice and much closer to 2D field solver impedance calculator
Regards
Cris
On Sun, May 13, 2018 at 6:16 PM Tim Smith <tgsmith81@xxxxxxxxx> wrote:
Thanks Lee,
I guess that really validates a comment you one made that the value
provided by a free tool is equal to its cost...
I've seen may PCB designers rely heavily on these free tools (as decent
tools cost money), but their differential pair calculators don't change the
value produced for Zo as the spacing changes. This, it would seem, is a
severe error and completely invalidates the result.
Why is it that companies expect these designers to produce quality PCBs
without investing the money to actually do so?
On Mon, May 14, 2018 at 11:01 AM, <leeritchey@xxxxxxxxxxxxx> wrote:
As mentioned in that cited paper, if you choose to tightly couple aand
differential pair, each line will drive the impedance of the other down
you will have to narrow each trace to get back to 50 ohms or 100 ohmsthrough
differential if you prefer to think that way. In the bargain you will
increase skin effect loss. However, that is not the big down side.
Wherever the pair travels it will have to remain tightly coupled. If for
some reason you cannot do that and they are separated as when going
a BGA array, the impedance will increase dramatically.learn
When gain experience in this area, you will learn that differential
impedance is not the important driver. Two good 50 ohm lines is. We
that a "not closer than" rule avoids all of these problems. By notcloser
we mean that the lines are far enough apart that they don't drive thedifferential
other's impedance down.
In closing, there is not real value in "tight coupling" in a
pair."differential"
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx <si-list-bounce@xxxxxxxxxxxxx> On
Behalf Of Tim Smith
Sent: Sunday, May 13, 2018 5:46 PM
To: Adam Dixon <lanterna.viridis@xxxxxxxxx>; si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: Fwd: Differential and single-ended impedances
Yes, theoretical only. I would not expect any fab shop to accept that
geometry.
I've been reading through one of Lee's papers, " A TREATMENT OF
DIFFERENTIAL SIGNALING AND ITS DESIGN REQUIREMENTS" and in it, the
following statement is made:
"The reason that differential impedance is almost always specified rather
than single-ended impedance is that it is thought that differential
impedance is different than the sum of the two impedances when the
individual impedance is measured from ââ¬Ågroundâ⬠to either of the
two
traces."
Is it true that as we bring the two traces together both the
impedance and the single-ended impedance reduce so that the"differential"
is always 2x that of the single ended?such
If so, this is where simple tools such as Saturn PCB fall over. Tools
as these seem to be heavily relied on due them being free.wrote:
Should we really be specifying "odd-mode" instead of "single-ended"?
On Mon, May 14, 2018 at 10:23 AM, Adam Dixon <lanterna.viridis@xxxxxxxxx
wrote:
This is a theoretical question, I assume, as from a fabricationthe channel.
perspective, 0.05mm spacing will be a major major yield challenge (if
any fabricator will accept producing the design reliably). You have
to know your receiver VIH/VIL/noise specs to understand the potential
performance impact or at what point you cross a threshold that breaks
Ultimately it's a pair of single-ended nets, each of which has
impedance matching and VIH/VIL requirements, right?
Regards,
Adam in Atlanta
adam.dixon@xxxxxxxx
On Sun, May 13, 2018 at 7:48 PM, Tim Smith <tgsmith81@xxxxxxxxx>
wrote:
Thanks for the responses.
So, say I route the two traces with very tight coupling, something in
the order of only 0.05 mm between them. This will greatly reduce the
"differential impedance".
Logic tells me that as long as each trace is still a 50R line, the
system will work, but what effect does reducing this differential
impedance actually have on the system performance?
On Sat, May 12, 2018 at 2:25 AM, Joel Brown <joel@xxxxxxxxxx> wrote:
Tim,due
As you have alluded, two traces routed close together will have a
lower differential impedance than two 50 ohm traces routed far
apart. This is
to the coupling between the traces. Routing a differential pairclose
with
spacing has the benefit of higher noise immunity and lowerdue to
radiation
cancellation of the fields. A differential impedance of 97 ohms vsohms
100
is not going to be significant. Most boards shops have a tolerance+/-
of
10% on controlled impedance traces. You could run simulations andthe
vary
impedance from 90 to 110 ohms to see what effect it has on the
signal integrity.
Regards,
Joel
On Thu, May 10, 2018 at 9:29 PM, Tim Smith <tgsmith81@xxxxxxxxx>
research of
Hi experts,
I'm aware that this subject has been well discussed, but in my
inboth the SI list and many Google searches, I seem to have found
myself
differentiala
bit of a muddle.
Let us consider a PCIe "differential" pair that needs to be routed
on a PCB from a processor (i.MX6) to a PCIe to GbE bridge (I211).
A "differential" impedance of 100R is called out as the I211
contains on-die terminations.
I know from reading some literature that some insist that the
transmissionimpedance is not important and to just route them as two 50R
apart.lines. This makes sense given the theory of the differential
signalling and the 100R termination.
Now comes the practical application of placing these two traces on
the PCB.
There are two methods, route them close together, or route them
far
differentialThis is where I start to not be able to get a solid answer.
The math states that for these signals, the differential impedance
is twice that of the odd mode impedance. We know that the odd mode
impedance is dependent on the traces separation. Therefore, so too
is the
single-endedimpedance.
the first-order approximation equations that many designers use
(those without the capabilities of 3D field solvers) state that
for two 50R single-ended transmission lines operating as
differential signals, you need infinite separation in order to
achieve 100R differential impedance.
In my designs, I've always focused more on targeting the 50R
butrather than the 100R differential.
I've heard many times that the differential impedance does not
matter,
differential,my questions are these:
- Why is there so much emphasis placed on this concept of
differential impedance?
- Does if affect the performance of the signals in any way if it's
not matched to the termination resistor(s)?
- If I target 50R single-ended and route them so I get 97.3R
do I need to adjust the termination resistor(s) to match?
Looking forward to your thoughts.
Dr. Tim
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
