[SI-LIST] Re: 50 Ohm Via?
- From: wolfgang.maichen@xxxxxxxxxxxx
- To: "Joel Brown" <joel@xxxxxxxxxx>
- Date: Thu, 10 Jan 2008 16:34:27 -0800
Joel,
actually your numbers are borderline for being concerned. Keep in mind,
the 6x rule is really just a rough rule of thumb. For example, I did a
quick simulation for a signal with 40ps rise time (T10/90), your 7.5 ps
via, assuming the via impedance is 25 Ohms (i.e. it is too capacitive).
Looking at the simulated TDR shows a reflection of about 10%. Now is that
something to be concerned? Depends on your situation.
First, a 10% reflection can cause data dependent jitter of (again, rough
rule of thumb) +/-(Tr x 10%/100) = +/-4 ps. That means your data eye
opening will shrink by 8ps. That assumes the reflection bounces oof the
driver and eventually makes it to the receiver. If that is an issue will
depend on how large the timing margins in your design are.
Second, you may have more than one via in your path. If you are really
unlucky, then the reflections from both vias just coincide (e.g.
relfection from previous edge coming back from one via, and reflection
from two edges before from second via). If that happens or not will be
highly sensitive to your data rate and to the location of those vias. In
this worst case your eye degradation would now be 16ps.
One the other hand, reflection may not matter too much if your driver is
impedance matched to 50 Ohms (or 100 Ohms differential). That's the case
for many CML drivers, but not for PECL driver (they are around 7 Ohms). In
this case the driver will swallow the reflection.
Similar simple estimates and simulations can be done for e.g. rise time
degradation, or for the stub (e.g. approximate stub and surrounding planes
as a cylindrical capacitor).
The way I usually decide how much effort to put into simulation, I usually
start out like this:
(1) use rough rulse of thumb, order-of-magnitude-estimates, or experience
from previous similar situations to get a feeling where I am. Three
possible outcomes:
- E.g. if the via has 7.5ps prop delay and I am using a signal from a
Microcontroller with 5ns rise time, I can already tell I won't have a
problem. Done. No need to spend a lot of time simulating this, the answer
would stay the same.
- On the other hand, if my rise time is 15ps I can already tell I will
have a big issue. Done. No need to run a lot of simulations to find that
out. Instead spend the effort on figuring out fundamental improvements to
the design: maybe use controlled impedance vias (this may take some field
solver work); maybe I can reduce the board thickness. Maybe I should try
to avoid vias on this critical path, keep it a surface trace. And so on.
- Finally, if it's borderline (like the case above), that's the situation
where I feel a good model and a good simulator adds most value, because
only this can tell me beforehand if I should change my design or if I am
fine.
(2) once I decided that I have to do more modeling and simulation, I still
wouldn't go straight to the most powerful, complicated, expensive piece of
software I can find. Oftentimes you can get very far with simple,
easy-to-use tools to improve your understanding. Personally I particularly
like the Student version of PSpice (because it can deal with differential
transmission lines), the TNT field solver (from Sourceforge, for 2D
simulations of impedance, crosstalk), and recently Gore's TLineSim (online
tool, http://www.tlinesim.com - lossy lines, eye diagrams and much more).
Other people will have different preferences, and it also depends what you
have access to. Note that the tools I mentioned here are all free, so you
don't have to go to your manager to get budget approval to start playing
around with. I just think that starting out simple helps understand the
basic issues before diving into more sophisticated tools (otherwise you
may spend a lot of time and effort in a top-notch tool just to find out
that your model bears little resemblance to real life).
(3) finally, there are cases when you have to use more sophisticated
tools, but in my experience for most of us that happens less often than
you may think. Of course this is changing when you move to faster and
faster speeds. Also, I believe that understanding of the basic behavior
should come before going to a lot of math (or modeling). Simple tools and
rules of thumb will help you sanity-check any results you get back from
e.g. your high-end 3D simulator. A simple tool combined with good
understanding of your design goes much further than a complicated tool
that you have to trust blindly. E.g. if that full-blown 3D model predicts
0.01% reflection for the via example above, that would make me highly
suspicious of the result, and I'd immediately go looking for the bug in my
model setup... which wouldn't happen if I had never estimated the rough
effect in the first place.
Wolfgang
"Joel Brown" <joel@xxxxxxxxxx>
01/10/2008 03:43 PM
To
<wolfgang.maichen@xxxxxxxxxxxx>, <Aubrey_Sparkman@xxxxxxxx>
cc
<luant@xxxxxxxxxxx>, <si-list@xxxxxxxxxxxxx>,
<si-list-bounce@xxxxxxxxxxxxx>
Subject
RE: [SI-LIST] Re: 50 Ohm Via?
Wolfgang,
So I crunched some numbers. Assuming a PCB thickness of .09 inches and the
signals travels through the via from top to bottom the prop delay is 7 ps.
6 times this is 42 ps. The minimum rise time for PCI express gen 1 is 50
ps
so the via impedance should not be a factor. The minimum rise time for gen
2
is 30 ps so now whether the impedance is a factor is border line. If the
signal only travels half way through, now the prop delay is 3.5 ps for the
signal with a stub length of 3.5 ps. Does this sound right?
Joel
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]
On
Behalf Of wolfgang.maichen@xxxxxxxxxxxx
Sent: Thursday, January 10, 2008 3:09 PM
To: Aubrey_Sparkman@xxxxxxxx
Cc: joel@xxxxxxxxxx; luant@xxxxxxxxxxx; si-list@xxxxxxxxxxxxx;
si-list-bounce@xxxxxxxxxxxxx; wolfgang.maichen@xxxxxxxxxxxx
Subject: [SI-LIST] Re: 50 Ohm Via?
Aubrey,
what I tried to say is, if the transition time through your via (or
through the stub hanging off) is small (rule of thumb < 16/th) of your
signal rise time, then in most cases the impedance of the via structure
does not matter much, and the reflection (and rise time degradation) from
the stub does not matter much (i.e. they have negligiblke influence on
your signal integrity). Of course there are cases when this simple rule
breaks down. E.g. assume a short stub with VERY small clearance to
surrounding planes - this will add a lot of capacitance, so even though
the physical length of the stub may be very short, it's parasitic
capacitance in combination with the transmission line impedance will
create an untolerably large time constant - i.e. a strong reflection, and
strong bandwidth degradation. But in practice such extreme cases are .
If the via impedance is not 50 Ohms, and the transition time through the
via gets into the order of magnitude of your signal rise time, then you
will see the effects of those reflections. In this case it is necessary to
get the via transition close to 50 Ohms as well so the reflections are
small.
Wolfgang
<Aubrey_Sparkman@xxxxxxxx>
01/10/2008 11:56 AM
To
<wolfgang.maichen@xxxxxxxxxxxx>, <joel@xxxxxxxxxx>
cc
<luant@xxxxxxxxxxx>, <si-list@xxxxxxxxxxxxx>,
<si-list-bounce@xxxxxxxxxxxxx>
Subject
RE: [SI-LIST] Re: 50 Ohm Via?
All,
I have not been paying close attention to this thread, so feel free to
blast me if I'm off base or missed something, but my reaction on what
I've read: If all you have to worry about is the time through the via,
then you probably don't have to worry about the via. My $0.02 on when
you really have to worry about vias is when you do a layer transition
that causes a dangling stub that causes a resonance in your frequencies
of interest. The thicker the board, the lower the frequency.
Aubrey Sparkman
Enterprise Engineering Signal Integrity Team
Dell, Inc.
Aubrey_Sparkman@xxxxxxxx
(512) 723-3592
"A Measurement for every Model and a Model for every Measurement.
Without Correlation, I don't believe either." - Aubrey Sparkman
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]
On Behalf Of wolfgang.maichen@xxxxxxxxxxxx
Sent: Thursday, January 10, 2008 1:02 PM
To: Joel Brown
Cc: luant@xxxxxxxxxxx; si-list@xxxxxxxxxxxxx;
si-list-bounce@xxxxxxxxxxxxx; wolfgang.maichen@xxxxxxxxxxxx
Subject: [SI-LIST] Re: 50 Ohm Via?
Joel,
a good estimate for the prop delay is simply
T_prop = length / (speed_of_light x eps_r)
where length is the length of the via, speed_of_light is 30cm/ns (or 6
inches/ns) - make sure lengths has the same dimension (cm or inches),
and eps_r is the dielectric constant (2.5 ... 4.5 for typical PCB
materials).
For example, for a board made out of FR-4 (eps_r approx 4), Of course
that does not take into account where the signal traces attach to the
via, on the other hand you wouldn't want to have any stubs hanging off
that are even close to 1/6th of your signal rise time.
As for loosely vs. closely coupled, that depends. I would NOT recommend
leaving out the return vias simply because you have a closely coupled
differential pair. That would make your design very sensitive to any
common mode component on your signal - causing e.g. excessive EMI. There
have benn quite a few threads on this duscussion list in the past.
Regards,
Wolfgang
"Joel Brown" <joel@xxxxxxxxxx>
01/09/2008 08:30 PM
To
<wolfgang.maichen@xxxxxxxxxxxx>, <luant@xxxxxxxxxxx> cc
<si-list@xxxxxxxxxxxxx>, <si-list-bounce@xxxxxxxxxxxxx> Subject
RE: [SI-LIST] Re: 50 Ohm Via?
Wolfgang,
Your point about how much simulation is worthwhile is well taken.
I work for a small company and wear a lot of hats, I am not a full time
SI engineer. We do have some tools such as Hyperlynx and Hspice which in
my opinion have been under utilized. I know Hyperlynx claims to have
some GHz via modeling capability but I am not sure how accurate it is
and I don't think it takes the return path such as stitching vias into
account. I have been trying to do more simulation as time allows and
learning along the way.
It's certainly not easy to learn multiple simulation environments and
all the pitfalls. I have yet to get to the point to where I can
correlate measurements against simulations.
How would I know what the prop delay through a via will be?
To Chris:
I have been reading several places that recommend using loosely coupled
differential pairs, that is why I mentioned 50 ohms. I know there are
religious beliefs about tightly coupled vs loosely coupled pairs. The
material I read regarding loosely coupled pairs mentioned advantages
such as wider trace widths for a given impedance and avoiding
degradation of rise time caused by coupling between signals within a
pair.
Thanks - Joel
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]
On
Behalf Of wolfgang.maichen@xxxxxxxxxxxx
Sent: Wednesday, January 09, 2008 7:19 PM
To: luant@xxxxxxxxxxx
Cc: si-list@xxxxxxxxxxxxx; si-list-bounce@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: 50 Ohm Via?
As a simple rule of thumb:
Usually not very important if the prop delay through the via is less
than about 1/6th of your signal rise time (you may be able to get away
with 1/4th). Rise time is much more important than bit rate or clock
frequency.
As to the number of vias - this can of course aggravate the problem; but
on the other hand, I wouldn't attempt to design a 10 Gb/s channel and
put in more than maybe two vias...
just my 2 cents
Wolfgang
"Tony Luan" <luant@xxxxxxxxxxx>
Sent by: si-list-bounce@xxxxxxxxxxxxx
01/09/2008 07:06 PM
Please respond to
luant@xxxxxxxxxxx
To
<si-list@xxxxxxxxxxxxx>
cc
Subject
[SI-LIST] Re: 50 Ohm Via?
How critical the characteristic impedance of via transition is? It
depends on the bit rate, channel insertion loss and the number of vias
on each channel.=20
BR
Tony
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]
On Behalf Of Harry Selfridge
Sent: Wednesday, January 09, 2008 6:50 PM
To: 'SI LIST'
Subject: [SI-LIST] Re: 50 Ohm Via?
There was an article written about controlled impedance vias several=20
years ago by Thomas Neu of Texas Instruments. I haven't seen any=20
followup articles by anyone on the subject since. You can read Neu's=20
article online at:
http://www.edn.com/index.asp?layout=3Darticle&articleid=3DCA324403 .
Others may have experienced different results, but I've never found=20
controlled impedance vias to be necessary or useful. The distances=20
involved in a via are so short that any pretense of matching=20
impedance is negligible compared with other variations that you might=20
encounter over the full length of a signal path. One board we built=20
for a customer provided two signal paths, one with Neu's controlled=20
impedance vias, and duplicates without. Testing of the loaded board=20
showed no appreciable difference in performance, and the loss of=20
board space to the structure necessary to achieve the controlled=20
impedance vias was considerable.
Regards - Harry
At 05:51 PM 1/9/2008, you wrote:
>Is there such a thing as a design methodology for designing a PCB via
with
>50 ohm impedance, or does it have to be done iteratively using a 3D
field
>solver?
>Are controlled impedance vias necessary, worthwhile or helpful for
>multi-gigabit serial links running at 1 to 5 Gbps?
>
>
>
>Thanks - Joel
------------------------------------------------------------------
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.net
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 technical documents are available at:
http://www.si-list.net
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.net
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.net
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.net
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.net
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:
