- 积分
- 38
- 兑换点
- 点
- 声望度
-
- 金钱
- 元
- 银行存款
- 元
- 贡献度
-
- 精华
|
楼主 |
发表于 2002-8-8 15:31:00
|
显示全部楼层
Differential Trace Impedance
*-----------------------------------------------------*
High-Speed Digital Design
*On-Line Newsletter*
Dr. Howard Johnson, Vol. 5 Issue 2
*-----------------------------------------------------*
A RARE EVENT -- YOU MAY BENEFIT
A rare, last-minute cancellation has opened a window
in my schedule for private seminars. A private
seminar gives you and your co-workers a perfect
opportunity to learn the latest in high-speed
digital design within the context of YOUR designs.
If you are located in the Southwest US and have
30 or more digital engineers at your site, please
write to hsdd@sigcon.com by Feb 15 for more
information about this opportunity.
*----------------------(QUESTION)---------------------*
Differential Trace Impedance
Mitch Morey, San Diego, CA
I'm working on a board with 100-ohm differential
signaling that I would like to design for
microstrip routing. I've used the Polar Instrument
calc, the ADS LineCalc software, and have got two
additional stackup constructions for our fab
houses, and have talked to numerous people on this.
Here are the recommendations I have gathered so
far. All configurations represent
- 100-ohm differential microstrips,
- operating at 2.4Ghz speeds,
- using a 5mil-thick FR4 dielectric,
- with an underlying solid copper reference plane.
.005" lines with .005" edge to edge (fab shop 1)
.004" lines with .008" edge to edge (fab shop 2)
.005" lines with .008" edge to edge (ADS LineCalc)
.006" lines with .0065" edge to edge (ADS LineCalc #2)
.016" lines with .016" edge to edge (engineer #1)
etc. etc.
???**!!*!???
*--------------(REPLY FROM DR. JOHNSON)---------------*
Thanks for your interest in High-Speed Digital
Design.
What you need is a piece of software called a two-
dimensional E&M field solver. This program
calculates the magnetic and electric fields
surrounding your traces, and from that data
extracts the impedance and delay. This is the best
way to do impedance calculations. The good field
solvers allow you to specify the trace width,
height, spacing, thickness, dielectric constant,
AND they allow you to overlay the trace with a
solder-mask layer.
I'm not sure what ADSlinecalc uses, but if it's not
a two-dimensional field solver you shouldn't trust
its results. I have reason to distrust the accuracy
of the examples you have provided.
First let me give you some general principles to
help you understand what's happening and then I'll
rule out a couple of the solutions below.
The first thing you need to know is that the
patterns of electric field lines in a dielectric
medium follow the same shapes as patterns of
current flow in solid conductors. This sounds
pretty obtuse, but it's going to help you in a
major way, because it will help you SEE what is
happening when you change the trace geometry.
Follow me for a minute on this mental experiment.
Start with a microstrip trace of length X. I want
you to mentally replace the dielectric medium
surrounding this trace with a slightly conductive
solid material. Now imagine that you connect an
ordinary ohmmeter between the trace and the ground
plane. The value of DC resistance you measure in
this experiment will be exactly proportional to the
IMPEDANCE of the trace. I hope you can now imagine
what would happen if you press the trace closer to
the ground plane. Can you see that the impedance
must go DOWN, because there is now less material
between the trace and the reference plane? If the
trace is pressed down to the point where it nearly
touches the reference plane, its resistance to
ground (i.e., impedance) approaches zero.
What about doubling the width? This adjustment
practically doubles the conductive surface area,
substantially lowering the resistance to the
reference plane (i.e., impedance). I like using
this DC analogy because most engineers find it a
lot easier to imagine simple patterns of DC current
flow than they do high-frequency electromagnetic
fields. The constant of proportionality isn't
important -- I just want you to see what's going to
happen as you make various adjustments.
So far I've shown two things that decrease the
impedance in microstrips:
(1) Moving a trace closer to the reference
plane decreases its impedance.
(2) Fattening a trace (i.e., increasing its
width) decreases its impedance.
And the converse statements are also true,
(3) Moving a microstrip further away from the
reference plane increases its impedance.
(4) Shaving down the trace width increases
its impedance.
Stripline traces are a little more complicated in
that you must account for the distance from your
trace to both top and bottom reference planes. The
general result for offset striplines is that
whichever plane lies closest to the trace has the
most influence on the impedance. Smack in the
middle the planes are both equally important.
Let's now imagine a differential configuration with
TWO traces. Connect the ohmmeter BETWEEN the two
traces (from one to the other). The resistance you
read now will be proportional to the DIFFERENTIAL
impedance of two-trace configuration. [NOTE: one-
half the differential impedance is DEFINED as the
odd-mode impedance.]
If your two traces are set far apart, and they have
the same dimensions as in the first experiment,
your new differential measurement will be exactly
TWICE as great as before. If you draw out the
patterns of DC current flow you can see why. For
*widely* separated traces the current flows mostly
from one trace straight down to the nearest
reference plane, then it shoots across the plane to
a position underneath the second trace, and from
there it leaks back up to the second trace. As this
current flows, it encounters a resistance R1 when
leaving the first trace, practically zero
resistance flowing across the plane, and then
another amount R1 as it flows back up to the second
trace. The total resistance encountered is 2*R1.
(5) The differential impedance of two widely
separated traces equals twice the impedance
to ground of either trace alone.
Now let's see what happens to the differential
impedance as you slide the two traces towards each
other. When they get close enough, significant
amounts of current begin to flow directly between
the traces. You still get the same old currents
going to and from the reference plane, but in
addition to those currents you have now developed a
new pathway for current, direct from trace-to-
trace. This additional current pathway acts like a
new resistance in *parallel* with the original,
widely-spaced current pathways. The new parallel
pathway lowers the differential impedance of the
configuration. You may conclude:
(6) The differential impedance of a tightly-
spaced pair is less than twice the impedance
to ground of either trace alone.
If the traces are moved so close that they nearly
touch, the differential resistance (impedance)
approaches zero. In general, the differential
impedance is a monotonic function of the trace
separation.
(7) All other factors being equal, the
tighter the inter-trace spacing, the less the
differential impedance.
I view any decrease in impedance as an annoying
side-effect of close spacing. If I could re-design
the universe, I'd try to make it not happen.
Fortunately, you can counteract the annoying drop
in impedance by shaving down the width of your
traces. If you shave off just enough width you can
push the impedance back up to where it belongs. In
this way, the trace separation and trace width can
be made somewhat interchangeable.
(8) To maintain constant impedance, a
reduction in spacing must be accompanied by a
reduction in trace width (or an increase in
trace height).
With these eight rules in mind, let's now look at
the specific recommendations you have been given.
With your 5-mil dielectric, the individual
impedance of a 16-mil trace on FR-4 already falls
below 50 ohms, so the differential impedance will
be less than 100 ohms regardless of what spacing
you use. You can there rule out the 16-mil
configuration. I suspect your engineer #1 may have
been thinking about using a thicker dielectric than
what you propose.
The two ADSlinecalc results conflict with each
other. Staring from a pair 5-mil wide with an 8-mil
space, INCREASING the trace width to 6 mils will
lower the impedance, and DECREASING the spacing to
6.5 mils will lower it even further. Therefore, one
of these results must be wrong. They cannot both be
100-ohm solutions. Therefore, I suspect something
is either wrong with your copy of ADSlinecalc, or
(dare I say it) your use of the tool.
Here's some data from a commercial 2-D field solver
(HyperLynx). All these combinations should give you
a 100-ohm differential microstrip impedance under
the following conditions:
- Dielectric thickness = 5 mil
- Relative permittivity at 1 GHz = 4.3
- Trace thickness = 1/2-oz cu + 1-oz plating
(1.5-oz total)
- No solder mask (***when your vendor adds
solder mask he or she will somewhat reduce the
trace width to compensate for the extra
dielectric material above the traces.
Each combination is listed as a pair [xW, yS],
where x is the finished, plated trace width in
mils, and y is the finished, plated edge-to-edge
separation in mils.
100-OHM DIFFERENTIAL MICROSTRIP DIMENSIONS
( All at h=0.005", Er=4.3. 1.5-oz Cu.
w s
8 14
7 11
6 7
5 5
Whatever you choose to do, insist that your board
fabrication shop place differential impedance test
coupons on your panels and test each one to verify
that you are getting the correct impedance.
Below I have attached a listing of 100-ohm
stripline configurations. Obviously, this is just a
small sampling of all possible combinations. In the
chart, dimension "b" is the interplane separation,
"h" the height of the trace above the nearest
plane, "w" the trace width, and "s" the edge-to-
edge separation, all in mils. Parameter rSKIN is
the effective AC skin-effect resistance at 1 GHz,
Z0 is the (high-frequency value of) characteristic
impedance, and the column marked "dB/in. @1GHz" is
the trace attenuation due to the skin effect, in
dB/in., at a frequency of 1 GHz. Don't forget to
also consider dielectric losses. All the stripline
configurations assume 1/2-oz Copper on an FR-4
substrate with Er=4.3 at 1GHz.
I hope this information is useful to you.
Best Regards,
Dr. Howard Johnson
100-OHM DIFFERENTIAL STRIPLINE DIMENSIONS
( All at Er=4.3. 1/2-oz Cu.)
b h w s rSKIN Z0 (dB/in.@1GHz)
10 3 3 40 3.501 99.03 0.1522
10 4 3 7 3.235 100.4 0.1389
10 5 3 7 3.218 101.2 0.1371
10 5 4 40 2.76 94.59 0.1258
14 4 3 5.5 3.191 101 0.1361
14 4 4 12 2.738 100.3 0.1177
14 5 3 4.5 3.136 100.1 0.135
14 5 4 7.5 2.599 100.5 0.1116
14 5 5 40 2.329 99.51 0.1011
14 7 3 4.5 3.112 101.8 0.1317
14 7 4 6.5 2.556 100.6 0.1096
14 7 5 13 2.236 100.9 0.09574
14 7 6 40 2.006 94.98 0.09126
20 5 3 4.4 3.141 101 0.134
20 5 4 6.5 2.592 100.7 0.1111
20 5 5 11 2.271 100.6 0.09746
20 5 6 40 2.087 98.41 0.0916
20 7 3 3.9 3.132 101.1 0.1336
20 7 4 5.2 2.547 100.9 0.1089
20 7 5 7 2.165 100.7 0.0929
20 7 6 10 1.908 100.3 0.08218
20 7 7 19 1.75 100.7 0.0751
20 7 8 40 1.613 96.34 0.07242
20 10 3 3.7 3.143 100.6 0.1347
20 10 4 5 2.54 101.6 0.1079
20 10 5 6.5 2.148 101.4 0.0915
20 10 6 8.5 1.876 100.7 0.08054
20 10 7 12 1.682 100.5 0.07236
20 10 8 25 1.562 100.3 0.06735
30 5 3 4.3 3.147 100.7 0.1347
30 5 4 6.3 2.595 100.7 0.1112
30 5 5 10 2.268 100.7 0.09729
30 5 6 22 2.087 100.2 0.08996
30 6 3 4 3.139 101 0.1339
30 6 4 5.4 2.564 100.7 0.1099
30 6 5 7.5 2.195 100.7 0.09415
30 6 6 11.2 1.955 100.6 0.08399
30 6 7 20 1.81 100.4 0.07795
*-----------------------------------------------------*
Join our next public seminar:
San Jose, Feb. 4-5, 2002.
A full schedule of our public seminar cities and
dates appears at http://signalintegrity.com. Register
today!
If you have an idea that would make a good topic
for a future newsletter, please send it to
hsdd@signalintegrity.com.
To unsubscribe from this list: send an email to
hsdd@sigcon.com with "unsubscribe" in the subject
line. To subscribe to this list: send an email to
hsdd@sigcon.com with "subscribe" in the subject
line. Include your name and email address in the
body of the message. (NOTE: If you received this
message, you do not need to re-subscribe.)
Newsletter Archives:
http://www.sigcon.com/newsletter.htm
Copyright 2002, Signal Consulting, Inc.
All Rights Reserved. |
|