What are microstrips and how are they used in PCB designs？Robert
sheds some light on the topic of microstrips and describes
microstripping techniques that you can use at your workbench.
Welcome back to The Darker Side. This month， I am really a happy
guy because I have achieved two of my goals. First， it should
please my editors because I will present a subject in line with
Circuit Cellar‘s monthly theme， which is， if you haven't read the
cover， wireless communications. Second， the title of this column
has never been more appropriate，because I will talk about something
that may really seem magical to the novice. Follow along as I
introduce microstrip techniques and explain how to implement
zero-cost components by simply drawing PCB tracks.
BACK TO IMPEDANCE MATCHING
In "Antenna Basics，" I explained why impedance matching can make
the difference between a working and a nonworking project，
especially in RF designs where signal power is an expensive
resource （Circuit Cellar 211，2008）。 In a nutshell， the power
transfer between a source and a receiver is maximized when
impedances are matched. This means that the source impedance is the
complex conjugate of the load impedance. Both resistances are equal
and both reactances are equal in value， but with opposite signs.
Roughly speaking， a capacitive load must be matched with an
inductive source and vice versa. If the source impedance is a 50-Ω
pure resistance，matching will be achieved when the load is also a
pure 50-Ω resistance. And if a cable or wire is used between them，
it must also have a 50-Ω characteristic impedance. If the matching
is not perfect， you won‘t get as much power as you could： some
power will be dissipated somewhere else than in your load. It is
usually reflected back to the source and dissipated， but it could
also generate nasty effects like distortion or spurious signals.
You must be concerned with impedance matching， especially in any
high-frequency project， and 90% of the time you should try to keep
a 50-Ω characteristic impedance through your circuit， or may be 75
Ω if you are working on video. Do you know where these usual 50-
and 75-Ωvalues come from？ I must admit that I discovered the
supposed explanation only recently in Thomas H. Lee‘s book， Planar
Microware Engineering： A Practical Guide to Theory， Measurement，
and Circuits. According to Lee， for a given coaxial cable
diameter，there is a precise ratio of inner to outer conductor size，
which gives the minimum intrinsic resistive loss. This ratio
corresponds to a characteristic impedance of 77 Ω。 That's why a
close value，75 Ω， is used for video where signals are small and
where attenuation should be kept as small as possible， even on long
cables. Okay，but why 50 Ω elsewhere？Because there is another
optimization to deal with. A coaxial cable can transmit a given
maximum peak power，corresponding to the dielectric breakdown of the
cable due to high RF voltages. It happens that， for a fixed
external size，this power-handling capacity is maximized with
another ratio of inner to outer conductor size， corresponding to a
characteristic impedance of 30 Ω， at least when air is used as a
dielectric. Back in the 1930s， engineers hesitated between 77 and
30 Ω and chose an intermediate value for common coaxial cables， 50
Ω。 To be honest， there are other explanations on the ‘Net， but this
one seems plausible.
TRANSMISSION TO MICROSTRIPBefore digging into the microstrip topic， let's spend a minute on
transmission lines. （see Figure 1）。 If you ignore parasitic
resistances， each section could be modeled as a small serial
inductance，because any wire has a nonnull inductance，and as a small
capacitor between the wire and the ground， because the central wire
is not far from the grounded shield. These parasitic inductances
and capacitances are roughly proportional to the length of the
small section，so they can be noted L.dZ and C.dZ， with L and C in
henries per meter and farads per meter. Therefore，the wire can be
approximated as a serially connected set of identical L.dZ/C.dZ
networks. If you apply a voltage on one end of the cable， some
current will flow until all capacitors are charged. If you are，
well， rich and have an infinite length of cable， this current will
flow forever. And if you apply an AC input， you will get a given
impedance. This impedance is what is called the cable‘s
characteristic impedance. In fact， it can be easily demonstrated
that this characteristic impedance is simply the square root
Imagine you have a piece of coaxial cable divided into a large
number of small sections， each of length dZof L/C. Just remember
that the characteristic impedance of the cable increases with L and
decreases with C.
Figure 1-A transmission line can be modeled as a succession of
small L/C networks. The mathematical relationship between the L and
C parameters and the characteristic impedance of the line is simple
to apply and slightly more complex to demonstrate.
What happens if you do not have a coaxial cable but simply a copper
track on a side of a PCB with a complete ground plane on the other
side？ The situation is the same as it is with the coaxial example.
The track can be split into small sections， and each section can be
modeled the same way. So， this track will have a characteristic
impedance. Such a PCB track on a full ground plane is called a
microstrip， which is the most common way to connect RF components
on a PCB（see Figure 2）。 You can use other settings like
stripline-which is a track sandwiched between two ground planes on
a multilayer PCB-but microstrip is the most frequently used option
because it is affordable and well-suited to SMT components.
How do you control the characteristic impedance of a microstrip
track？ Usually with the only parameter that you can easily manage
on your PCB CAD tool： track width. Intuitively， if the track is
wider，the capacitance between the track and the ground plane will
increase and the characteristic impedance will decrease. If the
track is thinner， its inductance and its characteristic impedance
will increase too. So， there should be a given track width that
corresponds exactly to 50 Ω，at least for a given PCB technology.
This width is dependent on the PCB substrate（FR4 is the most
common） through its dielectric constant and the PCB thickness（1.6
mm or 0.8 mm for double-sided designs） and slightly on the copper
thickness，which is 35 μm most of the time. The formula and the
usual values are given in Figure 2， even if there are good free
calculation tools on the 'Net， such as Agilent Technologies AppCad
（see Photo 1）。 Roughly a 50-Ω track corresponds to a 3-mm wide
track on a standard 1.6-mm thick PCB and to 1.5 mm on a 0.8-mm PCB.
That‘s why it is often more appropriate to use a 0.8-mm thick PCBs
for RF projects， simply because the tracks have a more manageable
width. In summary， whenever you design a highfrequency project， you
must always use tracks with the width for proper impedance matching
with a full ground plane on the opposite layer. The only exception
is when the length of the track is short，compared to the signal‘s
wave length （e.g.，a couple of millimeters， as in case impedance
matching may be neglected）。
A word of caution. Be careful if you use a multilayer PCB. The
track width will need to be calculated based on the distance
between the microstrip track and the ground plane， which is usually
on the first inner layer. Ask your PCB supplier for the actual
distance because this could be process-dependent. Also remember
that the standard FR4 PCB substrate has a fuzzy dielectric constant
（specified as±10%） and high losses， which make it difficult to use
when the working frequency exceeds a couple of gigahertz. Specific
high-frequency substrates （e.g.， Rogers RO4003） are much more
efficient and well characterized， but this has a cost （see Figure
2）。
DISTRIBUTED COMPONENTSNow you know how to calculate the width of a PCB track to get a
precise 50-Ω impedance. But what happens if you have a
50-Ωmicrostrip track and you increase or decrease its width on a
small length？ Remember the transmission line L/C model？ If you
decrease the track width， you will create a small section with a
higher impedance，which is roughly equivalent to a serial
inductance. And if you increase it， you will create a section with
a lower impedance corresponding to a parallel capacitor to ground！
Figure 3 shows how zerocost L or C can be integrated on a
microstrip design；it also shows how to calculate their values.
Usually， the impedance of the small section is arbitrarily fixed to
the largest or smallest value corresponding to a reasonable track
width， often around 10 or 20 Ω for capacitors and 100 to 200 Ω for
inductors. The track length calculation is based on this hypothesis
and the desired component value thanks to the supplied formulas.
You need to be careful for two reasons. One， the dielectric
coefficient used in the formulas is not the raw dielectric constant
of the substrate found in the supplier‘s datasheets，but the
effective dielectric constant of the microstrip wire， which is
between the substrate and the air with a slightly different
behavior. The formula and usual values are provided in Figure 2.
For example， the dielectric constant of FR4 is around 4.5， but the
effective dielectric constant of a microstrip on FR4 is 3.38.
Two， you must remember that I took the hypothesis of "small
sections" of a track for this discussion. What does it mean in
practical terms？ Simply that the L/C model will be erroneous as
soon as the track dimensions （width or length） are not
significantly small compared to the wavelength of the signal you
are working on. This wavelength is the speed of the signal on the
PCB track divided by the working frequency. The signal speed is c
（the speed of light， 3.108 m/s） divided by the square root of the
effective dielectric constant. For example，this corresponds to a
wavelength of 6.7 cm at 2.4 GHz on FR4. At that frequency， you can
expect to have issues as soon as the component‘s dimension is
larger than 1 cm or so. This fixes a limit to the value of the
components you can design in microstrip form.
NEED A ZERO-COST FILTER？Enough theory. Now it‘s time for some funny experiments. What could
you do with L and C devices？ You can try to design a 50-Ω 1-GHz
low-pass filter with absolutely no discrete components. Such a
filter would be made only with specific copper tracks on the PCB，so
its cost would be virtually null， at least if you consider PCB
surface as free. The first step is to design the filter as if you
were using classical lumped components. Because I‘m lazy from time
to time， I used a free online filter calculator developed by Tony
Fisher at The University of York. The result in Figure 4 includes
three inductances （9.12， 15.7， and 9.12 nH） and two 4.36-pF
capacitors. The 3-dB cut-off frequency is precisely 1 GHz. The
calculated attenuation at 1.5 GHz is around 20 dB. You can build
this filter using standard components. It will work if you are
lucky enough to find a 9.12-nH inductance somewhere.
点击查看Figure 4How can you transform these values into microstrip components？
Let's assume that the PCB will be a standard 1.6-mm， double-sided
FR4 substrate. Figure 2 indicates that the width of a 50-Ω track is
a little less than 3 mm. To build the inductors，you need to use a
thinner track with any arbitrary but convenient track width， say
100 Ω， which corresponds to a width of 0.678 mm. You then just have
to calculate the corresponding lengths， thanks to the equations in
Figure 3. With this 100-Ω track， the 9.12-nH value can be achieved
with a track length of 14.62 mm， and 15.7 nH corresponds to 25.16
mm. Similarly，for the capacitors， you must select an arbitrary
small impedance value，say 15 Ω， which corresponds to a track width
of 15.2 mm， and the calculated track length for 4.36 pF is 10.48
mm. The final mandatory phase is to check that the largest
dimension of the components is reasonably smaller than the
wavelength of the highest frequency you are working with. Here， the
largest length is the capacitor length，around 2.5 cm. You already
calculated that 2.4 GHz was safe up to dimensions of 1 cm. So， you
can expect the filter to work correctly at 1 GHz， but it may start
to be a little far from the predictions at frequencies of 2 to 3
GHz and higher.
The next step is to simulate the filter design. With RF designs， a
simulator phase is always less expensive than some tens of PCBs
thrown to the garbage bin. You have a couple of options for the
simulator. The simplest solution would be to use a circuit-only
simulator， which has provisions for microstrip models， such as the
free，useful QUCS simulator. It is efficient and easy， but the
disadvantage is that you won‘t get a drawing of the physical
microstrip design. At the other extreme， you can use a
full-featured 2- D or 2.5-D electromagnetic simulator，such as
Sonnet Software， which has a free Sonnet Lite version that can be
used for designs as simple as this one. Results will be accurate，
but the tool's complexity and calculation time are significantly
higher. I like an intermediate approach： PUFF. This old DOS-based
simulator is based on circuit models rather than EM simulation， but
it includes a pretty graphical input of the microstrip design.
Moreover， it is nearly free because it comes with a couple of
books. It runs well in a DOS box under Windows XP； but
unfortunately， I wasn‘t able to make a screen copy， so you have
only Photo 2. The layout windows are a graphical representation of
the filter design， with a 50-Ω track on both ends and a succession
of thin， inductive， and wide capacitive segments. The simulation
took just 5 s on my standard PC and shows a good 1-GHz lowpass
behavior but with a drastically reduced attenuation of around 3.5
GHz. A tool like PUFF can't explain why， but you already know the
answer. At such a high frequency， the circuit dimensions are no
longer "small" compared to the wavelength and it‘s likely a given
track of the filter forms a tuned resonator at exactly 3.5 GHz. By
the way， you can use a tool like Sonnet Lite to find it out. With
the current density plot feature， a Sonnet design file is posted
for your convenience on Circuit Cellar's FTP site.
I couldn‘t resist the pleasure of building and testing this filter.
Look at the PCB in Photo 3. You should be able to recognize the
successive L， C， L， C， and L sections. I soldered two SMA
connectors for the test， and voila， the filter was ready. I hooked
it on my old Hewlett-Packard HP8754A/H26 vectorial analyzer， which
has a measurement range of 4 MHz to 2.6 GHz （see Photo 4）。 Quite
nice， isn't it？ I measured the 3-dB cut-off frequency at 1，030 MHz，
close to the specification. The attenuation at 1.5 GHz is a
reasonable 18 dB. I had to switch to a different test setup to
evaluate the performances of the filter at frequencies above 2.6
GHz. I used an even older Hewlett-Packard HP8620C microwave sweeper
with a 2- to 8.4-GHz plug-in connected to the input of the filter，
and a Hewlett-Packard HP8755 scalar analyzer on its output. The
result I got is in Photo 5. The first odd behavior was measured at
3.47 GHz with an unwanted peak response， exactly as expected
through the PUFF simulation. At higher frequencies， the filter was
no longer filtering anything. This was anticipated. Theoretical
analysis showed that the filter dimensions were starting to be too
large compared to the wavelengths.
I hope you are as pleased as I was when I saw that the actual
performances were so close to the simulation， at least up to 4 GHz！
I must admit that this was the first time I saw actual results so
close to the simulation. I was encouraged by this experiment， so I
checked another aspect of microstrip circuits with the test PCB
shown in Photo 6. Textbooks explain that a 90° turn on a microstrip
track must have a precisely calculated chamfered corner to keep the
impedance under control. This is understandable. If you design a
nonchamfered 90° turn， there is some "extra"
copper on the corner， which acts as a small capacitor， which
impacts performances. My test PCB included two identical 50-Ω
tracks on an FR4 substrate， one with chamfers and one without. I
tested it with the same two test setups as the 1- GHz filter and
was a little disappointed. There was no visible difference between
both designs up to 4 GHz. However， I then tested them at a high
frequency thanks to a 12.4- to 18-GHz plug-in I bought years ago
for my HP8620C. I admit that trying to use an FR4 PCB at 18 GHz is
a little risky， but it enabled me to see an impressive difference
between the two versions. Refer to Photo 7 to see why you should
always use chamfered corners on microstrips.
点击查看Photo 7WRAPPING UPObviously， microstrip designs are unnecessary for a standard
low-speed microcontroller design. However， knowledge of PCB track
impedance matching rules is mandatory when dealing with a large
number of high-speed digital boards. Your gigahertz-clocked PC
probably won‘t work without impedance- matched tracks. And， of
course，their use is mandatory for RF designs.
"At which minimal frequency should I start to be worried about
track impedance matching？" That's a common question. The easiest
way is to compare the wavelength of the signal and the length of
the longest track on your PCB. If the wavelength is far longer than
your PCB dimensions，then you can usually safely ignore track
matching. However， if you have a track that starts to be close to
the wavelength you are working on， then you‘d better take care and
use impedance matching. Take the example of a classic 10-cm track
on FR4. If you consider "safe" as a factor of 10， then you should
use matched tracks as soon as the wavelength on FR4 is shorter than
1 m （i.e.， 10 × 10 cm），which corresponds to a wavelength in the air
of 1 m times the square root of the 3.38 effective dielectric
constant. The result is 1.84 m， which corresponds to a frequency of
300，000，000/1.84 = 163 MHz. Do you use signals faster than about
150 MHz？ If so， I hope that microstrips are no longer on the darker
side for you.
Robert Lacoste lives near Paris， France. He has 18 years of
experience working on embedded systems， analog designs，and wireless
telecommunications. He has won prizes in more than 15 international
design contests. In 2003， Robert started a consulting company，
ALCIOM， to share his passion for innovative mixed-signal designs.
You can reach him at rlacoste@alciom. com. Don‘t forget to write
"Darker Side" in the subject line to bypass his spam filters.
PROJECT FILESTo download code, go to
ftp://ftp.circuitcellar.com/pub/Circuit_Cellar/2009/223.
RESOURCESD. Brooks, "Embedded Microstrip: Impedance Formula," Printed
Circuit Design, 2000.
T. Lee, Planar Microware Engineering: A Practical Guide to Theory,
Measurement,and Circuits, Cambridge University Press, Cambridge,
U.K.,2004.
The University of York Department of Computer Science, "LC Filter
Design calculator," www-users.cs.york.ac.uk/~fisher/lcfilter.
SOURCESAppCad
Agilent Technologies, Inc.
www.hp.woodshot.comPUFF Microstrip layout and simulator
California Institute of Technology RF and Microwave Group
www.its.caltech.edu/~mmic/puff.html
HP8620C Microwave sweeper, HP8754A/H26 vector network analyzer,and
HP8755 scalar analyzer
Hewlett-Packard
www.hp.com
Qucs project
Qucs team
http://qucs.sourceforge.net
RO4003 Substrate
Rogers Corp.
www.rogerscorp.com
Sonnet Lite
Sonnet Software, Inc.
www.sonnetsoftware.com/products/lite
;){kind=link}