Several
weeks ago I saw a RF circuit that scared me from the “Measurement
Repeatability” standpoint. The circuit in question had RF at one
end and DC at the other, simple enough and any number of modern
devices contain such circuits. Whether it be a Bluetooth module or a
PLL Synthesizer IC, a simple RF switch or as in this case one of
those very useful little RF Power to DC converter IC's.
The
design intent here was to make a decent RF power measurement at the
input to the circuit and then digitize the output and pass that
result on to a controller. The design was straight forward enough.
The board was laid out with a reasonable SMA edge launch connector
and passable RF trace design to the IC. What caught my eye however
was the DC portion of the circuit layout. This should have been the
easy part, but as it turns out the physical implementation of the DC
circuit had a very large impact on the circuits RF performance.
Figure
1 – A simplified representation of the physical layout is shown
above, straightforward enough, but as it turns out the DC portion of
this circuit had a very large impact on its RF performance of this
particular circuit.
The
DC output trace looked exactly like the RF input trace.
Now the RF input trace would be properly terminated by whatever is
connected to the SMA input one end and by the IC + Matching network
on the other end. If you remember your transmission line theory a
matched transmission line will have a low VSWR (also known as low
reflection) and exhibit very little amplitude ripple due to mismatch
and hence will have low measurement uncertainty.
An
improperly matched transmission line will act like a resonant
structure with the potential for an amazingly large Q. The DC output
trace was clearly the same width as the RF input trace, it was also
longer than the RF input trace (about 0.6” long). Since the operating
frequency range of the circuit was upwards of 10 GHz, this means that
the supposedly DC output trace would will likely resonate in the band
of operation. Schematically the equivalent circuit could be modeled
as in Figure 2.
Figure
2 – Above is a schematic representation of the circuit and below is
the simplified transmission line equivalent. Estimating 0.1 to 0.2 pF
of coupling across a small IC die like this seems entirely likely and
at high frequency’s will certainly be a significant amount of
coupling. The 3mm QFN also adds effective length to the circuit so it
has to be taken into to account also if one wants to simulate the
resonance peaks at the proper frequencies.
I
Hooked the circuit board up to my network analyzer and measured the
S11 and found the expected result. The input match was not well
controlled and did indeed show all the characteristics of coupling to
a high Q structure (Figure 3).
Figure
3 – The actual measured S11 (Input Match) to the circuit showed the
expected and undesired coupling. The actual measured S11 was less
than -5dB in a couple of spots. That poor of a match (under 3 dB!)
can add quite a bit of amplitude uncertainty to any measurement.
To
make sure that the coupling was indeed caused by the DC Output trace
and not some other problem, I removed the QFN and replaced it by
using two 100 ohm 0402 resistors connected in parallel to the ground
plane on either side of the RF input trace directly at the QFN Pads,
this gives a very low inductance and capacitance 50 ohm load to
analyze just the RF input trace, I also modified the input matching
to account for this. The results of just measuring the RF input trace
are shown in figure 4.
Figure
4 – Repeating the S11 measurement with the IC replaced by two 100
Ohm 0402 resistors in parallel directly at the QFN input pins shows
that the RF portion of the circuit was quite well behaved and
actually had an outstanding match all the way up to 10 GHz.
Repeating
the measurement a third time with just a 0.2 pF capacitor bridged
across the RF trace to the DC output showed essentially the same
results as figure 3, thus confirming the cause of the bad match as
the DC output trace resonating. A simulation of the transmission line
equivalent circuit of Figure 2B also showed about the same response
as the actual measurements as is shown in Figure 5.
Figure
5 – Simulating the equivalent circuit of Figure 2B and we see
essentially the same as the measured response, the first peak is at
about 4 GHz as was measured. The continued sharp resonances in the
simulation are because this simple linear simulation does not include
real PCB and circuit losses, hence the simulated Q's are higher than
actual.
Decoupling
Is The Solution
The
basic solution to this problem is to decouple the DC output trace
properly.
Step
#1 When designing the PCB in the first place, narrow the trace to a
more reasonable width for a DC signal, narrowing this trace from 20
mils to 6 mils changes it's impedance from 50 ohms to around 95 ohms.
There was simply no reason to have the DC trace the width of a 50 Ohm
line other that it: “Looked Pretty”. By making the trace narrower
it will have more loss at high frequencies and when it is a higher
impedance, it will be easier to decouple.
Step
#2 Is to keep the RF off the trace as best we can in the first place.
This can be accomplished by decoupling the DC output from the trace.
This solution can also be hacked on an already built PCB as a
band-aid.
Decoupling
essentially puts some sort of low pass filter between the IC and the
output trace to keep the RF off the trace in the first place. This
can be accomplished many ways here I will present one of my
favorites, simple RC filtering.
By
adding a simple and low cost RC Low Pass Filter as close as possible
to the IC (Figure 6), RF can effectively kept off the output trace
really reducing coupling.
Figure
6 – Modifying the original circuit by adding R2, R3, C1 & C2 to
decouple the RF energy at the IC from getting on the long output
trace and causing resonances can be accomplished by one of my
favorite techniques shown above. I size the resistors and capacitors
based on the technology that the majority of the rest of the design
is using, normally this means either 0603 or 0402 sized parts.
Figure
7 shows the measurement results of this simple addition when it was
hacked on to the test PCB.
In
circuits like Figure 6 shows I usually start with 200 to 511 Ohm resistors
as they are relatively flat over a large frequency range such as this
and the largest COG capacitor I can find in whatever size the design
is using, in this case it was a 1000 pF / 0603 Sized part. COG
Temperature coefficient parts typically have better RF Performance
because of lower losses.
The
circuit of Figure 6 also adds a voltage divider that must be taken
into account in the overall final design, in this case the A/D's gain
was adjusted to compensate for the extra drop across the two 511 ohm
resistors. Simulation also showed that the resistors can be made
about 200 ohms each with nearly the same decoupling result.
Of
note: Normally we would like to add a capacitor directly at every DC
pin on the IC, but this particular pin is an OPAMP output and we
don't want to make the OPAMP unstable with the addition of a
capacitor directly at it's output.
Finally
to test the decoupling circuit itself to make sure that no unruly
resonances are occurring there, I connected SMA cables to both sides
of the DC output trace and did a S21 through line measurement. The
results shown in figure 8 show a nicely damped response with no funny
resonances.
Variations
on a Theme
There
are naturally as many possible variations on making a suitable
decoupling network as there are designers and there are many
different circuit requirements too. For instance, the RC decoupling
circuit of Figure 6 would not work very well for a DC bias line as it
would produce a lot of voltage drop when the current get's into the
MilliAmp range. Likewise the 3dB bandwidth of Figure 6 is just a
little over 100 kHz, so using this decoupling network on a I2C or SPI
line won't work very well either unless the clock frequency is very
low. So there are many requirements to consider before selecting the
actual circuit values.
Figure
7 – Adding Figure 6's decoupling to the original circuit tamed
resonance on that long and wide DC trace to a very reasonable level,
there is still coupling but the input Match is much more well behaved
(Better than 17 dB everywhere). All this without even touching the
actual input trace or match at all.
Figure
8 – S21 Measurement of the through response from one side of the
long DC trace to the other shows a nicely damped response with no
troublesome resonances anywhere. The reason the response is rising instead of falling is because at high frequencies the 1000 pF decoupling capacitors are actually inductive because of the package parasitics. 0402 Sized parts have less package inductance and for higher frequency circuits may be more appropriate.
Appendix:
Sometimes finding the culprit resonance is not so easy
Sometimes
it is not clear on a complex PCB what is causing the problem
resonances, in these cases a bit of detective work is required.
Remember that a poorly terminated transmission line will resonate
when the frequency reaches a quarter wavelength and every quarter
wavelength after that it will resonate with the opposite impedance.
Start
off by measuring the resonant peak frequency or if multiple peaks, the
delta frequency between peaks, then calculate the transmission line
length that will give these frequency peaks and start looking for
trace lengths on the PCB that match the calculation and pretty
rapidly you will find the culprit. Sometimes you can also use the "Move your finger around touching things" method.
If
your frequency sweep is from a low frequency and your circuit
is fine, then suddenly there is a resonance, you are probably
seeing a first quarter wavelength effect (Also see Reference [1]).
On
the other hand if you are sweeping across some very high frequency
band and you see some repeating ripple pattern then you are probably
seeing a one half wavelength effect. At every half wavelength the
impedance of "whatever" that is resonating will circle around to the
same impedance again, hence giving rise to a repeating pattern.
In
practice I have found problems in the range of 7 inches for a cable
that ran off the PCB and then back on again causing a resonance to
traces like this example PC that were a few tenths of an inch long.
Some common approximate frequencies and quarter wavelength for Microstrip on FR4 are given in the table below,
The Table can be written as a formula like,
-
Where the Microstrip quarter wavelength on FR4 is in inches and F is the frequency in GHz.
Where the Microstrip quarter wavelength on FR4 is in inches and F is the frequency in GHz.
Figure
A.1 – As an example of the kind of repeating pattern that can be
seen on a transmission line. Here an open circuited line was
simulated. The Y axis here is Impedance Magnitude in Ohms and the X
Axis is frequency.
The
blue arrows on the bottom mark off ¼ wavelengths. As can be seen, a
open circuit transmission line resonates every ¼ wavelength but the
impedance at each ¼ wavelength goes from high impedance to low
impedance and back again.
The
red arrows at the top mark off ½ wavelength segments. On this open
circuited line the ½ wavelength repeating pattern is at a very high
impedance and there is also a repeating ½ wavelength pattern at low
impedances (the peaks on the bottom of the graph, not marked).
As
a note, a short circuited line has exactly the same pattern, it is
just reversed in impedance. That is, instead of starting at a high
impedance at low frequencies, it starts at a low impedance and the
first ¼ resonant peak is at a high impedance, not the low impedance
shown here. Then the pattern repeats the same as for this simulation.
The simulated response shown in Figure A.1 is for some randomly selected line length. Note that a longer line would produce peaks closer together while a shorter line would produce peaks that are farther apart.
The simulated response shown in Figure A.1 is for some randomly selected line length. Note that a longer line would produce peaks closer together while a shorter line would produce peaks that are farther apart.
References:
[1]
A resonance effect on a RF circuit can also be caused by any
shielding or box that the circuit is put into. You can read more
about that here,
By: Steve Hageman www.AnalogHome.com
We design custom: Analog, RF and Embedded system for a wide variety of industrial and commercial clients. Please feel free to contact us if we can help on your next project.
This Blog does not use cookies (other than the edible ones).
This Blog does not use cookies (other than the edible ones).
