This article is based on a presentation I held at a seminar
and BK Services in
Linköping 2012-10-01. The presentation described some findings from
research I did at SP Devices.
The presentation slides (in Swedish)
Filtering of Power Supplies for Sensitive Analog Applications
While this article describes a circuit solution to a power supply
filtering problem, I think the main value of it is not the specific
solution arrived at, but rather the methods used to get there as well
as some general insights about how some components and circuits behave
and how to utilize or mitigate that behavior.
The method I use consists of both simulations (in LTspice) and
measurements using a network analyzer.
The solution is far from universally applicable since different
applications have vastly different requirements in terms of current
capability, maximum voltage drop allowed, amount of filtering
required, cost, size etc. The methodology and general observations
here are however hopefully more or less universally applicable to this
kind of problem.
Sometimes a power supply rail is needed that has very little noise *)
on it. Such a supply rail may be required to improve the performance
- Analog-to-digital converters
- Radio frequency circuits
- Phase-lock loops
Switching AC/DC and DC/DC converters are often used to generate
supply voltages in today's electronics, largely because they provide
good efficiency even when the difference in input voltage to output
voltage is big. These switchers are however notorious generators of
noise, typically in the frequency range from a few hundred kHz up to
at least several tens of MHz.
Figure 1 below shows the spectrum of noise present on a supply
generated by a DC/DC-converter switching at 280 kHz. As can be seen,
the noise extends out to at least 100 MHz and it is composed mainly of
harmonics of the 280 kHz switching frequency.
Figure 1. Noise spectrum from a 280 kHz DC/DC
converter. (Click to enlarge.)
Other noise sources such as the mains AC frequency, variations in the
mains voltage, I*R or L*di/dt drop modulated by fluctuating current
consumption in the system can contribute disturbances with frequency
components from less than a Hz and up to very high frequencies.
Linear regulators provide cleaner outputs than switching regulators,
but typically requirements on size, cost and power consumption often
mandate the use of switching regulators in the system. So in order to
provide a sub-circuit with a clean supply voltage, one is often faced
with the problem of cleaning up the output of a swicthing converter.
How can this be done?
*) By noise I here mean both random noise as well as deterministic
noise from e.g. DC/DC-converters, fluctuating mains voltages,
perturbations generated by varying current consumption etc.
There are a number of different strategies that one could follow to
try to filter out the noise while maintaining a nice low-impedance
supply rail. The two most obvious methods are perhaps LC-filters and
linear regulators. LC-links can be configured as low-pass filters and
attenuate higher frequencies while letting lower frequencies through.
Linear regulators on the other hand generally have good supply
rejection at low frequencies, while the rejection deteriorates as the
frequency increases. A combination of an LC-filter and a linear
regulator therefore seems like a good candidate solution to the
In order to test how well different configurations perform, I
designed and built a test board that would allow me to use a (vector)
network analyzer (VNA) to measure the filtering performance of a
circuit aimed to deliver a low-noise 400 mA, 5 V supply. (A spectrum
analyzer with a tracking generator would have worked as well as a VNA
in this case as we are not interested in the phase of the transfer
function.) Other requirements in this case was low cost and small size
while high efficiency was not a major concern, so I could allow a few
volts of drop over the filtering circuitry.
The schematic and layout of the test board are shown in figures 2-4
Figure 2. Schematic of test board (click to enlarge).
Figures 3 and 4. 3D rendering and photo of test
board. The grayed-out parts of the board are not treated in this
article. (Click to enlarge.)
The board consists of:
- an input power connector isolated from the filtering circuitry by a
shunting capacitor and a big series inductor. The idea here is that
the lab supply that is used to power the test board shall not affect
- two AC-coupled coaxial connectors that allow a good high-frequency
connection of the VNA to the input of the filter. The reason that
there are two connectors is that we need to first measure how much
signal the VNA is able to inject at different frequencies in this node
so that we know the actual amplitude of the signal here and can
divide that from the signal observed further down the filter chain
to obtain the true transfer function in terms of voltage out/voltage
- an LC-link based on a power inductor and two ceramic capacitors. A
resistor is placed in series with the inductor for reasons to be
discussed below. The two capacitors are not meant to both be present
in the final design, but they were included to allow testing of the
effectiveness of two different capacitor layouts. The reason for using
ceramic caps and not e.g. electrolytics is that small size was a
primary focus in this design. The smallest electrolytics are bigger
and have a larger parasitic series resistance as well as larger series
inductance than the ceramic caps used here.
- a second LC-link formed by a ferrite bead and ceramic capacitors.
The series resistor and dual capacitors are there for the same reason
- coaxial connectors are present after these two LC links. When
testing the links individually, one of the links can be disabled by
removing the capacitor(s) and shorting the inductor. These connectors
are also used when testing the filtering characteristics of the linear
- a linear regulator with part number AP1117 from Diodes Inc. This
regulator was chosen based on its low price.
- supporting components for the regulator (voltage divider and output
- coaxial connectors and an output connector to connect an external
The board is 1.6 mm thick and made of standard FR4. It has two
copper layers of which the bottom one is a solid ground plane. Most
boards I do for real products have many more layers (at least 8) and
this makes a bit of a difference in this application, at least at
higher frequencies as the inductance of the vias from the top side
down to the ground plane is increased due to the longer distance.
Also, some undesired coupling paths may be stronger since the
components and conductors are further away from the shielding ground
plane. In general, the filtering is likely to be at least as effective
on a multi-layer board as on this test board.
A bit of a confession: The layout was done before I realized the
utility of having dual coaxial connectors at each test point, so I had
to patch in the extra connectors after the board was manufactured.
This was made easier by the fact that the board has no solder mask and
that the bottom side is a solid ground plane.
Filtering Strategy 1 - Ferrite
Ferrite beads are often used in various signal and power filtering
applications. Sometimes the designer might have an overly strong
confidence in the abilities of a ferrite, namely that it lets
everything desired through and blocks everything that is undesired.
Maybe there also exists a belief that circuits with ferrites never
have resonances since one of their virtues is their loss (at high
The first filter we will examine is shown in figure 5 below and
consists of a ceramic capacitor and a ferrite bead. The ferrite is
part number 742792023 from Würth which is rated for 3 A and has an
equivalent series resistance (ESR) of 30 mΩ.
Figure 5. Schematic of ferrite filter. (Click to
The filter is measured on the test board and also simulated in
LTspice using the circuit shown in figure 6. Here I use the model for
this particular ferrite that happens to be supplied with LTspice. I
have also modeled the capacitor as a series LCR circuit. The reason
the capacitance is 2.2 µF and not 4.7 µF is that the
capacitance is voltage dependent and is reduced when the voltage
increases. The resistance can be found in the datasheet for the
capacitor while the inductance is a combination of the inductance of
the capacitor and the layout (mainly the ground via). This value can
be estimated through experience (see e.g.
this article (in
Swedish)) and if necessary tweaked so that the simulated response
matches the measured response. The 50 Ω resistor is the
impedance of the input port of the VNA and the current source is a
crude model of the load (linear regulator).
Figure 6. LTspice schematic of ferrite filter. (Click to enlarge.)
The results from simulation and measurements are shown in figure 7
Figure 7. Measured and simulated response of initial
ferrite filter. (Click to enlarge.)
A number of interesting things can be concluded from this experiment.
- The low-pass filtering effect is not well behaved. There is a large
peak in the frequency response in both simulations and measurements.
This is because the Q-value of the filter is too high. It is not well
- There is good agreement between measurements and simulation when the
load current is zero (this simulation is not affected by the value of
the load current).
- There is not a very good agreement at I = 400 mA. The model of the
ferrite does apparently not change the inductance as a function of
current, whereas the real ferrite does lower its inductance at higher
It turns out that Würth has published better LTspice models for some
of their ferrites on their web site:
The behavior of this particular ferrite (742 792 023) is shown in the
plot in figure 8.
Figure 8. Impedance as a function of frequency and
bias current for ferrite 742792023 according to Würth. (Click to
Replacing the ferrite model that came with LTspice with the one from
Würth's web site, we get the circuit in figure 9 and the simulation
results in figure 10.
Figure 9. LTspice schematic with better ferrite model.
(Click to enlarge.)
Figure 10. Measured and simulated response of
ferrite filter using better model. (Click to enlarge.)
In figure 10 we can see a much better agreement between measured and
simulated data. The plots for 0 mA are almost perfectly on top of
each other. For 400 mA we see a little more inductance in reality
than what the model indicates, but the general behavior of the curves
are very similar.
Apparently it is important to use the model downloaded from the
manufacturer web site instead of the model shipped with LTspice if one
is to get dependable simulation results for this component. Despite
this extra hassle, it is nice to be able to with good accuracy
simulate a component that behaves in such a relatively complex manner
as a ferrite, since it allows us to make good predictions of the
efficacy of various power filters without building and testing them.
This can save both time and money.
So, here are some conclusions about this particular ferrite filter.
- The filter is not effective below 500 kHz.
- A large peak occurred at 300 kHz, which is a possible DC/DC converter
frequency and could cause a big problem in a system.
- It is therefore highly advisable to simulate ferrite filters
before using them to see if they actually do any good or if they make
- The model shipped with LTspice did not show the big decline in
inductance as a result of the DC bias current.
- Therefore it is necessary to use a model from the manufacturer site
in this case.
- The virtue of ferrites is primarily loss (attenuation) in the
frequency range from ~10 MHz to 1 GHz (see data sheets).
- Below 10 MHz a ferrite acts as a small inductor with relatively
So, can we improve this filter to get rid of the peak?
Filtering Strategy 2 - Dampened Ferrite
The main problem with the ferrite filter above is that the losses are
too small (the Q value is too high), so a resonance peak occurs. This
increases the amplitude of the noise for a range of frequencies and we
need to introduce loss to improve the situation. Loss means increased
resistance and a resistor can be added either in series with the
ferrite or in series with the capacitor.
Adding it in series with the capacitor has the advantage that the DC
drop over the filter does not increase, but the disadvantage that
the maximum attenuation is much reduced as the capacitor-resistor
combination can never have an impedance below the value of the
resistor and so cannot short the signal arbitrarily well for any
frequency. Another disadvantage is that the inductance to ground is
increased, which also worsens the high frequency properties of the
An alternative to add a discrete resistor is to use a more lossy
capacitor, like an electrolytic capacitor. This has the drawbacks of
increased size and worse high-frequency performance as the inductance
is typically much larger for an electrolytic than for a ceramic
Adding a resistor in series with the ferrite gets around these
problems, but increases the DC drop. In the application at hand, a
larger DC drop was permissible and therefore I went forward with that
Figure 11 below shows the modified filter and figure 12 shows the
resulting simulated and measured response. The resistor value was
chosen based on trial and error in the simulation as a tradeoff
between getting rid of the peak while introducing as little resistance
(and therefore DC drop) as possible.
Figure 11. Dampened ferrite filter. (Click to enlarge.)
Figure 12. Simulated and measured response of
a dampened ferrite filter. (Click to enlarge.)
With the addition of the 0.33 Ω resistor, the peak is gone at
the cost of increased DC drop. The agreement between simulation and
measurement is decent. This resistor/ferrite/capacitor combination is
not harmful at any frequency and is quite effective above 1 MHz. It is
however insufficient for filtering a DC/DC-converter that switches at
a few hundred kHz. In order to address noise at lower frequencies we
need additional filtering and that can be addressed with a filter
based on an inductor that has larger inductance than the ferrite.
Filtering Strategy 3 - LC-filter
The LC filter schematic is shown in figure 13 and an LTspice version
of it in figure 14. LTspice ships with a model for the inductor that
was chosen here (Würth 744 029 003) and that model was used in the
Figure 13. LC filter (Click to enlarge.)
Figure 14. LTspice model of LC filter. (Click to
The filter was simulated and measured and the results are shown in
the graphs of figure 15.
Figure 15. Measured and simulated frequency response
of LC filter. (Click to enlarge.)
As one could guess from the results of the initial ferrite filter,
there is an undesired peak in this filter as well. Other than that one
can notice a good agreement between simulation and measurement. The
filter starts to attenuate signals above around 100 kHz. If this had
not been low enough, a larger inductor or capacitor could have been
Apparently, the inductance of this inductor is not very dependent
upon the DC bias current and the LTspice model works fine. There is
also no better model of the inductor to be downloaded from the
Filtering Strategy 3 - Dampened LC filter
Like with the ferrite filter, we need to get rid of the peak and we
try the same solution as previously, namely a series resistor. After a
little bit of experimentation I opted for the value of 1 Ω.
Schematic and test results are shown in figures 16 and 17 below.
Figure 16. Dampened LC filter. (Click to enlarge.)
Figure 17. Measured and simulated frequency response
of dampened LC filter. (Click to enlarge.)
As previously, there is a tradeoff between dampening the peak and
getting a larger DC drop.
The next step is to combine the dampened ferrite and LC filters to
one filter with better attenuation.
Filtering Strategy 4 - Combined ferrite and LC filter
Figures 18 and 19 show the combined filter schematics. The resulting
frequency response, both simulated and measured is shown in figure 20
together with the responses of the individual filters for comparison.
Simulation and measurement agree very well up to about 2 MHz. Above
that the measurements indicate between 85 and 90 dB of attenuation
whereas the simulation say that we should get even more attenuation.
This discrepancy could in part be due to the measurement setup as well
as coupling via paths that are not modeled. Anyway, 85 dB of
attenuation is remarkably good, so we should not have much trouble
with noise in the 2-100 MHz range getting through this filter.
Figure 18. Dual link LC filter. (Click to enlarge.)
Figure 19. LTspice model of dual link LC filter.
(Click to enlarge.)
Figure 20. Measured and simulated frequency response
of combined filter and the two individual filter links for reference.
(Click to enlarge.)
At 280 kHz (the DC/DC converter frequency in this case) we have about
35 dB of attenuation, which might not be good enough. Increaseing the
capacitance or inductance in the LC-filter could help with this, but
we will look at other solutions below, after first taking a little
detour to look at layout effects.
As mentioned above, the test board had two alternative layouts for
the shunting capacitors. The two variants are shown in figure 21.
Figure 21. Two layout variants for the shunting
capacitors. One GND via and three GND vias. (Click to enlarge.)
The two layouts were tested in the combined filter. First the two
capacitors (one in each LC link) were placed on the footprints with one
via and the response was measured (blue curve in figure 22) and then
the two capacitors were moved to the footprints with three vias (red
curve in figure 22).
Figure 22. Plot showing the difference in attenuation
of dual-link LC filter when each capacitor has one GND via and when
they have three GND vias. (Click to enlarge.)
As can be seen, there is a noticeable effect of ~5 dB extra
attenuation above the resonance frequency of the capacitors (~2 MHz).
In the region below the capacitor resonance frequency, the capacitive
reactance of the capacitors dominates the shunting sections and the
reduced inductance makes no discernible difference.
In this test board, the distance to the ground plane was the full
board thickness of 1.6 mm, which makes the via inductance larger than
on a typical multi-layer board, so the effect of adding more vias is
more pronounced here than what one might encounter in a real
application using a multi-layer PCB.
One should also note that we probably have a significant measurement
uncertainty at these high attenuations (80-90 dB), so the size of the
magnitude of the difference in attenuation might be unreliable,
although the fact that there is indeed an improvement above 2 MHz can
be reliably concluded.
Filtering Strategy 5 - Linear Regulator
So far we have only looked at filtering techniques that reject high
frequencies, but pass low frequencies. To clean up the lower part of
the spectrum from DC and upwards we can use a linear regulator of some
sort. In this particular application, it was important to keep the
cost down, so a regulator called
from Diodes Inc was selected. The
data sheet is
quite sketchy and does not contain any ripple rejection plot. I have
also been unable to find a Spice model for the regulator, so
we have to do our own measurements in order to figure out the
Looking at the data sheet for a similar regulator,
LM1117 from Texas
Instruments, I found a recommendation to bypass the lower resistor of
the voltage setting resistive divider with a capacitor to improve
ripple rejection. I therefore included this option in the design,
despite the fact that the data sheet from Diodes Inc. did not mention
it. The schematic is shown in figure 23.
Figure 23. Schematic of linear regulator circuit.
(Click to enlarge.)
The measured frequency responses of the regulator for a number of
different cases are shown in figure 24.
Figure 24. Frequency response of AP1117 for a few
different cases. (Click to enlarge.)
A few parameters were varied to see how they affect the frequency
response. The curves in figure 24 show the following cases:
Some conclusions are:
- Blue curve: 400 mA of load current, 1.3 V drop over regulator, Cadj=0
- Red curve: 400 mA of load current, 3 V drop over regulator, Cadj=0
- Green curve: 400 mA of load current, 1.3 V drop over regulator,
- Black curve: 400 mA of load current, 3 V drop over regulator,
- Magenta curve: 0 mA of load current, 3 V drop over regulator,
- Attenuation decreases with increased frequency up to about 2 MHz.
- Cadj gives between 5 and 10 dB of extra attenuation for frequencies
below 1 MHz.
- Allowing a larger voltage drop over the regulator gives better
attenuation than a smaller voltage drop.
- A smaller load current results in more attenuation than a higher
Filtering Strategy 6 - LC-filters and Linear Regulator
We have finally come to the point where it is time to combine the
passive filters with the linear regulator. The full schematic is shown
in figure 25.
Figure 25. LC filter and linear regulator combined.
(Click to enlarge.)
Measurement results are shown in figure 26 for both 3V drop and 1.3V
drop over the regulator. Cadj was of course used and the load current
was 400 mA as required by the application.
Figure 26. Frequency response of combined LC filter
and regulator. (Click to enlarge.)
The main conclusions are:
- The attenuation is at least 48 dB from 10 kHz to 100 MHz.
- The attenuation is more than 70 dB from 400 kHz to 100 MHz.
- The fundamental tone and harmonics of typical DC/DC converters are
- The efficiency (with 1.3 V drop) is ~5 V/6.9 V = 72%
A test was done where the noise spectra from a 280 kHz DC/DC
converter were measured before and after the filter. The results are
shown in figure 27.
Figure 27. Noise spectra from DC/DC converter before
and after filter. Upper plot shows 0 Hz to 100 MHz and lower plot
shows a zoom-in of 0 Hz to 5 MHz. (Click to enlarge.)
For comparison, the idle channel noise of the instrument is also
plotted (green curve) and it shows that it is mostly the instrument
noise floor that shows up in the curve after the filtering.
In the zoomed-in view, one can however notice an interesting
phenomenon. The red curve points up above the noise floor at low
frequencies, but not following the shape of the blue noise spectrum.
This noise is probably flicker noise generated by the regulator itself
and might be something to watch out for if a very low noise supply is
required. Better (and more expensive) regulators than AP1117 might
have specifications for the output noise as well as a lower noise
So to summarize the findings in this article:
- Do not willy-nilly throw in a ferrite or LC-filter and expect good
results without analysis. Instead, make sure to simulate the filter
using good models to make sure there are no surprises (peaks) and that
the filter is effective enough in the frequencies of interest.
- There are models in LTspice for inductors and ferrites from several
manufacturers. Better ferrite models for Würth's parts do however seem
to be available from the manufacturer web site.
- Models for e.g. capacitors can be crafted by applying some
experience and by matching to measurement results.
- Ideally, the simulation models should be validated by measurements
if it is important to get reliable results.
- It is easy and inexpensive to simulate and with a little care, the
results can be quite accurate.
As mentioned at the beginning of this article, it is not the
particular circuit that was developed here that is the main point of
this article. For many applications it is certainly not particularly
suitable and other requirements mandate other solutions using other
components. Rather, the takeaway it to use simulation and (if
possible) measurements to analyze the circuits instead of just
throwing some components together and assuming they will work well.
Some of the pitfalls to look out for are filter peaking, DC voltage
drop, regulator characteristics and layout details.
My hope is that the reader will be able to design better DC power
filters after reading this text.