Circuit Surgery
Regular clinic by Ian Bell
Distortion and distortion circuits – Part 2
L
ast month, we started looking
at distortion, which is the changing of the shape of waveforms
due to nonlinearities in circuits such
as amplifiers. This was inspired by a
couple of PE projects by John Clarke
on sound processing effects for musicians, including the recent Digital FX
system and the Nutube Guitar Overdrive
and Distortion Pedal from March 2021.
Although deliberate distortion is used
creatively by musicians, distortion is
often an unwanted characteristic and
circuit designers make significant efforts
to minimise it. The amount of unwanted distortion is often measured using
Total Harmonic Distortion (THD), particularly in audio applications.
Distortion and Spectra
In Part 1 last month we covered the
basic principles of distortion, including
the importance of the spectrum of a
signal in understanding distortion and
the mathematics behind THD. To recap
briefly, a spectrum is a plot of signal
strength (amplitude or power) against
frequency, which therefore shows all the
frequencies present in a signal (within
the range plotted).
Any periodic waveform can be formed
by adding together a set of sinewaves
of various frequencies and different
amplitudes. This ‘sum of sinewaves’ is
known as a Fourier series. The spectrum
plot of a periodic signal therefore
comprises a set of peaks at various
frequencies, and the sinewave itself is
the only signal that has just one peak in
its spectrum.
When a sinewave is input to an ideal
amplifier the output spectrum has the
same form as the input – a single peak
– but with the amplitude changed by
the amplifier’s gain. For a non-ideal
(non-linear) amplifier the output will
contain frequencies which were not
present in the input. The presence of the
additional frequencies changes the shape
of the waveform. Change of wave shape is
an intuitive idea of what distortion does,
but is not sufficient to define distortion.
A change of waveform shape will also
occur for non-sinusoidal inputs to
perfect linear filters (eg, ‘rounding off’
of a square wave). This is because the
relative amplitude of the spectral peaks
is changed – but the output does not
contain additional frequencies.
The theory we discussed last month
shows that for a sinewave input the
additional output frequencies due to
distortion will be at multiples of the
input frequencies, that is, harmonics of
the input. If we find the ratio between
the power of the output signal at the
input frequency and the power of the
sum of all the additional frequencies
due to distortion, then we get a useful
indication of how much distortion a
circuit produces. Because we are adding
up all the contributions of the harmonics,
this measure is called ‘Total Harmonic
Distortion’. If the input signal contains
multiple non-harmonically related
frequencies the effects of distortion are
Fig.1. A
very simple
circuit for
investigating
spectra in
LTspice.
more complex, containing sum, difference
and other combination frequencies – this
is called ‘intermodulation distortion’.
In the context of a single music note, the
input will in most cases already contain
harmonics – these define the timbre of
the note (musical quality other than pitch
loudness), thus distortion will change the
relative harmonic content and hence the
timbre, typically producing a ‘fuzzier’,
‘grittier’ or ‘harsher’ sound.
Using LTspice
Last month, we illustrated parts of the
article with LTspice simulations, including
plots of signal spectra. However, we did
not explain how these were obtained, so
this month we will look at how to plot
signal spectra and calculate THD with
LTspice. THD can be calculated manually
from a spectral plot, but LTspice has a
Simulation files
Most, but not every month, LTSpice
is used to support descriptions and
analysis in Circuit Surgery.
The examples and files are available
for download from the PE website.
54
Fig.2. The waveform of V(x) from the transient analysis of Fig.1.
Practical Electronics | July | 2022
The circuit in Fig.1 is
the minimum needed to
g e t LTs p i c e t o d i s p l a y
a spectrum. To obtain a
waveform to analyse with
the FFT we need to run a
transient simulation; the
figure shows that a 5ms
transient analysis has
been set up. The resulting
waveform is shown in Fig.2.
‘FFT’ refers to the ‘Fast
Fourier Transform’, which is
the mathematical algorithm
used to calculate a spectrum
from a waveform. The
fundamental mathematics
is the Discrete Fourier
Transform (DFT) – ‘discrete,’
because the waveform
data is a set of sample
points, not a continuous
mathematical function. The
FFT is an efficient computer
implementation of the DFT.
FFT plot
Fig.3. The FFT dialog in LTspice.
command for calculating it automatically.
This does not mean that the spectral
plots are not useful – they provide a
visual insight into the harmonic content
of a distorted waveform. For example,
musicians often discuss the relative
merits of distortion dominated by odd
or even harmonics and relative levels
of higher and lower order harmonics in
terms of quality of sound. The spectrum
plot allows a quick assessment of such
properties of a signal. Next month, we
will look at analogue circuits used to
create distortion for musical effects.
To see the spectrum for the
waveform, right click on the
waveform and select ‘View’
from the pop-up and then
‘FFT’ from the submenu.
The dialog shown in Fig.3 will appear.
Make sure the signal of interest, in this
case V(x), is selected and click OK. This
will display a spectrum similar to the
one in Fig.4 – note that the frequency
range plotted in Fig.4 has been changed
from the default to focus on the lower
frequencies closer to the input frequency.
To change the axis range right-click on
axis numbers and enter the new range
values in the dialog.
The expected spectrum for a pure 1kHz
sinewave is simply a single very sharp
peak at 1kHz. The spectrum in Fig.4 has
a very wide peak and plenty of content
at other frequencies. Fortunately, there
are several things we can do to obtain
a more convincing spectrum.
The spectrum in Fig.4 is plotted
in decibels. The largest peaks, other
than the expected one at 1kHz, are
about 65dB below the 1kHz peak, this
is about 2000-times smaller (10-65/20 =
5.6x10 -4). This may seem small, but
remember the spectrum should be zero
at all frequencies except 1kHz. LTspice
spectral plots will always have some
content where ideally the value is zero
due to the limitations in the accuracy of
the calculations, but we need to make
sure the errors are acceptable. In this
case, we would expect much smaller
errors given that we have an ideal
sinewave and perfect (linear) resistor.
Compression
One problem with this initial simulation
is due to the waveform data compression
that LTspice employs. This is often
useful because a compressed waveform
file can be 50-times smaller than an
un-compressed one. However, the
compression is lossy, which means that
information is lost during compression.
Although it usually does not detract from
the look of a waveform plot, this loss
may degrade the quality of a spectrum
calculated from the waveform data, so
when you intend to analyse spectral
data, compression should be turned off.
You can turn off compression using
Control Panel from the Tools menu:
go to the Compression tab and set
the Window Size (No. of Points):
value to zero. However, this setting
is not remembered between program
invocations, so it is better to put the
command on the schematic. To do this,
click on the schematic window and then
on the .op (SPICE Directive) button on
the menu bar. Enter the following text
into the dialog
.option plotwinsize=0
Next, click on the schematic to add
the command. Close the spectrum
window and then run the simulation
again (this is necessary to generate the
uncompressed waveform data). Then
display the spectrum again – see Fig.5.
Noise floor
Fig.4. The initial spectrum does not look very convincing.
Practical Electronics | July | 2022
For real circuits, there is always random
noise present, and in measurements of
signal spectra this will produce results
similar to the relatively flat part of the
spectrum away from the peak in Fig.5.
Pure random noise over an infinite
time has a perfectly flat spectrum (no
peaks) at all frequencies, but with real
measurements there will be variations,
55
Accuracy
Fig.5. Avoiding data compression greatly reduces noise in the spectrum
Fig.6. Using a longer simulation (more cycles) gives a narrower peak, but this attempt
has more noise due to lack of simulation accuracy.
as in Fig.5. The general level of the
flattish part of the spectrum between
the signal peaks is called the noise floor.
In simulations, like the example here,
there is no random noise in the signal,
but numerical errors in the simulation
produce a noise floor in the spectrum.
The decibel scale appears to exaggerate
the noise level if you are not used to
reading decibel-scaled graphs. In Fig.5
the noise floor is around 160dB below
the peak, this corresponds to a voltage
300 million times smaller than the peak.
This is much smaller than the noise
floor in typical real circuits.
We now have a clean spectrum, but the
peak is still much wider than expected.
This is due to not having enough good
waveform data for the FFT to use. One
thing we can do is to run the simulation for
longer, so that more waveforms cycles are
included. To do this use Edit Simulation
Cmd from the Simulate menu and change
the Stop Time to 50m. Run the simulation
again and you will see about 50 cycles.
56
The spectrum should now look like Fig.6
– the frequency range has been changed
to match the previous plots.
The peak at 1kHz is now much narrower,
but the noise floor is worse again. This
is again due to lack of accuracy in the
simulation. This time it is not data
compression, but the number of data
points at which the simulator has
calculated the waveform that is the
problem. The data points used by the
FFT are not at the same points in time as
the points on the waveform calculated
by the simulator. This is simply because
they work in different ways.
The FFT uses regularly spaced
samples, whereas the simulator
calculates the waveform at the ‘next
time step’, and this length of time can
vary depending on how the simulator’s
calculations perform. If there is not a
simulator waveform data point at the
time required by the FFT, the FFT has
to interpolate the required value using
the nearest data points, which may lead
to errors. However, we can force the
simulator to use a certain minimum
time step, so that more waveform
data points are calculated during the
simulation, providing better data for
the FFT.
To reduce the time step, again use Edit
Simulation Cmd, this time entering 10n
in the Minimum Timestep box. Leave
the Stop Time at 50m. This will force
the simulator to calculate waveform data
points at least every 10ns (nanoseconds).
Run the simulation again – you will
find it takes longer. View the spectrum
again; it should look like Fig.7. We now
have a sharp peak and a noise floor well
below the peak. The spectrum is much
closer to that of an ideal sinewave than
our initial attempt.
Another way to improve accuracy is
to set another option:
.options numdgt=7
Fig.7. Improving simulation accuracy (at the expense of run time) gives a spectrum with
a much better noise floor.
Practical Electronics | July | 2022
Fig.8. Further improvements in accuracy using double-precision maths.
This is added to the schematic in the
same way the plotwinsize directive
used earlier. The LTspice help informs
us that historically (in SPICE) this was
used to set the number of significant
figures used for output data, but in
LTspice setting numdgt greater than 6
causes double-precision maths to be
used in calculations.
Plotting
Once a good quality spectrum has been
obtained it is not essential to include
the noise floor in the plot. For results
such as those in Fig.8, the noise is so
small that it is not relevant, and we can
limit the decibel range to values close
to the peak. This makes it easier to see
the relative levels of different peaks. For
example, Fig.9 shows a circuit to create
a signal comprising two sinewaves,
from sources V1 and V2 at 1kHz and
5kHz respectively. The 1kHz signal has
twice the amplitude of the 5kHz one.
This figure also illustrates use of the
.plotwinsize and .numdgt directives
discussed above.
Plotting the results from Fig.9 using
the full decibel range (as in Fig.8)
makes it difficult to see the relative
amplitude of the two frequencies. The
plot in Fig.10 is the FFT results from
the circuit in Fig.9 with the decibel
range set to more convenient values.
From this we can clearly see that the
5kHz signal (V2) is 6dB below the 1kHz
signal (V1). This is a signal amplitude
ratio of 20log(V2/V1) = –6dB or V1/V2
= 10–6/20 = 0.5, that is the 5kHz signal
is at half the amplitude of the 1kHz
Fig.9. Generating two sinewaves at 1kHz
and 5kHz.
signal, as we woud expect from the
source configurations.
This brings us to an issue which
sometimes confuses people: what exactly
the FFT result is plotting. The V1 source
in Fig.9 has an amplitude of 1.4142V
(√2). This value was chosen because it
represents an RMS (root mean square)
AC voltage of 1V. The RMS value of an
AC voltage is the value of the DC voltage
which would dissipate the same power
in a given resistor and represents an
Fig.10. Results from simulation of the circuit in Fig.9.
average of the power delivered over a
waveform cycle. For a sinewave, the
RMS value is the peak value divided by
2. The default LTspice FFT plot is in
dBV – that is, decibels relative to 1Vrms,
specifically 20log(Vrms/1Vrms), so 1.4142
(1Vrms) is plotted as 0dB (20log(1)) and
0.7071V as –6dB (20log(0.5)), as shown
in Fig.10. The FFT plot can also be set up
to display RMS values instead of decibels
by right-clicking the amplitude axis and
selecting Linear in the Representation
section. This version of the plot in Fig.10
is shown in Fig.11.
FFT settings
Fig.11. Linear (voltage) plot of the results from simulation of circuit in Fig.9.
Practical Electronics | July | 2022
The FFT dialog (Fig.3) provides a variety
of settings which we can use to control
57
Fig.12. Using the wrong time range for a periodic signal produces an inaccurate spectrum.
the way in which the FFT is calculated.
So far, we have only used the default
settings. The number of samples used
by the FFT can be changed. The default
is 262144. Increasing this value will
slow the FFT calculation but increase
the maximum frequency for which the
spectrum is valid (for a given time range
of data used by the FFT). The transient
simulation maximum time step should
be sufficiently small when extending the
FFT frequency range. As we are using
a low frequency here the number of
points can be reduced and still provide
a reasonable spectrum. However, the
accuracy will also reduce, so the peak
may get wider and the noise floor higher.
The time range over which the FFT
is calculated (the window) can have
a significant impact on the results,
particularly for periodic waveforms
like our sinewave. For such waveforms
the range should be an exact number of
waveform cycles. The FFT is effectively
calculated on a waveform which is
made up of infinitely repeated copies
of the window range. Discontinuities at
the ends of the range introduce errors
into the spectrum – this is known as
‘spectral leakage’.
By default, the entire simulation is
used for the FFT. This may not be the best
approach to use; for example, if a circuit
takes several cycles to stabilise, it would
be best to start any FFT analysis after
this. The FFT time range can be set in
LTspice by zooming in on the waveform,
or by typing in specific time values. To
try this, open the FFT dialog again and
select ‘Specify a time range’ in the ‘Time
range to include’ section. Change the
‘End time’ from 50ms to 49.5ms and
click OK to obtain the spectrum. It will
look like Fig.12. The peak is wide and
slopes off slowly.
If the signal is not periodic, windowing
functions can be used to ‘fade out’ the
edges of the time range to prevent any
discontinuities causing spectral leakage.
Normally, these would not be needed
for periodic waveforms such as sines –
if we correctly used an exact number
of cycles.
THD Analysis
LTspice is able to perform THD analysis.
Fig.13 shows the circuit from last month
which we used to illustrate the output
spectra from a couple of nonlinear
functions. It is a good idea to check that
the spectrum looks reasonable (using
the FFT plot) before looking at THD
results to make sure that the results will
be valid. The .four SPICE directive on
the schematic shown in Fig.13 instructs
LTspice to perform a Fourier component
and THD analysis on a periodic signal.
The syntax of the .four directive is
.four <frequency> [Nharmonics]
[Nperiods] <data trace1> [<data
trace2> ...]
Fig.13. LTspice schematic for example THD analysis.
The frequency parameter specifies the
fundamental frequency for which the
analysis is performed. This will usually
be the fundamental frequency of the
input signal. Nharmonics specifies
the number of harmonics for which the
Fourier components will be calculated
(the default is 9). Nperiods specifies
how many waveform periods back from
the end of the simulation are used to
perform the analysis. The default setting
is 1, but changing to –1 causes the entire
simulation to be used. The example in
Fig.13 is:
.four 1kHz 10 V(y1) V(y2) V(y3)
Fig.14. Fourier component and THD analysis results for signal y2 in Fig.13.
58
This calculates ten Fourier components
for a fundamental of 1kHz for signals y1,
y2 and y3 using one waveform period.
The results are accessed using View ->
Spice Error Log. A table listing part of
the results from the circuit in Fig.13 is
shown in Fig.14. The THD for signal
y2 is 10.4%.
Practical Electronics | July | 2022
