Circuit Surgery
Regular clinic by Ian Bell
LTspice sources and waveform import/export
I
n last month’s article on class
D, G and H amplifiers we made use
of behavioural sources in the LTspice
circuit simulator to draw waveforms to illustrate the article. There was insufficient
space to explain much about this aspect
of LTspice, so now we are going to take
a more in-depth look at LTspice sources
in general. Also, I was recently asked
by someone about how you can get data
in and out of LTspice for use with other
applications. This is related to the uses
of sources in creating and manipulating
complex waveforms, so we will look at
that too, including importing and exporting WAV audio files as these provide the
opportunity to have some fun listening
to the results of your circuit simulations.
Sources
In SPICE, and electronics in general,
a source is something which outputs
voltage or current, which, depending on
the context of its use, will be regarded
as a signal, a reference level or a power
supply. The output from a source may
Fig.2. Example arbitrary PWL waveform imported from a text file (for file contents see text).
be anything from a constant (DC) value
(typical for references and power supplies)
through basic AC signals, such pulses and
sinewaves, to highly complex waveforms
such as audio. In LTspice (and SPICE in
general) there are a variety of components
that can be added to a circuit to act as
sources. The most basic of these are simply
called Voltage and Current. The names
of components in SPICE start with a letter
indicating the type of component –
for these basic sources it is V and I.
The V and I sources can be configured
to produce a variety of outputs via a
dialog. Once the component is placed
on the schematic (see Fig.1 below)
right-clicking it allows a DC value
to be set, but clicking the Advanced
button opens another dialog (see
Fig.1 left) which allows a variety
of signals to be set up. Specifically,
these are DC (none), pulses (PULSE),
sinewave (SINE), exponential (EXP),
frequency-modulated sinewave (SFFM)
and arbitrary piece-wise linear (PWL).
Selecting one of these options provides
access to dialog inputs to configure the
sources as required (for example, the
frequency of a sinewave), see Fig.1.
The PWL option allows you to define
an arbitrary waveform by entering a
Fig.1. (right) LTspice symbols for independent voltage
and current sources and (above) part of the source
configuration dialog showing parameters for a
sinewave source.
Practical Electronics | July | 2020
set of value pairs (a time and the voltage
at that time). The main source dialog
provides just four points, but you can open
another dialog to add more. For more than
just a few data points it is often better to
use a file for the data (PWL FILE option).
The PWL file must be a text file containing
the list of time and value pairs (one per
line) in a tab or comma-delimited format.
Unlike some similar data files there must
not be any header information, such as a
first line with the column headings. You
can create the file with a text editor, or use
a spreadsheet such as Excel or LibreOffice
Calc and work with CSV (comma-separated
values) files.
Fig.2 shows an example of a waveform
produced from the following text file using
the schematic in Fig.3.
0,
0.001,
0.002,
0.0021,
0.0022,
0.0023,
0.003,
0.004,
0.005,
0.006,
0.007,
0.008,
0
0.5
2
-1
-1.5
2
2
4
8
5
0.5
0
The data points in the waveform are
those created by the simulation – not the
original input data. Here, they are similar,
but simulation has an additional data
43
time
0.000000000000000e+000
1.000781250000000e-003
2.000000000000000e-003
2.100000000000000e-003
2.200000000000000e-003
2.300000000000000e-003
3.002343750000000e-003
V(wave)
0.000000e+000
5.011719e-001
2.000000e+000
-1.000000e+000
-1.500000e+000
2.000000e+000
2.004688e+000
I(R1)
0.000000e+000
5.011719e-004
2.000000e-003
-1.000000e-003
-1.500000e-003
2.000000e-003
2.004687e-003
Data exported from the circuit in Fig.3.
Fig.3. LTspice schematic used to check
import of the PWL waveform file in Fig.2.
point at 6.5ms. In this case the file was in
the same folder as the LTspice schematic
file, so no path is included with the file;
however, the full path can be specified.
If you are familiar with using formulae in
spreadsheet applications, there is potential
to use these to create waveforms that are not
available from the basic sources settings.
If you are a coder then you can write
software to generate PWL waveforms and
write the data to a text file. Mathematical
applications such as MATLAB can also be
used to write data out in CSV format that
can be read as PWL waveforms in LTspice.
LTspice can also export waveform
data to a text file. This is done using the
main menu: File > Export data as text
with waveform window selected. This
opens a dialog which allows you to select
the currents and voltages you want into
include in the file – for example, see
Fig.4 which shows the voltage V(wave)
and the current in R1 (I(R1)) from the
circuit in Fig.3 selected for export. Part
of the resulting file is shown above-right.
The files exported by LTspice are tab
separated and include a header row with
the column (field) names. The first value
on each row is the time, which is followed
by the other selected values. These files
are readily loaded into spreadsheets and
mathematical applications like MATLAB.
Controlled (dependent) sources
The V and I sources we have discussed
so far can produce a wide variety of
waveforms, but these are entirely controlled
Fig.4. Exporting LTspice waveforms to a text file.
44
‘inside’ the source – there is no direct effect
on their output from other signals in the
circuit, although loading effects may be
modelled if a source’s internal resistance
is defined (this can be done in the source
setup dialog). A source controlled by
another voltage or current elsewhere in
the circuit is a very useful way to model
common circuit behaviours. For example,
a voltage amplifier is effectively a voltage
source controlled by another voltage – its
input signal.
Controlled sources can be used to create
simulations of circuits based on their
operating principles, characteristics and
behaviour, rather than a full componentbased design – these are referred to as
‘macromodels’ or ‘behavioural models’.
This is useful for trying out ideas
without having to develop a full design
at component level. It is also used by
manufacturers of components such as
op amps to publish accurate simulation
models of their ICs without revealing full
design details. Furthermore, controlled
sources are used within SPICE itself to
model active devices such as transistors,
and they are used in some published
models of common components which
are not built into SPICE simulators. The
most-basic controlled sources are:
E Voltage-controlled voltage source
F Current-controlled current source
G Voltage-controlled current source
H Current-controlled voltage source
These sources are also referred to
individually as, for example, a ‘voltagedependent voltage source, and collectively
as ‘linear dependent sources’. The
letters E, F, G and H are the initial
letters of the element names of
these components. The circuit
symbols are shown in Fig.5. Note
the additional connections for
the voltage-dependent sources
Fig.5. Dependent source
symbols.
– the voltage across these points is used
to control the source’s output. The currentdependent sources do not have control
inputs – their control can only come from
a voltage source in the circuit.
Transfer Function
To define the behaviour of a controlled
source it is necessary to specify the
relationship (transfer function) between
the controlling voltage or current and the
source’s output. The simplest version is a
constant gain – the source’s output is the
controlling value multiplied by the gain. It
is also possible to specify the coefficients
of a polynomial (a type of mathematical
expression) relating the output to the input,
however, use of mathematical expressions
is better done with a behavioural source,
which we will discuss soon. This option is
mainly provided to support legacy models.
For voltage-dependent sources only, it
is possible to define the input-output
relationship using a piecewise-linear
lookup table – pairs of numbers specify
input voltage and corresponding output
with that input.
Fig.6 shows an LTspice schematic that
illustrates use of controlled sources.
V1 outputs a 1V, 1kHz sinewave across
resistor R1. The voltage across R1 is used
to control the voltage-dependent voltage
source E1. E1’s gain is 5, so the output
will be a 5V, 1kHz sinewave. The current
through V1 and R1 is used to control the
current-dependent voltage source H1.
The waveforms from the simulation are
shown in Fig.7.
Ammeter
In Fig.6 we see a use for voltages sources
in SPICE that is not immediately obvious –
as ammeters. A 0V voltage source behaves
like a short circuit, so has no effect if
inserted into a wire, but can then be used
by a current dependent source to control
its output. In Fig.6 the voltage source
Vmeas is used in this way. The control
for H1 is specified as Vmeas 5000 – this
means: use the current through voltage
source Vmeas and multiply by the gain
5000 to obtain the output voltage.
The 1V peak across R1 will result
in a 1mA peak current, which when
multiplied by 5000 will produce a peak
output of 5V. The gain for an H1 source
is a transresistance (voltage/current). In
this circuit we could have used V1 as the
Practical Electronics | July | 2020
Fig.6. Circuit to illustrate use of dependent sources.
Fig.7. Waveforms from the circuit in Fig.6.
Fig.8. Circuit
to illustrate
use of
behavioural
sources.
in WAV format, and LTspice can export
simulation data to WAV files too.
An audio wave file will typically contain
data in a commonly used audio format, that
is, in terms of its sample rate, number of
channels and number of bits – for example,
as stereo CD-quality audio with two channels
of 16-bit data at a sample rate of 44.1 kHz.
However, WAV is not limited to standard
audio formats and can have sample rates in
the range 1Hz to 4.3GHz and any number
of channels up to 65,536. This means uses
of WAV files with LTspice can go beyond
working with audio circuits and they can
be used for inputting and recording data
for a wide range of circuits.
Unlike the PWL data files discussed
above, WAV is not directly compatible with
spreadsheets, but it can read and written by
mathematical software such as MATLAB. Of
course, using WAV files for audio circuits
means that you can listen to the inputs and
outputs of your simulations using a media
player application – although you will need
the format to be compatible with an audio
standard for this to work. Furthermore, other
audio generating and processing applications
will be usable with your simulation data.
To read a WAV file into LTspice you need
to place a voltage or current source on your
schematic and change its ‘value’ to the form:
wavefile=filename
controlling source, but we included Vmeas to illustrate what to
do if the current required is not flowing via an existing source.
The voltage from H1 is inverted with respect to the control voltage
because the current in Vmeas is negative due to the convention
used by LTspice for current directions through sources.
Behavioural sources
The E, F, G and H sources have relatively limited options for
controlling their outputs – the only controlling inputs available
are other circuit voltages and currents and, more importantly
they are difficult to use beyond simply gains. Much greater
flexibility is provided by the behavioural sources (BV and BI
elements) which allow the use of a large range of mathematical
expressions to define their output. These expressions can involve
time as well as circuit voltages on any wire (to ground), voltage
differences (between two wires) and the current in any element
(not just voltage sources).
Behavioural sources are configured by setting their value to
an equation that specifies their operation. For example, for gains
equivalent to those for E1 and H1 in Fig.6 we would use the values:
V=5*V(control)
V=-5000*I(R1)
This is illustrated in Fig.8. The waveforms on b1_out and b2_
out are the same as for e_out and h_out respectively in Fig.7.
Simulating with WAV files
WAV is a standard audio file format, which was released, by
Microsoft and IBM in the early 1990s. WAV files can contain
compressed audio data, but they are most commonly used with
uncompressed data. Although it is not available via the sources
dialog or menus, LTspice V and I sources can also read files
Practical Electronics | July | 2020
Where filename is the name of a WAV
file in the same folder as the schematic, or the full path to the
file if it is elsewhere. If the path contains spaces it needs to be
put in double quotes. Right click the source value and enter the
text to set this up. WAV files support multiple channels, so the
required channel can be specified in the source value using:
wavefile=filename chan=channel
Where channel is the channel number. If it is not specified,
then the default is channel 0 (the first channel).
To write a WAV file you need to place an LTspice .wave
directive on the schematic. This can be done by clicking the .op
toolbar button, entering the appropriate text, clicking OK and
then clicking on the schematic. The syntax of the directive is:
.wave filename nbits samplerate V(net) …
Where filename is the name of the WAV file for the waveforms
to be written to – in the same folder, or with a full path, as with
file reading. The number of bits used is set by nbits and can
range from 1 to 32. The sample rate is set by samplerate and,
as indicated above, can range from 1 to 4,294,967,295. The
settings are followed by the list of net voltages to include in
the file (the number listed determines the number of channels).
For example, the following will create a file called output1.wav
with CD format stereo audio (16-bit 44.1 kHz) with the signals
on nets ou1 and out2 in the two stereo channels:
.wave output1.wav 16 44.1K V(out1) V(out2)
WAV Example
As an example of using WAV files as input and output to a
simulation we will simulate a simple transistor amplifier. The
45
file. Finally the .wave directive has
been added to the schematic to write the
amplifier’s output to another WAV file. The
settings are similar to the example above
except that both channels are being written
with the same signal – this will create
a file that will play the same waveform
through both stereo channels.
Audacity
Fig.9. LTspice schematic for simulating a basic amplifier with a signal from a WAV file.
Fig.10. LTspice simulation results for ten seconds of audio (speech) from a WAV file
used as input to the circuit in Fig.9, and the resulting output.
When working with WAV files in LTspice
it is useful to be able to see the waveforms
as recorded in the WAV file, as well as
recording audio to save as WAV, listening
to the files and maybe manipulating the
sound in various ways. A particularly
useful tool for doing this is the application
Audacity. Audacity is described by its
creators as a free, open-source, easy-touse, multi-track audio editor and recorder
for Windows, Mac OS X, GNU/Linux and
other operating systems. It is available to
download from: www.audacityteam.org
Opening output1.wav in Audacity and
zooming to the same range as shown in
Fig.11 will reveal that things are not as
we might have hoped – see Fig.12. The
waveform is much more severely clipped
than in the simulation. This is because
unlike the PWL files, which can cover any
voltage range, LTspice’s WAV output is
limited to an amplitude of ±1V to conform
to the WAV format. This is a problem here
because the output is larger than this.
To get around the ±1V limit imposed by
using WAV files we need to be able to scale
the simulated signal being output so that
it stays within this range. To do this we
need to know the maximum (peak) value
of the waveform and then divide the signal
by this value to create a new waveform
that stays within ±1V (we say this new
waveform is the output ‘normalised’ to a
peak amplitude of 1V). Similarly, when
a WAV file is used as input an amplitude
of ±1V may not be appropriate for the
circuit we are simulating. For the circuit
in Fig.9 this is slightly too large, although
the clipping produced may provide an
opportunity for a listening test – to hear
any distortion created by the circuit – but
first we have to overcome the clipping
caused by the WAV range limits.
Normalising
Fig.11. Zoom-in on the waveforms from Fig.10 at around 9s showing an example of
clipping of the signal.
schematic is shown in Fig.9 – this is the
circuit from the August 2019 Circuit Surgery
article where we discussed the design of
basic common-emitter BJT amplifiers.
There are three changes from the original
simulation. First, the value of input signal
46
voltage source (V1) has been changed
from the original sinewave definition to
reading a WAV file (wav1.wav). Second,
the simulation has been set to run for
10s instead of the original 30ms to match
the duration of the audio in the WAV
In some circuits the range of signal we are
outputting may be obvious, but in other
cases it may be less so. It is therefore
helpful if we can measure the actual peak
value. You could try to do this manually
by looking through the waveform, but
this is far from ideal. Fortunately, LTspice
has a better means of doing this via
the .measure (.meas) directive. The
.measure directive provides a large range
of possibilities for obtaining measurements
from simulation data; examples include
finding the maximum, minimum, average
Practical Electronics | July | 2020
Fig.12. Viewing the WAV file created by the circuit in Fig.9 in Audacity (compare with Fig.11).
or RMS value of a waveform. Mathematical expressions can be
applied to circuit signals to which the measurement is applied,
increasing the scope of the basic measurements. To find the
peak value of a signal we can add the following directive to
the schematic (using the .op button):
.meas peakvalue max abs(v(out))
Here, peakvalue is just a name give to the measurement result,
max is the measurement type we are using (find the maximum)
and abs(v(out)) is the value to which the measurement is
being applied. This is taking the signal V(out) and applying the
mathematical ‘absolute value’ function to it. The abs function
removes the sign, so that we find the magnitude of the largest
peak in the signal, whether it is negative or positive.
To find the peak value run the simulation and select View >
Spice Error Log from the menu. This will open the log file, in
which you should find a line similar to the following:
peak: MAX(abs(v(out)))=4.99165 FROM 0 TO 10
Here we see the peak value is 4.99165 V. The normalisation of
signals for WAV output is easily performed using a behavioural
source – create a new voltage equal to the signal of interest divided
by the peak value calculated using the .measure directive. For
the circuit in Fig.9, adding the behavioural source shown in Fig.13
does the job. Here, the dividing value has been set to a value slightly
larger than the peak. The .wave directive also has to be edited to
use the new signal (out_n rather than out in this example). In
our example the WAV file name was
also changed, to wave2.wav
Listening
Using normalisation requires the
simulation to be run twice – first to
obtain the peak value and then again
with the correct normalisation set up
to produce the WAV file. The results
from Fig.5, modified as described,
and loaded into Audacity to display
the same range as Fig.8 are shown
in Fig.10. We see that the WAV file
now matches the LTspice waveform Fig.13. Behavioural source
(v(out) in Fig.8). The WAV file can added to the circuit in Fig.9
now be listened to in comparison with to normalise the out signal
the input, although the difference for WAV output.
in this example was not dramatic as only the largest peaks were
clipped. Another behavioural source could be added to boost the
input signal to cause the circuit to create more distortion, so the
effect could be clearly heard. Another experiment worth trying is to
reduce the coupling
capacitors to a much
Simulation files
smaller value (say
Most, but not every month, LTSpice
1nF), which will
is used to support descriptions and
cut the gain at low
analysis in Circuit Surgery.
frequencies and
The
examples
and files are available
make the speech
for download from the PE website.
sound different.
Fig.14. Wave file waveform for the output from the circuit in Fig.9 after normalisation using a behavioural source.
Practical Electronics | July | 2020
47
