LTspice THD+N and other questions...

[Mike Deblis]

Forgive my ignorance...

Is there a way to get an estimation of the THD+N of an audio amp in
LTSpice? Ideally, I'd like to plot THD+N against frequency & possibly
temperature...

next question - what is the simplist way of generating a fairly
complex repetative sequence of pulses on a number of nets? What I'm
trying to do is to open & close a lot of analogue gates in a fairly
complex repative sequence. Again, ideally I'd like to manipulate this
sequence fairly simply, rather than change a load of PULSE statements
as I do at the moment (its rather prone to error).

Thanks

Mike

 

[Mike Rocket J. Squirrel Elliott]

Forgive my ignorance...

Is there a way to get an estimation of the THD+N of an audio amp in
LTSpice? Ideally, I'd like to plot THD+N against frequency & possibly
temperature...

next question - what is the simplist way of generating a fairly
complex repetative sequence of pulses on a number of nets? What I'm
trying to do is to open & close a lot of analogue gates in a fairly
complex repative sequence. Again, ideally I'd like to manipulate this
sequence fairly simply, rather than change a load of PULSE
statements as I do at the moment (its rather prone to error).

Another Mike. Welcome, Mike.

The lack of a THD+N meter in SPICE is a problem that I've always wanted
a solution to.

SPICE guys, who are not usually audio engineers, will suggest the FFT as
a way to examine the spectral output, but it's not as informative as
looking at the output of a harmonic analyzer, which not only gives you
the ratio of the sum of the amplitudes of the various generated
harmonics (minus the fundamental, and within the bandwidth specified by
the user) to the total amplitude of the circuit's output, but -- and
this next is very useful to the experienced analog circuit designer user
-- by using an oscilloscope, one can view the actual distortion of the
device under test with the stimulus sine wave subtracted. This
"distortion residue" output is a graphic display of how the device is
distorting the sine wave. One trick that is often used is to sum the
(greatly amplified) distortion residue with the input signal on an
oscilloscopes screen so you can see how the sine wave has been changed
as a result of the various nonlinearities in
the device.

These bits are all modelable in SPICE using subcircuits, but it's
cumbersome -- to me, because I am not very clever with SPICE. To see the
distortion residue minus the fundamental, you need to basically build a
band-reject filter with a very narrow (less than an octave so as not to
attenuate the 2nd harmonic), very deep (like 120dB) notch. If you want
to change the generator frequency to examine the performance of the
circuit at a different frequency, you need to change the notch filter's
center frequency, and that's tedious as hell, esp. since the component
value have to be specified to many digits to get the notch spot-on and
narrow enough.

Another way of getting rid of the stimulus signal so the nonlinearities
can be made viewable is to subtract the input from the output. This does
not require a notch filter, but the gain of the circuit needs to be
established to a high enough degree so that the results are accurate to
within, say, 80dB. Math again -- calculate the gain, then feed that
number into the summer to get the residual output. This might not be
useful in circuits that change their gain intentionally -- like
limiters, expanders or compressors, or unintentionally, due to bias
point shifts that can occur when a circuit element is driven into
nonlinearity. But maybe the gain calculations could be made in real-time.

Making a "virtual" THD meter in SPICE that is parameter-driven seems
very do-able for some of the wizards that hang out in CAD-land.
Generally speaking, one need to take the output of the circuit and notch
out or subtract the fundamental sine wave. A way to specify the upper
cutoff frequency (usually 20kHz, but should be user-adjustable). A
little waveform math to compare the amplitude of this distortion reside
as a percentage of the device's total output would then provide the
usual THD number. One could easily sum the distortion residue with the
input sine wave to get a sense of what's happening to cause high THD
numbers.

Of course, SPICE models generally provide a simplified version of real
components' nonlinearities, so the results of our virtual THD meter
would only be as good as our models, and would need to be verified in
real life. But even so, this tool, which is basic to audio design, would
be very useful during the initial design phase of a complex analog audio
circuit.

The "N" portion of THD+N is not likely to be modelable unless you add
noise sources of the appropriate amplitude and spectrum to all your
component models -- then, of course, the aforementioned virtual THD
meter would simply sum the noise with the distortion reside and give you
that "N" number, just like a real harmonic analyzer.

 

[Mike Engelhardt]

Mike,

Is there a way to get an estimation of the THD+N of an
audio amp in LTSpice? Ideally, I'd like to plot THD+N
against frequency & possibly temperature...

Noise and distortion would come from different simulations.
You can compute noise from .noise analysis. An example
is supplied as ./examples/Educational/noise.asc. Noise
density is automatically plotted as a function of frequency.
You can integrate that in the waveform viewer to the noise
over a bandwidth. You can also plot noise density as a
function of temperature or anything else. See the example
stepnoise.asc to plot noise density as a function of tail
resistor of a diff pair. Note that many SPICE models don't
have noise modeled. Unless you verify that each device's
noise is modeled, you're just going to be looking at the
Johnson noise of the resistances.

The distortion can be reached with a .tran analysis and
subsequent FFT's of the waveform data or a .four commands.
Usually you have to turn off waveform compression and
stipulate a small timestep for this to give meaning full
results. The .four command can give THD from a specified
number of harmonics. The simulation can be stepped over
temperature or a parameter to step frequency. The results
are printed in the .log file.

next question - what is the simplist way of generating
a fairly complex repetative sequence of pulses on a
number of nets? What I'm trying to do is to open & close
a lot of analogue gates in a fairly complex repative
sequence. Again, ideally I'd like to manipulate this
sequence fairly simply, rather than change a load of
PULSE statements as I do at the moment (its rather prone
to error).

The method you're using is fine. Other methods would be
to use PWL's saved in files for .wav file input/output.
See the appropriate sections of the help documentation.

--Mike

 

[ldg]

On Tue, 11 Nov 2003 16:29:24 GMT, "Mike Rocket J. Squirrel Elliott"


Here's something to play with. It's sort of a start on your spice
based thd meter, but very primitive. I decided to play with the
LTspice Laplace transforms today. Using the .params statement makes
changing the frequency easy enough. You'll probably have a much
better implementation since I've never seen the inside of a thd meter.
I saw some thd meters use a 400 hz high pass filter. This is easy to
add. So is bandlimiting with a lowpass (first order section provided)

It would help to know the characteristics of the bandstop and a block
diagram of such an instrument. I've done something very simple here.
Perhaps someone can extend this. I'm out of play time right now.

The answer comes out on meter3 in percent. The error signal is at
ERROR.

Regards,
Larry


*********************************************************************


BPFtest

* This file fakes a Distortion Analyzer. It cheats in that it uses
the
* frequency of the error component to drive a synchronous detector.
* An AC analysis will show the bandpass filter at BPout and the
Bandstop
* filter at ERROR. (Uses the BPF to BSF transformation 1-H(S))
* It still has a -65 fundamental component in the ERROR signal, so
could
* be better. The notch sure looks deep enough though.

***********************************************************************
.param tone = 1000
.param noise = 2000

VIN1 1 0 SIN(0 0.005 'noise' 0 0 0) AC 1
* noise signal 5mv pk

VIN2 2 1 SIN(0 0.5 'tone' 0 0 0)
* input tone 0.5v pk

XU1 2 BPout bpf1p PARAMS: HO = 1 FOP = 'tone' ZETAP = 0.2
* Bandpass filter

Esum ERROR 0 BPout 2 1
* Sums output of filter with input to make BSF

Vpul1 Pulse1 0 pulse(1 -1 0 1n 1n '0.5/noise' '1/noise')
* ok, I faked a rectifier

XU2 0 ERROR 0 Pulse1 RECT1 0 idmult
* does the rectification

Vpul2 Pulse2 0 pulse(-1 1 0 1n 1n '0.5/tone' '1/tone')
* faked another rectifier
XU3 0 Bpout 0 Pulse2 RECT2 0 idmult
* does the other rectification

XU4 Rect1 Fil1 LPF1P PARAMS: HO = 1 FOP = 20
* LPF at 20 hz
XU5 Rect2 Fil2 LPF1P PARAMS: HO = 1 FOP = 20
* LPF at 20 hz

Escale1 meter1 0 Fil1 0 'pi/2'
* I didn't have to scale this here, but I did . . .
* And I really faked a meter %
Escale2 meter2 0 Fil2 0 '(pi/2)'
Bscale3 meter3 0 v = 106*V(meter1)/V(meter2)
* note the 06 fudge . . .

***********************************************************************
*.AC DEC 200 1 1E8
.TRAN 10u 0.055 .005

***********************************************************************
..SUBCKT BPF1P IN OUT PARAMS: Ho='1' Fop=1000 Zetap=0.01
EBPF OUT 0 IN 0 LAPLACE =
+
(Ho*((2*Zetap*S)/(2*pi*Fop))/((S/(2*pi*Fop))^2+(2*Zetap*S)/(2*pi*Fop)+1))
..ENDS BPF1P

***********************************************************************
.SUBCKT IDMULT NIN1 PIN1 NIN2 PIN2 OUT REF
EMUL OUT REF POLY(2) (PIN1, NIN1) (PIN2, NIN2) 0 0 0 0 1
.ENDS IDMULT

***********************************************************************
..SUBCKT LPF1P IN OUT PARAMS: Ho='1' Fop='1000'
ELP OUT 0 IN 0 LAPLACE = Ho/(1+S/(2*pi*Fop))
.ENDS LPF1P

***********************************************************************
.END

 

[ldg]

next question - what is the simplist way of generating a fairly
complex repetative sequence of pulses on a number of nets? What I'm
trying to do is to open & close a lot of analogue gates in a fairly
complex repative sequence. Again, ideally I'd like to manipulate this
sequence fairly simply, rather than change a load of PULSE statements
as I do at the moment (its rather prone to error).

Use the .params? It's still a pain to set up, but easier with
equations. Then it's really easy to change . .

Regards,
Larry

 

[Mike Rocket J. Squirrel Elliott]

On Tue, 11 Nov 2003 16:29:24 GMT, "Mike Rocket J. Squirrel Elliott"


Here's something to play with. It's sort of a start on your spice
based thd meter, but very primitive. I decided to play with the
LTspice Laplace transforms today. Using the .params statement makes
changing the frequency easy enough. You'll probably have a much
better implementation since I've never seen the inside of a thd meter.
I saw some thd meters use a 400 hz high pass filter. This is easy to
add. So is bandlimiting with a lowpass (first order section provided)

Generally speaking, the high-pass function on a THD meter is used to
block powerline-related noise (ripple) so that you are measuring the
harmonics of the input signal and not those harmonics plus a bunch of
hum and stuff. Not needed, I don't think, in a SPICE meter, since our
power supplies are so supremely quiet.

It would help to know the characteristics of the bandstop and a block
diagram of such an instrument.

Hm. For the bandstop, your hardware-based harmonic analyzers usually
have 20kHz and 80kHz cutoffs. A fourth-order Butterworth would be fine.

A block diagram. I could probably source the block diagram of a Sound
Technology 1701A -- an industry workhorse. It would take a couple of
days. Interested? E-mail me at my (munged) e-mail address.

I've done something very simple here.

Perhaps someone can extend this. I'm out of play time right now.

Larry, that you even took some time to work on this is very cool.

Oh -- for the LTspice conversant, is Larry's syntax okay? The OP asked
about LTspice (which I use, too). He uses ^2 to mean square, doesn't
that have to be ** in LTspice?

Mike Rocket J Squirrel Elliott

 

[ldg]

Oh -- for the LTspice conversant, is Larry's syntax okay? The OP asked
about LTspice (which I use, too). He uses ^2 to mean square, doesn't
that have to be ** in LTspice?

I was using LTspice for the sims. I found the ^2 in the help file.

Actually the filters came from something I did a long while ago in
another simulator. I think it was called Pspice or P something at any
rate . (Where's JIm? I'm in trouble.)

At any rate, I converted the syntax to LTspice as follows:
..
SUBCKT BSF1P IN OUT PARAMS: Ho=1 Foz=1000 Fop=1000 Zetap=0.02
EBSF OUT 0 IN 0 LAPLACE =
+(Ho*POW(S/(2*pi*Foz),2)+1)/(POW(S/(2*pi*Fop),2)+2*Zetap*S/(2*pi*Fop)+1)
..ENDS BSF1P

I sort of had this working in LTspice for a direct bandstop. It
worked in the ac analysis, but not in the transient. At that point I
converted it to the bandpass which is very close and did the
transformation. At the same time I found the note in the help file
for the ^ exponentiation,



Regards,
Larry

 

[Mike Rocket J. Squirrel Elliott]

I was using LTspice for the sims. I found the ^2 in the help file.

Oh right. "The Boolean XOR operator, "^" is understood to mean
exponentiation "**" when used in a Laplace expression."

Actually the filters came from something I did a long while ago in
another simulator. I think it was called Pspice or P something at any
rate . (Where's JIm? I'm in trouble.)

At any rate, I converted the syntax to LTspice as follows:
.
SUBCKT BSF1P IN OUT PARAMS: Ho=1 Foz=1000 Fop=1000 Zetap=0.02
EBSF OUT 0 IN 0 LAPLACE =
+(Ho*POW(S/(2*pi*Foz),2)+1)/(POW(S/(2*pi*Fop),2)+2*Zetap*S/(2*pi*Fop)+1)
.ENDS BSF1P

I sort of had this working in LTspice for a direct bandstop. It
worked in the ac analysis, but not in the transient. At that point I
converted it to the bandpass which is very close and did the
transformation. At the same time I found the note in the help file
for the ^ exponentiation,

Thanks for the update!

 

[Kevin Aylward]

Mike,

So Mike, have you ever consisded basing a Spice engine on evolutionary
GA, Genetic Algorithms? It might be that for really large circuits they
might be much faster. People are using it for all sorts of stuff, like
optimisation, but I don't recall anyone actually trying the make the
basic engine GA based. It certainly works for our brains pretty
effectively, well unless your name happens to end in Bush.


http://www.anasoft.co.uk/replicators/index.html

Kevin Aylward
[email protected]
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.

Understanding, is itself an emotion, i.e. a feeling.
Emotions or feelings can only be "understood" by
consciousness. "Understanding" consciousness can
therefore only be understood by consciousness itself,
therefore the "hard problem" of consciousness, is
intrinsically unsolvable.

Physics is proven incomplete, that is, no
understanding of the parts of a system can
explain all aspects of the whole of such system.

 

[Mike Deblis]

The .four command can give THD from a specified
number of harmonics. The simulation can be stepped over
temperature or a parameter to step frequency. The results
are printed in the .log file.

Thanks for that - A typical THD analyser is essentially a 6 terminal
device - floating input for source, floating input for output from
amplifier, ground and output. The output is typically in % or dB of
the DUT output. Units normaly have a 400Hz high pass filter and a
30KHz & 80KHz low-pass (Butterworth 4 pole or similar). You can't just
subtract the input from the output of the DUT as there may be phase &
amplitude differences - you need to extract the fundamental of the
input and notch that from the DUT output. I would hope that this could
be done but I know little about the subtleties of SPICE in general...

Whatever, such a device would be of *great* use to audio engineers. If
the "black box" also supported intermodulation tests (notch both
signals), all the better ;-) The "Black box" could contain the test
signal source, thus simplifying the determination of the test
frequenc(y|ies) and hence the notches required for the output of the
DUT. Help from the SPICE gurus? Please?

The method you're using is fine. Other methods would be
to use PWL's saved in files for .wav file input/output.
See the appropriate sections of the help documentation.

As suggested elsewhere, I've moved to using .params which make life a
whole lot easier - so many features, so little time!

Thanks for a great utility - I like the manual on the Yahoo forum -
very useful reading when on the train ;-)

Mike

 

[Kevin Aylward]

Thanks for that - A typical THD analyser is essentially a 6 terminal
device - floating input for source, floating input for output from
amplifier, ground and output. The output is typically in % or dB of
the DUT output. Units normaly have a 400Hz high pass filter and a
30KHz & 80KHz low-pass (Butterworth 4 pole or similar). You can't just
subtract the input from the output of the DUT as there may be phase &
amplitude differences - you need to extract the fundamental of the
input and notch that from the DUT output. I would hope that this could
be done but I know little about the subtleties of SPICE in general...

Standed Spice itself (e.g. SuperSpice) also has direct small signal
plots of THD and IMD against frequency. This is a ".disto" run. This can
be a lot easier for doing initial design.

Kevin Aylward
[email protected]
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.

http://www.anasoft.co.uk/replicators/index.html

Understanding, is itself an emotion, i.e. a feeling.
Emotions or feelings can only be "understood" by
consciousness. "Understanding" consciousness can
therefore only be understood by consciousness itself,
therefore the "hard problem" of consciousness, is
intrinsically unsolvable.

Physics is proven incomplete, that is, no
understanding of the parts of a system can
explain all aspects of the whole of such system.

 

[Jim Thompson]

So Mike, have you ever consisded basing a Spice engine on evolutionary
GA, Genetic Algorithms? It might be that for really large circuits they
might be much faster. People are using it for all sorts of stuff, like
optimisation, but I don't recall anyone actually trying the make the
basic engine GA based. It certainly works for our brains pretty
effectively, well unless your name happens to end in Bush.

[snip]

Careful there. We're going to start drafting smart-asses who are here
on H1B's ;-)

...Jim Thompson

 

[Mike Rocket J. Squirrel Elliott]

Thanks for that - A typical THD analyser is essentially a 6 terminal
device - floating input for source, floating input for output from
amplifier, ground and output. The output is typically in % or dB of
the DUT output. Units normaly have a 400Hz high pass filter and a
30KHz & 80KHz low-pass (Butterworth 4 pole or similar). You can't just
subtract the input from the output of the DUT as there may be phase &
amplitude differences - you need to extract the fundamental of the
input and notch that from the DUT output.

You're right -- I overlooked that.

 

[Mike Rocket J. Squirrel Elliott]

Kevin Aylward wrote:

[snip]

Standed Spice itself (e.g. SuperSpice) also has direct small
signal plots of THD and IMD against frequency. This is a ".disto"
run. This can be a lot easier for doing initial design.

That's true, and I've used it in my ISspice days. I seem to recall it
wasn't very sensitive -- could not read low values of distortion or
something.

Regardless, a proper THD meter needs to operate during .TRAN runs as
viewing the distortion residue waveform is, to a designer very useful
and more informative than just the %THD number.

A THD v Frequency plot test is useful for production testing -- it's a
handy QC test that doesn't require a lot of skill to interpret.

 

[Mike Engelhardt]

Jim,

[snip]

Careful there. We're going to start drafting
smart-asses who are here on H1B's ;-)

Isn't KA a naturalized US citizen that
retreated back to the UK when he couldn't
make it as an IC designer in the US? He
should be able to renounce citizenship to
avoid the draft.

--Mike

 

[Jim Thompson]

Jim,

[snip]

Careful there. We're going to start drafting
smart-asses who are here on H1B's ;-)

Isn't KA a naturalized US citizen that
retreated back to the UK when he couldn't
make it as an IC designer in the US? He
should be able to renounce citizenship to
avoid the draft.

--Mike

I'm not sure. I had the impression he was a Brit working for TI in
the Dallas area.

But, no matter, can't we just use him for target practice ?

...Jim Thompson

 

[ldg]

As Kevin pointed out, it's a small signal analysis. Since much of thd
is associated with the nonidentities of large signal swings (crossover
distortion, distortion near the rails, etc.) it has limited use (also
pointed out by Kevin).

Regards,
Larry

 

[Jim Thompson]

As Kevin pointed out, it's a small signal analysis. Since much of thd
is associated with the nonidentities of large signal swings (crossover
distortion, distortion near the rails, etc.) it has limited use (also
pointed out by Kevin).

Regards,
Larry

Distortion analysis in PSpice is done in a .TRAN situation and applies
accurately to the amplitude used for test.... you must vary amplitude
to get a full picture of distortion.

...Jim Thompson

 

[ldg]

Distortion analysis in PSpice is done in a .TRAN situation and applies
accurately to the amplitude used for test.... you must vary amplitude
to get a full picture of distortion.

...Jim Thompson

In Smartspice .disto is small signal - like ac analysis. I hope we're
talking about the same statement call.

Examples

..DISTO DEC 10 1KHZ 100Meghz
..DISTO DEC 10 1KHZ 100Meghz 0.9

(From their very own help file

Regards,
Larry

 

[Jim Thompson]

In Smartspice .disto is small signal - like ac analysis. I hope we're
talking about the same statement call.

Examples

.DISTO DEC 10 1KHZ 100Meghz
.DISTO DEC 10 1KHZ 100Meghz 0.9

(From their very own help file

Regards,
Larry

Differences between PSpice and Berkeley SPICE2

The version of SPICE2 referred to is SPICE2G.6 from the University of
California at Berkeley.

PSpice runs any circuit that SPICE2 can run, with these exceptions:

1. Circuits that use .DISTO (small-signal distortion) analysis. U.C.
Berkeley SPICE supports the .DISTO analysis, but contains errors.

Also, the special distortion output variables (e.g., HD2 and DIM3) are
not available.

Instead of the .DISTO analysis, we recommend running a transient
analysis and looking at the output spectrum using the Fourier
transform mode in Probe. This technique shows the distortion
(spectral) products for both small-signal and large-signal distortion.

===

You also get a list of percent THD and percent distortion versus
harmonic number in the .OUT file. (You need to ask for it in the
..TRAN setup boxes.)

...Jim Thompson