Can anyone explain this effect?

[Paul Burridge]

Hi guys,

May I direct your attention to the following:

http://www.burridge8333.fsbusiness.co.uk/triangle.gif

Where you will find a very simple common-source FET stage that gives
some rather odd results when simulated. It feeds a 0.5mV AC sine
voltage of 10Khz to the gate of the FET. The output is a reasonable
replication of the input signal shape, but upon removing the inductor
(which I had to insert to prevent this problem) the output turns into
a perfect triangle wave. This gross distortion of the input signal
only seems to happen at very small input levels, but nevertheless, I
can think of nothing in the real world that might explain it. Could it
be some sort of peculiarity with the intricacies of spice signal
sources of which I am ignorant? If not, how is this sine-to-triangle
conversion taking place?

THanks,

p.

 

[Kevin Aylward]

Hi guys,

May I direct your attention to the following:

http://www.burridge8333.fsbusiness.co.uk/triangle.gif

Where you will find a very simple common-source FET stage that gives
some rather odd results when simulated. It feeds a 0.5mV AC sine
voltage of 10Khz to the gate of the FET. The output is a reasonable
replication of the input signal shape, but upon removing the inductor
(which I had to insert to prevent this problem) the output turns into
a perfect triangle wave. This gross distortion of the input signal
only seems to happen at very small input levels, but nevertheless, I
can think of nothing in the real world that might explain it. Could it
be some sort of peculiarity with the intricacies of spice signal
sources of which I am ignorant? If not, how is this sine-to-triangle
conversion taking place?

Your obviously not using SS, cos it works fine here.

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.

 

[analog]

May I direct your attention to the following:

http://www.burridge8333.fsbusiness.co.uk/triangle.gif

Where you will find a very simple common-source FET stage that gives
some rather odd results when simulated. It feeds a 0.5mV AC sine
voltage of 10Khz to the gate of the FET. The output is a reasonable
replication of the input signal shape, but upon removing the inductor
(which I had to insert to prevent this problem) the output turns into
a perfect triangle wave. This gross distortion of the input signal
only seems to happen at very small input levels, but nevertheless, I
can think of nothing in the real world that might explain it. Could it
be some sort of peculiarity with the intricacies of spice signal
sources of which I am ignorant? If not, how is this sine-to-triangle
conversion taking place?

Turn off waveform compression and try again.

 

[Helmut Sennewald]

Turn off waveform compression and try again.

Hello Paul,
you have two chances to do that.

1.
Control Panel -> Compression
Disable any compression


2. The better method is to control the compression mode in your schematic.

Add the following command line to your schematic.

..options plotwinsize=0


Compression is a great feature of LTSPICE. It can reduce your output
file size by a decade. And that counts a lot when you reach the
hundreds of megabytes in file size.


Best regards,
Helmut

 

[Leon Heller]

Hi guys,

May I direct your attention to the following:

http://www.burridge8333.fsbusiness.co.uk/triangle.gif

Where you will find a very simple common-source FET stage that gives
some rather odd results when simulated. It feeds a 0.5mV AC sine
voltage of 10Khz to the gate of the FET. The output is a reasonable
replication of the input signal shape, but upon removing the inductor
(which I had to insert to prevent this problem) the output turns into
a perfect triangle wave. This gross distortion of the input signal
only seems to happen at very small input levels, but nevertheless, I
can think of nothing in the real world that might explain it. Could it
be some sort of peculiarity with the intricacies of spice signal
sources of which I am ignorant? If not, how is this sine-to-triangle
conversion taking place?

It works fine for me, using Pulsonix SPICE.

Leon

 

[Paul Burridge]

Hello Paul,
you have two chances to do that.

1.
Control Panel -> Compression
Disable any compression


2. The better method is to control the compression mode in your schematic.

Add the following command line to your schematic.

.options plotwinsize=0


Compression is a great feature of LTSPICE. It can reduce your output
file size by a decade. And that counts a lot when you reach the
hundreds of megabytes in file size.

Thanks, guys. That's sorted the problem out pretty damn quick! But it
does beg the question of whether one should run LT with compression on
by default. In what circumstances is it safe to leave it on and when
should one disable it? I'm a bit worried now about getting false
results (not quite so obvious as this!) and not realising it could be
the compression feature causing it. :-/ It's not a problem I've
*knowingly* encountered before...

 

[Paul Burridge]

Your obviously not using SS, cos it works fine here.

Hi Kev,
I did *try* simulating it with SS, but came up against the familiar
old problem of the size of the graphs it produces. The plot was too
small to make out its shape. I thought you'd have addressed that
niggle by now but maybe I'm the only one who has a problem with it.
Running on a laptop didn't help though, I must admit! BTW, if there is
a way to get a full-screen view of the graph by toggling a function
key, then please let me know!

p.

 

[Kevin Aylward]

Thanks, guys. That's sorted the problem out pretty damn quick! But it
does beg the question of whether one should run LT with compression on
by default. In what circumstances is it safe to leave it on and when
should one disable it? I'm a bit worried now about getting false
results (not quite so obvious as this!) and not realising it could be
the compression feature causing it. :-/ It's not a problem I've
*knowingly* encountered before...

Personally, I think its bloody daft having compresion on by default. In
fact, its insane. The only time to have it on, is when you *really* need
it, like running out disk space. Its like cleaning the house up by
sweeping all the shit under the carpet.


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.

 

[Kevin Aylward]

Hi Kev,
I did *try* simulating it with SS, but came up against the familiar
old problem of the size of the graphs it produces.
Oh?

The plot was too
small to make out its shape.

This makes little sense to me.

I thought you'd have addressed that
niggle by now but maybe I'm the only one who has a problem with it.

Send me a gif screen shott of what you have.

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.

 

[Fred Bartoli]

Hello Paul,
you have two chances to do that.

1.
Control Panel -> Compression
Disable any compression


2. The better method is to control the compression mode in your schematic.

Add the following command line to your schematic.

.options plotwinsize=0


Compression is a great feature of LTSPICE. It can reduce your output
file size by a decade. And that counts a lot when you reach the
hundreds of megabytes in file size.

I use another spice but have LTspice installed and tried this, just out of
curiosity.
Wave compression is a nice feature but I guess I would have been caught on
this one. Well, maybe not, since I'd know the expected output frequency.
Anyway, at least in this case, compression has the same effect as
undersampling and gives plausible waveforms to the inattentive user.
Wouldn't it be feasible to detect such "undersampling" conditions and either
automatically adapt the compression or issue a warning message ?

 

[Paul Burridge]

Personally, I think its bloody daft having compresion on by default. In
fact, its insane. The only time to have it on, is when you *really* need
it, like running out disk space. Its like cleaning the house up by
sweeping all the shit under the carpet.

Hehe! Great analogy, Kev.
Anyway, about the graph problem: is there a way to copy the graph to
clipboard (as in LT) or do I have to photograph the screen with me
digicam? I'm quite happy to photograph it if there's no quick way.

p.

 

[Paul Burridge]

I use another spice but have LTspice installed and tried this, just out of
curiosity.
Wave compression is a nice feature but I guess I would have been caught on
this one. Well, maybe not, since I'd know the expected output frequency.
Anyway, at least in this case, compression has the same effect as
undersampling and gives plausible waveforms to the inattentive user.
Wouldn't it be feasible to detect such "undersampling" conditions and either
automatically adapt the compression or issue a warning message ?

Good idea. I iniitally suspected it was a time-step problem, but after
trying various combinations of frequency and time-step, it was
evidently something else, hence my query.
Do the graph files really need to be so big, anyway?? IFAICS, LT saves
the plots from *every* node, even if you're only interested in one or
two points in the circuit. Seems an unnecessary waste of disk space
IMHO. :-/

 

[analog]

In the case of Paul's circuit, the small size of the signal coming
from the voltage source seems to slip in under the compression
algorithm's radar. I suppose Mike E could modify the algorithm to
restrict compression based on the a priori knowledge of the presence
of sources with periodic waveforms.

Good idea. I iniitally suspected it was a time-step problem, but
after trying various combinations of frequency and time-step, it
was evidently something else, hence my query.
Do the graph files really need to be so big, anyway?? IFAICS, LT
saves the plots from *every* node, even if you're only interested
in one or two points in the circuit. Seems an unnecessary waste of
disk space IMHO. :-/

Yes it can be under certain circumstances. That is why there already
is a "dot" command to address this very issue. See if you can pick
it out from the "Dot Commands" sections of the help file.

 

[Leon Heller]

Hehe! Great analogy, Kev.
Anyway, about the graph problem: is there a way to copy the graph to
clipboard (as in LT) or do I have to photograph the screen with me
digicam? I'm quite happy to photograph it if there's no quick way.

Just capture it with the Prt Sc key, and then paste it into MS Paint.

Leon

 

[Kevin Aylward]

Hehe! Great analogy, Kev.
Anyway, about the graph problem:

There aint on my system. Send me a screen shott so I can determine what
your problem is.

is there a way to copy the graph to
clipboard (as in LT) or do I have to photograph the screen with me
digicam? I'm quite happy to photograph it if there's no quick way.

Yes. Click on its invisible title bar to select it. Use the menu
"Edit\copy to clipboard". This copies it as a standard bit map. You can
then paste to any other app.

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.

 

[Paul Burridge]

There aint on my system. Send me a screen shott so I can determine what
your problem is.

Will do. As soon as I get back from the pub. (abt. 3 hrs.)

 

[Paul Burridge]

Yes it can be under certain circumstances. That is why there already
is a "dot" command to address this very issue. See if you can pick
it out from the "Dot Commands" sections of the help file.

Thanks. I'll take a look...

 

[Helmut Sennewald]

Good idea. I iniitally suspected it was a time-step problem, but after
trying various combinations of frequency and time-step, it was
evidently something else, hence my query.
Do the graph files really need to be so big, anyway?? IFAICS, LT saves
the plots from *every* node, even if you're only interested in one or
two points in the circuit. Seems an unnecessary waste of disk space
IMHO. :-/
--

Hello Paul,
you can limit the nodes beeing saved.
Just add a command line withe nodes you are interested.

Example: It will save only two items in the output file.

..save V(out) I(V1)


Best regards,
Helmut

 

[analog]

Hello Paul,
you can limit the nodes beeing saved.
Just add a command line withe nodes you are interested.

Example: It will save only two items in the output file.

.save V(out) I(V1)

Best regards,
Helmut

Hi Helmut,

More than he needs the answers, Paul needs to learn how to find
the answers for himself. I may be wrong, but I think you are
enabling a grown bird to stay in the nest going "peep, peep, peep".
He should be finding at least some of his own worms by now.

Regards

 

[JeffM]

is there a way to copy the graph to clipboard (as in LT)

or do I have to photograph the screen with me digicam?
Paul Burridge

A work-around (screen capture utility):
http://www.google.com/search?&q=ScreenRip-32