Can anyone explain this effect?

P

Paul Burridge

Guest
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.
--

"What is now proved was once only imagin'd." - William Blake, 1793.
 
Paul Burridge wrote:
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?
Click to expand...
Your obviously not using SS, cos it works fine here.

Kevin Aylward
salesEXTRACT@anasoft.co.uk
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 wrote:

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?
Click to expand...
Turn off waveform compression and try again.
 
"analog" <analog@ieee.org> schrieb im Newsbeitrag
news:4148886D.8C30D055@ieee.org...
Paul Burridge wrote:

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.
Click to expand...
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
 
On Wed, 15 Sep 2004 20:56:11 +0200, "Helmut Sennewald"
<helmutsennewald@t-online.de> wrote:

"analog" <analog@ieee.org> schrieb im Newsbeitrag
news:4148886D.8C30D055@ieee.org...

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.
Click to expand...
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...
--

"What is now proved was once only imagin'd." - William Blake, 1793.
 
On Wed, 15 Sep 2004 18:11:52 GMT, "Kevin Aylward"
<salesEXTRACT@anasoft.co.uk> wrote:

Paul Burridge wrote:
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.
Click to expand...
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.
--

"What is now proved was once only imagin'd." - William Blake, 1793.
 
Paul Burridge wrote:
On Wed, 15 Sep 2004 18:11:52 GMT, "Kevin Aylward"
salesEXTRACT@anasoft.co.uk> wrote:

Paul Burridge wrote:
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.

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.
Click to expand...
Oh?

The plot was too
small to make out its shape.
Click to expand...
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.
Click to expand...
Send me a gif screen shott of what you have.

Kevin Aylward
salesEXTRACT@anasoft.co.uk
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.
 
"Helmut Sennewald" <helmutsennewald@t-online.de> a écrit dans le message de
news:cia2te$i5b$00$1@news.t-online.com...
"analog" <analog@ieee.org> schrieb im Newsbeitrag
news:4148886D.8C30D055@ieee.org...

Paul Burridge wrote:

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.

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.
Click to expand...
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 ?


--
Thanks,
Fred.
 
On Thu, 16 Sep 2004 06:16:01 GMT, "Kevin Aylward"
<salesEXTRACT@anasoft.co.uk> wrote:

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.
Click to expand...
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.
--

"What is now proved was once only imagin'd." - William Blake, 1793.
 
Paul Burridge wrote:
Fred Bartoli wrote:

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 ?
Click to expand...
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. :-/
Click to expand...
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. :)
 
"Paul Burridge" <pb@notthisbit.osiris1.co.uk> wrote in message
news:eek:ttik0lc2glmku9d0tmke144g663jigrm1@4ax.com...
On Thu, 16 Sep 2004 06:16:01 GMT, "Kevin Aylward"
salesEXTRACT@anasoft.co.uk> wrote:

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

Leon
 
On Thu, 16 Sep 2004 17:26:55 GMT, "Kevin Aylward"
<salesEXTRACT@anasoft.co.uk> wrote:

Paul Burridge wrote:
On Thu, 16 Sep 2004 06:16:01 GMT, "Kevin Aylward"
salesEXTRACT@anasoft.co.uk> wrote:

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:

There aint on my system. Send me a screen shott so I can determine what
your problem is.
Click to expand...
Will do. As soon as I get back from the pub. (abt. 3 hrs.)
--

"What is now proved was once only imagin'd." - William Blake, 1793.
 
On Thu, 16 Sep 2004 14:11:49 GMT, analog <analog@ieee.org> wrote:


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. :)
Click to expand...
Thanks. I'll take a look...

--

"What is now proved was once only imagin'd." - William Blake, 1793.
 
"Paul Burridge" <pb@notthisbit.osiris1.co.uk> schrieb im Newsbeitrag
news:q2uik0p8i3hrav9qpbspfpl8qgeeeht1bg@4ax.com...
On Thu, 16 Sep 2004 08:19:29 +0200, "Fred Bartoli"
fred._canxxxel_this_bartoli@RemoveThatAlso_free.fr_AndThisToo> wrote:


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. :-/
--
Click to expand...

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
 
"JeffM" <jeffm_@email.com> wrote in message
news:f8b945bc.0409161245.4db50a28@posting.google.com...
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
Click to expand...
If your in an MS-OS you can hit <shift> <Print Screen> go to paint and past it.
Crop the portion you want to save and save it as a image. Is THAT want you
wanted?
 
"Kevin Aylward" <salesEXTRACT@anasoft.co.uk> schrieb im Newsbeitrag
news:Bca2d.8123$U04.6730@fe1.news.blueyonder.co.uk...
Paul Burridge wrote:
On Wed, 15 Sep 2004 20:56:11 +0200, "Helmut Sennewald"
helmutsennewald@t-online.de> wrote:

"analog" <analog@ieee.org> schrieb im Newsbeitrag
news:4148886D.8C30D055@ieee.org...

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.

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.
Click to expand...
Hello Kevin and Paul,
the reason for compression "on" as a default are the DC/DC converter
simulations. Here the total simulation time is very long compared to
the oscillator period and thus a lot of data is generated. Compression
keeps that at a reasonable size. It's simply some kind of LT-customers
have first prority.

Maybe the hint to switch it off for any distortion measurement or some
other simulations should be more clearly stated in the help file.


Best Regards,
Helmut
 
On Thu, 16 Sep 2004 21:35:11 GMT, "Clarence" <No@No.Com> wrote:

"JeffM" <jeffm_@email.com> wrote in message
news:f8b945bc.0409161245.4db50a28@posting.google.com...
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

If your in an MS-OS you can hit <shift> <Print Screen> go to paint and past it.
Crop the portion you want to save and save it as a image. Is THAT want you
wanted?
Click to expand...
It doesn't work. Maybe that key's died. I've now e-mailed a photo of
the screen to Kev so don't worry about it.
--

"What is now proved was once only imagin'd." - William Blake, 1793.
 
On Thu, 16 Sep 2004 23:52:02 +0200, "Helmut Sennewald"
<helmutsennewald@t-online.de> wrote:

Hello Kevin and Paul,
the reason for compression "on" as a default are the DC/DC converter
simulations. Here the total simulation time is very long compared to
the oscillator period and thus a lot of data is generated. Compression
keeps that at a reasonable size. It's simply some kind of LT-customers
have first prority.

Maybe the hint to switch it off for any distortion measurement or some
other simulations should be more clearly stated in the help file.
Click to expand...
Thanks, Helmut.
I may as well turn it off, then. One thing I never get involved with
simulating is power supplies (ironic, given it's half the rationale -
SwitcherCAD).
--

"What is now proved was once only imagin'd." - William Blake, 1793.
 
On Thu, 16 Sep 2004 20:09:23 GMT, analog <analog@ieee.org> wrote:

Helmut Sennewald wrote:

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 :)
Click to expand...
Don't take any notice, Helmut; he's just jealous. :)

--

"What is now proved was once only imagin'd." - William Blake, 1793.
 
analog wrote:
Helmut Sennewald wrote:

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.
Click to expand...
I have to agree.

Kevin Aylward
salesEXTRACT@anasoft.co.uk
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top