Circuits that shouldn't work...?

[[email protected]]

I remember someone once posted about a circuit that Spice said should
be unstable, yet when built, the circuit works perfectly fine.

What circuit was this? What other circuits don't work in simulations,
but work perfectly fine in real life???

 

[Charles Schuler]

I remember someone once posted about a circuit that Spice said should
be unstable, yet when built, the circuit works perfectly fine.

What circuit was this? What other circuits don't work in simulations,
but work perfectly fine in real life???

Oscillators.

 

[Tim Wescott]

Oscillators.

LTSpice, surprisingly enough, seems to do a pretty good job with
oscillators. Whatever they did to it to optimize it for switching power
supplies seems to have made it fit for this, as well.

You still have all those dang parasitics, so it won't go into the RF
without lots of work characterizing components, but that's another story.

 

[Jim Thompson]

I remember someone once posted about a circuit that Spice said should
be unstable, yet when built, the circuit works perfectly fine.

What circuit was this?

Don't know. But my experience is that Spice failures mostly are
caused by bad models, or cockpit error ;-)

What other circuits don't work in simulations,
but work perfectly fine in real life???

Circuits designed by people claiming no trust in Spice ?

...Jim Thompson

 

[Helmut Sennewald]

I remember someone once posted about a circuit that Spice said should
be unstable, yet when built, the circuit works perfectly fine.

What circuit was this? What other circuits don't work in simulations,
but work perfectly fine in real life???

Hello,

we still wait for the circuits. I remember that somebody
(sorry I forgot his name) want bring the circuits
next week. This was many months ago. Let's hope he reads
this thread and bring the circuits now. I admit that
there may be circuits where SPICE fails because the
models are not good enough or SPICE doesn't take noise
into account.

I know of one circuit where SPICE calculates very precisely
a mathematical correct solution for a noiseless circuit,
but in real life the output of this circuit would run to
the rails because of noise at the inputs. It' a very very
simple circuit. You wouldn't believe it when you haven't seen it.

Best regards,
Helmut

 

[Joerg]

I remember someone once posted about a circuit that Spice said should
be unstable, yet when built, the circuit works perfectly fine.

What circuit was this? What other circuits don't work in simulations,
but work perfectly fine in real life???

Happens a lot. IIRC there was a clear statement but NASA engineers that
they have mathematical proof that a bumblebee cannot fly. Well, all I
can tell is that until last summer they did fly. Not very graciously,
but fly they did.

Regards, Joerg

 

[John Larkin]

I remember someone once posted about a circuit that Spice said should
be unstable, yet when built, the circuit works perfectly fine.

What circuit was this? What other circuits don't work in simulations,
but work perfectly fine in real life???

If you set the time step wrong, you can make an R-C oscillate in
Spice. It gets especially nasty with high-Q things like crystal
oscillators, or circuits having a huge range of time constants.

John

 

[[email protected]]

Happens a lot. IIRC there was a clear statement but NASA engineers that
they have mathematical proof that a bumblebee cannot fly. Well, all I
can tell is that until last summer they did fly. Not very graciously,
but fly they did.

Regards, Joerg

That engineer made a mistake and found his error...

http://quest.arc.nasa.gov/people/journals/aero/wellman/bumblebee.html

 

[Spehro Pefhany]

Happens a lot. IIRC there was a clear statement but NASA engineers that
they have mathematical proof that a bumblebee cannot fly. Well, all I
can tell is that until last summer they did fly. Not very graciously,
but fly they did.

Argh-- a myth dating back to the 1930s-- a myth popular because it
attacks the sience and engineering world.

http://www.math.niu.edu/~rusin/known-math/98/bees



Best regards,
Spehro Pefhany

 

[Joerg]

Hello Spehro,

Argh-- a myth dating back to the 1930s-- a myth popular because it
attacks the sience and engineering world.

http://www.math.niu.edu/~rusin/known-math/98/bees

You are right, seems like one of those. I guess that scientist threw
quite a fit when he learned that media folks had overheard him say that.

Regards, Joerg

 

[Kevin Aylward]

Hello,

we still wait for the circuits. I remember that somebody
(sorry I forgot his name) want bring the circuits
next week. This was many months ago. Let's hope he reads
this thread and bring the circuits now. I admit that
there may be circuits where SPICE fails because the
models are not good enough or SPICE doesn't take noise
into account.

I know of one circuit where SPICE calculates very precisely
a mathematical correct solution for a noiseless circuit,
but in real life the output of this circuit would run to
the rails because of noise at the inputs. It' a very very
simple circuit. You wouldn't believe it when you haven't seen it.

Ho hum, *any* high gain amp with zero offset will give zero output in
spice with zero input yet its real life embodiment will rail out. So,
whats new?

GIGO.

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.

 

[Helmut Sennewald]

Ho hum, *any* high gain amp with zero offset will give zero output in
spice with zero input yet its real life embodiment will rail out. So,
whats new?

GIGO.

Kevin Aylward

Hello Kevin,

My circuit is an amplifier(E-source) in an inverting circuit,
but by mistake the resistors are connected to the positive input.
LTspice and any other SPICE will find a solution which
is mathematically correct, but you will be unable to reproduce
that with any real circuit. The calculated ouput voltage is
-1.0002V with the wrong circuit and -0.9998V with the correct
inverting circuit.

Again, the math done by SPICE is correct in both cases!
Everybody would say the inputs are wrongly connected,
but SPICE is so clever and finds a solution you never
have seen in any book! Patent pending!


Have fun and a happy new year.

Best regards,
Helmut


R2 R1
in ___ N001 ___
V1 ---<___>----o-----<___>------o----out
(1V) | | (-1.0002V)
| --- |
---|+ |--------
---|- |-- v=10000
_|_ --- _|_
- E1 -



This would be the correct circuit.

R2 R1
in ___ N001 ___
V1 ---<___>----o-----<___>------o----out
(1V) | | (-0.9998V)
| --- |
---|- |--------
---|+ |-- v=10000
_|_ --- _|_
- E1 -



The result(V(out)=-1.0002V) from all SPICE programs.

--- Operating Point ---

V(out): -1.0002 voltage
V(n001): -0.00010002 voltage
V(in): 1 voltage




Here is the netlist for every SPICE.

* D:\Share\strange1.asc
E1 out 0 N001 0 10000
R1 out N001 1k
R2 in N001 1k
V1 in 0 1
..op
..end



The schematic file "strange1.asc" for LTspice.

Version 4
SHEET 1 880 680
WIRE -112 128 -112 48
WIRE -112 256 -112 208
WIRE -48 48 -112 48
WIRE 128 48 32 48
WIRE 128 160 128 48
WIRE 192 160 128 160
WIRE 192 256 192 208
WIRE 208 48 128 48
WIRE 240 144 240 112
WIRE 240 256 240 224
WIRE 320 48 288 48
WIRE 320 112 240 112
WIRE 320 112 320 48
WIRE 368 112 320 112
FLAG 192 256 0
FLAG 240 256 0
FLAG -112 256 0
FLAG 368 112 out
FLAG -112 48 in
SYMBOL e 240 128 R0
SYMATTR InstName E1
SYMATTR Value 10000
SYMBOL res 304 64 M270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R1
SYMATTR Value 1k
SYMBOL res -64 64 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R2
SYMATTR Value 1k
SYMBOL voltage -112 112 R0
SYMATTR InstName V1
SYMATTR Value 1
TEXT -120 -56 Left 0 !.op

 

[Jim Thompson]

Hello Kevin,

My circuit is an amplifier(E-source) in an inverting circuit,
but by mistake the resistors are connected to the positive input.
LTspice and any other SPICE will find a solution which
is mathematically correct, but you will be unable to reproduce
that with any real circuit. The calculated ouput voltage is
-1.0002V with the wrong circuit and -0.9998V with the correct
inverting circuit.

Again, the math done by SPICE is correct in both cases!
Everybody would say the inputs are wrongly connected,
but SPICE is so clever and finds a solution you never
have seen in any book! Patent pending!


Have fun and a happy new year.

Best regards,
Helmut


R2 R1
in ___ N001 ___
V1 ---<___>----o-----<___>------o----out
(1V) | | (-1.0002V)
| --- |
---|+ |--------
---|- |-- v=10000
_|_ --- _|_
- E1 -



This would be the correct circuit.

R2 R1
in ___ N001 ___
V1 ---<___>----o-----<___>------o----out
(1V) | | (-0.9998V)
| --- |
---|- |--------
---|+ |-- v=10000
_|_ --- _|_
- E1 -

[snip]

But you haven't proven anything. The ideal E-source (infinite input
Z, zero output Z, no phase shift, no offset voltage, noiseless)
doesn't exist in the real world.

...Jim Thompson

 

[Winfield Hill]

Helmut Sennewald wrote...

My circuit is an amplifier(E-source) in an inverting circuit,
but by mistake the resistors are connected to the positive
input. LTspice and any other SPICE will find a solution which
is mathematically correct, but you will be unable to reproduce
that with any real circuit. The calculated ouput voltage is
-1.0002V with the wrong circuit and -0.9998V with the correct
inverting circuit.

Again, the math done by SPICE is correct in both cases!
Everybody would say the inputs are wrongly connected,
but SPICE is so clever and finds a solution you never
have seen in any book! Patent pending!

R2 R1
in ___ N001 ___
V1 ---<___>----o-----<___>------o----out
(1V) | | (-1.0002V)
| --- |
---|+ |--------
---|- |-- v=10000
_|_ --- _|_
- E1 -


This would be the correct circuit.

R2 R1
in ___ N001 ___
V1 ---<___>----o-----<___>------o----out
(1V) | | (-0.9998V)
| --- |
---|- |--------
---|+ |-- v=10000
_|_ --- _|_
- E1 -

The result(V(out)=-1.0002V) from all SPICE programs.

--- Operating Point ---

V(out): -1.0002 voltage
V(n001): -0.00010002 voltage
V(in): 1.00 voltage

Like Jim, I'm not surprised to see this for E voltage-controlled
voltage-sources, but I was surprised when I substituted an opamp
model (I tired NSC's LF411 and a uA741, doesn't matter), and got
the same result for the initial DC operating point. However,
when I did something real, a transient analysis, the improperly
wired opamp nicely latched up immediately after the input-signal
was disturbed (even a nV of change was enough).

So I'm sorry, Helmut, but as Jim says, we can still rely on our
spice programs, if properly used.

BTW, when I tried the wrong opamp pins in Electronics Workbench a
few years ago, it gave the improper answer you saw for E elements.
But it's possible they've fixed their default opamp model by now.

 

[Tim Shoppa]

I remember someone once posted about a circuit that Spice said should
be unstable, yet when built, the circuit works perfectly fine.

What circuit was this? What other circuits don't work in simulations,
but work perfectly fine in real life???

Getting back to basics, Spice doesn't handle two capacitors in series
with no DC connection to the inner node. But in the real world
it often makes sense to put resistors etc in parallel to share
voltages etc equitably too.

With overly simplistic models of op-amps etc., circuits that depend on
noise or certain behavior as outputs/inputs hit rails won't work well
at all. This is not a fundamental weakness of Spice but just overly
simplistic models.

Spice at one point was a rather bad way to model an oscillator
but the increase in CPU horsepower over the past couple of decades
has made it reasonable... sometimes!

Tim.

 

[Lacy]

I use Multisim 2001 and the only circuits I know it will not handle at all
are CMOS Oscillators. For some goofy reason (which may just be normal for
Spice), it doesn't "see" the capacitor and treats it as a short( this is
what I have found at EWB website). The result is that the gate propogation
delay is what is determining the frequency of oscillation.

If anyone has come up with a solution, I would be more than happy to listen.
Otherwize I just have to use a signal source and pretend it is made up of
CMOS gates.

 

[Jim Thompson]

I use Multisim 2001 and the only circuits I know it will not handle at all
are CMOS Oscillators. For some goofy reason (which may just be normal for
Spice), it doesn't "see" the capacitor and treats it as a short( this is
what I have found at EWB website). The result is that the gate propogation
delay is what is determining the frequency of oscillation.

If anyone has come up with a solution, I would be more than happy to listen.
Otherwize I just have to use a signal source and pretend it is made up of
CMOS gates.

Post a circuit, that doesn't sound right, even with Multisim.

...Jim Thompson

 

[Charles Schuler]

Real oscillators start up because of noise.

 

[Ken Smith]

Real oscillators start up because of noise.

or supply turn on

 

[Cor blimey mate]

Oscillators.

Thye do work but you need to supply an impulse to get them going.

Tam