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???
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.
-- Tim Wescott Wescott Design Services http://www.wescottdesign.com
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
That engineer made a mistake and found his error...
Don't know. But my experience is that Spice failures mostly are caused by bad models, or cockpit error ;-)
Circuits designed by people claiming no trust in Spice ?:-)
...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC\'s and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |
"Winners never quit, quitters never win", Jack Bradley Budnik ~1956
Oscillators.
Argh-- a myth dating back to the 1930s-- a myth popular because it attacks the sience and engineering world.
Best regards, Spehro Pefhany
-- "it\'s the network..." "The Journey is the reward" speff@interlog.com Info for manufacturers: http://www.trexon.com Embedded software/hardware/analog Info for designers: http://www.speff.com
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
schrieb im Newsbeitrag news: snipped-for-privacy@z14g2000cwz.googlegroups.com...
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
Hello Spehro,
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
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.
--
Thanks,
- Win
[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
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC\'s and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |
"Winners never quit, quitters never win", Jack Bradley Budnik ~1956
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 snipped-for-privacy@anasoft.co.uk
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.
Post a circuit, that doesn't sound right, even with Multisim.
...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC\'s and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |
"Winners never quit, quitters never win", Jack Bradley Budnik ~1956
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.
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
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.
----== Posted via Newsfeeds.Com - Unlimited-Unrestricted-Secure Usenet News==----
----= East and West-Coast Server Farms - Total Privacy via Encryption =----
Real oscillators start up because of noise.
Or power-on transients, and if you include that in your simulation in LTSpice then they start just fine.
-- Tim Wescott Wescott Design Services http://www.wescottdesign.com
or supply turn on
-- -- kensmith@rahul.net forging knowledge
ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.