OpAmp - LTspice XVII

Thread Starter

Ramussons

Joined May 3, 2013
871
I was trying to simulate some opamp circuit in LTSpice and was coming to a dead end everywhere. I did some trouble shooting and finally landed on a strange behaviour.
Attached is a simple asc file of an opamp with the + input tied to output, - input grounded.

Under this condition, afaik, the output should be at Vcc+ or Vcc-. But it is at 0 volts.

Can someone please tell me what is going on?
 

Attachments

OBW0549

Joined Mar 2, 2015
3,551
Under this condition, afaik, the output should be at Vcc+ or Vcc-. But it is at 0 volts.

Can someone please tell me what is going on?
I think @Alec_t nailed it.

Unless told to do otherwise, Spice begins every .TRAN and .AC analysis with a .OP analysis to determine a starting point for the circuit's operation. I've found that very often with bi-stable circuits such as the one you posted, Spice will perversely converge on some initial operating point wherein the circuit is "balanced on a knife edge" between its two stable states-- something that simply doesn't happen in real life due to natural random noise or outside interference acting to get things underway. Oscillator circuits that mysteriously refuse to start oscillating are another common result of this behavior.

To get around this I usually insert something into the circuit (like a PWL or PULSE voltage source) to force the starting state I want.
 
Last edited:

ci139

Joined Jul 11, 2016
1,696
? what circuit model you use for the x741 chip
// -- /!\ the uAh741.asc is experimental transistor model of the thing not too much tested /!\
// -- i may have better v. of it but it's what i found now ... to be compared with the macro models
Draft2.png
 

Attachments

Thread Starter

Ramussons

Joined May 3, 2013
871
? what circuit model you use for the x741 chip
// -- /!\ the uAh741.asc is experimental transistor model of the thing not too much tested /!\
// -- i may have better v. of it but it's what i found now ... to be compared with the macro models
View attachment 216622




I used this.
https://forum.allaboutcircuits.com/threads/how-to-add-op-amp-741-to-lt-spice.139069/

And I get this.
1599574482452.png

Maybe, I'll have to look for other 741 models or use Bordodynov's LM358.

Thank you all.
 
Last edited:

Thread Starter

Ramussons

Joined May 3, 2013
871
Not quite 0, but a theoretically stable point. Try editing the simulation command by ticking the 'Skip initial operating point solution ' check box.
Thank you. This makes the difference in the given asc. Let me try this in my main simulation.
 
Top