Schmitt trigger using opamp simulation problem

[kgavionics]

Hi
It have a little problem simulating non inverting schmitt trigger using orcad and multisim.
this is the schematic and the simulation values in orcad and i have the same values in multisim.



According to my calculation when i apply 1 v dc the output should go to the positive rail 15V, but here i have -2V why?????
when i apply -5V in input i got 10V in output. it completely false.It's suppose to work like a normal comparator with hysteresis and the UT and LT is accordingly 7.5 and -7.5V.

can someone figure out what's the problem?

thanks in advance

 

[BradtheRad]

I was fooled by the response the first time I ran this (or similar) circuit in a simulator. Evidently its model (of an ideal op amp) fails to duplicate some correct behavior that occurs in a real op amp.

With some experimentation, it turned out that the input voltage needed to go above or below the supply rails, and then the output started to do what it's supposed to do.

- - - Updated - - -

I'm running a similar schematic to yours. At first the output would not change state.

I played with volt level at the inverting input. I played with resistor values. I increased the gain. Finally I got the output to change state.

I'm sure you'll get proper response by experimenting the same way.

 

[kgavionics]

Thanks BradtheRad for this quick reply.I'm a long time multisim user and when run the simulation on it,i suspected that the problem is coming from it.I have some friend that told me that Orcad is the best sim for analog components.it turned out that it's not that good.I can tell you that nothing can replace actual experimentation.

 

[kgavionics]

Update:
I tried the circuit on falstad circuit simulator and believe or not it is working like a charm despite it's basic functionality it surpassed pspice. We must not under estimate this basic simulator.

 

[LvW]

kgavionics - it is not the simulator who is wrong.
Make a calculation by hand - and you will see that a stable bias point is possible (theoretically !).
So - what was wrong? You have made a dc analysis assuming (perhaps without knowing) that there is a stable bias point (the dc sources are on since infinite times).
To see the latching behaviour it is necessary to perform an analysis in the time domain (TRAN analysis) with a real opamp model (including a certain time delay because of its frequency-dependence).
This works satisfactorily with any Spice-based simulator.

 

[kgavionics]

thanks LvW for your reply.I tried Time domain analysis ( transient) in pspice with an LM324 opamp and it gives me the same thing.you told me to add a certain time delay and i'am wondering how can i do it for DC source.

thanks in advance

 

[BradtheRad]

Update:
I tried the circuit on falstad circuit simulator and believe or not it is working like a charm despite it's basic functionality it surpassed pspice. We must not under estimate this basic simulator.

Glad to hear Falstad's simulator brought you success this time. I think it deserves notice for its ease of use, animation, and interaction.

Just the same it appears that every simulator requires some getting used to. You see, Falstad's was the simulator I was running and it gave me the incorrect behavior I mentioned.

Op amps are a complicated component, making it more difficult to create a model of their behavior. You can aim for simplicity (making it easy for the novice to use), or you can aim for realism (which is needed by the professional).

 

[LvW]

thanks LvW for your reply.I tried Time domain analysis ( transient) in pspice with an LM324 opamp and it gives me the same thing.you told me to add a certain time delay and i'am wondering how can i do it for DC source.
thanks in advance

While saying "time domain analysis" I think, of course, on a signal source which is switched on at t=0 (Vpulse instead instead of a dc source).
It makes no real sense to make a TRAN analysis with a dc source that is considered to be existent since infinite times.

 

[FvM]

I don't see power supply terminals in the simulation circuit, thus I guess you simply selected an inappropriate ideal OP model. If you use a real OP, you won't get a physically inplausible operation point.

Where do the claimed +/- 7.5 V come from? Can you show the complete set of model parameters?

 

[kgavionics]

Now i understand your point LvW.I'm gonna try the simulation with a pulse source.
@FvM : I tried with LM324 opamp with -15 and +15V power rails and it gave me the same thing.The -7.5 and +7.5 Vols are the lower and upper trigger levels.

thanks

 

[LvW]

kgavionics - If you like - I could give you some background information.

Imagine the case of two balls - one upon the other one.
Ist this a stable system? Yes - under idealized conditions, which means: Absolutely no external mechanical disturbance! Of course, this is not realistic, hence it will be unstable.
Here, we have a similar situation:
Assuming that the power rails and the input signal do exist (and remain absolutely constant) during calculation of the bias point we have no step signal (with corresponding transients) and the amplifier output will not latch because a stable bias point was found by the program. Therefore, we must use realistic conditions - at least as far the input signal is concerned (switch-on at t=0). Even more realistic is a switch-on of the power supplies (step voltage) at t=0 or some milliseconds later.

 

[FvM]

I get saturation of the LM324 schmitt-trigger output to +14V with LTSpice starting from the initial transient solution. Maybe it's behaving slightly different than Orcad. It's however known that SPICE solution can converge to an unstable operation point under certain conditions. The latest when you apply a disturbance, e.g. a small voltage step, the equilibrium will be destroyed.

 

[kgavionics]

kgavionics - If you like - I could give you some background information.

Imagine the case of two balls - one upon the other one.
Ist this a stable system? Yes - under idealized conditions, which means: Absolutely no external mechanical disturbance! Of course, this is not realistic, hence it will be unstable.
Here, we have a similar situation:
Assuming that the power rails and the input signal do exist (and remain absolutely constant) during calculation of the bias point we have no step signal (with corresponding transients) and the amplifier output will not latch because a stable bias point was found by the program. Therefore, we must use realistic conditions - at least as far the input signal is concerned (switch-on at t=0). Even more realistic is a switch-on of the power supplies (step voltage) at t=0 or some milliseconds later.

Thanks for the analogy.Now i understand very well.

- - - Updated - - -

I get saturation of the LM324 schmitt-trigger output to +14V with LTSpice starting from the initial transient solution. Maybe it's behaving slightly different than Orcad. It's however known that SPICE solution can converge to an unstable operation point under certain conditions. The latest when you apply a disturbance, e.g. a small voltage step, the equilibrium will be destroyed.

thanks Fvm for this clarification.