square triangle wave generator -[NOob]

Thread Starter

Santa klaus

Joined Nov 16, 2014
32
I did the simulation for square triangle wave opamp on ltspice. but i don't know where to put the input signal. i get zero signals everywhere help
 

Attachments

RichardO

Joined May 4, 2013
2,271
You have told LTspice to stop simulating at 2 seconds. What frequency do you expect to see?

Also, it is often a problem using an op-amp without selecting a specific part. LTspice defaults to a model that does not always do what you would expect.
 

Thread Starter

Santa klaus

Joined Nov 16, 2014
32
You have told LTspice to stop simulating at 2 seconds. What frequency do you expect to see?

Also, it is often a problem using an op-amp without selecting a specific part. LTspice defaults to a model that does not always do what you would expect.
i tried increasing simulation time but i don't get the square and triangle signals. there is no signal at all
 

RichardO

Joined May 4, 2013
2,271
Did you select specific models for the op-amps?

You need to answer the question... What frequencies do you expect to see?
 

Thread Starter

Santa klaus

Joined Nov 16, 2014
32
maybe my question wasn't clear. what i meant was, do i need to apply an input voltage at the first stage, or is the circuit supposed to work like this. I am confused because there needs to be an input voltage/current for an opamp circuit, right?
 
Last edited:

shteii01

Joined Feb 19, 2010
4,644
maybe my question wasn't clear. what i meant was, do i need to apply an input voltage at the first stage, or is the circuit supposed to work like this. I am confused because there needs to be an input voltage/current for an opamp circuit, right?
Astable multivibrator does not need external input to start it.
 

crutschow

Joined Mar 14, 2008
25,675
An alternate way to get it to oscillate is to check the "Skip Initial operating point solution" (uic) in the "Edit Simulation Command" box.

Hint: The no-oscillation problem is related to the calculated circuit DC initial operating point that Spice performs at the start of the simulation by default.

As another interesting experiment with this problem, try injecting a small single short current pulse (say 1us, 1ua) into the input of one of the op amp inputs delayed by 1ms (without the .ic or uic commands).
 

MikeML

Joined Oct 2, 2009
5,444
great it works. i don't know why though. could you explain the .ic V(Y) = 1u?
That is the key to making it oscillate. Prior to a TRANSIENT (time domain) simulation, all Spice-derived simulators try to place all of the nodes in the circuit to a voltage derived from the way the circuit is biased. That puts the nodes where the circuit is ready to do what it is going to do later, but because, unlike in the real world, the simulation is noiseless, there is no perturbation to get amplified so that oscillation starts.
Try Goggling "metastability".

The .ic directive tells LTSpice that you want to override the zero V that would have come from the bias solution at node Y with 1uV instead. When the time domain solution begins, the feedback loop is now unbalanced (by a tiny 1uV), but that is amplified and the feedback causes the oscillation to begin (immediately). There are an infinite number of ways to create this initial perturbation that it takes to get the circuit going...

This is a common problem when simulating oscillators. You have to account for the normal thermal noise that is naturally occurring in any circuit when dealing with oscillators...
 

JoeJester

Joined Apr 26, 2005
4,390
You don't need initial conditions IF you can start the transient analysis at zero and not compute the operating conditions prior to the start of the analysis.

Here are my options for doing a transient analysis. I typically start with zero and do not need to apply initial conditions .... even when using the ideal op amps.
 

Attachments

Last edited:

MikeML

Joined Oct 2, 2009
5,444
I quote myself:
... There are an infinite number of ways to create this initial perturbation that it takes to get the circuit going...
The metastability problem comes up only in simulating oscillators or flip-flops; not with amplifiers. Skipping the initial DC bias solution is not appropriate for most of the circuits you will simulate.
 
Top