Why is the output of this LM324 op-amp circuit 0V? Orcad/pspice question

Question

I'm trying to make a function generator using three op-amps, specifically the LM324. Right now I'm trying make the first square wave output using a DC input:

My OrCad simulation's output constant comes out as a zero, no matter what I do:

What did I do wrong?

This is the full circuit I am trying to make:

This is my attempt at it. Since my op-amp outputs keep coming out as a 0 I can not seem to produce any wave function at all:

I feel like if I can just get the first op-amp result going then the rest of my op-amps will produce the desired graphs as well. (Unless I'm missing something.)

Answer 1

Seems that power supplies are not "wired" (no dots ?).
Your timebase is too short. It should be at least of 300 ms.
With my simulator, it start promptly. (2 ways).

Here is the simulation of the circuit you are trying to make ...
Change of one resistor R4 (100k -> 10k).

Answer 2

It is likely stuck in a quasi-stable state. It may eventually start oscillating if your simulation runs long enough.

Rather than that, try replacing one or both power supplies with sources that switch on just into the simulation.

Here is an LTspice simulation with universal op-amp 2 (a single pole op-amp with one internal node, slew rate limit and output voltage and current limit):

It does not start oscillating until more than 1 second of simulated time has passed. The simulated output voltage starts at zero (a red flag with positive feedback) and only changes by a few microvolts during the first 500ms.

Here is the same circuit with the V+ supply delayed by one nanosecond after simulation starts:

The difference is obvious even with the short simulation time- the output immediately jumps to +5V rather than unnaturally sitting at 0V, though with 10ms of simulation you don't see the start of oscillation because it's too short for the 100ms time constant.

Answer 3

In your circuit, the triangle wave amplitude will vary inversely with frequency; as you vary the freq of the squarewave oscillator, the integrator has more or less time to ramp, changing the resulting peak-to-peak amplitude.

There is a better configuration of three opamps for what you are trying to do. The first amp is a comparator with hysteresis. One input is the reference and one is the output of the integrator. As you vary R9 (the integrator input), the integration time changes but the amplitude remains constant, determined only by the comparator.

Here is a screen grab from way back. It looks like part of a TI app note. It shows the comparator reference as Vcc/2. If you replace this with a pot, changing the pot wiper voltage changes the triangle wave symmetry.

Here is another example of the square and triangle parts.

http://www.piclist.com/images/www/hobby_elec/e_ckt16.htm