I am trying to simulate the following circuit:

https://www.learningaboutelectronics.com/Articles/Astable-multivibrator-with-a-4011-NAND-gate.php


I have watched a video explaining how to add the CD4000 series of chips to LTSpice, and have done that correctly, I think.. When I try to run the simulation, I get a very fast oscillation frequency. When I try to increase the period with more capacitance, strange things happen, depending on how much I increase it. Increasing it by a factor of 10, it stops oscilating altogther




Increasing the Capicance to 10000 uF (100 times more), I get the following result!

 

Please post your SPICE file.

 

The one in question comes from CD4000.zip. I have attached other files and models that are thrown into the spice file, that are not of interest to this thread, just in case.

 

Below is the sim of the circuit with some mods.

The standard LTspice model gates have a problem in that they can go into a linear mode at their input voltage transition point, causing high frequency oscillations, so I used the CD4093 Schmitt-trigger gates with input hysteresis, that prevents them from entering the linear mode.

R1 limits the input protection diodes' current when the input goes above the supply 5V or below ground, which would otherwise increase the oscillator frequency.

I used a larger timing resistor to reduce the size of the timing capacitor.
Note that the timing capacitor sees both voltage polarities across it so needs to be non-polarized, not polarized as shown in the reference schematic.

Edit: See corrected schematic in post #6.

 

Shouldn't R1 be protecting the inputs of U3?

 

Shouldn't R1 be protecting the inputs of U3?

Opps.
You are correct.
Corrected schematic below: