I am trying to get an oscillator using CD4069 inverters to work in LT Spice. It doesn't oscillate. What's the trick?

 

hi d335,
Welcome to AAC.
Please post your LTS asc file and we can try to run it.
E

 

Oscillators rely on a variety of small effects to get started. These effects are often missing from simulations with ideal components. They are "too ideal" to oscillate. Techniques range from introducing parasitic elements to noise into the simulation.

 

hi d335,
Created this LTS model from a Pspice model.net cd4069UB
Works fairly well, little tweak required , the 1nn.
E

 

Look here:

 

Here is my simple drawing. I don't have a real model of a 4069; I just used the generic 'inv' available.

 

Yikes why are you connecting pin 8 on the "A" parts to a voltage source!!?

 

Didn't know what pin that 'extra' pin was, so I assumed it was the supply pin. How shoul;d I draw it?

 

Didn't know what pin that 'extra' pin was, so I assumed it was the supply pin. How shoul;d I draw it?

It is for unconnected inputs. The voltage that the device uses defaults to 1 volt. It is set by a device parameter.
Read the Help page for the "A" devices. Here is an excerpt:

A. Special functions.
INV, BUF, AND, OR, and XOR are generic idealized behavioral gates. All gates are netlisted with eight terminals. These gates require no external power. Current is sourced or sunk from the complementary outputs, terminals 6 and 7, and returned through device common, terminal 8. Terminals 1 through 5 are inputs. Unused inputs and outputs are to be connected to terminal 8.

I would connect it to GND

 

I did connect it to ground. Got this message: "time step too small; initial timepoint: trouble with buf-instance a1". Still no oscillation

 

If you do not have a model of a CD4069 they why and how can you simulate a circuit that uses it??

 

I just thought that the generic inverter symbol would work. Where can I get a CD4069 model?

 

If you do not have a model of a CD4069 they why and how can you simulate a circuit that uses it??

Either he doesn't know of or hasn't downloaded a library, like the one from Bordodynov, which has a symbol with correct parameters to model the behavior of CD4000 series chips.

 

I just thought that the generic inverter symbol would work. Where can I get a CD4069 model?

I don't have a good answer for you at the moment, but I'm working on it.

 

Either he doesn't know of or hasn't downloaded a library, like the one from Bordodynov, which has a symbol with correct parameters to model the behavior of CD4000 series chips.

In your opinion, how accurate are these models? A 4069 for example?

 

Simulation models have only typical specs. The datasheet lists the minimum and maximum range of specs that are very different.

 

In your opinion, how accurate are these models? A 4069 for example?

They are behavioral models. You can read read the actual text files that implement them. Besides the logic functions they model propagation delay, rise time, fall time and voltage levels. In some cases they use the LTspice OTA devices and in other cases they use a combination of ideal components with generic parameters. Here is the one for the 4069. It uses two diodes, a resistor, a capacitor, two MOS transistors, one n-channel and one p-channel, and a final capacitor. What do you think?

.subckt HEF4069UB a out VDD VSS params: speed=1
D1 A VDD di
D2 VSS A di
R a o 700
Ca o VSS {10p*M} Rpar=1G
M3 OUT o VSS VSS HEFn
M4 OUT o VDD VDD HEFp
C4 OUT VSS {10p*M} Rpar=1G
.model di d vfwd=0.5 ron={100/M}
.model Hefn vdmos vto=1.3 kp={speed*1.1m*M} lambda=15m rs={50/speed/m} mtriode=2.5
.model Hefp vdmos pchan vto=-1.5 kp={speed*1.1m*M} lambda=45m rs={70/speed/m} mtriode=1
.ENDS

 

See

 

The simulation shows perfectly symmetrical N-channel and P-channel Mosfets.
I wish they could make them and sell all of them like that.

 

hi d335,
This is a LTSpice zip file for the CD4069UB.
Unzip it, move the asy file to the Auto Generated folder, see image.
Keep the other files in there own folder.

Ask if you have a problem

E