MOSFET ring oscillator LT SPICE

Question

I am designing a ring oscillator using MOSFETS to create the inverters however, I am encountering problems with the output. Please check my understanding. Here is what I understand: the oscillating frequency should be:

$$F_{osc} = \frac{1}{2NT_{p}}$$

This is the most general case. To change the propagation delay, you can add load capacitors between each inverter stage and the frequency of oscillation can be calculated if you know the current through the transistor and the load capacitor. The frequency of oscillation becomes:

$$SlewRate = \frac{I_{ss}}{C_{L}}$$

$$T_{propagation} = \frac{V_{sw}}{SlewRate}$$

where $$V_{sw}$$ is the switching voltage of the inverter. And the equation for the oscillation frequency becomes:

$$F_{osc}=\frac{I_{ss}}{2NV_{sw}C_{L}}$$

And the inverter propagation delay is the average of the low to high and high to low propagation delay:

$$T_{prop} = \frac{T_{PLtoH}+T_{PHtoL}}2$$

So with all of this information, what I understood was that you can change the oscillation frequency by changing the supply voltage, the load capacitor, or by changing the size of the transistors. The supply voltage will change Iss. The load capacitor will change the slew rate which will change the propagation delay. Changing the size of the transistors will change the Iss current which will also change the slew rate which will change the propagation delay. Let me know if I messed up anywhere.

The next part is that if I want the output to swing from VCC/2 to VCC (I chose this arbitrarily not for any specific reason but to observe behavior), then I need to set W and L the same for both transistors. I did this and simulated the oscillator. The output is a flat line that doesn't oscillate. Here is the simulated output:

Here is the schematic:

I set w=50nm and L =1u. Can someone please explain why my inverter isn't oscillating and check if I made any errors with my understanding? I appreciate the effort. If any additional information is needed, please let me know and I will provide this information. The MOSFET models I am using are nmos4 and pmos4.

update: I added a pulse source on the feedback network and got this result

here is the schematic.

The circuit did not oscillate after adding a disturbance siganl. The disturbance signal was a pulse.

Answer 1

Of course, you are not seeing any oscillations, as you use a default N/PMOS model, and this model is the Shichman-Hodges model, threshold-based model, which does not model device capacitances.

You can introduce device capacitances into consideration by specifying the model level parameter. Setting LEVEL=14, like in a statement '.model NL14 NMOS LEVEL=14' below, gives you the BSIM4.6.1 model:

The other directives to notice are '.ic V(inout)=0.3' -- without this directive the oscillation start is delayed; and length/width parameters of the transistors. To bring MOSFET length/width parameter to the screen, right-click on the device symbol with ctrl key pressed and mark the Vis field. The parameter values are in the field 'Value2'.

You can experiment with different model level parameter values, like 9 or 12 -- see LTspice help, only do not forget to read messages appearing in the SPICE Error Log.