Colpitt Oscillator in LTSpice

Thread Starter

MikeElec

Joined Jul 13, 2020
3
Hello everybody,

I am new to this forum and also to LTSpice.
I try to use this software to simulate a common-base Colpitts oscillator as described on the Wikipedia page.
https://fr.wikipedia.org/wiki/Oscillateur_Colpitts

I have tested this circuit on a breadboard vith a 3.3V power supply . It works and delivers a 1.3 Vpp sine wave at 16.72 MHz.
But I cannot get any sine wave with my simulation. The collector voltage goes to 3.3 V and stays there.

I suspect a bad configuration of the simulation parameters. I have used the .STARTUP directive in TRAN but without success.
I have also tryied Tina-TI from Texas. Same bad results.

Thank you for your help

MikeElec
 

Attachments

Last edited by a moderator:

Alec_t

Joined Sep 17, 2013
12,744
Try inserting a voltage source of, say, 1mV @ 1meg in series in the power rail to provide a bit of 'noise' to kick the oscillator into action. Run the sim for a few mS, not umpteen seconds.
 

crutschow

Joined Mar 14, 2008
29,521
Here's the working simulation:
I removed the STARTUP directive, and a value for the Maximum Timestep (why did you put that in?).
Normally you don't need a Maximum Timestep value as LTspice automatically adjusts that.

1594649896759.png
 

DarthVolta

Joined Jan 27, 2015
521
Try inserting a voltage source of, say, 1mV @ 1meg in series in the power rail to provide a bit of 'noise' to kick the oscillator into action. Run the sim for a few mS, not umpteen seconds.
Thanks I'll have to try that, I haven't done much with osc. circuits in general, and in LTspice I've had sim fail when real world worked and I didn't know why.
 

Bordodynov

Joined May 20, 2015
2,983
For more realistic results, I took a single-layer 5mm diameter inductive coil. I made the calculation using the free Russian program Coil64. This program takes into account the skin effect. I also added parasitic inductances of elements. Their magnitude is determined by the design of the circuit. I took 10nHenry.
2020-07-14_08-46-29.png2020-07-14_09-18-48.png2020-07-14_09-21-08.png
 

Thread Starter

MikeElec

Joined Jul 13, 2020
3
Thanks to everybody.
I do appreciate your responsiveness.

Meanwhile I have found the directive : .tran 0 1m 0 01n on a LTSpice related video on Youtube. I tryied it and it worked !

However, I am a little bit surprised by the amplitude resulting from the various computations : about 5 Vpp.
I found the same value with my simulation. But from my breadboard I only get 1.3 Vpp. It is not so critical for my application but this difference is quite surprising.

MikeElec
 

crutschow

Joined Mar 14, 2008
29,521
As Bordodynov's last simulation shows, just a small stray output load capacitance due to wiring and the scope probe can cause a significant difference in the output voltage.
Those and other strays aren't simulated unless they are deliberately added.
Stray circuit impedances usually have only a small effect on circuit performance at low frequencies, but become more significant as the signal frequency gets higher.
 

Thread Starter

MikeElec

Joined Jul 13, 2020
3
Yes, you are right !
One do not imagine the influence of these additional R and C at these frequencies but it is real.
Moreover, I was observing the signal with a TEK2201 which has a 20 MHz bandwith. A little bit short.
Now, with an other scope with a 500 MHz bandwith the story is different.

MikeElec
 

Bordodynov

Joined May 20, 2015
2,983
Hey Bordodynov, how did you add those inductances to the wires in LTspice??

I'm using LTspice IV and I don't know if it is a feature in this version.

Thanks
I have an extensive library of additional models. I've also included my models of parasitic elements in it. In order not to distort (clutter) the circuit very much, I depicted parasitic resistances and inductances as a small line. I also have a parasitic capacitance depicted as a point. Initially the values of these elements are not shown in the symbol - just small lines and dots. In this example, I entered the symbols of the parasite elements and made their values visible.
You can find more models on my web page:
http://bordodynov.ltwiki.org/
 

LvW

Joined Jun 13, 2013
1,428
However, I am a little bit surprised by the amplitude resulting from the various computations : about 5 Vpp.
I found the same value with my simulation. But from my breadboard I only get 1.3 Vpp. It is not so critical for my application but this difference is quite surprising.
Did you consider the limited slew rate in your analyses?
Did you check the SPICE model in this regard?
 

sparky 1

Joined Nov 3, 2018
704
Wikapedia example could be improved. The circuit could be arranged differently. So that first time experieced could include setting the gain and setting the LC tank resonance. To me that has a better incentive. A more simplified approach might look like this:
https://www.a8blog.com/en_cap3.htm
 
Last edited:
Top