EEVblog Electronics Community Forum
Electronics => Beginners => Topic started by: petergriffin56 on October 25, 2020, 06:34:05 pm

I've been following schematics and explanations regarding how to make an LC oscillator (with the goal being a regen receiver) using an op amp. Unfortunately I don't understand why this circuit doesn't work, I've tried quite a few things but to no avail. What am I missing here ?
All the examples are from typical LC oscillators :
(https://i.stack.imgur.com/l0Xz0.png)
(https://i.stack.imgur.com/c9NY2.png)
And here is an example of the same circuit being used as a regen receiver :
(https://www.celnav.de/hamradio/ELFReceiver1.jpg)

What is the resonant frequency of your LC circuit?
Your operational amplifier probably has a too low slew rate for the resonant frequency of your LC circuit, choose a fast operational amplifier

Resonant frequency is 17KHz, the bode plot above the circuit is 130000Hz and its flat. The OP AMP is rated to 500MHz, I don't think this is the issue.

Resonant frequency is 17KHz, the bode plot above the circuit is 130000Hz and its flat. The OP AMP is rated to 500MHz, I don't think this is the issue.
You should choose a higher value for C1 (90pF is too low for such a low frequency) , lat's say at least 1nF and a inductance L2 of 90mH

I don't see the difference between 900mH  100pF and 90mH  1nF but I tried it anyway, doesn't make a difference.

So how exactly it does not work? What is on the output? Your circuit should oscillate. 17khz? Choose something like 20mH and 3.3nF. Ratio of L and C may need tuning to achieve desired receiving characteristics.

I provided the test circuit with the output plot (freq vs amplitude). As you can see it is flat. The ratio of L/C is correct, when keeping L and C only (by removing the amplifier) it is resonant at the correct frequency. I am just trying to add some regeneration with the op amp, hoping to increase the Q and narrow the bandwidth. I have basically copied the circuit from the "ELF regenerative receiver" at this point, but mine just does not work and I have no idea why.

People have posted similar difficulties with oscillators before.
A likely problem is that simulation components are perfect.
A "real world" oscillator depends on the presence of a small amount of noise to start the feedback,no initial signal, no feedback, no oscillation.
There is a workaround which has appeared on this forum, but knowing next to nothing about simulation packages, I can 't remember what it was.

If you have too much positive feedback and it does oscillate into saturation, then it will not be an amplifier anymore.

Before the AC analysis you should try a transient analysis to see if it oscillates, if the gain is too high then it will saturate immediately and you won't see anything in the ac analysis. In such case try lowering the gain and positive feedback e.g. R1=100ohm, R2=100k.
The optimal gain will of course depend on the L2 series resistance.

Before the AC analysis you should try a transient analysis to see if it oscillates, if the gain is too high then it will saturate immediately and you won't see anything in the ac analysis. In such case try lowering the gain and positive feedback e.g. R1=100ohm, R2=100k.
The optimal gain will of course depend on the L2 series resistance.
Good point, this may be a case of a simulated "perfect" LC tank if there is no ESR modeled. In that case very little feedback will send it into oscillation, which is not expected if we compare to real life LC tank.

I have tried different gains and feedback resistor values, doesn't change anything really. In fact it oscillates at any frequency with the same amplitude, not just the resonant. I have a series resistance in the inductor of 3.7K, I just used the values from the datasheet of the inductor I plan to use. The series resistance is there but just no visible on the schematic.
I've simplified the circuit in the hopes of making things clearer, right now I'm trying a colpitts type oscillator. Still no luck. I don't know what to do, still the same flat response... In transient simulation nothing either, tried feeding an AC waveform, DC and no input signal at all, does nothing.
By the way the OP AMP is not the problem here, BW is 500MHz, and I've tried a few different models.

Try building a real world oscillator instead of wasting your time with LTspice simulations.
You will understand a lot of things .... for example, try to build a 900mH inductor !!!!! ://
You will understand why you have to use a much larger capacitor and a smaller inductor.
In addition, it is necessary to adjust the gain of the amplifier if not, either it does not oscillate, or it saturates.

Series resistance of inductor 3.7k? That looks way too large, Q will be extremely small and resonant behavior almost non exixting. In my opinion, try something like 10  50 Ohms.

The inductor is a 900mH telecoil from Knowles, with series resistance of 3.7K. Q is around 26 at 17.4KHz, I was under the impression you could negate losses in an LC circuit with feedback, effectively increasing the Q. Just not sure how to do that.

Such inductor is probably used for filtering and not LC tanks. Also note, that if you have very large L and small C the frequency may be right, but the bandwith will be large, Q very small and again resonace not expressed strongly. I never build a regen receiver, but I imagine, that in general you want smaller L, and bigger C and not too high ESR to begin with.

The system is for detecting nearby magnetic fields at the resonance frequency, so more turns = higher voltage. Of course it comes with downsides but I'm hoping with a regen receiver I can increase the Q factor of the LC resonant circuit.
It seems to work better, but I'm not sure what the component values mean, I just changed them until I got something decent. But I have no idea if this is optimal.

It seems to work better, but I'm not sure what the component values mean, I just changed them until I got something decent. But I have no idea if this is optimal.
The openloop gain is G=1+R1/R2 and R3 controls the positive feedback via the voltage divider R3LC tank, the positive feedback gain GFB is given by this voltage divider. At resonance the LC tank will have a real impedance (resistance) proportional to the Q factor of the tank circuit so that GFB is real and positive. The closed loop gain is given by G/(1G*GFB) therefore oscillations will appear spontaneously when G*GFB=1. You increase GFB by decreasing R3.
But you probably won't easily see the threshold in an AC analysis, you need a transient analysis. Close to the threshold the simulation time has to be long enough to see if the amplitude stabilizes or grows exponentially. Maybe another method would be to replace the sin input by a noise and see if spontaneous oscillations occur. Yet another method is to modify momentarily the circuit to measure GFB separately and then calculate the threshold values.

It seems what you are describing is similar to this : (https://upload.wikimedia.org/wikipedia/en/thumb/f/fa/Negative_resistance_by_positive_feedback.svg/800pxNegative_resistance_by_positive_feedback.svg.png)
I've tried this, voltage follower OP AMP with a resistor to match the DC resistance of the inductor. It seems to be working as the oscillation is more stable in the long run.
In the same wikipedia article they talk about "Q multiplication" : https://en.wikipedia.org/wiki/Negative_resistance#Q_enhancement (https://en.wikipedia.org/wiki/Negative_resistance#Q_enhancement)
I was under the impression this was how regeneration receivers operated, by cancelling the inductor resistance and therefor increasing the Q factor of the circuit. But with my circuit the frequency analysis stays the same with or without the feedback, the bandpass doesn't get narrower or "peakier".
They mention "So if the loop gain A is greater than one, Rin will be negative". I've switched from a voltage follower to an non inverting amplifier with a gain of 1.1 while keeping the same regeneration resistor. Looks very strange, both in transient and frequency analysis.
Results from both simulations are attached.

It seems what you are describing is similar to this : (https://upload.wikimedia.org/wikipedia/en/thumb/f/fa/Negative_resistance_by_positive_feedback.svg/800pxNegative_resistance_by_positive_feedback.svg.png)
I've tried this, voltage follower OP AMP with a resistor to match the DC resistance of the inductor. It seems to be working as the oscillation is more stable in the long run.
It is not quite the same, because you don't necessarily want to match the DC resistance of the inductor at all frequencies, only at the resonance frequency.
In the same wikipedia article they talk about "Q multiplication" : https://en.wikipedia.org/wiki/Negative_resistance#Q_enhancement (https://en.wikipedia.org/wiki/Negative_resistance#Q_enhancement)
I was under the impression this was how regeneration receivers operated, by cancelling the inductor resistance and therefor increasing the Q factor of the circuit.
Yes, negative resistance is just another way to express the effect of closedloop gain enhancement by positive feedback. Actually I prefer the closedloop formulation for practical calculations but it will be the same if you calculate the effective resistance.
But with my circuit the frequency analysis stays the same with or without the feedback, the bandpass doesn't get narrower or "peakier".
You must be careful with the ac analysis, actually I don't know how many periods LTSpice effectively uses to measure the gain. Close to the threshold the buildup of oscillation amplitude is so slow that I'm not sure the ac analysis will capture it (numerically speaking it will appear only in higher order terms in the expansion around the DC bias point ? I don't see it yet).
Any LTSpice experts here ? I'm curious to know it too.
They mention "So if the loop gain A is greater than one, Rin will be negative". I've switched from a voltage follower to an non inverting amplifier with a gain of 1.1 while keeping the same regeneration resistor. Looks very strange, both in transient and frequency analysis.
Maybe your feedback gain is so high (regenaration resistor too small) that you won't see much difference between a gain of 1 and 1.1 (G*GFB>>1 anyway)
I suggest to measure the GFB directly: remove the opamp and record the Bode plot of the feedback voltage divider composed by R3 and LC tank.
For a regen you should then set G*GFB slightly lower than 1 at resonance. (For a superregen it would be slightly higher).

I don't want to match the DC resistance of the inductor only at the resonant frequency ? So I have to take the DC resistance (80ohm) and add the AC losses e.g reactance at the resonant frequency ?
Could you explain how to calculate the correct feedback resistor value ? I'm not sure I understood your suggestion to test it in LTspice. I've tried lots of values for the resistor, with barely any change.
As for LTspice AC analysis, I had a feeling something fishy was going on here, I was wondering the same thing (how many oscillations per frequency). Can't quite put my finger on it yet. I'll try a few more things and tell you if I can pinpoint what is going on.

I don't want to match the DC resistance of the inductor only at the resonant frequency ? So I have to take the DC resistance (80ohm) and add the AC losses e.g reactance at the resonant frequency ?
Just forget it for the moment, actually the calculations made this way are more complicated.
Could you explain how to calculate the correct feedback resistor value ? I'm not sure I understood your suggestion to test it in LTspice. I've tried lots of values for the resistor, with barely any change.
Make a circuit with just a voltage divider: R3 (top) and the LC tank (bottom). Then apply a sin to the top of the divider and measure the voltage (attenuation) at the middle point. This will give you GFB vs frequency. The gain will have a maximum at the resonance frequency, let's say it's 6db , a factor of two attenuation. The threshold G*GFB=1 will then be defined by G=2, i.e 1+R1/R2=2 or R1=R2.

I think I got it down, at the verge of oscillation I get a really high selectivity. Thanks a lot for the help.
I think the AC analysis for LTspice works fine until you reach the point of oscillation, once you do it gets messy. One funny thing I've noticed is that the plot gives you the maximum value at a specific frequency, regardless of how long it gets there. This means at resonance, the AC plot gives me "26mv", only thing is, it takes around 150 milliseconds to get there, at 17.4KHz, thats a lot of time.
Last thing, what kind of OP AMP should I look for ? What specifications matter most ? Assuming the bandwidth is sufficient, should I be looking at offset voltage ? Voltage noise ? Since this is a feedback circuit, isn't the output noise just as important as input noise ?

I think the AC analysis for LTspice works fine until you reach the point of oscillation, once you do it gets messy. One funny thing I've noticed is that the plot gives you the maximum value at a specific frequency, regardless of how long it gets there. This means at resonance, the AC plot gives me "26mv", only thing is, it takes around 150 milliseconds to get there, at 17.4KHz, thats a lot of time.
Yes, this was a question I was asking myself too in my last post, I don't know how the ac mode exactly works in LTSpice and I suspected it might not be reliable when the circuit is close to an instability like in regen conditions (maybe there is a way to tune some numerical parameters but I didn't find any info on that). At least we have both learned something :)
Last thing, what kind of OP AMP should I look for ? What specifications matter most ? Assuming the bandwidth is sufficient, should I be looking at offset voltage ? Voltage noise ? Since this is a feedback circuit, isn't the output noise just as important as input noise ?
Offset voltage shouldn't be a concern because your gain G=1+R1/R2 is not very high I suppose. You just need a good low noise opamp. Don't forget that the effective bandwidth is the opamp gainbandwidth product divided by G you actually have, that said for 17kHz most models should provide a very large bandwidth margin. Actually I'm not a specialist in this low frequency range (I'm doing RFVHF most of the time) but I'm sure you will get many great advices from experts here.