Phase shift oscillator and circuit

26 replies · 6K views · last reply
suv79
Messages
65
Reaction score
0

Homework Statement


upload_2016-2-13_18-16-57.png

Circuit schematic of a phase-shift oscillator built around a TL072 op-amp, with three RC stages of 1n capacitors C1 to C3 and 1k resistors R1 to R3, a 33k feedback resistor R4, and supply labels -5V and +5V.

Gain & phase response of TL072 op-amp
Log-log Bode plot of large-signal differential voltage amplification (left axis, 1 to 10^6) and phase shift (right axis, 0 to 180 degrees) against frequency from 1 Hz to 10 MHz; amplification is flat near 10^5 at low frequency, then falls roughly linearly to about 1 at 10 MHz, while phase shift rises from 0 to 180 degrees.


Homework Equations


'Frequency of oscillation was observed to be about 15 % lower'[/B]
Why ?

The Attempt at a Solution


Handwritten working for a phase shift oscillator: f0 = 1/(2π√6RC) = 0.065/RC, then f0 = 0.065/((1×10³)(1×10⁻⁹)) giving f0 = 65000 Hz = 65 kHz, and 65000 − 15% = 55250 Hz.

so at this frequency the op-amp has 45 phase shift, but why will this impact the oscillator and lower the frequency.

PSpice simulation
Schematic of a phase shift oscillator built around a TL072 op-amp: three RC stages (C1, C2, C3 at 1n and R1, R2 at 1K, R3 at 1K) feed back from the output to the non-inverting input, with R4 at 33k in the gain network and a scope probe on the output.

analysis
PSpice transient plot of Diff Probe voltage in uV against time in seconds, showing a damped start then a sustained triangular-looking oscillation after about 0.2 s; the frequency readout reads 21.996111 Hz.

why is my frequency 22 Hz
 
An ideal opamp model in PSpice is simply called up with "OPAMP".
Regarding your result - I suppose the critical parameter is the limited slew rate which drastically lowers the frequency (and causes a triangle form).
 
but would the slew rate effect the frequency or only distort the waveform,
the phase shift oscillator should producesa sine wave output.
 
suv79 said:
but would the slew rate effect the frequency or only distort the waveform,
the phase shift oscillator should producesa sine wave output.
Yes - the slew rate SR lowers the frequency because SR causes in addition a negative phase shift (delay corresponds with phase shift).
 
I have simulated your circuit - and the result is at 55 kHz.
What are the time steps you have chosen?
My choice: End of simulation 1ms and resolution 1µs.
Why such a large simulation time for 55 kHz(1s)?

Comment: A much better waveform can be achieved if you split the feedback resistor in two (33k=23k +10k) and connect two diodes (antiparallel) across the 10k resistor.
 
Last edited:
you got 55 kHz that is what it should be about 15% lower.
 
Simulator schematic of a phase-shift oscillator: three RC stages (C3, C2, C1 at 1n and R1, R2, R3 at 1K) feeding a TL072 op-amp with R4 at 33K feedback, output to an oscilloscope, and +5 and -5 V supplies.

i think something is wrong with this iam still getting 22 Hz
 
i have to write a report about why the circuit is 15% lower from designed frequency, when the TL072 op-amp was used.

have simulated your circuit - and the result is at 55 kHz.
What are the time steps you have chosen?
My choice: End of simulation 1ms and resolution 1µs.
Why such a large simulation time for 55 kHz(1s)?

Comment: A much better waveform can be achieved if you split the feedback resistor in two (33k=23k +10k) and connect two diodes (antiparallel) across the 10k resistor.


did you use PSpice to simulated the circuit? can you see any differences between your circuit and my one ?
 
suv79 said:
could you email me your simulated circuit ?

I have simulated exactly your circuit using a realistic model for TL072.
Why didn`t you answer my question regarding simulation time amd time resolution??
 
Last edited:
the time i used was 1 Second
Simulator plot titled Tran1 Diff Probe showing Diff Probe in uV against Time in seconds from 0 to 1 with 200 ms per division, with a Frequency readout of 21.996111 Hertz above. The red trace starts with large damped oscillations near zero, then settles into a steady triangular-looking oscillation after about 0.2 seconds.

but time resolution i have no idea.
Screenshot of the Choose Analysis dialog in a circuit simulator, Transient tab selected, with Stop time set to 1, Start data output at 0, .PRINT step 20m, and Analysis Mode checkbox Transient ticked.
 
suv79 said:
the run time should not change the frequency
OK - if you know better I have no problems.
It seems you are very familiar with simulation programs.

I have again removed my explanation for the frequency variation in my answer#12.
I see no necessity to give you hints if you know better.
 
but i don't understand what is wrong with my circuit, why is it not getting 55 kHz
 
i have chanced the run time to 1m the freq is now 21 kHz
Simulator plot of Diff Probe in microvolts against time in milliseconds, 0 to 1 ms, showing an oscillating red waveform whose amplitude grows over time; top bar reads Frequency 21.081964kHertz.

but where can i change time resolution ?
 
What is the DC value of your circuit's output, and what value were you expecting it to be?

What pk-pk amplitude are the oscillations you are seeing?
 
i have no idea how to work out the amplitude of the waveform
 
Screenshot of a circuit simulator's Transient analysis settings tab, showing a Stop time field set to 1m.

why when the stop time is change dose it effect the frequency.
 
Oscilloscope-style plot of Diff Probe in microvolts against Time in microseconds, showing three oscillating traces of growing amplitude: red, green and blue, with the blue trace spreading furthest across the time axis.

red is 50 u
green is 100u
blue is 200u
 
Attachments
  • Oscilloscope-style plot of Diff Probe in uV against Time in uSecs, 20uSecs/div, with three growing oscillating traces in red, green and blue; the blue trace grows largest and the red smallest.
    upload_2016-2-15_14-58-38.png
    5 KB · Views: 561
I can't help because I don't use (or know about) Pspice (For a simple cct like this, I'd just build it!)

But going back to your first post, why do you say that the phase shift of the op amp is 45o at 55kHz? AFAI can see, it would still be close to 90o. It would appear to be 45o around 12Hz (and maybe 50MHz.) (Both taken from your graph - not checked by me.)

Looking at your Pspice output from an innocent perspective I wonder;
why your output amplitude is so small?
whether you would be able to see 50-60kHz oscillations?
what the waveform you are seeing really is?
what sort of mathematical accuracy Pspice is capable of? Does it give "digital noise" like rounding errors?

If I were you I'd listen to people like LvW, who know about this stuff.
 
suv79 said:
why when the stop time is change dose it effect the frequency.

In my post#7 I gave you my simulation data (PSpice) with the result of app. 55kHz (clean sinewave).
I cannot understand why you didn`t try the same end time (1ms) and resolutiuon (1µs).

Are you aware that for an end time of 1s you expect to see on the screen 55000 oscillations? Does this make sense?
More than that, you should know that the simulator automatically selects a resolution (a certain percentage of the end time) which in many cases (as in yours) is bad because you had specified an end time which is much too large (1s).

That is the reason you see no sine wave - and the frequency is incorrect (too small).
Therefore you must override this automatic and specify a maximum time step as I did for my simulation.(1µs).
It should be possible for you to find out how you can command such an upper limit for the time step.

Furthermore, for a quick and save start of oscillations it is to be recommended to give one of the capacitors an "initial voltage".
Otherwise it takes a long time to see oscillations (if any).

EDIT: Which simulator are you using? Try ".print step" or "advanced options" for specifying the maximum time step.
 
i used, real time noise, which should help start the oscillation
Simulator plot of Diff Probe voltage in mV against Time in mSecs from 0 to 1, showing a red oscillating waveform whose amplitude grows from near zero to about plus or minus 4.5 mV.
 
Screenshot of a transient simulation plot titled tran8 Diff Probe showing a dense red oscillating waveform, Diff Probe in V from about -3 to 3 against Time in mSecs from 0 to 1, with the amplitude settling to a steady sinusoid after about 0.2 ms.

ok with the initial voltage on the capacitors this is much better :)

thank you LvW
sorry iam a bit slow
 
Attachments
  • Simulator screenshot of a transient plot titled Diff Probe, showing a red oscillating voltage vs time in ms with amplitude growing then settling near plus and minus 3 V over 0 to 1 ms.
    upload_2016-2-15_16-11-55.png
    36.1 KB · Views: 493
OK - I hope you have learned now how to simulater an oscillator:
* Use a simulation time of app. 20-50 periods (maximum)
* Use a resolution (time step) of app 1/1000 of the max. simulation time
* Provide a starting aid by using an initial voltage for a capacitor.
* For a better waveform (low distortions, lowTHD) use a smooth amplitude limiting device (diodes, for example).