Phase shift oscillator and circuit

Join the discussion
Registration is free. Ask a follow-up in this thread, or start your own.
Sign up Log in
26 replies · 6K views
suv79
Messages
65
Reaction score
0

Homework Statement


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

upload_2016-2-13_18-17-20.png

Gain & phase response of TL072 op-amp
upload_2016-2-13_18-19-1.png


Homework Equations


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

The Attempt at a Solution


upload_2016-2-13_18-24-39.png

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

PSpice simulation
upload_2016-2-13_18-32-10.png

analysis
upload_2016-2-13_18-33-34.png

why is my frequency 22 Hz
 

Discussion

Physics news on Phys.org
how can i find an 'ideal op-amp' in PSpice ?
 
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).
 
65 kHz is my worked out frequency but PSpice is 22 Hz
 
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.
 
upload_2016-2-14_17-36-57.png

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 ?
 
could you email me your simulated circuit ?
 
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
upload_2016-2-14_21-4-47.png

but time resolution i have no idea.
upload_2016-2-14_21-5-42.png
 
the run time should not change the frequency
 
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
upload_2016-2-14_21-35-13.png

but where can i change time resolution ?
 
i have no idea how to work out the amplitude of the waveform
 
upload_2016-2-15_14-55-14.png

why when the stop time is change dose it effect the frequency.
 
upload_2016-2-15_14-58-48.png

red is 50 u
green is 100u
blue is 200u
 

Attachments

  • upload_2016-2-15_14-58-38.png
    upload_2016-2-15_14-58-38.png
    5 KB · Views: 548
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
upload_2016-2-15_16-5-42.png
 
upload_2016-2-15_16-13-9.png

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

thank you LvW
sorry iam a bit slow
 

Attachments

  • upload_2016-2-15_16-11-55.png
    upload_2016-2-15_16-11-55.png
    36.1 KB · Views: 482
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).
 

Similar threads

Why Does the Phase Shift Oscillator Frequency Drop with the TL072?

  • topcat123
  • · Replies 30 ·
  • Engineering and Comp Sci Homework Help
2
Replies
30

RC Phase Shift Oscillator not Oscillating

  • Cup of Joe
  • · Replies 41 ·
  • Electrical Engineering
2
Replies
41

Purely passive RC Phase Shift Oscillator?

  • Cup of Joe
  • · Replies 27 ·
  • Electrical Engineering
Replies
27

I have tried building a phase shift oscillator, but it won't work

  • David lopez
  • · Replies 33 ·
  • Electrical Engineering
2
Replies
33

Zero phase shift Op-Amp bandpass filter design

  • kyle111
  • · Replies 3 ·
  • Engineering and Comp Sci Homework Help
Replies
3

How does LC phase shift oscillator work?

  • Neyolight
  • · Replies 1 ·
  • Electrical Engineering
Replies
1

Phase Shift Oscillator Question

  • Garengineer
  • · Replies 4 ·
  • Electrical Engineering
Replies
4

Will an infinite impedance cause no phase shift?

  • kostoglotov
  • · Replies 6 ·
  • Engineering and Comp Sci Homework Help
Replies
6

Phase Shift Oscillator: Why, What & How

  • samieee
  • · Replies 5 ·
  • Electrical Engineering
Replies
5

PLL with adjustable constant phase shift

  • Greg-ulate
  • · Replies 1 ·
  • Electrical Engineering
Replies
1