OTA-C quadrature oscillator : not working

[puruparajuli]

I tried to design an OTA-C oscillator , (in a 1.2um CMOS process.)
The supply voltage are +2.5 -2.5 volts.
the circuit is exactly the same as found in the tutorials of ota-c oscillators.
But when I simulate the output voltage over time all I get is flat dc voltage ,

The circuit is not oscillating no matter what gm i use for ota, or the value of capacitance i use for it. and I've always made sure that the condition of oscillation is met.

Can someone help please.

 

[dick_freebird]

Have you tried "kicking" it?

 

[puruparajuli]

how do I 'Kick' it?. I thought it should have just worked without any input given.
I'm hearing the therm "kicking" the oscillator first time.
not actually kicking it , is it? lol my old tape recorder works that way.

 

[JoannesPaulus]

you need to inject a current pulse in the oscillator loop.

 

[puruparajuli]

Well for ota-c oscillators, I can't find the input terminal for the current pulse to be given in. Also the paper doesn't talk about 'kicking'. The output voltage should've oscillated with the frequency given by the characteristic polynomial.
I have attached the paper , and I've tried all the oscillator combinations given there without any success.
Surely I'm missing something, can't figure it out.

Any help would be very precious.

 

[LvW]

Well for ota-c oscillators, I can't find the input terminal for the current pulse to be given in. Also the paper doesn't talk about 'kicking'. The output voltage should've oscillated with the frequency given by the characteristic polynomial.

If the design contains no errors the oscillator should work also without any "kick"; instead you should give one of the capacitors an initial condition (voltage 1 mV or so). Try it. If it does not work, check the loop gain (ac simulation) which should be unity at the oscillating frequency.

Added after 26 minutes:

The circuit is not oscillating no matter what gm i use for ota, or the value of capacitance i use for it. and I've always made sure that the condition of oscillation is met.

I just have simulated the simplest two-OTA circuit with success.
OTA: Two ideal VCCS with gm=10mS
3 equal capacitors: 100 pF (with 1 Megohm in parallel because of bias point)
Initial condition: IC=100mV across one earthed capacitor.
Result: selfsustained oscillation at 9 MHz.

Regards

Added after 1 hours 41 minutes:

Additional info: For ideal OTA´s (VCCS) you can remove the capacitance between both outputs. The whole circuit resambles an active (grounded) inductance in parallel with a capacitor resulting in a losless LC tank circuit if the OTAs are ideal.
For real active devices the 3rd capacitor is necessary because it cancels losses due to pos. feedback. But this capacitor also influences the frequency (16 MHz instead of 6 MHz).

 

[puruparajuli]

thanks Lvw,
I made a circuit with the values of capacitances and VCCS, and the parallel resistor exactly the same as you've made.
but all I get at the output is the 0V dc,
I simulated for 1ms in transient analysis in pspice,

I can't figure out whats been missing. Please help me find the mistake I've made.
I've also attached the pspice file,

regards

 

[LvW]

.................
.................
I've also attached the pspice file,
..................

Just for clarification: No, you haven´t attached the pspice file. It is the schematic.
This is important as the true pspice file contains simulation commands - and I could see your time steps you have chosen. I am afraid that´s the error you have made.
Please, realize that in 1 ms a 10 MHz signal has 10000 periods. Would you like to see 10000 periods on your screen ?
Make a simulation for 1 us and use a step ceiling of 1ns - and you most probably will have success. Try it and confirm it.
Regards

And don´t forget the initial condition !

 

[puruparajuli]

Well I tried that, but still i can't get it. It still shows 0v at the output.
I have attached the pspice file this time.

I've been stuck in this for past few days now, and still can't figure it out.
your help would be precious.
regards.

 

[LvW]

OK, I think I have found the error source.
Your first picture you have sent was OK.
But the second one differs from the first one in an important aspect: The polarity of the VCCS to the right is false. I have corrected your file and have simulated it with success in PSpice.

Either you allocate -10m to this VCCS or you exchange the output connections.
Then everything will be OK and you can successively change the values of gm and C as you want. But don´t forget the initial conditions and try to simulate only for 10-20 periods.
Good luck.

Added after 1 hours 2 minutes:

Hi puruparajuli

There is one catastrophic error I forgot to mention:
1M means only 1 milli-Ohm.
For 1 Megohm you should write 1E12 or 1000k or 1Meg
Correction (thanks to FvM): 1E6

 

[FvM]

Yes a popular SPICE user fault. But 1Mohm is 1E6 rather than 1E12.

 

[puruparajuli]

Wow its working now. Finally
Thank you LvW for the help. Without it, I would've been stuck in it don't know how many days.

 

[LvW]

Fine !

Here is a hint (perhaps it helps) for calculation:

1.) Both OTA´s together with C1 (see the schematic in the paper) simulate an active inductor with L=C1/(gm1*gm2).
2.) Without C3 (not necessary if OTAs ideal) the oscillating frequency is
f=1/(2Pi*sqrt(L*C2)). This is confirmed by simulation.
3.) With C3: I don´t know yet, but it should be mentioned in the paper.
Regards