Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

OTA-C quadrature oscillator : not working

Status
Not open for further replies.

puruparajuli

Newbie level 4
Joined
Sep 2, 2009
Messages
7
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Location
usa
Activity points
1,332
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.
 

puruparajuli

Newbie level 4
Joined
Sep 2, 2009
Messages
7
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Location
usa
Activity points
1,332
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

Advanced Member level 3
Joined
Mar 19, 2008
Messages
773
Helped
233
Reputation
466
Reaction score
134
Trophy points
1,323
Location
USA
Activity points
5,006
you need to inject a current pulse in the oscillator loop.
 

puruparajuli

Newbie level 4
Joined
Sep 2, 2009
Messages
7
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Location
usa
Activity points
1,332
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

Advanced Member level 5
Joined
May 7, 2008
Messages
5,817
Helped
1,738
Reputation
3,478
Reaction score
1,337
Trophy points
1,393
Location
Germany
Activity points
39,028
puruparajuli said:
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:

puruparajuli said:
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

Newbie level 4
Joined
Sep 2, 2009
Messages
7
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Location
usa
Activity points
1,332
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

Advanced Member level 5
Joined
May 7, 2008
Messages
5,817
Helped
1,738
Reputation
3,478
Reaction score
1,337
Trophy points
1,393
Location
Germany
Activity points
39,028
puruparajuli said:
.................
.................
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

Newbie level 4
Joined
Sep 2, 2009
Messages
7
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Location
usa
Activity points
1,332
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

Advanced Member level 5
Joined
May 7, 2008
Messages
5,817
Helped
1,738
Reputation
3,478
Reaction score
1,337
Trophy points
1,393
Location
Germany
Activity points
39,028
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

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
47,436
Helped
14,034
Reputation
28,321
Reaction score
12,684
Trophy points
1,393
Location
Bochum, Germany
Activity points
275,912
Yes a popular SPICE user fault. But 1Mohm is 1E6 rather than 1E12.
 

puruparajuli

Newbie level 4
Joined
Sep 2, 2009
Messages
7
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Location
usa
Activity points
1,332
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

Advanced Member level 5
Joined
May 7, 2008
Messages
5,817
Helped
1,738
Reputation
3,478
Reaction score
1,337
Trophy points
1,393
Location
Germany
Activity points
39,028
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
 

Status
Not open for further replies.
Toggle Sidebar

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top