The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> LC VCO Simulation Help needed !!
https://designers-guide.org/forum/YaBB.pl?num=1505358844

Message started by umberabbas on Sep 13th, 2017, 8:14pm

Title: LC VCO Simulation Help needed !!
Post by umberabbas on Sep 13th, 2017, 8:14pm

I need help in LC VCO simulation with differential outputs in Cadence spectre. I have designed a simple circuit but it isn't oscillating at all. I have run a transient analysis but it isn't showing any results. Kindly help.


Title: Re: LC VCO Simulation Help needed !!
Post by cheap_salary on Sep 13th, 2017, 10:47pm

Delete V0.

Title: Re: LC VCO Simulation Help needed !!
Post by Ken Kundert on Sep 14th, 2017, 8:34pm

Oscillators generally do not self-start in SPICE. To start this oscillator you should place a damped sinusoidal current source across the resonator.

-Ken

Title: Re: LC VCO Simulation Help needed !!
Post by umberabbas on Sep 15th, 2017, 1:02am

It is cadence Spectre. I have tried to perform transient analysis but it isn't working.

Title: Re: LC VCO Simulation Help needed !!
Post by cheap_salary on Sep 15th, 2017, 3:49am


umberabbas wrote on Sep 15th, 2017, 1:02am:
It is cadence Spectre.
I have tried to perform transient analysis
but it isn't working.

Code:
The following branches form a loop of rigid branches (shorts) when added to the circuit. V0: p (from vdd to 0)
V0 and Vpulse consitute rigid loop.
Delete V0.


Title: Re: LC VCO Simulation Help needed !!
Post by Geoffrey_Coram on Sep 15th, 2017, 7:59am


umberabbas wrote on Sep 15th, 2017, 1:02am:
It is cadence Spectre. I have tried to perform transient analysis but it isn't working.


Ken meant Spice-like simulators (analog/transistor-level), meaning also Spectre. Sometimes you can start an oscillator with a well-chosen initial condition (ic) statement.

Title: Re: LC VCO Simulation Help needed !!
Post by Ken Kundert on Sep 15th, 2017, 10:35pm


Quote:
I have tried to perform transient analysis but it isn't working.

You should explain what you mean by "it isn't working". Certainly if it is printing an error message you should give it.

I think Cheap Salary has identified the problem. You cannot have two ideal voltage sources in parallel. But I disagree with him that you should keep Vpulse. Vpulse is clearly there simply to start the oscillator, but that is a terrible way to start a differential oscillator. A differential oscillator is naturally immune to changes on the supply voltage. You are much better served by starting the oscillator with a short differential stimulus.

-Ken

Title: Re: LC VCO Simulation Help needed !!
Post by umberabbas on Sep 19th, 2017, 8:01pm

I have removed V0 along with the resistors so it is giving me this type of output. I have also attached the netlist.
i/p voltage is 1v.
c1 and c2 are 37fF while L1 and L2 are 83pH.
Ibias is 12mA.

Title: Re: LC VCO Simulation Help needed !!
Post by umberabbas on Sep 19th, 2017, 8:01pm

This one is the output from the circuit.

Title: Re: LC VCO Simulation Help needed !!
Post by Ken Kundert on Sep 20th, 2017, 1:44am

You should not use changes in the supply voltage to start an oscillator. Differential oscillators are designed to be immune to variation in the supply voltage. A better approach is to apply a differential transient stimulus directly across the resonator. I recommend a damped sinuosoid.

-Ken

Title: Re: LC VCO Simulation Help needed !!
Post by umberabbas on Sep 22nd, 2017, 4:17am

I did the same as Ken specified. The circuit is kinda oscillating but not at the desired frequency. It is oscillating around 46.1 GHz but this doesn't sound right because the oscillation is going down in negative values.

Title: Re: LC VCO Simulation Help needed !!
Post by umberabbas on Sep 22nd, 2017, 4:18am

Netlist for the above generated waveform.

Title: Re: LC VCO Simulation Help needed !!
Post by Geoffrey_Coram on Sep 22nd, 2017, 4:47am


umberabbas wrote on Sep 19th, 2017, 8:01pm:
I have removed V0 ....


But I still see
V0 (vdd! 0) vsource dc=1 type=dc
in the screen-shot. (BTW: if you put the netlist in a "code" block, then others could copy&paste, rather than having to re-type. I'm not sure if it would be useful, since we don't have the device models, but we might be able to use a basic model.)

Title: Re: LC VCO Simulation Help needed !!
Post by Ken Kundert on Sep 22nd, 2017, 9:01am

Well, you did not indicate what you plotted, but I assume it is the differential output voltage, and I would certainly expect that to go negative.

I think your problem has been solved.

You might consider making the amplitude of your tickler source larger so your oscillation starts up faster. Doing so would speed up your simulations.

-Ken

Title: Re: LC VCO Simulation Help needed !!
Post by cheap_salary on Sep 22nd, 2017, 8:59pm


umberabbas wrote on Sep 22nd, 2017, 4:17am:
I did the same as Ken specified.
No.
You invoke supply voltage pertubation(step pulse) for kicking oscillator start up.

You don't set "maxstep" in previous netlist.
http://www.designers-guide.org/Forum/YaBB.pl?num=1505358844/7#7

Now you set "mastep=(1/60G*20)" and "method=trap" in new netlist.
http://www.designers-guide.org/Forum/YaBB.pl?num=1505358844/11#11

However I don't think your oscillator work with your netlist, since you set "delay=2" in V1.

I think "delay" is around 5nsec.
Show us true netlist.


Geoffrey_Coram wrote on Sep 22nd, 2017, 4:47am:

umberabbas wrote on Sep 19th, 2017, 8:01pm:
I have removed V0 ....
But I still see
V0 (vdd! 0) vsource dc=1 type=dc
in the screen-shot.
"vdd!" is a lonley node.




The Designer's Guide Community Forum » Powered by YaBB 2.2.2!
YaBB © 2000-2008. All Rights Reserved.