The Designer's Guide Community
Forum
Welcome, Guest. Please Login or Register. Please follow the Forum guidelines.
Jun 24th, 2019, 3:04pm
Pages: 1
Send Topic Print
LC VCO Simulation Help needed !! (Read 4666 times)
umberabbas
Junior Member
**
Offline



Posts: 13

LC VCO Simulation Help needed !!
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.

Back to top
 

Screenshot_014.png
View Profile   IP Logged
cheap_salary
Senior Member
****
Offline



Posts: 162

Re: LC VCO Simulation Help needed !!
Reply #1 - Sep 13th, 2017, 10:47pm
 
Delete V0.
Back to top
 
 
View Profile   IP Logged
Ken Kundert
Global Moderator
*****
Offline



Posts: 2173
Silicon Valley
Re: LC VCO Simulation Help needed !!
Reply #2 - 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
Back to top
 
 
View Profile WWW   IP Logged
umberabbas
Junior Member
**
Offline



Posts: 13

Re: LC VCO Simulation Help needed !!
Reply #3 - Sep 15th, 2017, 1:02am
 
It is cadence Spectre. I have tried to perform transient analysis but it isn't working.
Back to top
 
 
View Profile   IP Logged
cheap_salary
Senior Member
****
Offline



Posts: 162

Re: LC VCO Simulation Help needed !!
Reply #4 - 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.

Back to top
 
 
View Profile   IP Logged
Geoffrey_Coram
Senior Fellow
******
Offline



Posts: 1963
Massachusetts, USA
Re: LC VCO Simulation Help needed !!
Reply #5 - 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.
Back to top
 
 

If at first you do succeed, STOP, raise your standards, and stop wasting your time.
View Profile WWW   IP Logged
Ken Kundert
Global Moderator
*****
Offline



Posts: 2173
Silicon Valley
Re: LC VCO Simulation Help needed !!
Reply #6 - 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
Back to top
 
 
View Profile WWW   IP Logged
umberabbas
Junior Member
**
Offline



Posts: 13

Re: LC VCO Simulation Help needed !!
Reply #7 - 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.
Back to top
 

netlist4.png
View Profile   IP Logged
umberabbas
Junior Member
**
Offline



Posts: 13

Re: LC VCO Simulation Help needed !!
Reply #8 - Sep 19th, 2017, 8:01pm
 
This one is the output from the circuit.
Back to top
 

Screenshot4.png
View Profile   IP Logged
Ken Kundert
Global Moderator
*****
Offline



Posts: 2173
Silicon Valley
Re: LC VCO Simulation Help needed !!
Reply #9 - 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
Back to top
 
 
View Profile WWW   IP Logged
umberabbas
Junior Member
**
Offline



Posts: 13

Re: LC VCO Simulation Help needed !!
Reply #10 - 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.
Back to top
 

Screenshot5.png
View Profile   IP Logged
umberabbas
Junior Member
**
Offline



Posts: 13

Re: LC VCO Simulation Help needed !!
Reply #11 - Sep 22nd, 2017, 4:18am
 
Netlist for the above generated waveform.
Back to top
 

Screenshot-5_002.png
View Profile   IP Logged
Geoffrey_Coram
Senior Fellow
******
Offline



Posts: 1963
Massachusetts, USA
Re: LC VCO Simulation Help needed !!
Reply #12 - 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.)
Back to top
 
 

If at first you do succeed, STOP, raise your standards, and stop wasting your time.
View Profile WWW   IP Logged
Ken Kundert
Global Moderator
*****
Offline



Posts: 2173
Silicon Valley
Re: LC VCO Simulation Help needed !!
Reply #13 - 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
Back to top
 
 
View Profile WWW   IP Logged
cheap_salary
Senior Member
****
Offline



Posts: 162

Re: LC VCO Simulation Help needed !!
Reply #14 - 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.



Back to top
 
« Last Edit: Sep 23rd, 2017, 5:07am by cheap_salary »  
View Profile   IP Logged
Pages: 1
Send Topic Print
Copyright 2002-2019 Designer’s Guide Consulting, Inc. Designer’s Guide® is a registered trademark of Designer’s Guide Consulting, Inc. All rights reserved. Send comments or questions to editor@designers-guide.org. Consider submitting a paper or model.