Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics 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.

High Q circuit Simulation

farshaddd

Newbie level 6
Newbie level 6
Joined
Jun 7, 2021
Messages
13
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
88
Hi every one.

I'm simulating a very high quality factor RLC circuit in cadence.
The AC analysis is OK (correct answer) if I take a very small frequency step size.

However, the transient analysis is not correct (even with very small time step size) !!!!!.
I should mention that the TRAN analysis is performed in resonant frequency (8.563 kHz).
What should I do?

The circuit schematic has been attached.
Thanks a lot.

123.png
 
Quote from Microsims Application notes.
"The simulation run must a minimum of Q cycles before the circuit reacts....
For a crystal with moderately high-Q (20000) it can take close to a million cycles before the oscillator reaches a steady state condition.....
But it is possible to use AC analysis to simulate high-Q circuits"
 
tran has sloppy tolerances that can let solvers "lose track of" minuscule-amplitude activity before it can "bloom out of the noise".

Simulating XOs is a special art, this what I have learned from failed test chips after successful (looking) analyses. And high enough Q starts to look like the same problem-set.
 
I can't speak to cadence, but I know LTspice also has issues with tran simulations of high Q circuits. Usually it's just a matter of setting the maximum timestep very low (like <<1/(Q*fc)) and allowing it plenty of time to reach steady state (like >> Q/fc). I think this has worked for Q values as high as 500, but at some point I assume other factors like numerical precision and charge/voltage tolerances would matter as well.

For your circuit with a Q of ~200,000,000, I don't know what you'd have to do to get "real" results, but I'm not sure how useful it is to simulate such an unrealistic system anyways...

A harmonic balance or periodic steady state solution might be better suited for you.
 
What is your stimulus source's initial voltage?

If it isn't in the center (zero crossing) of the sine
then you have a built in initial offset which will
average away over time (but never completely
settle).

The schematic looks like LTSpice, not Virtuoso.
 


Write your reply...

LaTeX Commands Quick-Menu:

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top