Designer’s Guide Community

georgejor Junior Member Offline Posts: 15	Simulation setting of CMFB in HSpice Mar 13^th, 2005, 8:07am Can anyone tell me the HSpice setting for simulating ac respone of a SC-CMFB amplifier? Thank you very much!
Back to top	IP Logged

Mighty Mouse

Community Member

Offline

Here I come to save
the day!

Posts: 75
Fantasyland

Re: Simulation setting of CMFB in HSpice
Reply #1 - Mar 13^th, 2005, 12:34pm

You cannot simulate an SC-CMFB circuit with AC analysis. The problem is that in order to operate properly, the switches must be operating. But an AC analysis is performed about a DC operating point, which means the switches are either stuck open or stuck closed.

If you want to simulate an SC-CMFB cirucit, you will need a simulator like SpectreRF. It provides PAC, a type of AC analysis performed about a periodic operating point.

- MM -

Back to top

IP Logged

georgejor Junior Member Offline Posts: 15	Re: Simulation setting of CMFB in HSpice Reply #2 - Mar 13^th, 2005, 6:30pm Thank you for your reply! Then, if i have no spectreRF or spectre, how could i do? thanks!
Back to top	IP Logged

Mighty Mouse Community Member Offline Here I come to save the day! Posts: 75 Fantasyland	Re: Simulation setting of CMFB in HSpice Reply #3 - Mar 13^th, 2005, 9:16pm Transient analysis. Hit it with a common mode step and look for ringing. If it rings without much damping, your CMFB is close to being unstable. Consider using the test bench for differential circuits described in the paper at www.designers-guide.org/Analysis. - MM -
Back to top	IP Logged

Sid

Community Member

Offline

Posts: 35

Re: Simulation setting of CMFB in HSpice
Reply #4 - Apr 15^th, 2005, 9:29am

Actually, there is a way to simulate the CMFB circuit for determining LOOP-GAIN using a simple SPICE AC analysis (no need for a SpectreRF PAC).

P.J. Hurst, S.H. Lewis, "Determination of stability using return ratios in balanced fully differential feedback circuits", Circuits and Systems II: Analog and Digital Signal Processing, IEEE Transactions on [see also Circuits and Systems II: Express Briefs, IEEE Transactions on]
Volume 42, Issue 12, Dec. 1995 Page(s):805 - 817

However, note that this is an IDEALIZED simulation and you need to model the cap loadings correctly to getter a better estimate of your stability.

I do NOT use this to check stability of my CMFB, but use it for defining a DC operating point for my Op Amp for AC sweep analysis. I prefer using transient simulations for testing stability of my CMFB. Anyway, finally a transient simulation is the true check for stability.

Sid

Back to top

IP Logged

Mighty Mouse

Community Member

Offline

Here I come to save
the day!

Posts: 75
Fantasyland

Re: Simulation setting of CMFB in HSpice
Reply #5 - Apr 15^th, 2005, 5:43pm

The SC in SC-CMFB stand for 'switched capacitor'. Switched-capacitor circuits require a clock to operate properly. The small-signal analyses in HSpice cannot properly simulate a switched-capacitor circuit because they linearize the circuit about its DC operating point, meaning that the clock is not operating. For this reason you cannot use HSpice for this analysis, SpectreRF is required.

- MM -

Back to top

IP Logged

Sid

Community Member

Offline

Posts: 35

Re: Simulation setting of CMFB in HSpice
Reply #6 - Apr 15^th, 2005, 8:04pm

Hi MM,

Please take a look at Appendix B of the paper I mentioned in my previous email. It presents an "equivalent DC model" for the SC CMFB circuit! This can be used to define an operating point for the OTA, allowing one to do regular SPICE AC analysis. An even more simplified DC model is presented in Fig 10 of that paper. The authors claim that one can then check the PM of the SC-CMFB loop using this model. The model uses voltage controlled voltage sources to provide CMFB and hence defines a unique bias point for the system. All cap loading is carefully modeled.

While I agree this may not be as accurate as using PAC in SpectreRF, this is certainly a useful way of verifying the PM of a SC-CMFB loop for those who only have access to SPICE. Transient simulations are of course the final/ultimate test of stability.

Sid

Back to top

IP Logged

wued New Member Offline Posts: 7	Re: Simulation setting of CMFB in HSpice Reply #7 - Apr 29^th, 2005, 6:46pm I think there is a way to use ac analysis for SC-CMFB.Firstly you can run transient analysis without initial conditional until convergence, then record all states of circuit when the capcitor in CMFB is connented to amplifier. Secondly you can using recorded initial condition to perform ac analysis.
Back to top	IP Logged

Sid Community Member Offline Posts: 35	Re: Simulation setting of CMFB in HSpice Reply #8 - Apr 29^th, 2005, 6:51pm Which is identical to using DC sources to define biasing conditions (i.e. charge across capacitors) and using the caps to ensure accurate loading (for AC analysis). This is very similar to the approach described in the paper I reference in one of my earlier posts on this topic. -Sid
Back to top	IP Logged