How to simulate the fully differential opamp with SC CMFB?

[BackerShu]

sc cmfb

After adding the SC CMFB circuit to a fully differential opamp, I can only check whether the output common mode voltage could stay at the expected value with a certain time of tran. simulation to determine how the SC CMFB circuit works. Could someone tell me how to exactly find out its infulence on the opamp's AC performance GBW, PM, etc. by simulation? In another word, how to simulate the GBW and PM of a opamp with SC CMFB?
I have tried pss and pac simulation in SpectreRF. But the simulation result donesn't resonable. So I doubt this method may not work or I did it wrong way.

Methods using any tools would be helpful!

Thx in advance!!

 

[LvW]

how to simulate op-amp

There is an alternative, which - I guess - could work in your case.
It is described by an author from tschechoslovakia. Today, I will try to locate the paper and then I will give further notice if you are interested. Are you ?
The principle of the method is to duplicate the complete circuit, that means to scetch it for both switching periods and then to combine both results in a certain manner.
I have tried it for complete sc filter circuits and it worked very well.
Regards
LvW

 

[BackerShu]

Thanks LvW!
Of cousre I'm interested in your altenative method and waiting for your further notice. Something that I must take into my mind when using this method would also be appreciated.

BTW, an article telling about how to use SpectreRF to simulate the sc-filter is worth reading: https://www.designers-guide.org/Analysis/
I think the method could also be used in my case, but I haven't got the resonable simulation result by now. If you have spare time, I think you can to take a look and make some discussion, that may also be helpful to your case.

 

[LvW]

Re: How to simulate the fully differential opamp with SC CMF

Hi BackerShu,

here is the link for the paper I have mentioned.

http://www.vabo.cz/stranky/biolek/veda/articles/CSCC07.pdf

In addition, I enclose a pdf sheet showing the simulation arrangement for an SC integrator I have used with very good success (AC analysis).
Please note, that the controlled current sources are controlled each with the current flowing in the other part of the circuit (the other clock phase). Thus, both parts are connected together.
To measure the current (with the aim to define it as a control parameter) you probably must include a zero-volt-source in series with the corresponding resistor (as I did for PSpice).
The output signal of the combined circuit simply consists of the sum of both parts.
(The paper was in german, therefore Ue means input and Ua means output voltages).

Im sorry that the opamp symbols are not correctly translated to pdf.

 

[BackerShu]

Hi LvW!
Thank you very much for the paper and the simulation tips.
I'll read the paper and do some simulation to check if this method is suitable to the opamp with SC CMFB as soon as possible.

I'll let you know if it works or run into some problems.

 

[tyanata]

Re: How to simulate the fully differential opamp with SC CMF

I have same problem. I have designed amplifier which in AC simulation with ideal CMFB (using system from several VCVS) achieves about 75dB gain. Using PSS and PAC with real SC CMFB I achieve about 33dB. It is strange that in spectre.out file for DC levels for OUTP and OUTN are about 300mV output N cascodes are in triode region, but if I plot OUTP and OUTN from PSS analysis it is seen that they achieve required from design CM. So it seems that there is some option to be mark PAC to takes steady state DC OP after stabilization time, but not DC OP after beginning of simulation. My clock is 2MHz. I entered for tstab 500us which is quite enough and tstart is 200us.
My be your problem is same!