Hi Robert,

for DC and small signal analysis, you may replace the switched cap CMFB by a resistive one, using equivalent resistors as given by the capacitor values and the switching frequency.

Paul

Hi Paul and Ken,

Thank you for your replies.
Ken, could you suggest similar tools in Mentor Graphics that I can use for the steps you mention (such as PSS etc.)?

Cheers,
Robert

I am using Mentor Tools and I especially like the extended control language of Eldo, but that's a personal point of view I don't want to argue about. True that MGC doesn't offer the kind of simulation you ask for.

What you can do, other than computing the equivalent resistor value and replacing it in the schematic, is run a transient simulation up to reaching equilibrium (all nodes have reached their correct operating point). From that point you can run AC or noise simulations (not sure whether you can use harmonic balance from Eldo RF, I'm only using "plain" Eldo).

I copied the following section from the Eldo documentation:
--------
AC in the middle of a .TRAN
Whenever a .AC command, a .TRAN command, and a .OP command containing time specifications are in the .cir file, then an AC analysis will be performed at each of these time points. In the following example Eldo will perform AC, NOISE and TRAN analyses at time 0, time 5n, and time 7n:
.AC DEC 10 1 1e9
.NOISE v(5) vin 70
.TRAN 1n 20n
.OP 5n 7n
--------
I never used PAC, PXF in SpectreRF so I cannot really compare. For my analog (not RF) designs, this works fine. Does this answer your question?

Paul

Ken,

you are totally right that this doesn't work for SC filters. I do use this kind of simulation for SC amplifiers where the CM takes some clock periods for converging to its operating point, but where the voltage gain is defined by a capacitor ratio, i.e. there is a AC direct path from input to output.

It depends on Roberts topology whether this kind of simulation is usable for him or not. As far as I understood his first post, he only considers the bare amplifier and the SC CMFB. In that case I believe he can use this kind of simulation. Am I wrong?

Paul

Ravi,
I've never heard of TPUNCH and TRANAC, but if I understood your explanation, the transient and AC analyses in Spectre can be configured to do the same thing. I occasionally use such an analysis approach to provide some insight as to how the circuit is behaving, but I am always somewhat dubious of the results as this approach violates the basic assumptions behind operating points and AC analysis.

-Ken

Hi Stan

You can use the Spectre RF simulator....the analysis is called PSS and PAC analysis.

By the way, do you know how to design the SC CMFB? any general guidelines, eg. how to choose the correct value for the capacitors? thx

Hello all experienced guys:

I am new here and new about SC_CMFB design.
I know this post is three years ago!!
I have some thoughts on this topic,
Could anyone comment on it and enlighten me

Robert said "designing a fully differential folded cascode (FC) opamp for switched capacitor (SC) circuits". The OPamp is used for discrete-time
applications. The OP gain which he concerned about is the gain in some phase rather than an averaged gain. If we use a resistor to replace the switched-capacitor or just do PSS/PAC simulation, we will get a lower gain.
In this case, we just do a transient simulations followed by AC simulation.
Then, we will get what we want. Is this right?

Shano