I have a differential opamp using SC-CMFB ckt and I would like to see the DCOP and the AC analysis. I found out that to do so I would need to use the PSS, PAC and PXF analysis priovided by spectreRF. However, I really do not know how to perform the test. Please help. THanks

I tried to do a PSS analysis and there are some of the questions I want to ask. Is it possible to see all the node voltages on the schematic itself rather than plotting out the voltage of each node? Thanks

Thanks for your rapid reply.
I hope I don't really bother you too much. One more question i.e. how do I test the configuration in figure 1 of http://www.dessent.net/resume/ee240-dessent.pdf ?

I tried using transient analysis but I guessed this is not the right way. Please enlighten me. Thanks a lot.

Here is the basic circuit ...

There is nothing in this circuit that sets the DC differential input level. Only capacitors are connected to the inputs of the opamp, and so DC input level is free to drift. And because the opamp is a high-gain amplifier, and offset on the input will cause the output to drift much faster. The drift on the input is often so small as to be unnoticeable, but the drift on the output can be substantial. Soon the amplifier drifts out of its proper operating region.

Having switched-capacitor common-mode feedback (SC-CMFB) aggravates this situation by injecting charge into the system that can cause the drift. This problem can be made even worse by the simulator itself, because it does not completely conserve charge (there is a section in my book about this). HSpice is notoriously bad at this. With Spectre you can dramatically reduce the charge error without slowing down the simulations much be tightening reltol by a factor of 10-100 while simultaneously loosening lteratio by the same factor. (reltol is a global simulator options, lteratio is an option of the transient and PSS analyses).

Tightening the tolerance acts to reduce the problem, but it does not eliminate it. The basic issue is that this circuit is not viable. If it were placed on chip as is, it would not take very long before charge would build up on the inputs and the amplifier would stop working. To eliminate the problem completely means that some way must be provided to properly fix the DC operating conditions at the input of the amplifier.  Clearly this amplifier is sitting in a test bench consisting of capacitors and voltage sources that is meant to "represent" the rest of the circuit. Well, an important piece was left out, the DC biasing. Somehow that aspect of the circuit must be included in the test bench.

There are a two basic ways of performing these simulations. The first is to simply force the circuit to the right operating point using switches, initial conditions, etc. and then hope it stays there long enough for you to make your measurements. For example, you can use the "switch" component in Spectre and configure it so that it forces the DC operating point in the DC analysis but opens up in AC or transient. Or you can set the operating point using initial conditions, perform a brief transient analysis, and then follow it up with an AC analysis with "prevoppoint=yes" set so that it performs the analysis using the last transient point as the operating point.

The other way is to include the DC biasing aspect of the larger circuit into the test bench. Presumably this involves more switches and clocks. Then you can use SpectreRF to perform the small-signal analyses and transient to predict slew rate and settling time.

-Ken

When you say that transient analysis failed, do you really mean that it failed? Or do you mean that you did not get the result you expected? I expect it is the latter, which implies that transient analysis is telling you something about your circuit that you did not know.

The low frequency feedback in your circuit only applies to the common-mode signal. And as you point out, the common mode signal is not drifting off. It is the differential mode signal that it drifting. It is differential feedback you need to apply at DC.

-Ken

There must be something in the larger circuit that provides differential DC feedback to the circuit. It could be large value resistors in parallel with the feedback capacitors, but more likely it is some switching network, such as auto-zero switches across the feedback capacitors or a switched-capacitor resistor that provides the feedback.

-Ken

Hi ken

I m using cadence icfb tool for running simulations with the NCSU kit, as u said above in order to run pac simulation we need to set pacmag=1 on one of the source. How do I do that, i tried setting AC magnitude on a simple DC voltage source as 1 but seems like that is not helping with the pac magnitude.

thanks

Thanks Andrew

But I dont see any such component in my library, the analog library has a library voltage_sources which has the sources as ccvs, vcvs, vdc, vexp,vpulse,vpwl,vsin.

If i choose vdc, then the parameters are 'AC magnitude' 'AC phase' 'Noise' 'Temperature Coeff 1' 'Temperature Coeff 2'.

I dont think this 'AC magnitude' is 'pac magnitude'.

Is there any other way to get around this problem??

Thanks