The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> PSRR and CMRR for fully differential OTA using xf analysis
https://designers-guide.org/forum/YaBB.pl?num=1503407184

Message started by kabir_fakir on Aug 22^nd, 2017, 6:06am

Title: PSRR and CMRR for fully differential OTA using xf analysis
Post by kabir_fakir on Aug 22^nd, 2017, 6:06am

Hello everyone,
Before making this thread i went to following thread
http://www.designers-guide.org/Forum/YaBB.pl?num=1073321544

so by definition CMRR= Adm/Acm
PSRR = Aps/Adm
To simulate FD OTA((with CMFB inside)) I followed the famous Ken Kundert paper to make test bench ( http://www.designers-guide.org/analysis/diff.pdf) f. The feedback network is capacitive so I put resistance of 1G in feedback path to provide the DC bias. To simulate the transfer function ( like Aps, Acm, Adm) with XF analysis, small ac signal is put in every input port. For example, common mode input signal is V4 is given 4.5 of dc signal along with 100uV of ac magnitude, same is done with power supply, V2 is given 9 V of Dc voltage along with 100uV of ac signal.
After setting this test bench the XF SIMULATION is run along with DC simulation. But I have found some unexpected results which I am not able to understand. You can see the results in below comments.
So Please explain me what is wrong(or I am analyzing it wrong) with the testbench/simulation. Kindly let me know if you need more information

Title: Re: PSRR and CMRR for fully differential OTA using xf analysis
Post by kabir_fakir on Aug 22^nd, 2017, 6:11am

Here is the setting for the xf analysis (see most right img). With this setting I have plotted the plotted the Aps=Voutd/Vsupply and Adm= Voutd/Vind
Vout= Differential o/p
Vind= Differential i/p

What i dnt understand is: Aps? Why the power supply gain is so erratic in behavior?

Title: Re: PSRR and CMRR for fully differential OTA using xf analysis
Post by kabir_fakir on Aug 22^nd, 2017, 6:20am

To simulate the common mode gain Acm=Vcm_out/Vcmin setting of the XF is shown in the image. Here Vcmin =V4.
So can is say that my CMRR is 78db ?(as Acm= 54dB , Adm= 24dB)
is that right?
Also is that make sense to define CMRR in close loop or should it be defined for open loop?

Title: Re: PSRR and CMRR for fully differential OTA using xf analysis
Post by Ken Kundert on Aug 23^rd, 2017, 11:18am

Two things.
1. With XF analysis, you need not specify an input magnitude on any input source. The input magnitude is assumed to be 1 on every source in XF, though you can adjust it using xfmag if needed.

2. The reason why Aps is erratic is because it is zero. You circuit is perfectly symmetric, and as such any variation on the supply results is no differential variation on the output. All you are seeing is roundoff error 260dB down (fempto volts).

-Ken

Title: Re: PSRR and CMRR for fully differential OTA using xf analysis
Post by kabir_fakir on Aug 24^th, 2017, 10:03am

Ken Kundert wrote on Aug 23^rd, 2017, 11:18am:

thanks a lot of replying.
Regarding first point
1. You are right. I did the simulation without any input. . Actually in your book(The Designer Guide to spice and spectre) you have written "Transfer functions for nodes are computed assuming that a unit magnitude current source is connected from the gnd..." and so on. Thanks for clarifying this.

Second point (PSRR)
2. I got the point. It means i will see some reasonable value of PSRR when i introduce some mismatch or offset

Could you please comment on my value of CMRR(78dB)? Is that right ?