The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> Switched Cap Noise in Hspice and Spectre
https://designers-guide.org/forum/YaBB.pl?num=1046226871

Message started by sch on Feb 25^th, 2003, 6:34pm

Title: Switched Cap Noise in Hspice and Spectre
Post by sch on Feb 25^th, 2003, 6:34pm

How can one to simulate the Switch Cap noise in Hspice and
the results is same as SpectreRF?

Title: Re: Switched Cap Noise in Hspice and Spectre
Post by Ken Kundert on Feb 26^th, 2003, 7:48am

With SpectreRF you can use the RF analyses to directly measure characteristics of an SC filter that would either be very difficult or impossible to measure with HSpice. For example, you could use the PAC analysis to measure the filter's transfer function versus frequency. Doing so in HSpice would require either a long transient analysis where you swept the input frequency or a series of individual transient analyses, one for each frequency at which you want the transfer function. Finally, in HSpice you would have to compose the transfer function from the results of the transient analysis, whereas with SpectreRF the transfer function is available directly. You can get the transfer function with HSpice, but it is a very painful process, especially if you are interested in the low-frequency transfer function. The low frequencies necessitate a very long and expensive transient analysies. In SpectreRF, the PAC analysis time is independent of frequency.

SpectreRF provides PXF analysis, which allows you to directly compute several transfer functions at once (say gain, PSRR, etc.). There is no equivalent in HSpice. You would simply have to perform the painful process described above multiple times.

The SpectreRF PNoise analysis directly computes the noise produced by the SC filter, including kT/C noise, noise from the amplifiers, flicker noise, etc. It also includes sampling and noise folding effects, etc. This is imposible to do in HSpice.

Finally, you can use SpectreRF's QPSS analysis to directly and efficiently compute the steady state response when one or two large sinusoids are present at the input. In this way you can quickly compute the distortion of narrowband filters (either harmonic or intermodulation distortion). With HSpice this would require a very long transient analysis and so would be much more expensive.

Title: Re: Switched Cap Noise in Hspice and Spectre
Post by pwm on Apr 11^th, 2003, 9:16pm

Hi Ken,
Thanks for the advice on PSS using spectreRF. I have problems trying to determine total harmonic distortion (THD) for my switched capacitor filter. It would take pretty long simulation time with input signal of many cycles for a simple transient run. I am not sure if QPSS can help with my problem (more info on how to use please)? or should I use PSS analysis (take me about 2 days of simulation time) or should I use Pdisto ?
Thanks.

Title: Re: Switched Cap Noise in Hspice and Spectre
Post by August West on Apr 22^nd, 2003, 9:34pm

PDisto and QPSS are two different names for the same analysis. PDisto is being phased out, QPSS is the preferred name.

If a PSS analysis is taking two days because of a large ratio between the beat frequency and the clock frequency, then QPSS sounds like your best bet.

August