The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl Measurements >> Phase Noise and Jitter Measurements >> DAC's phase noise https://designers-guide.org/forum/YaBB.pl?num=1239205157 Message started by maxiao0116 on Apr 8th, 2009, 8:39am |
Title: DAC's phase noise Post by maxiao0116 on Apr 8th, 2009, 8:39am i want to simulate the phase noise of a 14bit Didigtal to Analog Converter . but i am not sure if my pss and pnoise configurations are right i use a digital module to generate a 80MHz sinewave data and pass it to the DAC, DAC and digital module are both using 400MHz sampling frequency. The final differential outputs from DAC is a 14bits 80MHz square wave. i set the pss fundamental freq to 400MHz and beat freq to 80MHz, 15 harnomics. The PSS converged after 11 iterations. my question is 1. are those configurations right? i got a pnoise plot from 100Hz@-130dBc/Hz downto 10MHz@-140dBc/Hz, almost flat! 2. what can i do if i want to simulate a 160MHz output frequency which doesn't have integer multiples with 400MHz sampling frequency 3. what type of noise i should use in Pnoise Analysis, source?jitter?, i used source. 4. if i combine the digital module and DAC together (sampling clock is generated from digital module in verilog), it seems like an oscillator, Can i use the "Noise aware PLL flow" to convert the whole circuit to PPV based behaviour module ? thanks |
Title: Re: DAC's phase noise Post by pancho_hideboo on Apr 10th, 2009, 7:59pm maxiao0116 wrote on Apr 8th, 2009, 8:39am:
See http://www.designers-guide.org/Forum/YaBB.pl?num=1232036048/4#4 maxiao0116 wrote on Apr 8th, 2009, 8:39am:
How do you set "sweeptype" in Pnoise ? You should set like followings. aho pss fund=80M harms=0 maxacfreq=4G errpreset=moderate annotate=status outputtype=time boke pnoise start=10 stop=100M dec=11 maxsideband=50 + sweeptype=relative relharmnum=1 annotate=status maxiao0116 wrote on Apr 8th, 2009, 8:39am:
There is no problem if you set 80MHz as Fundamental frequency in PSS. 160MHz=2*80MHz, 400MHz=5*80MHz. In this case you have to set relharmnum=2. maxiao0116 wrote on Apr 8th, 2009, 8:39am:
maxiao0116 wrote on Apr 8th, 2009, 8:39am:
Some Cadence guys in this forum, e.g. sheldon, Andrew Beckett, Tawna Wilsey might answer for this. |
Title: Re: DAC's phase noise Post by Andrew Beckett on Apr 12th, 2009, 8:27am maxiao0116 wrote on Apr 8th, 2009, 8:39am:
I don't really see why you think it's like an oscillator? It's not autonomous, is it? Or perhaps I've misunderstood your circuit... Regards, Andrew. |
Title: Re: DAC's phase noise Post by sheldon on Apr 12th, 2009, 9:15am Max, Some additional comments, 1) Why is the output a square wave? As Panchoo Hideboo commented the choice of frequencies is probably not appropriate. Attached is an example using the results for PSS analysis of a DAC using the setup described in previous appends related to ADC test setup. Note: The DAC output should be a sine wave if the input is a sine wave. In this case, the time domain waveform is not shown, however, it was a sine wave as can be seen by the output spectrum. 2) The circuit is driven, using autonomous analysis is not is not appropriate. 3) The Noise-Aware PLL flow supports PLL simulation and is not appropriate for this case. Best Regards, Sheldon |
Title: Re: DAC's phase noise Post by maxiao0116 on Apr 12th, 2009, 10:59pm Thank you very much pancho hideboo. i think i misunderstood "beat freq" and "funda freq". i should use such fundamental frequency whose multiples can represent all the frequency components in real spectrum, is that right? if i want to get PSS solution for a 160MHz outputs, i should use 80MHz whose 2nd harnomics is the actual signal, and 5th harnomics is clocking feedthrough. To Andrew Beckett: My system is a Direct Digital Synthesizer, it tunes the output frequency by just modifing the digital "Frquency Ctrol Word", like F = Kvco*V in digital, expect a constant sampling frequency should be provide in addition. if i encapsulate the digital part, DAC and sampling frequency source, i can pin to pin match a typical VCO symbol, and also the general functions. i am wondering if it's work because it's very time consuming to simulate the DDS's narrow band spurs. To sheldon: i think i made a misunderstanding, the "square wave" i mentioned is acutally "sine weighted square wave". I say it square because the output is not filtered by LPF yet. I got a similar SFDR plot like you. I know it's not an autonomous system, but can i force it to use perturbation vector if i encapsulate the whole system to a pin2pin matched vco in Noise-Aware PLL flow and finish all the required simulations in that flow? Thank you all. |
The Designer's Guide Community Forum » Powered by YaBB 2.2.2! YaBB © 2000-2008. All Rights Reserved. |